Simxpert R3.2 Explicit Workspace Guide

Introduction 1

MD Explicit Workspace Guide Introduction

2 Overview and Definition

Overview and Definition An overview of the SimXpert MD Explcit workspace is given here.

Introduction SimXpert MD Explicit is a preprocessor for graphically preparing input data for MD Nastran Explcit, an explicit dynamic software, used in applications such as crash, crush, and drop test simulations. Use of this workspace allows users to work within one common modeling environment with other SimXpert workspaces such as Structures. Thus, for example, a model originally prepared for NVH, linear, or implicit nonlinear analysis can be easily used in explicit applications (e.g. crash). This dramatically reduces the time spent to build different models for implicit and explicit analysis and prevents you from making mistakes because of unfamiliarity between different programs.

Theory A detailed theory of explicit analysis is outside the scope of this guide. However, it is important to understand the basics of the solution technique, since it is critical to many aspects of using the SimXpert MD Explicit workspace. If you are already familiar with explicit methods and how they differ from implicit methods, you may disregard this section.

Method of Solution Although MD Nastran Explicit Nonlinear uses the Explicit methods, a brief overview of both the Implicit and the Explicit Methods for the solution of dynamic response calculations is given below. Implicit Methods Most finite element programs use implicit methods to carry out a transient solution. Normally, they use Newmark schemes to integrate in time. If the current time step is step n , a good estimate of the acceleration at the end of step n + 1 will satisfy the following equation of motion: ext

Ma' n + 1 + Cv' n + 1 + Kd' n + 1 = F n + 1 where:

M

=

mass matrix of the structure

C

=

damping matrix of the structure

K

=

stiffness matrix of the structure

=

vector of externally applied loads at step

ext

Fn + 1

n+1

Introduction 3 Overview and Definition

a' n + 1

=

estimate of acceleration at step

v' n + 1

=

estimate of velocity at step

d' n + 1

=

estimate of displacement at step

n+1

n+1 n+1

and the prime denotes an estimated value. The estimates of displacement and velocity are given by: 2

d'n + 1 = d n + v n Δt + ( ( 1 – 2β )a n Δt ) ⁄ 2 + βa'n + 1 Δt

2

v' n + 1 = v n + ( 1 – γ )a n Δt + γa'n + 1 Δt or

d'n + 1 = d *n + βa'n + 1 Δt

2

v' n + 1 = v n* + γa'n + 1 Δt where

Δt is the time step, and β and γ are constants.

The terms

d n* and v n* are predictive and are based on values already calculated.

Substituting these values in the equation of motion results in 2

ext

Ma' n + 1 + C ( v* n + γa' n + 1 Δt ) + K ( d* n + βa' n + 1 Δt ) = F n + 1 or 2

ext

M + CγΔt + KβΔt ]a'n + 1 = F n + 1 – Cvn* – Kd The equation of motion may then be defined as residual

M*a' n + 1 = F n + 1

The accelerations are obtained by inverting the –1

residual

a' n + 1 = M* F n + 1

M* matrix as follows:

4 Overview and Definition

This is analogous to decomposing the stiffness matrix in a linear static analysis. However, in dynamics, mass and damping terms are also present. Explicit Methods The equation of motion ext

Ma n + Cv n + Kd n = F n can be rewritten as ext

int

Ma n = F n – F n –1

residual

an = M Fn where

ext

Fn

int

Fn

M

=

vector of externally applied loads

=

vector of internal loads (e.g., forces generated by the elements and hourglass forces)

=

Cv n + Kd n

=

mass matrix

The acceleration can be found by inverting the mass matrix and multiplying it by the residual load vector. In LS_DYNA, like any explicit finite element code, the mass matrix is lumped which results in a diagonal mass matrix. Since M is diagonal, its inversion is trivial, and the matrix equation is a set of independent equations for each degree of freedom, as follows: residual

a ni = F ni

⁄ Mi

The Leap-frog scheme is used to advance in time. The position, forces, and accelerations are defined at time level n , while the velocities are defined at time level n + 1 ⁄ 2 . Graphically, this can be depicted as:

Introduction 5 Overview and Definition

n–1 d, F, a

n–1§2 v

n d, F , a

n+1§2

v

n+1 d, F , a

time

v n + 1 ⁄ 2 = v n – 1 ⁄ 2 + a n ( Δt n + 1 ⁄ 2 + Δt n – 1 ⁄ 2 ) ⁄ 2 d n + 1 = d n + v n + 1 ⁄ 2 Δt n + 1 ⁄ 2 The Leap-frog scheme results in a central difference approximation for the acceleration, and is secondorder accurate in Δt . Explicit methods with a lumped mass matrix do not require matrix decompositions or matrix solutions. Instead, the loop is carried out for each time step as shown in the following diagram:

Grid-Point Accelerations Leap-frog Integration in Time Grid-Point Velocities

Grid-Point Displacements

Element Formulation and Gradient Operator Element Stain Rates Constitutive Model and Integration Element Stresses Element Formulation and Divergence Operator Element Forces at Grid-Points CONTACT, Fluid-Structure Interaction, Force/Pressure boundaries + External Forces at Grid Points

Explicit Time Step Implicit methods can be made unconditionally stable regardless of the size of the time step. However, for explicit codes to remain stable, the time step must subdivide the shortest natural period in the mesh. This means that the time step must be less than the time taken for a stress wave to cross the smallest element

6 Overview and Definition

in the mesh. Typically, explicit time steps are 100 to 1000 times smaller than those used with implicit codes. However, since each iteration does not involve the costly formulation and decomposition of matrices, explicit techniques are very competitive with implicit methods. Because the smallest element in an explicit solution determines the time step, it is extremely important to avoid very small elements in the mesh. Courant Criterion Since it is impossible to do a complete eigenvalue analysis every cycle to calculate the timestep, an approximate method, known as the Courant Criterion, is used. This is based on the minimum time which is required for a stress wave to cross each element:

Δt = SL/c where

Δt

=

Timestep

S

=

Timestep scale factor (<1)

L

=

Smallest element dimension

c

=

Speed of sound in the element material

For 1-D elements, the speed of sound is defined as:

E⁄ρ

c = where,

E

=

Young’s modulus

ρ

=

density

Implicit vs. Explicit Analysis The time step for implicit solutions can be much larger than is possible for explicit solutions. This makes implicit methods more attractive for transient events that occur over a long time period and are dominated by low frequency structural dynamics. Explicit solutions are better for short, transient events where the effects of stress waves are important. There is, of course, an area where either method is equally advantageous and may be used. Explicit solutions have a greater advantage over implicit solutions if the time step of the implicit solution has to be small for some reason. This may be necessary for problems that include:

Introduction 7 Overview and Definition

• Material nonlinearity. A high degree of material nonlinearity may require a small time step

for accuracy. • Large geometric nonlinearity. Contact and friction algorithms can introduce potential

instabilities, and a small time step may be needed for accuracy and stability. • Those analyses where the physics of the problem demands a small time step (e.g. stress wave

effects as in crash, crush, and impact analyses). • Material and geometric nonlinearity in combination with large displacements. Convergence

in implicit methods becomes more difficult to achieve as the amount of nonlinearity for all types increases. Explicit methods have increasing advantages over implicit methods as the model gets bigger, and bigger.

Typical Applications Some of the typical structural applications which are well suited for the SOL 700 explicit analysis are: • • • • • • • • • •

Automotive and Aircraft crash worthiness Crash/Crush simulations Drop testing Ship Collision Projectile penetration Bird Strike Simulation with structural Bird Metal forming, stamping, and deep drawing Jet engine blade containment Golf Club simulation Rollover events

8 Parts and Geometry

Parts and Geometry The geometry of the parts can be either created in SimXpert, or more likely imported from CAD program such as Catia, Pro/E.

Units SimXpert interprets all dimensions and input data with respect to a system of units. It is important to set the appropriate units prior to importing any unitless analysis files (such as a Nastran Bulk Data file) or creating materials, properties, or loads. You can control the system of units by selecting Units Manager from the Tools -> Options->Options Editor menu. If you import a file that contains units, SimXpert will convert them into those specified in the Units Manager.

Creating geometry In the first release SimXpert has very limited geometry creation capabilities. It is possible to create curves and very simple surfaces. For the most part you will be importing geometry from an external source. The imported geometry can be edited in SimXpert

Importing geometry If the geometry of the part is available in a CATIA, parasolid, IGES, or STL file, it can be directly imported into the SimXpert MD Explicit Workspace.

Creating local coordinate systems Sometimes it is convenient to use local coordinate systems for specifying loads, and or boundary conditions. For example, a certain node may have a roller support placed in an inclined plane. A local

Introduction 9 Parts and Geometry

coordinate system with one of its axes normal to the inclined plane needs to be created and used to specify the fixity (SPC) of the displacement component along the direction normal to the inclined plane. CONSTRAINT

Local coordinate systems can be in cartesian, cylindrical or spherical systems. Coordinate system created in SimXpert are represented by the following icons, corresponding to the method selected. Spherical

Cylindrical

Cartesian

Coordinate System

Direction 1

Direction 2

Direction 3

1-3 plane

Cartesian

x

y

z

x-z (y=0)

Cylindrical

r

z

r-z ( θ =0)

Spherical

r

θ θ

φ

r- φ ( θ =0)

You can create local coordinate systems by selecting Cartesian, Cylindrical, or Spherical from the Coordinate System group under the Geometry tab. There are numerous methods to create local coordinate systems in SimXpert:

10 Parts and Geometry

1. 3 Points: Three points are used to define the coordinate system. The first point corresponds to the location of origin. The second point defines the point on a specified axis and the third point defines a point in a specified plane. 2. Euler: Creates a coordinate system through three specified rotations about the axes of an existing coordinate system. 3. Normal: Creates a coordinate system with its origin at a point location on a surface. A specified axis is normal to the surface. 4. Two Vectors: Creates a coordinate system with its origin at a designated location and two of the coordinate frame axes are defined using vectors 5. Advanced: Location and orientation can be independently defined. There are 4 different ways to define the location of the origin of the coordinate system: Geometry, Point/Node, Coordinate System, and Center of Part. Further, the orientation can also be defined 3 ways: Global, Two Axes, and Coordinate System.

Elements 11

Elements

12 Elements

Elements The heart of a finite element program lies in its element library which allows you to model a structure for analysis. MD Nastran has a very comprehensive element library which lets you model 1-D, 2-D, or 3-D structures. This section gives some basic definitions of the element types available in MD Nastran Explicit Nonlinear. For a more detailed description of all the available elements in MD Nastran Explicit, please refer to MD R2 Nastran Quick Reference Guide.

Element Types Each element has five definitive characteristics that determine its behavior: • • • • •

Class Number of Nodes Interpolation Degrees of Freedom Integration Method

Class The type of geometric domain that an element represents determines the class of the element. Listed below are the classes of elements in the MD Nastran Explicit Nonlinear element library. • Beam Elements - a 3-D bar with axial, bending, and torsional stiffness. • Shell Elements - a curved, thin or thick structure with membrane/bending capabilities. • Plate Elements - a flat thin structure carrying in-plane and out-of-plane loads. • Continuum Elements - Solid elements used to model thick sections. • Plane stress - a thin plate with in-plane stresses only. All normal and shear stresses associated

with the out-of-plane direction are assumed to be zero. (All plane strain elements lie in the global x-y plane.) • Plane strain - a region where there is no out-of-plane motion and the normal and transverse

strains are zero. • Generalized plane strain is the same as plane strain except that the normal z-strain can be a

prescribed constant or function of x and y. • Axisymmetric elements are describe in 2-D, but represent a full 3-D structure where the

geometry and loading are both axisymmetric. • 3-D solid - a solid structure with only translational degrees of freedom for each node (linear or

quadratic interpolation functions). • Truss Elements - a 3-D rod with axial stiffness only (no bending). • Membrane Elements - a thin sheet with in-plane stiffness only (no bending resistance). • Concentrated mass/Springs/Damper Elements • Rigid Constraints -

Elements 13 Elements

Number of Nodes The number of nodes for an element define where the displacements are calculated in the analysis. Elements with only corner nodes are classified as first order elements and the calculation of displacements at locations within the element are made by linear interpolation. Elements that contain midside nodes are second order elements and quadratic interpolations are made for calculating displacements. MD Nastran SOL 700 do not support second order elements. In MD Nastran the number of nodes is designated at the end of the element name. For example, a CQUAD4 has 4 nodes. Interpolation Interpolation (shape) function is an assumed function relating the displacements at a point inside an element to the displacements at the nodes of an element. In MD Nastran, three types of shape functions are used: linear, quadratic, and cubic. Degrees of Freedom Degrees of freedom is the number of unknowns at a node. In the general case, there are six degrees of freedom at a node in structural analysis (three translations, three rotations). For example there are three (translations) for 3-D truss element; six (three translations, three rotations) for a 3-D beam element and only three translations for the 3-D solid elements. Integration Numerical integration is a method used for evaluating integrals over an element. Element quantities – such as stresses, strains, and temperatures – are calculated at each integration point of the element. Full integration (quadrature) requires, for every element, 2-D integration points for linear interpolation and 3-D points for quadratic interpolation, where scalar “d” is the number of geometric dimensions of an element (that is, d = 2 for a quad; d = 3 for a hexahedron). Reduced integration uses a lower number of integration points than necessary to integrate exactly. For example, for an 8-node quadrilateral, the number of integration points is reduced from 9 to 4 and, for a 20-node hexahedron, from 27 to 8. For some elements, an “hourglass” control method is used to insure an accurate solution. Table 0-1 summarizes the elements available in MD Nastran SOL 700. This section describes the characteristics of the elements. For shell element CTRIA3 and CQUAD4 shell elements, PARAM,DYNSHELLFORM is used to control the behavior. Table 0-1 MD Nastran

Elements in MD Nastran SOL 700 Available in SOL 700

Fatal Error

CBAR

Y

CBEAM

Y

CBELT

Y

CBEND

N

Y

CBUSH

N

Y

14 Elements

Table 0-1 MD Nastran

Elements in MD Nastran SOL 700 Available in SOL 700

Fatal Error

CBUTT

Y

CCONEAX

N

CCRSFIL

Y

CDAMP1

Y

CDAMP2

Y

CDAMP1D

Y

CDAMP2D

Y

CELAS1

Y

CELAS2

Y

CELAS1D

Y

CELAS2D

Y

CFILLET

Y

CFLUID

N

Y

CGAP

N

Y

CHACAB

N

Y

CHACBR

N

Y

CHEXA

Y

Y (8 Nodes only)

COMBWLD

Y

CONM2

Y

CONROD

Y

CONSPOT

Y

CPENTA

Y (6 Nodes only)

CQUAD4

Y

CQUAD8

Y (4 Nodes only)

CQUADR

Y

CQUADX

N

CROD

Y

CSHEAR

N

CSPOT

Y

CSPR

Y

CTETRA

Y (4 and 10 Nodes)

CTRIA3

Y

Y Y

Elements 15 Elements

Table 0-1 MD Nastran CTRIA6

Elements in MD Nastran SOL 700 Available in SOL 700

Fatal Error

Y (3 Nodes only)

CTRIA3R

Y

CTRIAX

N

Y

CTRIAX6

N

Y

CTQUAD

Y

CTTRIA

Y

CTUBE

Y

CVISC

Y

CWELD

N

Y

16 Preliminaries

Preliminaries Consider the body shown in Figure 0-1. We are interested in time-dependent deformation in which a point in b initially at point x i

X α ( α = 1, 2, 3 ) in a fixed rectangular Cartesian coordinate system moves to a

( i = 1, 2, 3 ) in the same coordinate system. Since a Lagrangian formulation is considered,

the deformation can be expressed in terms of the convected coordinates

x i = x i ( X α, t ) At time

X α , and time t (0-1)

t = 0 , we have the initial conditions

x i ( X α, 0 ) = X α

(0-2)

x· i ( X α, 0 ) = V i ( X α )

(0-3)

where

V i defines the initial velocities.

Governing Equations We seek a solution to the momentum equation

σ ij, j + ρf i = ρx··i

(0-4)

satisfying the traction boundary conditions

σ ij n j = t i ( t ) on boundary

∂b 1 , the displacement boundary conditions

x i ( X α, t ) = D i ( t ) on boundary -

(0-5)

(0-6)

∂b 2 , the contact discontinuity

( σ ij+ – σ ij )n i = 0

(0-7)

Elements 17 Preliminaries

∂b 3 when X i+ = x i- . Here σ ij is the Cauchy stress, ρ is the current density, f is the body force density, x·· is acceleration, the comma denotes covariant differentiation, and n j is a unit outward normal to a boundary element of ∂b . along an interior boundary

x

X

3

3

n x

2

X

2

∂

t = 0

b

b ∂B B0

x1

Figure 0-1

X1

Notation

Mass conservation is trivially stated

ρV = ρ 0 where

V is the relative volume, i.e., the determinant of the deformation gradient matrix, F ij ,

∂x i F ij = -------∂X j and

(0-8)

(0-9)

ρ 0 is the reference density. The energy equation

· E· = Vs ij ε ij – ( p + q )V·

(0-10)

18 Preliminaries

is integrated in time and is used for equation of state evaluations and a global energy balance. In Equation (0-10), s ij and

p represent the deviatoric stresses and pressure,

s ij = σ ij + ( p + q )δ ij

(0-11)

1 1 p = – --- σ ij δ ij – q = – --- σ kk – q 3 3

(0-12)

q is the bulk viscosity, δ ij is the Kronecker delta ( δ ij = 1 if i = j ; otherwise · δ ij = 0 ) and ε ij is the strain rate tensor. The strain rates and bulk viscosity are discussed later.

respectively,

We can write:

 ( ρx··i – σij, j – ρfi )δxi dν +  ( σij nj – ti )δxi ds

(0-13)

∂b 1

v



+

( σ ij+

-

– σ ij )n j δx i ds = 0

∂b 3

where

δx i satisfies all boundary conditions on ∂b 2 , and the integrations are over the current geometry.

Application of the divergence theorem gives

 ( σij δxi ), jdυ

υ

=

 σ ij nj δxi ds +  ( σij – σ ij )nj δxi ds +

∂b 1

-

(0-14)

∂b 3

and noting that

( σ ij δx i ) ,j– σ ij, j δx i = σ ij δx i, j

(0-15)

leads to the weak form of the equilibrium equations:

δπ =

 ρx··i δxi dυ +  σij δxi, j dυ –  ρfi δxi dυ –  ti δxi ds

υ

υ

υ

= 0

(0-16)

∂b 1

a statement of the principle of virtual work. We superimpose a mesh of finite elements interconnected at nodal points on a reference configuration and track particles through time; i.e.,

Elements 19 Preliminaries

k

x i ( X α ,t ) = x i ( X α ( ξ ,η ,ζ ) ,t ) =

 φ j ( ξ ,η ,ζ )xi ( t ) j

(0-17)

j=1

where φ j are shape (interpolation) functions of the parametric coordinates

( ξ ,η ,ζ ) , k is the number of

nodal points defining the element, and x ij is the nodal coordinate of the jth node in the ith direction. Summing over the n elements we may approximate

δπ with

n



δπ =

δπ m = 0

(0-18)

m=1

and write n





   ρx··i Φi dυ +  σij Φi,j dυ –  ρfi Φi dυ –  ti Φi ds  m

m = 1 υm

m

m

m

υm

m

υm

= 0

(0-19)

∂b 1

where

Φ im = ( φ1 ,φ 2 ,… ,φ k ) im

(0-20)

In matrix notation (0-19) becomes: n

 m=1

 m t Na dυ + t σ dυ – t b dυ – t t ds ρN B ρN N   = 0    υ  υ υ ∂b

where

m

m

m

(0-21)

1

N is an interpolation matrix, σ is the stress vector

σ t = ( σ xx, σ yy, σ zz, σ xy, σ yz, σ zx ) B is the strain-displacement matrix, a is the nodal acceleration vector

(0-22)

20 Preliminaries

a x1 …

x··1 a y1 = Na x··2 = N a yk x··3 a zk

(0-23)

b is the body force load vector, and t are applied traction loads. fx

tx

b = fy

t = ty

fz

tz

(0-24)

Elements 21 CHEXA Solid Elements

CHEXA Solid Elements For a mesh of 8-node hexahedron solid elements, (0-17) becomes: 8

x i ( X α, t ) = x i ( X α ( ξ ,η ,ζ ), t ) =

 φj ( ξ ,η ,ζ )xi ( t ) j

(0-25)

j=1

The shape function

φ j is defined for the 8-node hexahedron as

1 φ j = --- ( 1 + ξξ j ) ( 1 + ηη j ) ( 1 + ζζ j ) 8 where ξ j ,η j ,ζ j take on their nodal values of

(0-26)

( ± 1, ± 1, ± 1 ) and x ij is the nodal coordinate of the j th

node in the i th direction (see Figure 0-2).

ζ 5 8

6 7

ξ

4

1

η

Node 1 2 3 4 5 6 7 8

2 3

Figure 0-2

Eight-node Solid Hexahedron Element

For a solid element,

N is the 3 x 24 rectangular interpolation matrix given by

ξ

η

ζ

-1 1 1 -1 -1 1 1 -1

-1 -1 1 1 -1 -1 1 1

-1 -1 -1 -1 1 1 1 1

22 CHEXA Solid Elements

φ1 0 0 φ2 0 … 0 0 N ( ξ ,η ,ζ ) =

0 φ1 0 0 φ2 … φ8 0

(0-27)

0 0 φ 1 0 0 … 0 φ8 σ is the stress vector σ t = ( σ xx, σ yy, σ zz, σ xy, σ yz, σ zx )

(0-28)

B is the 6 x 24 strain-displacement matrix ∂ ----0 0 ∂x ∂ 0 ----- 0 ∂y ∂ 0 0 ----∂z N B = ∂ ----∂ ----0 ∂y ∂x ∂ ∂ 0 ----- ----∂z ∂y ∂ ∂ ----- 0 ----∂z ∂x

(0-29)

In order to achieve a diagonal mass matrix the rows are summed giving the

k th diagonal term as

8

m kk =

 ρφk  φi dυ

υ

i=1

=

 ρφk dυ

υ

since the basis functions sum to unity. Terms in the strain-displacement matrix are readily calculated. Note that

(0-30)

Elements 23 CHEXA Solid Elements

∂φ i ∂φ ∂x ∂φ i ∂y ∂φ i ∂z ------- = -------i ----- + ------- ------ + ------- -----∂ξ ∂x ∂ξ ∂y ∂ξ ∂z ∂ξ ∂φ ∂φ ∂x ∂φ i ∂y ∂φ i ∂z -------i = -------i -----+ ------- ------ + ------- -----∂η ∂x ∂η ∂y ∂η ∂z ∂η ∂φ i ∂φ ∂x ∂φ i ∂y ∂φ i ∂z ------- = -------i ----- + ------- ------ + ------- -----∂ζ ∂x ∂ζ ∂y ∂ζ ∂z ∂ζ

(0-31)

which can be rewritten as

∂φ i ∂φ i ∂x- ----∂y- ----∂z- ∂φ -------------i ----------∂ξ ∂x ∂ξ ∂ξ ∂ξ ∂x ∂φ ∂φ ∂x ∂y ∂z ∂φ -------i = ------ ------ ------ -------i = J -------i ∂η ∂η ∂η ∂y ∂η ∂y ∂x- ----∂y- ----∂z- ∂φi ∂φ i ∂φ i ----------------------∂ζ ∂ζ ∂ζ ∂z ∂ζ ∂z Inverting the Jacobian matrix,

∂φ i ------∂x ∂φ i = J – 1 ------∂y ∂φ i ------∂z

(0-32)

J , we can solve for the desired terms

∂φ i ------∂ξ ∂φ i ------∂η ∂φ i ------∂ζ

(0-33)

Volume Integration Volume integration is carried out with Gaussian quadrature. If volume, and

 g dυ

υ

=

g is some function defined over the

n is the number of integration points, then

–1 –1 –1 g J dξ dη dζ 1

1

is approximated by

1

(0-34)

24 CHEXA Solid Elements

n

n

n

   gjkl Jjkl wj wk wl

(0-35)

j = 1k = 1l = 1

where

w j, w k, w l are the weighting factors,

g jkl = g ( ξ j, η k, ζ l ) and

(0-36)

J is the determinant of the Jacobian matrix. For one-point quadrature

n = 1 wi = wj = w k = 2 ξ1 = η1 = ζ1 = 0

(0-37)

and we can write

 g dv

= 8g ( 0 ,0 ,0 ) J ( 0 ,0 ,0 )

Note that

(0-38)

8 J ( 0 ,0 ,0 ) approximates the element volume.

Perhaps the biggest advantage to one-point integration is a substantial savings in computer time. An antisymmetry property of the strain matrix

∂φ 1 ∂φ -------- = – --------7 ∂x i ∂x i

∂φ ∂φ --------3 = – --------5 ∂x i ∂x i

∂φ ∂φ --------2 = – --------8 ∂x i ∂x i

∂φ ∂φ --------4 = – --------6 ∂x i ∂x i

(0-39)

at ξ = η = ζ = 0 reduces the amount of effort required to compute this matrix by more than 25 times over an 8-point integration. This cost savings extends to strain and element nodal force calculations where the number of multiplies is reduced by a factor of 16. Because only one constitutive evaluation is needed, the time spent determining stresses is reduced by a factor of eight. Operation counts for the

Elements 25 CHEXA Solid Elements

constant stress hexahedron are given in Table 0-2. Included are counts for the Flanagan and Belytschko [1981] hexahedron and the hexahedron used by Wilkins [1974] in his integral finite difference method, which was also implemented [Hallquist 1979]. .

Table 0-2

Operation Counts for Constant Stress Hexahedron* Flanagan-Wilkins SOL 700

Belytschko [1981]

FDM

Strain displacement matrix

94

357

843

Strain rates

87

56

Force

117

195

270

Subtotal

298

708

1,113

Hourglass control

130

620

680

Total

428

1,328

1,793

*Includes adds, subtracts, multiplies, and divides in major subroutines, and is independent of vectorization. It may be noted that 8-point integration has another disadvantage in addition to cost. Fully integrated elements used in the solution of plasticity problems and other problems where Poisson’s ratio approaches .5 lock up in the constant volume bending modes. To preclude locking, an average pressure must be used over the elements; consequently, the zero energy modes are resisted by the deviatoric stresses. If the deviatoric stresses are insignificant relative to the pressure or, even worse, if material failure causes loss of this stress state component, hourglassing will still occur, but with no means of resisting it. Sometimes, however, the cost of the fully integrated element may be justified by increased reliability and if used sparingly may actually increase the overall speed.

Hourglass Control The biggest disadvantage to one-point integration is the need to control the zero energy modes, which arise, called hourglassing modes. Undesirable hourglass modes tend to have periods that are typically much shorter than the periods of the structural response, and they are often observed to be oscillatory. However, hourglass modes that have periods that are comparable to the structural response periods may be a stable kinematic component of the global deformation modes and must be admissible. One way of resisting undesirable hourglassing is with a viscous damping or small elastic stiffness capable of stopping the formation of the anomalous modes but having a negligible affect on the stable global modes. Two of the early three-dimensional algorithms for controlling the hourglass modes were developed by Kosloff and Frazier [1974] and Wilkins et al. [1974]. Since the hourglass deformation modes are orthogonal to the strain calculations, work done by the hourglass resistance is neglected in the energy equation. This may lead to a slight loss of energy; however, hourglass control is always recommended for the under integrated solid elements. The energy

26 CHEXA Solid Elements

dissipated by the hourglass forces reacting against the formations of the hourglass modes is tracked and reported in the output files MATSUM and GLSTAT. This is only provided if the PARM,DYENERGYGE is included. It is easy to understand the reasons for the formation of the hourglass modes. Consider the following strain rate calculations for the 8-node solid element

 8 ∂φ  1---  · k · k ∂φ k · k ------------ε ij =   x + x 2 ∂x i j ∂x j i  k = 1 

(0-1)

Whenever diagonally opposite nodes have identical velocities; i.e.,

x· i1 = x· i7, x· i2 = x· i8, x· i3 = x· i5, x· i4 = x· i6

(0-2)

the strain rates are identically zero:

· ε ij = 0

(0-3)

due to the asymmetries in (0-39). It is easy to prove the orthogonality of the hourglass shape vectors, which are listed in Table 0-3 and shown in Figure 0-2 with the derivatives of the shape functions: 8

 k=1

∂φ k -------- Γ αk = 0 ∂x i

Table 0-3

i = 1 ,2 ,3

α = 1 ,2 ,3 ,4

(0-4)

Hourglass Base Vectors

α = 1

α = 2

α = 3

α = 4

Γ j1

1

1

1

1

Γ j2

-1

1

-1

-1

Γ j3

1

-1

-1

Γ j4

-1

-1

1

-1

Γ j5

1

-1

-1

-1

Γ j6

-1

-1

1

1

Elements 27 CHEXA Solid Elements

Table 0-3

Hourglass Base Vectors

α = 1

α = 2

α = 3

α = 4

Γ j7

1

1

1

-1

Γ j8

-1

1

-1

1

The hourglass modes of an 8-node element with one integration point are shown [Flanagan and Belytschko 1981] (Figure 0-3). A total of twelve modes exist.

Figure 0-3

Γ1k

Γ2k

Γ3k

Γ4k

Hourglass Modes

The product of the base vectors with the nodal velocities 8

h iα =

 x· i Γαk k

= 0

(0-1)

k=1 k are nonzero if hourglass modes are present. The 12 hourglass-resisting force vectors, f iα are k f iα = a h h iα Γ αk

where

(0-2)

28 CHEXA Solid Elements

c a h = Q hg ρν e2 ⁄ 3 --4 in which

(0-3)

ν e is the element volume, c is the material sound speed, and Q hg is a user-defined constant

usually set to a value between .05 and .15. This is defined by DYHRGQH PARAM. The hourglass resisting forces of (0-2) are not orthogonal to rigid body rotations; however, the approach of Flanagan and Belytschko [1981] is orthogonal. This is controlled by using the DYHRGIHQ PARAM. Material subroutines add as little as 60 operations for the bilinear elastic-plastic routine to ten times as much for multi-surface plasticity and reactive flow models. Unvectorized material models will increase that share of the cost a factor of four or more. Instead of resisting components of the bilinear velocity field that are orthogonal to the strain calculation, Flanagan and Belytschko resist components of the velocity field that are not part of a fully linear field. They call this field, defined below, the hourglass velocity field HG LIN x· ik = x· i – x· ik

(0-4)

where LIN · · x· ik = x i + x i ,j ( x jk – x j )

8

1 x i = --8



(0-5) 8

1 · x i = --8

x ik

k=1

 x· i

k

(0-6)

k=1

Flanagan and Belytschko construct geometry-dependent hourglass shape vectors that are orthogonal to the fully linear velocity field and the rigid body field. With these vectors they resist the hourglass velocity deformations. Defining hourglass shape vectors in terms of the base vectors as 8

γ ak = Γ ak – φ k ,i

 x i Γan n

n=1

(0-7)

Elements 29 CHEXA Solid Elements

and setting 8

g ia =

 x· i γαk k

= 0

(0-8)

k=1

the 12 resisting force vectors become k f iα = a h g iα γ αk

where

(0-9)

a h is a constant given in (0-2).

The hourglass forces given by (0-2) and (0-9) are identical if the, hexahedron element is a parallelepiped. The default hourglass control method for solid element is given by (0-2); however, we recommend the Flanagan-Belytschko approach for problems that have large rigid body rotations since the default approach is not orthogonal to rigid body rotations. A cost comparison in Table 0-2 shows that the default hourglass viscosity requires approximately 130 adds or multiplies per hexahedron, compared to 620 and 680 for the algorithms of Flanagan-Belytschko and Wilkins. Hourglass stabilization for the 3-D hexahedral element is available. Based on material properties and element geometry, this stiffness type stabilization is developed by an assumed strain method [Belytschko and Bindeman 1993] such that the element does not lock with nearly incompressible material. This is activated by using the PARAM,DYHRGIHG,6. When the user-defined hourglass constant

Q hg is set to

1.0, accurate coarse mesh bending stiffness is obtained for elastic material. For nonlinear material, a smaller value of

Q hg is suggested and the default value is set to 0.1.

Fully Integrated Brick Elements and Mid-Step Strain Evaluation To avoid locking in the fully integrated brick elements strain increments at a point in a constant pressure, solid element are defined by [see Nagtegaal, Parks, and Rice 1974]

30 CHEXA Solid Elements

∂Δu Δε xx = -----------------+φ ∂x n + 1 ⁄ 2

Δε xy

∂Δv Δε yy = -----------------+φ ∂y n + 1 ⁄ 2

Δε yz

∂Δw Δε zz = -----------------+φ ∂z n + 1 ⁄ 2

Δε zx

∂Δν - -----------------∂Δu -----------------+ n + 1 ⁄ -2 n + 1⁄2 ∂x ∂y = --------------------------------------------2 ∂Δw - -----------------∂Δv -----------------+ ∂y n + 1 ⁄ 2 ∂z n + 1 ⁄ 2 = -------------------------------------------2 ∂Δu ∂Δw -----------------+ -----------------n + 1⁄2 ∂z ∂x n + 1 ⁄ 2 = -------------------------------------------2

(0-10)

where φ modifies the normal strains to ensure that the total volumetric strain increment at each integration point is identical

∂Δu - -----------------∂Δν - -----------------∂Δw -----------------+ + ∂x n + 1 ⁄ 2 ∂y n + 1 ⁄ 2 ∂z n + 1 ⁄ 2 φ = Δε vn + 1 ⁄ 2 – ---------------------------------------------------------------------3 and

n+1⁄2

Δε ν

(0-11)

is the average volumetric strain increment in the midpoint geometry

1--∂Δu - -----------------∂Δν - -----------------∂Δw  n + 1 ⁄ 2  -----------------+ + dv 3   ∂x n + 1 ⁄ 2 ∂y n + 1 ⁄ 2 ∂z n + 1 ⁄ 2 vn + 1 ⁄ 2 ---------------------------------------------------------------------------------------------------------------n + 1⁄2  dv

(0-12)

vn + 1 ⁄ 2

Δu, Δv , and Δw are displacement increments in the x, y , and z directions, respectively, and (xn + xn + 1 ) x n + 1 ⁄ 2 = ---------------------------2

(0-13)

(yn + yn + 1 ) y n + 1 ⁄ 2 = ---------------------------2

(0-14)

( zn + zn + 1) z n + 1 ⁄ 2 = ---------------------------2

(0-15)

Elements 31 CHEXA Solid Elements

To satisfy the condition that rigid body rotations cause zero straining, it is necessary to use the geometry at the mid-step in the evaluation of the strain increments. The explicity formulation uses the geometry at step n + 1 to save operations; however, for calculations, which involve rotating parts, the mid-step geometry should be used especially if the number of revolutions is large. Since the bulk modulus is constant in the plastic and viscoelastic material models, constant pressure solid elements result. In the thermoelastoplastic material, a constant temperature is assumed over the element. In the soil and crushable foam material, an average relative volume is computed for the element at time step n + 1 , and the pressure and bulk modulus associated with this relative volume is used at each integration point. For equations of state, one pressure evaluation is done per element and is added to the deviatoric stress tensor at each integration point. The foregoing procedure requires that the strain-displacement matrix corresponding to (0-10) and consistent with a constant volumetric strain, It is easy to show that:

F =

 vn + 1

B n + 1 σ n + 1 dv n + 1 = t



B , be used in the nodal force calculations [Hughes 1980].

B n + 1 σ n + 1 dv n + 1 t

(0-16)

vn + 1

and avoid the needless complexities of computing

B.

CTETRA - Four Node Tetrahedron Element The four node tetrahedron element with one point integration, shown in Figure 0-4, is a simple, fast, solid element that has proven to be very useful in modeling low density foams that have high compressibility. For most applications, however, this element is too stiff to give reliable results and is primarily used for transitions in meshes. The formulation follows the formulation for the one point solid element with the difference that there are no kinematic modes, so hourglass control is not needed. The basis functions are given by:

32 CHEXA Solid Elements

N 1 ( r, s, t ) N 2 ( r, s, t ) N 3 ( r, s, t ) N 4 ( r, s, t )

= = = =

r s 1–r–s– t

(0-17)

t

4

3

1 r

2 s

Figure 0-4

Four-node tetrahedron

If a tetrahedron element is needed, this element should be used instead of the collapsed solid element since it is, in general, considerably more stable in addition to being much faster.

CPENTA - Six Node Pentahedron Element The pentahedron element with two point Gauss integration along its length, shown in Figure 0-5, is a solid element that has proven to be very useful in modeling axisymmetric structures where wedge shaped elements are used along the axis-of-revolution. The formulation follows the formulation for the one point solid element with the difference that, like the tetrahedron element, there are no kinematic modes, so hourglass control is not needed. The basis functions are given by:

Elements 33 CHEXA Solid Elements

1 N 1 ( r, s, t ) = --- ( 1 – t )r 2 1 N 2 ( r, s, t ) = --- ( 1 – t ) ( 1 – r – 2 1 N 3 ( r, s, t ) = --- ( 1 + t ) ( 1 – r – 2 1 N 4 ( r, s, t ) = --- ( 1 + t )r 2 1 N 5 ( r, s, t ) = --- ( 1 – t )s 2 1 N 6 ( r, s, t ) = --- ( 1 + t )s 2

(0-18)

If a pentahedron element is needed, this element should be used instead of the collapsed solid element since it is, in general, more stable and significantly faster. Selective-reduced integration is used to prevent volumetric locking; i.e., a constant pressure over the domain of the element is assumed. t

4 6

r 2

s

1 5

Figure 0-5

Six Node Pentahedron

34 CBEAM - Belytschko Beam

CBEAM - Belytschko Beam The Belytschko beam element formulation [Belytschko et. al.1977] is part of a family of structural finite elements, by Belytschko and other researchers that employ a ‘co-rotational technique’ in the element formulation for treating large rotation. This section discusses the co-rotational formulation, since the formulation is most easily described for a beam element, and then describes the beam theory used to formulate the co-rotational beam element.

Co-rotational Technique In any large displacement formulation, the goal is to separate the deformation displacements from the rigid body displacements, as only the deformation displacements give rise to strains and the associated generation of strain energy. This separation is usually accomplished by comparing the current configuration with a reference configuration. The current configuration is a complete description of the deformed body in its current spatial location and orientation, giving locations of all points (nodes) comprising the body. The reference configuration can be either the initial configuration of the body (i.e., nodal locations at time zero) or the configuration of the body at some other state (time). Often, the reference configuration is chosen to be the previous configuration, say at time t n

= t n + 1 – Δt .

The choice of the reference configuration determines the type of deformations that will be computed: total deformations result from comparing the current configuration with the initial configuration, while incremental deformations result from comparing with the previous configuration. In most time stepping (numerical) Lagrangian formulations, incremental deformations are used because they result in significant simplifications of other algorithms, chiefly constitutive models. A direct comparison of the current configuration with the reference configuration does not result in a determination of the deformation, but rather provides the total (or incremental) displacements. We will use the unqualified term displacements to mean either the total displacements or the incremental displacements, depending on the choice of the reference configuration as the initial or the last state. This is perhaps most obvious if the reference configuration is the initial configuration. The direct comparison of the current configuration with the reference configuration yields displacements, which contain components due to deformations and rigid body motions. The task remains of separating the deformation and rigid body displacements. The deformations are usually found by subtracting from the displacements an estimate of the rigid body displacements. Exact rigid body displacements are usually only known for trivial cases where they are prescribed a priori as part of a displacement field. The co-rotational formulations provide one such estimate of the rigid body displacements. The co-rotational formulation uses two types of coordinate systems: one system associated with each element; i.e., element coordinates which deform with the element, and another associated with each node; i.e., body coordinates embedded in the nodes. (The term ‘body’ is used to avoid possible confusion from referring to these coordinates as ‘nodal’ coordinates. Also, in the more general formulation presented in

Elements 35 CBEAM - Belytschko Beam

[Belytschko et al., 1977], the nodes could optionally be attached to rigid bodies. Thus, the term ‘body coordinates’ refers to a system of coordinates in a rigid body, of which a node is a special case.) These two coordinate systems are shown in the upper portion of Figure 0-6.

Y

^ Y

b2 0

e2

0

e1

^ X

b1 J

I X (a) Initial Configuration ^X J

Y ^Y

b2 e1 e2 X I

b1 (b) Rigid Rotation Configuration ^ Y

Y b2

^ X

e2 e1

J

0

e1 b1

X (c) Deformed Configuration

Figure 0-6

Co-rotational Coordinate System

36 CBEAM - Belytschko Beam

xˆ originating at node I and terminating at node J ; the local y-axis yˆ and, in three dimension, the local z-axis zˆ , are constructed normal to xˆ . The element coordinate system ( xˆ , yˆ , zˆ ) and associated unit vector triad ( e , e , e ) are The element coordinate system is defined to have the local x-axis

1

2

3

updated at every time step by the same technique used to construct the initial system; thus the unit vector

e 1 deforms with the element since it always points from node I to node J . The embedded body coordinate system is initially oriented along the principal inertial axes; either the assembled nodal mass or associated rigid body inertial tensor is used in determining the inertial principal values and directions. Although the initial orientation of the body axes is arbitrary, the selection of a principal inertia coordinate system simplifies the rotational equations of motion; i.e., no inertial cross product terms are present in the rotational equations of motion. Because the body coordinates are fixed in the node (or rigid body), they rotate and translate with the node and are updated by integrating the rotational equations of motion, as will be described subsequently. The unit vectors of the two coordinate systems define rotational transformations between the global coordinate system and each respective coordinate system. These transformations operate on vectors with

A = ( A x, A y, A z ) , body coordinates components A = A x, A y, Az , and ˆ ˆ ˆ ˆ element coordinate components A = A , A , A which are defined as: global components

x

   Ax  b 1x b 2x b 3x   A =  A y  = b 1y b 2y b 3y   b 1z b 2z b 3z  Az   

y

z

   Ax     Ay  = [ λ ] { A }    Az   

(0-19)

where b ix, b iy, b iz are the global components of the body coordinate unit vectors. Similarly for the element coordinate system:

   Ax  e 1x e 2x e 3x   A =  A y  = e 1y e 2y e 3y   e 1z e 2z e 3z  Az   

      

ˆ Ax ˆ Ay ˆ Az

   ˆ  = [μ]{A}   

(0-20)

where e ix, e iy, e iz are the global components of the element coordinate unit vectors. The inverse transformations are defined by the matrix transpose: i.e.,

Elements 37 CBEAM - Belytschko Beam

T

{A} = [λ] {A}

(0-21)

T ˆ {A} = [μ] {A}

(0-22)

since these are proper rotational transformations. The following two examples illustrate how the element and body coordinate system are used to separate the deformations and rigid body displacements from the displacements. Rigid Rotation First, consider a rigid body rotation of the beam element about node I , as shown in the center of

I to be a pinned connection. Because the beam does not deform during the rigid rotation, the orientation of the unit vector e 1 in the initial and rotated configuration will be the Figure 0-6b; i.e., consider node

same with respect to the body coordinates. If the body coordinate components of the initial element unit vector e 10 were stored, they would be identical to the body coordinate components of the current element unit vector e 1 . Deformation Rotation Next, consider node I to be constrained against rotation; i.e., a clamped connection. Now node J is moved, as shown in the lower portion of Figure 0-6, causing the beam element to deform. The updated element unit vector e 1 is constructed and its body coordinate components are compared to the body coordinate components of the original element unit vector e 10 . Because the body coordinate system did not rotate, as node I was constrained, the original element unit vector and the current element unit vector are not co-linear. Indeed, the angle between these two unit vectors is the amount of rotational deformation at node I ; i.e.,

e 1 × e 10 = θ  e 3

(0-23)

Thus the co-rotational formulation separates the deformation and rigid body deformations by using: • a coordinate system that deforms with the element; i.e., the element coordinates or • a coordinate system that rigidly rotates with the nodes; i.e., the body coordinates.

Then, it compares the current orientation of the element coordinate system with the initial element coordinate system, using the rigidly rotated body coordinate system, to determine the deformations.

Belytschko Beam Element Formulation The deformation displacements used in the Belytschko beam element formulation are:

38 CBEAM - Belytschko Beam

ˆT ˆ ˆ ˆ ˆ ˆ d = { δ IJ, θ xJI, θ yI, θ yJ, θ zI, θ zJ }

(0-24)

where

δ IJ = length change ˆ θ xJI = torsional deformation ˆ ˆ ˆ ˆ θ yI, θ yJ, θ zI, θzJ = bending rotational deformations The superscript and

ˆ emphasizes that these quantities are defined in the local element coordinate system,

I and J are the nodes at the ends of the beam.

The beam deformations, defined in (0-19), are the usual small displacement beam deformations (see, for example, [Przemieniecki 1986]). Indeed, one advantage of the co-rotational formulation is the ease with which existing small displacement element formulations can be adapted to a large displacement formulation having small deformations in the element system. Small deformation theories can be easily accommodated because the definition of the local element coordinate system is independent of rigid body rotations and hence deformation displacement can be defined directly.

Calculation of Deformations The elongation of the beam is calculated directly from the original nodal coordinates the total displacements

( XI, Y I, Z I ) and

( uxI, u yI, u zI ) :

1 2 2 2 δ IJ = -----------o- [ 2 ( X JI u xJI + Y JI u yJI + Z JI u zJI ) + u xJI + u yJI + u zJI ] l+l

(0-25)

where

X JI = X J – X I

(0-26)

u xJI = u xJ – u xI etc.

(0-27)

The deformation rotations are calculated using the body coordinate components of the original element coordinate unit vector along the beam axis; i.e., e 10 , as outlined in the previous section. Because the body coordinate components of initial unit vector e 10 rotate with the node, in the deformed configuration it

Elements 39 CBEAM - Belytschko Beam

indicates the direction of the beam’s axis if no deformations had occurred. Thus comparing the initial unit vector e 10 with its current orientation e 1 indicates the magnitude of deformation rotations. Forming the vector cross product between e 10 and e 1 :

ˆ ˆ e 1 × e 10 = θ y e 2 + θ z e 3

(0-28)

where

ˆ θ y is the incremental deformation about the local yˆ axis ˆ θ z is the incremental deformation about the local zˆ axis The calculation is most conveniently performed by transforming the body components of the initial element vector into the current element coordinate system:

      

  0 0 eˆ 1x   e 1x   0  = [ μ]T[λ ] 0 e 1y eˆ 1y   0  0  e 1z eˆ 1z  

      

(0-29)

Substituting the above into (0-28)

e1 e2 e3

e1 ×

e 10

ˆ ˆ 0 0 = det 1 0 0 = – eˆ 1z e 2 + eˆ 1y e3 = θy e2 + θz e3 0 ˆ0 ˆ0 eˆ 1x e 1y e 1z

(0-30)

Thus, 0 θˆy = – eˆ 1z

(0-31)

0 θˆz = eˆ 1y

(0-32)

40 CBEAM - Belytschko Beam

The torsional deformation rotation is calculated from the vector cross product of initial unit vectors, from 0 0 0 each node of the beam, that were normal to the axis of the beam, i.e., eˆ 2I and eˆ 2J ; note that eˆ 3I and 0 eˆ 3J could also be used. The result from this vector cross product is then projected onto the current axis

of the beam; i.e.,

e1

e2

e3

ˆ 0 0 0 ˆ0 0 ˆ0 0 0 0 θ xJI = e 1 ⋅ ( eˆ 2I × eˆ 2J ) = e 1 det eˆ x2I = eˆ y2I e z2J – eˆ y2J e z2I eˆ y2I eˆ z2I

(0-33)

0 0 0 eˆ x2J eˆ y2J eˆ z2J 0 0 Note that the body components of e 2I and e 2J are transformed into the current element coordinate system before performing the indicated vector products.

Calculation of Internal Forces There are two methods for computing the internal forces for the Belytschko beam element formulation: • Functional forms relating the overall response of the beam- e.g., moment-curvature relations, • Direct through-the-thickness integration of the stress.

Currently only the former method, as explained subsequently, is implemented; the direct integration method is detailed in [Belytschko et al., 1977]. Axial Force The internal axial force is calculated from the elongation of the beam axial stiffness:

ˆ f xJ = K a δ where:

K a = AE ⁄ l 0 is the axial stiffness A is the cross sectional area of the beam E is Young’s Modulus l 0 is the original length of the beam

δ , as given by (0-25), and an

(0-34)

Elements 41 CBEAM - Belytschko Beam

Bending Moments The bending moments are related to the deformation rotations by

ˆ  θyI  ˆ   θ yJ 

(0-35)

b ˆ K z 4 + φ z 2 – φ z  θˆ zI   m zI   ˆ  = ------------1 + φ z 2 – φ 4 + φ  θˆ   m zJ  zJ z z

(0-36)

ˆ K yb 4 + φ y 2 – φ y  m yI  ------------= ˆ  1 + φy 2 – φ 4 + φ  m yJ  y y

where (0-35) is for bending in the constants are given by

xˆ – zˆ plane and (0-36) is for bending in the xˆ – yˆ plane. The bending

EI yy b K y = --------l0

(0-37)

EI zz b K z = --------l0

(0-38)

I yy =

  zˆ 2 dyˆ dzˆ

(0-39)

I zz =

  yˆ 2 dyˆ dzˆ

(0-40)

12EI yy φ y = ---------------GA s l 2 Hence

12EI zz φ z = ---------------2GA s l

(0-41)

φ is the shear factor, G the shear modulus, and A s is the effective area in shear.

Torsional Moment The torsional moment is calculated from the torsional deformation rotation as

ˆ = K t θˆ xJI m xJ where

(0-42)

42 CBEAM - Belytschko Beam

GJK t = -----l0 J =

(0-43)

  yˆ zˆ dyˆ dzˆ

(0-44)

The above forces are conjugate to the deformation displacements given previously in (0-24); i.e.,

ˆT ˆ ˆ ˆ ˆ ˆ d = { δ IJ, θ xJI, θ yI, θ yJ, θ zI, θ zJ }

(0-45)

where

ˆ T ˆ int {d} {f} = W

(0-46)

ˆT ˆ ˆ ˆ ˆ ˆ ˆ f = { f xJ, m xJ, m yI, m yJ, m zI, m zJ }

(0-47)

The remaining internal force components are found from equilibrium:

ˆ ˆ f xI = –f xJ ˆ +m ˆ m ˆ yI yJ f zI = – ---------------------0 l ˆ +m ˆ m ˆ zI zJ f yJ = – ---------------------0 l

ˆ = –m ˆ m xI xJ ˆ ˆ f zI = – f zJ (0-48)

ˆ ˆ f yI = – f yJ

Updating the Body Coordinate Unit Vectors The body coordinate unit vectors are updated using the Newmark

β -Method [Newmark 1959] with

β = 0 , which is almost identical to the central difference method [Belytschko 1974]. In particular, the body component unit vectors are updated using the formula j

j+1 bi

=

j bi

j

dbi Δt 2 d 2 b i + Δt -------- + -------- --------dt 2 dt 2

(0-49)

where the superscripts refer to the time step and the subscripts refer to the three unit vectors comprising the body coordinate triad. The time derivatives in the above equation are replaced by their equivalent forms from vector analysis: j

db --------i = ω × b i dt

(0-50)

Elements 43 CBEAM - Belytschko Beam

j

d2 bi ---------- = ω × ( ω × b i ) + ( α i × b i ) dt 2

(0-51)

where ω and α are vectors of angular velocity and acceleration, respectively, obtained from the rotational equations of motion. With the above relations substituted into (0-49), the update formula for the unit vectors becomes j+1

bi

Δt 2 j = bi + Δt ( ω × b i ) + -------- { [ ω × ( ω × b i ) + ( α i × b i ) ] } 2

(0-52)

To obtain the formulation for the updated components of the unit vectors, the body coordinate system is temporarily considered to be fixed and then the dot product of (0-52) is formed with the unit vector to be updated. For example, to update the formed with j+1

b x3

x component of b 3 , the dot product of (0-52), with i = 3 , is

b 1 , which can be simplified to the relation j

j+1

j

j+1

j

j+1

= b1 ⋅ b y3

Δt 2 j j j j = Δtω y + -------- ( ω x ω z + αy ) 2

(0-53)

Δt 2 j j j j = Δtω x + -------- ( ω y ω z + αx ) 2

(0-54)

Δt 2 j j j j = Δtω z + -------- ( ω x ω y + αz ) 2

(0-55)

Similarly, j+1

= b2 ⋅ b 3

j+1

= b1 ⋅ b 2

b y3 b x2

j+1

The remaining components b 3

j+1

and b 1

is assumed that the angular velocities

ω are small during a time step so that the quadratic terms in the j+1

update relations can be ignored. Since b 3 j+1

b z3

=

j+1 2

are found by using normality and orthogonality, where it

is a unit vector, normality provides the relation

j+1 2

1 – ( b x3 ) – ( b y3 )

Next, if it is assumed that

j+1

b x1 ≈ 1 , orthogonality yields

(0-56)

(0-57)

44 CBEAM - Belytschko Beam

j+1

j+1 b z1

j+1 j+1

b x3 + b y1 by3 = – ----------------------------------------j+1 b z3 j+1

The component b x1 j+1

b x1

=

(0-58)

is then found by enforcing normality:

j+1 2

j+1 2

1 – ( b y1 ) – ( b z1 )

The updated components of

(0-59)

b 1 and b 3 are defined relative to the body coordinates at time step j . To

j + 1 , the updated unit vectors b 1 and b 3 are transformed to the global coordinate system, using (0-19) with [ λ ] defined at complete the update and define the transformation matrix, (0-19), at time step

step j , and their vector cross product is used to form

b2

Elements 45 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

CBEAM - DYSHELFORM = 1, Hughes-Liu Beam The Hughes-Liu beam element formulation, based on the shell [Hughes and Liu 1981a, 1981b] discussed later. It has several desirable qualities: • It is incrementally objective (rigid body rotations do not generate strains), allowing for the

treatment of finite strains that occur in many practical applications. • It is simple, which usually translates into computational efficiency and robustness. • It is compatible with the brick elements, because the element is based on a degenerated brick

element formulation. • It includes finite transverse shear strains. The added computations needed to retain this strain

component, compare to those for the assumption of no transverse shear strain, are insignificant.

Geometry The Hughes-Liu beam element is based on a degeneration of the isoparametric 8-node solid element, an approach originated by Ahmad et al., [1970]. Recall the solid element isoparametric mapping of the biunit cube

x ( ξ ,η ,ζ ) = N a ( ξ ,η ,ζ )x a

(0-60)

( 1 + ξa ξ ) ( 1 + ηa η ) ( 1 + ζa ζ ) N a ( ξ ,η ,ζ ) = ----------------------------------------------------------------------8

(0-61)

where

x is an arbitrary point in the element, ( ξ ,η ,ζ ) are the parametric coordinates, x a are the global

nodal coordinates of node

a , and N a are the element shape functions evaluated at node a , i.e.,

ξ a ,η a ,ζ a are ( ξ ,η ,ζ ) evaluated at node a . In the beam geometry, ξ determines the location along the axis of the beam and the coordinate pair

( η ,ζ ) defines a point on the cross section. To degenerate the 8-node brick geometry into the 2-node beam geometry, the four nodes at ξ = – 1 and at ξ = 1 are combined into a single node with three translational and three rotational degrees of freedom. Orthogonal, inextensible nodal fibers are defined at each node for treating the rotational degrees of freedom. Figure 0-7 shows a schematic of the bi-unit cube and the beam element. The mapping of the bi-unit cube into the beam element is separated into three parts:

x ( ξ ,η ,ζ ) = x ( ξ ) + X ( ξ ,η ,ζ ) = x ( ξ ) + X ζ ( ξ ,ζ ) + X η ( ξ ,η )

(0-62)

46 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

ζ Bi-unit Cube

ζ

x

η

ξ

η

Beam Element

ξ Nodal Fibers

+

zζ

Top Surface +1

+

Xζ

ζ

Xζ ˆ Xζ ˆ X

0

η

Xζ -1 Bottom Surface

Figure 0-7 where

zζ

Hughes-Liu Beam Element

x denotes a position vector to a point on the reference axis of the beam, and Xζ and X η are

position vectors at point

x ( ξ ) = N a ( ξ )x a

x on the axis that define the fiber directions through that point. In particular, (0-63)

Elements 47 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

X η ( ξ, η ) = N a ( ξ )X ηa ( η )

(0-64)

X ζ ( ξ, ζ ) = N a ( ξ )X ζa ( ζ )

(0-65)

With this description, arbitrary points on the reference line shape function

x are interpolated by the one- dimensional

N ( ξ ) operating on the global position of the two beam nodes that define the reference

axis, i.e., x a . Points off the reference axis are further interpolated by using a one-dimensional shape function along the fiber directions; i.e.,

Xη a ( η ) and X ζa ( ζ ) where

ˆ X ηa ( η ) = z η ( η )X ηa

(0-66)

+ + N ( η )z z η ( η ) = N + ( η )z ηa ηa

(0-67)

(1 + η) N + ( η ) = ----------------2

(0-68)

( 1 – η) N - ( η ) = ----------------2

(0-69)

ˆ X ζa ( ζ ) = z ζ ( ζ )X ζa

(0-70)

+ + N ( ζ )z z ζ ( ζ ) = N + ( ζ )z ζa ζa

(0-71)

(1 + ζ) N + ( ζ ) = ----------------2

(0-72)

(1 – ζ) N - ( ζ ) = ---------------2

(0-73)

where z ζ ( ζ ) and z η ( η ) are “thickness functions”. The Hughes-Liu beam formulation uses four position vectors, in addition to

ξ , to locate the reference

+ and x - located on axis and define the initial fiber directions. Consider the two position vectors x ζa ζa

the top and bottom surfaces, respectively, at node

1 – + ( 1 + ζ ) ]x + x ζa = --- [ ( 1 – ζ )x ηa ζa 2

a . Then (0-74)

48 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

+ – x- ) x ζa ζa ˆX = (------------------------ζa + x ζa – x ζa

(0-75)

+ = 1 + – x--- ( 1 – ζ ) ⋅ x ζa z ζa ζa 2

(0-76)

- = –1 + – x--- ( 1 + ζ ) ⋅ x ζa z ζa ζa 2

(0-77)

1 – + ( 1 + ζ ) ]x + x ηa = --- [ ( 1 – ζ )x ηa ηa 2

(0-78)

+ – x- ) ( x ηa ηa ˆ X ηa = -------------------------+ x ηa – x ηa

(0-79)

+ = 1 + – x--- ( 1 – η ) ⋅ x ηa z ηa ηa 2

(0-80)

- = –1 + – x--- ( 1 + η ) ⋅ x ηa z ηa ηa 2

(0-81)

.

where is the Euclidean norm. The reference surface may be located at the midsurface of the beam or offset at the outer surfaces. This capability is useful in several practical situations involving contact surfaces, connection of beam elements to solid elements, and offsetting elements such as for beam stiffeners in stiffened shells. The reference surfaces are located within the beam element by specifying the value of the parameters

η and ζ , (see lower portion of Figure 0-7). When these parameters take on

the values – 1 or +1 , the reference axis is located on the outer surfaces of the beam. If they are set to zero, the reference axis is at the center. The same parametric representation used to describe the geometry of the beam elements is used to interpolate the beam element displacements; i.e., an isoparametric representation. Again, the displacements are separated into the reference axis displacements and rotations associated with the fiber directions:

u ( ξ, η, ζ ) = u ( ξ ) + U ( ξ, η, ζ ) = u ( ξ ) + U ζ ( ξ, ζ ) + U η ( ξ, η )

(0-82)

u ( ξ ) = N a ( ξ )u a

(0-83)

U η ( ξ, η ) = N a ( ξ )U ηa ( η )

(0-84)

Elements 49 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

U ζ ( ξ, ζ ) = N a ( ξ )U ζa ( ζ )

(0-85)

ˆ U ηa ( η ) = z ηa ( η )U ηa

(0-86)

ˆ U ζa ( ζ ) = z ζa ( ζ )U ζa

(0-87)

where u is the displacement of a generic point,

u is the displacement of a point on the reference surface,

and U is the ‘fiber displacement’ rotations. The motion of the fibers can be interpreted as either displacements or rotations as will be discussed. Hughes and Liu introduced the notation that follows, and the associated schematic shown in Figure 0-8, to describe the current deformed configuration with respect to the reference configuration:

y = y+Y

(0-88)

y = x+u

(0-89)

ya = xa + ua

(0-90)

Y = X+U

(0-91)

Ya = Xa + Ua

(0-92)

ˆ ˆ ˆ Y ηa = X ηa + U ηa

(0-93)

ˆ Yˆ ζa = Xˆ ζa + U ζa

(0-94)

u X

Parallel Construction Reference axis in undeformed geometry

x

y u

x

Figure 0-8

U

Y

y Deformed Configuration Reference Surface

Schematic of Deformed Configuration Displacements and Position Vectors

50 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

x quantities refer to the reference configuration, the y quantities refer to the updated (deformed) configuration and the u quantities are the displacements. The notation consistently uses a superscript bar ( ) to indicate reference surface quantities, a superscript caret ( ˆ ) to indicate unit vector quantities, lower case letter for translational displacements, and upper

In the above relations, and in Figure 0-8, the

case letters for fiber displacements. Thus to update to the deformed configuration, two vector quantities are needed: the reference surface displacement u and the associated nodal fiber displacement U . The nodal fiber displacements are defined in the fiber coordinate system, described in the next subsection.

Fiber Coordinate System For a beam element, the known quantities will be the displacements of the reference surface u obtained from the translational equations of motion and the rotational quantities at each node obtained from the rotational equations of motion. What remains to complete the kinematics is a relation between nodal

U . The linearized relationships between the incremental components ˆ ΔU the incremental rotations are given by

rotations and fiber displacements

 ˆ  ΔU η1  ˆ  ΔU η2  ˆ  ΔU η3 

  0 Yˆ η3 – Yˆ η2   = – Yˆ η3 0 Yˆ η1  ˆ ˆ  Y η2 – Y η1 0 

 ˆ  ΔU ζ1  ˆ  ΔU ζ2  ˆ  ΔU ζ3 

  0 Yˆ ζ3 – Yˆ ζ2   = – Yˆ ζ3 0 Yˆ ζ1   Yˆ ζ2 – Yˆ ζ1 0 

   Δθ 1     Δθ 2  = h η Δθ    Δθ 3       Δθ 1     Δθ 2  = h ζ Δθ    Δθ 3   

(0-95)

(0-96)

(0-95) and (0-96) are used to transform the incremental fiber tip displacements to rotational increments in the equations of motion. The second-order accurate rotational update formulation due to Hughes and Winget [1980] is used to update the fiber vectors: n+1 n Yˆ ηi = R ij ( Δθ )Yˆ ηj

(0-97)

n+1 n Yˆ ζi = R ij ( Δθ )Yˆ ζi

(0-98)

then

Elements 51 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

ˆ ˆn+1 ˆn ΔU ηa = Y ηa – Y ηa

(0-99)

ˆ ˆn+1 ˆn ΔU ζa = Y ζa – Y ζa

(0-100)

where

( 2δ ik + ΔS ik )ΔS jk R ij ( Δθ ) = δ ij + ------------------------------------------2D

(0-101)

ΔS ij = e ikj Δθ k

(0-102)

1 2D = 2 + --- ( Δθ 12 + Δθ 22 + Δθ32 ) 2

(0-103)

Here

δ ij is the Kronecker delta and e ikj is the permutation tensor.

Local Coordinate System In addition to the above described fiber coordinate system, a local coordinate system is needed to enforce the zero normal stress conditions transverse to the axis. The orthonormal basis with two directions eˆ 2 and eˆ 3 normal to the axis of the beam is constructed as follows:

y2 – y1 eˆ 1 = -------------------y2 – y1 e 2′

Yˆ η1 + Yˆ η2 --------------------------= ˆ ˆ Y η1 + Y η2

(0-104)

(0-105)

From the vector cross product of these local tangents.

eˆ 3 = eˆ 1 × e 2′

(0-106)

and to complete this orthonormal basis, the vector

eˆ 2 = eˆ 3 × eˆ 1

(0-107)

is defined. This coordinate system rigidly rotates with the deformations of the element. The transformation of vectors from the global to the local coordinate system can now be defined in terms of the basis vectors as

52 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

   ˆ A =    

ˆ Ax ˆ Ay ˆ Az

  e 1x   = e 1y  e 1z  

e 2x e 2y e 2z

 T e 3x  A x    e 3y  A y  = [ q ] { A }   e 3z  A z   

where e ix, e iy, e iz are the global components of the local coordinate unit vectors, local coordinates, and

(0-108)

ˆ A is a vector in the

A is the same vector in the global coordinate system.

Strains and Stress Update Incremental Strain and Spin Tensors The strain and spin increments are calculated from the incremental displacement gradient

∂Δu i G ij = ----------∂y j where

(0-109)

Δu i are the incremental displacements and y j are the deformed coordinates. The incremental

strain and spin tensors are defined as the symmetric and skew-symmetric parts, respectively, of

G ij :

1 Δε ij = --- ( G ij + G ji ) 2

(0-110)

1 Δω ij = --- ( G ij – G ji ) 2

(0-111)

The incremental spin tensor

Δω ij is used as an approximation to the rotational contribution of the

Jaumann rate of the stress tensor. Here the Jaumann rate update is approximated as n n σ ij = σ ijn + σ ip Δω pj + σ jp Δω pi

(0-112)

where the superscripts on the stress tensor refer to the updated ( n + 1 ) and reference ( n ) configurations. This update of the stress tensor is applied before the constitutive evaluation, and the stress and strain are stored in the global coordinate system.

Elements 53 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

Stress Update To evaluate the constitutive relation, the stresses and strain increments are rotated from the global to the local coordinate system using the transformation defined previously in (0-108), viz. n

σ ijl = q ik σ kn q jn

(0-113)

Δε ijl = q ik Δε kn q jn

(0-114)

where the superscript l indicates components in the local coordinate system. The stress is incrementally updated: n+1 σ ijl

=

n σ ijl

+

1 n + --2

Δσ ijl

(0-115)

and rotated back to the global system: n+1

l σ ijn + 1 = qki σ kn qnj

(0-116)

before computing the internal force vector. Incremental Strain-Displacement Relations After the constitutive evaluation is completed, the fully updated stresses are rotated back to the global coordinate system. These global stresses are then used to update the internal force vector

f aint =

 Ba σ dυ T

int

where f a

are the internal forces at node

(0-117)

a and B a is the strain-displacement matrix in the global

coordinate system associated with the displacements at node a . The B matrix relates six global strain components to eighteen incremental displacements [three translational displacements per node and the six incremental fiber tip displacements of (0-99)]. It is convenient to partition the

B = [ B 1, B 2 ] Each

B matrix: (0-118)

B a sub matrix is further partitioned into a portion due to strain and spin with the following sub

matrix definitions:

54 CBEAM - DYSHELFORM = 1, Hughes-Liu Beam

Ba =

B1

0

0

B4

0

0

B7

0

0

0

B2

0

0

B5

0

0

B8

0

0

0

B3

0

0

B6

0

0

B9

B2

B1

0

B5

B4

0

B8

B7

0

0

B3

B2

0

B6

B5

0

B9

B8

B3

0

B1

B6

0

B4

B9

0

B7

(0-119)

where

∂N a N a, i = --------∂y i

for i = 1,2,3

∂ ( N a z ηa ) ( N aηa ) ,( i – 3 ) = ---------------------- for i = 4,5,6 ∂y i – 3 ∂ ( N a z ηa ) ( N a z ζa ) ,( i – 6 ) = ---------------------- for i = 7,8,9 ∂y i – 6

Bi =

(0-120)

With respect to the strain-displacement relations, note that: • The derivative of the shape functions are taken with respect to the global coordinates;

B matrix is computed on the cross-section located at the mid-point of the axis; The resulting B matrix is a 6 × 18 matrix.

• The •

The internal force, f , given by

f ′ = T t f aint

(0-121)

is assembled into the global right hand side internal force vector.

I T = 0

0 hη

0

hζ

where

I is a 3 × 3 identity matrix.

T is defined as (also see (0-95)):

(0-122)

Elements 55 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell The Belytschko-Lin-Tsay shell element ([Belytschko and Tsay 1981], [Belytschko et al., 1984a]) was implemented as a computationally efficient alternative to the Hughes-Liu shell element. For a shell element with five through thickness integration points, the Belytschko-Lin-Tsay shell elements requires 725 mathematical operations compared to 4050 operations for the under integrated Hughes-Liu element. The selectively reduced integration formulation of the explicit Hughes-Liu element requires 35,350 mathematical operations. Because of its computational efficiency, the Belytschko-Lin-Tsay shell element is usually the shell element formulation of choice. For this reason, it has become the default shell element formulation for explicit calculations. The Belytschko-Lin-Tsay shell element is based on a combined co-rotational and velocity-strain formulation. The efficiency of the element is obtained from the mathematical simplifications that result from these two kinematical assumptions. The co-rotational portion of the formulation avoids the complexities of nonlinear mechanics by embedding a coordinate system in the element. The choice of velocity-strain or rate-of-deformation in the formulation facilitates the constitutive evaluation, since the conjugate stress is the physical Cauchy stress. We closely follow the notation of Belytschko, Lin, and Tsay in the following development.

Co-rotational Coordinates The midsurface of the quadrilateral shell element, or reference surface, is defined by the location of the element’s four corner nodes. An embedded element coordinate system (see Figure 0-9) that deforms with the element is defined in terms of these nodal coordinates. Then the procedure for constructing the co-rotational coordinate system begins by calculating a unit vector normal to the main diagonal of the element:

s3 eˆ 3 = --------s3 s3 =

(0-123)

2 2 2 s 31 + s 32 + s 33

s 3 = r 31 × r 42 where the superscript caret

(0-124) (0-125)

( ˆ ) is used to indicate the local (element) coordinate system.

56 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

s3

yˆ

3 4 eˆ r42

eˆ

3

r31

2 s1

1 eˆ

1

Figure 0-9

r21

xˆ 2

Construction of Element Coordinate System

x axis xˆ approximately along the element edge between nodes 1 and 2. This definition is convenient for interpreting the element stresses, which are defined in the local xˆ – yˆ coordinate system. The procedure for constructing this unit vector is to define a vector s 1 that is nearly It is desired to establish the local

parallel to the vector r 21 , viz.

s 1 = r 21 – ( r 21 ⋅ eˆ 3 )eˆ 3

(0-126)

s1 eˆ 1 = --------s1

(0-127)

The remaining unit vector is obtained from the vector cross product

eˆ 2 = eˆ 3 × eˆ 1

(0-128)

If the four nodes of the element are coplanar, then the unit vectors eˆ 1 and eˆ 2 are tangent to the midplane of the shell and eˆ 3 is in the fiber direction. As the element deforms, an angle may develop between the actual fiber direction and the unit normal eˆ 3 . The magnitude of this angle may be characterized as

eˆ 3 ⋅ f – 1 < δ

(0-129)

Elements 57 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

f is the unit vector in the fiber direction and the magnitude of δ depends on the magnitude of the strains. According to Belytschko et al., for most engineering applications, acceptable values of δ are on where

the order of 10-2 and if the condition presented in (0-129) is met, then the difference between the rotation of the co-rotational coordinates

eˆ and the material rotation should be small.

The global components of this co-rotational triad define a transformation matrix between the global and local element coordinate systems. This transformation operates on vectors with global components

ˆ ˆ ˆ ˆ A = ( Ax, Ay, A z ) and element coordinate components A = ( A x, A y, A z ) , and is defined as:    Ax  e 1x e 2x e 3x   { A } =  A y  = e 1y e 2y e 3y   e 1z e 2z e 3z  Az   

      

ˆ Ax ˆ Ay ˆ Az

   ˆ ˆ  = [μ]{A} = [ q]T{A}   

(0-130)

where e ix, e iy, e iz are the global components of the element coordinate unit vectors. The inverse transformation is defined by the matrix transpose; i.e.,

ˆ { A } = [ μ]T{ A }

(0-131)

Velocity-Strain Displacement Relations The above small rotation condition, (0-129), does not restrict the magnitude of the element’s rigid body rotations. Rather, the restriction is placed on the out-of-plane deformations, and, thus, on the element strain. Consistent with this restriction on the magnitude of the strains, the velocity-strain displacement relations used in the Belytschko-Lin-Tsay shell are also restricted to small strains. As in the Hughes-Liu shell element, the displacement of any point in the shell is partitioned into a midsurface displacement (nodal translations) and a displacement associated with rotations of the element’s fibers (nodal rotations). The Belytschko-Lin-Tsay shell element uses the Mindlin [1951] theory of plates and shells to partition the velocity of any point in the shell as:

v = v m – zˆ e 3 × θ

(0-132)

where v m is the velocity of the mid-surface, θ is the angular velocity vector, and zˆ is the distance along the fiber direction (thickness) of the shell element. The corresponding co-rotational components of the velocity strain (rate of deformation) are given by

58 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

ˆ ˆ 1  ∂υ-i ∂υ ˆ --------j d ij = ---  ------+ 2  ∂xˆ j ∂xˆ i 

(0-133)

Substitution of (0-132) into the above yields the following velocity-strain relations:

ˆ ∂vˆ xm ∂θ ˆ - + zˆ --------y d x = -------∂xˆ ∂xˆ

(0-134)

ˆm ˆ ∂υ y ˆ ∂θ x ˆ --------------dy = – z ˆ∂yˆ ∂y

(0-135)

ˆm ˆm ˆ ˆ ∂υ x ∂υ y ˆ  ∂θy ∂θ x ˆ - + ---------- + z -------- – -------2d xy = -------- ∂yˆ ∂yˆ ∂xˆ ∂xˆ 

(0-136)

ˆm ∂υ z ˆ ˆ - – θx 2d yz = --------∂yˆ

(0-137)

ˆm ∂υ z ˆ ˆ - + θy 2d xz = --------∂xˆ

(0-138)

The above velocity-strain relations need to be evaluated at the quadrature points within the shell. Standard bilinear nodal interpolation is used to define the mid-surface velocity, angular velocity, and the element’s coordinates (isoparametric representation). These interpolations relations are given by

ν m = N I ( ξ, η )ν I

(0-139)

θ m = N I ( ξ, η )θ I

(0-140)

x m = N I ( ξ, η )x I

(0-141)

I is summed over all the nodes of the element and the nodal velocities are obtained by differentiating the nodal coordinates with respect to time, i.e., υ = x· . The bilinear where the subscript

I

I

shape functions are

1 N 1 = --- ( 1 – ξ ) ( 1 – η ) 4

(0-142)

Elements 59 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

1 N 2 = --- ( 1 + ξ ) ( 1 – η ) 4

(0-143)

1 N 3 = --- ( 1 + ξ ) ( 1 + η ) 4

(0-144)

1 N 4 = --- ( 1 – ξ ) ( 1 + η ) 4

(0-145)

The velocity-strains at the center of the element (i.e., at ξ = 0 , and η = 0 ) are obtained by substitution of the above relations into the previously defined velocity-strain displacement relations, (0-134) through (0-138). After some algebra, this yields

ˆ ˆ ˆ d x = B 1I υ xI + zˆ B 1I θ yI

(0-146)

ˆ ˆ ˆ d y = B 2I υ yI – zˆ B 2I θ xI

(0-147)

ˆ ˆ ˆ ˆ ˆ 2d xy = B2I υ xI + B 1I υ yI + zˆ ( B2I θ yI – B1I θ xI )

(0-148)

ˆ ˆ ˆ 2d xz = B 1I υ zI + N I θyI

(0-149)

ˆ ˆ ˆ 2d yz = B 2I υ zI – N I θ xI

(0-150)

where

∂N I B 1I = -------∂xˆ

(0-151)

∂N I B 2I = -------∂yˆ

(0-152)

The shape function derivatives

B aI are also evaluated at the center of the element; i.e., at ξ = 0 , and

η = 0.

Stress Resultants and Nodal Forces After suitable constitutive evaluations using the above velocity-strains, the resulting stresses are integrated through the thickness of the shell to obtain local resultant forces and moments. The integration formula for the resultants are

60 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

ˆR f αβ =

ˆ

 σαβ dzˆ

ˆ R = – zˆ σˆ dzˆ m αβ  αβ

(0-153)

(0-154)

where the superscript, R , indicates a resultant force or moment, and the Greek subscripts emphasize the limited range of the indices for plane stress plasticity. The above element midplane force and moment resultants are related to the local nodal forces and moments by invoking the principle of virtual power and integrating with a one-point quadrature. The relations obtained in this manner are

ˆ ˆR ˆR f xI = A (B 1I f xx + B 2I f xy )

(0-155)

ˆ ˆR ˆR f yI = A (B 2I f yy + B 1I f xy )

(0-156)

ˆ ˆR ˆR f zI = Aκ (B 1I f xz + B 2I f yz )

(0-157)

R ˆ = AB m ˆR +B m ˆ R κ- ˆf yz m xI 1I xy – - 2I yy 4 

(0-158)

R ˆ = –A  B m ˆR ˆR κ --- ˆ  m yI  1I xx + B 2I m xy – 4 f xz

(0-159)

ˆ = 0 m zI

(0-160)

A is the area of the element, and κ is the shear factor from the Mindlin theory. In the BelytschkoLin-Tsay formulation, κ is used as a penalty parameter to enforce the Kirchhoff normality condition as where

the shell becomes thin. The above local nodal forces and moments are then transformed to the global coordinate system using the transformation relations given previously as (0-130). The global nodal forces and moments are then appropriately summed over all the nodes and the global equations of motion are solved for the next increment in nodal accelerations.

Elements 61 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

Hourglass Control (Belytschko-Lin-Tsay) In part, the computational efficiency of the Belytschko-Lin-Tsay and the under integrated Hughes-Liu shell elements are derived from their use of one-point quadrature in the plane of the element. To suppress the hourglass deformation modes that accompany one-point quadrature, hourglass viscosity stresses are added to the physical stresses at the local element level. The discussion of the hourglass control that follows pertains to the Hughes-Liu and the membrane elements as well. The hourglass procedure is controlled by the DYHRGIHQ PARAM. The hourglass control used by Belytschko et al., extends an earlier derivation by Flanagan and Belytschko [1981], (see also Kosloff and Frazier [1978], Belytschko and Tsay [1983]). The hourglass shape vector, τ I , is defined as

τ I = h I – ( hJ xˆ aJ )B aI

(0-161)

where

+1 h = –1 +1 –1

(0-162)

is the basis vector that generates the deformation mode that is neglected by one-point quadrature. In (0-161) and the reminder of this subsection, the Greek subscripts have a range of 2; e.g.,

x aI = ( xˆ 1I, xˆ 2I ) = ( xˆ I, yˆ I ) . The hourglass shape vector then operates on the generalized displacements, in a manner similar to (0-146) through (0-150), to produce the generalized hourglass strain rates

ˆ q· αB = τ I θαI

(0-163)

ˆ q· 3B = τ I υ zI

(0-164)

ˆ q· αM = τ I υ αI

(0-165)

where the superscripts B and M denote bending and membrane modes, respectively. The corresponding hourglass stress rates are then given by

62 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

r θ Et 3 A ·B Q α = ----------------- B βI B βI q· αB 192

(0-166)

r w κGt 3 A ·B Q 3 = ---------------------- BβI B βI q· B 3 12

(0-167)

r m EtA ·M Q α = --------------- B βI B βI q· αM 8

(0-168)

where t is the shell thickness and the parameters, r θ, r w , and r m are generally assigned values between 0.01 and 0.05. Finally, the hourglass stresses, which are updated from the stress rates in the usual way; i.e.,

· Q n + 1 = Q n + ΔtQ

(0-169)

and the hourglass resultant forces are then

ˆ H = τ QB m αI I α

(0-170)

ˆf H = τ Q B I 3 3I

(0-171)

ˆf H = τ Q M αI I α

(0-172)

where the superscript H emphasizes that these are internal force contributions from the hourglass deformations. These hourglass forces are added directly to the previously determined local internal forces due to deformations (0-155) through (0-160). These force vectors are orthogonalized with respect to rigid body motion.

Hourglass Control (Englemann and Whirley) Englemann and Whirley [1991] developed an alternative hourglass control, which they implemented in the framework of the Belytschko, Lin, and Tsay shell element. We will briefly highlight their procedure here that has proven to be cost effective-only twenty percent more expensive than the default control. In the hourglass procedure, the in-plane strain field (subscript field plus the stabilization strain field:

· ·0 ·s εp = εp + εp

p ) is decomposed into the one point strain

(0-173)

Elements 63 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

where the stabilization strain field, which is obtained from the assumed strain fields of Pian and Sumihara [1984], is given in terms of the hourglass velocity field as

·s ε p = W m q· m + zW b q· b Here,

(0-174)

W m and W b play the role of stabilization strain velocity operators for membrane and bending: p

p

Wm =

f 1( ξ, η )

f 4 ( ξ, η )

f 2( ξ, η )

f 5 ( ξ, η )

f 3( ξ, η )

f 6 ( ξ, η )

p

p

p

(0-175)

p

p

p

– f 4( ξ, η )

f 1( ξ, η )

W b = – f p( ξ, η ) 5

f 2 ( ξ, η )

– f 6 ( ξ, η )

f 3 ( ξ, η )

p

(0-176)

p

p

p

where the terms f i ( ξ, η ) i = 1, 2, …, 6 , are rather complicated and the reader is referred to the reference [Englemann and Whirley, 1991]. To obtain the transverse shear assumed strain field, the procedure given in [Bathe and Dvorkin, 1984] is used. The transverse shear strain field can again be decomposed into the one point strain field plus the stabilization field:

· ·0 ·s εs = εs + ε s

(0-177)

that is related to the hourglass velocities by

·s ε s = W s q· s

(0-178)

where the transverse shear stabilization strain-velocity operator

Ws =

f s( ξ, η ) – g s ξ g s η g s ξ g s η 1

1

2

3

3

f 2s( ξ, η ) g 4s ξ g 4s η – g 2s ξ g1s η

W s is given by

(0-179)

64 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

Again, the coefficients

f 1s( ξ, η ) and g 1s are defined in the reference.

In their formulation, the hourglass forces are related to the hourglass velocity field through an incremental hourglass constitutive equation derived from an additive decomposition of the stress into a “one-point stress,” plus a “stabilization stress.” The integration of the stabilization stress gives a resultant constitutive equation relating hourglass forces to hourglass velocities. The in-plane and transverse stabilization stresses are updated according to:

· τ ss, n + 1 = τ ss, n + Δtc s C s ε ss where the tangent matrix is the product of a matrix scalar

(0-180)

C , which is constant within the shell domain, and a

c that is constant in the plane but may vary through the thickness.

The stabilization stresses can now be used to obtain the hourglass forces: h --T 2 W m τ ps dA d h – --2A h --T s 2 W τ p dA dz b h – --2A h--T s 2 W τ s dA dz s h – --2A

Qm =

 

Qb =

 

Qs =

 

(0-181)

CQUAD4 DYSHELLFORM = 10, Belytschko-Wong-Chiang Improvements Since the Belytschko-Tsay element is based on a perfectly flat geometry, warpage is not considered. Although this generally poses no major difficulties and provides for an efficient element, incorrect results in the twisted beam problem, See Figure 0-10, are obtained where the nodal points of the elements used in the discretization are not coplanar. The Hughes-Liu shell element considers non-planar geometry and gives good results on the twisted beam, but is relatively expensive. The effect of neglecting warpage in typical a application cannot be predicted beforehand and may lead to less than accurate results, but the latter is only speculation and is difficult to verify in practice. Obviously, it would be better to use shells that consider warpage if the added costs are reasonable and if this unknown effect is eliminated. In this section, we briefly describe the simple and computationally inexpensive modifications necessary in the Belytschko-Tsay shell to include the warping stiffness. The improved transverse shear treatment is also described which is necessary for the element to pass the Kirchhoff patch test. Readers are directed to the references [Belytschko, Wong, and Chang 1989, 1992] for an in depth theoretical background.

Elements 65 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

In order to include warpage in the formulation it is convenient to define nodal fiber vectors as shown in Figure 0-11. The geometry is interpolated over the surface of the shell from:

x = x m + ζp = ( x I + ζp I )N I ( ξ, η ) where:

(0-182)

ζh ζ = ------ and ζ is a parametric coordinate which varies between -1 to +1. 2

The in plane strain components are given by: c d xx = b xI vˆ xI + ζ ( b xI vˆ xI + b xI p· xI )

(0-183)

c

d yy = b yI vˆ yI + ζ ( b yI vˆ yI + b yI p· yI )

(0-184)

c c 1 d xy = --- bxI vˆ yI + b yI vˆ xI + ζ ( b xI vˆ yI + b xI p· yI + b yI vˆ xI + b yI p· xI ) 2

(0-185)

Twisted Beam Problem

Displacement-time History 30 29

Y Displacement (104)

24 L = 12 b = 1.1 t = .32 twist = 90 degrees E = 29 000 000 ν = .22

Belystchkno-Tsay

20 16

Hughes-Liu Belytschko-Wong-Chiang

12 8 4 0

0

5

10 time (ms)

15

19

66 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

Figure 0-10

The Twisted Beam Problem Fails with the Belytschko-Tsay Shell Element

p3

p1 p2 h

Figure 0-11

Nodal Fiber Vectors

p 1, p 2 , and p 3 where h is the Thickness

The coupling terms are come in through

c b iI which is defined in terms of the components of the fiber

vectors as:

 c  b xI   bc  yI

 p yˆ 2 – p yˆ 4   = p xˆ 2 – p xˆ 4  

p yˆ 3 – p yˆ 1

p yˆ 4 – p yˆ 2

p yˆ 1 – p yˆ 3

p xˆ 3 – p xˆ 1

p xˆ 4 – p xˆ 2

p xˆ 1 – p xˆ 3

(0-186)

For a flat geometry the normal vectors are identical and no coupling can occur. Two methods are used c

by Belytschko for computing b iI and the reader is referred to his papers for the details. Both methods have been tested and comparable results were obtained. The transverse shear strain components are given as

γˆ xz = – N I ( ξ ,η )θ yˆ I

(0-187)

γˆ yz = – N I ( ξ ,η )θ xˆ I

(0-188)

where the nodal rotational components are defined as: I

I

K

K

θ xˆ I = ( e n ⋅ e xˆ )θn + ( e n ⋅ e xˆ )θ n

(0-189)

Elements 67 CQUADA - DYSHELLFORM = 2, Belytschko-Lin-Tsay Shell

I

I

K

K

θ yˆ I = ( e n ⋅ e yˆ )θ n + ( e n ⋅ e yˆ )θ n The rotation

(0-190)

I

θ n comes from the nodal projection

I 1 I 1- ˆ I θ n = --- ( θnI + θnJ ) + -----( υ zJ – υˆ zJ ) 2 L IJ

where the subscript length of side

(0-191)

n refers to the normal component of side I as seen in Figure 0-12 and L IJ is the

IJ . yˆ

K r L e

eˆ y K en

nk

i J K

I

Figure 0-12

eˆ X

Vector and Edge Definitions for Computing the Transverse Shear Strain Components

68 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell The C 0 shell element due to Kennedy, Belytschko, and Lin [1986] has been implemented as a computationally efficient triangular element complement to the Belytschko-Lin-Tsay quadrilateral shell element ([Belytschko and Tsay 1981], [Belytschko et al., 1984a]). For a shell element with five throughthe-thickness integration points, the element requires 649 mathematical operations (the Belytschko-LinTsay quadrilateral shell element requires 725 mathematical operations) compared to 1417 operations for the Marchertas-Belytschko triangular shell [Marchertas and Belytschko 1974] (referred to as the BCIZ [Bazeley, Cheung, Irons, and Zienkiewicz 1965] triangular shell element). Triangular shell elements are offered as optional elements primarily for compatibility with local user grid generation and refinement software. Many computer aided design (CAD) and computer aided manufacturing (CAM) packages include finite element mesh generators, and most of these mesh generators use triangular elements in the discretization. Similarly, automatic mesh refinement algorithms are typically based on triangular element discretization. Also, triangular shell element formulations are not subject to zero energy modes inherent in quadrilateral element formulations. The triangular shell element’s origins are based on the work of Belytschko et al., [Belytschko, Stolarski, and Carpenter 1984b] where the linear performance of the shell was demonstrated. Because the triangular shell element formulations parallels closely the formulation of the Belytschko-Lin-Tsay quadrilateral shell element presented in the previous section, the following discussion is limited to items related specifically to the triangular shell element.

Co-rotational Coordinates The mid-surface of the triangular shell element, or reference surface, is defined by the location of the element’s three nodes. An embedded element coordinate system (see Figure 0-13) that deforms with the element is defined in terms of these nodal coordinates. The procedure for constructing the co-rotational coordinate system is simpler than the corresponding procedure for the quadrilateral, because the three nodes of the triangular element are guaranteed coplanar. zˆ yˆ 3 eˆ 3

1

eˆ 2

eˆ 1

Figure 0-13

xˆ 2

Local Element Coordinate System for

C 0 Shell Element

Elements 69 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

xˆ , is directed from node 1 to 2. The element’s normal axis, zˆ , is defined by the vector cross product of a vector along xˆ with a vector constructed from node 1 to node 3. The local y-axis, yˆ , is defined by a unit vector cross product of eˆ with eˆ , which are the unit vectors in the zˆ directions, The local x-axis,

3

1

respectively. As in the case of the quadrilateral element, this triad of co-rotational unit vectors defines a transformation between the global and local element coordinate systems (see (0-130) and (0-131)).

Velocity-Strain Relations As in the Belytschko-Lin-Tsay quadrilateral shell element, the displacement of any point in the shell is partitioned into a mid-surface displacement (nodal translations) and a displacement associated with rotations of the element’s fibers (nodal rotations). The Kennedy-Belytschko-Lin triangular shell element also uses the Mindlin [Mindlin 1951] theory of plates and shells to partition the velocity of any point in the shell (recall (0-132)):

ν = v m – zˆ e 3 × θ

(0-192)

where ν m is the velocity of the mid-surface, θ is the angular velocity vector, and zˆ is the distance along the fiber direction (thickness) of the shell element. The corresponding co-rotational components of the velocity strain (rate of deformation) were given previously in (0-146) through (0-150). Standard linear nodal interpolation is used to define the midsurface velocity, angular velocity, and the element’s coordinates (isoparametric representation). These interpolation functions are the area coordinates used in triangular element formulations. Substitution of the nodally interpolated velocity fields into the velocity-strain relations (see Belytschko et al., for details), leads to strain rate-velocity relations of the form

dˆ = Bvˆ

(0-193)

dˆ are the velocity strains (strain rates), the elements of B are derivatives of the nodal ˆ are the nodal velocities and angular velocities. interpolation functions, and the ν where

It is convenient to partition the velocity strains and the contributions. The membrane relations are given by

B matrix into membrane and bending

70 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

  dˆ x   dˆ y   2dˆ xy 

M

      

1= --------ˆx yˆ 2 3

yˆ 3

0

yˆ 3

0

xˆ 3 – xˆ 2 –yˆ

0 – xˆ

xˆ 3 – xˆ 2

3

3

0 – xˆ

0 3

yˆ 3

0 xˆ

2

0 xˆ

2

0

            

υˆ x1 υˆ y1

υˆ x2 υˆ y2

υˆ x3 υˆ y3

            

(0-194)

or

ˆM d = B M νˆ

(0-195)

The bending relations are given by

  κˆ x   κˆ y   2κˆ xy 

  0  – 1 - xˆ – xˆ  = --------xˆ 2 yˆ 3 3 2  yˆ 3  

– yˆ 3 0

0 xˆ

xˆ 3 – xˆ 2

– yˆ 3

3

yˆ 3 0 – xˆ

3

0 –xˆ 0

0 2

0 xˆ

2

            

ˆ θ x1 ˆ θ y1 ˆ θ x2 ˆ θ y2 ˆ θ x3 ˆ θ y3

            

(0-196)

or

ˆ def κˆ M = BM θ The local element velocity strains are then obtained by combining the above two relations:

(0-197)

Elements 71 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

 ˆ  dx   dˆ y   2dˆ xy 

  ˆ   d x     dˆ y     2dˆ xy  

M

    κˆ x    – zˆ  κˆ y     2κˆ xy  

   ˆM ˆ ˆ  = d – z κ   

(0-198)

The remaining two transverse shear strain rates are given by

 ˆ  2d xz   2dˆ yz 

  1  = ------------ˆ 6x 2 yˆ 3   – yˆ 2 yˆ 3 ( 2xˆ 2 + xˆ 3 ) 3

yˆ 3 ( xˆ 2 –def 2xˆ 2 )  ˆ   θx1   ˆ   θy1   ˆ   θx2     θˆ y2     θˆ x3     θˆ y3   

xˆ 22 – xˆ 32

yˆ 32

yˆ 3 ( 3xˆ 2 – xˆ 3 )

0

xˆ 2 yˆ 3

– yˆ 32 ( xˆ 2 + xˆ 3 ) xˆ 3 ( xˆ 3 – 2xˆ 2 ) – 3xˆ 2 yˆ 3 xˆ 2 ( 2xˆ 3 – xˆ 2 )

(0-199)

or

ˆS ˆ def d = BS θ

(0-200)

All of the above velocity-strain relations have been simplified by using one-point quadrature. In the above relations, the angular velocities

ˆ θ def are the deformation component of the angular velocity

ˆ θ obtained by subtracting the portion of the angular velocity due to rigid body rotation; i.e., ˆ def ˆ ˆ rig θ = θ–θ The two components of the rigid body angular velocity are given by

(0-201)

72 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

υˆ z1 – υˆ z2 ˆ rig θ y = --------------------xˆ 2

(0-202)

υˆ z3 – υˆ z1 )xˆ 2 – ( υˆ z2 – υˆ z1 )xˆ 3 ˆθ rig = (--------------------------------------------------------------------x xˆ 2 yˆ 3

(0-203)

The first of the above two relations is obtained by considering the angular velocity of the local x-axis about the local y-axis. Referring to Figure 0-14, by construction nodes 1 and 2 lie on the local x-axis and the distance between the nodes is xˆ 2 ; i.e., the

xˆ distance from node 2 to the local coordinate origin at

node 1. Thus, the difference in the nodal zˆ velocities divided by the distance between the nodes is an average measure of the rigid body rotation rate about the local y-axis. zˆ yˆ 3

xˆ 1

2

zˆ yˆ 3

xˆ 1

Figure 0-14

2

Element Configurations with Node 3 Aligned with Node 1 (left) and Node 3 Aligned with Node 2 (right)

The second relation is conceptually identical, but is implemented in a slightly different manner due to the arbitrary location of node 3 in the local coordinate system. Consider the two local element configurations shown in Figure 0-14. For the left-most configuration, where node 3 is the local y-axis, the rigid body rotation rate about the local x-axis is given by

Elements 73 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

υˆ z3 – υˆ z1 ˆθ rig x – left = --------------------yˆ 3

(0-204)

and for the rightmost configuration the same rotation rate is given by

υˆ z3 – υˆ z2 ˆθ rig x – right = --------------------yˆ 3

(0-205)

Although both of these relations yield the average rigid body rotation rate, the selection of the correct relation depends on the configuration of the element; i.e., on the location of node 3. Since every element in the mesh could have a configuration that is different in general from either of the two configurations shown in Figure 0-14, a more robust relation is needed to determine the average rigid body rotation rate about the local x-axis. In most typical grids, node 3 will be located somewhere between the two configurations shown in Figure 0-14. Thus, a linear interpolation between these two rigid body rotation rates was devised using the distance xˆ 3 as the interpolant:

xˆ xˆ 3 ˆ rig ˆ rig ˆ rig - + θ x – right  ----3- θ x = θ x – left  1 – --- xˆ 2 xˆ 2

(0-206)

Substitution of (0-204) and (0-205) into (0-206) and simplifying produces the relations given previously as (0-203).

Stress Resultants and Nodal Forces After suitable constitutive evaluation using the above velocity strains, the resulting local stresses are integrated through the thickness of the shell to obtain local resultant forces and moments. The integration formulae for the resultants are

ˆR f αβ =

 σαβ dzˆ ˆ

ˆ R = – zˆ σˆ dzˆ m  αβ αβ

(0-207)

(0-208)

where the superscript R indicates a resultant force or moment and the Greek subscripts emphasize the limited range of the indices for plane stress plasticity. The above element midplane force and moment resultant are related to the local nodal forces and moments by invoking the principle of virtual power and performing a one-point quadrature. The relations obtained in this manner are

74 CTRIA3 - DYSHELLFORM = 4, C0 Triangular Shell

            

ˆ f x1 ˆ f y1 ˆ f x2 ˆ f y2 ˆ f x3 ˆ f y3

            

 ˆ  m x1  ˆ   R m y1 ˆ  m  xx ˆ m x2  T ˆR  = AB M  m yy ˆ m y2   ˆR   m ˆ  m  xy x3 ˆ  m y3 

where

     ˆR   f xx  T R  = AB M  ˆf yy     ˆf R   xy   

      

(0-209)

    T  + ABS      

ˆR f xz ˆR f yz

    

(0-210)

A is the area of the element ( 2A = xˆ 2 yˆ 3 ) .

The remaining nodal forces, the

ˆ ˆ ˆ zˆ component of the force ( f z3, f z2, f z1 ) , are determined by

successively solving the following equilibration equations

ˆ +m ˆ +m ˆ + yˆ ˆf = 0 m x1 x2 x3 3 z3

(0-211)

ˆ +m ˆ +m ˆ – xˆ ˆf – xˆ ˆf = 0 m y1 y2 y3 3 z3 2 z2

(0-212)

ˆ ˆ f z1 + f z2 + ˆf z3 = 0

(0-213)

which represent moment equilibrium about the local x-axis, moment equilibrium about the local y-axis, and force equilibrium in the local z-direction, respectively.

Elements 75 CTRIA3 - DYSHELLFORM = 3, Marchertas-Belytschko Triangular Shell (BCIZ)

CTRIA3 - DYSHELLFORM = 3, Marchertas-Belytschko Triangular Shell (BCIZ) The Marchertas-Belytschko [1974] triangular shell element, or the BCIZ triangular shell element, was developed in the same time period as the Belytschko beam element [Belytschko, Schwer, and Klein, 1977], see “CBEAM - Belytschko Beam” on page 34, forming the first generation of co-rotational structural elements developed by Belytschko and co-workers. Although the Marchertas-Belytschko shell element is relatively expensive (i.e., the C 0 triangular shell element with five through-the-thickness integration points requires 649 mathematical operations compared to 1,417 operations for the Marchertas-Belytschko triangular shell), it is maintained in SOL 700 for compatibility with earlier user models. However, as the user community moves to application of the more efficient shell element formulations, the use of the Marchertas-Belytschko triangular shell element will decrease. As mentioned above, the Marchertas-Belytschko triangular shell has a common co-rotational formulation origin with the Belytschko beam element. The interested reader is referred to the beam element description, see “Co-rotational Technique” on page 34 for details on the co-rotational formulation. In the next subsection a discussion of how the local element coordinate system is identical for the triangular shell and beam elements. The remaining subsections discuss the triangular element’s displacement interpolants, the strain displacement relations, and calculations of the element nodal forces.

Element Coordinates Figure 6-15a shows the element coordinate system, ( xˆ , yˆ , zˆ ) originating at Node 1, for the MarchertasBelytschko triangular shell. The element coordinate system is associated with a triad of unit vectors

( e 1, e 2, e 3 ) the components of which form a transformation matrix between the global and local coordinate systems for vector quantities. The nodal or body coordinate system unit vectors b 1, b 2, b 3 are defined at each node and are used to define the rotational deformations in the element, see “Co-rotational Technique” on page 34. The unit normal to the shell element e 3 is formed from the vector cross product

e 3 = l 21 × l 31

(0-214)

where l 21 and l 31 are unit vectors originating at Node 1 and pointing towards Nodes 2 and 3,

76 CTRIA3 - DYSHELLFORM = 3, Marchertas-Belytschko Triangular Shell (BCIZ)

Materials 71

Materials

72 Materials

Materials In addition to most materials available in structures workspace, the following material models suitable for explicit applications are also available in MD Explicit. Here, we will highlight the theoretical background of these material models. These are the material models that are most commonly used for typical structural applications. For a more detailed description of all the available materials in MD Explicit, please refer to MD R2 Nastran Quick Reference Guide.

1

Elastic

2

Orthotropic Elastic

3

Kinematic/Isotropic Elastic-Plastic

5

Soil and Crushable/Non-crushable Foam

6

Viscoelastic

7

Blatz-Ko Rubber

9

Null Hydrodynamics

10

Isotropic-Elastic-Plastic-Hydrodynamic

12

Isotropic-Elastic-Plastic

13

Elastic-Plastic with Failure Model

14

Soil and Crushable Foam with Failure Model

15

Johnson/Cook Strain and Temperature Sensitive Plasticity

18

Power Law Isotropic Plasticity

19

Strain Rate Dependent Isotropic Plasticity

20

Rigid

22

Composite Damage Model

24

Piecewise Linear Isotropic Plasticity

26

Honeycomb

27

Compressible Mooney-Rivlin Rubber

28

Resultant Plasticity

29

Forced Limited Resultant Fomulation

30

Shape-Memory Superelastic Material

31

Slightly Compressible Rubber Model

32

Laminated Glass Model

34

Fabric

40

Nonlinear Orthotropic

54-55

Composite Damage Model

Materials 73 Materials

57

Low Density Urethane Foam

58

Laminated Composite Fabric

59

Composite Failure Model - Plasticity Based

62

Viscous foam

63

Isotropic Crushable Foam

64

Strain Rate Sensitive Power-Law Plasticity

66

Linear Elastic Discrete Beam

67

Nonlinear Elastic Discrete Beam

68

Nonlinear Plastic Discrete Beam

69

SID Damper Discrete Beam

70

Hydraulic Gas Damper Discrete Beam

71

Cable Discrete Beam

72

Concrete Damage

72R

Concrete Damage Release III

73

Low Density Viscoelastic Foam

74

Elastic Spring Discrete Beam

76

General Viscoelastic

77

Hyperviscoelastic Rubber

80

Ramberg-Osgood Plasticity

81

Plastic with Damage

83

Fu-Chang’s Foam with Rate Effects

87

Cellular Rubber

89

Plastic Polymer

93

Elastic Six Degrees of Freedom Spring Discrete Beam

94

Inelastic Spring Discrete Beam

95

Inelastic Spring Six Degrees of Freedom Discrete Beam

97

General Joint Discrete Beam

98

Simplified Johnson-Cook

99

Simplified Johnson-Cook Orthotropic Damage

100

Spot weld

112

Finite Elastic Strain Plasticity

114

Layered Linear Plasticity

119

General Nonlinear Six Degrees of Freedom Discrete Beam

121

General Nonlinear One Degree of Freedom Discrete Beam

74 Materials

123

Modified Piecewise Linear Plasticity

126

Modified Honeycomb

127

Arruda-Boyce rubber

158

Composite Fabric

181

Simplified Rubber

196

General Spring Descrete Beam

B01

Seatbelt

S01

Spring Elastic (Linear)

S02

Damper Viscous (Linear)

S03

Spring Elastoplastic (Isotropic)

S04

Spring Nonlinear Elastic

S05

Damper Nonlinear Viscous

S06

Spring General Nonlinear

S07

Spring Maxwell (Three parameter Viscoelastic)

S08

Spring Inelastic (Tension or Compression)

S13

Spring Tri-linear Degrading

S14

Spring Squat Shearwall

S15

Spring Muscle

SW1

Spot Weld (Simple Damage-Failure)

SW2

Spot Weld (Resultant-based Failure Criteria)

SW3

Spot Weld (Stress-based Failure)

SW4

Spot Weld (Rate Dependent Stress-based Failure)

SW5

Spot Weld (Additional Failure)

In the table below, a list of the available material models and the applicable element types are given. Some materials include strain rate sensitivity, failure, equations of state, and thermal effects and this

Materials 75 Materials

Strain-Rate Effects Failure Equation-of-State Thermal Effects

Material Title

Bricks Beams Thin Shells Thick Shells

Material Number

is also noted. General applicability of the materials to certain kinds of behavior is suggested in the last column. Gn General Cm Composites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro-dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Cone

1 Elastic

Y Y Y Y

Gn, Fl

2 Orthotropic Elastic (Anisotropic - solids)

Y

Cm, Mt

3 Plastic Kinematic/Isotropic

Y Y Y Y Y Y

Cm, Mt, Pl

5 Soil and Foam

Y

Fm, Sl

6 Linear Viscoelastic

Y Y Y Y Y Y

7 Blatz-Ko Rubber

Y

9 Null Material

Y

Y Y Y Fl, Hy

10 Elastic Plastic Hydro (dynamics)

Y

Y Y

12 Isotropic Elastic Plastic

Y

13 Isotropic Elastic-Plastic with Failure

Y

Y

Mt

14 Soil and Foam with Failure

Y

Y

Fm, Sl

15 Johnson/Cook Plasticity Model

Y

18 Power Law Plasticity (Isotropic)

Y Y Y Y Y

Mt, Pl

19 Strain Rate Dependent Rate Plasticity

Y

Mt, Pl

20 Rigid

Y Y Y Y

22 Composite Damage

Y

24 Piecewise Linear Isotropic Plasticity

Y Y Y Y Y Y

Mt, Pl

26 Honeycomb

Y

Cm, Fm, Sl

27 Mooney-Rivlin Rubber

Y

Y Y

Y

Rb, Polyurethane

Y Y

Y

Hy, Mt Y Mt

Y Y Y Y Hy, Mt

Y Y Y Y Y Y

Y Rb

Y Y Y

Cm

Y

Rb

28 Resultant Plasticity

Y Y

Mt

29 Forced Limited Resultant Formaultion

Y

30 Shaped Memory Alloy

Y

Mt

31 Slightly Compressible Rubber

Y

Rb

32 Laminated Glass (Composite)

Y Y

Y

Cm, Gl

76

Strain-Rate Effects Failure Equation-of-State Thermal Effects

Material Title

Bricks Beams Thin Shells Thick Shells

Material Number

Materials

Gn General Cm Composites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro-dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Cone

34 Fabric

Y

40 Nonlinear Orthotropic

Y

Y

Y Cm

54 Composite Damage with Chang Failure

Y

Y

Cm

55 Composite Damage with Tsai-Wu Failure

Y

Y

Cm

Y Y

Fm

57 Low Density Urethane Foam

Y

58 Laminated composite Fabric

Y

59 Composite Failure - Plasticity Based

Y

Y

Y

62 Viscous foam (Crash Dummy)

Y

Y

Fm

63 Isotropic Crushable Foam

Y

Y

Fm

64 Rate Sensitive Power-Law Plasticity

Y

Y Y Y

Mt

66 Linear Elastic Discrete Beam

Y

Y

67 Nonlinear Elastic Discrete Beam

Y

Y

68 Nonlinear Plastic Discrete Beam

Y

Y Y

69 SID Damper Discrete Beam

Y

Y

70 Hydraulic Gas Damper Discrete Beam

Y

Y

71 Cable Discrete Beam

Y

72 Concrete Damage

Cm, Cr

Y

Y Y Y

Sl

72R Concrete Damage Release III

Y

Y Y Y

Sl

73 Low Density Viscous Foam

Y

Y Y

Fm

Y

Rb

74 Elastic Spring Discrete Beam

Y

76 General Viscoelastic (Maxwell model)

Y

77 Hyperelastic and Ogden Rubber

Y

79 Hysteretic Soil (Elasto-Perfectly Plastic)

Y

80 Ramberg-Osgood

Y Y Y Y Y Y Y Y

81 Plastic with Damage (Elasto-Plastic)

Y Y Y Y Y Y

Mt, Pl

83 Fu-Chang’s Foam

Y

Y Y

Fm

87 Cellular Rubber

Y

Y

Rb

Rb Y

Sl

Materials 77

89 Plastic Polymer Y

94 Inelastic Spring Discrete Beam

Y

95 Inelastic Six Degrees of Freedom Spring Discrete Beam

Y

97 General Joint Discrete Beam

Y

98 Simplified Johnson-Cook

Y Y Y Y

99 Simplified Johnson-Cook Orthotropic Damage

Y Y Y Y

100 Spot weld

Y Y

114 Layered Linear Plasticity

Y Y

119 General Nonlinear Six Degrees of Freedom Discrete Beam

Y

121 General Nonlinear One Degree of Freedom Discrete Beam

Y

123 Modified Piecewise Linear Plasticity

Y Y

126 Modified Honeycomb

Y

127 Arruda-Boyce rubber

Y

158 Composite Fabric 181 Simplified Rubber 196 General Spring Discrete Beam

Gn General Cm Composites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro-dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Cone

Y

93 Elastic Six Degrees of Freedom Spring Discrete Beam

112 Finite Elastic Strain Plasticity

Strain-Rate Effects Failure Equation-of-State Thermal Effects

Material Title

Bricks Beams Thin Shells Thick Shells

Material Number

Materials

Y Y Y Y Y

Cm RB

Y

B01 Seatbelt S01 Spring Elastic (Linear)

Y

S02 Damper Viscous (Linear)

Y

S03 Spring Elastoplastic (Isotropic)

Y

S04 Spring Nonlinear Elastic

Y

Y Y

78

S05 Damper Nonlinear Viscous

Y

S06 Spring General Nonlinear

Y

S07 Spring Maxwell (Three Parameter Viscoelastic)

Y

S08 Spring Inelastic (Tension or Compression

Y

Strain-Rate Effects Failure Equation-of-State Thermal Effects

Material Title

Bricks Beams Thin Shells Thick Shells

Material Number

Materials

Gn General Cm Composites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro-dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Cone

Y Y

S13 Spring Tri-linear Degrading S14 Spring Squat Shearwall S15 Spring Muscle SW1 Spot Weld (Simple Damage-Failure)

Y

SW2 Spot Weld (Resultant-based Failure Criteria)

Y

SW3 Spot Weld (Stress-based Failure)

Y

SW4 Spot Weld (Rate Dependent Stress-based Failure)

Y

SW5 Spot Weld (Additional Failure)

Y

Material Model 1: Elastic In this elastic material we compute the co-rotational rate of the deviatoric Cauchy stress tensor as

s ij∇

n+1⁄2

· n+1⁄2 = 2Gε' ij

(3-1)

and pressure

p n + 1 = K ln V n + 1 where G and K are the elastic shear and bulk moduli, respectively, and the ratio of the current volume to the initial volume.

(3-2)

V is the relative volume; i.e.,

For standard MD Nastran solution sequence, this would be the same as using MAT1 to define a linear elastic material.

Materials 79 Materials

Material Model 2: Orthotropic Elastic The material law that relates second Piola-Kirchhoff stress

S to the Green-St. Venant strain E is

S = C ⋅ E = TtClT ⋅ E where

T =

(3-3)

T is the transformation matrix [Cook 1974]. l 12

m 12

n 12

l1 m1

m1 n1

n1 l1

l 22

m 22

n 22

l2 m2

m2 n2

n2 l2

l 32

m 32

n 32

l3 m3

m3 n3

n3 l3

2l 1 l 2 2m 1 m 2 2n 1 n 2 ( l 1 m 2 + l 1 m 1 ) ( m 1 n 2 + m 2 n 1 ) ( n 1 l 2 + n 2 l 1 )

(3-4)

2l 2 l 3 2m 2 m 3 2n 2 n 3 ( l 2 m 3 + l 3 m 2 ) ( m 2 n 3 + m 3 n 2 ) ( n 2 l 3 + n 3 l 2 ) 2l 3 l 1 2m 3 m 1 2n 3 n 1 ( l 3 m 1 + l 1 m 3 ) ( m 3 n 1 + m 1 n 3 ) ( n 3 l 1 + n 1 l 3 ) l i , m i , n i are the direction cosines x' i = l i x 1 + m i x 2 + n i x 3 and

for i = 1,2,3

(3-5)

x' i denotes the material axes. The constitutive matrix C l is defined in terms of the material axes as

C l–1

υ 21 υ 31 1 - ------------– - – -------- 0 E11 E 22 E 33

0

0

υ 12 1 υ 32 – -------- -------- – -------- 0 E 11 E 22 E 33

0

0

0

0

υ 13 υ 23 1 – -------- – -------- -------= E 11 E 22 E33

0

(3-6)

1-------0 G 12

0

0

0

0

0

0

0

1 0 --------- 0 G 23

0

0

0

0

1 0 --------G 31

80 Materials

where the subscripts denote the material axes; i.e.,

υ ij = υ x' i x' j and E ii = E x'i Since

(3-7)

C l is symmetric

υ 21 υ 12 ------- = ------- , ect. E 11 E 22

(3-8)

The vector of Green-St. Venant strain components is

Et =

E 11 ,E 22 ,E 33 ,E 12 ,E 23 ,E 31

(3-9)

ρ ∂x ∂x σ ij = ----- --------i- --------j- S k  ρ o ∂X k ∂X 

(3-10)

After computing S ij , we use Equation 3-10 to obtain the Cauchy stress. This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. For standard MD Nastran solution sequences, this would be the same as using MAT9 to define a linear anisotropic material. For shell elements, you would have used the MAT2 or MAT8 option.

Material Model 3: Elastic Plastic with Kinematic Hardening Isotropic, kinematic, or a combination of isotropic and kinematic hardening may be obtained by varying a parameter, called

β

between 0 and 1. For

β

equal to 0 and 1, respectively, kinematic and isotropic

hardening are obtained as shown in Figure 3-1 where l 0 and l are the undeformed and deformed length of uniaxial tension specimen, respectively. Krieg and Key [1976] formulated this model and the implementation is based on their paper. In isotropic hardening, the center of the yield surface is fixed but the radius is a function of the plastic strain. In kinematic hardening, the radius of the yield surface is fixed but the center translates in the direction of the plastic strain. Thus the yield condition is

σ y2 1--φ = ξ ij ξ ij – ------ = 0 2 3

(3-11)

where

ξ ij = S ij α ij

(3-12)

p σ y = σ 0 + βE p ε eff

(3-13)

Materials 81 Materials

The co-rotational rate of

α ij is

2 ·p α ij∇ = ( 1 – β ) --- Ep ε ij 3

(3-14)

Hence,

α ijn + 1 = α ijn + ( α ij∇

n+1⁄2

n Ω n + 1 ⁄ 2 + α n + 1 ⁄ 2 Ω n + 1 ⁄ 2 )Δt n + 1 ⁄ 2 + α ik ik jk ki

(3-15)

Et

E

Yield Stress

l ln  ---- l0

β = 0 β = 1

Figure 3-1

Kinematic Hardening Isotropic Hardening

Elastic-plastic Behavior with Isotropic and Kinematic Hardening

Strain rate is accounted for using the Cowper and Symonds [Jones 1983] model which scales the yield stress by a strain rate dependent factor

· ε 1⁄p p ρ y = 1 +  ---- ( σ 0 + βE p ε eff C where

· p and C are user-defined input constants and ε is the strain rate defined as:

(3-16)

82 Materials

· · · ε + ε ij ε ij

(3-17)

The current radius of the yield surface,

σ y , is the sum of the initial yield strength, σ 0 , plus the growth

p , where E p is the plastic hardening modulus βE p ε eff

Et E E p = -------------E – Et

(3-18)

p

and ε eff is the effective plastic strain t p ε eff

=

  --3- εij εij 2·p ·p

1/2

dt

(3-19)

0

The plastic strain rate is the difference between the total and elastic (right superscript) strain rates:

·p · ·e ε ij = ε ij – ε ij

(3-20)

In the implementation of this material model, the deviatoric stresses are updated elastically, as described for model 1, but repeated here for the sake of clarity:

σ ij* = σ ijn + C ijkl Δε kl

(3-21)

where

σ ij* is the trial stress tensor, σ ijn is the stress tensor from the previous time step, C ijkl is the elastic tangent modulus matrix, Δε kl is the incremental strain tensor. and, if the yield function is satisfied, nothing else is done. If, however, the yield function is violated, an increment in plastic strain is computed, the stresses are scaled back to the yield surface, and the yield surface center is updated. *

Let s ij represent the trial elastic deviatoric stress state at

n+1

Materials 83 Materials

* * 1 * s ij = σ ij – --- σ kk σ ij 3

(3-22)

and

ξ ij* = s ij* – α ij

(3-23)

Define the yield function,

3 φ = --- ξ ij* ξ ij* – σ y2 = Λ 2 – σ y2 < 0 for elastic or neutral loading > 0 for plastic harding 2

(3-24)

For plastic hardening then: n+1

p ε eff

Λ – σy pn pn p - = ε eff = ε eff + ------------------+ Δε eff 3G + Ep

(3-25)

Scale back the stress deviators:

σ ijn + 1

=

σ ij*

p 3GΔε eff ------------------- ξ ij* – Λ

(3-26)

and update the center:

α ijn + 1

=

α ijn

p ( 1 – β )E p Δε eff + -----------------------------------Λ

(3-27)

Plane Stress Plasticity The plane stress plasticity options apply to beams, shells, and thick shells. Since the stresses and strain increments are transformed to the lamina coordinate system for the constitutive evaluation, the stress and strain tensors are in the local coordinate system. The application of the Jaumann rate to update the stress tensor allows for the possibility that the normal stress,

σ 33 , will not be zero. The first step in updating the stress tensor is to compute a trial plane stress

update assuming that the incremental strains are elastic. In the above, the normal strain increment

Δε 33

is replaced by the elastic strain increment

σ 33 + λ ( Δε 11 + Δε 22 ) Δε 33 = – ---------------------------------------------------λ + 2μ where

λ and γ are Lamé’s constants.

(3-28)

84 Materials

When the trial stress is within the yield surface, the strain increment is elastic and the stress update is completed. Otherwise, for the plastic plane stress case, secant iteration is used to solve Equation (3-26) for the normal strain increment i σ 33

=

* σ 33

pi ξ 3GΔε eff 33 – ---------------------------Λ

Here, the superscript

=

i–1 Δε 33

(3-29)

i indicates the iteration number.

The secant iteration formula for

i+1 Δε 33

( Δε33 ) required to produce a zero normal stress:

Δε 33 (the superscript p is dropped for clarity) is

i i–1 Δε 33 – Δε 33 i–1 – -------------------------------σ 33 i – σi – 1 σ 33 33

(3-30)

where the two starting values are obtained from the initial elastic estimate and by assuming a purely plastic increment; i.e., 1 Δε 33 = – ( Δε 11 – Δε 22 )

(3-31)

These starting values should bound the actual values of the normal strain increment. The iteration procedure uses the updated normal stain increment to update first the deviatoric stress and then the other quantities needed to compute the next estimate of the normal stress in Equation (3-29). The iterations proceed until the normal stress

i is sufficiently small. The convergence criterion requires σ 33

convergence of the normal strains: i i–1 Δε 33 – Δε 33 ----------------------------------- < 10 – 4 i+1 Δε 33

(3-32)

After convergence, the stress update is completed using the relationships given in Equations (3-26) and (3-27) For SOL SEQ 106, 129, or 600, this material model is the same as using MATS1, with the hardening rule (HR) set to either Isotropic or Kinematic. These models do not allow

β between 0 and 1.

Material Model 5: Soil and Crushable Foam This model, due to Krieg [1972], provides a simple model for foam and soils whose material properties are not well characterized. We believe the other foam models (such as material models 57, 62, and 63) in SOL 700 are superior in their performance and are recommended over this model which simulates the crushing through the volumetric deformations. If the yield stress is too low, this foam model gives nearly fluid like behavior.

Materials 85 Materials

A pressure-dependent flow rule governs the deviatoric behavior:

1 φ s = --- s ij s ij – ( a 0 + a 1 p + a 2 p 2 ) 2 where

(3-33)

a 0 , a 1 , and a 2 are user-defined constants. Volumetric yielding is determined by a tabulated

curve of pressure versus volumetric strain. Elastic unloading from this curve is assumed to a tensile cutoff as illustrated in Figure 3-2.

Pressure

Loading and unloading follows the input curve if the volumetric crushing option is off (VCR = 1.0).

The bulk unloading modulus is used if the volumetric crushing option is on (VCR = 0).

V ln  ------ V0

Volumetric Strain (Compression)

Tension Tension Cutoff Value

Figure 3-2

Volumetric Strain Versus Pressure Curve for Soil and Crushable Foam Model

Implementation of this model is straightforward. One history variable, the maximum volumetric strain in compression, is stored. If the new compressive volumetric strain exceeds the stored value, loading is indicated. When the yield condition is violated, the updated trial stresses, s ij* , are scaled back using a simple radial return algorithm:

s ijn + 1

 a + a p + a p 2 1 ⁄ 2 0 1 2 =  -------------------------------------- s ij* 1--s s   2 ij ij

(3-34)

If the hydrostatic tension exceeds the cutoff value, the pressure is set to the cutoff value and the deviatoric stress tensor is zeroed.

86 Materials

Material Model 6: Viscoelastic In this model, linear viscoelasticity is assumed for the deviatoric stress tensor [Herrmann and Peterson 1968]: t

∂ε' ij s ij = 2  φ ( t – τ ) ---------- dτ ∂τ

(3-35)

0

where

φ ( t ) = G ∞ + ( G 0 – G ∞ )e – βt

(3-36)

is the shear relaxation modulus. A recursion formula is used to compute the new value of the hereditary integral at time t n + 1 from its value at time t n . Elastic bulk behavior is assumed:

p = K ln V

(3-37)

where pressure is integrated incrementally.

Material Model 7: Continuum Rubber The hyperelastic continuum rubber model was studied by Blatz and Ko [1962]. In this model, the second Piola-Kirchhoff stress is given by 1

S ij

– --------------= G  V –1 C ij – V 1 – 2υ δ ij

where

(3-38)

G is the shear modulus, V is the relative volume, υ is Poisson’s ratio, and C ij is the right

Cauchy-Green strain:

∂x ∂x C ij = -------k- -------k∂X i ∂X j after determining

(3-39)

S ij , it is transformed into the Cauchy stress tensor, σ ij :

ρ ∂x i ∂x j σ ij = ----- --------- -------- S kl ρ 0 ∂X k ∂X l where

(3-40)

ρ 0 and ρ are the initial and current density, respectively. The default value of υ is 0.463.

Material 27 and 31 better represent incompressible materials.

Materials 87 Materials

Material Model 9: Null Material For solid elements equations of state can be called through this model to avoid deviatoric stress calculations. A pressure cutoff may be specified to set a lower bound on the pressure. This model has been very useful when combined with the reactive high explosive model where material strength is often neglected. The null material should not be used to delete solid elements. A optional viscous stress of the form

σ ij = με′ ij

(3-41)

is computed for nonzero

μ where ε′ ij is the deviatoric strain rate.

Sometimes it is advantageous to model contact surfaces via shell elements which are not part of the structure, but are necessary to define areas of contact within nodal rigid bodies or between nodal rigid bodies. Beams and shells that use this material type are completely bypassed in the element processing. The Young’s modulus and Poisson’s ratio are used only for setting the contact interface stiffnesses, and it is recommended that reasonable values be input.

Material Model 10: Elastic-Plastic-Hydrodynamic For completeness we give the entire derivation of this constitutive model based on radial return plasticity. The pressure,

· · ρ ; deviatoric strain rate, ε' ij ; deviatoric stress rate, s· ij ; and volumetric strain rate, ε v ,

are defined in Equation (3-42):

1 p = – --- σ ij δ ij 3 s ij = σ ij + pδ ij · · s ij∇ = 2με' ij = 2Gε' ij

1· · · ε' ij = ε ij – --- ε v 3 · · ε v = ε ij δ ij (3-42)

The Jaumann rate of the deviatoric stress, s ij∇ , is given by:

s ij∇ = s· ij – s ip Ω pj – s jp Ω pi

(3-43)

First we update s ijn to s ijn + 1 elastically *s n + 1 ij

· · = s ijn + s ip Ω pj + s jp Ω pi + 2Gε' ij dt = s ijn + R ij + 2Gε' ij dt s ijR

n

2GΔε'ij

(3-44)

88 Materials

where the left superscript, *, denotes a trial stress value. The effective trial stress is defined by 1⁄2 3 s * =  --- *s ijn + 1 *s ijn + 1 2

(3-45)

y and if s * exceeds yield stress σ , the von Mises flow rule:

σ y2 1 φ = --- s ij s ij – ------ ≤ 0 3 2

(3-46)

is violated and we scale the trial stresses back to the yield surface; i.e., a radial return

σ s ijn + 1 = -----*y *s ijn + 1 = m * s ijn + 1 s

(3-47)

The plastic strain increment can be found by subtracting the deviatoric part of the strain increment that is elastic,

1 - n + 1 Rn -----(s – s ij ) , from the total deviatoric increment, Δε' ij , i.e., 2G ij

1 Δε ijp = Δε' ij – ------- ( s ijn + 1 – s ijR n ) 2G

(3-48)

Recalling that,

Δε' ij

*s n + 1 ij

R

– s ij n -------------------------= 2G

(3-49)

and substituting Equation (3-49) into Equation (3-48) we obtain,

Δε ijp

( *s ijn + 1 – s ijn + 1 ) = ------------------------------------2G

(3-50)

Substituting Equation (3-47)

s ijn + 1 = m * s ijn + 1 into Equation (3-50) gives,

(1 – m) 1–m Δε ijp = ------------------ *s ijn + 1 = ------------- s ijn + 1 = dλs ijn + 1 2G 2Gm

(3-51)

Materials 89 Materials

By definition an increment in effective plastic strain is 1⁄2 2 Δε p =  --- Δε ijp Δε ijp 3

(3-52)

Squaring both sides of Equation (3-51) leads to:

1–m 2 Δε ijp Δε ijp =  ------------- *s ijn + 1 *s ijn + 1 2G

(3-53)

or from Equations (3-45) and (3-52):

3--- p 2 1 – m 22 Δε =  ------------- --- s *2  2G  3 2

(3-54)

Hence,

s∗ – σ y 1–m ∴Δε p = ------------- s∗ = ----------------3G 3G

(3-55)

where we have substituted for m from Equation (3-47)

σy m = ----s∗ If isotropic hardening is assumed then:

σ yn + 1 = σ yn + E p Δε p

(3-56)

and from Equation (3-55)

Δε p

( s∗ – σ yn + 1 ) ( s∗ – σ yn – E p Δε p ) ---------------------------= = -------------------------------------------3G 3G

(3-57)

Thus,

( 3G + E p )Δε p = ( s∗ – σ yn ) and solving for the incremental plastic strain gives

( s∗ – σ yn ) Δε p = -----------------------( 3G + E p )

(3-58)

90 Materials

The algorithm for plastic loading can now be outlined in five simple stress. If the effective trial stress exceeds the yield stress then 1. Solve for the plastic strain increment:

( s∗ – σ yn ) Δε p = -----------------------( 3G + E p ) 2. Update the plastic strain:

εp

n+1

= ε p + Δε p n

3. Update the yield stress:

σ yn + 1 = σ yn + E p Δε p 4. Compute the scale factor using the yield strength at time

n + 1:

σ yn + 1 m = ------------s∗ 5. Radial return the deviatoric stresses to the yield surface:

s ijn + 1 = m *s ijn + 1

Material Model 12: Isotropic Elastic-Plastic The von Mises yield condition is given by:

σ y2 φ = J 2 – -----3

(3-59)

where the second stress invariant, J 2 , is defined in terms of the deviatoric stress components as

1 J 2 = --- s ij s ij 2

(3-60)

p and the yield stress, σ y , is a function of the effective plastic strain, ε eff , and the plastic hardening

modulus,

Ep :

p σ y = σ 0 + Ep ε eff

(3-61)

Materials 91 Materials

The effective plastic strain is defined as: t p ε eff

=

 dεeff p

(3-62)

0

where: p dε eff =

2--- p p dε dε 3 ij ij

and the plastic tangent modulus is defined in terms of the input tangent modulus,

(3-63)

E t , as:

EE t E p = -------------E – Et

(3-64)

Pressure is given by the expression

1 -  p n + 1 = K  -----------–1 n V +1  where

(3-65)

K is the bulk modulus. This is perhaps the most cost effective plasticity model. Only one history

p variable, ε eff , is stored with this model.

This model is not recommended for shell elements. In the plane stress implementation, a one-step radial return approach is used to scale the Cauchy stress tensor to if the state of stress exceeds the yield surface. This approach to plasticity leads to inaccurate shell thickness updates and stresses after yielding. This is the only model in SOL 700 for plane stress that does not default to an iterative approach. For MD Nastran SOL SEQ 106, 129, and 600, this material model is similar to using the MATS1 option to define an elastic-plastic material.

Material Model 13: Isotropic Elastic-Plastic with Failure This highly simplistic failure model is occasionally useful. Material model 12 is called to update the stress tensor. Failure is initially assumed to occur if either

p n + 1 < p min

(3-66)

or p p ε eff > ε max

(3-67)

92 Materials

where

p p min and ε max are user-defined parameters. Once failure has occurred, pressure may never be

negative and the deviatoric components are set to zero:

s ij = 0

(3-68)

for all time. The failed element can only carry loads in compression.

Material Model 14: Soil and Crushable Foam With Failure This material model provides the same stress update as model 5. However, if pressure ever reaches its cutoff value, failure occurs and pressure can never again go negative. In material model 5, the pressure is limited to its cutoff value in tension.

Material Model 15: Johnson and Cook Plasticity Model Johnson and Cook express the flow stress as n · σ y = ( A + Bε p ) ( 1 + C ln ε∗ ) ( 1 – T∗ m )

where

(3-69)

A , B , C , n , and m are user-defined input constants, and:

ε p = effective plastic strain ·p ε----·∗ · ε = · effective plastic strain rate for ε 0 = 1s –1 ε0 T – T room T∗ = ------------------------------T melt – T room Constants for a variety of materials are provided in Johnson and Cook [1983]. Due to the nonlinearity in the dependence of flow stress on plastic strain, an accurate value of the flow stress requires iteration for the increment in plastic strain. However, by using a Taylor series expansion with linearization about the current time, we can solve for

σ y with sufficient accuracy to avoid iteration.

The strain at fracture is given by

ε f = [ D 1 + D 2 exp D 3 s∗ ] [ 1 + D 4 ln ε∗ ] [ 1 + D 5 T∗ ] where

(3-70)

Di , i = 1 ,… ,5 , are input constants and σ∗ is the ratio of pressure divided by effective stress:

Materials 93 Materials

p σ∗ = -------σ eff

(3-71)

Fracture occurs when the damage parameter,

D =

p Δε ------- εf -

(3-72)

reaches the value 1. A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model limits the minimum hydrostatic pressure to the specified value,

p ≥ p min . If pressures more tensile than this limit are calculated, the pressure is reset to p min . This option is not strictly a spall model since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff and the pressure cutoff value

p min remains unchanged throughout the analysis. The

maximum principal stress spall model detects spall if the maximum principal stress, limiting value

σ max , exceeds the

σ p . Once spall is detected with this model, the deviatoric stresses are reset to zero and no

hydrostatic tension is permitted. If tensile pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as rubble. The hydrostatic tension spall model detects spall if the pressure becomes more tensile than the specified limit, p min . Once spall is detected, the deviatoric stresses are set to zero and the pressure is required to be compressive. If hydrostatic tension is calculated then the pressure is reset to 0 for that element. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element,

Δt max . Generally, Δt max goes

down as the element becomes more distorted. To assure stability of time integration, the global time step is the minimum of the

Δt max values calculated for all elements in the model. Using this option allows

the selective deletion of elements whose time step step,

Δt max has fallen below the specified minimum time

Δt crit . Elements which are severely distorted often indicate that material has failed and supports

little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. Material type 15 is applicable to the high rate deformation of many materials including most metals. Unlike the Steinberg-Guinan model, the Johnson-Cook model remains valid down to lower strain rates and even into the quasistatic regime. Typical applications include explosive metal forming, ballistic penetration, and impact. This material is similar to the use of the ISOTROPIC option with the Johnson-Cook hardening rule.

94 Materials

Material Type 18: Power Law Isotropic Plasticity Elastoplastic behavior with isotropic hardening is provided by this model. The yield stress,

σ y , is a

function of plastic strain and obeys the equation:

σ y = kε n = k ( ε yp + ε p ) n

(3-73)

where ε yp is the elastic strain to yield and ε p is the effective plastic strain (logarithmic). A parameter, SIGY, in the input governs how the strain to yield is identified. If SIGY is set to zero, the strain to yield if found by solving for the intersection of the linearly elastic loading equation with the strain hardening equation:

σ = Eε σ = lε n

(3-74)

which gives the elastic strain at yield as:

ε yp

E =  --- k

1 -----------n–1

(3-75)

If SIGY yield is nonzero and greater than 0.02 then:

σy ε yp  ----- k

1 --n

(3-76)

Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor

· ε 1/p 1 +  ---- C ·

(3-77)

where ε is the strain rate. A fully viscoplastic formulation is optional with this model which incorporates the Cowper and Symonds formulation within the yield surface. An additional cost is incurred but the improvement is results can be dramatic. This material model is a subset of what may be specified through the MATEP option for SOL600.

Materials 95 Materials

Material Type 19: Elastic Plastic Material Model with Strain Rate Dependent Yield In this model, a load curve is used to describe the yield strength

σ 0 as a function of effective strain rate

· ε where · 2· · 1⁄2 ε =  --- ε' ij ε' ij 3 

(3-78)

and the prime denotes the deviatoric component. The yield stress is defined as

· σy = σ0 ( ε ) + Ep ε p where ε p is the effective plastic strain and

(3-79)

E p is given in terms of Young’s modulus and the tangent

modulus by

EE t E p = -------------E – Et

(3-80)

Both Young's modulus and the tangent modulus may optionally be made functions of strain rate by specifying a load curve ID giving their values as a function of strain rate. If these load curve ID's are input as 0, then the constant values specified in the input are used.

Note:

All load curves used to define quantities as a function of strain rate must have the same number of points at the same strain rate values. This requirement is used to allow vectorized interpolation to enhance the execution speed of this constitutive model.

This model also contains a simple mechanism for modeling material failure. This option is activated by specifying a load curve ID defining the effective stress at failure as a function of strain rate. For solid elements, once the effective stress exceeds the failure stress the element is deemed to have failed and is removed from the solution. For shell elements the entire shell element is deemed to have failed if all integration points through the thickness have an effective stress that exceeds the failure stress. After failure the shell element is removed from the solution. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element,

Δt max . Generally, Δt max goes

down as the element becomes more distorted. To assure stability of time integration, the global time step is the minimum of the

Δt max values calculated for all elements in the model. Using this option allows

the selective deletion of elements whose time step

Δt max has fallen below the specified minimum time

96 Materials

step,

Δt crit . Elements which are severely distorted often indicate that material has failed and supports

little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. This material model is a subset of what may be specified through the MATEP option for SOL600.

Material Type 20: Rigid The rigid material type 20 provides a convenient way of turning one or more parts comprised of beams, shells, or solid elements into a rigid body. Approximating a deformable body as rigid is a preferred modeling technique in many real world applications. For example, in sheet metal forming problems the tooling can properly and accurately be treated as rigid. In the design of restraint systems the occupant can, for the purposes of early design studies, also be treated as rigid. Elements which are rigid are bypassed in the element processing and no storage is allocated for storing history variables; consequently, the rigid material type is very cost efficient. Two unique rigid part IDs may not share common nodes unless they are merged together using the rigid body merge option. A rigid body may be made up of disjoint finite element meshes, since this is a common practice in setting up tooling meshes in forming problems. All elements which reference a given part ID corresponding to the rigid material should be contiguous, but this is not a requirement. If two disjoint groups of elements on opposite sides of a model are modeled as rigid, separate part ID's should be created for each of the contiguous element groups if each group is to move independently. This requirement arises from the fact that SOL 700 internally computes the six rigid body degrees-of-freedom for each rigid body (rigid material or set of merged materials), and if disjoint groups of rigid elements use the same part ID, the disjoint groups will move together as one rigid body. Inertial properties for rigid materials may be defined in either of two ways. By default, the inertial properties are calculated from the geometry of the constituent elements of the rigid material and the density specified for the part ID. Alternatively, the inertial properties and initial velocities for a rigid body may be directly defined, and this overrides data calculated from the material property definition and nodal initial velocity definitions. Young's modulus, E , and Poisson's ratio, υ , are used for determining sliding interface parameters if the rigid body interacts in a contact definition. Realistic values for these constants should be defined since unrealistic values may contribute to numerical problem in contact.

Material Model 22: Chang-Chang Composite Failure Model Five material parameters are used in the three failure criteria based upon Chang and Chang 1987a, 1987b:

Materials 97 Materials

•

S 1 , longitudinal tensile strength

• , S 2 transverse tensile strength • , S 12 shear strength

and

•

C 2 , transverse compressive strength

•

α , nonlinear shear stress parameter.

C 2 are obtained from material strength measurement. α is defined by material shear stress-strain

measurements. In plane stress, the strain is given in terms of the stress as

1 ε 1 = ------ ( σ 1 – υ 1 σ 2 ) E1 1 ε 2 = ------ ( σ 2 – υ 2 σ 1 ) E2 1 2ε 12 = --------- τ 12 + ατ 13 G 12

(3-81)

The third equation defines the nonlinear shear stress parameter

α.

A fiber matrix shearing term augments each damage mode: 2 τ 12 4 ----------- + 3--- ατ 12 2G 12 4 τ = ---------------------------------2 S 12 ----------- + 3--- αS 4 2G 12 4 12

(3-82)

which is the ratio of the shear stress to the shear strength. The matrix cracking failure criteria is determined from

σ2 2 F matrix =  ------ + τ S2 where failure is assumed whenever

G 12 , υ , and υ 2 are set to zero.

(3-83)

F matrix > 1 . If F matrix > 1 , then the material constants E2 ,

98 Materials

The compression failure criteria is given as

σ2 σ2 2 C2 2 F comp =  ----------- +  ----------- – 1 ------ + τ  2S 12  2S 12 C2 where failure is assumed whenever and

(3-84)

F comp > 1 . If F comp > 1 , then the material constants E2 , υ 1 ,

υ 2 are set to zero.

The final failure mode is due to fiber breakage.

σ1 2 F fiber =  ------ + τ S1 Failure is assumed whenever

(3-85)

F fiber > 1 . If F fiber > 1 , then the constants E 1 , E 2 , G 12 , υ 1 , and

υ 2 are set to zero.

Material Model 24: Piecewise Linear Isotropic Plasticity This plasticity treatment in this model is quite similar to Model 3 but only isotropic hardening occurs. Deviatoric stresses are determined that satisfy the yield function

σ2 1 φ = --- s ij s ij – -----y- ≤ 0 2 3

(3-86)

where p σ y = β [ σ 0 + f h ( ε eff )]

(3-87)

p ) can be specified in tabular form as an option. Otherwise, linear where the hardening function f h ( ε eff hardening of the form p p f h ( ε eff ) = E p ( ε eff )

is assumed where

(3-88)

p are given in Equations (3-16) and (3-17), respectively. The parameter β Ep and ε eff

accounts for strain rate effects. For complete generality a table defining the yield stress versus plastic strain may be defined for various levels of effective strain rate. In the implementation of this material model, the deviatoric stresses are updated elastically (see material model 1), the yield function is checked, and if it is satisfied the deviatoric stresses are accepted. If it is not, an increment in plastic strain is computed:

Materials 99 Materials

1⁄2

p Δε eff

 3--- s * s *  – σy  2 ij ij = ---------------------------------------3G + Ep

is the shear modulus and

(3-89)

E p is the current plastic hardening modulus. The trial deviatoric stress state

s ij* is scaled back: σy - s ij* s ijn + 1 = --------------------------1 ⁄ 2  3--- s * s *   2 ij ij

(3-90)

For shell elements, the above equations apply, but with the addition of an iterative loop to solve for the normal strain increment, such that the stress component normal to the mid surface of the shell element approaches zero. Three options to account for strain rate effects are possible: • Strain rate may be accounted for using the Cowper and Symonds model which scales the yield

stress with the factor

· ε- 1 ⁄ p  --β = 1+  C where

(3-91)

· ε is the strain rate.

• For complete generality a load curve, defining

β , which scales the yield stress may be input

instead. In this curve the scale factor versus strain rate is defined. • If different stress versus strain curves can be provided for various strain rates, the option using

the reference to a table definition can be used. A fully viscoplastic formulation is optional which incorporates the different options above within the yield surface. An additional cost is incurred over the simple scaling but the improvement is results can be dramatic. If a table ID is specified a curve ID is given for each strain rate. Intermediate values are found by interpolating between curves.

Material Model 26: Crushable Foam This orthotropic material model does the stress update in the local material system denoted by the subscripts, •

a , b , and c . The material model requires the following input parameters:

E , Young’s modulus for the fully compacted material;

100 Materials

•

ν , Poisson’s ratio for the compacted material;

•

σ y , yield stress for fully compacted honeycomb;

• LCA, load curve number for sigma-aa versus either relative volume or volumetric strain (see Figure 3-3);

σ

ij Unloading and reloading path

0

Strain

Curve extends into negative strain quadrant since SOL 700 extrapolates using the two end points. It is important that the extrapolation does not extend into the negative stress region.

Figure 3-3

–ε

ij Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent.

Stress Quantity Versus Volumetric Strain

Note that in Figure 3-3, the “yield stress” at a volumetric strain of zero is nonzero. In the load curve definition, the “time” value is the volumetric strain and the “function” value is the yield stress. • LCB, load curve number for sigma-bb versus either relative volume or volumetric strain

(default: LCB = LCA); • LCC, the load curve number for sigma-cc versus either relative volume or volumetric strain

(default: LCC = LCA); • LCS, the load curve number for shear stress versus either relative volume or volumetric strain

(default LCS = LCA); •

V f , relative volume at which the honeycomb is fully compacted;

•

E aau , elastic modulus in the uncompressed configuration;

•

E bbu , elastic modulus in the uncompressed configuration;

Materials 101 Materials

•

E ccu , elastic modulus in the uncompressed configuration;

•

G abu , elastic shear modulus in the uncompressed configuration;

•

G bcu , elastic shear modulus in the uncompressed configuration;

•

Gcau , elastic shear modulus in the uncompressed configuration;

• LCAB, load curve number for sigma-ab versus either relative volume or volumetric strain

(default: LCAB = LCS); • LCBC, load curve number for sigma-bc versus either relative volume or volumetric strain

default: LCBC = LCS); • LCCA, load curve number for sigma-ca versus either relative volume or volumetric strain

(default: LCCA = LCS); • LCSR, optional load curve number for strain rate effects.

The behavior before compaction is orthotropic where the components of the stress tensor are uncoupled; i.e., an a component of strain will generate resistance in the local a direction with no coupling to the local b and c directions. The elastic moduli vary linearly with the relative volume from their initial values to the fully compacted values:

E aa = E aau + β ( E – E aau ) E bb = E bbu + β ( E – E bbu ) E cc = E ccu + β ( E – E ccu ) G ab = G abu + β ( G – G abu ) G bc = G bcu + β ( G – G bcu ) G ca = G cau + β ( G – G cau )

(3-92)

where

1 – Vmin  -, 1 , 0 β = max min  ------------------ 1 – Vf  and

(3-93)

G is the elastic shear modulus for the fully compacted honeycomb material

E G = -------------------2(1 + ν)

(3-94)

V is defined as the ratio of the current volume over the initial volume; typically, V = 1 at the beginning of a calculation. The relative volume, V min , is the minimum value reached

The relative volume

during the calculation.

102 Materials

The load curves define the magnitude of the average stress as the material changes density (relative volume). Each curve related to this model must have the same number of points and the same abscissa values. There are two ways to define these curves: as a function of relative volume of volumetric strain defined as:

εV = 1 – V

V , or as a function (3-95)

In the former, the first value in the curve should correspond to a value of relative volume slightly less than the fully compacted value. In the latter, the first value in the curve should be less than or equal to zero corresponding to tension and should increase to full compaction.

Note:

When defining the curves, care should be taken that the extrapolated values do not lead to negative yield stresses.

At the beginning of the stress update we transform each element’s stresses and strain rates into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated moduli according to: n+1

trial

n+1

trial

n+1

trial

n+1

trial

n+1

trial

n+1

trial

σ aa σ bb σ cc

σ ab σ bc

σ ca

n

= σ aa + E aa Δε aa n

= σ bb + E bb Δε bb n

= σ cc + E cc Δε cc n

= σ ab + E ab Δε ab n

= σ bc + E bc Δε bc n

= σ ca + E ca Δε ca

(3-96)

Then we independently check each component of the updated stresses to ensure that they do not exceed the permissible values determined from the load curves; e.g., if

σ ijn + 1

trial

> λσ ij ( V min )

(3-97)

then

λσ ijn + 1 = σ ij ( V min ) ---------------------trial σ ijn + 1

trial

σ ijn + 1

(3-98)

Materials 103 Materials

The parameter λ is either unity or a value taken from the load curve number, LCSR, that defines λ as a function of strain rate. Strain rate is defined here as the Euclidean norm of the deviatoric strain rate tensor. For fully compacted material we assume that the material behavior is elastic-perfectly plastic and updated the stress components according to:

s ijtrial = s ijn + 2GΔε ijdev

n+1⁄2

(3-99)

Where the deviatoric strain increment is defined as:

1 Δε ijdev = Δε ij – --- Δε kk δ ij 3

(3-100)

We next check to see if the yield stress for the fully compacted material is exceeded by comparing: 1⁄2 3 trial s eff =  --- s ijtrial s ijtrial 2

the effective trial stress, to the yield stress

(3-101)

σ y . If the effective trial stress exceeds the yield stress, we

simply scale back the stress components to the yield surface:

σ y trial -s s ijn + 1 = ---------trial ij s eff We can now update the pressure using the elastic bulk modulus,

(3-102)

K:

n+1⁄2 p n + 1 = p n – KΔε kk E K = ----------------------3 ( 1 – 2ν )

(3-103)

and obtain the final value for the Cauchy stress:

σ ijn + 1 = s ijn + 1 – p n + 1 δ ij After completing the stress update, we transform the stresses back to the global configuration.

(3-104)

104 Materials

Material Model 27: Incompressible Mooney-Rivlin Rubber This material model, available for solid elements only, provides an alternative to the Blatz-Ko rubber model. The strain energy density function is defined as in terms of the input constants

A , B ,, and υ as:

1 W ( I 1 ,I 2 ,I 2 ) = A ( I 1 – 3 ) + B ( I 2 – 3 ) + C  ---2- – 1 + D ( I 3 – 1 ) 2 I  3

(3-105)

where

C = .5∗ A + B

(3-106)

A ( 5υ – 2 ) + B ( 11υ – 5 ) D = ---------------------------------------------------------2 ( 1 – 2υ )

(3-107)

υ = Poisson’s ratio G = 2 ( A + B ) = shear modulus of linear elasticity I 1 ,I 2 ,I 3 = strain invariants in terms of the principal stretches: 2

2

2

I1 = λ 1 + λ 2 + λ3 2 2

2 2

2 2

I2 = λ 1 λ 2 + λ 2 λ 3 + λ3 λ 1 2 2 2

I3 = λ1 λ2 λ3

(3-108)

Recommended values for Poisson’s ratio are between .490 and .495 or higher. Lower values may lead to instabilities. In the derivation of the constants

C and D incompressibility is assumed.

Material Model 28: Resultant Plasticity This plasticity model, based on resultants as illustrated in Figure 3-4, is very cost effective but not as accurate as through-thickness integration. This model is available only with the C 0 triangular, Belytschko-Tsay shell, and the Belytschko beam element since these elements, unlike the Hughes-Liu

Materials 105 Materials

elements, lend themselves very cleanly to a resultant formulation. The elements are set by the SHELLFORM parameter.

σy

Membrane

ny =



= hσ y

σy

Bending

my = Figure 3-4

h --2 σ dζ h y – --2

h --2 σ ζ dζ h--- y – 2



h2 = ----- σ y 4

Full Section Yield using Resultant Plasticity

In applying this model to shell elements the resultants are updated incrementally using the midplane strains ε m and curvatures

κ:

Δn = ΔtCε m

(3-109)

h3 Δm = Δt ------ Cκ 12

(3-110)

where the plane stress constitutive matrix is given in terms of Young’s Modulus

E and Poisson’s ratio

ν as: 2 – m m + m 2 + 3m 2 m = mxx xx yy yy xy

(3-111)

Defining 2 – n n + n 2 + 3n 2 n = n xx xx yy yy xy

(3-112)

2 – m m + m 2 + 3m 2 m = mxx xx yy yy xy

(3-113)

1 1 mn = m xx n xx – --- m xx n yy – --- n xx m yy + m y n y + 3m xy n xy 2 2

(3-114)

the Ilyushin yield function becomes

4 mn 16mf ( m, n ) = n + ------------- + --------≤ n y2 = h 2 σ y2 h2 h 3

(3-115)

106 Materials

In our implementation we update the resultants elastically and check to see if the yield condition is violated:

f ( m, n ) > n y2 If so, the resultants are scaled by the factor

α =

(3-116)

α:

n y2 ----------------f ( m, n )

(3-117)

We update the yield stress incrementally: eff σ yn + 1 = σ yn + E p Δε plastic

where

(3-118)

E p is the plastic hardening modulus which in incremental plastic strain is approximated by

f ( m, n ) – n y eff Δε plastic = ------------------------------h ( 3G + E p )

(3-119)

Kennedy, et. al., report that this model predicts results that may be too stiff; users of this model should proceed cautiously. In applying this material model to the Belytschko beam, the flow rule changes to

ˆ y2 4m ˆ z2 4m f ( m, n ) = ˆf x2 + ---------- + ---------- ≤ n y2 = A 2 σ y2 3I yy 3I zz

(3-120)

have been updated elastically according to Equations (3-112) through (3-114). The yield condition is checked Equation (3-116), and if it is violated, the resultants are scaled as described above. This model is frequently applied to beams with nonrectangular cross sections. The accuracy of the results obtained should be viewed with some healthy suspicion. No workhardening is available with this model.

Material Model 29: FORCE LIMITED Resultant Formulation This material model is available for the Belytschko beam element only. Plastic hinges form at the ends of the beam when the moment reaches the plastic moment. The momentversus- rotation relationship is specified by the user in the form of a load curve and scale factor. The point pairs of the load curve are (plastic rotation in radians, plastic moment). Both quantities should be positive for all points, with the first point pair being (zero, initial plastic moment). Within this

Materials 107 Materials

constraint any form of characteristic may be used including flat or falling curves. Different load curves and scale factors may be specified at each node and about each of the local s and t axes. Membrane

σy ny =

Bending



= hσ y

σy my =

Figure 3-5

h --2 σ dζ h y – --2

h --2 σ ζ dζ h--- y – 2



h2 = ----- σ y 4

Full Section Yield using Resultant Plasticity

Axial collapse occurs when the compressive axial load reaches the collapse load. The collapse loadversus-collapse deflection is specified in the form of a load curve. The points of the load curve are (true strain, collapse force). Both quantities should be entered as positive for all points, and will be interpreted as compressive i.e., collapse does not occur in tension. The first point should be the pair (zero, initial collapse load). The collapse load may vary with end moment and with deflection. In this case, several load-deflection curves are defined, each corresponding to a different end moment. Each load curve should have the same number of point pairs and the same deflection values. The end moment is defined as the average of the absolute moments at each end of the beam, and is always positive.

108 Materials

It is not possible to make the plastic moment vary with axial load. M8 M7 M6 M5 M4 Force

M3 M2 M1

Displacement

Figure 3-6

The Force Magnitude Limited Applied End Moment

For an intermediate value of the end moment, MD Nastran SOL 700 interpolates between the curves to determine the allowable force. A co-rotational technique and moment-curvature relations are used to compute the internal forces. The co-rotational technique will not be treated here as we will focus solely on the internal force update and computing the tangent stiffness. For this, we use the notation:

E = G = A = As = ln = l n + 1= I yy = I zz = J = ei = yI = zI =

Young’s modulus Shear modulus Cross sectional area Effective area in shear Reference length of beam Current length of beam Second moment of inertia about y Second moment of inertia about z Polar moment of inertia ith local base vector in the current configuration nodal vector in y direction at node I in the current configuration nodal vector in z direction at node I in the current configuration

Materials 109 Materials

We emphasize that the local y and z base vectors in the reference configuration always coincide with the corresponding nodal vectors. The nodal vectors in the current configuration are updated using the Hughes-Winget formula while the base vectors are computed from the current geometry of the element and the current nodal vectors. Internal Forces Elastic Update In the local system for a beam connected by nodes I and J, the axial force is updated as

f ael = f an + K ael δ

(3-121)

where

EAK ael = -----ln

(3-122)

δ = l n + 1 – l n ..

(3-123)

The torsional moment is updated as m tel = m tn + K tel θ t

(3-124)

where

GJK tel = -----ln

(3-125)

1 θ t = --- eTl ( y I × y J + z I × z J ) . 2

(3-126)

The bending moments are updated as n el mel y = my + Ay θy

(3-127)

n el mel z = mz + Az θz

(3-128)

where

1 EI **-  4 + φ* 2 – φ *  A *el = --------------- --------  1 + φ* l n  2 – φ 4 + φ  * *

(3-129)

110 Materials

12EI ** φ * = ------------------GA * l n t n

(3-130)

θTy = eT3  y I × z I y J × z J   

(3-131)

θTz = eT2  y I × z I y J × z J   

(3-132)

In the following, we refer to

A *el as the (elastic) moment-rotation matrix.

Plastic Correction After the elastic update the state of force is checked for yielding as follows. As a preliminary note we emphasize that whenever yielding does not occur the elastic stiffnesses and forces are taken as the new stiffnesses and forces. The yield moments in direction i at node I as functions of plastic rotations are denoted

mYiI ( θ iIP ) . This

function is given by the user but also depends on whether a plastic hinge has been created. The theory for plastic hinges is given in the LS-DYNA Keyword User’s Manual [Hallquist 2003] and is not treated here. Whenever the elastic moment exceeds the plastic moment, the plastic rotations are updated as

θ iIP ( n + 1 )

=

θ iIP ( n )

m iIel – mYiI + --------------------------------------------------------------∂mYiI   - max  0.001, A iel( II ) + ---------∂θ iIP  

(3-133)

and the moment is reduced to the yield moment

m iIn + 1 = m iIY ( θ iIP ( n + 1 ) ) sgn ( m iIel )

(3-134)

The corresponding diagonal component in the moment-rotation matrix is reduced as

A in( II+ )1

where

    el A i ( II )  el  = A i ( II )  1 – α ---------------------------------------------------------------  ∂m iIY    el -   max  0.001, Ai ( II ) + ---------  ∂θ iIP  

(3-135)

α ≤ 1 is a parameter chosen such that the moment-rotation matrix remains positive definite.

Materials 111 Materials

The yield moment in torsion is given by

mYt ( θPt ) and is provided by the user. If the elastic torsional

moment exceeds this value, the plastic torsional rotation is updated as

θ tP ( n + 1 )

=

θ tP ( n )

m tel – mYt -----------------------------------------------------------+ Y ∂m t   max  0.0001, K tel + ----------  ∂θ tP 

(3-136)

and the moment is reduced to the yield moment

m tn + 1 = mYt ( θ tP ( n + 1 ) ) sgn ( mel t ) The torsional stiffness is modified as

K tn + 1

  el   K t el  - = K t  1 – α -----------------------Y el ∂m t   + ---------P- K t  ∂θ

(3-137)

t

where again

α ≤ 1 is chosen so that the stiffness is positive. Y

Axial collapse is modeled by limiting the axial force by f a ( ε, m ) ; i.e., a function of the axial strains and the magnitude of bending moments. If the axial elastic force exceeds this value it is reduced to yield

f an + 1 = fYa ( ε n + 1, m n + 1 ) sgn ( f ael )

(3-138)

and the axial stiffness is given by

K an + 1

Y el ∂f a   = max  0.05K a ,-------- ∂ε

We neglect the influence of change in bending moments when computing this parameter. Damping Damping is introduced by adding a viscous term to the internal force on the form

(3-139)

112 Materials

δ d θt f v = D ----dt θ y

(3-140)

θz K ael K tel

D = γ

(3-141)

Ael y A zel

where γ is a damping parameter. Transformation The internal force vector in the global system is obtained through the transformation

f gn + 1 = Sf tn + 1

(3-142)

where

– e1 0 – e3 ⁄ l n + 1 –e3 ⁄ l n + 1 e2 ⁄ l n + 1 e2 ⁄ l n + 1 S =

0 –e1 e1

0

0

e1

e2

0

e3

0

e3 ⁄ l n + 1 e3 ⁄ l n + 1 –e2 ⁄ l n + 1 –e2 ⁄ l n + 1 0

e2

0

(3-143)

e3

f an + 1 f ln + 1

=

mnt + 1 m yn + 1 m zn + 1

(3-144)

Materials 113 Materials

Tangent Stiffness Derivation The tangent stiffness is derived from taking the variation of the internal force

δf gn + 1 = δSf ln + 1 + Sδf ln + 1

(3-145)

which can be written

δf gn + 1 = K geo δu + K mat δu where T

δu =  δxTI δωTI δxTJ δωTj  .

(3-146)

There are two contributions to the tangent stiffness: geometrical and material. The geometrical contribution is given (approximately) by

1 Tf n + 1 L K geo = R ( f ln + 1 ⊗ I )W – ---------------------n + 1 l ln + 1 l

(3-147)

where

R =

R1

0

0

R1

R 3 ⁄ l n + 1 R 3 ⁄ l n + 1 – R2 ⁄ l n + 1 –R 2 ⁄ ( n + 1 ) –R2

–R1 0 –R 3 ⁄ 0 –R1

0

ln + 1

0

–R3 ⁄

ln + 1

–R2

–R3 R2 ⁄

ln + 1 0

W =  – R 1 ⁄ l n + 1 e 1 eT1 ⁄ 2 R 1 ⁄ l n + 1 e 1 eT1 ⁄ 2   

0 R2 ⁄

(3-148)

ln + 1

–R3 (3-149)

0 0 –e3 –e3 e2 e2 T = 00 0 0 0 0 0 0 e 3 e3 – e2 –e 2 00 0

0

L =  eT1 0 eT1 0 

0

(3-150)

0 (3-151)

114 Materials

and I is the 3 by 3 identity matrix. We use ⊗ as the outer matrix product and define

Ri v = ei × v .

(3-152)

The material contribution can be written as

K mat = SKS T

(3-153)

where

K an + 1 K =

K tn + 1

(3-154)

A yn + 1 A zn + 1

Material Model 30: Shape Memory Alloy This section presents the mathematical details of the shape memory alloy material in MD Nastran SOL 700. The description closely follows the one of Auricchio and Taylor [1997] with appropriate modifications for this particular implementation. Mathematical Description of the Material Model The Kirchhoff stress

τ in the shape memory alloy can be written

τ = pi + t

(3-155)

where i is the second order identity tensor and

p = K ( θ – 3αξ S ε L

.

(3-156)

t = 2G ( e – ξ S ε L n ) Here K and G are bulk and shear modulii,

θ and e are volumetric and shear logarithmic strains and α

and ε L are constant material parameters. There is an option to define the bulk and shear modulii as functions of the martensite fraction according to

K = KA + ξS ( K S – K A ) G = GA + ξ S ( G S – GK A

(3-157)

Materials 115 Materials

in case the stiffness of the martensite differs from that of the austenite. Furthermore, the unit vector n is defined as

n = e ⁄ ( e + 10 –12 )

(3-158)

and a loading function is introduced as

F = 2G e + 3αKθ – βξ S

(3-159)

where

β = ( 2G + 9α 2 K )ε L .

(3-160)

For the evolution of the martensite fraction ξ S in the material, the following rule is adopted

  ·  F -----------------  ξS = –( 1 – ξS ) F – R fAS     F – R sSA < 0  ·  F · ----------------- = ξ ξ  S S F>0 F – R fSA  ξS > 0   F – R sAS > 0 · F>0 ξS < 1

Here

.

(3-161)

R sAS , R fAS , RsSA , and R fSA are constant material parameters. The Cauchy stress is finally

obtained as

σ = τ⁄J

(3-162)

where J is the Jacobian of the deformation. Algorithmic Stress Update n

For the stress update, we assume that the martensite fraction ξ s and the value of the loading function

F n is known from time t n and the deformation gradient at time t n + 1 , F , is known. We form the left Cauchy-Green tensor as

B = FF T which is diagonalized to obtain the principal values and directions

Λdiag ( λ i ) and Q . The volumetric and principal shear logarithmic strains are given by

116 Materials

θ = log ( J ) e i = log ( λ i ⁄ J 1 ⁄ 3 where

J = λ1 λ2 λ3 n

is the total Jacobian of the deformation. Using Equation (3-159) with ξ S = ξ S , a value F trial of the loading function can be computed. The discrete counterpart of Equation (3-161) becomes

 F trial – R sAS > 0  F trial – βΔξ S – min ( max ( F n ,RsAS ) ,R fAS )  n F trial – F n > 0   Δξ S = – ( 1 – ξ S – Δξ S ) -----------------------------------------------------------------------------------------------AS trial F – βΔξ S – R f  ξ Sn < 1    F trial – R sSA > 0  F trial – βΔξ S – min ( max ( F n ,R sSA ) ,R fSA )  n F trial – F n > 0   Δξ S = ( ξ S + Δξ S ) -----------------------------------------------------------------------------------------------trial – βΔξ – R SA F  S f ξ Sn < 1   (3-163)

n+1

If none of the two conditions to the left are satisfied, set ξ S the stress

= ξ Sn , F n + 1 = F trial , and compute

σ n + 1 using Equations (3-155), (3-156), (3-157), (3-162) and ξ S = ξ Sn . When phase

transformation occurs according to a condition to the left, the corresponding equation to the right is solved for well as

.

Δξ S . If the bulk and shear modulii are constan,t this is an easy task. Otherwise, F trial as

β depends on this parameter and makes things a bit more tricky. We have that

ES – EA F trial = F ntrial  1 + ------------------ Δξ S En ES – EA β = β n  1 + ------------------ Δξ S En

where

E S and EA are Young’s modulii for martensite and austenite, respectively. The subscript n is

introduced for constant quantities evaluated at time t n . To simplify the upcoming expressions, these relations are written

Materials 117 Materials

F trial = F ntrial + ΔF trial Δξ S β = β n + ΔβΔξ S

(3-164)

respectively, where we have for simplicity set Inserting these expressions into Equation (3-163) results in

˜n f ( Δξ S ) = Δβ ( 1 – ξ Sn )Δξ S2 + ( R fAS – F AS + ( β n – ΔF trial ) ( 1 – ξ Sn ) )Δξ S + ˜n ( 1 – ξ Sn ) ( F AS – F ntrial ) = 0

(3-165)

and

˜n f ( Δξ S ) = Δβξ Sn Δξ S2 + ( FSA – R fSA + ( β n – ΔF trial )ξ Sn )Δξ S + ˜n ξ Sn ( F SA – F ntrial ) = 0 respectively, where we have for simplicity set

˜n F AS = min ( max ( F n, RsAS ) ,R fAS ) ˜n F SA = min ( max ( F n, RfSA ) ,R sSA )

.

The solutions to these equations are approximated with two Newton iterations starting in the point

Δξ S = 0 .. Now set ξ Sn + 1 = min ( 1 ,max ( 0 ,ξ Sn + Δξ S ) ) and compute σ n + 1 and F n + 1 according to Equations (3-155), (3-156), (3-157), (3-158), (3-160) and

ξ S = ξ Sn + 1 .

Tangent Stiffness Matrix An algorithmic tangent stiffness matrix relating a change in true strain to a corresponding change in Kirchhoff stress is derived in the following. Taking the variation of Equation (3-156) results in

δp = K ( δθ – 3αδξ S ε L ) + δK ( θ – 3αξ S ε L ) δt = 2G ( δe – δξS ε L n – ξ S ε L δn ) + 2δG ( e – ξ S ε L n )

.

The variation of the unit vector in Equation (3-157) can be written

1 ( I – n ⊗ n )δe δn = -------------------------e + 10 – 12

(3-166)

118 Materials

where I is the fourth order identity tensor. For the variation of martensite fraction, we introduce the indicator parameters

H AS and H SA that should give information of the probability of phase

transformation occurring in the next stress update. Set initially according to

H AS = H SA = 0 and change them

 F trial – R sAS > 0   AS F trial – F n > 0   H = 1  ξ Sn + Δξ S ≤ 1    F trial – R sSA > 0   SA F trial – F n > 0   H = 1  ξ Sn + Δξ S ≥ 0   using the quantities computed in the previous stress update. For the variation of the martensite fraction we take variations of Equations(3-165) and (3-166) with

δF ntrial = 2Gn:δe + 3αKδθ which results in

δξ S = γ ( 2Gn:δe + 3αKδθ ) where n

( 1 – ξ S )H AS ξ Sn H SA - + ----------------------------------------------------------------------. γ = -----------------------------------------------------------------------------------˜n ˜n R fAS – F AS + ( β n – ΔF ntrial ) ( 1 – ξ Sn ) F SA – R fSA + ( β n – ΔFntrial )ξ Sn As can be seen, we use the value of γ obtained in the previous stress update since this is easier to implement and will probably give a good indication of the current value of this parameter. The variation of the material parameters K and G results in

δK = ( K S – K A )δξ S δG = ( G S – G A )δξ and, finally, using the identities

Materials 119 Materials

n:δe = n:δε δθ = i:δε δτ = iδp + δt results in

ξ S ε L  dev  I + K ( 1 – 9α 2 Kγε L + 3αγ ( K S – K A ) ( θ – 3αξ S ε L ) )i ⊗ i + δτ =  2G  1 – -------------------------– 12  e + 10  2γG ( K S – K A ) ( θ – 3αξ S ε L )i ⊗ n + 6γαK ( G S – G A ) ( e – ξ S ε L )n ⊗ i + ξS εL 2G  ----------------------------------– 2Gγε L + 2γ ( G S – G A ) ( e – ξ D ε L )  e + 1 – 10 –12  n ⊗ n – 6KGαγε L ( i ⊗ n + n ⊗ i ) }δε where I dev is the fourth order deviatoric identity tensor. In general this tangent is not symmetric because of the terms on the second line in the expression above. We simply use a symmetrization of the tangent stiffness above in the implementation. Furthermore, we transform the tangent to a tangent closer related to the one that should be used in the MD Nastran SOL 700 implementation,

ξS εL    I dev + K ( 1 – 9α 2 Kγε L + 3αγ ( K S – K A ) ( θ – 3αξ S ε L ) )i ⊗ i +  2G  1 – -------------------------– 12 e + 10  K S – K A ) ( θ – 3αξ S ε L ) + 3γαK ( G S – G A ) ( e – ξ S ε L ) – 6KGαγε L ) ( i ⊗ n + n ⊗ i ) +

–1

ξS εL  n ⊗ n δε 2Gγε 2G  -------------------------– + 2γ ( G – G ) ( e – ξ ε )  L S A S L  e + 10 –12 

Material Model 31: Slightly Compressible Rubber Model This model implements a modified form of the hyperelastic constitutive law first described in [Kenchington 1988]. The strain energy functional,

U , is defined in terms of the input constants as:

= C 100 I 1 + C 200 I 12 + C 300 I 13 + C 400 I 14 + C 110 I 1 I 2 + C 210 I 12 I 2 + C 010 I 2 + C 020 I 22 + j

(3-167)

where the strain invariants can be expressed in terms of the deformation gradient matrix, Green-St. Venant strain tensor,

E ij :

F ij , and the

120 Materials

J = F ij I 1 = E ii . 1--- ij I 2 = δ pq E pi Eq 2 The derivative of

U with respect to a component of strain gives the corresponding component of stress

∂U S ij = --------∂E ij where,

(3-168)

(3-169)

S ij , is the second Piola-Kirchhoff stress tensor which is transformed into the Cauchy

stress tensor:

ρ ∂x i ∂x j σ ij = ----- --------- -------- S kl ρ o ∂X k ∂X l where

(3-170)

ρ o and ρ are the initial and current density, respectively.

Material Model 32: Laminated Glass Model This model is available for modeling safety glass. Safety glass is a layered material of glass bonded to a polymer material which can undergo large strains. The glass layers are modeled by isotropic hardening plasticity with failure based on exceeding a specified level of plastic strain. Glass is quite brittle and cannot withstand large strains before failing. Plastic strain was chosen for failure since is increases monotonically and, therefore, is insensitive to spurious numberical noise in the solution. The material to which the glass is bonded is assumed to stretch plastically without failure. The user defined integration rule option must be used with this material. The user defined rule specifies the thickness of the layers making up the safety glass. Each integration point is flagged with a zero if the layer is glass and with a one if the layer is polymer. An iterative plane stress plasticity algorithm is used to enforce the plane stress condition.

Material Model 34: Fabric The fabric model is a variation on the Layered Orthotropic Composite material model (Material 22) and is valid for only 3 and 4 node membrane elements. This material model is strongly recommended for modeling airbags and seatbelts. In addition to being a constitutive model, this model also invokes a special membrane element formulation that is better suited to the large deformations experienced by fabrics. For thin fabrics, buckling (wrinkling) can occur with the associated inability of the structure to support compressive stresses; a material parameter flag is included for this option. A linear elastic liner

Materials 121 Materials

is also included which can be used to reduce the tendency for these material/elements to be crushed when the no-compression option is invoked. If the airbag material is to be approximated as an isotropic elastic material, then only one Young’s modulus and Poisson’s ratio should be defined. The elastic approximation is very efficient because the local transformations to the material coordinate system may be skipped. If orthotropic constants are defined, it is very important to consider the orientation of the local material system and use great care in setting up the finite element mesh. If the reference configuration of the airbag is taken as the folded configuration, the geometrical accuracy of the deployed bag will be affected by both the stretching and the compression of elements during the folding process. Such element distortions are very difficult to avoid in a folded bag. By reading in a reference configuration, such as the final unstretched configuration of a deployed bag, any distortions in the initial geometry of the folded bag will have no effect on the final geometry of the inflated bag. This is because the stresses depend only on the deformation gradient matrix:

∂x i F ij = -------∂X j where the choice of

(3-171)

X j may coincide with the folded or unfold configurations. It is this unfolded

configuration which may be specified here. When the reference geometry is used, then the no-compression option should be active. With the reference geometry, it is possible to shrink the airbag and then perform the inflation. Although the elements in the shrunken bag are very small, the time step can be based on the reference geometry so a very reasonable time step size is obtained. The reference geometry based time step size is optional in the input. The parameters fabric leakage coefficient, FLC, fabric area coefficient, FAC, and effective leakage area, ELA, for the fabric in contact with the structure are optional for the Wang-Nefske and hybrid inflation models. It is possible for the airbag to be constructed of multiple fabrics having different values of porosity and permeability. The gas leakage through the airbag fabric then requires an accurate determination of the areas by part ID available for leakage. The leakage area may change over time due to stretching of the airbag fabric or blockage when the outer surface of the bag is in contact with the structure. MD Nastran SOL 700 can check the interaction of the bag with the structure and split the areas into regions that are blocked and unblocked depending on whether the regions are in contact or not, respectively. Typically, the parameters, FLC and FAC, must be determined experimentally and their variation with time and pressure are optional inputs that allow for maximum modeling flexibility.

Material Models 54 and 55: Enhanced Composite Damage Model These models are very close in their formulations. Material 54 uses the Chang matrix failure criterion (as Material 22), and Material 55 uses the Tsai-Wu criterion for matrix failure. Arbitrary orthothropic materials, e.g., unidirectional layers in composite shell structures can be defined. Optionally, various types of failure can be specified following either the suggestions of [Chang and Chang, 1984] or [Tsai and Wu, 1981]. In addition special measures are taken for failure under

122 Materials

compression. See [Matzenmiller and Schweizerhof, 1990]. This model is only valid for thin shell elements. The Chang/Chang criteria is given as follows: for the tensile fiber mode,

σ ab aa > 0 failed , σ aa > 0 then e 2 =  σ ------- + β  ------f  Xt   S c  – 1 < 0 elastic E a = E b = G ab = ν ba = ν ab = 2

(3-172)

for the compressive fiber mode,

σ aa σ aa > 0 then e c2 =  -------- – 1 > 0 failed , < 0 elastic Xc E a = ν ba = ν ab = 0 2

(3-173)

for the tensile matrix mode, 2 σ ab 2 bb σ bb > 0 then e 2 =  σ ------- +  ------- – 1 > 0 failed , m  Yt   Sc  < 0 elastic E b = ν ba = 0. → G ab =

(3-174)

and for the compressive matrix mode, 2 σ bb  σ ab 2 Yc  2 bb σ bb < 0 then e 2 =  σ  ------------------- + -------- – 1 > 0 failed + – 1 d  2Sc  2S t < 0 elastic Yc  Sc  E b = ν ba = ν ab = 0. → G ab = X c = 2Y c for 50% fiber volume

(3-175)

In the Tsai/Wu criteria the tensile and compressive fiber modes are treated as in the Chang/Chang criteria. The failure criterion for the tensile and compressive matrix mode is given as: 2 σ bb σ ab 2 ( Y c – Y t )σ bb 2 e md = ---------- +  -------- + ------------------------------ – 1 > 0 failed < 0 elastic Yc Yt Sc Yc Yt

(3-176)

For

β = 1 , we get the original criterion of Hashin [1980] in the tensile fiber mode.

For

β = 0 , we get the maximum stress criterion which is found to compare better to experiments.

Failure can occur in any of four different ways:

Materials 123 Materials

1. If DFAILT is zero, failure occurs if the Chang/Chang failure criterion is satisfied in the tensile fiber mode. 2. If DFAILT is greater than zero, failure occurs if the tensile fiber strain is greater than DFAILT or less than DFAILC. 3. If EFS is greater than zero, failure occurs if the effective strain is greater than EFS. 4. If TFAIL is greater than zero, failure occurs according to the element time step as described in the definition of TFAIL above. When failure has occurred in all the composite layers (through-thickness integration points), the element is deleted. Elements which share nodes with the deleted element become “crashfront” elements and can have their strengths reduced by using the SOFT parameter with TFAIL greater than zero. Information about the status in each layer (integration point) and element can be plotted using additional integration point variables. The number of additional integration point variables for shells written to the database is input by the PARAM, DYNEIPS definition as variable NEIPS. For Models 54 and 55 these additional variables are tabulated below (i = shell integration point): History Variable

Description

Value

d3plot Component

1. ef(i)

tensile fiber mode

81

2. ec(i)

compressive fiber mode

1 - elastic

82

3. em(i)

tensile matrix mode

0 - failed

83

4. ed(i)

compressive matrix mode

84

5. efail

max[ef(ip)]

85

6. dam

damage parameter

-1 - element intact 10-8 - element in crashfront +1 - element failed

86

124 Materials

These variables can be plotted in MD Patran as element components 81, 82, ..., 80+ NEIPS. The following components, defined by the sum of failure indicators over all through-thickness integration points, are stored as element component 7 instead of the effective plastic strain: Description

Integration Point

nip

1------ef ( i ) nip 

1

i=1 nip

1 --------  ec ( i ) nip

2

i=1 nip

1------cm ( i ) nip 

3

i=1

Material Model 57: Low Density Urethane Foam The urethane foam model is available to model highly compressible foams such as those used in seat cushions and as padding on the Side Impact Dummy (SID). The compressive behavior is illustrated in Figure 3-7 where hysteresis on unloading is shown. This behavior under uniaxial loading is assumed not to significantly couple in the transverse directions. In tension the material behaves in a linear fashion until tearing occurs. Although our implementation may be somewhat unusual, it was first motivated by Shkolnikov [1991] and a paper by Storakers [1986]. The recent additions necessary to model hysteretic

Materials 125 Materials

unloading and rate effects are due to Chang, et. al., [1994]. These latter additions have greatly expanded the usefulness of this model.

σ

Typical unloading curves determined by the hysteric unloading factor. With the shape factor equal to unity.

σ

Typical unloading for a large shape factor; e.g., 5.-8 and a small hysteric factor; e.g., .010.

Unloading Curves Strain

Strain

Figure 3-7

Behavior of the Low-density Urethane Foam Model

The model uses tabulated input data for the loading curve where the nominal stresses are defined as a function of the elongations, ε i , which are defined in terms of the principal stretches,

λ i , as:

εi = λ i – 1

(3-177)

The stretch ratios are found by solving for the eigenvalues of the left stretch tensor, obtained via a polar decomposition of the deformation gradient matrix,

V ij , which is

F ij :

F ij = R ik U kj = V ik R kj The update of

(3-178)

Vij follows the numerically stable approach of Taylor and Flanagan [1989]. After solving

for the principal stretches, the elongations are computed and, if the elongations are compressive, the corresponding values of the nominal stresses, τ i , are interpolated. If the elongations are tensile, the nominal stresses are given by

τ i = Eε i

(3-179)

The Cauchy stresses in the principal system become

τi σ i = ---------λiλk The stresses are then transformed back into the global system for the nodal force calculations.

(3-180)

126 Materials

When hysteretic unloading is used, the reloading will follow the unloading curve if the decay constant,

β , is set to zero. If β is nonzero the decay to the original loading curve is governed by the expression: 1 – e – βt

(3-181)

The bulk viscosity, which generates a rate dependent pressure, may cause an unexpected volumetric response and, consequently, it is optional with this model. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form

σ ij =



∂ε kl – τ ) --------∂τ

t g (t 0 ijkl

where g ijkl ( t – from the foam,

(3-182)

τ ) is the relaxation function. The stress tensor, , σ ijr augments the stresses determined

σ ijf ; consequently, the final stress, σ ij , is taken as the summation of the two

contributions:

σ ij = σ ijf + σ ijr

(3-183)

Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: N

g ( t ) = α0 +



α m e – βt

(3-184)

m=1

given by,

g ( t ) = E d e –β1 t

(3-185)

This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a Young's modulus,

E d , and decay constant, β 1 . The formulation is

performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate effects necessitates twelve additional history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches.

Material Type 58: Laminated Composite Fabric Parameters to control failure of an element layer are: ERODS, the maximum effective strain; i.e., maximum 1 = 100 % straining. The layer in the element is completely removed after the maximum

Materials 127 Materials

effective strain (compression/tension including shear) is reached. The stress limits are factors used to limit the stress in the softening part to a given value,

σ min = SLIMxx ⋅ strength ,

(3-186)

thus, the damage value is slightly modified such that elastoplastic like behavior is achieved with the threshold stress. As a factor for SLIMxx a number between 0.0 and 1.0 is possible. With a factor of 1.0, the stress remains at a maximum value identical to the strength, which is similar to ideal elastoplastic

SLIMTx is often reasonable; however, for compression SLIMCx = 1.0 is preferred. This is also valid for the corresponding shear value. If SLIMxx is

behavior. For tensile failure a small value for

smaller than 1.0, then localization can be observed depending on the total behavior of the lay-up. If the user is intentionally using SLIMxx < 1.0 , it is generally recommended to avoid a drop to zero and set the value to something in between 0.05 and 0.10. Then elastoplastic behavior is achieved in the limit which often leads to less numerical problems. Defaults for

SLIMxx = 1.0E-8 .

The crashfront-algorithm is started if and only if a value for TSIZE (time step size, with element elimination after the actual time step becomes smaller than TSIZE) is input The damage parameters can be written to the postprocessing database for each integration point as the first three additional element variables and can be visualized. Material models with FS=1 or FS=-1 are favorable for complete laminates and fabrics, as all directions are treated in a similar fashion. For material model FS=1, an interaction between normal stresses and shear stresses is assumed for the evolution of damage in the a- and b-directions. For the shear damage is always the maximum value of the damage from the criterion in a- or b- direction is taken. For material model FS=-1, it is assumed that the damage evolution is independent of any of the other stresses. A coupling is present only via the elastic material parameters and the complete structure. In tensile and compression directions and in a- as well as in b- direction, different failure surfaces can be assumed. The damage values, however, increase only when the loading direction changes. Special Control of Shear Behavior of Fabrics For fabric materials a nonlinear stress strain curve for the shear part of failure surface FS=-1 can be assumed as given below. This is not possible for other values of FS. The curve, shown in Figure 19.58.1, is defined by three points: a. a) the origin (0,0) is assumed, b. the limit of the first slightly nonlinear part (must be input), stress (TAU1) and strain (GAMMA1), see below. c. the shear strength at failure and shear strain at failure.

128 Materials

In addition, a stress limiter can be used to keep the stress constant via the SLIMS parameter. This value must be less than or equal to 1.0 and positive, which leads to an elastoplastic behavior for the shear part. The default is 1.0E-08, assuming almost brittle failure once the strength limit SC is reached. τ

SC TAU1 SLIMS*SC

GAMMA1

Figure 3-8

GMS

γ

Stress-strain Diagram for Shear

Material Type 62: Viscous Foam This model was written to represent the energy absorbing foam found on certain crash dummies, i.e., the ‘Confor Foam’ covering the ribs of the Eurosid dummy. The model consists of a nonlinear elastic stiffness in parallel with a viscous damper. A schematic is shown in Figure 3-9. The elastic stiffness is intended to limit total crush while the viscous damper absorbs energy. The stiffness

E 2 prevents timestep problems. E1

V2

Figure 3-9

E

2

Schematic of Material Model 62

Materials 129 Materials

Both

E 1 and V 2 are nonlinear with crush as follows:

E 1t = E 1 ( V –n 1 )

(3-187)

V 2t = V 2 ( abs ( 1 – V ) ) n

V is the relative volume defined by the ratio of the current to initial volume. Typical values are (units of N ,mm, s ) where

E 1 = 0.0036 n 1 = 4.0 V 2 = 0.0015 E 2 = 100.0 n 2 = 0.2 ν = 0.05

Material Type 63: Crushable Foam The intent of this model is model crushable foams in side impact and other applications where cyclic behavior is unimportant. This isotropic foam model crushes one-dimensionally with a Poisson’s ratio that is essentially zero. The stress versus strain behavior is depicted in Figure 3-10 where an example of unloading from point a to the tension cutoff stress at b then unloading to point c and finally reloading to point d is shown. At point the reloading will continue along the loading curve. It is important to use nonzero values for the tension cutoff to prevent the disintegration of the material under small tensile loads. For high values of tension cutoff the behavior of the material will be similar in tension and compression. In the implementation we assume that Young’s modulus is constant and update the stress assuming elastic behavior.

·n σ ijtrial = σ ijn + Eε ij + 1 ⁄ 2 Δt n + 1 ⁄ 2 The magnitudes of the principal values,

(3-188)

σ itrial , i = 1 ,3 , are then checked to see if the yield stress,

σ y , is exceeded and if so they are scaled back to the yield surface: if

σ itrial σ y < σ itrial then σ in + 1 = σ y --------------σ itrial

(3-189)

130 Materials

After the principal values are scaled, the stress tensor is transformed back into the global system. As seen in Figure 3-10, the yield stress is a function of the natural logarithm of the relative volume, volumetric strain.

σ ij

V ; i.e., the

a

E

d

c

b Volumetric Strain – ln V

Figure 3-10

Yield Stress Versus Volumetric Strain Curve for the Crushable Foam

Material Model 64: Strain Rate Sensitive Power-Law Plasticity This material model follows a constitutive relationship of the form:

· σ = kε m ε n

(3-190)

· σ is the yield stress, ε is the effective plastic strain, ε is the effective plastic strain rate, and the constants, k , m , and n can be expressed as functions of effective plastic strain or can be constant with where

respect to the plastic strain. The case of no strain hardening can be obtained by setting the exponent of the plastic strain equal to a very small positive value; i.e., 0.0001. This model can be combined with the superplastic forming input to control the magnitude of the pressure in the pressure boundary conditions in order to limit the effective plastic strain rate so that it does not exceed a maximum value at any integration point within the model. A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement is results can be dramatic.

Material Model 65: Modified Zerilli/Armstrong The Armstrong-Zerilli Material Model expresses the flow stress as follows.

Materials 131 Materials

For fcc metals, ·*

σ = C 1 + { C 2 ( ε p ) 1 ⁄ 2 [ e ( – C3 + C4 ln ( ε

) )τ

μ(T) ] + C 3 }  -----------------  μ ( 293 )

(3-191)

ε p = effective plastic strain · ε· · ε * = ---· effective plastic strain rate where ε 0 = 1 , 1e-3, le-6 for time units ε0 of seconds, milliseconds, and microseconds, respectively. For bcc metals, ·*

σ = C 1 + C 2 e ( – C3 + c4 lm ( ε

) )τ

μ( T) + [ C 5 ( ε p ) n + C 6 ]  ----------------- μ ( 293 )

(3-192)

where

μ( T) ---------------= B1 + B2 T + B3 T 2 μ ( 293 )

(3-193)

The relationship between heat capacity (specific heat) and temperature may be characterized by a cubic polynomial equation as follows:

Cp = G1 + G2 T + G3 T 2 + G4 T 3

(3-194)

A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement in results can be dramatic.

Material Model 67: Nonlinear Stiffness/Viscous 3-D Discrete Beam The formulation of the discrete beam (Type 6) assumes that the beam is of zero ngth and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (r, s, t) is given by the coordinate ID in the cross-sectional input where the global system is the default. The local coordinate system axes rotate with the average of the rotations of the two nodes that define the beam. For null load curve IDs, no forces are computed. The force resultants are found from load curves (see Figure 3-11) that are defined in terms of the force resultant versus the relative displacement in the local coordinate system for the discrete beam. The resultant forces and moments are determined by a table

132 Materials

lookup, if the origin of the load curve is at [0,0], as shown in Figure 3-11b, and the tension and compression responses are symmetric. R E S U L T A N T

R E S U L T A N T DISPLACEMENT

(a)

Figure 3-11

DISPLACEMENT (b)

Resultant Forces and Moments Determined by Table Lookup

Material Model 68: Nonlinear Plastic/Linear Viscous 3-D Discrete Beam The folmulation of the discrete beam (Type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system, which determines (r, s, t) is given by the coordinate ID in the cross-sectional input where the global system is the default. The local coordinate system axes rotate with the average of the rotations of the two nodes that define the beam. Each force resultant in the local system can have a limiting value defined as a function of plastic displacement by using a load curve (see Figure 3-12). For the degrees of freedom where elastic behavior is desired, the load curve ID is simply set to zero.

R E S U L T A N T

PLASTIC DISPLACEMENT

Figure 3-12

Resultant Forces and Moments Limited by the Yield Definition

Materials 133 Materials

Catastrophic failure, based on force resultants, occurs if the following inequality is satisfied:

 Fr  2  Fs  2  Ft  2  Mr  2  Ms  2  Mt  2 - +  ------------ +  ------------ – 1 ≥ 0  --------- +  --------- +  --------- +  ---------- F rfail  F sfail  F tfail  M rfail  M sfail  M tfail

(3-195)

Likewise, catastrohic failure based on displacement resultants occurs if:

 ur  2  u s  2  u t  2  θ r  2  θs  2  θ t  2 - +  ---------- +  ---------- +  ---------- +  ---------- +  ---------- – 1 ≥ 0  -------- u rfail  u sfail  u tfail  θ rfail  θ sfail  θ tfail

(3-196)

After failure, the discrete element is deleted. If failure is included, either one or both of the criteria may be used.

Material Model 69: Side Impact Dummy Damper (SID Damper) The side impact dummy uses a damper that is not adequately treated by nonlinear force versus relative velocity curves, since the force characteristics are also dependent on the displacement of the piston. As the damper moves, the fluid flows through the open orifices to provide the necessary damping resistance. While moving as shown in Figure 3-13, the piston gradually blocks off and effectively closes the orifices. The number of orifices and the size of their openings control the damper resistance and performance. The damping force is computed from the equation.

 C F = SF  KA p V p  -----t-l + C 2 V p ρ fluid   A0 where

 Ap  2   ---------t- – 1  – f ( s + s 0 ) + V p g ( s + s 0 ) } (3-197)  CA0  

K is a user defined constant or a tabulated function of the absolute value of the relative velocity,

V p is the piston's relative velocity, C is the discharge coefficient, A p is the piston area, A 0t is the total

134 Materials

open areas of orifices at time t ,

ρ fluid is the fluid density, C 1 is the coefficient for the linear term, and

C 2 is the coefficient for the quadratic term.

Figure 3-13

Mathematical Model for Side Impact Dummy Damper

In the implementation, the orifices are assumed to be circular with partial covering by the orifice controller. As the piston closes, the closure of the orifice is gradual. This gradual closure is taken into account to insure a smooth response. If the piston stroke is exceeded, the stiffness value, k , limits further movement; i.e., if the damper bottoms out in tension or compression, the damper forces are calculated by replacing the damper by a bottoming out spring and damper, k and c , respectively. The piston stroke must exceed the initial length of the beam element. The time step calculation is based in part on the stiffness value of the bottoming out spring. A typical force versus displacement curve at constant relative

Materials 135 Materials

velocity with only the linear velocity term active is shown in Figure 3-14. The factor, the force defaults to 1.0 and is analogous to the adjusting ring on the damper.

SF , which scales

Linear loading after ofifices close

F O R C E

Last orfice closes

Force increases as orfice is gradually covered Displacement

Figure 3-14

Force Versus Displacement

Material Model 70: Hydraulic/Gas Damper This special purpose element represents a combined hydraulic and gas-filled damper which has a variable orifice coefficient. A schematic of the damper is shown in Figure 3-15. Dampers of this type are sometimes used on buffers at the end of railroad tracks and as aircraft undercarriage shock absorbers. This material can be used only as a discrete beam element. As the damper is compressed two actions contribute to the force that develops. First, the gas is adiabatically compressed into a smaller volume. Secondly, oil is forced through an orifice. A profiled pin may occupy some of the cross-sectional area of the orifice; thus, the orifice area available for the oil varies with the stroke. The force is assumed proportional to the square of the velocity and inversely proportional to the available area. The equation for this element is:

C0 n   V 2 F = SCLF ⋅  K h  ----- + P 0  --------------- – P a ⋅ A p  a0 C0 – S  

(3-198)

136 Materials

where

S is the element deflection and V is the relative velocity across the element.

Figure 3-15

Schematic of Hydraulic/Gas Damper

Material Model 71: Cable This material can be used only as a discrete beam element. The force, nonzero only if the cable is in tension. The force is given by:

F , generated by the cable is

F = K ⋅ max ( ΔL, 0. ) where

(3-199)

ΔL is the change in length

ΔL = current length – ( initial length – offset )

(3-200)

and the stiffness is defined as:

E ⋅ area K = ------------------------------------------------------------( initial length – offset )

(3-201)

The area and offset are defined on either the cross section or element cards in the SOL 700 input. For a slack cable the offset should be input as a negative length. For an initial tensile force the offset should be positive. If a load curve is specified, the Young’s modulus will be ignored and the load curve will be used instead. The points on the load curve are defined as engineering stress versus engineering strain; i.e., the change in length over the initial length. The unloading behavior follows the loading.

Material Model 73: Low Density Viscoelastic Foam This viscoelastic foam model is available to model highly compressible viscous foams. The hyperelastic formulation of this model follows that of material 57. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form

Materials 137 Materials

σ ijr = where

∂ε kl

- dτ 0 gijkl ( t – τ ) -------∂τ t

(3-202)

g ijkl ( t – τ ) is the relaxation function. The stress tensor, σ ijr , augments the stresses

determined from the foam,

σ ijf ; consequently, the final stress, σ ij , is taken as the summation of the

two contributions:

σ ij = σ ijf + σ ijr

(3-203)

Since we wish to include only simple rate effects, the relaxation function is represented by up to six terms of the Prony series: N

g ( t ) = α0 +



α m e –βt

(3-204)

m=1

This model is effectively a Maxwell fluid which consists of a dampers and springs in series. The formulation is performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate effects necessitates 42 additional history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches and the evaluation of the viscous stress components

Material Model 74: Elastic Spring for the Discrete Beam This model permits elastic springs with damping to be combined and represented with a discrete beam element type 6. Linear stiffness and damping coefficients can be defined and, for nonlinear behavior, a force versus deflection and force versus rate curves can be used. Displacement based failure and an initial force are optional If the linear spring stiffness is used, the force,

F , is given by:

F = F 0 + FΔL + DΔL where

 

K is the stiffness constant, and D is the viscous damping coefficient.

If the load curve ID for given by:

f ( ΔL ) . is specified, nonlinear behavior is activated. For this case the force is

138 Materials

  ΔL· -  · · ----------F = F 0 + Kf ( ΔL ) 1 + C1 ⋅ ΔL + C2 ⋅ sgn ( ΔL ) ln  max  1. ,    DLE  +DΔL· + g ( ΔL )h ( ΔL· )

(3-206)

C1 and C2 are damping coefficients for nonlinear behavior, DLE is a factor to scale time units, and g ( ΔL ) . is an optional load curve defining a scale factor versus deflection for load curve ID, h ( ΔL ⁄ dt ) . where

In these equations,

ΔL is the change in length

ΔL = currentlength – initiallength . Failure can occur in either compression or tension based on displacement values of CDF and TDF, respectively. After failure no forces are carried. Compressive failure does not apply if the spring is initially zero length. The cross sectional area is defined on the beam property card for the discrete beam elements. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment.

Material Model 76: General Viscoelastic Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form:

σ ij = where



t g (t 0 ijkl

∂ε – τ ) --------kl- dτ ∂τ

(3-207)

g ijkl ( t – τ ) is the relaxation function.

If we wish to include only simple rate effects for the deviatoric stresses, the relaxation function is represented by six terms from the Prony series: N

g(t) =

 m=1

G m e –βm t

(3-208)

Materials 139 Materials

We characterize this in the input by shear modulii,

G i , and decay constants, β i . An arbitrary number of

terms, up to 6, may be used when applying the viscoelastic model.

Figure 3-16

Note:

Relaxation Curve

This curve defines stress versus time where time is defined on a logarithmic scale. For best results, the points defined in the load curve should be equally spaced on the logarithmic scale. Furthermore, the load curve should be smooth and defined in the positive quadrant. If nonphysical values are determined by least squares fit, SOL 700 will terminate with an error message after the initialization phase is completed. If the ramp time for loading is included, then the relaxation which occurs during the loading phase is taken into account. This effect may or may not be important.

For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk modulii: N

k( t) =



Km e

–βk t m

(3-209)

m=1

Material Model 77: Hyperviscoelastic Rubber Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term,

140 Materials

W H ( J ) , is included in the strain energy functional which is function of the relative volume, ( J ) , [Ogden, 1984]: n

W ( J 1 ,J 2 ,J ) =



J 1 = I 1 I 3– 1 ⁄ 2 J 2 = I 2 I 3– 1 ⁄ 2

p ,q = 0

C pq ( J 1 – 3 ) p ( J 2 – 3 ) q + W H ( J )

(3-210)

In order to prevent volumetric work from contributing to the hydrostatic work the first and second invariants are modified as shown. This procedure is described in more detail by Sussman and Bathe [1987]. For the Ogden model the energy equation is given as: 3

n

μj

-(λ   ---αj i

W∗ =

*α 1

1 – 1 ) + --- K ( J – 1 ) 2 2

(3-211)

i = 1j = 1

where the asterisk

( * ) indicates that the volumetric effects have be eliminated from the principal

λ j* . See Ogden [1984] for more details.

stretches,

Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form:

σ ij =

∂ε kl --------- dτ g ( t – τ ) ijkl 0 ∂τ t

or in terms of the second Piola-Kirchhoff stress,

(3-212)

S ij , and Green's strain tensor, E ij ,

∂Ekl t S ij  G ijkl ( t – τ ) ---------- dτ 0 ∂τ where g ijkl ( t

(3-213)

– τ ) and G ijkl ( t – τ ) are the relaxation functions for the different stress measures. This

stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: N

g ( t ) = α0 +

 m=1

given by,

α m e – βt

(3-214)

Materials 141 Materials

n

g(t) =

 Gi e

–βi t

(3-215)

j=1

This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli,

G i , and decay constants, β i . The viscoelastic behavior is

optional and an arbitrary number of terms may be used. The Mooney-Rivlin rubber model is obtained by specifying n + 2 . In spite of the differences in formulations with Model 27, we find that the results obtained with this model are nearly identical with those of Model 27 as long as large values of Poisson’s ratio are used. When viscoelastic terms are not included, this model is similar to the use of the Ogden model in solution 600, defined on the MATHE option.

Material Model 79: Hysteretic Soil This model is a nested surface model with five superposed “layers” of elasto-perfectly plastic material, each with its own elastic modulii and yield values. Nested surface models give hysteretic behavior, as the different “layers” yield at different stresses. The constants ( a 0 , a 1 , a 2 ) govern the pressure sensitivity of the yield stress. Only the ratios between these values are important - the absolute stress values are taken from the stressstrain curve. The stress strain pairs ( ( γ1 ,τ1 ) , … ( γ5 ,τ5 ) ) define a shear stress versus shear strain curve. The first point on the curve is assumed by default to be (0,0) and does not need to be entered. The slope of the

γ . Not all five points need be to be defined. This curve applies at the reference pressure; at other pressures, the curve variesaccording to a 0 , a 1 , and a 2 as in the soil curve must decrease with increasing

and crushable foam model, Material 5. The elastic moduli G and K are pressure sensitive.

G = G0 ( p – p 0 ) b K = K0 ( p – p0 ) b where

G 0 and K 0 are the input values, p is the current pressure, p o the cut-off or referencepressure

(must be zero or negative). If

p attempts to fall below p o (i.e., more tensile) the shear stresses are set to

zero and the pressure is set to p o . Thus, the material has no stiffness orstrength in tension. The pressure in compression is calculated as follows:

142 Materials

p = [ –K0 where

1 -----------1 – ln ( V ) ] b

V is the relative volume; i.e., the ratio between the original and current volume.

Material Model 80: Ramberg-Osgood Plasticity The Ramberg-Osgood equation is an empirical constitutive relation to represent the one-dimensional elastic-plastic behavior of many materials, including soils. This model allows a simple rate independent representation of the hysteretic energy dissipation observed in soils subjected to cyclic shear deformation. For monotonic loading, the stress-strain relationship is given by:

γ τ τ r if γ ≥ 0 ---- = ---- + α ---γy τy τy τ τ r if γ < 0 ---γ- = ---– α ---τy γy τ y

(3-216)

γ is the shear strain and τ is the shear stress. The model approaches perfect plasticity as the stress exponent r → ∞ . These equations must be augmented to correctly model unloading and reloading · material behavior. The first load reversal is detected by γγ < 0 . After the first reversal, the stress-strain where

relationship is modified to

( γ – γ0 ) ( τ – τ0 ) ( τ – τ 0 ) rif γ ≥ 0 ------------------ = ----------------- + α ----------------2γ y 2τ y 2τ y ( γ – γ0 ) ( τ – τ0 ) ( τ – τ 0 ) rif γ < 0 ------------------ = ----------------- – α ----------------2γ y 2τ y 2τ y

(3-217)

where γ 0 and τ 0 represent the values of strain and stress at the point of load reversal. Subsequent load reversals are detected by

(γ − γ 0 ) γ < 0 .

The Ramberg-Osgood equations are inherently one-dimensional and are assumed to apply to shear components. To generalize this theory to the multidimensional case, it is assumed that each component of the deviatoric stress and deviatoric tensorial strain is independently related by the one-dimensional stress-strain equations. A projection is used to map the result back into deviatoric stress space if required. The volumetric behavior is elastic, and, therefore, the pressure

p = K εv where ε v is the volumetric strain.

p is found by (3-218)

Materials 143 Materials

Material Model 81 and 82: Plasticity with Damage and Orthotropic Option With this model an elasto-viscoplastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. Damage is considered before rupture occurs. Also, failure based on a plastic strain or a minimum time step size can be defined. An option in the keyword input, ORTHO, is available, which invokes an orthotropic damage model. This option, which is implemented only for shell elements with multiple integration points through thickness, is an extension to include orthotropic damage as a means of treating failure in aluminum panels. Directional damage begins after a defined failure strain is reached in tension and continues to evolve until a tensile rupture strain is reached in either one of the two orthogonal directions. The stress versus strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure 3-17 is expected to be defined by (EPS1,ES1) - (EPS8,ES8); however, an effective stress versus effective plastic strain curve (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most general approach is to use the table definition (LCSS) discussed below. Two options to account for strain rate effects are possible. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor,

· ε 1⁄p 1 +  ---- C where

(3-219)

· · ε is the strain rate, ε =

· ε ij ε ij . If the viscoplastic option is active, VP=1.0, and if SIGY is > 0

p ) , which is typically then the dynamic yield stress is computed from the sum of the static stress, σ ys ( ε eff

given by a load curve ID, and the initial yield stress, SIGY, multiplied by the Cowper-Symonds rate term as follows: p ·p σ y ( ε eff ,ε eff )

=

p σ ys ( ε eff )

·p ε eff  1 ⁄ p  ------+ SIGY ⋅  - C

(3-220)

where the plastic strain rate is used. If SIGY=0, the following equation is used instead where the static stress,

p σ ys ( ε eff ) , must be defined by a load curve:

p ·p σ y ( ε eff ,ε eff )

=

σ ys

·p ε eff  1 ⁄ p  1 + ------- C

(3-221)

This latter equation is always used if the viscoplastic option is off. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined.

144 Materials

The constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, ω , which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by:

P σ nominal = --A where

(3-222)

P is the applied load and A is the surface area. The true stress is given by:

P σ true = --------------------A – A loss where

(3-223)

A loss is the void area. The damage variable can then be defined:

A loss ω = ----------A

0≤ω≤1 (3-224)

In this model damage is defined in terms of plastic strain after the failure strain is exceeded: p p ε eff – ε failure p p ≤ εp - if ε failure ω = ---------------------------------------≤ ε eff rupture p p – ε failure ε rapture

(3-225)

After exceeding the failure strain softening begins and continues until the rupture strain is reached. By default, deletion of the element occurs when all integration points in the shell have failed.

Materials 145 Materials

Note in Figure 3-18 that the origin of the curve is at (0,0). It is permissible to input the failure strain, fs , as zero for this option. The nonlinear damage curve is useful for controlling the softening behavior after the failure strain is reached. Yield stress versus effective plastic strain for undamaged material

σ yield Nominal stress after failure

Damage increases linearly with plastic strain after failure

0

ω = 1

Failure Begins

ω = 0

Figure 3-17

Rupture

Stress Strain Behavior When Damage is Included.

Damage

1

p

ε eff – fs Figure 3-18

p

ε eff

Failure

A Nonlinear Damage Curve (Optional)

146 Materials

Material Model 83: Fu-Chang’s Foam With Rate Effects This model allows rate effects to be modeled in low and medium density foams, see Figure 3-19. Hysteretic unloading behavior in this model is a function of the rate sensitivity with the most rate sensitive foams providing the largest hysteresis and visa versa. The unified constitutive equations for foam materials by Fu-Chang [1995] provide the basis for this model. This implementation incorporates the coding in the reference in modified form to ensure reasonable computational efficiency. The mathematical description given below is excerpted from the reference. The strain is divided into two parts: a linear part and a non-linear part of the strain

E( t ) = EL( t) + EN( t )

(3-226)

and the strain rate become

E· ( t ) = E· L ( t ) + E· N ( t )

(3-227)

E· N is an expression for the past history of E N . A postulated constitutive equation may be written as: ∞



σ( t) =

[ E tN ( τ ) ,S ( t ) ] dτ

(3-228)

τ=0 ∞

where



S ( t ) is the state variable and

is a functional of all values of

τ in T τ : 0 ≤ τ ≤ ∞ and

τ=0

E tN ( τ ) = E N ( t – τ )

(3-229)

where τ is the history parameter:

E tN ( τ = ∞ ) ⇔ the virgin material

(3-230)

It is assumed that the material remembers only its immediate past, i.e., a neighborhood about Therefore, an expansion of E tN ( τ ) in a Taylor series about

E tN ( τ )

=

EN( 0 )

∂ E tN --------- ( 0 ) dt + ∂t

τ = 0.

τ = 0 yields: (3-231)

Hence, the postulated constitutive equation becomes:

σ ( t ) = σ∗ ( E N ( t ), E· N ( t ), S ( t ) )

(3-232)

Materials 147 Materials

∂ E tN · where we have replaced ---------- by E N , and σ∗ is a function of its arguments. ∂t For a special case,

σ ( t ) = σ∗ ( E· N ( t ), S ( t ) )

(3-233)

we may write

E· tN = f ( S ( t ), s ( t ) )

(3-234)

which states that the nonlinear strain rate is the function of stress and a state variable which represents the history of loading. Therefore, the proposed kinetic equation for foam materials is:

σ tr ( σ S ) 2n0 E· N = -------- D 0 exp –c 0  -------------- ( σ 2) σ where

(3-235)

D 0, c 0 and n0 are material constants, and S is the overall state variable. If either D 0 = 0 or

c 0 → ∞ then the nonlinear strain rate vanishes. S· ij = [ c 1 ( a ij R – c 2 S ij ) P + c 3 W n1 ( W· N ) n2 I ij ] R

(3-236)

E· N -  n3  ---------R = 1 + c4 – 1 c5

(3-237)

P =

 tr ( σ E

· N)

(3-238)

W =

 tr ( σ dE )

(3-239)

where c 1, c 2, c 3, c 4, c 5, n 1, n 2, n 3, and a ij are material constants and:

σ = ( σ ij σ ij ) 1 / 2 E· = ( E· ij E· ij ) 1 / 2 · N N E N = ( E· ij E· ij ) 1 / 2

(3-240)

148 Materials

In the implementation by Fu Chang the model was simplified such that the input constants state variables

a ij and the

S ij are scalars.

Figure 3-19

Rate Effects in Fu Chang's Foam Model

Material Model 87: Cellular Rubber This material model provides a cellular rubber model combined with linear viscoelasticity as outlined by Christensen [1980]. Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term,

W H ( J ) , is included in the strain energy functional which is function of the relative volume, J , [Ogden, 1984] n

W ( J 1 ,J 2 ,J ) = –1 ⁄ 3

J1 = I1 I3



C pq ( J 1 – 3 ) p ( J 2 – 3 ) q + W H

p, q = 0

(3-241)

–2 ⁄ 3

J2 = I2 I3

In order to prevent volumetric work from contributing to the hydrostatic work the first and second invariants are modified as shown. This procedure is described in more detail by Sussman and Bathe [1987].

Materials 149 Materials

The effects of confined air pressure in its overall response characteristics are included by augmenting the stress state within the element by the air pressure.

σ ij = σ ijsk – δ ij σ air where

(3-242)

σ ijsk is the bulk skeletal stress and σ air is the air pressure computed from the equation:

p0 γ σ air = – -------------------1+γ–φ where

(3-243)

p 0 is the initial foam pressure usually taken as the atmospheric pressure and γ defines the

volumetric strain

γ = V – 1 + γ0

(3-244)

where V is the relative volume of the voids and γ 0 is the initial volumetric strain which is typically zero. The rubber skeletal material is assumed to be incompressible. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form:

σ ij =

∂ε kl

t

- dt 0 gijkl ( t – τ ) -------∂τ

or in terms of the second Piola-Kirchhoff stress,

(3-245)

S ij , and Green's strain tensor, , Eij

∂ E kl ---------- dt G ( t – τ ) ijkl 0 ∂τ t

S ij =

where g ijkl ( t

(3-246)

– τ ) and G ijkl ( t – τ ) are the relaxation functions for the different stress measures. This

stress is added to the stress tensor determined from the strain energy functional. Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: N

g ( t ) = a0 +



αm + e – βt

(3-247)

m=1

given by

g ( t ) = E d e –β1 t .

(3-248)

150 Materials

This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a shear modulus,

G , and decay constant, β 1 .

The Mooney-Rivlin rubber model is obtained by specifying n = 1 . In spite of the differences in formulations with Model 27, we find that the results obtained with this model are nearly identical with those of 27 as long as large values of Poisson’s ratio are used. By setting the initial air pressure to zero, an open cell, cellular rubber can be simulated as shown in Figure 3-20.

Figure 3-20

Cellular Rubber with Entrapped Air

Material Model 89: Plasticity Polymer Unlike other MD Nastran SOL 700 material models, both the input stress-strain curve and the strain to failure are defined as total true strain, not plastic strain. The input can be defined from uniaxial tensile tests; nominal stress and nominal strain from the tests must be converted to true stress and true strain. The elastic component of strain must not be subtracted out. The stress-strain curve is permitted to have sections steeper (i.e. stiffer) than the elastic modulus. When these are encountered the elastic modulus is increased to prevent spurious energy generation.

Material Model 94: Inelastic Spring Discrete Beam The yield force is taken from the load curve:

F Y = F y ( Δ L plastic ) where

L plastic is the plastic deflection. A trial force is computed as:

(3-249)

Materials 151 Materials

F T = F n + K ⋅ Δ L· ⋅ Δ t and is checked against the yield force to determine

 Y F =  F  FT

(3-250)

F:

if F T > F Y if F T ≤ F Y

(3-251)

The final force, which includes rate effects and damping, is given by:

Fn + 1 where

  Δ L· -  · · · ----------= F ⋅ 1 + C 1 ⋅ Δ L + C 2 ⋅ sgn ( Δ L ) ln  max  1. , h ( Δ L· )  + D Δ L + g ( Δ L )(3-252)    DLE  C 1 , C 2 are damping coefficients, DLE is a factor to scale time units.

Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate, of the curve is used whenever the force is positive. In these equations,

F y . The positive part

Δ L is the change in length

Δ L = current length – initial length

Material Model 97: General Joint Discrete Beam For explicit calculations, the additional stiffness due to this joint may require additional mass and inertia for stability. Mass and rotary inertia for this beam element is based on the defined mass density, the volume, and the mass moment of inertia defined in the beam property input. The penalty stiffness applies to explicit calculations. For implicit calculations, constraint equations are generated and imposed on the system equations; therefore, these constants, RPST and RPSR, are not used.

Material Model 98: Simplified Johnson Cook Johnson and Cook express the flow stress as n · σ y = ( A + B ε p ) ( 1 + c ln ε * )

where

A, B, C and n are input constants

152 Materials

εp · ε · ε * = ---·ε0

ellective plastic strain

·

effective strain rate for ε 0

= 1 s –1

The maximum stress is limited by sigmax and sigsat by: n · σ y = min { min [ A + B ε p ,sigmax ] ( 1 + c ln ε * ) ,sigsat }

Failure occurs when the effective plastic strain exceeds psfail. If the viscoplastic option is active, VP=1.0, the SIGMAX and SIGSAT parameters are ignored since these parameters make convergence of the viscoplastic strain iteration loopdifficult to achieve. The viscoplastic option replaces the plastic strain in the forgoing equationsby the viscoplastic strain and the strain rate by the viscoplastic strain rate. Numerical noise issubstantially reduced by the viscoplastic formulation.

Material Model 100: Spot Weld This material model applies to beam element type 9 for spot welds. These beam elements may be placed between any two deformable shell surfaces, see Figure 3-21, and tied with type 7 constraint contact which eliminates the need to have adjacent nodes at spot weld locations. Beam spot welds may be placed between rigid bodies and rigid/deformable bodies by making the node on one end of the spot weld a rigid body node which can be an extra node for the rigid body. In the same way, rigid bodies may also be tied together with this spot weld option.

Figure 3-21

Deformable Spotwelds

It is advisable to include all spot welds which can be arbitrarily placed within the structure, which provide the slave nodes, and spot welded materials, which define the master segments, within a single type 7 tied interface. As a constraint method, multiple type 7 interfaces are treated independently which can lead to significant problems if such interfaces share common nodal points. The offset option, “o 7”, should not be used with spot welds.

Materials 153 Materials

The weld material is modeled with isotropic hardening plasticity coupled to two failure models. The first model specifies a failure strain which fails each integration point in the spot weld independently. The second model fails the entire weld if the resultants are outside of the failure surface defined by:

N rr  2  N rs  2  N rt  2  M rr  2  M ss  2 T rr  2  --------- + ---------- + --------- + ----------- + ----------- – 1  -------- = 0  N rr   N rs   N rt   M rr   M ss   T rr  F F F F F F

(3-253)

where the numerators in the equation are the resultants calculated in the local coordinates of the cross section, and the denominators are the values specified in the input. If the user defined parameter, NF, which the number of force vectors stored for filtering, is nonzero the resultants are filtered before failure is checked. The default value is set to zero which is generally recommended unless oscillatory resultant forces are observed in the time history databases. Even though these welds should not oscillate significantly, this option was added for consistency with the other spot weld options. NF affects the storage since it is necessary to store the resultant forces as history variables. If the failure strain is set to zero, the failure strain model is not used. In a similar manner, when the value of a resultant at failure is set to zero, the corresponding term in the failure surface is ignored. For example, if only

N rrF is nonzero, the failure surface is reduced to N rr = N rrF . None, either, or both of the

failure models may be active depending on the specified input values. The inertias of the spot welds are scaled during the first time step so that their stable time step size is Δt. A strong compressive load on the spot weld at a later time may reduce the length of the spot weld so that stable time step size drops below Δ t . If the value of Δ t is zero, mass scaling is not performed, and the spot welds will probably limit the time step size. Under most circumstances, the inertias of the spot welds are small enough that scaling them will have a negligible effect on the structural response and the use of this option is encouraged. Spotweld force history data is written into the SWFORC ASCII file. In this database the resultant moments are not available, but they are in the binary time history database. The constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, ω , which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by

P σ nominal = --A where

(3-254)

P is the applied load and A is the surface area. The true stress is given by:

P σ true = --------------------A – A loss

(3-255)

154 Materials

where

A loss is the void area. The damage variable can then be defined:

A loss ω = ----------A

0≤ω≤1 (3-256)

In this model damage is defined in terms of plastic strain after the failure strain is exceeded: p

p

ε eff – ε failure - if ε pfailure ≤ ε peff ≤ ε prupture ω = --------------------------------------p p ε rupture – ε failure

(3-257)

After exceeding the failure strain softening begins and continues until the rupture strain is reached.

Material Model 119: General Nonlinear Six Degrees of Freedom Discrete Beam Catastrophic failure, which is based on displacement resultants, occurs if either of the following inequalities are satisfied:

 ur  2  us  2  ut  2  θt  2  θ s  2  θt  2  ---------- +  ---------- +  ---------- +  ---------- +  ---------- +  ---------- – 1. ≥ 0  u rtfail  u stfail  u ttfail  θ rtfail  θ stfail  θ ttfail  u r  2  u s  2  ut  2  θt  2  θs  2  θt  2 - +  ------------ +  ------------ +  ------------ +  ------------ +  ------------ – 1. ≥ 0  ---------- u rcfail  u scfail  u tcfail  θrcfail  θ scfail  θ tcfail

(3-258)

Materials 155 Materials

After failure the discrete element is deleted. If failure is included either the tension failure or the compression failure or both may be used. R E S U L T A N T

R E S U L T A N T

Unloading Curve

Loading-unloading Curve DISPLACEMENT

DISPLACEMENT

Unload = 0

Unloading Curve

R E S U L T A N T

Unload = 1

R E S U L T A N T

Unloading Curve

DISPLACEMENT

DISPLACEMENT

Umin

Unload = 2

Figure 3-22

OFFSET x Umin

Unload = 3

Load and Unloading Behavior

Material Model 126: Modified Honeycomb For efficiency it is strongly recommended that the load curve ID’s: LCA, LCB, LCC, LCS, LCAB, LCBC, and LCCA, contain exactly the same number of points with corresponding strain values on the abscissa. If this recommendation is followed the cost of the table lookup is insignificant. Conversely, the cost increases significantly if the abscissa strain values are not consistent between load curves. The behavior before compaction is orthotropic where the components of the stress tensor are uncoupled; i.e., a component of strain will generate resistance in the local α-direction with no coupling to the local b and c directions. The elastic modulii vary from their initial values to the fully coaaumpacted values linearly with the relative volume:

E aa = E aau + βaa ( E – E aau ) G ab = G abu + β ( G – G abu ) E bb = E bbu + βbb ( E – E bbu ) G bc = G bcu + β ( G – G bcu ) E cc = E ccu + βcc ( E – E ccu ) G ca = G cau + β ( G – G cau )

(3-259)

156 Materials

where

1–v B = max min   ------------- ,1 , 0 1 – vf and

(3-260)

G is the elastic shear modulus for the fully compacted honeycomb material

E G = --------------------2(1 + υ) The relative volume, typically,

(3-261)

ν , is defined as the ratio of the current volume over the initial volume, and

V = 1 at the beginning of a calculation.

The load curves define the magnitude of the stress as the material undergoes deformation. The first value in the curve should be less than or equal to zero corresponding to tension and increase to full compaction. Care should be taken when defining the curves so the extrapolated values do not lead to negative yield stresses. At the beginning of the stress update we transform each element’s stresses and strain rates into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated modulii according to: n + 1 trial = σ n + E Δε σ aa aa aa aa

n+1 σ ab

trial

n + 2 G Δε = σ ab ab ab

n+1 σ bb

trial

n + E Δε = σ bb bb bb

n+1 σ bc

trial

n + 2 G Δε = σ bc bc bc

n+1 σ cc

trial

n + E Δε = σ cc cc cc

n + 1 trial = σ n + 2 G Δε σ ca ca ca ca

(3-262)

We then independently check each component of the updated stresses to ensure that they do not exceed the permissible values determined from the load curves, e.g., if

σ ijn + 1

trial

> λσ ij ( ε ij )

(3-263)

then

λσ ijn + 1 = σ ij ( ε ij ) ---------------------trial σ in + 1 trial

σ ijn + 1

The components of σ ij ( ε ij ) are defined by load curves. The parameter

(3-264)

λ is either unity or a value taken

from the load curve number, LCSR, that defines λ as a function of strain-rate. Strain-rate is defined here as the Euclidean norm of the deviatoric strain-rate tensor. For fully compacted material we assume that the material behavior is elastic-perfectly plastic and updated the stress components according to:

Materials 157 Materials

s ijtrial = s ijn + 2 G Δε ijdev

n+1⁄2

(3-265)

where the deviatoric strain increment is defined as

1 Δε ijdev = Δε ij – --- Δε kk δ ij 3

(3-266)

We now check to see if the yield stress for the fully compacted material is exceeded by comparing

3 trial s eff =  --- s ijtrial s ijtrial 2

1⁄2

the effective trial stress to the yield stress,

(3-267)

σ y . If the effective trial stress exceeds the yield stress, we

simply scale back the stress components to the yield surface

σ y trial -s s ijn + 1 = ---------trial ij s eff We can now update the pressure using the elastic bulk modulus,

(3-268)

K

n+1⁄2 p n + 1 = p n – K Δε kk E K = -----------------------3 ( 1 – 2υ )

(3-269)

and obtain the final value for the Cauchy stress

σ ijn + 1 = s ijn + 1 – p n + 1 δ ij After completing the stress update we transform the stresses back to the global configuration.

(3-270)

158 Materials

In Figure 3-23, note that the "yield stress" at a strain of zero is nonzero. In the load curve definition, the "time" value is the directional strain and the "function" value is the yield stress.

Curve extends into negative strain quadrant since SOL 700 will extrapolate using the two end points. It is important that the extrapolation does not extend into the negative stress region.

Figure 3-23

Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent.

Stress Quantity Versus Strain

Material Model 127: Arruda-Boyce Hyperviscoelastic Rubber This material model, described in the paper by Arruda and Boyce [1993], provides a rubber model that is optionally combined with linear viscoelasticity. Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude; therefore, to model the rubber as an unconstrained material, a hydrostatic work term, W H ( J ) , is included in the strain energy functional which is function of the relative volume,

J:

1 1 11 W ( J 1, J 2, J ) = nk θ --- ( J 1 – 3 ) + ---------- ( J 12 – 9 ) + ------------------2 ( J 13 – 2 20 N 1050 N 3 19 519 + nk θ  ---------------- ( J 14 – 81 ) + ------------------------4 ( J 15 – 243 ) + W H ( J )  7000 N 673750 N J 1 = I 1 J –1 ⁄ 3 J2 = I2 J The hydrostatic work term is expressed in terms of the bulk modulus,

K W H ( J ) = ---- ( H – 1 ) 2 2

(3-271)

K , and J , as: (3-272)

Materials 159 Materials

Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form:

σ ij =

∂ε kl

t

- dτ 0 gijkl ( t – τ ) -------∂τ

(3-273)

or in terms of the second Piola-Kirchhoff stress,

∂ E kl

t

S ij =

S ij , and Green's strain tensor, Eij ,

- dτ 0 Gijkl ( t – τ ) --------∂τ

where g ijkl ( t

(3-274)

– τ ) and G ijkl ( t – τ ) are the relaxation functions for the different stress measures. This

stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: N

g ( t ) = α0 +



α m e –βt

(3-275)

m=1

given by, N

 Gi e

g(t) =

–βi t

(3-276)

i=1

This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli,

G i , and decay constants, βi . The viscoelastic behavior is

optional and an arbitrary number of terms may be used. When viscoelastic terms are not included, this model is similar to the use of the Arruda Boyce model in solution 600, defined in the MATHE option. When viscoelasticity is included, the formulation of these two models are different.

Material Model 158: Rate Sensitive Composite Fabric See material type 58, Laminated Composite Fabric, for the treatment of the composite material. Rate effects are taken into account through a Maxwell model using linear viscoelasticity by a convolution integral of the form:

σ ij =

∂ε kl

- dτ 0 gijkl ( t – τ ) -------∂τ t

(3-277)

160 Materials

where g ijkl t – τ is the relaxation function for different stress measures. This stress is added to the stress tensor determined from the strain energy functional. Since we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: N

g(t) =



G m e –βm t

m=1

We characterize this in the input by the shear moduli,

G i , and the decay constants, β i . An arbitrary

number of terms, not exceeding 6, may be used when applying the viscoelastic model. The composite failure is not directly affected by the presence of the viscous stress tensor.

Material Model 181: Simplified Rubber Foam Material type 181 in SOL 700is a simplified “quasi”-hyperelastic rubber model defined by a single uniaxial load curve or by a family of curves at discrete strain rates. The term “quasi” is used because there is really no strain energy function for determining the stresses used in this model. However, for deriving the tangent stiffness matrix we use the formulas as if a strain energy function were present. In addition, a frequency independent damping stress is added to model the energy dissipation commonly observed in rubbers. Hyperelasticity Using the Principal Stretch Ratios A hyperelastic constitutive law is determined by a strain energy function that here is expressed in terms of the principal stretches; i.e., ) , constitutive tensor of interest,

W = W ( λ 1 ,λ 2 ,λ 3 ) . To obtain the Cauchy stress σ ij , as well as the

TC , they are first calculated in the principal basis after which they are C ijkl

transformed back to the “base frame”, or standard basis. The complete set of formulas is given by Crisfield [1997] and is for the sake of completeness recapitulated here. The principal Kirchhoff stress components are given by

∂W τ ijE = λi -------- ( no sum ) ∂λ i

(3-278)

that are transformed to the standard basis using the standard formula E τ ij = q ik q jl τ kl

The

(3-279)

q ij are the components of the orthogonal tensor containing the eigenvectors of the principal basis.

The Cauchy stress is then given by

σ ij = J –1 τ ij

(3-280)

Materials 161 Materials

where

J = λ1 λ2 λ3 is the relative volume change.

The constitutive tensor that relates the rate of deformation to the Truesdell (convected) rate of Kirchhoff stress can in the principal basis be expressed as

∂ iiE TKE C iijj = λj -------- – 2τ iiE δ ij ∂λj 2 E λj τ ii – λ i2 τ jjE TKE C ijij = ----------------------------λ 12 – λ j2 λi  ∂τ iiE ∂τ iiE TKE C ijij = ---- --------- – --------2  ∂λ i ∂λ j 

i ≠ j ,( λ i ≠ λj )

(no sum)

i ≠ j ,λ i = λ j (3-281)

These components are transformed to the standard basis according to TKE TKE C ijkl = qip q jg q kr q ls C pqrs

(3-282)

and finally the constitutive tensor relating the rate of deformation to the Truesdell rate of Cauchy stress is obtained through TC TK C ijkl = J –1 C ijkl

(3-283)

Stress and Tangent Stiffness The principal Kirchhoff stress is in material model 181 given by 3

τ iE

1 = f ( λ i ) + K ( J – 1 ) – --3

 f ( λk )

(3-284)

k=1

f is a load curve determined from uniaxial data (possible at different strain rates). Furthermore, K is the bulk modulus and J is the relative volume change of the material. This stress cannot be deduced from a strain energy function unless f ( λ ) = E ln λ for some constitutive parameter E . A

where

consequence of this is that when using the formulas in the previous section the resulting tangent stiffness matrix is not necessarily symmetric. We remedy this by symmetrizing the formulas according to

162 Materials

E ii   λ ∂τ ------- j ∂λ j  symn

 2  E E --- λ i f' ( λi ) if i = j ∂τ ∂τ  1 ii jj 3 = ---  λ j --------- + λi --------- = KJ +  ∂λ i 2 ∂λ j  –1 - ( λ i f·( λi ) + λ j f' ( λ j ) ) otherwise  -6 

(3-285)

Two Remarks The function f introduced in the previous section depends not only on the stretches but for some choices of input also on the strain rate. Strain rate effects complicate things for an implicit analyst and here one also has to take into account whether the material is in tension/compression or in a loading/unloading stage. We believe that it is of little importance to take into account the strain rate effects when deriving the tangent stiffness matrix and therefore this influence has been disregarded. For the fully integrated brick element, we have used the approach in material model 77 to account for the constant pressure when deriving the tangent stiffness matrix. Experiments have shown that this is crucial to obtain a decent implicit performance for nearly incompressible materials. Modeling of the Frequency Independent Damping An elastic-plastic stress

σ d is added to model the frequency independent damping properties of rubber.

This stress is deviatoric and determined by the shear modulus

G and the yield stress σ Y . This part of

the stress is updated incrementally as n+1 σ˜ d = σ dn + 2 GI dev Δε

(3-286)

where Δε . is the strain increment. The trial stress is then radially scaled (if necessary) to the yield surface according to

σY  n+1 σ dn + 1 = σ˜ d min  1 ,-------σ eff where

n+1 σ eff is the effective von Mises stress for the trial stress σ˜ d

The elastic tangent stiffness contribution is given by

C d = 2 GI dev and if yield has occurred in the last time step the elastic-plastic tangent is used

(3-287)

Materials 163 Materials

3G C d = 2 GI dev – ------2- σ d ⊗ σ d σY

(3-288)

Here I dev is the deviatoric fourth order identity tensor.

Material Model 196: General Spring Discrete Beam If TYPE=0, elastic behavior is obtained. In this case, if the linear spring stiffness is used, the force, F, is given by:

F = F 0 + K Δ L + D Δ L·

(3-289)

but if the load curve ID is specified, the force is then given by:

  Δ L·  F = F 0 + Kf ( Δ L ) 1 + C 1 ⋅ Δ L· + C 2 ⋅ sgn ( Δ L· ) ln  max  1. ,------------  + D Δ L· + g ( Δ L ) h ( Δ L· )   DLE  In these equations, .L is the change in length

Δ L = current length – initial length If TYPE=1, inelastic behavior is obtained. In this case, the yield force is taken from the load curve:

F Y = F y ( Δ L plastic ) where

(3-290)

L plastic is the plastic deflection. A trial force is computed as:

F T = F n + K Δ L· Δ t and is checked against the yield force to determine

 Y F =  F  FT

(3-291)

F:

if F T > F Y if F T ≤ F Y

(3-292)

The final force, which includes rate effects and damping, is given by:

  Δ L·  F n + 1 = F ⋅ 1 + C 1 ⋅ Δ L· + C 2 ⋅ sgn ( Δ L· ) ln  max  1. ,------------  + D Δ L· + g ( Δ L ) h ( Δ L· )   DLE 

164 Materials

Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate,

F y . The positive part of

the curve is used whenever the force is positive. The cross-sectional area is defined on the section card for the discrete beam elements. See *SECTION_BEAM. The square root of this area is used as the contract thickness offset if these elements are included in the contact treatment.

Boundary Conditions 157

Boundary Conditions

158 Boundary Conditions

Boundary Conditions The motion of part or all of a model can be prescribed by Boundary and Initial conditions.

Single-Point Constraints A single-point constraint is used to prescribe the motion of a translational or rotational degree of freedom. The constraint is effective throughout the analysis and is used to specify boundary conditions or planes of symmetry. A single-point constraint is defined by an SPCn entry. The SPC entry defines the constraints on one grid point, while the SPC1 defines the constraints to be applied to a set of grid points. Several sets of SPC entries can be defined in the Bulk Data Section, but only those selected in the Case Control Section using the SPC = n command are incorporated in the analysis. Single-point constraints can also be defined using the GRIDt entry. These constraints are present for the entire analysis and do not need to be selected in Case Control. This is valid only for SPC and SPC1. Since Sol 700 is an explicit code, there is no matrix decomposition. Therefore, the problems of singular matrices that occur with some implicit codes do not exist. All, or part of the Lagrangian mesh can be entirely unconstrained and can undergo rigid body motion. SOL 700 correctly calculates the motion of the mesh. Similarly, the redundant degrees of freedom, such as the in-plane rotation of shell elements, do not need to be constrained since they do not affect the solution. The only constraints that are needed are those representing the boundary conditions of the model and those necessary for any planes of symmetry. The following SPC types are supported in MD Nastran SOL 700. • SPC • SPC1 • SPCADD • SPCD (at present, only velocity is available) • SPCD2

Multi-Point Constraints MPCs are special element types which define a rigorous behavior between several specified nodes. The following MPC types which are supported for MD Nastran SOL 700: • MPC • RBAR • RBE2 • RBE2A • RBE2D • RBE2F

Boundary Conditions 159 Boundary Conditions

• RBE3 • RBE3D • RBJOINT • REJSTIFF • RCONN

Specifying Explicit MPCs MPC’s may be created between a dependent degree of freedom and one or more independent degrees of freedom. The dependent term consists of a node ID and a degree of freedom; an independent term consists of a coefficient, a node ID, and a degree of freedom. An unlimited number of independent terms can be specified, but only one dependent term can be specified. The constant term is not allowed in MD Nastran. Description

MPC Types MPC

Defines a multipoint constraint equation.

References: “MPC” in the MD Nastran Quick Reference Guide.

Contact in SOL 700 The contact methodology and definition as implemented in MD Nastran Explicit Nonlinear are discussed here. The detailed theory anf algorithm behind the imlementation of contact in SOL 700 is discussed in the next chapter: Contact The simulation of many physical problems requires the ability to model the contact phenomena. This includes impact simulations, drop testing, component crush, crash, and manufacturing processes among others. The analysis of contact behavior is complex because of the requirement to accurately track the motion of multiple geometric bodies, and the motion due to the interaction of these bodies after contact occurs. This includes representing the friction between surfaces if required. The numerical objective is to detect the motion of the bodies, apply a constraint to avoid penetration, and apply appropriate boundary conditions to simulate the frictional behavior and heat transfer. Several procedures have been developed to treat these problems including the use of Perturbed or Augmented Lagrangian methods, penalty methods, and direct constraints. Furthermore, contact simulation has often required the use of special contact or gap elements. MD Nastran Explicit Nonlinear allows contact analysis to be performed automatically without the use of special contact elements. A robust numerical procedure to simulate these complex physical problems has been implemented in MD Nastran Explicit Nonlinear. Contact problems can be classified as one of the following types of contact. • Deformable-Deformable contact between two and three-dimensional deformable bodies.

160 Boundary Conditions

• Rigid - Deformable contact between a deformable body and a rigid body, for two- or

three-dimensional cases. Contact problems involve a variety of different geometric and kinematic situations. Some contact problems involve small relative sliding between the contacting surfaces, while others involve large sliding or penetration followed by perforation and failure. Some contact problems involve contact over large areas, while others involve contact between discrete points. The general Contact Body approach in SOL 600 is also adopted by MD Nastran Explicit Nonlinear (SOL 700) to model contact and can be used to handle most contact problem definitions.

Contact Bodies There are two types of contact bodies in MD Nastran Explicit Nonlinear – deformable and rigid. Deformable bodies are simply a collection of finite elements as shown below.

Figure 4-1

Deformable Body

This body has three key aspects to it: 1. The elements which make up the body. 2. The nodes on the external surfaces which might contact another body or itself. These nodes are treated as potential contact nodes. 3. The edges (2-D) or faces (3-D) which describe the outer surface which a node on another body (or the same body) might contact. These edges/faces are treated as potential contact segments. Note that a body can be multiply connected (have holes in itself). It is also possible for a body to have a self contact where the entire surface folds on to itself. A contact may include 1-D elements such as beams and rods, 2-D elements such as shells and membranes, and 3-D elements such as solids. Each element should be in, at most, one body. The elements in a body are defined using the BCBODY option. It is not necessary to identify the grid points on the exterior surfaces as this is done automatically. The algorithm used is based on the fact that grid points on the boundary are on element edges or faces that belong to only one element. Each node on the exterior surface is treated as a potential slave grid point. The second type of a contact body is called Rigid bodies. Rigid bodies are composed of (2-D) or (3-D) meshes and their most significant aspect is that they do not distort. Deformable bodies can contact rigid bodies and contact between rigid bodies is also allowed.

Boundary Conditions 161 Boundary Conditions

Rigid Walls A rigid wall is a plane through which specified slave grid points cannot penetrate. The rigid wall provides a convenient way of defining rigid targets in impact analyses.

Any number of rigid walls can be specified using WALL entries. The orientation of each wall is defined by the coordinates of a point on the wall and a vector that is perpendicular to the wall and points towards the model. At each time step, a check is made to determine whether the slave grid points have penetrated the wall. These slave points are defined using a Case Control SET entry, and there can be any number of them. Since a check is made for every slave point at each time step, you should specify only those points as slave points that are expected to contact the wall in order to ensure the most efficient solution. If a slave point is found to have penetrated the wall, it is moved back towards the wall so that its momentum is conserved. If the slave point subsequently moves away from the wall, it is allowed to do so. Slave points cannot have any other constraint. They can, however, be part of other contact.

Contact Detection During the incremental procedure, each potential contact node is first checked to see whether it is near a contact segment. The contact segments are either edges of other 2- D deformable bodies, faces of 3-D deformable bodies, or segments from rigid bodies. By default, each node could contact any other segment including segments on the body that it belongs to. This allows a body to contact itself. To simplify the computation, it is possible to use the BCTABLE entry to indicate that a particular body will or will not contact another body. This is often used to indicate that a body will not contact itself. During the iteration process, the motion of the node is checked to see whether it has penetrated a surface by determining whether it has crossed a segment. For more detailed discussion on the Contact, refer to Chapter 5 of this guide and see Chapter 12 in the SOL 600 User’s Guide.

162 Lagrangian Loading

Lagrangian Loading This section covers the different ways that the analysis model can be loaded. The facilities available are: • Concentrated Loads and Moments • Pressure Loads • Initial Conditions

Concentrated Loads and Moments

Concentrated loads and moments can be applied to any grid point using the DAREA, FORCE, FORCE2, entries in combination with a TLOADn entry. The types of concentrated load that can be applied are discussed in the following section.

FORCE, FORCE2, or DAREA – Fixed-Direction Concentrated Loads The FORCE, FORCE2, and DAREA entries define fixed direction loads. In other words, the direction of the force is constant throughout the analysis and does not change as the structure moves. FORCE, FORCE2, and DAREA entries have the same effect but define the loading in different ways. With the DAREA entry, you specify the grid point, the direction in the basic coordinate system in which the load acts, and the scale factor. With the FORCE entry, a concentrated force remains in the same direction for the entire problem. For FORCE2, the direction of the force follows the deformation and you define the grid point and the components of a vector giving the loading direction and the scale factor. In this case, the magnitude of the vector also acts as a scale factor, so the force in direction i is given by

P i = AN i . On a rigid body, the concentrated load or enforced motion is specified by defining the load at the rigid body center of gravity. To do so, set the TYPE field of the TLOAD1 or TLOAD2 entries to 13 and 12, respectively. The G field in the FORCE entry references the property number of the rigid body.

Boundary Conditions 163 Lagrangian Loading

Pressure Loads Pressure loads are applied to the faces of solid elements and to shell elements. Pressure loads are defined using the PLOAD or PLOAD4 entry in combination with a TLOADn entry.

TLOAD2 also references a set of PLOAD and/or PLOAD4 entries. Each entry selects the face of the element to be loaded by its grid points and defines the scale factor to be applied to the curve of pressure versus time. The actual pressure acting on the element p el is given as follows:

p el ( t ) = Ap ( t ) where

A is the scale factor.

The direction of positive pressure is calculated according to the right-hand rule using the sequence of grid points on the PLOAD entry. For PLOAD4 entries, the pressure is inwards for solid elements and in the direction of the element normal vector for shell elements. G4

G3

G1

G3

G1 G2

G2

The RFORCE entry defines enforced motion due to a centrifugal acceleration field. This motion affects all structural elements present in the problem. The GRAV defines an enforced motion due to a gravitational acceleration field. This motion affects all Lagrangian elements. Grid points with enforced motion cannot be: • Attached to a rigid body. • A slave point for a rigid wall.

To specify the motion of a rigid body, the enforced motion of the rigid-body center of gravity must be defined. To do so, set the TYPE field of the TLOAD1 and TLOAD2 entries to 12. The G field on the DAREA, FORCE entry references the property number of the rigid body. Initial Conditions The initial velocity of grid points can be defined using TIC, TIC3, and TICD entries. This allows the initial state of the model to be set prior to running the analysis. It is important to recognize the difference

164 Lagrangian Loading

between initial velocities and enforced velocities. Enforced velocities specify the motion of grid points throughout the transient analysis. Initial velocities, on the other hand, specify the velocity of grid points at the beginning of the analysis. Thereafter, the velocities are determined by the calculation. Where TIC and TIC3 set only the initial grid-point velocity, the TICD entry can be used to set the initial value of any valid grid point variable. It can also refer to a local coordinate system by including the CID1 and/or CID2 entry in the list.

Boundary Conditions 165 Boundary and Loading Conditions - Theoretical Background

Boundary and Loading Conditions Theoretical Background Pressure Boundary Conditions Consider pressure loadings on boundary

∂ b 1 in (4-1). To carry out the surface integration indicated by

the integral:

∂b N t t ds

(4-1)

1

a Gaussian quadrature rule is used. To locate any point of the surface under consideration, a position vector,

γ , is defined:

r = f 1 ( ξ ,η ) i 1 + f 2 ( ξ ,η ) i 2 + f 3 ( ξ ,η ) i 3

(4-2)

where: 4

f i ( ξ ,η ) =

 φj xi

j

(4-3)

j=1

and i 1 , i 2 , and i 3 are unit vectors in the x 1 , x 2 , and x 3 directions (see 4-2). Nodal quantities are interpolated over the four-node linear surface by the functions:

1 φ i = --- ( 1 + ξξ i ) ( 1 + ηη i ) 4 so that the differential surface area

(4-4)

ds may be written in terms of the curvilinear coordinates as:

ds = J d ξ d η where

J is the surface Jacobian defined by:

∂r ∂r J = ------ × ------ = ( EG – F 2 ) 1 ⁄ 2 ∂ξ ∂η

(4-5)

166 Boundary and Loading Conditions - Theoretical Background

in which:

∂r ∂r E = ------ ⋅ -----∂ξ ∂ξ ∂r ∂r F = ------ ⋅ -----∂ξ ∂η ∂r ∂r G = ------ ⋅ -----∂η ∂η

(4-6)

A unit normal vector

n to the surface segment is given by:

∂r ∂r n = J –1  ------ × ------ ∂ξ ∂η

(4-7)

and the global components of the traction vector can now be written: 4

t i = n i  φj p j

(4-8)

j=1

where

p j is the applied pressure at the jth node. η 3

2

x3

x2

ξ

4

i3

i1

Figure 4-2

1

rξ,η

i2

x1

Parametric Representation of a Surface Segment

Boundary Conditions 167 Boundary and Loading Conditions - Theoretical Background

The surface integral for a segment is evaluated as:

 1 t  –1  –1 N t J ( dξ ) dη 1

(4-9)

One such integral is computed for each surface segment on which a pressure loading acts. Note that the Jacobians cancel when (4-7) and (4-6) are put into (4-9). Equation 4-9 is evaluated with one-point integration analogous to that employed in the volume integrals. The area of an element side is approximated by

4 J where J = J ( 0, 0 ) .

Kinematic Boundary Conditions In this subsection, the kinematic constraints are briefly reviewed. SOL 700 tracks reaction forces for each type of kinematic constraint and provides this information as output if requested. For the prescribed boundary conditions, the input energy is integrated and included in the external work.

Displacement Constraints Translational and rotational boundary constraints are imposed either globally or locally by setting the constrained acceleration components to zero. If nodal single point constraints are employed, the constraints are imposed in a local system. The user defines the local system by specifying a vector u l in the direction of the local x-axis, x l , and a local in-plane vector v l . After normalizing u l , the local x l ,

y l , and z l axes are given by: ul x l = --------ul

(4-10)

xl × vl z l = ------------------xl × vl

(4-11)

yl = zl × xl

(4-12)

A transformation matrix

q is constructed to transform the acceleration components to the local system:

x lt q = y lt z lt

(4-13)

168 Boundary and Loading Conditions - Theoretical Background

and the nodal translational and rotational acceleration vectors a I and the local system:

· ω I , for node I are transformed to

a I l = qaI

(4-14)

· · ωIl = q ω I

(4-15)

and the constrained components are zeroed. The modified vectors are then transformed back to the global system: t

a I = q aIl

(4-16)

t· · ωI = q ωIl

(4-17)

Prescribed Displacements, Velocities, and Accelerations Prescribed displacements, velocities, and accelerations are treated in a nearly identical way to displacement constraints. After imposing the zero displacement constraints, the prescribed values are imposed as velocities at time, t n + 1 ⁄ 2 . The acceleration versus time curve is integrated or the displacement versus time curve is differentiated to generate the velocity versus time curve. The prescribed nodal components are then set.

Body Force Loads Body force loads are used in many applications. For example, in structural analysis the base accelerations can be applied in the simulation of earthquake loadings, the gun firing of projectiles, and gravitational loads. The latter is often used with dynamic relaxation to initialize the internal forces before proceeding with the transient response calculation. In aircraft engine design the body forces are generated by the application of an angular velocity of the spinning structure. For base accelerations and gravity, we can fix the base and apply the loading as part of the body force loads element by element according to (4-18).

f ebody = where

v

ρ N t Na base dυ = m e abase m

a base is the base acceleration and m e is the element (lumped) mass matrix.

(4-18)

Contact 169

Contact

170 Contact

Contact This section will summarize those parts of the contact methods applicable to SOL 700, and will describe the theory of the algorithms used. To activate contact in SOL 700, the Case Control entry BCONTACT must be given. There are three methods available to define contact: 1. All elements in the model in one contact definition, using default settings Case Control: BCONTACT=ALL This will result in automatic contact detection between all elements in the model. For SOL 700, it is advisable to use this method. 2. User defined Contact Bodies, using default or non-default settings Case Control: BCONTACT = n Bulk Data:

BCBODY, BSURF, or BCBOX or BCPROP or BCMATL, and BCTABLE

It is possible to define contact bodies (BCBODY), and specify which contact bodies need to be checked for contact (BCTABLE). This method using BCBODY definitions provides extreme flexibility and is compatible with the Implicit Nonlinear solution (SOL 600). A contact body is defined by the Bulk Data entry BCBODY, which references a set of elements (BSURF), a set of elements inside a box (BCBOX), or certain property IDs (BCPROP) or with certain material IDs (BCMATL). Often used definitions related to contact methods are: Single Surface Contact: This refers to any contact definition where no master is defined. Master Slave Contact:

This refers to any contact definition where a master is defined.

SOL 600 Contact Capabilities not yet supported by SOL 700 • 2-D contact, since SOL 700 only applies to 3-D

(DIM

on BCBODY)

• A rigid BCBODY defined by patches or geometric entities

(BEHAV=RIGID

on BCBODY)

(ISTYP (CONTROL

on BCBODY) on BCBODY)

• Body smoothing

(IDSPL

on BCBODY)

• User-defined distance below which a node is

(ERROR

on BCTABLE)

• Separation Force

(FNTOL

on BCTABLE)

• Interference closure

(CINTERF

on BCTABLE)

- Rigid BCBODY as a symmetry plane - Motion/Load controlled rigid BCBODY (See note below on rigid body modeling in SOL 700)

considered touching

Contact 171 Contact

• Glue options

(IGLUE &

on BCTABLE)

JGLUE • Contact heat transfer

(HEATC

on BCTABLE)

• Searching order

(ISEARCH

on BCTABLE)

• Initial node movement for stress-free contact (SOL 700 contact offers similar capability by means of the IGNORE option on the BCTABLE)

(ICOORD

on BCTABLE)

• Option to identify relevant nodes

(BCHANGE entry)

• Initial approach, release, motion until contact

(BCMOVE entry)

Notes on Rigid Body Modeling in SOL 700: Currently, only BEHAV = DEFORM is supported in SOL 700 on the BCBODY option. Rigid body modeling is possible, however, by defining a rigid material (MATD020). • Elements belonging to a MATD020 are properly treated in the contact calculations, and it is allowed to include them in a BCBODY with BEHAV = DEFORM. The contact calculations will

operate as if the material is rigid. The penalty based contact forces applied on the nodes are accumulated for the whole rigid body and applied as an external force and moment to the centerof-gravity of the rigid body. • Rigid body motion is allowed and properly simulated by SOL 700. • Initial velocities and boundary conditions acting on the nodes will be applied to the rigid body. • Rigid body must be assigned in “Masters” field in BCTABLE.

With these capabilities, a faceted rigid body, similar to a BCBODY with BEHAV=RIGID can be easily modeled. The BEHAV=RIGID logic will be implemented in the next release of SOL 700.

SOL 600 Contact Limitations that do not apply to SOL 700 To allow switching between SOL 700 and SOL 600, it is advisable to work within these limits. In SOL 600, each node and element should be in at most one contact body. When using the penalty method of SOL700 (the default), this limitation does not apply. Forces as calculated by each contact are simply accumulated and applied as an external force vector. In SOL 600, only 1000 contact bodies are allowed. This limit does not apply to SOL 700. In SOL 600, it is important to properly define the order in which contact bodies are defined for deformable-to-deformable contact. The order of contact body definition has no influence on the results in SOL 700.

172 Penalty Methods

Penalty Methods The treatment of sliding and impact along interfaces is an important capability in SOL 700. Internally, the interfaces are defined in three dimensions by listing in arbitrary order all triangular and quadrilateral segments that comprise each side of the interface. One side of the interface is designated as the slave side, and the other is designated as the master side. Nodes lying in those surfaces are referred to as slave and master nodes, respectively. When slave nodes penetrate the master, normal interface springs are placed between the penetrated nodes and the master surface. See Slave Search in this chapter for details on the contact force calculations.

∂ b1 b

1

b

∂B B

1 0

Figure 5-1

∂ b2

1

2

∂ B2 2 B0

Reference and Deformed Configuration

Contact 173 Preliminaries

Preliminaries Consider the time-dependent motion of two bodies occupying regions B 1 and B 2 in their undeformed configuration at time zero. Assume that the intersection

B1∩ B2 = φ is satisfied. Let

(5-1) 1

2

∂ B 1 and ∂ B 2 denote the boundaries of B and B , respectively. At some later time,

these bodies occupy regions b 1 and b 2 bounded by the deformed configurations cannot penetrate,

∂ b 1 and ∂ b 2 as shown in Figure 5-1. Because

( b1 – ∂ b1 )∩ b2 = φ As long as

(5-2)

∂ b 1 ∩ ∂ b 2 = φ , the equations of motion remain uncoupled. In the foregoing and

following equations, the right superscript

α ( = 1, 2 ) denotes the body to which the quantity refers.

Before a detailed description of the theory is given, some additional statements should be made concerning the terminology. The surfaces ∂ b 1 and ∂ b 2 of the discretized bodies b 1 and b 2 become the master and slave surfaces respectively. Choice of the master and slave surfaces is arbitrary when the symmetric penalty treatment is employed. Otherwise, the more coarsely meshed surface should be chosen as the master surface, nodal points that define

∂ b 1 are called master nodes and nodes that define

∂ b 2 are called slave nodes. When ( ∂ b 1 ∩ ∂ b 2 ) ≠ φ , the constraints are imposed to prevent penetration. Right superscripts are implied whenever a variable refers to either the master surface or slave surface,

∂b1 ,

∂ b 2 ; consequently, these superscripts are dropped in the development which follows.

174 Slave Search

Slave Search The slave search is common to all interface algorithms implemented in SOL 700. This search finds for each slave node its nearest point on the master surface. Lines drawn from a slave node to its nearest point will be perpendicular to the master surface, unless the point lies along the intersection of two master segments, where a segment is defined to be a 3- or 4-node element of a surface. Consider a slave node, n s , sliding on a piecewise smooth master surface and assume that a search of the master surface has located the master node, master surface with nodes

m s , lying nearest to n s . Figure 5-2 depicts a portion of a

m s and n s labeled. If m s and n s do not coincide, n s can usually be shown

to lie in a segment s s via the following tests:

( ci × s ) ⋅ ( ci × ci + 1 ) > 0 ( ci × s ) ⋅ ( s × ci + 1 ) > 0 where vector c i and c i + 1 are along edges of s 1 and point outward from of the vector beginning at

(5-3)

m s . Vector s is the projection

m s , ending at n s , and denoted by g , onto the plane being examined (see

Figure 5-3).

s = g – ( g ⋅ m)m

(5-4)

Contact 175 Slave Search

Figure 5-2

Four Master Segments can Harbor Slave Node n s given that m s is the Nearest Master Node

Figure 5-3

Projection of

g onto master segment s 1

where for segment s 1

ci × ci + 1 m = -----------------------ci × ci + 1

(5-5)

Since the sliding constraints keep n s close but not necessarily on the master surface and since n s may lie near or even on the intersection of two master segments, the inequalities of Equation (5-3) may be inconclusive; i.e., they may fail to be satisfied or more than one may give positive results. When this occurs

n s is assumed to lie along the intersection which yields the maximum value for the quantity

g ⋅ ci ----------- i = 1, 2, 3, 4, … ci

(5-6)

When the contact surface is made up of badly shaped elements, the segment apparently identified as containing the slave node actually may not, as shown in Figure 5-4. Assume that a master segment has been located for slave node n s and that n s is not identified as lying on the intersection of two master segments. Then the identification of the contact point, defined as the point on the master segment which is nearest to

n s , becomes nontrivial. Each master surface segment

s 1 , is given the parametric representation: r = f 1 ( ξ ,η ) i 1 + f 2 ( ξ ,η ) i 2 + f 3 ( ξ ,η ) i 3

(5-7)

176 Slave Search

where 4

f i ( ξ, η ) –

 φj xi

j

(5-8)

j=1

When the nearest node fails to contain the segment that harbors the slave node, segments numbered 1-8 are searched in the order shown in Figure 5-4. 1

2

8

6

3

7

5 4

Figure 5-4

Search Order for Segments

Note that r 1 is at least once continuously differentiable and that

∂r ∂ r- ---------× ≠0 ∂ξ ∂η

(5-9)

r represents a master segment that has a unique normal whose direction depends continuously on the points of s 1 .

Thus,

Let

t be a position vector drawn to slave node n s and assume that the master surface segment s 1 has

been identified with

n s . The contact point coordinates ( ξ c, η c ) on s 1 must satisfy

∂ r----( ξ , η ) ⋅ [ t – r ( ξ c, η c ) ] = 0 ∂ξ c c

(5-10)

∂r -----( ξ , η ) ⋅ [ t – r ( ξ c, η c ) ] = 0 ∂η c c

(5-11)

The physical problem is illustrated in Figure 5-5, which shows n s lying above the master surface. Equations (5-10) and (5-11) are readily solved for ξ c and η c . One way to accomplish this is to solve

Contact 177 Slave Search

Equation (5-10) for ξ c in terms of in η c .

η c , and substitute the results into (5-11). This yields a cubic equation

η 3 ns

ξ

∂r----∂ξ

t

x3

2 ∂r -----∂η

4 r

1

x2 x1

Figure 5-5

Location of Contact Point when

n s lies above Master Segment

The equations are solved numerically. When two nodes of a bilinear quadrilateral are collapsed into a single node for a triangle, the Jacobian of the minimization problem is singular at the collapsed node. Fortunately, there is an analytical solution for triangular segments since three points define a plane. Newton-Raphson iteration is a natural choice for solving these simple nonlinear equations. The method diverges with distorted elements unless the initial guess is accurate. An expanded search procedure as discussed in Improvements to the Contact Searching section is used. Three iterations with a least-squares projection are used to generate an initial guess:

ξ 0 = 0,

η 0 = 0,

r   [ r ,ξ r ,η ]  Δξ  = ,ξ { r ( ξ i, η i ) –t }, r ,η r ,η  Δη  ξ i + 1 = ξ i + 1 + Δξ, η i + 1 = η i + Δη r ,ξ

followed by the Newton-Raphson iterations which are limited to ten iterations, but which usually converges in four or less.

(5-12)

178 Slave Search

 Δξ   r ,ξ  [ H ]   = –   { r ( ξ i, η i ) –  Δη   r ,η  0 r ⋅ r,  r ,χ  [ H ]  [ r ,ξ r ,η ] + r ⋅ r ,ξη 0  r ,η  ξ i + 1 = ξ i + Δξ η i + 1 = η i + Δη

(5-13)

In concave regions, a slave node may have isoparametric coordinates that lie outside of the [ – 1 ,+1 ] range for all of the master segments, yet still have penetrated the surface. A simple strategy is used for handling this case, but it can fail. The contact segment for each node is saved every time step. If the slave node contact point defined in terms of the isoparametric coordinates of the segment, is just outside of the segment, and the node penetrated the isoparametric surface, and no other segment associated with the nearest neighbor satisfies the inequality test, then the contact point is assumed to occur on the edge of the segment. In effect, the definition of the master segments is extended so that they overlap by a small amount. In the hydrocode literature, this approach is similar to the slide line extensions used in two dimensions. This simple procedure works well for most cases, but it can fail in situations involving sharp concave corners.

Contact 179 Contact Force Calculation

Contact Force Calculation Each slave node is checked for penetration through the master surface. If the slave node does not penetrate, nothing is done. If it does penetrate, an interface force is applied between the slave node and its contact point. The magnitude of this force is proportional to the amount of penetration. This may be thought of as the addition of an interface spring. Penetration of the slave node n s through the master segment which contains its contact point is indicated if

l = n i ( [ t – r ( ξ c, η c ) ] < 0 )

(5-14)

where

n i = n i ( ξ c, η c )

(5-15)

is normal to the master segment at the contact point. The amount of penetration is equal to the value of l. If slave node

ns has penetrated through master segment s i , we add an interface force vector f s :

f s = –lk i n i if l < l < 0 to the degrees of freedom corresponding to

(5-16)

n s and

f mi = φ 2 ( ξ c, η c ) f s if l < 0

(5-17)

( i = 1, 2, 3, 4 ) that comprise master segment s i . By default, SOFT=1 on the BCTABLE entry, and the stiffness factor k i is given in terms of the nodal masses and the global timestep,

to the four nodes

dt as m slave m master 1 k i = f si ⋅ --------------------------------------- ⋅ ------2m slave + m master dt

(5-18)

With SOFT=1, it is mostly not needed to scale the contact stiffness, even if materials with very different stiffness properties come into contact. When SOFT=0 on the BCTABLE entry, the stiffness factor k i for master segment s i is given in terms of the bulk modulus

K i , the volume V i , and the face area A i of the element that contains s i as

f si K i A i2 k i = ----------------Vi for brick elements and

(5-19)

180 Contact Force Calculation

f si K i A i k i = ------------------------------------------------max ( shell diagonal )

(5-20)

for shell elements. When too much penetration is observed, the contact stiffness can be increased by the interface stiffness scale factor, f si . This scale factor is 0.1 by default, and can be defined by FACT on the BCTABLE entry. Larger values may cause instabilities unless the time step size is scaled back in the time step calculation.

Contact 181 Improvements to the Contact Searching

Improvements to the Contact Searching A number of recent changes have been made in the surface-to-surface contact including contact searching, accounting for thickness, and contact damping. Sometimes problems with the closest master node contact searching were found. The nearest node algorithm described above can break down since the nearest node is not always anywhere near the segment that harbors the slave node as is assumed in Figure 5-4 (see Figure 5-6). Such distorted elements are commonly used in rigid bodies in order to define the geometry accurately. closest nodal point

slave node

Figure 5-6

Failure to find the Contact Segment can be caused by Poor Aspect Ratios in the Finite Element Mesh

To circumvent the problem caused by bad aspect ratios, an expanded searching procedure is used in which we attempt to locate the nearest segment rather than the nearest nodal point.

1

2

3

4

5

Normal vector at node 3

Figure 5-7

Expanded Search

Nodes 2 and 4 share segments with node 3. Therefore, the two nearest nodes are 1 and 5. The nearest contact segment is not considered since its nodes are not members of the nearest node set.

k , is defined to be the first segment encountered when moving in a direction normal to the surface away from k . A major deficiency with the nearest node The nearest contact segment to a given node,

search is depicted in Figure 5-7 where the nearest nodes are not even members of the nearest contact

182 Improvements to the Contact Searching

segment. Obviously, this would not be a problem for a more uniform mesh. To overcome this problem we have adopted segment based searching in both surface to surface and single surface contact.

Contact 183 Bucket Sorting

Bucket Sorting Bucket sorting is now used extensively in the SOL 700 contact algorithms. The reasons for eliminating slave node tracking by incremental searching is illustrated in Figure 5-8 where surfaces are shown which cause the incremental searches to fail. With bucket sorting incremental searches may still be used but for reliability they are used after contact is achieved. As contact is lost, the bucket sorting for the affected nodal points must resume. In a direct search of a set of

N nodes to determine the nearest node, the number of distance comparisons

N – 1 . Since this comparison needs to be made for each node, the total number of comparisons is N ( N – 1 ) , with each of these comparisons requiring a distance calculation required is

1 2 = ( xi – xj ) 2 + ( yi – yj ) 2 + ( zi – z j ) 2

(5-21)

that uses eight mathematical operations. The cumulative effect of these mathematical operations for

N ( N – 1 ) compares can dominate the solution cost at less than 100 elements. The idea behind a bucket sort is to perform some grouping of the nodes so that the sort operation need only calculate the distance of the nodes in the nearest groups. With this partitioning the nearest node will either reside in the same bucket or in one of the two adjoining buckets. The number of distance calculations is now given by

3-----N–1 α

(5-22)

where α is the number of buckets. The total number of distance comparisons for the entire onedimensional surface is

3N N  ------- – 1 α

(5-23)

Thus, if the number of buckets is greater than 3, then the bucket sort will require fewer distance comparisons than a direct sort. It is easy to show that the corresponding number of distance comparisons for two-dimensional and three-dimensional bucket sorts are given by

9N N  ------- – 1 for 2-D αb

(5-24)

27 N N  ---------- – 1 for 3-D  α bc 

(5-25)

where

b and c are the number of partitions along the additional dimension.

184 Bucket Sorting

Incremental searching may fail on surfaces that are not simply connected. The contact algorithm in SOL 700 avoids incremental searching for nodal points that are not in contact and all these cases are considered (see Figure 5-8).

tied interface not yet supported

Figure 5-8

Examples of Models where Incremental Searching may Fail

The cost of the grouping operations, needed to form the buckets, is nearly linear with the number of nodes

N . For typical SOL 700 applications, the bucket sort is 100 to 1000 times faster than the corresponding direct sort. However, the sort is still an expensive part of the contact algorithm, so that, to further minimize this cost, the sort is performed every ten or fifteen cycles and the nearest three nodes are stored. This can be specified by BSORT on the BCTABLE entry. Typically, three to five percent of the calculational costs will be absorbed in the bucket sorting when most surface segments are included in the contact definition.

Contact 185 Bucket Sorting in Single Surface Contact

Bucket Sorting in Single Surface Contact We set the number of buckets in the x, y, and z coordinate directions to NX, NY, and NZ, respectively. The product of the number of buckets in each direction always approaches NSN or 5000 whichever is smaller,

NX ⋅ NY ⋅ NZ ≤ MIN ( NSN ,5000 ) where the coordinate pairs

(5-26)

( x min, x max ) , ( y min, y max ) , and ( z min, z max ) span the entire contact

surface. In this procedure, we loop over the segments rather than the nodal points. For each segment we use a nested DO LOOP to loop through a subset of buckets from

IMIN to IMAX , JMIN to

JMAX , and KMIN to KMAX where: IMIN = MIN ( PXI, PX 2, PX 3, PX 4 ) IMAX = MAX ( PX 1, PX 2, PX 3, PX 4 ) JMIN = MAX ( PY 1, PY 2, PY 3, PY 4 ) JMAX = MAX ( PY 1, PY 2, PY 3, PY 4 ) KMIN = MAX ( PZ 1, PZ 2, PZ 3, PZ 4 ) kMAX = MAX ( PZ 1, PZ 2, PZ 3, PZ 4 )

(5-27)

and PXk , PYk , PZk are the bucket pointers for the kth node. Figure 5-9 shows a segment passing through a volume that has been partitioned into buckets. The orthogonal distance of each slave node contained in the box from the segment is determined. The box is subdivided into sixty buckets.

z

Nodes in buckets shown are checked for contact with the segment

y

x

Figure 5-9

The Orthogonal Distance of each Slave Node

186 Bucket Sorting in Single Surface Contact

We check the orthogonal distance of all nodes in the bucket subset from the segment. As each segment is processed, the minimum distance to a segment is determined for every node in the surface and the two nearest segments are stored. Therefore the required storage allocation is still deterministic. This would not be the case if we stored for each segment a list of nodes that could possibly contact the segment. We have now determined for each node, k , in the contact surface the two nearest segments for contact. Having located these segments we permanently store the node on these segments which is nearest to node

k . When checking for interpenetrating nodes we check the segments surrounding the node including the nearest segment since during the steps between bucket searches it is likely that the nearest segment may change. It is possible to bypass nodes that are already in contact and save some computer time; however, if multiple contacts per node are admissible then bypassing the search may lead to unacceptable errors.

Contact 187 Accounting For the Shell Thickness

Accounting For the Shell Thickness Shell thickness effects are important when shell elements are used to model sheet metal. Unless thickness is considered in the contact, the effect of thinning on frictional interface stresses due to membrane stretching will be difficult to treat. In the treatment of thickness we project both the slave and master surfaces based on the mid-surface normal projection vectors as shown in Figure 5-10. The surfaces, therefore, must be offset by an amount equal to 1/2 their total thickness (Figure 5-11). This allows the program to check the node numbering of the segments automatically to ensure that the shells are properly oriented.

Length of projection vector is 1/2 the shell thickness Projected Contact Surface

Figure 5-10

Contact Surface Based Upon Midsurface Normal Projection Vectors

Figure 5-11

The Slave and Master Surfacess

Thickness changes in the contact are accounted for “if and only if” the shell thickness change option is flagged on the PARAM* DYCONTHKCHG. Each cycle, as the shell elements are processed, the nodal thicknesses are stored for use in the contact algorithms. The interface stiffness may change with thickness depending on the input options used. To account for the nodal thickness, the maximum shell thickness of any shell connected to the node is taken as the nodal thickness and is updated every cycle. The projection of the node is done normal to the contact surface:

188 Initial Contact Penetrations

Initial Contact Penetrations The need to offset contact surfaces to account for the thickness of the shell elements contributes to initial contact penetrations. These penetrations can lead to severe numerical problems when execution begins so they should be corrected if SOL 700 is to run successfully. Often an early growth of negative contact energy is one sign that initial penetrations exist. Currently, warning messages are printed to the D3HSP file to report penetrations of nodes through contact segments and the modifications to the geometry made by SOL 700 to eliminate the penetrations. Sometimes such corrections simply move the problem elsewhere since it is very possible that the physical location of the shell mid-surface and possibly the shell thickness are incorrect. In the single surface contact algorithms any nodes still penetrating on the second time step are removed from the contact with a warning message. In some geometry's, penetrations cannot be detected since the contact node penetrates completely through the surface at the beginning of the calculation. Such penetrations are frequently due to the use of coarse meshes. This is illustrated in Figure 5-12. Another case contributing to initial penetrations occurs when the edge of a shell element is on the surface of a solid material as seen in Figure 5-13. Currently, shell edges are rounded with a radius equal to one-half the shell thickness. Detected Penetration

Figure 5-12

Undetected Penetration

Undetected Penetration

brick

shell

Inner penetration if edge is too close

Figure 5-13

Undetected Penetration due to rounding the Edge of the Shell Element

To avoid problems with initial penetrations, the following recommendations should be considered: • Adequately offset adjacent surfaces to account for part thickness during the mesh

generation phase. • Use consistently refined meshes on adjacent parts which have significant curvatures. • Be very careful when defining thickness on shell and beam section definitions - especially for

rigid bodies.

Contact 189 Initial Contact Penetrations

• Scale back part thickness if necessary. Scaling a 1.5mm thickness to .75mm should not cause

problems but scaling to .075mm might. Alternatively, define a smaller contact thickness by part ID. Warning: if the part is too thin contact failure will probably occur • Use spot welds instead of merged nodes to allow the shell mid surfaces to be offset.

190 Contact Energy Calculation

Contact Energy Calculation Contact energy,

E contact , is incrementally updated from time n to time n + 1 for each contact

interface as: nsn n+1 n E contact = E contact +

nmn

 Δ Fi

slave

× Δ dist islave +

i=1

Where

 Δ Fi

master

× Δ dist imaster

1 n + --2

i=1

nsn is the number of slave nodes, nmn is the number of master nodes, Δ F islave is the

interface force between the ith slave node and the contact segment between the ith master node and the contact segment,

Δ F imaster is the interface force

Δ dist islave is the incremental distance the ith

slave node has moved during the current time step, and

Δ dist imaster is the incremental distance the ith

master node has moved during the current time step. In the absence of friction the slave and master side energies should be close in magnitude but opposite in sign. The sum,

E contact , should equal the stored

energy. Large negative contact energy is usually caused by undetected penetrations. Contact energies are reported in the GLSTAT file. In the presence of friction and damping discussed below the interface energy can take on a substantial positive value especially if there is, in the case of friction, substantial sliding.

Contact 191 Friction

Friction Friction in SOL 700 is based on a Coulomb formulation. Let

f * be the trial force, f n the normal force,

n

k the interface stiffness, μ the coefficient of friction, and f the frictional force at time n. The frictional algorithm, outlined below, uses the equivalent of an elastic plastic spring. The steps are as follows: 1. Compute the yield force,

Fy :

Fy = μ fn

(5-28)

2. Compute the incremental movement of the slave node

Δ e = r n + 1 ( ξ cn + 1, η cn + 1 ) – r n + 1 ( ξ cn, η cn )

(5-29)

3. Update the interface force to a trial value:

f∗ = f n – k Δ e

(5-30)

4. Check the yield condition:

f n + 1 = f∗ if f∗ ≤ F y

(5-31)

5. Scale the trial force if it is too large:

F y f∗ f n + 1 = ---------- if f∗ > F y f∗

(5-32)

An exponential interpolation function smooths the transition between the static,

μ s , and dynamic, μ d ,

coefficients of friction where

ν is the relative velocity between the slave node and the master segment:

μ = μ d + ( μ s – μ d ) e –c ν

(5-33)

where

ΔeΔT ν = --------------

(5-34)

Δ t is the time step size, and C is a decay constant. Typical values of friction, see Table 5-1, can be found in Marks Engineering Handbook. Table 5-1

Typical Values of Coulomb Friction [Marks]

MATERIALS

STATIC

SLIDING

Hard steel on hard steel

0.78 (dry)

.08 (greasy), .42 (dry)

Mild steel on mild steel

0.74 (dry)

.10 (greasy), .57 (dry)

192 Friction

Table 5-1

Typical Values of Coulomb Friction [Marks]

MATERIALS

STATIC

SLIDING

Aluminum on mild steel

0.61 (dry)

.47 (dry)

Aluminum on aluminum

1.05 (dry)

1.4 (dry)

Tires on pavement (40psi)

0.90 (dry)

.69(wet), .85(dry)

Airbag and Occupant Safety 193

Airbag and Occupant Safety

194 Airbag and Occupant Safety

Airbag and Occupant Safety The MD Nastran r2 release, SOL 700 includes a Fluid Structure Interaction (FSI) capability that is based on the advanced Finite Volume (Eulerian) and General Coupling Technology available in MSC.Dytran. The FSI capability in the MD Nastran r2 release, however, is only limited to airbag and occupant safety simulation. The objective of fluid-structure interaction using the coupling algorithm is to enable the material modeled in Eulerian and Lagrangian meshes to interact. Initially, the two solvers are entirely separate. Lagrangian elements that lie within an Eulerian mesh do not affect the flow of the Eulerian material and no forces are transferred from the Eulerian material back to the Lagrangian structure. The coupling algorithm computes the interaction between the two sets of elements. It thus enables complex fluid-structure interaction problems to be analyzed. The first task in coupling the Eulerian and Lagrangian sections of a model is to create a surface on the Lagrangian structure. This surface is used to transfer the forces between the two solver domains. The surface acts as a boundary to the flow of material in the Eulerian mesh. At the same time, the stresses in the Eulerian elements cause forces to act on the coupling surface, distorting the Lagrangian elements. The method used for airbag simulation is full gas dynamics and is based on General Coupling with adaptive Euler. SOL 700 computes the fluid flow and Coupling based on MSC.Dytran solver while the Contact and Fabric models are co-simulated by LS-DYNA. Unlike other techniques such as the ALE (Arbitrary Lagrange Euler) where the Eulerian mesh is fixed in space or GBAG method where the gas flow is modeled by applying a pre-determined pressure profile to inflate the bag, in the General Coupling technique, the Eulerian mesh will “adapt” itself to the Lagrangian fabric model as the airbag is inflated. In other words, when the airbag is initially at the folded stage, there is a small Eulerian domain encapsulating the Lagrangian mesh. When the airbag is inflated, the Eulerian mesh expands as the gas jet flows through the airbag compartments and adapts itself to follow the airbag fabric. This technique is unique in MD Nastran r2 and is considered the most accurate method to predict the complex airbag behavior such as Out-of-Position (OOP) simulation, as required by FMVSS 208, where the occupant is already leaning forward when the airbag is inflated. In addition, CFD deployment of multicompartmented airbags can easily be modeled with this technique by using multiple, fully automatic, adaptive Euler domains. The following capabilities are available: • Analyze multiple compartments with the CFD approach. • Simulate flow from one CFD domain into another CFD domain. • The individual CFD domains are dynamic and adaptive. The user does not need to mesh the CFD

domains, nor does he have to worry about the size, since the CFD domains will automatically follow the deploying airbag compartments. • Flow through both small and large holes is accurately calculated.

Airbag and Occupant Safety 195 Airbag and Occupant Safety

• Inflator models

(a) Shape of Side Curtain airbag at Start of Simulation

(b) Euler Meshes for all Six Regions

(c) Shape of Bag after 20 milliseconds

Figure 6-1

Multi-compartment Side Curtain Airbag

196 Airbag Definition

Airbag Definition The airbags are defined by using the AIRBAG entry in SOL 700. Airbags can be automatically inflated by defining a gas flow rate in Eulerian domain using full gas dynamics method. A second method, the conventional uniform pressure method, is also available but it is not as accurate as the full gas dynamics. All related airbag input definitions such as inflator and porosity models, environmental parameters, are grouped in enties that can be directly input in the AIRBAG entry. Every entity has certain parameters associated with it that has to be input immediately following the name of the entity. The order of which entity is entered first in the AIRBAG card is immaterial as long as the associated parameters are defined right after the name of the entity. The following entity groups are available:

“CFD”

Entries for this entity describe the properties of the Eulerian domain. Only one "CFD" section can be defined. If this section is not defined, the uniform pressure method is used.

“ENVIRONM” Entries for this entity describe the properties of the environmental conditions for the airbag. Only one “ENVIRONM” section can be defined. If not defined, the values for “INITIAL” will be used. “INITIAL”

Entries for this entity describe the properties of the environmental conditions for the airbag. Only one “INITIAL” section can be defined and is required.

“INFLATOR”

Entries for this entity describe the properties of an inflator that is attached to the airbag. More than one inflator may be defined.

“CGINFLTR”

Entries for this entity describe the properties of a cold gas inflator that is attached to the airbag. More than one inflator may be defined.

“SMALHOLE” Entries for this entity describe the properties of a small hole in the airbag. More than one SMALHOLE may be defined. A small hole should be used when the size of the hole is of the same order as the size of the elements of the Euler mesh. “LARGHOLE” Entries for this entity describe the properties of a large hole in the airbag. More than one LARGHOLE may be defined. A large hole should be used when the size of the hole is of the larger than the size of the elements of the Euler mesh. “PERMEAB”

Entries for this entity describe the properties of the permeability of the airbag fabric. More than one PERMEAB may be defined.

“CONVECT”

Entries for this entity describe the properties of the loss of energy of the gas in the airbag by means of convection through the airbag surface. More than one CONVECT may be defined.

Airbag and Occupant Safety 197 Airbag Definition

“RADIATE”

Entries for this entity describe the properties of the loss of energy of the gas in the airbag by means of radiation through the airbag surface. More than one RADIATE may be defined. When this option is used, the Stephan-Boltzmann constant must be defined by PARAM, SBOLTZ.

“GAS”

Entries for this entity describe the properties of gases. More than 1 GAS may be defined and the gases defined in one AIRBAG entry can be referenced by other AIRBAG entries.

There are other entries in SOL 700 to define airbag properties. These are:

PARAM, UGASC

defines a value for the universal gas constant.

PARAM, SBOLTZ

defines a value for the Stephan-Boltzmann constant

PARAM, DYDEFAUL controls the default setting of the simulation INFLFRC

defines the hybrid inflator gas fraction

EOSGAM

Gamma Law Gas Equation of State

GRIA

grid point in airbag reference geometry

Please see MD Nastran r2 QRG for more details.

Inflator Models in Airbags There are several methods available to define an inflator in airbag analyses. The most general inflator definitions are:

INFLATR1

Standard inflator defined by mass flow rate and static temperature of a single inflowing gas.

INFLHYB1

Hybrid inflator defined by mass flow rate and static temperature of multiple inflowing gasses.

Figure 6-2

Airbag and Occupant Safety using SOL 700

198 Airbag Definition

For both the uniform pressure model and the full gas dynamics (CFD) method, the inflator location and area are defined by means of a subsurface created by a BSURF, BCPROP, BCMATL, or BCSEG parameters. These parameters are referenced by BFID field on the INFLATOR entity. It can only reference shell elements that belong to the airbag surface, as defined by BFID. The characteristics of the inflator are specified on an INFLATOR entity on AIRBAG card. This entry references tables for the mass flow rate and the temperature of the inflowing gas. A model can be defined containing both (CFD) and uniform pressure model for the airbag. These two options can be defined with identical inflator characteristics. When the CFD entity and its associated parameters are omitted from the AIRBAG card, the uniform pressure method will be used. In case the CFD entity is present, the airbag will use the Euler method from the start of the simulation. In case the value of SWITCH is nonzero, the airbag will switch from an Eulerian representation to a Uniform Pressure formulation.

Constant Volume Tank Tests Constant volume tank tests are used to characterize inflators. The inflator is ignited within the tank and, as the propellant burns, gas is generated. The inflator temperature is assumed to be constant. From experimental measurements of the time history of the tank pressure it is straightforward to derive the mass flow rate,

m· .

From energy conservation, where

T i and T t are defined to be the temperature of the inflator and tank,

respectively, we obtain:

c p m· T i = c v m· T t + c v m· T· t For a perfect gas under constant volume,

V· = 0 , hence,

p· V = m· RT t + mRT· t and, finally, we obtain the desired mass flow rate:

c v p· V · ------------m = c p RT t

Porosity in Airbags Porosity is defined as the flow of gas through the airbag surface. There are two ways to model this: 1. Holes: The airbag surface contains a discrete hole. 2. Permeability: The airbag surface is made from material that is not completely sealed.

Airbag and Occupant Safety 199 Airbag Definition

The same porosity models are available for both the uniform pressure airbag model as the Eulerian coupled (CFD) airbag model. The porous flow can be either to and from the environment or into and from another uniform pressure model. Holes Flow through holes as defined on the SMALHOLE entries is based on the theory of one-dimensional gas flow through a small orifice. LARGHOLE entries define flow through a hole with the velocity method. The velocity method can only be active for Eulerian airbags. When the SMALHOLE is used on the AIRBAG card, the theory of one-dimensional gas flow through a small orifice is applied. Velocity Method The transport of mass through the porous area is based on the velocity of the gas in the Eulerian elements,relative to the moving of coupling surface (airbag fabric). Eulerian Element

SX int v

Face of the coupling surface that intersects the Eulerian element

Coupling Surface

The volume of the Eulerian materian transported through the faces of the coupling surface that intersect an Eulerian element is equal to

V trans = – d t ⋅ α ⋅ ( v ⋅ A ) where

V trans = transported volume during one time step ( V trans > 0 for the outflow; V trans < 0 for the inflow).

dt α v A

= time step. = porosity coefficient. = velocity vector of the gas in the Eulerian mesh = area of the face of the coupling surface that intersects the Eulerian element the area of the face that lies inside the Eulerian element.

The transport mass through the porous area is equal to the density of the gas times the transported volume.

A is equal to

200 Airbag Definition

Pressure Method The transport of mass through the porous area is based on the pressure difference between the gas in the Eulerian element and the outside pressure. The outside pressure is the pressure as specified on the ENVIRONM section in the AIRBAG entry. Eulerian Element

SX int v

Face of the coupling surface that intersects the Eulerian element

Coupling Surface

The volume of the Eulerian material transported through the faces of the coupling surface that intersect an Eulerian element is equal to: γ+1

V trans

2 p ργ pexh 2 / γ p exh ----------= dt ⋅ α ⋅ ( A ⋅ A ) ⋅ ------------  --------- –  --------- γ p p γ–1

where

V trans dt α v A

= transported volume during one ture step ( V trans

p= ρ γ p exh

= pressure of the gas in the Eulerian element.

> 0 for outflow; V trans < 0 for inflow).

= time step. = porosite coefficient. = velocity vector of the gas in the Eulerian mesh. = area of the face of the coupling surface that intersects the Eularian element the area of the face that lies inside the Eulerian element.

A is equal to

= density of the gas in the Eulerian element. = adiabatic exponent =

C p ⁄ Cv .

= pressure of the face.

The pressure at the face is approximated by the one-dimensional isentropic expansion of the gas to the critical pressure or the environmental pressure ascending to

Airbag and Occupant Safety 201 Airbag Definition

  p > pc p =  env  p env < p c  where

p c is the critical pressure: r

2 ----------p c p ⋅  ----------- r – 1 γ+1 In case the outside pressure is greater than the pressure of the gas, inflow through the coupling surface occurs. This porosity model can only be used for ideal gases; i. e., materials modeled with the gamma law equation of state (EOSGAM). Permeability Permeability is defined as the velocity of gas through a surface area depending on the pressure differenceover that area. On the PERMEAB entity in AIRBAG card, permeability can be specified by either a coefficient or a pressure dependent table: 1. Coefficient:

Massflow = coeff * pressure_difference

Gas Velocity

δ ( massflow) ) coeff = --------------------------------δ ( pressdiff ) Coeff press_diff

2. Table Gas Velocity

Pressure Dependent Table

press_diff

The velocity of the gas flow can never exceed the sonic speed:

202 Airbag Definition

V max – V sonic – γ RT crit where

γ is the gas constant of in- or outflowing gas and T crit is the critical temperature.

The critical temperature can be calculated as follows:

T crit 2 --------- – --------------T gas ( γ + 1 ) where

T gas is the temperature of outflowing gas.

Initial Metric Method for Airbags If the reference configuration of the airbag is taken as the folded configuration, the geometrical accuracy of the deployed bag will be affected by both the stretching and the compression of elements during the folding process. Such element distortions are very difficult to avoid in a folded bag. By reading in a reference configuration such as the final unstretched configuration of a deployed bag, any distortions in the initial geometry of the folded bag will have no effect on the final geometry of the inflated bag. This is because the stresses depend only on the deformation gradient matrix:

∂ xi F ij = -------∂ Xj where the choice of

X j may coincide with the folded or unfold configurations. It is this unfolded

configuration which may be specified here. Note that a reference geometry which is smaller than the initial airbag geometry will not induce initial tensile stresses. If a liner is included and the LNRC parameter set to 1 in MATD034, compression is disabled in the liner until the reference geometry is reached; i.e., the fabric element becomes tensile.

Heat Transfer in Airbags For airbags with high temperature, energy is exchanged with the environment. There are two ways to define heat transfer in airbags, convection (CONVECT) and radiation (RADIATE). The heat-transfer rates due to convection and radiation are defined by: 1. Convection:

q conv – h ( t ) A ( T – T env )

Airbag and Occupant Safety 203 Airbag Definition

where h ( t ) is the time-dependent heat transfer coefficient, A is the (sub)surface area for heat transfer, T is the temperature inside the airbag, and T env is the environment temperature. 2. Radiation: A ] q rad = eAs [ T A – T env

where e is the gas emissivity, A is the (sub)surface area for heat transfer, inside the airbag, and T env is the environment temperature.

T is the temperature

204 Seatbelts

Seatbelts Belt elements are single degree of freedom elements connecting two nodes. When the strain in an element is positive (i.e. the current length is greater then the unstretched length), a tension force is calculated from the material characteristics and is applied along the current axis of the element to oppose further stretching. The unstretched length of the belt is taken as the initial distance between the two nodes defining the position of the element plus the initial slack length. Seatbelt shell elements must be used with caution. The seatbelt shells distribute the loading on the surface of the dummy more realistically than the two node belt elements. For the seatbelt shells to work with sliprings and retractors it is necessary to use a logically regular mesh of quadrilateral elements. Slipring

Retractor

Top View: RN5

SN5

RE4 RN4

SRE14

SRE24

SN4

RE3 RN3

SRE13

SRE23

SN3

RE2

SRE12

RE1

SRE11

RN2

SRE22

SN2

SRE21

RN1 SN1

Figure 6-3

Seatbelt Shell Elements Definition

The ordering of the nodes and elements are important for seatbelt shells.

Airbag and Occupant Safety 205 Seatbelts

SEATBELT_PRETENSIONER Pretensioners allow modeling of five types of active devices which tighten the belt during the initial stages of a crash. Types 1 and 5 represent a pyrotechnic device which spins the spool of a retractor, causing the belt to be reeled in. The user defines a pull-in versus time curve which applies once the pretensioner activates. Types 2 and 3 represent preloaded springs or torsion bars which move the buckle when released. The pretensioner is associated with any type of spring element including rotational. Note that when the preloaded spring, locking spring, and any restraints on the motion of the associated nodes are defined in the normal way; the action of the pretensioner is merely to cancel the force in one spring until (or after) it fires. With the second type, the force in the spring element is canceled out until the pretensioner is activated. In this case, the spring in question is normally a stiff, linear spring which acts as a locking mechanism, preventing motion of the seat belt buckle relative to the vehicle. A preloaded spring is defined in parallel with the locking spring. This type avoids the problem of the buckle being free to ‘drift’ before the pretensioner is activated. Type 4, a force type, is described below. To activate the pretensioner, the following sequence of events must occur: 1. Any one of up to four sensors must be triggered. 2. Then a user-defined time delay occurs. 3. Then the pretensioner acts. Type 1 pretensioner is intended to simulate a pyrotechnic retractor. Each retractor has a loading (and optional unloading) curve that describes the force on the belt element as a function of the amount of belt that has been pulled out of the retractor since the retractor locked. The type 1 pretensioner acts as a shift of this retractor load curve. An example will make this clear. Suppose at a particular time that 5mm of belt material has left the retractor. The retractor responds with a force corresponding to 5mm pull-out on it's loading curve. But suppose this retractor has a type 1 pretensioner defined, and, at this instant of time, the pretensioner specifies a pull-in of 20mm. The retractor then responds with a force that corresponds to (5mm + 20mm) on it's loading curve. This results in a much larger force. The effect can be that belt material will be pulled in, but there is no guarantee. The benefit of this implementation is that the force vs. pull-in load curve for the retractor is followed and no unrealistic forces are generated. Still, it may be difficult to produce realistic models using this option, so two new types of pretensioners have been added. These are available in MD Nastran r2 and later versions. Types 2 and 3 are simple triggers for activating or deactivating springs, which then pull on the buckle. No changes have been made to these, and they are not discussed here. The type 4 pretensioner takes a force vs. time curve (see Figure 6-4). Each time step, the retractor computes the desired force without regard to the pretensioner. If the resulting force is less than that specified by the pretensioner load curve, then the pretensioner value is used instead. As time goes on, the pretensioner load curve should drop below the forces generated by the retractor, and the pretensioner is then essentially inactive. This provides for good control of the actual forces, so no unrealistic values are generated. The actual direction and amount of belt movement is unspecified, and depends on the

206 Seatbelts

other forces being exerted on the belt. This is suitable when the force the pretensioner exerts over time is known. Force Retractor Pull-out Force

Defined Force vs. Time Curve Retractor Lock Time

Time

Figure 6-4

Force versus Time Pretensioner. At the intersection, the retractor locks.

The type 5 pretensioner is essentially the same as the old type 1 pretensioner, but with the addition of a force limiting value. The pull-in is given as a function of time, and the belt is drawn into the retractor exactly as desired. However, if at any point the forces generated in the belt exceed the pretensioner force limit, then the pretensioner is deactivated and the retractor takes over. In order to prevent a large discontinuity in the force at this point, the loading curve for the retractor is shifted (in the abscissa) by the amount required to put the current (pull-out, force) on the load curve. For example, suppose the current force is 1000, and the current pull-out is -10 (10mm of belt has been pulled in by the pretensioner). If the retractor would normally generate a force of 1000 after 25mm of belt had been pulled OUT, then the load curve is shifted to the left by 3, and remains that way for the duration of the calculation. So that at the current pull-in of 10, it generates the force normally associated with a pull out of 25. If the belt reaches a pull out of 5, the force is as if it were pulled out 40 (5 + the shift of 35), and so on. This option is included for those who liked the general behavior of the old type 1 pretensioner, but has the added feature of the force limit to prevent unrealistic behavior. The type 6 pretensioner is a variation of the type 4 pretensioner, with features of the type 5 pretensioner. A force vs. time curve is input and the pretensioner force is computed each cycle. The retractor linked to this pretensioner should specify a positive value for PULL, which is the distance the belt pulls out before it locks. As the pretensioner pulls the belt into the retractor, the amount of pull-in is tracked. As the pretensioner force decreases and drops below the belt tension, belt will begin to move back out of the retractor. Once PULL amount of belt has moved out of the retractor (relative to the maximum pull in encountered), the retractor will lock. At this time, the pretensioner is disabled, and the retractor force curve is shifted to match the current belt tension. This shifting is done just like the type 5 pretensioner. It

Airbag and Occupant Safety 207 Seatbelts

is important that a positive value of PULL be specified to prevent premature retractor locking which could occur due to small outward belt movements generated by noise in the simulation. SEATBELT_RETRACTOR The unloading curve should start at zero tension and increase monotonically (i.e., no segments of negative or zero slope). Retractors allow belt material to be paid out into a belt element. Retractors operate in one of two regimes: unlocked when the belt material is paid out, or reeled in under constant tension and locked when a user defined force-pullout relationship applies. The retractor is initially unlocked, and the following sequence of events must occur for it to become locked: 1. 2. 3. 4.

Any one of up to four sensors must be triggered. (The sensors are described below.) Then a user-defined time delay occurs. Then a user-defined length of belt must be paid out (optional). Then the retractor locks and once locked, it remains locked.

In the unlocked regime, the retractor attempts to apply a constant tension to the belt. This feature allows an initial tightening of the belt and takes up any slack whenever it occurs. The tension value is taken from the first point on the force-pullout load curve. The maximum rate of pull out or pull in is given by 0.01 × fed length per time step. Because of this, the constant tension value is not always achieved. In the locked regime, a user-defined curve describes the relationship between the force in the attached element and the amount of belt material paid out. If the tension in the belt subsequently relaxes, a different user-defined curve applies for unloading. The unloading curve is followed until the minimum tension is reached. The curves are defined in terms of initial length of belt. For example, if a belt is marked at 10mm intervals and then wound onto a retractor, and the force required to make each mark emerge from the (locked) retractor is recorded, the curves used for input would be as follows:

0

Minimum tension (should be > zero)

10mm Force to emergence of first mark 20mm Force to emergence of second mark . . .

. . .

Pyrotechnic pretensions may be defined which cause the retractor to pull in the belt at a predetermined rate. This overrides the retractor force-pullout relationship from the moment when the pretensioner activates. If desired, belt elements may be defined which are initially inside the retractor. These will emerge as belt material is paid out, and may return into the retractor if sufficient material is reeled in during unloading.

208 Seatbelts

Elements e2, e3 and e4 are initially inside the retractor, which is paying out material into element e1. When the retractor has fed

L crit into e1, where

L crit = fed length – 1.1 × minimum length (minimum length defined on belt material input) (fed length defined on retractor input) Element e2 emerges with an unstretched length of 1.1∞minimum length ; the unstretched length of element e1 is reduced by the same amount. The force and strain in e1 are unchanged; in e2, they are set equal to those in e1. The retractor now pays out material into e2. If no elements are inside the retractor, e2 can continue to extend as more material is fed into it. As the retractor pulls in the belt (for example, during initial tightening), if the unstretched length of the mouth element becomes less than the minimum length, the element is taken into the retractor. To define a retractor, the user enters the retractor node, the ‘mouth’ element (into which belt material will be fed), e1 in Figure 6-5, up to 4 sensors which can trigger unlocking, a time delay, a payout delay (optional), load and unload curve numbers, and the fed length. The retractor node is typically part of the vehicle structure; belt elements should not be connected to this node directly, but any other feature can be attached including rigid bodies. The mouth element should have a node coincident with the retractor but should not be inside the retractor. The fed length would typically be set either to a typical element initial length, for the distance between painted marks on a real belt for comparisons with high speed film. The fed length should be at least three times the minimum length. If there are elements initially inside the retractor (e2, e3 and e4 in the Figure 6-5) they should not be referred to on the retractor input, but the retractor should be identified on the element input for these elements. Their nodes should all be coincident with the retractor node and should not be restrained or constrained. Initial slack will automatically be set to 1.1 × minimum length for these elements; this overrides any user-defined value.

Airbag and Occupant Safety 209 Seatbelts

Weblockers can be included within the retractor representation simply by entering a ‘locking up’ characteristic in the force pullout curve (see Figure 6-6. The final section can be very steep (but must have a finite slope).

Element 1

Before Element 1 Element 2

Element 3 Element 2 Element 4

After

Element 3 Element 4 All nodes within this area are coincident

210 Seatbelts

Figure 6-5

Elements in a Retractor with weblockers

FORCE

without weblockers

PULLOUT

Figure 6-6

Retractor Force Pull Characteristics

SEATBELT_SENSOR Sensors are used to trigger locking of retractors and activate pretensioners. Four types of sensors are available which trigger according to the following criteria:

Type 1 – When the magnitude of x-, y-, or z- acceleration of a given node has remained above a given level continuously for a given time, the sensor triggers. This does not work with nodes on rigid bodies. Type 2 – When the rate of belt payout from a given retractor has remained above a given level continuously for a given time, the sensor triggers. Type 3 – The sensor triggers at a given time. Type 4 – The sensor triggers when the distance between two nodes exceeds a given maximum or becomes less than a given minimum. This type of sensor is intended for use with an explicit mass/spring representation of the sensor mechanism. By default, the sensors are inactive during dynamic relaxation. This allows initial tightening of the belt and positioning of the occupant on the seat without locking the retractor or firing any pretensioners. However, a flag can be set in the sensor input to make the sensors active during the dynamic relaxation phase. SEATBELT_SLIPRING Sliprings allow continuous sliding of a belt through a sharp change of angle. Two elements (1 & 2 in Figure 6-7) meet at the slipring. Node B in the belt material remains attached to the slipring node, but belt material (in the form of unstretched length) is passed from element 1 to element 2 to achieve slip. The amount of slip at each timestep is calculated from the ratio of forces in elements 1 and 2. The ratio of forces is determined by the relative angle between elements 1 and 2 and the coefficient of friction,

μ.

Airbag and Occupant Safety 211 Seatbelts

The tension in the belts are taken as T 1 and T 2 , where T 2 is on the high tension side and T1 is the force on the low tension side. Thus, if sufficient to reduce the ratio

T 2 is sufficiently close to T 1 , no slip occurs; otherwise, slip is just

T 2 ⁄ T 1 to e μΘ . No slip occurs if both elements are slack. The out-of-

balance force at node B is reacted on the slipring node; the motion of node B follows that of slipring node. If, due to slip through the slipring, the unstretched length of an element becomes less than the minimum length (as entered on the belt material card), the belt is remeshed locally: the short element passes through the slipring and reappears on the other side (see Figure 6-7). The new unstretched length of e1 is

1.1 × minimum length . Force and strain in e2 and e3 are unchanged; force and strain in e1 are now equal to those in e2. Subsequent slip will pass material from e3 to e1. This process can continue with several elements passing in turn through the slipring. To define a slipring, the user identifies the two belt elements which meet at the slipring, the friction coefficient, and the slipring node. The two elements must have a common node coincident with the slipring node. No attempt should be made to restrain or constrain the common node for its motion will automatically be constrained to follow the slipring node. Typically, the slipring node is part of the vehicle body structure and, therefore, belt elements should not be connected to this node directly, but any other feature can be attached, including rigid bodies.

Slipring B Element 2 Element 1

Element 1 Element 3 Element 2

Element 3

Before Figure 6-7

After

Elements Passing Through Slipring

212 Occupant Dummy Models

Occupant Dummy Models The occupant dummy models, also known as ATDs (Anthropomorphic Test Devices) were introduced in the previous release of SOL 700 for those applications that airbag was not needed. Many applications such as sled test and aircraft seat design, or armored vehicle design where the occupant behavior is studied when a land mine is detonated do not require airbag simulation. SOL 700 supports occupant dummies that are readily available in LS-DYNA *key file format. These include: 1. LS-DYNA public domain dummies: • 5th percentile deformable female dummy • 50th percentile deformable male dummy • 95th percentile deformable male dummy • 5th percentile rigid female dummy • 50th percentile rigid male dummy • 95th percentile rigid male dummy

2. FTSS (First Technology Safety Systems) ATDs. The FTSS ATD’s are high fidelity dummies and are available with additional licensing. The following FTSS dummies are supported through SimX Crash or ETA – VPG: • • • • •

5% Female dummy SID II Hybrid III - 3% Child Dummy (W.I.P.) Hybrid III - 6% Child Dummy (W.I.P.) BIOSID (W.I.P.)

Simulation 213

Simulation

214 Perform the Simulation

Perform the Simulation Create an Analysis job You set up and submit the analysis of your model by expanding Analysis from the ModelBrowser tree, then right click Nastran Jobs, and select Create new Job. The Job Name you type in the textbox will become the filename for all analysis files created from this execution. Select Explicit Nonlinear (SOL 700) as the Solution Type. You have 5 choices for Job Type: 1. Export Bdf and Run Solver - writes the model including all model data, all load case information, analysis type, and analysis parameters to an analysis-ready file called job name.bdf, then runs the solver. 1. Export an Analysis Deck only - writes your model including all model data, all load case information, analysis type, and analysis parameters to an analysis-ready file called job name.bdf. 1. Export the Model only - writes your model data: nodes, elements, coordinate frames, element properties, material properties, and loads and boundary conditions without any analysis parameters to a file called job name.bdf. 2. Run a Model Check - analysis is submitted but will exit after initial model assembly. No solution is generated. 3. Submit Job to Batch Queue - allows submittal of multiple models to be analyzed sequentially with a single analysis request. Case Control Section The Case Control commands are used to • Define subcases (e.g., loading and boundary conditions). • Make selections of loads, constraints, etc. • Specify output requests. • Define titles, subtitles and labels for documenting the analysis.

Common subcase Common subcase defines the master output requests for your analysis. Output requested in the common case will become the default for all subcases. The software will write all of these requests and conditions to the Case Control section. In addition, you can define cases which let you perform multiple analyses with different load and/or constraint sets. Create Subcase The subcase dialog box lets you select the loads and constraints to apply to your analysis.You can apply boundary conditions as both the common level or in subcases. If your analysis requires multiple load or constraint sets, you must create subcases. MPCs: pick a constraint set to define constraint equations.

Simulation 215 Perform the Simulation

Output Requests Use the Output Requests dialog box to identify the types of output that you want from the analysis. You can select to output any combination of the results shown on the following form: Solution Parameters Here you can specify Solution Parameters such as whether or not to include Large Displacements, Follower Forces, etc. .

216 Perform the Simulation

Subcase Parameters Here you specify Subcase Parameters such as Ending Time for the simulation, Number of Time Steps.

Simulation 217 Perform the Simulation

Output File The purpose of this section is to introduce the output file generated by a typical run. After an input file is submitted for execution, several output files may be generated.

218 Results

Results If you submitted your analysis directly from SimXpert, the results will be attached upon job completion. If your analysis ran externally to SimXpert but you have the model in SimXpert, select Attach Results from the File menu and navigate to your results file. If your analysis ran externally to SimXpert and you do not have the model in SimXpert, select Import Results from the File menu and navigate to your results file. This will read in model information as well as results from the results file. Output data is also stored in Result Cases. If you run your model with several different loading conditions or through several different analysis types, SimXpert will keep the output data from each analysis in a different Result Case. Postprocessing can be divided into two main categories: Chart and State Plot. State Plot postprocessing can be further divided into the following types of plots: 1. Deformation Can be displayed in any available render style. You can turn the display of the undeformed shape on or off as desired. 2. Fringe Color code your model based on result value 3. Vector Show vectors representing direction and magnitude of result value. All plot types can be animated. You can animate a single result case by applying a progressive scale factor to the deformation result or you can animate over a selection of result sets. All plot types can be displayed together in the same window if desired. State Plots The State Plot properties form is the main control for postprocessing. It is from here you can control which result set is being displayed, how your model is displayed and select your desired postprocessing options. You can use dynamic rotation to manipulate your model while results are displayed and also during animation. • How to Select the Data used for postprocessing

The state plot properties form is accessed by clicking on the Results toolbox and selecting State Plot. To choose the data used in the display, in the Results Cases list click the desired Result Case (A in figure), then click the Results Type to use (B), and, if desired, you can make selections for Derivation and Target Entities. You can limit the Results Cases listed using the Filter text box. If you are animating multiple Results Cases, simply select all desired cases in the Results Cases list. • Deformed Shape Plots

The following are some of the options control the appearance of your deformed shape plot:

Simulation 219 Results

1. Deformed display scaling - True: applies the related scale factor to the actual computed values for displacement To see a plot of your actual displacement set the scale factor to 1. Relative: applies the scale factor to display the maximum displacement as a percentage of your maximum model dimension. This is usually an exaggerated plot for ease in visualization. 2. Deformed Shape - controls rendering for Deformed shape display. 3. Undeformed Shape - can display or remove the undeformed model, as well as control how it is Contour Style View Options • Fringe Plots

The Fringe tab allows access to data transforms. These options are very important to understand since they control how the data is converted from pure discrete numbers to a visual representation. Improper selection of data transforms can lead to erroneous interpretation of the results. You can specify which domain in the model to use for result averaging in order to obtain an accurate representation of the results. The following domains are available: 1. Property - results will not be averaged across property boundaries 2. Material - results will not be averaged across material boundaries 3. All Entities - results will be averaged at all common nodes 4. Target Entities - results will be averaged only between the elements selected as the target entities 5. Element Type - results will not be averaged across boundaries between different types of elements 6. None - no averaging of results between any elements. Fringe values are based on individual element results only. When the averaging domain is set to anything other than All Entities the resulting graphics may not be as smooth but this is a more accurate representation of the results when discontinuities exist in the structure. You can compare the difference between using an averaging domain of None to one of the other averaged domains to assess your mesh quality. If there is a large difference in the maximum result these between the two fringe plots, especially at locations that do not have sharp corners or breaks in the model, the mesh may need to be refined in that area. The Result averaging method controls how SimXpert converts the results from pure data at element centroids, corners, and nodes to the actual continuous graphical representation. The following methods are available. 1. Derive/Average - calculates the selected result value first then applies a simple average of all the contributing nodes. 2. Average/Derive - averages the contributions of the common nodes then derives the result 3. Difference - computes the minimum and maximum results for the elements sharing a common node. The difference between the maximum and minimum contributor to each node is plotted. The fringe plot of this difference is an indicator of mesh quality: result differences between neighboring elements should not be large. If large discontinuities are found the mesh should be refined in that area. Nodal results will have zero max-difference.

220 Results

4. Sum - Sums the result values of all contributing nodes. No averaging. • Fringe attributes

Style allows you to choose between 1. Discrete - Each range on the spectrum is given a unique color block 2. Continuous Colors - The model is displayed with smooth transitions between each color 3. Element Fill - Elements are displayed with one solid color • Vector Plots

Vector attributes - allows you to choose whether to scale vector lengths are adjusted, and how the vectors are color coded. • Animation

Animation attributes- controls number of frames, delay, and type of scale factor used to generate the animation (Sinusoid, Linear, etc.) Chart Plots SimXpert can create XY plots of results. Control over the contents of a chart is provided by the chart properties form. The chart properties form is accessed by clicking on the Results toolbox and selecting Chart. It allows you to control the Results Cases and Results Type shown on the XY data plots. Choose the Results Cases and the Results Type from the appropriate list boxes. You can limit the Results Cases you see in the list box by using the Filter button.The Chart Properties form controls whether an XY plot is displayed, and what type of chart to display.

Example 221

Example

Impact of a tapered beam

222 Impact of a Tapered Beam

Impact of a Tapered Beam Problem Statement Simulate the impacting of a square cross section solid, tapered beam with a rigid wall. The impacting is to be simulated by moving the beam with an initial velocity toward wall, while the other end is free. The basic FEA model containing the nodes and the elements is imported from a nastran input file. Complete the model with materials, sections, boundary conditions, loads, and analysis options for performing the simulation. Beam Dimensions: Length: 40 in. Cross Section: 2 in. square at one end, and 4 in. square at the other end. Plate Dimensions: 6 in. X 6 in. ; Thickness: 0.60 Impact velocity = 7,200 in./sec Material Properties E = 30.E6 psi ν = 0.3 ρ = 7.33E-4 lb-mass/in^3 σy = 58.E3 psi ET = 29.E3 psi Steps Following are the steps to complete the impact model. 1. Launch SimXpert Select MD Explicit as the Workspace 2. Turn off the Solver Card GUI Option Tools -> Options -> GUI Options Make sure the Solver Card is not checked in Click Apply 3. Set the units for the model Clik Units Manager

223 Impact of a Tapered Beam

Click Standard Units Select in, lb, s as the units for Length, Mass, and Time respectively Click OK (twice) 4. Import the FEA mesh from a .Nastran input file File -> Import -> Nastran Select the file tapered_beam_model.bdf Hint:

You can find the above file in the PartFiles folder under the help folder in the SimXpert installation directory. Click Open Close the (pop-up) nastran.err Notepad window The imported FEA mesh as shown here represents the beam and the rigid wall.

Figure 8-1

The Tapered Beam Impacting a Rigid Wall

224 Impact of a Tapered Beam

5. Create the material. Materials and Properties-> MAT [21 to 40] -> [024]MAT_PIECEWISE_LINEAR_PLASTICITY Enter steel as the Title for the material Enter value for RO: 7.33E-4 Enter value for E: 30.E6 Enter value for PR: 0.30 Enter value for SIGY: 58.E3 Enter value for ETAN: 29.E3 Click Create 6. Modify the element properties for the shell elements From the Model Browser, Double Click on PSHELL_2... (under Property) Click on the Material ID selection icon, and Click Select Select steel, and Click Ok Click on the Bending Material ID icon, and Click Select Select steel, and Click Ok Click on the Transverse Shear Material ID icon, and Click Select Select steel, and Click Ok Click Modify 7. Modify the element properties for the solid elements From the Model Browser, Double Click on PSOLID_1... (under Property) Click on the MID selection icon, and Click Select Select steel, and Click Ok Click Modify

225 Impact of a Tapered Beam

8. Create the Boundary conditions for the rigid plate LBCs -> LBC -> SPC BC -> Fully Fixed Constraint Pick all the nodes on the plate Click Done on the Pick panel This fixes the plate against all translations and rotations, essentially making it a rigid plate.

Figure 8-2

Boundary condition for the rigid plate

9. Create the Initial Velocity on the beam nodes LBCs -> LBC -> Nodal BC -> Initial Transient Condition Enter 7200 for ZVEL Click Define App Region Pick all the nodes on the beam Click Create 10. Create Contact for the Beam Elements CONTACT -> Deformable Body Select Deformable Solid as Type Type beam for Name Select all the beam elements Click OK 11. Create Contact for the Plate Elements

226 Impact of a Tapered Beam

CONTACT -> Deformable Body Select Deformable Surface as Type Type plate for Name Select all the plate elements Click OK 12. Create an analysis job Model Browser: Right Click on tapered_beam_model.bdf Select Create new Nastran Job Enter name for the Job Name: tapered_beam Click OK 13. Create the analysis parameters for the job Right Click on Loadcase Control-> Properties Enter 0.005 for Ending Time Enter 100 for Number of Time Steps Click Apply Click Close 14. Specify the time step for d3plot and time hstory output Job Parameters -> PARAM Enter DYDTOUT for N1 Enter 0.0001 for V1 Enter STEPFCTL for N1 Enter 0.1 for V1 Click Create Click Exit 15. Specify output requests Right-Click on Output Requests Click Add Velocity Output Request Click OK

227 Impact of a Tapered Beam

16. Save the SimXpert database File -> Save As Enter name for the file: tapered_beam Click Save 17. Export an MD Explicit Analysis Input File Right Click on tapered_beam Click Export Enter tapered_beam for File name Click Save 18. Submit the exported input file tapered_beam.bdf for analysis by MD Nastran. Open MD Nastran Select the input file: tapered_beam.bdf Click Open Click Run 19. Attach the Analysis Results (after the spawned MD Nastran job is completed) File -> Attach Results Select Results Click the File Path icon Select the result file: tapered_beam.dytr.d3plot Click Open Click OK 20. View the Simulation Results Results -> Fringe Result Cases: Select Time 0.005 (the last result case) Result type: Stress, Components Derivation: Von Mises Click Update

228 Impact of a Tapered Beam