Simxpert R3.2 Modeling Guide

CHAPTER 1 Introduction

Modeling Guide Introduction

2 Modeling Guide

Overview of Model Generation This document gives a general overview of the steps used to create a finite element analysis model. For detailed information on commands, refer to the SimXpert Quick Reference. You may also refer to the Example Problems or Workspace Guides for sample problems with step by step instructions.

CHAPTER 1 Model Generation

Model Generation

2 Modeling Guide

Geometry Overview Geometry for FEA is created for the purpose of describing the physical shape of the model to be analyzed. It forms the base upon which the finite element mesh will be created. Geometry can be created in SimXpert, imported from CAD, or directly accessed from CAD files with a live link to the CAD code.

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 Options Editor in the Tools menu. If you import a file that contains units, SimXpert will convert them into those specified in the Units Manager.

Create Point In addition to Geometric points , vertices on curves, surfaces, and solids are also considered points. You can also create Mesh Control Points which mark locations where nodes will be placed when meshing is performed. Points can be suppressed so that a node will not be forced to be placed at that location when meshing.

CHAPTER 3 Model Generation

Elements and Meshing This section describes the different element types supported in SimXpert, as well as the procedures used to create these elements. Check your Workspace Guide to determine which elements are supported for your analysis type.

Element Types There are four basic element groups in SimXpert: scalar (0-D), line (1-D), surface (2-D), and solid (3D) elements. There are also a number of specialty elements. A list of the elements currently supported by SimXpert, including a brief description of each, follows. Scalar (0D) Elements • Concentrated Mass - Three

dimensional mass and/or inertia element located at a node. Used to represent parts of a structure which contain mass but do not add stiffness.

• Spring - Used to provide a specified stiffness between a nodal degree of freedom and ground. • Damper - Used to provide viscous damping between a nodal degree of freedom and ground.

Line (1D) Elements • Bar - Uniaxial element with tension, compression, torsion and bending. Used to model general beam/frame structures for linear analysis. • Beam - Uniaxial element with tension, compression, torsion and bending. It can be tapered and

have different properties along its axis. The shear center can be offset from the neutral axis. Used to model both linear and nonlinear beam/frame structures and beams with open sections. • Curved Beam or Pipe - Curved beam, pipe, or elbow element with an arc for the neutral axis.

Useful for modeling piping systems. • Bushing - Vibration control device that has impedance values (stiffness and damping) that are

frequency dependent. Recommended as a replacement for spring elements. • Damper - Used to provide viscous damping between two selected degrees-of freedom or

between one degree-of-freedom and ground. • Spring - Used to provide a specified stiffness between two selected degrees of freedom. Other

properties can include a damping coefficient and a stress coefficient to be used in stress recovery. It is recommended to create this element between two coincident nodes. • Gap - Nonlinear element with different tension, compression and shear stiffness. Used to

represent surfaces or points which can separate, close or slide relative to each other. • Scalar Mass - Useful for the selective representation of inertia properties, such as occurs when a

concentrated mass is effectively isolated for motion in one direction only. • Rod - Uniaxial element with tension, compression and torsional stiffness. No bending or shear.

Typically used to model trusses.

4 Modeling Guide

• Tube - Rod element with tubular cross section. Often used to model pipes. • Plot Only - Nonstructural element used to represent structural features that are not being

analyzed but aid in the visualization of the model. Surface (2D) Elements • Plate/Shell - Two dimensional plate or shell element used to represent any three dimensional structure. Resists membrane, shear and bending forces. Used to model structures comprised of thin plate shells. • Tria - Three or six noded element (linear or quadratic element, respectively). • Quad - Four or eight noded element (linear or quadratic element, respectively). • Cohesive - Four or eight noded element used to simulate the process of delamination (linear

or quadratic element, respectively). • Axisymmetric - (Three or six) or (four or eight) noded element. The element can be linear or

fully nonlinear. Also, the element can be cohesive, for which it is either four or eight noded (linear or quadratic element, respectively). • Shear Panel - Resists only shear forces. Used to model structures which contain very thin elastic

sheets, typically supported by stiffeners. This is a four noded element. • Acoustic Absorber - Defines a frequency -dependent acoustic absorber element. Used in coupled

fluid - structural analysis. Solid (3D) Elements • Solid - Three dimensional solid element used to represent any three dimensional structure. Specialty Elements • Rigid - Include both rigid and interpolation elements. General use rigid elements consist of RBAR, RROD, RBE2, RBE1, and RSSCON. Of these elements, the RBAR and RBE2 are the most commonly used. Interpolation elements consist of the RBE3 and RSPLINE. The RBE3 is a linear interpolation element often used to distribute either loading or mass. The RSPLINE is often used to model mesh transitions. • Weld - General purpose connector element which can connect non congruent meshes. Used in

linear analysis. • Contact - Used to identify bodies which are potential candidates for contact during analysis.

Bodies can be rigid or deformable. Self contact is also permitted FAQs 1. Why Should I Use Coincident Nodes for Spring Elements? In 1-D elements such as a bar, a positive axial force or stress indicates that the member is in tension. This is not the case for scalar elements. Since the scalar elements do not have any geometry, the sign of the output force or stress does not necessarily indicate compression or tension in the spring. The force in the spring is recovered as follows:

CHAPTER 5 Model Generation

F = K ( U1 – U2 ) Simply by reversing the order of the endpoints of the spring the sign of the force and stress output for these elements reverse. For example, consider the spring shown in Figure 1 where D1 and D2 are scalar displacements. Before Deformation D1

D2

1

1

2

After Deformation

Figure 1

Spring – Before and After Deformation

For D2 > D1, If the spring is defined from node 1 to node 2 the axial force would be negative. If the spring is defined from node 2 to node 1 the axial force would be positive. Whenever a spring element is connected across two nodes, it is good modeling practice to make sure that the nodes are coincident and use the same output coordinate system. If the nodes are not coincident, a difference in displacement may be caused by a rigid body rotation. This situation causes forces in the spring and a net moment on the structure. This condition is an example of an internal constraint, which is allowed because it is valid for some types of modeling. Unless it is desired to have these internal constraints, use coincident nodes. Since the length of the spring is zero when coincident nodes are used, no internal moments are created. Also, the spring’s degrees of freedom are in the output coordinate system. 2. Why is a bushing recommended as a replacement for spring elements? As discussed in the previous question, if spring elements are used and the geometry is not aligned properly, internal constraints may be induced. Bushing elements have all the features of the spring elements without the drawback of the potential internal constraint. Furthermore, since a spring element needs to be defined for each connected degree of freedom, several spring elements can be reduced to a single bushing element.

2

6 Modeling Guide

Control of Mesh Size and Why Mesh sizes can be set interactively using Seed in the Automesh group under the Meshing tab. It is possible to specify a default mesh size for surfaces, or the size of an element at a vertex. For curves there are several options for creating mesh seeds; they are, 1) uniform, 2) one way bias, 3) two way bias, 4) curvature based, and 5) tabular. • Uniform -- causes elements to be distributed evenly along a curve. • One Way Bias -- specifies the mesh sizing for a given curve with an increasing or decreasing

element edge length. • Two Way Bias -- specifies the mesh sizing for a given curve with symmetric non-uniform

element edge lengths. • Curvature Based -- specifies the mesh sizing for a given curve with the element edge length

controlled by curvature of the curve. • Tabular -- for specifying either parametric locations (place seeds at parametric locations of the

curve), arc length ratio locations (place seeds at arc length ratio locations of the curve arc), or node/point locations (place seeds at the location of selected nodes or points) for mesh seeds. A mesh seed consists of two adjacent control points. While meshing to create linear finite elements, a mesh seed defines a single element edge -- the two control points cause the creation of two finite element nodes at opposite ends of the element edge. When meshing to create parabolic finite elements (elements with mid-side nodes), two mesh seeds are used to define one element edge. A example of this is when there are ten mesh seeds on an edge of a geometric solid (cube), and parabolic tetrahedral elements are created by meshing, five elements are created along the solid edge where the mesh seeds are.

CHAPTER 7 Model Generation

In addition it is possible to define mesh control points on curves or surfaces to ensure that a node is placed at that location. This is done using the FEM Tool Control > Points/Curves in the Misc group under the Meshing tab. Mesh should have high density in areas of large stress gradients. Nodes along common edges of adjoining geometry entities may need to match. If these nodes are not coincident, equivalencing nodes will not cause all of the adjacent elements to become connected. If the adjacent elements are not connected, the model will have free edges or free faces at these locations. For a linear analysis, always merge coincident nodes before analyzing the model using Equivalence in the Modify group under the Nodes/Elements tab.

Element Creation In SimXpert you can use a number of methods to create elements: Automesh • Mesh Geometry - used to create a set of elements on curves, surfaces, or solids.

8 Modeling Guide

• Curves: a geometric curve is defined parametrically (one parameter). The meshing is done in

parametric space using 1D elements. • Surfaces: a geometric surface is defined either parametrically or non-parametrically. The

mesher either follows the parametric directions (surface defined parametrically), or initially follows the perimiter of the surface, subsequently meshing inward following the inner most perimiter defined by the created element edges (surface defined non-parametrically). • Solids: controls automatic meshing of solid geometry or volumes (in space). The meshing can

be tetrahedral, or by sweeping, it can be hexahedral. Tetrahedral meshing is for a geometric solid or a set of contiguous tria elements that completely enclose a volume. The meshing is done, for a solid, by surface meshing its faces with tria elements, then creating one layer of tetrahedral elements that are congruent to the tria elements. Then, another layer of tetrahedral elements is created that is congruent to the first layer of tetrahedral elements. This is continued until the solid is filled with tetrahedral elements. The meshing for a set of contiguous tria elements is similar to that for a geometric solid, but the mesher begins with the set of tria elements. Hexahedral meshing is for a geometric solid, where the meshing is done by sweeping a set of 2D quadrilateral elements from one solid face (“starting” face) to the opposing face (“ending” face). This means that the solid must be sweepable, or 2 1/2/ D. The starting and ending face (opposing faces), are connected with a set of four edged faces (linking faces). Each of the four edged faces must have two of its opposing edges congruent with an edge of the “starting” or “ending” face. The mesher creates on one of the opposing faces a 2D quadrilateral element mesh, then sweeps it to the other opposing face, creating a hexahedral element mesh between the opposing faces. • Non-geometry meshing commands. • Skin - creates shell elements on the free faces of 3D solid elements • 2-3-4 line mesh - produces mesh between curves • 3-4 Point mesh - produces mesh between virtual curves created by selecting end points • On Mesh - used to modify an existing mesh. Useful for fixing or "cleaning-up" a distorted area

of a mesh Create elements one at a time. Useful for simple models, line elements, and to fix areas of distorted elements. Copy existing elements using the Transform option of the Tools menu. • Project elements onto plane, mesh, curve, surface • Reflect (mirror) elements through a plane. • Reorient - Move elements with respect to coordinate systems • Scale - Create a scaled copy of the elements around a given location. • Rotate - Move elements a specified angle • Translate - Move elements a specified distance

Sweep Shells into Solids or Node pairs into Quads using the FEM based group under the Meshing tab.

CHAPTER 9 Model Generation

• Revolve - Revolve around a vector • Extrude - Drag along a vector • Glide - Drag along a curve • Loft - Create linear mesh between destination and source elements • Normal - Drag elements along normals • Flange on Mesh - Drag node pairs along a specified angle.

Surface Meshing Guidelines Examine your model before you begin the meshing process to determine which method of mesh generation is most applicable. The items below provide some guidelines for meshing surfaces. • For Surface from Automesh under the Meshing tab, there are several methods of meshing . • Auto Decide -- meshes the surface(s) and uses the meshing algorithm which gives the best

quality elements. • Paver -- the mesh will be a paved mesh. The paving algorithm creates elements around any

edges and boundaries of the surface first, then fills with elements in the interior of the surface, and finally smooths the mesh. • Mapped -- the mesh will be a mapped (iso) mesh. Elements are created in ‘rows’. • Minimal -- using this will cause the creation of the smallest surface mesh (fewest number of

2D elements) possible, considering adjacent meshes and mesh seeds. Only one surface can be meshed at a time for this option. Currently (R3.2), minimal meshing only works with CATIA geometry (surfaces and curves). • Most meshes involve creating geometry first. If you have small features in your geometry that

are not critical to the analysis, you can suppress them in SimXpert. • You can use the FEM Based meshing Revolve / Extrude / Glide commands to generate Surface

elements from node pairs. • Utilize symmetry whenever possible to reduce model size. Model size (and therefore run time)

is significantly reduced if the loading/constraints are also symmetrical. If loads/constraints are not symmetrical, you can use the Tools > Transform > Reflect command to mirror the mesh through a plane • Remember, you may also want to use Translate from the Element group of the Nodes/Elements

tab or one of the commands under Tools > Transform to replicate elements instead of performing more surface or boundary meshing • Use the Equivalence command in the Modify group of the Nodes/Elements tab to merge

coincident nodes and connect the meshes • Use the View, Highlight FE Boundary command to verify that you do not have any unwanted

free edges in the model.

10 Modeling Guide

Solid Meshing Guidelines • Often you can avoid using volumes or solids by extruding or revolving planar elements to create

solid elements. If your part has a consistent third dimension, use one of the Fem based sweep methods under the Meshing tab to create solid elements. • Use Skin from the Automesh group if planar elements are required on faces of solid elements.

Once the solid elements are created, planar elements can be created by skinning. • If you have solid models with holes or other complicated features, use the solid mesher. This

mesher creates a surface mesh first, so all items applicable to surface meshing apply. You can associate a property with the mesh as it is being created. Properties can also be assigned to parts or to parent geometry.

Minimal Meshing As previously mentioned, if minimal meshing is performed the smallest surface mesh (fewest number of 2D elements) will be created for the surface (only one surface can be meshed at a time for this option.). The mesh created will be congruent to adjacent meshes and mesh seeds. Also, it is possible to simultaneously mesh curves on the perimeter, and interior to the perimeter, of the surface that is being minimally meshed. For this to occur, it is necessary to associate the curves to the surface. The meshes created for associated curves will be congruent to the mesh created for the surface. These two things are requested using the surface meshing form, Surface from Automesh under the Meshing tab. • Curve minimal meshing -- specify what type of curves (curves at the perimeter of the surface and

hard curves internal to the perimeter) are to be meshed. • None -- No curves will be meshed. Only the surface will be meshed, and it will be meshed

minimally. • Boundary curves -- curves at the perimeter of the surface are meshed to be congruent with

the surface mesh that is created. • Boundary curves + hard curves -- curves at the perimeter of the surface and the hard curves

internal to the perimeter are meshed to be congruent with the surface mesh that is created. • Hard curve association -- specify how the curves will be selected for association to the surface. • None -- do not associate any curves to the surface. Any already associated curves will be

recognized (used) by the surface mesher. • Auto -- automatically associate curves on the surface (if the distance between a curve and

the surface is < the tolerance, the curve is considered as being on the surface) to the surface. • Selected -- set the form for selecting what curves are to be associated to the surface. • Curves to mesh -- select the curves the are to be associated to the surface.

Normally, a surface to be minimal meshed is 4-sided without any holes.

CHAPTER 11 Model Generation

For hard curves, they need to divide the surface being meshed into a number of patch shapes. Each patch shape should be a 3 or 4 sided region. If seeds or existing nodes are defined for the hard curves, the numbers of seeds or nodes on the opposite sides of each patch should be equal. A node will be created at the intersection of two hard curves. There can be problems if the two ends of a hard curve do not touch the perimeter of the surface -- the ends of a hard curve are outside or inside of the surface perimeter. Currently (R3.2), minimal meshing only works with CATIA geometry -- all the surfaces and curves being minimally meshed must be of CATIA type. A typical scenario is for the aerospace industry, that involves meshing a fuselage or wing model. Here, a single (large) surface represents the entire top skin of the wing. Similarly, a single surface represents the entire bottom skin of the wing. Between the two skins are individual ribs and spars (represented by curves) that act as stiffeners. When meshing the top or bottom surface (skin) of the wing, usually it is desired to have only a single element span the surface (skin) between the stiffener locations (at each skin and rib, or skin and spar sections). In such cases, it is important that only one element be generated on the surface (skin) between the stiffeners. The minimal mesh option satisfies this requirement. Users want to create a minimal mesh on a model with a single tool and the least possible number of picking and selecting.

Element Shape Quality Once you have created a surface mesh, check the elements using the Element Fringes icon on the Element Render toolbar. You can set maximum distortion criteria using Check Quality in the Checks group under the Quality tab. Fix all distorted elements if possible before adding any loads or constraints. This is especially important if the distorted elements are in a critical region of the model.

Improve Quality by Parts This method improves the quality of elements associated with selected parts. Use Repair in the Edit group under the Meshing tab. The parameters that are used are • Pick Parts: Select Parts whose elements are to be considered for remeshing.. • Remesh Poor Quality Elements: if checked, the elements with poor quality will be replaced. • Remesh Triangles: if checked, the current triangular elements are to be replaced either by quad

elements if possible, or by better quality tria elements. • Remesh Hole Rings: if checked, the elements around holes are replaced by better quality

elements. • Remesh Distance: used to specify the size of the region for remeshing. • Feature Angle: if mesh feature angles are greater than this specified angle the original mesh

features are preserved..

12 Modeling Guide

Auto Geometry Cleanup The Auto cleanup command in the Misc group under the Meshing tab is used to suppress curves at the interface between two adjacent surfaces. The curves are suppressed so the surface mesher will not automatically create nodes along them. The surfaces must be three or four sided. The parameters that are used are: • Surfaces: select surfaces, some of whose curves are to be suppressed. • Element Size: specify the size of the finite elements that are to be created during meshing. • Surface cross section length tolerance: for two congruent, adjacent surfaces, each with 4 edges,

SimXpert will determine the smallest edge length for the four edges emanating from the interface, L. If L is less than the specified tolerance, the curve along the interface of the two surfaces will be suppressed. • Small surface area tolerance: For two congruent, adjacent surfaces, each with 4 edges, SimXpert

will determine the area of both surfaces. The smallest area, S, will be determined. If S is less than the specified tolerance, the curve along the interface of the two surfaces will be suppressed. • Short curve length tolerance: If the length of curves associated to the selected surfaces is less

than the specified tolerance, they will be suppressed. • Small angle tolerance: for each surface in the list, SimXpert will determine the smallest interior

angle, A. If A is less than the specified tolerance, the shortest edge at the vertex of each angle will be suppressed. • Break Angle: for two congruent, adjacent surfaces, each with 4 edges, SimXpert will determine

the intersection angle, A. If A is less than the specified Break Angle, the curve along the interface of the two surfaces will be suppressed.

Lock / Unlock The Control > Lock / Unlock command in the Misc group under the Meshing tab is used to prevent geometric edges/curves from being modified. For example, if a curve is locked then selected for suppression, it cannot be suppressed. Subsequently, if the same curve is unlocked, it can be suppressed.

Collapse / Expand Edges The Edit edges command in the Edit group under the Meshing tab is used to 1) merge two nodes that define an edge or 2) expand (split) along the edge defined by the two nodes. The method to use is Element: Collapse / Expand Edges. The parameters that are used are • Pick Nodes: Select two nodes to define an edge. The nodes can be coincident. The nodes do not

have to belong to the same actual finite element edge. • Method: • Collapse: Collapses the edge formed by the two nodes. • Expand: Splits the edge formed by the two nodes.

CHAPTER 13 Model Generation

• Propagate: if checked, extends the collapse/expansion along all connected elements until the end

of the mesh path or a feature boundary is reached. • Force Editing: if checked, if a node that is associated with a hard point (vertex) can be moved,

otherwise the node cannot be moved.

Creating a Surface Mesh From an Existing Surface Mesh The On Mesh command in the Automesh group under the Meshing tab is used to create a surface mesh from an existing surface mesh. The parameters that are used are • Elements: select the set of surface elements that are to be remeshed. • Element Size: edge length of the new elements. • Mesh Type: Mixed (Quad and Tria), Tria only. • Mesh Method:. Paving, Mapped. • Seed Type: • Uniform: The mesher will create new boundary nodes based on input global edge length. • Existing Boundary: All boundary edges on input mesh will be preserved. • Defined Boundary. The mesher will use all the nodes selected in the Feature Selection sub-

form to define the boundary of the output mesh. No other boundary nodes will be created. • Delete Input Mesh -- Option to delete original elements • Element property -- Option to specify the property to be associated to the new elements. • Add to part -- Option to associate the new mesh to a desired Part. • Curvature check -- Option to adjust the mesh density to control the deviation between the input

mesh and the straight element edges on the output mesh. • Feature recognition -- Option to define features on the input mesh automatically based on

feature edge angles and vertex angles, and preserve them on the output mesh. • Feature selection -- Allows for manual selection of entities to be preserved in the new mesh. • Washers around holes -- used to create layers of elements that are well shaped around holes.

Remesh Elements Retaining Features The Remesh command in the Edit group under the Meshing tab is used to create a new mesh on an existing shell mesh without removing features, hard points, or connected rigid elements. The parameters that are used are: • Elements: select those elements to be remeshed. • Feature Angle:specify the angle between adjacent element normals that if exceeded will define a

feature line. • Free Edge Size: Edge length for free edges for those elements with free edges .

14 Modeling Guide

• Keep Better Quality Only: Option to keep the new elements only if they are of better quality

otherwise the older mesh will be retained..

Automatically Remesh CAD Geometry and Update LBCs When geometry is imported into SimXpert, the user will want to mesh it and possibly create LBCs that are associated to it. After this is done, the geometry may be changed. If the geometry is modified in a CAD program, then imported into a SimXpert database, it will be necessary to remesh the geometry and create new LBCs. Doing this manually could involve a considerable amount of work. There are several ways to deal with this task. One way is to use SimXpert’s capability of detecting changes in the geometry, then automatically remeshing as shown in the examples below. Steps to have SimXpert automatically update your CAD model: • Execute SimXpert. • Import CATIA geometry. • Mesh the geometry and create any LBCs, associating them to the geometry. • Exit SimXpert. • Execute CATIA. • Open the geometry in CATIA. • Make changes to the geometry. • Save the changes to the CATIA database, then exit CATIA. • Execute SimXpert, then open the database corresponding to the CATIA geometry. • SimXpert will detect that the geometry is different will automatically remesh changed regions.

Also, the corresponding LBCs will be updated. Possible variations to the above steps: • Variation 1 • Mesh geometry in SimXpert, then exit SimXpert. • Open the geometry in CATIA. • Create new geometry in CATIA, then exit. • Open the geometry (original and new) in SimXpert. • In SimXpert the original geometry will retain its mesh and the new geometry will be part of

the database. • Variation 2 • Mesh some of the geometry in SimXpert, then exit SimXpert. • Open the geometry in CATIA. • Delete the geometry that was meshed in SimXpert, then exit CATIA. • Open the geometry (original minus deleted) in SimXpert.

CHAPTER 15 Model Generation

• The geometry that was deleted in CATIA is gone, and the mesh the was associated to the

deleted geometry is gone. The second way to do this is to use Smart Update. File > Smart Update is used to access geometry that is currently being used in a CAD program. Any changes to the geometry in the CAD program will be indicated to SimXpert. If the geometry was previously meshed and had LBCs assigned to it, it will be remeshed and the LBCs modified. Using this approach requires both SimXpert and the CAD program to be executing simultaneously.

Element Modification To modify an element the user can can select one or more elements from the canvas and click Edit > Properties from the top menu.

Click Edit > Properties.

16 Modeling Guide

The form for modifying the element properties of the selected elements will appear.

Selecting a multiple number of elements to modify their properties will display only common properties, and the modified properties will be applied to all the selected elements. Instead of selecting Edit > Properties from the top menu, the user can RMB click on the selected elements, then select Properties in the drop-down menu that appears.

CHAPTER 17 Model Generation

18 Modeling Guide

Connections Connections can be created in the Connection group under the LBCs tab. A connection in SimXpert defines the location of the connection between parts. Before creating a connection, a Connection Type must first be selected. Creating a Connection alone does not create any elements. Once a Connection has been created, it must be “Rendered” to produce a specific connection type, eg. RBE2, CWELD, etc.

Connection Groups Connections are stored in Connection Groups. A connection group references up to four parts that will be connected when the Connections in it are rendered. A Maximum Length tolerance defines the maximum distance between parts for which to generate connections.

Parts Geometry

Meshing

Elements

Connection Group Connections

Render

Elements

The diagram above is an analogy between Parts and Connection Groups. Parts are like Connection Groups, but Parts contain surfaces, while Connection Groups contain Connections. And surfaces are like connections in that neither are exported to a solver file. Surfaces and Connections can be re-used across different disciplines (eg. Structures and Crash). Also, as compared in the boxed regions of the diagram, automeshing is like rendering. Automeshing has several algorithms - some for surfaces and some for solids, while rendering has several methods for each connection type. Meshing and Rendering are both procedures that create actual elements that can be exported to a solver file. Along with the various Connection Types, there are also two Connection Group Options to choose from when creating connections.

CHAPTER 19 Model Generation

1. Auto Create Connection Group - Determines Parts that lie within the tolerance of the connection. If no Connection Group exists for those parts, a new Connection Group will be created. 2. Use Current Connection Group - Connections are placed into the current Connection Group (Current group can be set by Right-Clicking the group name in the Model Browser and selecting Set Current from the context menu).

Creating Connections In order to create a connection, it is first necessary to select one of the following seven Connection Types. 1. Spot Weld 2. Bolt 3. Hinge Pin 4. Seam Weld 5. Adhesive Curve 6. Adhesive Surface 7. Trim Mass Spot Weld Spot Weld creates a general connection between shell parts. To create a spot weld connection, select the points defining the spot weld locations. The locations do not need to be at existing nodes. There are also various rendering options for Spot Weld: • ACM2 - Solid HEXA element connected with RBE3 elements • RBE2 - Node-to-Node Rigid element • CFAST - Mesh independent CFAST element • CWELD - Mesh independent CWELD element • RBAR - Node-to-Node Rigid Bar element • Generic - Node-to-Node multi-element connector defined by a SimXpert Generic Template

For the Node-to-Node connections, if the connection location does not coincide with a node on the surface mesh, near nodes will be moved or the shell elements split. Bolt Bolt creates a rigid connection between aligning holes in shell element parts. It is rendered with RBE2 elements which create a “spider web” at each hole by linking the elements around the perimeter. To create a bolt connection, select any node on the perimeter of one of the holes. The aligning holes on the other parts will be automatically detected.

20 Modeling Guide

Bolt has two rendering options: • Clevis Search - Searches for a co-linear hole in the same part and connects if found • Release Rotate Dof - CBAR elements will be created instead of the linking RBE2s with the pin

flag releasing the rotational DOF about the bolt axis at one end Hinge Pin Hinge Pin is a connection that can have rotational degrees of freedom released. It is effectively the same as a Bolt Connection, but instead has the Release Rotate Dof option selected by default. Seam Weld Seam Weld is a rigid connection representing a seam weld between parts. It is typically used for lap joints and T-connections. It is rendered with multiple RBE2 elements. Seam Weld also automatically handles mismatched meshes by element splitting and node adjustments. To create a seam weld connection, select a series of locations to define a polyline along which the seam weld will be created. Adhesive Curve Adhesive Curve creates a patch between two parts defined by a curve. Also, it generates solid HEXA elements connected to the parts through RBE3 elements. To create an adhesive curve connection, select a series of locations to define a polyline representing one side of the adhesive area. For Adhesive Curve, there are various rendering options such as: • Mesh Thickness - The thickness of the adhesive region (solid elements) • Mesh Width - The width of the adhesive region • Mesh Width Offset - The offset of the adhesive region from the adhesive curve • Mesh Length - The length of the individual solid elements • Young’s Modulus - Material property for the adhesive region • Poisson’s Ratio - Material property for the adhesive region

Adhesive Surface Adhesive Surface is very similar to Adhesive Curve Connection, but in Adhesive Surface, region is defined by selecting elements. To create an adhesive surface connection, select shell elements on one part that defines the adhesive area For Adhesive Surface, there are various rendering options such as: • Thickness - The thickness of the adhesive region (solid elements) • Young’s Modulus - Material property for the adhesive region

CHAPTER 21 Model Generation

• Poisson’s Ratio - Material property for the adhesive region

The Mesh Width and Length are assumed from the element selection. The Mesh Width Offset is zero. Trim Mass Trim Mass represents a lumped mass connected to various nodes. To create a trim mass connection select a location for the mass element followed by the locations to connect the mass to the structure. For Trim Mass, there are various rendering options such as: • Mass - The lumped mass • Search Tolerance - Distance to search for nodes from the selected locations • Stiffness Type - Select from RBE2 (rigid) or RBE3 (interpolation) element to connect the mass

to the structure

22 Modeling Guide

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 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. 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)

CHAPTER 23 Model Generation

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: 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. A Cartesian coordinate system consists of three mutually perpendicular axes (X, Y, & Z axis) which intersect at the origin. The three directions of a Cartesian coordinate system may be referred to as X,Y,Z; u, v, w; or 1,2,3 respectively. In a cartesian coordinate system, the principal axes 1, 2 and 3 correspond to the X, Y and Z axes, respectively. Points in space are entered in the order: x-coordinate, y-coordinate and z-coordinate. The principal axes of a cartesian coordinate system and a point, P(x, y,z) are shown in Figure 2. Z Axis 3 P = (x, y, z)

z Axis 2 x

Axis 1 y X

Figure 2

Cartesian Coordinate System

Y

24 Modeling Guide

The graphical representation for creating a coordinate system using 3 Points method is shown in Figure 3.

Second, a point location on the specified axis Third, a point location in the specified plane

Figure 3

First, a point location at the Origin

Coordinate system using 3 Points method

In Figure 4, the normal method to create a cartesian coordinate system is graphically represented. The origin of the coordinate system is at a node on a surface. The z-axis direction is normal to the surface by using right-hand rule and crossing the surface’s U direction with the V direction.The x-axis is parallel to the U direction.

Y X Z

v u Figure 4

Cartesian Coordinate system using Normal method

CHAPTER 25 Model Generation

The graphical representation for creating a coordinate system using 2 vector method is shown in Figure 5 Z

Third, two points to define the Vector for Axis-2

First, a point location for origin (0, 0, 0) (0, 0.9, 0) (0.5, 0, 0)

Y

(0, 1, 0)

(1, 0, 0) X

Figure 5

Second, two points to define the Vector for Axis-1

Coordinate System using 2 Vector Method

26 Modeling Guide

Loads and Boundary Conditions Loads and boundary conditions describe the physical environmen of the model to be analyzed. LBCs can be created under the LBCs tab.

CHAPTER 27 Model Generation

Material SimXpert supports the following material properties: • Isotropic. • Has the same properties in every direction. • Infinite number of planes of material property symmetry. • Two independent elastic constants. • Orthotropic 2D, 2D axisymmetric, and 3D. • Has the same properties in some directions, and different properties in other directions. • For 3D, there are three orthogonal planes of material property symmetry; nine independent

elastic constants; no interaction between normal and shear stresses. • Anisotropic 2D and 3D. • Has different properties for different directions. • For 3D, there are no planes of material property symmetry; 21 independent elastic constants.

For nonlinear analysis, supported properties are • Elasto plastic • Elastic behavior when total stress < yield stress of the material. • Plastic behavior when total stress > yield stress of the material. • Visco elastic (nonlinear elastic) • Elastic in the classical sence -- upon unloading, the stress-strain curve is retraced with no

permanent deformation/offset. The material is initially isotropic. • Viscous effects are modeled. • If the appropriate parameters are specified, is is possible to define a hypoelastic material. • Visco plastic • This is time-dependent cyclic plasticity. • Creep • This is time-dependent, inelastic behavior, and can occur at any stress level (below or above

the yield stress of the material). Temperature dependent material properties are also allowed, for both linear and nonlinear analysis.

Material Overview A wide variety of materials are encountered in stress analysis problems, and for any one of these materials a range of constitutive models is available to describe the material’s behavior. We can broadly classify the materials of interest as those which exhibit almost purely elastic response, possibly with some energy dissipation during rapid loading by viscoelastic response (the elastomers, such as rubber or

28 Modeling Guide

solid propellant); materials that yield, and exhibit considerable ductility beyond yield (such as mild steel and other commonly used metals, ice at low strain rates, and clay); materials that flow by rearrangement of particles which interact generally through some dominantly frictional mechanism (such as sand); and brittle materials (rock, concrete, ceramics). Table 5-1 Material

Common Material Characteristics Characteristics

Composites

Anisotropic:

(MATi, MATORT, PCOMP)

1) Layered, ds ij

Examples Aircraft panels

= C ijkl dε kl

21 Constants

Models Composite continuum elements

Tires, glass/epoxy

2)Fiber Reinforced,

E t S = --- ( T CT – 1 ) 2 One dimensional strain in fibers Creep (MATVP)

Elastic (MATi, MATORT) Elastoplasticity (MATEP)

Strains increasing with time under Metals at high constant load. Stresses decreasing temperatures, polymide films, semiconductor with time under constant materials deformations. Creep strains are noninstantaneous.

ORNL

Stress functions of instantaneous strain only. Linear load-displacement relation.

Small deformation (below yield) for most materials: metals, glass, wood

Hookes Law

Yield condition flow rule and hardening rule necessary to calculate stress, plastic strain. Permanent deformation upon unloading.

Metals

von Mises Isotropic

Norton Maxwell

Soils Cam -Clay Hill’s Anisotropic

CHAPTER 29 Model Generation

Table 5-1

Common Material Characteristics (continued)

Material Hyperelastic (MATHE)

Characteristics Stress function of instantaneous strain. Nonlinear loaddisplacement relation. Unloading path same as loading.

Examples Rubber

Models Mooney Ogden Arruda-Boyce Gent

Hypoelastic

Rate form of stress-strain law

Concrete

Buyukozturk

Viscoelastic

Time dependence of stresses in elastic material under loads. Full recovery after unloading.

Rubber,

Simo Model

Glass, industrial

Narayanaswamy

(MATVE)

plastics

Viscoplastic

Combined plasticity and creep phenomenon

(MATVP)

Metals

Power law

Powder

Shima Model

Constitutive Models A single material may contain multiple constitutive models. Each constitutive model characterizes distinct ranges of the material’s response. The constitutive models in MD Nastran Implicit Nonlinear contain a range of linear and nonlinear material models that can address or approximate the material response of most commonly encountered materials. The constitutive models in MD Nastran Implicit Nonlinear can be accessed by any of the solid or structural elements. The models are assessed independently at each “constitutive calculation point” (i.e., the numerical integration points in the elements). Thus, the constitutive models are concerned only with a single calculation point. The element then provides an estimate of the kinematic solution to the problem at the point under consideration.

30 Modeling Guide

MD Nastran Implicit Nonlinear Material Entries The following material bulk data entries are available in SOL 600. Each of these options are summarized in the sections of this chapter and detailed in the MD NASTRAN QRG. All standard MD Nastran materials are also available in SOL 600. Bulk Data Entry MATEP --MATTEP MATF MATG --MATTG MATHE --MATTHE MATED MATORT

--MATTORT

MATVE --MATTVE

MATVP

Description Specifies elasto-plastic material properties. Specifies temperature-dependent elasto-plastic material properties. Specifies failure model properties for linear elastic materials. Specifies gasket material properties to be used in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies gasket material property temperature variation to be used in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies hyperelastic (rubber-like) material properties for nonlinear (large strain and large rotation) analysis in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies temperature-dependent properties of hyperelastic (rubber-like) materials (elastomers) in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies damage model properties for hyperelastic materials in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies elastic orthotropic material properties for 3-dimensional and plane strain behavior for linear and nonlinear analyses in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies temperature-dependent properties of elastic orthotropic materials for linear and nonlinear analyses used in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies isotropic visco-elastic material properties in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies temperature-dependent visco-elastic material properties in terms of Thermo-Rheologically Simple behavior in MD Nastran Implicit Nonlinear (SOL 600) only. Specifies viscoplastic or creep material properties to be used for quasi-static analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

The following sections describe how to model material behavior in MD Nastran Implicit Nonlinear. Modeling material behavior consists of both specifying the constitutive models used to describe the material behavior and defining the actual material data necessary to represent the material. Directional dependency can be included for materials other than isotropic materials. Data for the materials can be entered into MD Nastran Implicit Nonlinear either directly through the input file or by user subroutines, or material models may be defined in the SimXpert Materials Application. Each section of this chapter discusses various options for organizing material data for input. Each section also discusses the constitutive (stress-strain) relation and graphic representation of the models and includes recommendations and cautions concerning the use of the models.

CHAPTER 31 Model Generation

Linear Elastic MD Nastran Implicit Nonlinear is capable of handling problems with any combination of isotropic, orthrotropic, or anisotropic linear elastic material behavior. The linear elastic model is the model most commonly used to represent engineering materials. This model, which has a linear relationship between stresses and strains, is represented by Hooke’s Law. Figure 5-1 shows that stress is proportional to strain in a uniaxial tension test. The ratio of stress to strain is the familiar definition of modulus of elasticity (Young’s modulus) of the material. (5-1)

Stress

E (modulus of elasticity) = (axial stress)/(axial strain)

E 1

Strain

Figure 5-1

Uniaxial Stress-Strain Relation of Linear Elastic Material

Experiments show that axial elongation is always accompanied by lateral contraction of the bar. The ratio for a linear elastic material is:

v = (lateral contraction)/(axial elongation)

(5-2)

This is known as Poisson’s ratio. Similarly, the shear modulus (modulus of rigidity) is defined as:

G (shear modulus) = (shear stress)/(shear strain)

(5-3)

A Poisson’s ratio of 0.5, which would be appropriate for an incompressible material, can be used for the following elements: Herrmann, plane stress, shell, truss, or beam. A Poisson’s ratio which is close (but not equal) to 0.5 can be used for constant dilation elements and reduced integration elements in situations which do not include other severe kinematic constraints. Using a Poisson’s ratio close to 0.5 for all other elements usually leads to behavior that is too stiff. A Poisson’s ratio of 0.5 can also be used with the updated Lagrangian formulation in the multiplicative decomposition framework using the standard displacement elements. In these elements, the treatment for incompressibility is transparent.

32 Modeling Guide

Isotropic Materials Most linear elastic materials are assumed to be isotropic (their elastic properties are the same in all directions). For an isotropic material, every plane is a plane of symmetry and every direction is an axis of symmetry. It can be shown that for an isotropic material:

G = E ⁄ ( 2( 1 + v ) ) The shear modulus are known.

(5-4)

G can be easily calculated if the modulus of elasticity E and Poisson’s ratio v

Specifying Isotropic Material Entries

Isotropic material models are designated with the MAT1 Bulk Data entry in the MD Nastran Input File. Entry

Description

MAT1

Defines the material properties for linear isotropic materials.

References • MAT1 in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define an isotropic material in SimXpert: 1. Select Materials and Properties>Isotropic. Isotropic linear elastic material models require the following material data via the Input Options subform on the Materials Application form. Isotropic-Linear Elastic

Description

Elastic Modulus

Defines the elastic modulus. This property is generally required. May vary with temperature via a defined material field.

Shear Modulus

Defines the shear modulus. This property is generally not required. May vary with temperature via a defined material field.

Poisson’s Ratio

Defines the Poisson’s ratio. This property is generally required. May vary with temperature via a defined material field.

Density

Defines the mass density. This property is optional.

The material density, used to define the mass of the structure, and the damping value are used in dynamic loadings, while the expansion coefficient is used to identify the thermal strains.

CHAPTER 33 Model Generation

Orthotropic Materials An orthotropic material has three mutually orthogonal planes of symmetry. With respect to a coordinate system parallel to these planes, the constitutive law for this material is given by the following more general form of Hooke’s Law:

ε 11

1 ⁄ ( E1 )

ε 22

( – υ 12 ) ⁄ ( E 1 )

ε 33 γ12

=

–( υ 12 ) ⁄ ( E 1 ) – ( υ 13 ) ⁄ ( E 1 )

0

0

σ 11

( – υ 23 ) ⁄ ( E 2 )

0

0

0

σ 22

1 ⁄ ( E3 )

0

0

0

σ 33

1 ⁄ ( E2 )

0

( – υ 13 ) ⁄ ( E 1 ) ( – υ 23 ) ⁄ ( E 2 ) 0

0

0

1 ⁄ ( G 12 )

0

0

τ 12

γ23

0

0

0

0

1 ⁄ ( G 23 )

0

τ 23

γ13

0

0

0

0

0

1 ⁄ ( G 13 ) τ 13

3-D Orthotropic

Due to symmetry of the compliance matrix, E11 ν 21 = E22 ν 12 , E22 ν 32 = E33 ν 23 , and E33 ν 13 = E11 ν 31 . Using these relations, a general orthotropic material has nine independent constants: E11, E22, E33,

ν 12 , ν23 , ν 31 , G12, G23, G31

These nine constants must be specified in constructing the material model. Note:

The inequalities E22 >

ν 23 E33, E11 > ν 12 E22, and E33 > ν 31 E11 must be satisfied in

order for the orthotropic material to be stable. This is checked by MD Nastran Implicit Nonlinear. 2-D Orthotropic

Orthotropic material models can be used with 2-D elements, such as plane stress, plane strain, and axisymmetric elements. For example, the orthotropic stress-strain relationship for a plane stress element is:

1 C = ----------------------------( 1 – ν 12 ν21 )

E1

ν 21 E 1

0

ν 12 E 2

E2

0

0

0

( 1 – ν 12 ν 21 )G

Specifying Orthotropic Material Entries

(5-5)

34 Modeling Guide

2-D and 3-D othrotropic materials are characterized in MD Nastran using the following bulk data entries. Entry

Description

MAT3

Defines the material properties for linear orthotropic materials used by the CTRIAX6 element entry.

MAT2

Defines the material property for an orthotropic material for solids and isoparametric shell elements.

MAT8 MATORT

Specifies elastic orthotropic material properties for three-dimensional and plane strain behavior for linear and nonlinear analyses in MD Nastran Implicit Nonlinear (SOL 600) only in a more general way than MAT2 or MAT8.

References • MAT3 in the MD NASTRAN QRG. • MAT8 in the MD NASTRAN QRG. • MATORT in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define an orthotropic material in SimXpert: 1. Select Materials and Properties>2D or 3D Orthotropic. The required properties for orthotropic linear elastic material models vary based on dimension, element type, and thermal dependencies. 3-D orthotropic material models require the following material data (2-D requires a reduced set) via the Input Properties subform on the Materials Application form. Orthotropic-Linear Elastic Description Elastic Modulus 11/22/33

Defines the elastic moduli in the element’s coordinate system. This is required data. May vary with temperature via a defined material field.

Poisson’s Ratio 12

Defines the Poisson’s ratios relative to the element’s coordinate system. This is required data. May vary with temperature via a defined material field.

Density

Defines the mass density which is an optional property.

Shear Modulus 12/23/31

Defines the shear moduli relative to the element’s coordinate system. This is required data. May vary with temperature via a defined material field.

Anisotropic Materials Anisotropic material exhibits different elastic properties in different directions. The significant directions of the material are labeled as preferred directions, and it is easiest to express the material behavior with respect to these directions. The stress-strain relationship for an anisotropic linear elastic material can be expressed as

CHAPTER 35 Model Generation

σ ij = C ijkl ε kl

(5-6)

The values of C ijkl (the stress-strain relation) and the preferred directions (if necessary) must be defined for an anisotropic material. Specifying Anisotropic Material Entries

Anisotropic materials are characterized in MD Nastran using the following bulk data entries. Entry

Description

MAT2

Defines the material properties for linear anisotropic materials for twodimensional elements.

References • MAT2 in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define anisotropic material in SimXpert: 1. Select Materials and Properties>2D or 3D Anisotropic>. Anisotropic linear elastic material models require the following material data via the Input Properties subform on the Materials Application form. Anisotropic-Linear Elastic Description Stress-Strain Matrix components, Cij

Defines the upper right portion of the symmetric stress-strain matrix relative to the element’s coordinate system.

Density

Defines the mass density which is an optional property.

Nonlinear Elastic Hypoelastic - Isotropic The hypoelastic model is able to represent a nonlinear elastic (reversible) material behavior. For this constitutive theory, MD Nastran Implicit Nonlinear assumes that

σ· ij = L ijkl ε· kl + g ij where

(5-7)

L is a function of the mechanical strain and g is a function of the temperature.

The stress and strains are true stresses and logarithmic strains, respectively, when used in conjunction with the updated Lagrange and large displacement options. When used in conjunction with the large displacement option only, Equation (5-7) is expressed as

36 Modeling Guide

· · S ij = L ijkl E kl + g ij where

(5-8)

E, S are the Green-Lagrangian strain and second Piola-Kirchhoff stress, respectively.

This model can be used with any stress element, including Herrmann formulation elements. The tensors

L and g may be defined by user subroutine HYPELA. In order to provide an accurate

solution, L should be a tangent stiffness evaluated at the beginning of the iteration. In addition, the total stress should be defined as its exact value at the end of the increment. This allows the residual load correction to work effectively. In user subroutine HYPELA2, besides the functionality of HYPELA, additional information is available regarding the kinematics of deformation. In particular, the deformation gradient ( F ), rotation tensor ( R ), and the eigenvalues ( λ ) and eigenvectors ( N ) to form the stretch tensor ( U ) are also provided. This information is available only for the continuum elements namely: plane strain, generalized plane strain, plane stress, axisymmetric, axisymmetric with twist, and three-dimensional cases. Hyperelastic - Isotropic Hyperelastic models are specified using either the MATHP or MATHE bulk data entries and are used to describe the behavior of materials that exhibit elastic response up to large strains, such as rubber, solid propellant, and other elastomeric materials. These materials are described in terms of a “strain energy potential”, U, which defines the strain energy stored in the material per unit of volume in the initial configuration as a function of the strain at that point in the material.

σ, Stress

Elastomeric materials are elastic in the classical sense. Upon unloading, the stress-strain curve is retraced and there is no permanent deformation. Elastomeric materials are initially isotropic. Figure 5-2 shows a typical stress-strain curve for an elastomeric material.

100%

ε, Strain

Figure 5-2

A Typical Stress-Strain Curve for an Elastomeric Material

CHAPTER 37 Model Generation

Calculations of stresses in an elastomeric material requires an existence of a strain energy function which is usually defined in terms of invariants or stretch ratios. Significance and calculation of these kinematic quantities is discussed next. Characteristics of Elastomeric Materials

Most solid rubberlike materials are nearly incompressible: their bulk modulus is several orders of magnitude larger than their shear modulus. For applications where the material is not highly confined, the assumption that the material is fully incompressible is usually a good approximation. In cases where the material is highly confined (such as in an O-ring), modeling the compressibility can be important for obtaining accurate results. In either case, the use of “hybrid” (mixed formulation) elements is recommended for this type of material in all but plane stress cases. Elastomeric foams on the other hand are elastic but very compressible. Elastomeric materials are considered to be isotropic in nature with random orientation of the long chain molecules. Strain Energy Potential and Representative Models

Calculations of stresses in an elastomeric material requires an existence of a strain energy function which is usually defined in terms of invariants or stretch ratios. In the rectangular block in Figure 5-3,

λ 1 , λ 2 , and λ 3 are the principal stretch ratios along the edges

of the block defined by

λi = ( Li + ui ) ⁄ Li

(5-9)

L3

λ3L3 λ2L2

λ1L1 L2

Undeformed Deformed

L1

Figure 5-3

Rectangular Rubber Block

In practice, the material behavior is (approximately) incompressible, leading to the constraint equation

λ1 λ2 λ3 = 1 the strain invariants are defined as

38 Modeling Guide

2

I 1 = λ 12 + λ 2 + λ 32 2 2

2 2

2 2

I2 = λ 1 λ 2 + λ 2 λ 3 + λ3 λ1 2 2 2

I3 = λ1 λ2 λ3

(5-10)

Depending on the choice of configurations, for example, reference (at t = 0 ) or current ( t = n + 1 ), you obtain total or updated Lagrange formulations for elasticity. The kinematic measures for the two formulations are discussed next. Total Lagrangian Formulation

The strain measure is the Green-Lagrange strain defined as:

1 E ij = --- ( C ij – δ ij ) 2 where

(5-11)

C ij is the right Cauchy-Green deformation tensor defined as:

C ij = F ki F kj in which

(5-12)

F kj is the deformation gradient (a two-point tensor) written as:

∂x k F kj = -------∂X j The Jacobian

(5-13)

J is defined as:

J = λ 1 λ 2 λ 3 = ( det C ij )

1--2

(5-14)

Thus, the invariants can be written as:

I 1 = C ii

(implied sum on i) 2

( C ij C ij – ( C ii ) ) I 2 = -------------------------------------2 1 I 3 = --- e ijk e pqr C ip C jq C kr = det ( C ij ) 6 in which e ijk is the permutation tensor. Also, using spectral decomposition theorem,

(5-15)

CHAPTER 39 Model Generation

2

A

A

C ij = λ A N i N j

(5-16)

in which the stretches the eigenvectors are

2

λ A are the eigenvalues of the right Cauchy-Green deformation tensor, C ij and A

Ni .

Updated Lagrange Formulation

The strain measure is the true or logarithmic measure defined as:

1 ε ij = --- ln b ij 2

(5-17)

where the left Cauchy-Green or finger tensor

b ij is defined as:

b ij = F ik F jk

(5-18)

Thus, using the spectral decomposition theorem, the true strains are written as:

1 ε ij = --- ( ln λ A )nAi n jA 2 where

(5-19)

nAi is the eigenvectors in the current configuration. It is noted that the true strains can also be

approximated using first Padé approximation, which is a rational expansion of the tensor, as:

ε ij = 2 ( V ij – δ ij ) ( V ij + δ ij )

–1

where a polar decomposition of the deformation gradient rotation tensor

(5-20)

F ij is done into the left stretch tensor V ij and

R ij as:

F ij = V ik R kj The Jacobian

J is defined as:

J = λ 1 λ 2 λ 3 = ( det b ij )

1 --2

and the invariants are now defined as:

(5-21)

40 Modeling Guide

I 1 = b ii 1 2 I 2 = --- ( b ij b ij – ( b ii ) ) 2 and

1 I 3 = --- e ijk e pqr b ip b jq b kr = det ( b ij ) 6

(5-22)

It is noted that either Equation (5-15) or Equation (5-22) gives the same strain energy since it is scalar and invariant. Also, to account for the incompressibility condition, in both formulations, the strain energy is split into deviatoric and volumertic parts as:

W = W deviatoric + W volumetric

(5-23)

Mooney-Rivlin Model

The generalized Mooney-Rivlin model for nearly-incompressible elastomeric materials is written as: N gmr W deviatoric

N

  Cmn ( I1 – 3 )

=

m

( I2 – 3 )

n

(5-24)

m=1 n=1

where I 1 and I 2 are the first and second deviatoric invariants. Jamus-Green-Simpson Model

A particular form of the generalized Mooney-Rivlin model, namely the third order deformation (tod) model, is implemented in MD Nastran Implicit Nonlinear (SOL 600). This is one of the few places where the formulation for SOLs 106 and 129 may be more appropriate because they can use up to fifth order terms. However, the Ogden formulation (below) is usually better for large strain behavior than even the fifth order Mooney-Rivlin. tod

W devratoric = C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 ) + C 11 ( I 1 – 3 ) ( I 2 – 3 ) + C 20 ( I 1 – 3 ) 2 + C 30 ( I 1 – 3 ) where

3

tod

W deviatoric is the deviatoric third order deformation form strain energy function,

C 10, C 01, C 11, C 20, C 30 are material constants obtained from experimental data. Simpler and popular forms of the above strain energy function are obtained as:

(5-25)

CHAPTER 41 Model Generation

nh

W deviatoric = C 10 ( I 1 – 3 ) mr

W deviatoric = C 10 ( I 1 – 3 ) + C 01 ( I 2 – 3 )

Neo-Hookean Mooney-Rivlin (5-26)

Ogden Model

The form of strain energy for the Ogden model in MD Nastran Implicit Nonlinear is, N ogden W deviatoric

=

 k=1

αk where λ i

=

μ αk αk αk -----k- ( λ 1 + λ 2 + λ 3 – 3 ) αk

α – -----k α 3 k J λ i are the deviatoric stretch ratios while

(5-27)

C mn , μ k , and α k are the

material constants obtained from the curve fitting of experimental data. The Ogden model is usually applied to slightly compressible materials. If no bulk modulus is given, it is taken to be virtually incompressible. This model is different from the Mooney model in several respects. The Mooney material model is with respect to the invariants of the right or left Cauchy-Green strain tensor and implicitly assumes that the material is incompressible. The Ogden formulation is with respect to the eigenvalues of the right or left Cauchy-Green strain, and the presence of the bulk modulus implies some compressibility. Using a two-term series results in identical behavior as the Mooney mode if:

μ 1 = 2C 10 , α 1 = 2 , μ 2 = – 2C 01 , and α 2 = – 2 Arruda-Boyce Model

In the Arruda-Boyce strain energy model, the underlying molecular structure of elastomer is represented by an eight-chain model to simulate the non-Gaussian behavior of individual chains in the network. The

nkΘ and N ( n is the chain density, k is the Botzmann constant, Θ is the temperature, and N is the number of statistical links of length l in the chain between chemical crosslinks) two parameters,

representing initial modules and limiting chain extensibility and are related to the molecular chain orientation thus representing the physics of network deformation. As evident in most models describing rubber deformation, the strain energy function constructed by fitting experiment data obtained from one state of deformation to another fails to accurately describe that deformation mode. The Arruda-Boyce model ameliorates this defect and is unique since the standard tensile test data provides sufficient accuracy for multiple modes of deformation.

42 Modeling Guide

j

λ2 α0 C1 i

λ3 α0 λ1 α0

k

Figure 5-4

Eight Chain Network in Stretched Configuration

The model is constructed using the eight chain network as follows: Consider a cube of dimension

r0 =

α0 with an unstretched network including eight chains of length

Nl , where the fully extended chain has an approximate length of Nl. A chain vector from the

center of the cube to a corner can be expressed as:

α0 α0 α0 C 1 = ------ λ 1 i + ------ λ 2 j + ------ λ 3 k 2 2 2

(5-28)

Using geometrical considerations, the chain vector length can be written as: 1⁄2 1 r chain = ------- Nl ( λ 12 + λ 22 + λ 32 ) 3

(5-29)

and

r chain 1 1⁄2 λ chain = ------------ = ------- ( I 1 ) r0 3

(5-30)

Using statistical mechanics considerations, the work of deformation is proportional to the entropy change on stretching the chains from the unstretched state and may be written in terms of the chain length as:

r chain β W = nkΘN  ------------ β + ln --------------  – ΘCˆ Nl sinh β ˆ

(5-31)

where n is the chain density and C is a constant. β is an inverse Langevin function correctly accounts for the limiting chain extensibility and is defined as:

CHAPTER 43 Model Generation

r chain β = L – 1  ------------ Nl

(5-32)

where Langevin is defined as:

1 ℑ ( β ) = coth β – --β

(5-33)

With Equation (5-30) through Equation (5-33), the Arruda-Boyce model can be written Arruda-Boyce

W dev

1 1 11 = nkΘ --- ( I 1 – 3 ) + ---------- ( I 12 – 9 ) + ------------------2 ( I 13 – 27 ) 2 20N 1050N 19 519 + ------------------3 ( I 14 – 81 ) + ------------------------4 ( I 15 – 243 ) ] 7000N 673750N

(5-34)

Gent Model Also, using the notion of limiting chain extensibility, Gent proposed the following constitutive relation:

– EI Im Gent W dev = -----------m- log --------------6 I m – I 1*

(5-35)

where

I 1* = I 1 – 3 The constant

(5-36)

EI m is independent of molecular length and, hence, of degree of crosslinking. The model

is attractive due to its simplicity, but yet captures the main behavior of a network of extensible molecules over the entire range of possible strains. The volumetric part of the strain energy is for all the rubber models in MD Nastran Implicit Nonlinear is: 1

W volumetric

9K = ------2

 --3-   J – 1  

2

(5-37)

when K is the bulk modulus. It can be noted that the particular form of volumetric strain energy is chosen such that: 1. The constraint condition is satisfied for incompressible deformations only; for example:

44 Modeling Guide

  > 0 if I 3 > 0  f ( I 3 )  = 0 if I 3 = 1   < 0 if I 3 < 0 

(5-38)

2. The constraint condition does not contribute to the dilatational stiffness. This yields the constraint function as: 1

 --6-  f ( I 3 ) = 3  I 3 – 1  

(5-39)

upon substitution of Equation (5-39) in Equation (5-35) and taking the first variation of the variational principle, you obtain the pressure variable as: 1

 --3-  p = 3K  J – 1  

(5-40)

The equation has a physical significance in that for small deformations, the pressure is linearly related to the volumetric strains by the bulk modulus

K.

The discontinuous or continuous damage models discussed in the models section on damage can be included with the generalized Mooney-Rivlin, Ogden, Arruda-Boyce, and Gent models to simulate Mullins effect or fatigue of elastomers when using the updated Lagrangian approach. In the total Lagrangian framework however, this is available for the Ogden model only. Foam Model

Sometimes elastomeric materials show large volumetric deformations. For this type of behavior, the models discussed above are not appropriate. Instead, the foam model expressed by: N

W =

 n=1

μ α α α -----n- ( λ 1 n + λ 2 n + λ 3 n – 3 ) + αn

N

 n=1

μn β ----- ( 1 – J n ) βn

(5-41)

should be used. In contrast to the Ogden model, the first part of the foam strain energy function is not purely deviatoric. The material constants

β n provide additional flexibility to describe the material

behavior also for a large amount of compressibility. Updated Lagrange Formulation for Nonlinear Elasticity

CHAPTER 45 Model Generation

The Mooney-Rivlin, Ogden, Arruda-Boyce, Gent and Foam models may be used either in the total Lagrange or updated Lagrange framework. This is selected using the PARAM,MARUPDAT. For plane stress analysis the total Lagrange procedure will always be used. The updated Lagrangian rubber elasticity capability can be used in conjunction with both continuous as well as discontinuous damage models. Thermal, as well as viscoelastic, effects can be modeled with the current formulation. While the Mooney model can account for the temperature dependent material properties, the Ogden model does not support the temperature dependence at this time. The singularity ratio of the system is inversely proportional to the order of bulk modulus of the material due to the condensation procedure. A consistent linearization has been carried out to obtain the tangent modulus. The singularity for the case of two- or three-equal stretch ratios is analytically removed by application of L’Hospital’s rule. The current framework with an exact implementation of the finite strain kinematics along with the split of strain energy to handle compressible and nearly incompressible response is eminently suitable for implementation of any nonlinear elastic as well as inelastic material models. In fact, the finite deformation plasticity model based on the multiplicative decomposition, implemented in the same framework.

e θ p

F = F F F is

To simulate elastomeric materials, incompressible element(s) are used for plane strain, axisymmetric, and three-dimensional problems for elasticity in total Lagrangian framework. These elements can be used with each other or in combination with other elements. For plane stress, beam, plate or shell analysis, conventional elements can be used. For updated Lagrangian elasticity, both conventional elements (as well as Herrmann elements) can be used for plane strain, axisymmetric, and threedimensional problems. Experimental Determination of Hyperelastic Material Parameters

In order to determine the material parameters to be used, like Mooney coefficients, Ogden moduli, relaxation times, etc., experiments must be carried out. In this section, the laboratory tests of which data can be used to fit the material parameters will be described. Once the test data is available the Experimental Data Fitting module in MSC SimXpert can be used to calculate appropriate coefficient values. For a homogeneous material, homogeneous deformation modes suffice to characterize the material constants. MD Nastran Implicit Nonlinear accepts test data from the following deformation modes: • • • • •

Uniaxial tension and compression. Biaxial tension and compression. Planar tension and compression (also known as pure shear). Simple Shear Volumetric tension and compression

46 Modeling Guide

Uniaxial Test Data

1

3 2

Biaxial Test Data

1

3 2

Planar Test Data

1

3 2

Volumetric Test Data

1

3 2

Figure 5-5

Test Data

Uniaxial Test

Probably the most popular test is the uniaxial test (see Figure 5-6). This test can be used in tension as well as in compression, both for incompressible and (slightly) compressible elastomeric materials. The shape

CHAPTER 47 Model Generation

of the specimen used in compression will usually be less slender than the shape used in tension. Within the region indicated by the dashed line, the state of deformation will be homogeneous, where the deformation can be described by:

λ 1 = λ = 1 + e 11 , λ 2 = λ 3 =

J⁄λ

(5-42)

while the corresponding engineering stresses are given by:

F σ 11 = σ = ------ , σ 22 = σ 33 = 0 A0 in which

(5-43)

F is the applied force and A0 is the cross sectional area of the undeformed specimen in the

E 2 - E 3 -plane, within the region indicated by the dashed line.

F

F E2

E3 Figure 5-6

E1

Uniaxial (Tensile) Test

Necessary input for the curve fitting program in MSC SimXpert consists of at least engineering strain ( e 11 ) versus engineering stress ( σ 11 ) data points. In case of (slightly) compressible materials, information about the volume changes is also needed. This data can be given either in terms of the area

A over the original cross sectional area A 0 . Similarly, the volume ratio is defined by the current volume V over the ratio or the volume ratio. The area ratio is defined by the current cross sectional area

undeformed volume

V 0 . Notice that the volume ratio and the area ratio are related by:

VA ----= J = ------ ( 1 + e 11 ) V0 A0 If, for a particular elastomeric material, both a tensile and a compression test have been performed, all the data points should be collected into one data file. The layout of a data file containing uniaxial test data is given in the figure below. The columns may be separated by either spaces or commas. For (nearly) incompressible material behavior, the third column can be omitted.

48 Modeling Guide

σ 11

e 11

A ⁄ A0

e 11

σ 11

V ⁄ V0

or

Figure 5-7

Layout of Data File for a Uniaxial Test

Equi-Biaxial Test

The equi-biaxial tensile test outlined in Figure 5-8 can be used to obtain, within the region indicated by the dashed line, a homogeneous state of deformation defined by:

F

F

F

E2

E3 Figure 5-8

E1

F

Equi-biaxial (Tensile) Test

λ 1 = λ 2 = λ = 1 + e 11 = 1 + e 22 , λ 3 = J ⁄ λ

2

(5-44)

with corresponding engineering stresses:

F σ 11 = σ 22 = σ = ------ , σ 33 = 0 A0

(5-45)

CHAPTER 49 Model Generation

with

A0

being the original cross sectional area of the elastomeric sheet in the direction perpendicular

to the applied forces, which is assumed to be the same in the

E 1 - E 3 -plane and the E 2 - E 3 -plane.

For compressible elastomers, volumetric information is needed. For the equi-biaxial test, this can be given in terms of a thickness ratio or, similar to the uniaxial test, a volume ratio. The thickness ratio is defined as the current sheet thickness

t over the original sheet thickness t 0 . The relation between the

thickness ratio and the volume ratio is:

Vt 2 ----= J = ---- ( 1 + e 11 ) V0 t0

(5-46)

The layout of a data file for an equi-biaxial tensile test is given in Figure 5-8. Planar Shear Test

A state of planar shear, also sometimes called pure shear, can be obtained by clamping and stretching an elastomeric rectangular sheet of material, as indicated in Figure 5-9.

F

F

E2

E3 Figure 5-9

E1 Planar Shear Test

Except for the vicinity of the free edges and the clamps, the state of strain can be found to be substantially uniform, according to:

J λ 1 = λ = 1 + e 11 , λ 2 = 1 , λ 3 = --λ where the known stress components are given by:

(5-47)

50 Modeling Guide

F σ 11 = σ = ------ , σ 33 = 0 A0 in which

(5-48)

A 0 is the cross sectional area of the undeformed specimen in the E 1 - E 3 -plane. Notice that

the engineering strain e 22 is zero, but that the corresponding engineering stress material behavior.

σ 22 depends on the

δU = T S δλ S T

S

=

(5-49)

– 3  ∂U ∂U  ∂ U = 2λ – λ   +   S S  ∂I ∂ λS 1 ∂ I 2

(5-50)

Simple Shear Test

A test which, compared to the above mentioned tests, leads to a more complex kinematic description, is the simple shear test (see Figure 5-10).Upon introducing the shear strain deformed configuration are given by:

γ , the coordinates in the

x 1 = X1 + γX 2, x 2 = X 2 , x 3 = X3

(5-51)

which yields for the deformation gradient:

1 γ 0 F = 0 10 0 01

(5-52)

2F

E2

E3 Figure 5-10

atan γ

E1 Simple Shear Test

CHAPTER 51 Model Generation

Notice that det ( F ) = 1 , irrespective of the value of shear test is a constant volume test.

γ , from which it can be concluded that a simple

Based on Equation (5-51), Equation (5-52) and Figure 5-10, the engineering strain tensor and the right Cauchy-Green strain tensor can be evaluated as:

0 γ⁄2 0 e = γ⁄2 0 0 0 0 0 γ

1

(5-53)

0

C = γ 1 + γ2 0 0 0 1

(5-54)

According to Equation (5-54), the principal stretch ratios follow from the principal values of and read: 2

λ 1, 2 =

C

2

γ γ 1 + ---- ± γ 1 + ---- , λ 3 = 1 2 4

It can easily be verified that

(5-55)

λ 1 λ 2 λ 3 = 1 , which again shows that the simple shear test is a constant

volume test. The relevant engineering stress is given by:

F σ 12 = -----A0 with

(5-56)

A0 being the cross sectional area of the undeformed specimen in the E 1 - E 3 -plane.

The layout of a data file containing measurements of a simple shear test is given in Figure 5-11.

2e 12 = γ

Figure 5-11

σ 12

Layout of Data File for a Simple Shear Test

52 Modeling Guide

Volumetric Test

Although a uniaxial, equi-biaxial and planar shear test can be used to obtain information about the volumetric behavior, for compressible materials an additional volumetric test may be preferable. This is especially true for slightly compressible materials, since volumetric data from other tests other than a volumetric one may easily be inaccurate (because most of the deformation is deviatoric). Two commonly used volumetric tests are outlined in Figure 5-12. In Figure 5-12a, a cylindrical specimen is compressed in a cylindrical hole. This test can be successfully applied for slightly compressible materials. In Figure 5-12b, a specimen is deformed by compressing the surrounding fluid. This volumetric test can also be used for highly compressible materials.

F

F

E1 (a)

E3

(b)

F

E2

Figure 5-12

Volumetric Tests

For a volumetric test, the direct true stress components are assumed to be equal to the hydrostatic pressure

p and given by: F T 11 = T 22 = T 33 = -----pA in which

(5-57)

p

A denotes the area of the piston in the E 2 - E 3 -plane. The deformation can be expressed in

terms of an engineering strain e and corresponding stretch ratio measured volume change according to:

e = λ–1 = Based on

3

V- – 1 = ----V0

3

λ , which can be determined from the

J–1

λ according to Figure 5-12b, the engineering stress σ follows from:

(5-58)

CHAPTER 53 Model Generation

σ = T 11 λ

2

(5-59)

Notice that only in the case of Figure 5-12b the engineering strain e and the engineering stress equal to the direct components of the engineering strain and the engineering stress tensor.

σ are

The layout of the data file corresponding to a volumetric test is given in Figure 5-13. Notice that because of Figure 5-12b, the entries of the first and the third column are not independent.

e

σ

Figure 5-13

V ⁄ V0

Layout of Data File for a Volumetric Test

Relaxation Test

The basic feature of a relaxation test is that the force or stress response to a prescribed fixed displacement or deformation is measured as a function of time. A relaxation test for a large strain elastomeric material is indicated in Figure 5-14. By measuring the force needed for a displacement Δu at different time intervals, the decay of the strain energy as a function of time can be determined. For linear elastic isotropic material, similar tests can be performed to get information about the shear modulus and/or the bulk modulus as a function of time. In order to properly measure the instantaneous values, application of the prescribed displacement should occur sufficiently fast. It should be noted, due to the assumption introduced in equation Equation (5-94), that for large strain visco-elastic materials the magnitude of (the instantaneous value of) the strain energy is not important, since every energy term in the Prony series expansion is related to the instantaneous strain energy using a scalar multiplier. The data does not need to be equispaced in time. Usually, at the beginning of the relaxation experiment the measurements are done at smaller time intervals than at the end of the experiment.

Δu

54 Modeling Guide

Figure 5-14

Relaxation Test

If, for linear visco-elastic materials, instead of a relaxation test only a creep test can be performed, the creep data must be transformed into relaxation data. Converting creep data into relaxation data can be done using a numerical integration scheme, but is not part of MD Nastran Implicit Nonlinear. Hyperelastic Foam Properties

Elastomeric foams are cellular solids that have the following primary mechanical characteristics: • They can deform elastically up to large strain: up to 90% strain in compression. In most

applications, this is the dominant mode of deformation. • Their porosity permits very large volumetric changes. This is in contrast to solid rubbers, which

are approximately incompressible. • Cellular solids are made up of interconnected networks of solid struts or plates which form the

edges and faces of cells. Foams are made up of polyhedral cells that pack in three dimensions. The foam cells can either be open (e.g., sponge) or closed (e.g., flotation foam). Common examples of elastomeric foam materials are cellular polymers such as cushions, padding, and packaging materials which utilize the excellent energy absorption properties of foams - for a certain stress level, the energy absorbed by foams is substantially greater than by ordinary stiff elastic materials. The figure below shows a typical compressive stress-strain curve for elastomeric foam.

STRESS

Densification

Plateau: Elastic buckling of cell walls

Cell wall bending STRAIN

Figure 5-15

Typical Compressive Stress-Strain Curve

Three stages can be distinguished during compression: At small strains (< 5%) the foam deforms in a linear elastic manner, due to cell wall bending. This is followed by a plateau of deformation at almost constant stress, caused by the elastic buckling of the columns or plates which make up the cell edges or walls. In closed cells, the enclosed gas pressure and membrane stretching increase the level and slope of the plateau.

CHAPTER 55 Model Generation

Finally, a region of densification occurs, where the cell walls crush together, resulting in a rapid increase of compressive stress. Ultimate compressive nominal strains of 0.7 to 0.9 are typical.

STRESS

The tensile deformation mechanisms for small strains are similar to the compression mechanisms but differ for large strains. The figure shows a typical tensile stress-strain curve.

Cell wall alignment

Cell wall bending STRAIN

Figure 5-16

Typical Tensile Stress-Strain Curve

There are two stages during tension: At small strains the foam deforms in a linear, elastic manner, due to cell wall bending, similar to that in compression. The cell walls rotate and align, resulting in rising stiffness. The walls are substantially aligned at a tensile strain of about 1/3. Further stretching results in increased axial strains in the walls. At small strains for both compression and tension, the average experimentally observed Poisson's ratio, ν, of foams is 1/3. At larger strains it is commonly observed that Poisson's ratio is effectively zero during compression - the buckling of the cell walls does not result in any significant lateral deformation. However, during tension, ν is nonzero, which is a result of the alignment and stretching of the cell walls. The manufacture of foams often results in cells with different principal dimensions. This shape anisotropy results in different loading responses in different directions. However, the foam model does not take this kind of initial anisotropy into account. Determination of Foam Material Parameters

The response of the material is defined by the parameters in the strain energy function, U, so that it is necessary to determine these parameters to use the foam model. MSC SimXpert contains a capability for obtaining the μi, αi and βi for the foam model with up to six terms (N=6) directly from test data. It is usually best to obtain data from several experiments involving different kinds of deformation, over

56 Modeling Guide

the range of strains of interest in the actual application, and to use all of these data to determine the parameters. Since the properties of foam materials can vary significantly from one batch to another, all of the experiments should be performed on specimens taken from the same batch of material or to use MSC.Stocastics in combination with SOL 600. Uniaxial, Equibiaxial and Planar Deformations

The deformation modes are characterized in terms of the principal stretches, λi, and the volume ratio, J. The elastomeric foams are not incompressible, so that J = λ1λ2λ3 != 1. The transverse stretches, λ2 and/or λ3, are independently specified in the test data either as individual values from the measured lateral deformations or through the definition of an effective Poisson’s ratio. Uniaxial mode: λ1=λU, λ2=λ3, J=λUλ22 Equibiaxial mode: λ1=λ2=λB, J=λB2λ3 Planar mode: λ1=λP, λ2=1, J=λPλ3 The three deformation modes above use a single form of the nominal stress-stretch relation, N ∂U 2 TL = = ------∂ λL λL

 i=1

μi αi – α i β i  -----  λ – J  αi  L

(5-60)

where TL is the nominal stress and LL is the stretch in the direction of loading. Because of the compressible behavior, the planar mode does not result in a state of pure shear. In fact, if the effective Poisson’s ratio is zero, planar deformation is identical to uniaxial deformation. Simple Shear Deformation

Simple shear is described by the deformation gradient

1 γ 0 F = 01 0 0 01

(5-61)

where γ is the shear strain. For this deformation, J=det F =1. A schematic illustration of simple shear deformation is shown in Figure 5-17. The nominal shear stress TS is:

CHAPTER 57 Model Generation

N 2   μi αi   2γ   ----- λ – 1   -----------------------------------  j α 2   2   i  j = 1  2  λ j – 1 – γ i = 1

∂U T = = S ∂γ





(5-62)

where λj= are the principal stretches in the plane of shearing, related to the shear strain, γ, by:

λ 1, 2 =

2 2 γ γ 1 + ----- ± γ 1 + ----2 4

(5-63)

.

2F E2

atan γ

E3

E1

Figure 5-17

Simple Shear Test

The stretch in the direction perpendicular to the shear plane is L3=1. The transverse (tensile) stress, TT, developed during simple shear deformation due to the Poynting effect, is 2 2  N  2  λ j – 1 μi αi     ∂U   ----- λ – 1  TT = =  ---------------------------------------- j  ∂ε 4 2 2 α  2λ – λ ( γ + 2 )  i j  j = 1 j i=1





(5-64)

Volumetric Deformation

The volumetric deformation mode consists of all principal stretches being equal, λ1=λ2=λ3=λV, J=λV3. The pressure-volumetric ratio relation is α  -i  – α i β i μ  ---i 3 -----  J – J  αi    =1  N

–p =

∂U 2 = --∂J J

 i

(5-65)

58 Modeling Guide

A volumetric compression test is illustrated Figure 5-18. The pressure exerted on the foam specimen is the hydrostatic pressure of the fluid and the decrease in the specimen volume is equal to the additional fluid entering the pressure chamber. The specimen is sealed against fluid penetration.

F

F

E1 (a)

E3

E2

Figure 5-18

(b)

F

Volumetric Compression Test Setup

Difference in Compression and Tension Deformation

For small strains (< 5%), foams behave similarly for both compression and tension. However, we have seen that at large strains, the deformation mechanisms differ for compression (buckling and crushing) and tension (alignment and stretching). Accurate modeling with the FOAM option therefore requires that the experimental data used to define the material parameters correspond to the dominant deformation modes of the actual problem being analyzed. If compression dominates in the problem, the pertinent tests are: • Uniaxial compression. • Simple shear.

ν ≠ 0 ). Volumetric compression (if Poisson’s ratio ν ≠ 0 ).

• Planar compression (if Poisson’s ratio •

If tension dominates, the pertinent tests are: • Uniaxial tension. • Simple shear.

ν ≠ 0 ). Planar tension (if Poisson’s ratio ν ≠ 0 ).

• Biaxial tension (if Poisson’s ratio •

CHAPTER 59 Model Generation

Lateral strain data can also be used to define the compressibility of the foam. Measurement of the lateral strains may make other tests redundant, e.g., providing lateral strains for a uniaxial test eliminates the need for a volumetric test. The foam model may not accurately fit Poisson's ratio if it varies significantly between compression and tension. Experimental Data Fitting Least Squares Fit

The equations derived above for TU, TB, and TS, with the assumption of material incompressibility, allow the material parameters Cij and μi, αi to be determined from the experimentally measured stressstrain relationships in the uniaxial, equibiaxial, and planar loading tests. A least squares fit, which minimizes the relative error in stress, is used for this purpose. The equation for TS alone will not determine the constants uniquely. The planar test data input must be augmented by either or both of the other two types of test data to determine the material parameters. The Ogden potential is linear in the coefficients μi but strongly nonlinear in terms of the exponents αi, thus necessitating use of a nonlinear least squares procedure. For the nominal stress-nominal strain data pairs, the error measure, E, is minimized by E = sum(i=1to n)(1-Tith/Titest2), where Titest is a stress value from the test data and Tith comes from one of the nominal stress expressions derived above. The foam parameters μi, αi, βi are determined from the experimentally measured stress-strain relationships in the various loading tests described above. A least squares fit, which minimizes the relative error in stress, is used for this purpose. The foam potential is linear in the coefficients μi but strongly nonlinear in terms of the exponents αi and βi thus necessitating use of a nonlinear least squares procedure. For the n nominal stress-nominal strain data pairs, the error measure E is minimized by E = sum(i=1to n)(1-Tith/Titest2, where Titest is a stress value from the test data and Tith comes from one of the nominal stress expressions derived above. Minimizing the relative error in stress implies that the error in slope (modulus) is minimized; minimization of the absolute error would decrease the error at larger strains, at the expense of the accuracy at small strains. Alternative Method for Determination of Constants for Moderate Strains

Since the polynomial form with N=1 is very commonly used for cases where the nominal strain is not too large, an alternative method of finding the material constants, assuming incompressibility, is to use the uniaxial test data as follows. The nominal strain in the direction of loading in the uniaxial test is εU=λU-1. Expanding the equation for TB in terms of εU, using the Mooney-Rivlin form, and neglecting terms of higher than second-order in εU, gives TU=6εU(C10+C01 -(C10+2C01)εU).

60 Modeling Guide

This is a parabola: the slope of this curve at the origin (the effective Young’s modulus at zero strain) is 6(C10+C01); this slope, together with the second-order term -6(C10+2C01)εU2, defines the constants C10 and C01. If compressibility should be modeled, then, under pure pressure loading, the compressible model with N=1 gives, to first-order in the volumetric strain εV=3ε11, p=-(2 / D1)εV, so that, at small nominal strains, the bulk modulus is defined as: K=(2 / D1) Hyperelastic Models in MD Nastran

Various options are provided for defining the material properties. The first (available in both MSC SimXpert and MD Nastran) is to give the parameters of the polynomial form parameters of the Ogden form

N, A ij and D i , or the

N, μ i, α i and D i as functions of the temperature. The second is to give

the value of N, and give experimental stress-data for up to four simple tests: uniaxial, equilibrium, planar and, if the material is compressible for volumetric compression test. MD Nastran Implicit Nonlinear will then compute the

Aij or [ μ i, α i ] and the D i . This method is available for N = 1 and N=2 for the

polynomial form and up to N = 6 for the Ogden form, and does not allow the properties to be temperature dependent. In either case, you should be careful about defining the

A ij or [ μ i, α i ] : especially when N > 1, the

behavior at higher strains is strongly sensitive to the values of the A ij or [ μ i,

αi ] , and unstable material

behavior may result if these values are not correctly defined. When some of the coefficients are strongly negative, instability at higher strain levels is likely to occur. Because the properties of rubber-like materials can vary significantly from one sample to another, it is important that test data are taken from experiments on the same sample (or samples cut from the same sheet), regardless whether the

A ij or [ μ i, α i ] are computed by the user or by the built-in method.

This material option can be used by itself, or can be combined with viscoelasticity to define time dependent hyperelastic behavior. It cannot be combined with other material options such as plasticity or creep. It may be used with the pure displacement formulation elements or with the “hybrid” (mixed formulation) elements. Because elastomeric materials are usually almost completely incompressible, fully integrated pure displacement method elements are not recommended for use with this material, except for plane stress cases. If fully or selectively reduced integration displacement method elements are used with the almost incompressible form of this material model in anything except plane stress analysis, a penalty method is used to impose the incompressibility constraint. This can sometimes lead to numerical difficulties, and the fully or selectively reduced integrated “hybrid” formulation elements are therefore recommended.

CHAPTER 61 Model Generation

Specifying Hyperelastic Material Entries

Nonlinear hyperelastic materials are characterized in MD Nastran with the following Bulk Data entries: .

Entry MATHP MATHE

Description Specifies material properties for use in fully nonlinear (i.e., large strain and large rotation) hyperelastic analysis of rubber-like materials (elastomers). Specifies hyperelastic (rubber-like) material properties for nonlinear (large strain and large rotation) analysis in (SOL 600) only.

References • MATHP in the MD NASTRAN QRG • MATHE in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define a hyperelastic material in SimXpert: 1. Select Materials and Properties>General Hyperelastic or Mooney-Rivlin or Odgen/Hyperfoam or Arruda-Boyce/Gent. 2. Select Coefficients or Test Data as the Data Type. 3. Enter parameter values. 4. Click OK. Hyperelastic material models require the following material data via the Input Properties subform on the Materials Application form. General Hyperelastic

Hyperelastic -General Hyperelastic

Description

Data Type

Coefficient

Density

Defines the mass density which is an optional property.

Destort. Def. Coeff. A10, A01

Strain energy densities as a function of the strain invariants in the material. May vary with temperature via a defined material field. This option consolidates several of the MSC.Marc hyperelastic material models.

Data Type

Test Data

Density

Defines the mass density which is an optional property.

62 Modeling Guide

Hyperelastic -General Hyperelastic

Description

Simple Tension/Compress. Data

Table identification number of a TABLES1 entry that contains simple tension/compression data to be used in the estimation of the material constants Aij. xi values in the TABLES1 entry must be stretch ratios l ⁄ l 0 and yi values must be values of the engineering stress F ⁄ A0 . Stresses are negative for compression and positive for tension. (Integer > 0 or blank)

Equivalent Tension Data

Table identification number of a TABLES1 entry that contains equibiaxial tension data to be used in the estimation of the material constants Aij. xi values in the TABLES1 entry must be stretch ratios l ⁄ l0 . yi values must be values of the engineering stress F ⁄ A0 . l is the current length, F is the current force, l 0 is the initial length and A0 is the cross-sectional area. In the case of pressure of a spherical membrane, the engineering stress is given 2 by Pr 0 λ ⁄ 2t 0 where P = current value of the pressure and r 0, t 0 = initial radius and thickness. (Integer > 0 or blank)

Simple Shear Data

Table identification number of a TABLES1 entry that contains simple shear data to be used in the estimation of the material constants Aij. xi values in the TABLES1 entry must be values of the shear tangent γ and yi values must be values of the engineering shear stress F ⁄ A 0 . (Integer > 0 or blank)

Pure Shear Data

Table identification number of a TABLES1 entry that contains pure shear data to be used in the estimation of the material constants Aij. xi and yi values in the TABLES1 entry must be stretch ratios λ 1 = l ⁄ l 0 and values of the nominal stress F ⁄ A 0 . l is the current length, F is the current force, l 0 and A0 are the initial length and cross-sectional area, respectively in the 1-direction. (Integer > 0 or blank)

Pure Volum. Compress. Data

Table identification number of a TABLES1 entry that contains pure volumetric compression data to be used in the estimation of the material constants Di. xi values in the TABLES1 entry must 3 be values of the volume ratio J = λ where λ = l ⁄ l0 is the stretch ratio in all three directions; yi values must be values of the pressure, assumed positive in compression. (Integer > 0 or blank)

Mooney-Rivlin

Hyperelastic -Mooney-Rivlin

Description

Data Type

Coefficient

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the mass density which is an optional property.

CHAPTER 63 Model Generation

Hyperelastic -Mooney-Rivlin

Description

Destort. Def. Coeff. A10, A01

Strain energy densities as a function of the strain invariants in the material. May vary with temperature via a defined material field. This option consolidates several of the MSC.Marc hyperelastic material models.

Data Type

Test Data

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the mass density which is an optional property.

Simple Tension/Compress. Data

Table identification number of a TABLES1 entry that contains simple tension-compression data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l0 and y-values must be values of the engineering stress F ⁄ A0 . l0 is the initial length and A0 is the initial cross-sectional area.

Equivalent Tension Data

Table identification number of a TABLES1 entry that contains equibiaxial tension data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l 0 and y-values must be values of the engineering stress F ⁄ A 0 . l 0 is the initial length and & is the initial cross-sectional area. (Integer > 0 or blank)

Simple Shear Data

Table identification number of a TABLES1 entry that contains simple shear data to be used in the estimation of the material constants Cij or μ k , α k , and βk . The x-values in the TABLES1 entry must be values of the shear strain and y-values must be values of the engineering shear stress. (Integer > 0 or blank)

Pure Shear Data

Table identification number of a TABLES1 entry that contains pure shear data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x and y values in the TABLES1 entry must be stretch ratios λ 1 = l ⁄ l 0 and the values of the nominal stress F ⁄ A0 . l 0 and A 0 are the initial length and cross-sectional area, respectively, in the l-direction.

Pure Volum. Compress. Data

Table identification number of a TABLES1 entry that contains pure volumetric compression data to be used in the estimation of the material constant K. The x-values in the TABLES1 entry must 3 be values of the volume ration J = λ where λ = l ⁄ l 0 is the stretch ratio in all three directions; y-values must be values of the pressure, assumed positive in compression.

Ogden

64 Modeling Guide

Hyperelastic-Ogden

Description

Data Type

Coefficient

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the material mass density.

Number of terms

The number of terms in the Ogden expression. There can be from 1 to 5 terms.

Ogden Terms, Modulus (k)

μ k in the Ogden equation.

Ogden Terms, Deviatoric Exponent (k)

α k in the Ogden equation.

Data Type

Test Data

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the mass density which is an optional property.

Number of terms

The number of terms in the Ogden expression. There can be from 1 to 5 terms.

Simple Tension/Compress. Data

Table identification number of a TABLES1 entry that contains simple tension-compression data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l0 and y-values must be values of the engineering stress F ⁄ A 0 . l 0 is the initial length and A 0 is the initial cross-sectional area.

Equivalent Tension Data

Table identification number of a TABLES1 entry that contains equibiaxial tension data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l 0 and y-values must be values of the engineering stress F ⁄ A0 . l 0 is the initial length and & is the initial cross-sectional area.

CHAPTER 65 Model Generation

Hyperelastic-Ogden

Description

Simple Shear Data

Table identification number of a TABLES1 entry that contains simple shear data to be used in the estimation of the material constants Cij or μ k , α k , and βk . The x-values in the TABLES1 entry must be values of the shear strain and y-values must be values of the engineering shear stress. (Integer > 0 or blank)

Pure Shear Data

Table identification number of a TABLES1 entry that contains pure shear data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x and y values in the TABLES1 entry must be stretch ratios λ 1 = l ⁄ l 0 and the values of the nominal stress F ⁄ A0 . l 0 and A 0 are the initial length and cross-sectional area, respectively, in the l-direction.

Pure Volum. Compress. Data

Table identification number of a TABLES1 entry that contains pure volumetric compression data to be used in the estimation of the material constant K. The x-values in the TABLES1 entry must 3 be values of the volume ration J = λ where λ = l ⁄ l 0 is the stretch ratio in all three directions; y-values must be values of the pressure, assumed positive in compression.

Hyperfoam

Hyperelastic-Hyperfoam

Description

Data Type

Coefficient

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the material mass density.

Number of terms

The number of terms in the Ogden expression. There can be from 1 to 5 terms.

Hyperfoam Terms, Modulus (k)

u k in the Foam equation.

Hyperfoam Terms, Deviatoric Exponent (k)

α k in the Foam equation.

Hyperfoam Terms, Volumetric Exponent (k)

β k in the Foam equation.

Data Type

Test Data

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

Defines the mass density which is an optional property.

Number of terms

The number of terms in the Ogden expression. There can be from 1 to 5 terms.

66 Modeling Guide

Hyperelastic-Hyperfoam

Description

Simple Tension/Compress. Data Table identification number of a TABLES1 entry that contains simple tension-compression data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l0 and y-values must be values of the engineering stress F ⁄ A0 . l0 is the initial length and A 0 is the initial cross-sectional area. Equivalent Tension Data

Table identification number of a TABLES1 entry that contains equibiaxial tension data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l 0 and y-values must be values of the engineering stress F ⁄ A0 . l 0 is the initial length and & is the initial cross-sectional area.

Simple Shear Data

Table identification number of a TABLES1 entry that contains simple shear data to be used in the estimation of the material constants Cij or μ k , α k , and β k . The x-values in the TABLES1 entry must be values of the shear strain and y-values must be values of the engineering shear stress. (Integer > 0 or blank)

Pure Shear Data

Table identification number of a TABLES1 entry that contains pure shear data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x and y values in the TABLES1 entry must be stretch ratios λ 1 = l ⁄ l0 and the values of the nominal stress F ⁄ A0 . l 0 and A 0 are the initial length and cross-sectional area, respectively, in the l-direction.

Pure Volum. Compress. Data

Table identification number of a TABLES1 entry that contains pure volumetric compression data to be used in the estimation of the material constant K. The x-values in the TABLES1 entry must be 3

values of the volume ration J = λ where λ = l ⁄ l0 is the stretch ratio in all three directions; y-values must be values of the pressure, assumed positive in compression. Arruda-Boyce

Hyperelastic-Arruda-Boyce

Description

Data Type

Coefficient

Bulk Modulus (K)

Defines the Bulk Modulus.

Density

This defines the material mass density.

Arruda-Boyce Material Const. Number of statistic Links

CHAPTER 67 Model Generation

Hyperelastic-Arruda-Boyce

Description

NKT

Chain density times Boltzmann constant times temperature.

Chain Length

Average chemical chain cross length.

Coefficient of Thermal Expansion

Defines the instantaneous coefficient of thermal expansion. This property is optional. May vary with temperature via a defined material field

Gent

Hyperelastic-Gent

Description

Data Type

Coefficient

Bulk Modulus

Defines the Bulk Modulus.

Density

This defines the material mass density.

Tensile Modulus

Defines standard tension modulus (E).

I 1* Maximum 1st Invariant

Defines I 1

Data Type

Test Data

Bulk Modulus

Defines the Bulk Modulus.

Density

This defines the material mass density.

Tensile Modulus

Defines standard tension modulus (E).

I 1* Maximum 1st Invariant

Defines I 1

*

*

= I1 – 3 .

= I1 – 3 .

Simple Tension/Compress. Data Table identification number of a TABLES1 entry that contains simple tension-compression data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l0 and y-values must be values of the engineering stress F ⁄ A 0 . l 0 is the initial length and A 0 is the initial cross-sectional area. Equivalent Tension Data

Table identification number of a TABLES1 entry that contains equibiaxial tension data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x-values in the TABLES1 entry must be stretch ratios l ⁄ l 0 and y-values must be values of the engineering stress F ⁄ A0 . l0 is the initial length and & is the initial cross-sectional area.

68 Modeling Guide

Hyperelastic-Gent

Description

Simple Shear Data

Table identification number of a TABLES1 entry that contains simple shear data to be used in the estimation of the material constants Cij or μ k , α k , and β k . The x-values in the TABLES1 entry must be values of the shear strain and y-values must be values of the engineering shear stress. (Integer > 0 or blank)

Pure Shear Data

Table identification number of a TABLES1 entry that contains pure shear data to be used in the estimation of the material constants Cij, μ k , α k , and β k . The x and y values in the TABLES1 entry must be stretch ratios λ 1 = l ⁄ l0 and the values of the nominal stress F ⁄ A0 . l 0 and A 0 are the initial length and cross-sectional area, respectively, in the l-direction.

Pure Volum. Compress. Data

Table identification number of a TABLES1 entry that contains pure volumetric compression data to be used in the estimation of the material constant K. The x-values in the TABLES1 entry must be 3 values of the volume ration J = λ where λ = l ⁄ l0 is the stretch ratio in all three directions; y-values must be values of the pressure, assumed positive in compression.

Viscoelastic The material models discussed in previous sections are considered to be time independent. However, rubber materials often show a rate-dependent behavior and can be modeled as viscoelastic materials. Viscoelasticity can be applied: • To determine the current state of deformation based on the entire time history of loading. • To characterize small strain and large strain problems. • With other material options for linear elastic response (small strain) and hyperelastic response

(large strain). • To include temperature dependencies. • For isotropic, anisotropic, and incompressible materials. Small Strain Viscoelasticity

In the stress relaxation form, the constitutive relation can be written as a hereditary integral formulation t σ ij ( t ) =

 0

dε kl ( τ ) G ijkl ( t – τ ) ------------------ dτ + G ijkl ( t )ε kl ( 0 ) dτ

(5-66)

CHAPTER 69 Model Generation

The functions G ijkl are called stress relaxation functions. They represent the response to a unit applied strain and have characteristic relaxation times associated with them. The relaxation functions for materials with a fading memory can be expressed in terms of Prony or exponential series. N ∞ G ijkl ( t ) = G ijkl +



n n G ijkl exp ( – t ⁄ λ )

(5-67)

n=1 in which

n

n

G ijkl is a tensor of amplitudes and λ is a positive time constant (relaxation time). In the

current implementation, it is assumed that the time constant is isotropic. In Equation (5-67),

∞ G ijkl

represents the long term modulus of the material. The short term moduli (describing the instantaneous elastic effect) are then given by N ∞ 0 G ijkl = G ijkl ( 0 ) = G ijkl +



n G ijkl

(5-68)

n=1 The stress can now be considered as the summation of the stresses in a generalized Maxwell model (Figure 5-19) N ∞ σ ij ( t ) = σ ij ( t ) +



n σ ij ( t )

(5-69)

n=1 where ∞ ∞ σ ij = G ijkl ε kl ( t ) t n σ = ij

 0

G

n dε kl ( τ ) n exp [ – ( t – τ ) ⁄ λ ] ------------------ dτ ijkl dτ

(5-70)

(5-71)

70 Modeling Guide

η1

η2

ηi

ε ηE

q1

E1

q2 E2

qi Ei

E0 τi = ηi/Ei

Figure 5-19

The Generalized Maxwell or Stress Relaxation Form

For integration of the constitutive equation, the total time interval is subdivided into a number of subintervals ( t m – 1, t m ) with time-step

h = t m – t m – 1 . A recursive relation can now be derived

expressing the stress increment in terms of the values of the internal stresses

σ ijn at the start of the

interval. With the assumption that the strain varies linearly during the time interval h, we obtain the increment stress-strain relation as ∞ Δσ ij ( t m ) = G ijkl +

N

N n

n β ( h )G ijkl Δε kl –

 n=1



n n α ( h )σ ij ( t m – h )

(5-72)

n=1

where n α n ( h ) = 1 – exp ( – h ⁄ λ )

(5-73)

and n n n β ( h ) = α ( h )λ ⁄ h

(5-74)

In MD Nastran Implicit Nonlinear, the incremental equation for the total stress is expressed in terms of the short term moduli (See Equation (5-68)). N 0 Δσ ( t ) = G – ij m ijkl



N n

n { 1 – β ( h ) }G Δε ( t ) – ijkl kl m

n=1



n n α ( h )σ ( t – h ) ij m

(5-75)

n=1

Note that the set of equations given by Equation (5-75) can directly be used for both anisotropic and isotropic materials. Isotropic Viscoelastic Material

CHAPTER 71 Model Generation

For an isotropic viscoelastic material, MD Nastran Implicit Nonlinear assumes that the deviatoric and volumetric behavior are fully uncoupled and that the behavior can be described by a time dependent shear and bulk modules. The bulk moduli is generally assumed to be time independent; however, this is an unnecessary restriction of the general theory. Both the shear and bulk moduli can be expressed in a series

G(t) = G

N

∞

+



n n G exp  – t ⁄ λ d

(5-76)

n n K exp  – t ⁄ λ v   

(5-77)

n=1

K( t) = K

∞

N +

 n=1

with short term values given by N G0 = G∞ +



Gn

(5-78)

Kn

(5-79)

n=1 N K0 = K∞ +

 n=1

Let the deviatoric and volumetric component matrices 4 ⁄ 3 –2 ⁄ 3 – 2 ⁄ 3 –2 ⁄ 3 4 ⁄ 3 – 2 ⁄ 3 π d = –2 ⁄ 3 –2 ⁄ 3 4 ⁄ 3 0 0 0 0 0 0 0 0 0

0 0 0 1 0 0

0 0 0 0 1 0

0 0 0 0 0 1

π d and π v be given by

72 Modeling Guide

1 1 πv = 1 0 0 0

1 1 1 0 0 0

1 1 1 0 0 0

0 0 0 0 0 0

0 0 0 0 0 0

0 0 0 0 0 0

The increment set of equations is then given by Nd   n n  0 Δσ ( t m ) =  G – [ 1 – β d ( h ) ]G πd Δε ( t m )     n=1 Nv   n n  0 [ 1 – βv ( h ) ]K π v Δε ( t m ) K –     n=1 Nv Nd n n n n – α v ( h )σ v ( t m – h ) α d ( h )σ d ( t m – h ) – n=1 n=1







(5-80)



and n n n n n Δσ d ( t m ) = β d ( h )G π d Δε ( t m ) – α d ( h )σ d ( t m – h ) n n n n n Δσ v ( t m ) = β v ( h )K π v Δε ( t m ) – α v ( h )σ v ( t m – h )

(5-81)

Note that the deviatoric and volumetric response are fully decoupled. Note that the algorithm is exact for linear variations of the strain during the increment. The algorithm is implicit; hence, for each change in time-step, a new assembly of the stiffness matrix is required. Anisotropic Viscoelastic Material Equation (5-75) can be used for the analysis of anisotropic viscoelastic materials.

Also, a complete set of moduli (21 components) can be specified in the HOOKVI user subroutine. Referencing a local coordinate system or use of the ORIENT user subroutine can be used to define a preferred orientation both for the short time moduli Incompressible Isotropic Viscoelastic Materials

0

n

G ijkl and the amplitude functions G ijkl .

CHAPTER 73 Model Generation

Incompressible elements in MD Nastran Implicit Nonlinear allow the analysis of incompressible and nearly incompressible materials in plane strain, axisymmetric and three-dimensional problems. The incompressibility of the element is simulated through the use of an perturbed Lagrangian variational principle based on the Herrmann formulation. The constitutive equation for a material with no time dependence in the volumetric behavior can be expressed as N   n n   0 1 Δσ ij ( t m ) = 2  G ijkl – [ 1 – β ( h ) ]G ijkl  Δε kl ( t m ) – --- Δε pp ( t m )δ kl 3     n =N 1 n n 1 – α ( h ) ( σ′ij ) ( t m ) + --- σ kk δ ij 3 n=1





0 Δσ pp ( t m ) = 3K Δε pp ( t m )

(5-82) (5-83)

The hydrostatic pressure term is used as an independent variable in the variational principle. The Herrmann pressure variable is now defined in the same way as in the formulation for time independent elastic materials. σ

pp H = ------------------------------0 2G ( 1 + ν 0 )

(5-84)

The constitutive Equation (5-82) and Equation (5-83) can then be rewritten N

e

Δσ ij ( t m ) = 2G ( Δε ij + ν∗ Hδ ij ) –

 αn ( h ) ( σ′ij )

n

( tm – h )

(5-85)

n=1

where N

Ge = G0 –

 [ 1 – βn ( h )G n ]

(5-86)

n=1 0

0

e

0

G ( 1 + ν ) – G ( 1 – 2ν ) ν∗ = ---------------------------------------------------------------e 3G Large Strain Viscoelasticity

(5-87)

74 Modeling Guide

For an elastomeric time independent material, the constitutive equation is expressed in terms of an energy function W . For a large strain viscoelastic material, Simo generalized the small strain viscoelasticity material behavior to a large strain viscoelastic material. The energy functional then becomes N n ψ ( E ij Q ij )

N



0

= ψ ( E ij ) –

n Q ij E ij

+

n=1

where

 ψI ( Qij ) n

n

(5-88)

n=1 n

0

E ij are the components of the Green-Lagrange strain tensor, Q ij internal variables and ψ the

elastic strain energy density for instantaneous deformations. In MD Nastran Implicit Nonlinear, it is 0

assumed that ψ = W , meaning that the energy density for instantaneous deformations is given by the third order James Green and Simpson form or the Ogden form. The components of the second Piola-Kirchhoff stress then follow from

S ij

∂ψ ∂ψ 0 = --------- = --------- – ∂E ij ∂E ij

N

 Qij n

(5-89)

n=1

The energy function can also be written in terms of the long term moduli resulting in a different set of n

internal variables

T ij

n ψ ( E ij, T ij )

ψ∞(E

N

=

ij )

+

 Tij Eij n

(5-90)

n=1 ∞

where ψ is the elastic strain energy for long term deformations. Using this energy definition, the stresses are obtained from

S ij

∂ψ ∞ ( E ) = ------------------- + ∂E ij

N

 Tij n

(5-91)

n=1

Observing the similarity with the equations for small strain viscoelasticity the internal variables can be obtained from a convolution expression n

T ij = where

0 S· ij ( τ )exp [ –( t – τ ) ⁄ λ t

n

n

n

]dτ

S ij are internal stresses obtained from energy functions.

(5-92)

CHAPTER 75 Model Generation

n ∂ψ n S ij = --------∂E ij

(5-93)

Let the total strain energy be expressed as a Prony series expansion N

ψ = ψ∞ +

 ψn exp ( –t ⁄ λ n )

(5-94)

n=1

If, in the energy function, each term in the series expansion has a similar form, Equation (5-94) can be rewritten N

ψ = ψ∞ +

 δ n ψ0 exp ( –t ⁄ λn )

(5-95)

n=1

where

n

δ is a scalar multiplier for the energy function based on the short term values.

The stress-strain relation is now given by N

S ij ( t ) =

∞ S ij ( t )

+

 Tij ( t ) n

(5-96)

n=1 N   ∞ ∂ψ ∂ψ 0  n S ij = ---------- =  1 –  δ  --------∂E ij ∂E ij  n=1 

(5-97)

t n T ij

=

δ

n 0 S ij ( t )exp [ – ( t

n

– τ ) ⁄ λ ]dτ

(5-98)

0

Analogue to the derivation for small strain viscoelasticity, a recursive relation can be derived expressing the stress increment in terms of values of the internal stresses at the start of the increment.

76 Modeling Guide

The equations are reformulated in terms of the short time values of the energy function N   0 0  ΔS ij ( t m ) =  1 –  1 – β n ( h ) δ n { S ij ( t m ) – S ij ( t m – h ) }  n =N 1 

 α n Sij ( tm – h ) n

–

n=1

(5-99) 0

n

n

ΔS ij ( t m ) = β n ( h )δ n [ S ij ( t m ) – S ij ( t m – h ) ] – α n ( h )S ij ( t m – h )

(5-100)

It is assumed that the viscoelastic behavior in MD Nastran Implicit Nonlinear acts only on the deviatoric behavior. Viscoelastic Models in MD Nastran

MD Nastran Implicit Nonlinear has two models that represent viscoelastic materials. The first can be defined as a Kelvin-Voigt model. The latter is a general hereditary integral approach. Kelvin-Voigt Model

The Kelvin model allows the rate of change of the inelastic strain to be a function of the total stress and previous strain. The Kelvin material behavior (viscoelasticity) is modeled by assuming an additional creep strain

k

ε ij ,

governed by

d- k k ---ε = Aijkl σ′kl – B ijkl ε kl dt ij where

(5-101)

A and B may be defined in the user subroutine CRPVIS and the total strain is

ε ij = ε ije + ε ijp + ε ijc + ε ijk + εth ij

(5-102)

εth ij = thermal strain components

(5-103)

ε ije = elastic strain components (instantaneous response)

(5-104)

ε ijp = plastic strain components

(5-105)

ε ijc = creep strains defined via the CRPLAW and VSWELL user subroutines

(5-106)

CHAPTER 77 Model Generation

ε ijk = Kelvin model strain components as defined above

(5-107)

The CRPVIS user subroutine is called at each integration point of each element when the Kelvin model is used. Use the NLPARM option and set a nonzero time increment to define the time step and to set the tolerance control for the maximum strain in any increment. This option allows Maxwell models to be included in series with the Kelvin model. Hereditary Integral Model

The stress-strain equations in viscoelasticity are not only dependent on the current stress and strain state (as represented in the Kelvin model), but also on the entire history of development of these states. This constitutive behavior is most readily expressed in terms of hereditary or Duhamel integrals. These integrals are formed by considering the stress or strain build-up at successive times. Two equivalent integral forms exist: the stress relaxation form and the creep function form. In MD Nastran Implicit Nonlinear, the stress relaxation form is used. The viscoelasticity option in MD Nastran Implicit Nonlinear can be used for both the small strain and large strain Mooney, Ogden, Arruda Boyce, and Gent material stress-relaxation problems. A description of these models is as follows: Experimental Determination of Viscoelastic Material Parameters

The free energy function versus time data being used for large strain viscoelasticity can be generated by fitting experimental data provided the following two tests are done: 1. Standard quasi-static tests (tensile, planar-shear, simple-shear, equi-biaxial tension, volumertic) to determine the elastomer free energy

0

W constants.

2. Standard relaxation tests to obtain stress versus time. Temperature Dependence of Viscoelastic Materials

The rate processes in many viscoelastic materials is known to be highly sensitive to temperature changes. Such temperature-dependent properties cannot be neglected in the presence of any appreciable temperature variation. For example, there is a large class of polymers which are adequately represented by linear viscoelastic laws at uniform temperature. These polymers exhibit an approximate translational shift of all the characteristic response functions with a change of temperature, along a logarithmic time axis. This shift occurs without a change of shape. These temperature-sensitive viscoelastic materials are characterized as Thermo-Rheologically Simple. A “reduced” or “pseudo” time can be defined for the materials of this type and for a given temperature field. This new parameter is a function of both time and space variables. The viscoelastic law has the same form as one at constant temperature in real time. If the shifted time is used, however, the transformed viscoelastic equilibrium and compatibility equations are not equivalent to the corresponding elastic equations.

78 Modeling Guide

In the case where the temperature varies with time, the extended constitutive law implies a nonlinear dependence of the instantaneous stress state at each material point of the body upon the entire local temperature history. In other words, the functionals are linear in the strains but nonlinear in the temperature. The time scale of experimental data is extended for Thermo-Rheologically Simple materials. All characteristic functions of the material must obey the same property. The shift function is a basic property of the material and must be determined experimentally. As a consequence of the shifting of the mechanical properties data parallel to the time axis, the values of the zero and infinite frequency complex moduli do not change due to shifting. Hence, elastic materials with temperature-dependent characteristics neither belong to nor are consistent with the above hypothesis for the class of Thermo-Rheologically Simple viscoelastic solids. In addition to the Thermo-Rheologically Simple material behavior variations of initial stress-strain moduli

0

Gijkl , the temperature of the other mechanical properties (coefficient of thermal expansion, etc.)

due to changes in temperature can be specified. Note, however, that only the instantaneous moduli are effected. Hence, the long term moduli given by N ∞ G ijkl

=

0 G ijkl ( t )

–

 Gijkl n

(5-108)

n=1

can easily become negative if the temperature effects are not defined properly. The effect of temperature, θ, on the material behavior is introduced through the dependence of the elastic modulus, G, on temperature, and through a reduced time concept: t   ·  τ = G  γ +  g ( ξ ( t ) – ξ ( s ) )γ ( s )ds   0

(5-109)

where G=G(θ), and xi(t) is the reduced time, defined by t

ξ(t ) =

ds

 A-----------------(θ( s) )

(5-110)

0

where A(θ(t)) is the shift function at time t. Often the shift function is approximated by the Williams Landell Ferry (WLF) form:

C1 ( θ – θ0 ) log ( A ) = – -------------------------------C2 + ( θ – θ0 )

(5-111)

CHAPTER 79 Model Generation

where C1, C2 and θ0 are constants (θ0 is the “glassy transition” temperature). Narayanaswamy Model The annealing of flat glass requires that the residual stresses be of an acceptable magnitude, while the specification for optical glass components usually includes a homogenous refractive index. The design of heat treated processes can be accomplished using the Narayanaswamy model. This allows you to study the time dependence of physical properties (for example, volumes) of glass subjected to a change in temperature. For more information pertaining to the Narayanaswamy Model, see MSC.Marc Volume A: Theory and User Information, Chapter 7 Material Library. Specifying Viscoelastic Material Entries

The viscoelastic MATVE and MATTVE material options are provided for cases where dissipative losses caused by “viscous” (internal friction) effects in materials must be modeled. For time domain analysis, this option is used with an elastic model to define classical linear, small strain, viscoelastic behavior, or with hyperelastic or foam models to define finite linear, large deformation, viscoelastic behavior. As described in the previous section, viscoelastic relaxation data can be fit using the experimental data fitting (EDF) capability available in SimXpert. Entry

Description

MATVE

Specifies isotropic visco-elastic material properties to be used for quasi-static or dynamic analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

MATTVE

Specifies temperature-dependent visco-elastic material properties in terms of Thermo-Rheologically Simple behavior to be used for quasi-static or transient dynamic analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

References • MATVE in the MD NASTRAN QRG. • MATTVE in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define a viscoelastic material in SimXpert: 1. Select Materials and Properties>Isotropic>Advanced>Add Constitutive Model>Visco Elastic. 2. Enter parameter values. 3. Click OK. This input data creates the viscoelastic options. All inputs must have the same number of time points (at the same times) in the referenced fields. The following equations may be useful when creating the Prony G = E ⁄ (2(1 + v) ) . series for the bulk and shear moduli: K = E ⁄ ( 3 ( 1 – 2v ) )

80 Modeling Guide

Viscoelastic material models require the following material data via the Input Properties subform on the Materials Application form. Isotropic -Visco Elastic

Description

Shift Function

No Function

Thermal Exp. Solid Coeff.

Solid coefficient of thermal expansion

Thermal Exp. Liquid Coeff.

Liquid coefficient of thermal expansion

Deviatoric Terms of Prony Series

Deviatoric Scale Factor -- Multiplier (scale factor) for deviatoric behavior in Prony series (Real > 0., Default = 0). Deviatoric Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0).

Volumetric Terms of Prony Series Volumetric Scale Factor -- Multiplier (scale factor) for volumetric behavior in Prony series (Real > 0., Default = 0.). Volumetric Time Constant -- Defines time constants for volumetric behavior in Prony series (Real > 0., Default = 1000.). Shift Function

Williams-Landel-Ferry

Thermal Exp. Solid Coeff.

Solid coefficient of thermal expansion

Thermal Exp. Liquid Coeff.

Liquid coefficient of thermal expansion

Deviatoric Terms of Prony Series

Deviatoric Scale Factor -- Multiplier (scale factor) for deviatoric behavior in Prony series (Real > 0., Default = 0). Deviatoric Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0).

Volumetric Terms of Prony Series Volumetric Scale Factor -- Multiplier (scale factor) for volumetric behavior in Prony series (Real > 0., Default = 0.). Volumetric Time Constant -- Defines time constants for volumetric behavior in Prony series (Real > 0., Default = 1000.). Reference Temperature

Reference or glass transition temperature.

Shift Function Coeff. 1

Constant A1.

Shift Function Coeff. 2

Constant A2.

Shift Function

Power Series Expansion

Thermal Exp. Solid Coeff.

Solid coefficient of thermal expansion

Thermal Exp. Liquid Coeff.

Liquid coefficient of thermal expansion

Deviatoric Terms of Prony Series

Deviatoric Scale Factor -- Multiplier (scale factor) for deviatoric behavior in Prony series (Real > 0., Default = 0). Deviatoric Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0).

CHAPTER 81 Model Generation

Isotropic -Visco Elastic

Description

Volumetric Terms of Prony Series Volumetric Scale Factor -- Multiplier (scale factor) for volumetric behavior in Prony series (Real > 0., Default = 0.). Volumetric Time Constant -- Defines time constants for volumetric behavior in Prony series (Real > 0., Default = 1000.). Reference Temperature

Reference or glass transition temperature.

Number of Power Terms

Number of coefficients in the power series representation.

Shift Function Coeff. 0

Coefficient C0 of the shift function.

Orthotropic-Visco Elastic

Description

Shift Function

No Function

Prony Terms

Dev. Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0) Youngs’s Modulus i Poisson’s Ratio ij Shear Modulus ij

Shift Function

Williams-Landel-Ferry

Prony Terms

Dev. Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0) Youngs’s Modulus i Poisson’s Ratio ij Shear Modulus ij

Reference Temperature

Reference or glass transition temperature.

Shift Function Coeff. 1

Constant A1.

Shift Function Coeff. 2

Constant A2.

Shift Function

Power Series Expansion

Prony Terms

Dev. Time Constant -- Defines time constants for deviatoric behavior in Prony series (Real > 0., Default = 0) Youngs’s Modulus i Poisson’s Ratio ij Shear Modulus ij

Reference Temperature

Reference or glass transition temperature.

Number of Power Terms

Number of coefficients in the power series representation.

Shift Function Coeff. 0

Coefficient C0 of the shift function.

82 Modeling Guide

Inelastic Most materials of engineering interest initially respond elastically. Elastic behavior means that the deformation is fully recoverable, so that, when the load is removed, the specimen returns to its original shape. If the load exceeds some limit (the “yield load”), the deformation is no longer fully recoverable. Some parts of the deformation will remain when the load is removed as, for example, when a paper clip is bent too much, or when a billet of metal is rolled or forged in a manufacturing process. Plasticity theories model the material’s mechanical response as it undergoes such nonrecoverable deformation in a ductile fashion. The theories have been developed most intensively for metals, but they are applied to soils, concrete, rock, ice, and so on. These materials behave in very different ways (for example, even large values of pure hydrostatic pressure cause very little inelastic deformation in metals, but quite small hydrostatic pressure may cause a significant, non-recoverable volume change in a soil sample), but the fundamental concepts of plasticity theories are sufficiently general that models based on these concepts have been successfully developed for a wide range of materials. A number of these plasticity modes are available in the MD Nastran Implicit Nonlinear material library. In nonlinear material behavior, the material parameters depend on the state of stress. Up to the proportional limit, i.e., the point at which linearity in material behavior ceases, the linear elastic formulation for the behavior can be used. Beyond that point, and especially after the onset of yield, nonlinear formulations are required. In general, two ingredients are required to ascertain material behavior: 1. an initial yield criterion to determine the state of stress at which yielding is considered to begin 2. mathematical rules to explain the post-yielding behavior. There are two major theories of plastic behavior that address these criterion differently. In the first, called deformation theory, the plastic strains are uniquely defined by the state of stress. The second theory, called flow or incremental theory, expresses the increments of plastic strain (irrecoverable strains) as functions of the current stress, the strain increments, and the stress increments. Incremental theory is more general and can be adapted in its particulars to fit a variety of material behaviors. The plasticity models in MD Nastran Implicit Nonlinear are “incremental” theories, in which the mechanical strain rate is decomposed into an elastic part and a plastic (inelastic) part through various assumed flow rules. The incremental plasticity models are formulated in terms of: • A yield surface, which generalizes the concept of “yield load” into a test function which can be

used to determine if the material will respond purely elastically at a particular state of stress, temperature, etc.; • A flow rule that defines the inelastic deformation that must occur if the material point is no

longer responding purely elastically; • and some evolution laws that define the hardening - the way in which the yield and/or flow

definitions change as inelastic deformation occurs. The models also need an elasticity definition, to deal with the recoverable part of the strain models divide into those that are rate-dependent and those that are rate-independent.

CHAPTER 83 Model Generation

MD Nastran Implicit Nonlinear includes the following models of inelastic behavior. • Metal Plasticity (von Mises or Hill) • ORNL (Oak Ridge National Laboratory) - characterizes creep behavior and cyclic loading

effects on stainless steel materials. • Porous Metal Plasticity (Gurson) - includes effects of hydrostatic pressure and failure processes

in ductile materials. • Pressure-Dependent models - models the behavior of granular (soil and rock) materials or

polymers, in which the yield behavior depends on the equivalent pressure stress. • Linear Mohr-Coulomb • Parabolic Morh-Coulomb • Buyukozturk Concrete

Yield Conditions The yield stress of a material is a measured stress level that separates the elastic and inelastic behavior of the material. The magnitude of the yield stress is generally obtained from a uniaxial test. However, the stresses in a structure are usually multiaxial. A measurement of yielding for the multiaxial state of stress is called the yield condition. Depending on how the multiaxial state of stress is represented, there can be many forms of yield conditions. For example, the yield condition can be dependent on all stress components, on shear components only, or on hydrostatic stress. A number of yield conditions are available in MD Nastran Implicit Nonlinear, and are discussed in this section. Metal Plasticity

The von Mises yield surface is widely used for plasticity in isotropic metals. It is assumed that the yield and plastic flow describe isotropic metals at low temperatures where creep effects can be ignored. Anisotropic metals and composite materials, can be treated by extensions of von Mises yield function, as described in Hill’s yield function. von Mises

The success of the von Mises criterion is due to the continuous nature of the function that defines this criterion and its agreement with observed behavior for the commonly encountered ductile materials. The von Mises criterion states that yield occurs when the effective (or equivalent) stress (σ) equals the yield stress (σy) as measured in a uniaxial test. Figure 5-20 shows the von Mises yield surface in two-dimensional and three-dimensional stress space.

84 Modeling Guide

σ′3

σ2 Yield Surface

Yield Surface Elastic Region

σ1 Elastic Region

σ′1

(a) Two-dimensional Stress Space

Figure 5-20

σ′2 (b) π-Plane

von Mises Yield Surface

For an isotropic material

σ = [ ( σ1 – σ2 )2 + ( σ2 – σ3 )2 + ( σ3 – σ1 )2 ] 1 ⁄ 2 ⁄ 2

(5-112)

where σ1, σ2, and σ3 are the principal Cauchy stresses.

σ can also be expressed in terms of nonprincipal Cauchy stresses. 2 2 2 ( σ = [ ( σ x – σ y ) 2 + ( σ y – σ z ) 2 + ( σ z – σ x ) 2 + 6 ( τ xy + τ yz + τ zx ) ]1 ⁄ 2 ) ⁄ 2

(5-113)

The yield condition can also be expressed in terms of the deviatoric stresses as:

σ = where

3--σ′ σ′ 2 ij ij

(5-114)

σ′ij is the deviatoric Cauchy stress expressed as

1 σ′ij = σ ij – --- σ kk δ ij 3 For isotropic material, the von Mises yield condition is the default condition in MD Nastran Implicit Nonlinear.

(5-115)

CHAPTER 85 Model Generation

Hill’s Yield Function

Hill’s yield surface has been widely used both as a yield surface and as a failure surface for anisotropic and composite materials. Hill’s yield function is a generalization of von Mises as expressed below.

σ yy σ zz xx σ ------- +  ------- +  ----- Fx   Fy   Fz  2

2

2

1 1 1 –  -----2- + -----2- – -----2- σ xx σ yy  Fx Fy Fz  1 1 1 –  -----2- – -----2- + -----2- σ xx σ zz  Fx Fy Fz   1 1 1 – – -----2- + -----2- + -----2- σ yy σ zz  Fx Fy Fz  τ xy 2 τ yz 2 τ zx 2 +  -------- +  ------- +  ------- = 1 F xy F yz F zx

(5-116)

Note the following points about Hill’s surface: 1. It degenerates into von Mises surface when all three direct yield stresses are equal (Fx = Fy = Fz) and all three shear yield stresses are equal. 2. It is invariant with respect to hydrostatic stress, as is von Mises. 3. Hill's surface, unlike von Mises, is not always an ellipsoid in stress space. When it is not an ellipsoid, it is not appropriate for use as a yield function (since it does not have an inside and an outside, thereby dividing stress space into elastic and plastic regions). Mohr-Coulomb Material (Hydrostatic Stress Dependence)

MD Nastran Implicit Nonlinear includes options for elastic-plastic behavior based on a yield surface that exhibits hydrostatic stress dependence. Such behavior is observed in a wide class of soil and rock-like materials. These materials are generally classified as Mohr-Coulomb materials (generalized von Mises materials). Ice is also thought to be a Mohr-Coulomb material. The generalized Mohr-Coulomb model developed by Drucker and Prager is implemented in MD Nastran Implicit Nonlinear. There are two types of Mohr-Coulomb materials: linear and parabolic. Each is discussed on the following pages.

86 Modeling Guide

Linear Mohr-Coulomb Material

The deviatoric yield function, as shown in Figure 5-21, is assumed to be a linear function of the hydrostatic stress.

σ f = αJ 1 + J 21 ⁄ 2 – ------- = 0 3

(5-117)

where

J 1 = σ ii

(5-118)

1 J 2 = --- σ′ij σ′ij 2

(5-119)

The constants

α and σ can be related to c and φ by

σ ; c = -----------------------------------------1⁄2 [ 3 ( 1 – 12α 2 ) ] where

3α ------------------------------ = sin φ ( 1 – 3α 2 ) 1 ⁄ 2

(5-120)

c is the cohesion and φ is the angle of friction. τ

Yield Envelope

R c

φ

σ

σx + σy 2

Figure 5-21

Yield Envelope of Plane Strain (Linear Mohr-Coulomb Material)

Parabolic Mohr-Coulomb Material

The hydrostatic dependence is generalized to give a yield envelope which is parabolic in the case of plane strain (see Figure 5-22).

CHAPTER 87 Model Generation

f = ( 3J 2 + 3βσJ 1 ) 1 ⁄ 2 – σ = 0

(5-121)

α β = ----------------------------------------( 3 ( 3c 2 – α 2 ) ) 1 ⁄ 2

2

2 α σ = 3  c – ------  3 2

where

(5-122)

c is the cohesion. τ

R

c σ

σx + σy

c2 α

2

Figure 5-22

Resultant Yield Condition of Plane Strain (Parabolic Mohr-Coulomb Material

Buyukozturk Criterion (Hydrostatic Stress Dependence)

The Buyukozturk concrete plasticity model is a particular form of the generalized Drucker-Prager plasticity model, which is developed specifically for plane stress cases by Buyukozturk. This yield criterion, which originally has been proposed as a failure criterion, has the general form: 2

f = β 3σJ 1 + γJ 1 + 3J 2 – σ

2

The Buyukozturk criterion reduces to the parabolic Mohr-Coulomb criterion if

(5-123)

γ = 0.

Oak Ridge National Laboratory Options

Oak Ridge National Laboratory (ORNL) has performed a large number of creep tests on stainless and other alloy steels. It has also set certain rules that characterize creep behavior for application in the nuclear structures. A summary of the ORNL rules on creep is discussed in MSC.Marc Volume A, Theory and User Information. In MD Nastran Implicit Nonlinear, the ORNL options are based on the definitions of ORNL-TM- 3602 [1] for stainless steels and ORNL recommendations [2] for 2 1/4 Cr-1 Mo steel. The initial yield stress should be used for the initial inelastic loading calculations for both the stainless steels and 2 1/4 Cr-1 Mo steel. The 10th-cycle yield stress should be used for the hardened material. The 100th-cycle yield stress must be used in the following circumstances:

88 Modeling Guide

1. To accommodate cyclic softening of 2 1/4 Cr-1 Mo steel after many load cycles. 2. After a long period of high temperature exposure. 3. After the occurrence of creep strain. Work Hardening Rules The work-hardening rule defines the way the yield surface changes with plastic straining. A material is said to be “perfectly plastic” if, upon the stress state touching the yield surface, an infinitesimal increase in stress causes an arbitrarily large plastic strain. MD Nastran Implicit Nonlinear models all materials as work hardening, and treats perfectly plastic materials as a special case. Because the tangent stiffness method is used, no difficulties arise in setting the work hardening slope equal to zero. Besides perfect plasticity, three possibilities are provided: isotropic hardening and kinematic hardening. The isotropic workhardening rule assumes that the center of the yield surface remains stationary in the stress space, but that the size (radius) of the yield surface expands, due to workhardening. This type of hardening is appropriate when the straining is the same in all directions. For many materials, the isotropic workhardening model is inaccurate if unloading occurs (as in cyclic loading problems). For these problems, the kinematic hardening model or the combined hardening model represents the material better. Isotropic Hardening

Kinematic Hardening Hardened Original

Isotropic, Kinematic, and Combined Hardening

The isotropic workhardening rule assumes that the center of the yield surface remains stationary in the stress space, but that the size (radius) of the yield surface expands, due to workhardening. The change of the von Mises yield surface is plotted in Figure 5-23b. A review of the load path of a uniaxial test that involves both the loading and unloading of a specimen will assist in describing the isotropic workhardening rule. The specimen is first loaded from stress free (point 0) to initial yield at point 1, as shown in Figure 5-23a. It is then continuously loaded to point 2. Then, unloading from 2 to 3 following the elastic slope E (Young’s modulus) and then elastic reloading from 3 to 2 takes place. Finally, the specimen is plastically loaded again from 2 to 4 and elastically unloaded from 4 to 5. Reverse plastic loading occurs between 5 and 6. It is obvious that the stress at 1 is equal to the initial yield stress

σ y and stresses at points 2 and 4 are

larger than σ y , due to workhardening. During unloading, the stress state can remain elastic (for example,

CHAPTER 89 Model Generation

point 3), or it can reach a subsequent (reversed) yield point (for example, point 5). The isotropic workhardening rule states that the reverse yield occurs at current stress level in the reversed direction.

σ 4 2

1

σy

E E

+σ4

E 3 0

−σ4

5 6

(a) Loading Path

σ′3

5 6

0 3 2 1 4

σ′1

σ′2 (b) von Mises Yield Surface

Figure 5-23 Let

Schematic of Isotropic Hardening Rule (Uniaxial Test)

σ 4 be the stress level at point 4. Then, the reverse yield can only take place at a stress level of – σ 4

(point 5).

90 Modeling Guide

For many materials, the isotropic workhardening model is inaccurate if unloading occurs (as in cyclic loading problems). For these problems, the kinematic hardening model or the combined hardening model represents the material better. Kinematic Hardening

Under the kinematic hardening rule, the von Mises yield surface does not change in size or shape, but the center of the yield surface can move in stress space. Figure 5-23d illustrates this condition. Ziegler’s law is used to define the translation of the yield surface in the stress space. The loading path of a uniaxial test is shown in Figure 5-23c. The specimen is loaded in the following order: from stress free (point 0) to initial yield (point 1), 2 (loading), 3 (unloading), 2 (reloading), 4 (loading), 5 and 6 (unloading). As in isotropic hardening, stress at 1 is equal to the initial yield stress σ y , and stresses at 2 and 4 are higher than

σ y , due to workhardening. Point 3 is elastic, and reverse yield

takes place at point 5. Under the kinematic hardening rule, the reverse yield occurs at the level of

σ 5 = ( σ 4 – 2σ y ) , rather than at the stress level of – σ 4 . Similarly, if the specimen is loaded to a higher stress level is

σ 7 (point 7), and then unloaded to the subsequent yield point 8, the stress at point 8

σ 8 = ( σ 7 – 2σ y ) . If the specimen is unloaded from a (tensile) stress state (such as point 4 and 7),

the reverse yield can occur at a stress state in either the reverse (point 5) or the same (point 8) direction. For many materials, the kinematic hardening model gives a better representation of loading/unloading behavior than the isotropic hardening model. For cyclic loading, however, the kinematic hardening model can represent neither cyclic hardening nor cyclic softening. Combined Hardening Figure 5-25 shows a material with highly nonlinear hardening. Here, the initial hardening is assumed to be almost entirely isotropic, but after some plastic straining, the elastic range attains an essentially constant value (that is, pure kinematic hardening). The basic assumption of the combined hardening model is that such behavior is reasonably approximated by a classical constant kinematic hardening constraint, with the superposition of initial isotropic hardening. The isotropic hardening rate eventually decays to zero as a function of the equivalent plastic strain measured by

·p ε =

·p  ε dt =

 2--- · p · p    3 εij εij

1⁄2

dt

(5-124)

CHAPTER 91 Model Generation

σ Initial Elastic Range

Fully Hardened Pure Kinematic Range

Combined Hardening Range

Stress

Initial Yield One-half Current Elastic Range

dα Kinematic Slope, 3 2 dεp ε

Strain

Figure 5-24

Basic Uniaxial Tension Behavior of the Combined Hardening Model

This implies a constant shift of the center of the elastic domain, with a growth of elastic domain around this center until pure kinematic hardening is attained. In this model, there is a variable proportion between the isotropic and kinematic contributions that depends on the extent of plastic deformation (as measured by

p

ε ).

The workhardening data at small strains governs the isotropic behavior, and the data at large strains ( ε p > 1000 ) governs the kinematic hardening behavior. If the last workhardening slope is zero, the behavior is the same as the isotropic hardening model. Experimental Determination of Work Hardening Slope

In a uniaxial test, the workhardening slope is defined as the slope of the stress-plastic strain curve. The workhardening slope relates the incremental stress to incremental plastic strain in the inelastic region and dictates the conditions of subsequent yielding. A number of workhardening rules (isotropic, kinematic, and combined) are available in MD Nastran Implicit Nonlinear. A description of these workhardening rules is given below. The uniaxial stress-plastic strain curve can be represented by a piecewise linear function or through the user subroutine WKSLP . This requires the use of MARCIN to specify the MARC WORKHARD option.

92 Modeling Guide

Stress

Δσ3

Δσ2 Δσ1

σ E

E

p

E

p

Δε1

Δε 2

Figure 5-25

Workhardening Slopes

Slope

Breakpoint

Δσ 1 ---------pΔε1

0.0

Δσ 2 ---------pΔε 2

Δε1

Δσ 3 ---------pΔε 3

Δε1 + Δε 2

p

Δε 3

p

p

p

You enter a table of yield stress, plastic strain points.

E Strain

CHAPTER 93 Model Generation

Note:

The data points should be based on a plot of the stress versus plastic strain for a tensile test. The elastic strain components should not be included.

The yield stress and the workhardening data must be compatible with the procedure used in the analysis. For small strain analyses, the engineering stress and engineering strain are appropriate. If only PARAM,LGDISP is used, the yield stress should be entered as the second Piola-Kirchhoff stress, and the workhard data be given with respect to plastic Green-Lagrange strains. If PARAM,LGDISP,1 or 2 are used, the yield stress must be defined as a true or Cauchy stress, and the workhardening data with respect to logarithmic plastic strains. Engineering stress and strain may be defined and Bulk Data parameter MRTABLS1 used to provide the program with rules to convert to the proper stress and strain measures. See MRTABLS1 in the MD NASTRAN QRG. Flow Rules Yield stress and workhardening rules are two experimentally related phenomena that characterize plastic material behavior. The flow rule is also essential in establishing the incremental stress-strain relations for p

plastic material. The flow rule describes the differential changes in the plastic strain components dε as a function of the current stress state. So long as a material point is elastic, Hooke’s law provides a relationship between total stress and strain. After a material becomes plastic, however, there is no longer a unique relationship between total stress and strain. The problem then is usually solved incrementally, following the exact loading path. For points which are plastic, a flow rule is used to relate increments of stress to plastic strain. MD Nastran Implicit Nonlinear uses an associated flow rule, which prescribes that increments of plastic strain are computed as a constant times the gradient of the yield function. In other words, considering the yield function as a surface in stress space, the plastic strain increment is a vector in the direction of the outward normal to the surface at the point where it is touched by the stresses on the loading path. The equation representing this is:

∂F dε ijp = λ --------∂σ ij

(5-125)

94 Modeling Guide

where λ is a constant. Writing the six equations explicitly:

∂F p = ---------dε xx ∂σ xx ∂F p = ---------dε yy ∂σ yy ∂F p = ---------dε zz ∂σ zz p dε xy

∂F = ---------∂τ xy

(5-126)

∂F p = --------dε yz ∂τ yz ∂Fp = --------dε zx ∂τ xz These stress vs. plastic strain equations are analogous to the stress vs. total strain equations of elasticity, where elastic strains can be computed as the gradient of a strain energy potential function, namely;

∂U dε ij = --------∂σ ij

(5-127)

Thus, the yield function F plays the role of a plastic potential. If a theory of plasticity uses something other than the yield function as a plastic potential, a so-called nonassociated flow rule results. Nonassociated flow rules are not available in MD Nastran Implicit Nonlinear.

CHAPTER 95 Model Generation

For the von Mises and modified Hill yield functions programmed in MD Nastran Implicit Nonlinear, the derivatives in the yield function are obtained simply by differentiating with respect to individual components of stress. For example, for the modified Hill function, we have:

2σ xx σ yy σ zz p = λ ---------- – ------------ – ----------dε xx 2 Fx Fy Fx Fz Fx σ xx 2σ yy σ zz p = λ – ----------- + ----------- – ----------dε yy F x Fy F y2 F y F z σ xx σ yy 2σ zz p = λ – ----------dε zz – ----------+ ---------F x F z F y F z F z2 σ xy p = λ ------dε xy 2 F xy σ xz 2 = λ ------dε yz 2 F yz σ yz p = λ ------dε zx 2 F zx

(5-128)

The constant in these flow rule equations is evaluated automatically by MD Nastran Implicit Nonlinear on the basis of material stability during plastic flow (i.e., by the requirement that the stress state remain on the yield surface during plastic straining). The Prandtl-Reuss representation of the flow rule is available in MD Nastran Implicit Nonlinear. In conjunction with the von Mises yield function, this can be represented as:

∂σ p dε ij = dε p ----------∂σ ij′ where

(5-129)

dε p and σ are equivalent plastic strain increment and equivalent stress, respectively.

The significance of this representation is illustrated in Figure 5-26. This figure illustrates the “stress-space” for the two-dimensional case. The solid curve gives the yield surface (locus of all stress states causing yield) as defined by the von Mises criterion. Equation (5-139) expresses the condition that the direction of inelastic straining is normal to the yield

surface. This condition is called either the normality condition or the associated flow rule. If the von Mises yield surface is used, then the normal is equal to the deviatoric stress.

96 Modeling Guide

σ2

p dε2

dεp

dεp 1

σ1 Yield Surface Figure 5-26

Yield Surface and Normality Criterion 2-D Stress Space

Rate Dependent Yield Strain rate effects cause the structural response of a body to change because they influence the material properties of the body. These material changes lead to an instantaneous change in the strength of the material. Strain rate effects become more pronounced for temperatures greater than half the melting temperature ( T m ), but are sometimes present even at room temperature. The following discussion explains the effect of strain rate on the size of the yield surface. Using the von Mises yield condition and normality rule, we obtain an expression for the stress rate of the form

·· p · · σ ij = L ijkl ε kl + r ij ε For elastic-plastic response

∂σ ∂σ L ijkl = C ijkl –  C ijmn ------------ ----------- C pqkl ⁄ D ∂σ mn ∂σ pq

(5-130)

and

∂σ 2 ∂σr ij = C ijmn ------------ --- σ ------·p ⁄ D ∂σ mn 3 ∂ε

(5-131)

where

4 ∂σ ∂σ ∂σ D = --- σ 2 -------p- + --------- C ijkl ---------9 ∂σ ∂σ ∂ε ij kl

(5-132)

CHAPTER 97 Model Generation

As strain rates increase, many materials show an increase in yield strength. The model provided in MD Nastran Implicit Nonlinear for this purpose is P · σ ε = D  ------ – 1 for α ≥ σ 0 σ0

where:

· pl ε

=

the uniaxial equivalent plastic strain rate

σ

=

the effective yield stress at a non-zero strain rate the static yield stress (which may depend on the equivalent plastic strain,

pl

σ0 ( ε , T )

=

pl

ε , via isotropic hardening, or on the temperature, T .

are material parameters that may be functions of temperature. D and p are D ( T ), p ( T ) = defined on the input forms. This model is effective in both static and dynamic procedures. Yield stress variation with strain rate is given using one of three options: 1. The breakpoints and slopes for a piecewise linear approximation to the yield stress strain rate curve are given. The strain rate breakpoints should be in ascending order, or 2. The Cowper and Symonds model is used. The yield behavior is assumed to be completely determined by one stress-strain curve and a scale factor depending on the strain rate. Note:

If multiple material models are used, they must all be expressed as piecewise linear, or as Cowper and Symonds model.

Perfectly Plastic

A material is said to be “perfectly plastic” if, upon the stress state touching the yield surface, an infinitesimal increase in stress causes an arbitrarily large plastic strain. The uniaxial stress-strain diagram for an elastic-perfectly plastic material is shown in Figure 5-27. Some materials, such as mild steel, behave in a manner which is close to perfectly plastic.

98 Modeling Guide

.

σxx

YS E 1

∋

xx

Figure 5-27

Perfectly Plastic Material Stress-Strain Relationship

Experimental Stress-Strain Curves Metals

In uniaxial tension tests of most metals (and many other materials), the following phenomena can be observed. If the stress in the specimen is below the yield stress of the material, the material behaves elastically and the stress in the specimen is proportional to the strain. If the stress in the specimen is greater than the yield stress, the material no longer exhibits elastic behavior, and the stress-strain relationship becomes nonlinear. Figure 5-28 shows a typical uniaxial stress-strain curve. Both the elastic and inelastic regions are indicated.

Inelastic Region

Stress

Yield Stress

Strain Elastic Region Note: Stress and strain are total quantities.

Figure 5-28

Typical Uniaxial Stress-Strain Curve (Uniaxial Test)

CHAPTER 99 Model Generation

Within the elastic region, the stress-strain relationship is unique. As illustrated in , if the stress in the specimen is increased (loading) from zero (point 0) to

σ 1 (point 1), and then decreased (unloading) to

zero, the strain in the specimen is also increased from zero to ε 1 , and then returned to zero. The elastic strain is completely recovered upon the release of stress in the specimen. The loading-unloading situation in the inelastic region is different from the elastic behavior. If the specimen is loaded beyond yield to point 2, where the stress in the specimen is

σ 2 and the total strain

e

is ε 2 , upon release of the stress in the specimen the elastic strain, ε , is completely recovered. 2 p

However, the inelastic (plastic) strain, ε 2 , remains in the specimen. Figure 5-29 illustrates this relationship. Similarly, if the specimen is loaded to point 3 and then unloaded to zero stress state, the plastic strain

p

p

p

ε 3 remains in the specimen. It is obvious that ε 2 is not equal to ε 3 . We can conclude that

in the inelastic region: • Plastic strain permanently remains in the specimen upon removal of stress. • The amount of plastic strain remaining in the specimen is dependent upon the stress level at

which the unloading starts (path-dependent behavior). The uniaxial stress-strain curve is usually plotted for total quantities (total stress versus total strain). The total stress-strain curve shown in Figure 5-29 can be replotted as a total stress versus plastic strain curve, as shown in Figure 5-30. The slope of the total stress versus plastic strain curve is defined as the workhardening slope (H) of the material. The workhardening slope is a function of plastic strain. Total Strain = Strain and Elastic Strain Stress

σ3 σ2 Yield Stress

σy

σ1 0

3 2

1

ε1

ε2 p

ε2

ε3

p

p

e

p

e

ε2 = ε 2 + ε2

ε 2e ε3

Strain

ε 3e

ε3 = ε 3 + ε3

100 Modeling Guide

Figure 5-29 Total Stress

σ

Schematic of Simple Loading - Unloading (Uniaxial Test)

θ

Plastic Strain H = tan θ (Workhardening Slope) = dσ/dεp

Figure 5-30

εp

Definition of Workhardening Slope (Uniaxial Test)

The stress-strain curve shown in Figure 5-29 is directly plotted from experimental data. It can be simplified for the purpose of numerical modeling. A few simplifications are shown in Figure 5-31 and are listed below: 1. Bilinear representation – constant workhardening slope. 2. Elastic perfectly-plastic material – no workhardening. 3. Perfectly-plastic material – no workhardening and no elastic response. 4. Piecewise linear representation – multiple constant workhardening slopes. 5. Strain-softening material – negative workhardening slope. In addition to elastic material constants (Young’s modulus and Poisson’s ratio), it is essential to include yield stress and workhardening slopes when dealing with inelastic (plastic) material behavior. These quantities can vary with parameters such as temperature and strain rate. Since the yield stress is generally measured from uniaxial tests, and the stresses in real structures are usually multiaxial, the yield condition of a multiaxial stress state must be considered. The conditions of subsequent yield (workhardening rules) must also be studied.

CHAPTER 101 Model Generation

σ

σ

ε

ε

(1) Bilinear Representation

(2) Elastic-Perfectly Plastic

σ

σ

ε

ε

(3) Perfectly Plastic

(4) Piecewise Linear Representation

σ

ε (5) Strain Softening

Figure 5-31

Simplified Stress-Strain Curves (Uniaxial Test)

Geological Materials

Data for geological materials are most commonly available from triaxial compression testing. In such a test, the specimen is confined by pressure and an additional compression stress is superposed in one direction. Thus, the principal stresses are all negative, with

-σ1

-σ3

σ1=σ2>σ3

−σ1 Figure 5-32

0 ≥ σ1 = σ2 ≥ σ3 .

−σ2

σ1>σ2=σ3

−σ2

Triaxial Compression and Tension

−σ3

102 Modeling Guide

The values of the stress invariants in a uniaxial compression experiment are: p=-{1/3}(2σ1+σ3) q=σ1-σ3 r3=-(σ1-σ3)3 so that t=q=σ1-σ3 The triaxial results may thus be plotted in the t-p plane shown above. Fitting the best straight line through the results then provides β and d. Triaxial tension data are also needed to define K. Under triaxial tension, the specimen is again confined by pressure, then the pressure in one direction is reduced. In this case, the principal stresses are . σ1 ≥

σ2 = σ3

The stress invariants are now: p=-{1/3}(σ1+2σ3), q=σ1-σ3, r3=(σ1-σ3)3, so that t={q/K}={1/K}(σ1-σ3) K may thus be found by plotting these test results as q versus p and again fitting the best straight line. The triaxial compression and tension lines must intercept the p-axis at the same point, and the ratio of values of q for triaxial tension and compression at the same value of p then gives K as shown in Figure 5-33.

q

Best fit to triaxial compression data Best fit to triaxial tension data

hc β

ht

d p

Figure 5-33

Triaxial Compression and Tension Data

Matching Mohr-Coulomb Parameters

CHAPTER 103 Model Generation

Sometimes, experimental data are not directly available. Instead, the user is provided with the friction angle and cohesion values for the Mohr-Coulomb model. We, therefore, need to calculate values for the parameters of the Drucker-Prager model to provide a reasonable match to the Mohr-Coulomb parameters. The Mohr-Coulomb failure model is based on plotting Mohr’s circle for states of stress at failure in the plane of the maximum and minimum principal stresses. The failure line is the best straight line that touches these Mohr’s circles. The Mohr-Coulomb model is thus s+σmsinϕ-c cosϕ=0, where s={1/2}(σ1-σ3) is half of the difference between the maximum and minimum principal stresses (and is, therefore, the maximum shear stress), and σm={1/2}(σ1+σ3) is the average of the maximum and minimum principal stresses. We see that the Mohr-Coulomb model assumes that failure is independent of the value of the intermediate principal stress. The Drucker-Prager model does not. The failure of typical geotechnical materials generally includes some small dependence on the intermediate principal stress. Matching Triaxial Test Response

One approach to matching Mohr-Coulomb and Drucker-Prager model parameters is to make the two models provide the same failure definition in triaxial compression and tension. For this purpose, we can rewrite the Mohr-Coulomb model in terms of principal stresses.

σ 1 – σ 3 + ( σ 1 + σ 3 ) sin ( φ ) – 2c cos φ = 0

(5-133)

Using the results above (for the stress invariants p, q, and r), in triaxial compression and tension, allows the Drucker-Prager model to be written for triaxial compression as

1 1 – --- tan β tan β 3 0 σ 1 – σ 3 + ------------------------------ ( σ 1 + σ 3 ) + ------------------------ σ c = 0 1  2 + 1--- tan β 1 + --- tan β 6   3 and, for triaxial tension, as

(5-134)

104 Modeling Guide

1 1 – --- tan β tan β 3 0 σ 1 – σ 3 + ---------------------------- ( σ 1 + σ 3 ) + ------------------------ σ c = 0 1- 1--2- 1-- -- --– tan β – tan β K 6 K 3 

(5-135)

We wish to make the equations for triaxial compression and biaxial tension identical to the general Mohr-Coulomb equation for all values of (σ1,σ3). Comparing the equations for triaxial compression and triaxial tension requires that:

1 1 1 1 + --- tan β = ---- – --- tan β 6 K 6

(5-136)

so that 1 K = -----------------------1 1 + --- tan β 3

(5-137)

Comparing the coefficients of (σ1+σ3) in the equation for triaxial compression and that for triaxial tension provides:

6 sin φ tan β -------------------3 – sin φ

(5-138)

and hence, from the derived equation for K:

3 – sin φ K = --------------------3 + sin Φ

(5-139)

Finally, comparing the last terms in the general expression for the Mohr-Coulomb model and the equation for triaxial compression and using the expression for tanβ provides: 0 2c cos Φ σ c = --------------------1 – sin Φ

(5-140)

The expression for tanβ, K, and this last expression and thus provide Drucker-Prager parameters that match the Mohr-Coulomb model in triaxial compression and tension. The value of K in the Drucker-Prager model is restricted to K ≥ 0.778 for the yield surface to remain convex. Rewriting the expression for K as: 1–K sin Φ = 3  -------------  1 + k

(5-141)

shows that this implies φ ≤ 22° . Many real materials have a larger Mohr-Coulomb friction angle than this value. In such circumstances, one approach is to choose K = 0.778 and then to use the expression for

CHAPTER 105 Model Generation

0 0 tan β to define β and the expression for σ c to define σ c , ignoring the expression for K. This matches the models for triaxial compression only, while providing the closest approximation that the model can provide to failure being independent of the intermediate principal stress. If ϕ is significantly larger than 22°, this approach may provide a poor Drucker-Prager match of the Mohr-Coulomb parameters. MD Nastran Implicit Nonlinear uses K=1 by default. Matching Plane Strain Response

Plane strain problems are often encountered in geotechnical analysis: examples are long tunnels, footings, and embankments. For this reason, the constitutive model parameters are often matched to provide the same flow and failure response in plane strain. The Drucker-Prager flow potential defines the plastic strain increment as:

dε



 1 ∂ = dε ------------------------- ( t – p tan ψ )   1 ∂σ  1 – --- tan ψ  3 pl 

pl

where dε

pl

(5-142)

is the equivalent plastic strain increment.

Since we only wish to match the behavior in one plane we can assume K=1, which implies that t=q. Then:

dε

pl



 1   ∂ q – tan ψ ∂p  -----------------------= dε    ∂σ 1 ∂ σ  1 – --- tan ψ 3 pl 

(5-143)

Writing this expression in terms of principal stresses provides: pl dε 1



 1 1 1 = dε  -------------------------  ------ ( 2σ 1 – σ 2 – σ 3 ) + --- tan ψ 1 2q 3  1 – --- tan ψ 3 pl 

(5-144)

pl pl with similar expressions for dε 2 and dε 3 . pl Assume plane strain in the 1-direction. Then, at limit load, we must have dε 1 =0. From the above expression, this provides the constraint: 1 1 ------ ( 2σ – σ – σ ) + --- tan ψ = 0 1 2 3 3 2q so that:

(5-145)

106 Modeling Guide

1 1 σ 1 = --- ( σ 2 + σ 3 ) – --- tan ψq 3 2

(5-146)

Using this constraint, we can rewrite q and p in terms of the principal stresses in the plane of deformation, 3 3 q = ------------------------------------- ( σ 2 – σ 3 ) 2 2 9 – ( tan ψ )

(5-147)

and 1 tan ψ p = – --- ( σ 2 + σ 3 ) + --------------------------------------------- ( σ 2 – σ 3 ) 2 2 2 3 ( 9 – ( tan ψ ) )

(5-148)

With these expressions, the Drucker-Prager yield surface can be written in terms of σ2 and σ3 as 9 – tan β tan ψ 1 --------------------------------------------- ( σ – σ ) + --- tan β ( σ + σ ) – d = 0 2 3 2 2 3 2 2 3 ( 9 – ( tan ψ ) )

(5-149)

The Mohr-Coulomb yield surface in the (2,3) plane is: σ 2 – σ 3 + sin ϕ ( σ 2 + σ 3 ) – 2c cos ϕ = 0

(5-150)

By comparison, 2 tan β 3 ( 9 – ( tan ψ ) ) sin ϕ = -----------------------------------------------------9 – tan β tan ψ 2 3 ( 9 – ( tan ψ ) ) c cos ϕ = ------------------------------------------ d 9 – tan β tan ψ

(5-151)

(5-152)

Now consider the two extreme cases of flow definition: associated flow, ψ=β, and nondilatant flow, when ψ=0. Assuming associated flow, the last two equations provide: 3 sin ϕ tan β = -----------------------------------2 1 1 + --- ( sin ϕ ) 3

(5-153)

and d 3 cos ϕ --- = ----------------------------------c 2 1 1 + --- ( sin ϕ ) 3

(5-154)

CHAPTER 107 Model Generation

while for nondilatant flow they give

tan β =

3 sin ϕ and d--- = ϕ cos ϕ c

0 In either case, σ c is immediately available as:

1 0 σ c = ----------------------- d 1 1 – -- tan β 3

(5-155)

The difference between these two approaches increases with the friction angle but, for typical friction angles, the results are not very different, as illustrated in the table below. Mohr-Coulomb Friction Angle, Φ

10 °

20 ° 30 ° 40 ° 50 °

Associated Flow Drucker-Prager friction angle, β

16.7 °

d/c 1.70

30.2 °

1.60

39.8 °

1.44

46.2 °

1.24

50.5 °

1.02

Nondilatant Flow Drucker-Prager friction angle, β

16.7 ° 30.6 ° 40.9 ° 48.1 ° 53.0 °

d/c 1.70 1.63 1.50 1.33 1.11

Plane strain matching of Drucker-Prager and Mohr-Coulomb models. As strain rates increase, many materials show an increase in yield strength. This effect often becomes important when the strain rates are in the range of -0.1 to 1 per second, and can be very important if the strain rates are in the range of 10 to 100 per second, as commonly occurs in high energy dynamic events or in manufacturing processes. Temperature-Dependent Behavior This section discusses the effects of temperature-dependent plasticity on the constitutive relation. The following constitutive relations for thermo-plasticity were developed by Naghdi. Temperature effects are discussed using the isotropic hardening model and the von Mises yield condition. The stress rate can be expressed in the form

· · · σ ij = L ijkl ε kl + h ij T For elastic-plastic behavior, the moduli

(5-156)

L ijkl are

108 Modeling Guide

∂σ ∂σ L ijkl = C ijkl –  C ijmn ------------ ----------- C pqkl ⁄ D ∂σ mn ∂σ pq

(5-157)

and for purely elastic response

L ijkl = C ijkl

(5-158)

The term that relates the stress increment to the increment of temperature for elastic-plastic behavior is

∂σ 2 ∂σ h ij = X ij – C ijkl α kl –  C ijkl ----------  σ pq X pq – --- σ ------  ⁄ D ∂σ kl 3 ∂T

(5-159)

and for purely elastic response

H ij = X ij – C ijkl αkl

(5-160)

where

4 ∂σ ∂σ ∂σ D = --- σ 2 -------p- + --------- C ijkl ---------9 ∂σ ij ∂σ kl ∂ε

(5-161)

and

∂C ijkl e X ij = -------------- ε kl ∂T and

(5-162)

α kl are the coefficients of thermal expansion.

Temperature-Dependent Stress Strain Curves Starting in MD Nastran 2005, SOL 600 offers the capability of stress-strain curve dependence as a function of temperature. The user specifies these stress strain curves at different temperatures and then specifies the temperature to use for each subcase. Linear interpolation between the supplied curves is used to determine the appropriate curve at the temperature specified for a particular subcase. MSC.Marc’s AF-Flowmat capability is used for this capability; therefore, user subroutines do not have to be supplied. This capability is best explained with an example (this example can be obtained from MD Nastran development. The name of the file is mattep20.dat). SOL 600,NLSTATIC path=1 stop=1 TIME 10000 CEND ECHO = NONE DISPLACEMENT(plot) = ALL SPCFORCE(PLOT) = ALL Stress(PLOT) = ALL Strain(PLOT) = ALL SPC = 1

CHAPTER 109 Model Generation

NLPARM = 2 temp(init)=10 subcase 1 temp(load)=11 LOAD = 100 subcase 2 temp(load)=12 LOAD = 200 subcase 3 temp(load)=13 LOAD = 300 BEGIN BULK param,mrafflow,mymat0 param,mrtabls1,4 param,mrtabls2,1 NLPARM 2 10 AUTO 1 20 P PARAM,LGDISP,1 tempd, 10, 70. tempd, 11, 110. tempd, 12, 700. tempd, 13, 1100. $LOAD, 20, 1.0, 2.0, 1, 1.0, 2 load, 100, 1., 1., 1 load, 200, 1., -.5, 1 load, 300, 1., 1.1, 1 PLOAD4 1 1 -15. . . . $ Constraint Set 1 : Untitled SPC 1 1 123456 0. SPC 1 8 123456 0. SPC 1 15 123456 0. SPC 1 22 123456 0. SPC 1 29 123456 0. $ Property 1 : Untitled PSHELL 1 1 0.125 1 1 0. $ Material 1 : AISI 4340 Steel MATEP, 1,TABLE, 35000., 2,CAUCHY,ISOTROP,ADDMEAN MAT1 1 2.9E+7 0.327.331E-4 6.6E-6 70. +MT +MT 1 215000. 240000. 156000. MAT4 14.861E-4 38.647.331E-4 $ 1 2 3 4 5 6 7 8 9 $2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 MATTEP 1 21 MATT1 1 7 TABLEM1 7 + 70.0 6.6E-6 1000. 6.5E-6 1200. 6.4E-6 1500. 6.3E-6 + 2000. 6.2E-6 ENDT $2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 2345678 TABLEST 21 + 70.0 31 1000. 32 1200. 33 1500. 34 + 2000. 35 ENDT TABLES1, 31 , 0., 15000., 1.0, 16000., 10., 25000., 100., 30000., , 99999., 40000., ENDT TABLES1, 32 , 0., 13000., 1.0, 14000., 10., 23000., 100., 28000., , 99999., 28000., ENDT TABLES1, 33

1

110 Modeling Guide

, 0., 11000., 1.0, , 99999., 25000., TABLES1, 34 , 0., 9000., 1.0, , 99999., 24000., TABLES1, 35 , 0., 5000., 1.0, , 99999., 15000., GRID 1 . . . CQUAD4 . . . ENDDATA

12000., 10., 21000., 100., 26000., ENDT 10000., 10., 19000., 100., 22000., ENDT 7000., 10., ENDT 0 0.

9000., 100., 13000., 0.

0.

0

In this input, the stress strain curves are specified by TABLES1 entries. The collection of stress-strain curves to be used is specified in the TABLEST entry and the corresponding temperatures at which they apply is specified in the TABLEM1 entry. The TABLEM1 ID is called out in field 7 of the MATT1 entry and the TABLEST ID is called out in field 5 of the MATTEP entry. TABLEST must list the stress strain TABLES1 IDs in order of increasing temperature and the first ID must be at the lowest temperature specified anywhere in the analysis. In this example, it is a temperature of 70 corresponding to temp(init)=10 in the Case Control. Similarly, the temperatures in the TABLEM1 entry must be in increasing order. The stress-strain curves should cover the entire range of temperatures for the analysis so that no extrapolation is needed. The actual temperatures for each subcase are given by the temp(load) specifications for each subcase. There is one parameter that is critical to this analysis: param,mrafflow,mymat0

Name of the file containing temperature dependent stress versus plastic strain curves in MSC.Marc’s AF_flowmat format. This file can be generated from the current MD Nastran run using TABLEST and TABLES1 entries or a pre-existing file can be used depending on the value of PARAM,MRAFFLOR. The extension “.mat” will be added to Name. If this is a new file, it will be saved in the directory from which the MD Nastran execution is submitted. If a pre-existing file is to be used, it can either be located in the directory where the MD Nastran execution is submitted and run or in the MSC.Marc AF_flowmat directory.

Specifying Elastoplastic Material Entries Each of the elastoplastic models described in this section can be selected with the MATEP bulk data entry.

CHAPTER 111 Model Generation

Entry MATEP MATTEP

Description Specifies elasto-plastic material properties to be used for large deformation analysis. Specifies temperature-dependent elasto-plastic material properties to be used for static, quasi-static, or transient dynamic analysis.

References • MATEP in the MD NASTRAN QRG. • MATTEP in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define an inelastic material in SimXpert: 1. Select Materials and Properties>Isotropic or Orthotropic or Anisotropic>Advanced>Add Constitutive Model>Elasto Plastic. 2. Enter parameter values. 3. Click OK. The required properties for describing elasticplastic behavior vary based on material type, dimension, type of nonlinear data input, hardening rule, yield criteria, strain rate method, and thermal dependencies. The table below shows the various input options and criteria available to you for defining elastoplastic behavior.

112 Modeling Guide

Elasto Plastic Model Summary Constitutive Nonlinear Data Hardening Yield Criteria Model Input Rule • Plastic • Stress/Strain • Isotropic • von Mises Curve • Kinematic • Tresca • Combined

• Mohr-Coulomb • Drucker-Prager

Strain Rate Method • Piecewise Linear • Cowper-

Symonds

• Parabolic Mohr-

Coulomb • Buyukozturk Concrete • Oak Ridge National

Lab • 2-1/4 Cr-Mo ORNL • Reversed Plasticity

ORNL • Full Alpha Reset • Hardening Slope

• Isotropic

ORNL • von Mises

• Kinematic

• Tresca

• Combined

• Mohr-Coulomb • Drucker-Prager

• None

CHAPTER 113 Model Generation

Elasto Plastic Model Summary Constitutive Hardening Model Rule Type Yield Criteria • Plastic • Perfectly Plastic • None • von Mises

Strain Rate Method • Piecewise Linear • Linear Mohr-Coulomb • Cowper• Parabolic MohrSymonds Coulomb • Buyukozturk Concrete • Oak Ridge National

Lab • 2-1/4 Cr-Mo ORNL • Reversed Plasticity

ORNL • Full Alpha Reset

ORNL • Power Law • Rate Power Law • Johnson-Cook • Kumar • Piecewise

Linear

• None

• Piecewise

Linear • Cowper-

Symonds Nonlinear Data Input

The type of nonlinear data input you choose to use to define elastoplastic material behavior determines the input data required for the Input Properties subform on the Materials Application form. • Stress/Strain Curve - All stress-strain curves are input as piecewise linear. SimXpert transfers the stress-strain curve input on the material property field directly to the TABLES1 entry.

The number of linear segments used to define the stress-strain curve may be different from one material to another. The same strain breakpoints need not be used for all of the different material’s stress-strain curves. It is recommended to define the stress-strain curves throughout the range of strains which the analysis is likely to predict. If the analysis predicts a plastic strain greater than the last point defined by the user, MD Nastran Implicit Nonlinear continues the analysis after shifting the last strain breakpoint on that curve to match the predicted value, thereby changing (reducing) the work hardening slope for the last segment of the curve. • Hardening Slope - The hardening slope and the yield point are required with this Nonlinear Data Input option. • Perfectly Plastic - Perfect plasticity is described by simply specifying the yield point.

114 Modeling Guide

The tables below provide descriptions for the input data for each of the four types of nonlinear input. Isotropic - Stress/Strain Curve or Perfectly Plastic: All Yield Functions Property Name

Description

Stress /Strain Curve

Defines the Cauchy stress vs. logarithmic strain (also called equivalent tensile stress versus total equivalent strain) by reference to a table. For Perfectly Plastic models, only a Yield Stress needs to be entered.

or Yield Stress

Can also be strain rate dependent if Strain Rate Method is Piecewise Linear. Accepts table of yield stress vs. strain rate. 10th Cycle Yield Stress vs. Plastic Strain

When set to ORNL, accepts field of 10th cycle yield stress vs. plastic strain. Can be temperature dependent also. For Perfectly Plastic models, only a 10th Cycle Yield Stress needs to be entered.

or 10th Cycle Yield Stress Coefficient C

Visible if Strain Rate Method is Cowper-Symonds.

Inverse Exponent P

Visible if Strain Rate Method is Cowper-Symonds.

Alpha

When set to Linear Mohr-Coulomb, defines the slope of the yield surface in square root J2 versus J1 space. This property is required.

Beta

When set to Parabolic Mohr-Coulomb, defines the beta parameter in the equation that defines the parabolic yield surface in square root J2 versus J1 space. This property is required.

Note:

2 1/4 Cr-Mo ORNL, Reversed Plasticity ORNL, Full Alpha Reset ORNL are the same as Oak Ridge National Labs. Generalized Plasticity is the same as von Mises. Perfectly Plastic is identical to Stress/Strain except that no hardening rules apply.

CHAPTER 115 Model Generation

Anisotropic/Orthotropic - Stress/Strain Curve or Perfectly Plastic: All Yield Functions Description Stress vs. Strain or Tensile Yield Stress

Same as description for Isotropic Elastic-Plastic. If Strain Rate Method is Piecewise Linear, accepts field of yield stress vs. strain rate. Or defines an isotropic yield stress. It is a required property when the plasticity type is Perfectly Plastic.

Stress 11/22/33 Yield Ratios Defines the ratios of direct yield stresses to the isotropic yield stress in the element’s coordinate system. Stress 12/23/31 Yield Ratios Defines the ratios of shear yield stresses to the isotropic shear yield stress (yield divided by square root three) in the element’s coordinate system. Note:

Perfectly Plastic is identical to Elastic-Plastic except that no hardening rules apply. Stress vs Plastic Strain is replaced with Yield Stress data only as is 10th Cycle Yield vs. Strain replaced with 10th Cycle Yield Stress data. Thus no tabular data is necessary.

Hardening Slope - Nonlinear Data Input

Isotropic/Orthotropic/Anisotropic - Hardening Slope Property Name

Description

Hardening Slope

Slope of the stress-strain curve once yielding has started.

Yield Point

Defines the stress level at which plastic strain begins to develop.

Internal Friction Angle

When yield function is set to Mohr-Coulomb or Drucker-Prager this gives the parameter describing the effect of hydrostatic pressure on the yield stress.

Failure and Damage Models One of the nonlinear features of a material's behavior is failure. When a certain criterion (failure criterion) is met, the material fails and no longer sustains its loading and breaks. In a finite-element method, this means that the element, where the material reaches the failure limit, cannot carry any stresses anymore. The stress tensor is effectively zero. The element is flagged for failure, and, essentially, is no longer part of the structure. Failure criteria can be defined for a range of materials and element types. The failure models are referenced from the material definition entries.

116 Modeling Guide

Isotropic/Orthotropic/Anisotropic Failure Models For isotropic, 2-D orthotropic, and 2-D anisotropic materials, you can implement one of five failure models in MD Nastran Implicit Nonlinear (SOL 600). Failure models are based on maximum stress criteria, maximum strain criteria, or one of three composite stress/strain failure theories. Failure Model

Applicable Material Type

Maximum Stress

Isotropic, 2-D Orthotropic, 2-D Anisotropic

Maximum Strain

2-D Orthotropic

Hill

Isotropic, 2-D Orthotropic (stress or strain based), 2-D Anisotropic

Hoffman

Isotropic, 2-D Orthotropic (stress or strain based), 2-D Anisotropic

Tsai-Wu

Isotropic, 2-D Orthotropic (stress or strain based), 2-D Anisotropic

Maximum Stress Criterion

At each integration point, MD Nastran Implicit Nonlinear calculates six quantities:

1.

2.

3.

4.

σ -----1- X  ⁄ F

if

σ1 > 0

–σ -----1-  X c ⁄ F

if

σ1 < 0

t

(5-163)

σ  -----2- ⁄ F  Yt 

if

σ2 > 0

σ  – -----2- ⁄ F  Yc 

if

σ2 < 0

σ -----3-  Zt  ⁄ F

if

σ3 > 0

–σ -----3-  Z c ⁄ F

if

σ3 < 0

σ 12  ⁄ F  ------S 12 

(5-164)

(5-165) (5-166)

CHAPTER 117 Model Generation

5.

σ 23  ⁄ F  ------S 23 

(5-167)

6.

σ 31  ⁄ F  ------S 31 

(5-168)

where

F

is the failure index (F =1.0).

X t, X c

are the maximum allowable stresses in the 1-direction in tension and compression.

Y t, Y c

are maximum allowable stresses in the 2-direction in tension and compression.

Z t, Z c

are maximum allowed stresses in the 3-direction in tension and compression.

S 12

is the maximum allowable in-plane shear stress.

S 23

is the maximum allowable 23 shear stress.

S 31

is the maximum allowable 31 shear stress.

Maximum Strain Failure Criterion

At each integration point, calculates six quantities:

1.

ε1   ----- ⁄F  e 1t ε1   – ----- e 1c ⁄ F

2.

ε2   ---- e 2t ⁄ F ε2   – ----- e 2c ⁄ F

if

ε1 > 0 (5-169)

if

if

ε1 < 0 ε2 > 0 (5-170)

if

ε2 < 0

118 Modeling Guide

3.

ε3   ---- e 3t ⁄ F

if

ε3   – ------ ⁄F  e 3c

if

ε3 > 0 (5-171)

ε3 < 0

4.

γ 12   -----⁄F  g - 12

(5-172)

5.

γ23   ----- g - ⁄F 23

(5-173)

6.

γ 31   ----- g - ⁄F 31

(5-174)

where

F

is the failure index (F=1.0).

e 1t, e 1c

are the maximum allowable strains in the 1 direction in tension and compression.

e 2t, e 2c

are the maximum allowable strains in the 2 direction in tension and compression.

e 3t, e 3c

are the maximum allowable strains in the 3 direction in tension and compression.

g 12

is the maximum allowable shear strain in the 12 plane.

g 23

is the maximum allowable shear strain in the 23 plane.

g 31

is the maximum allowable shear strain in the 31 plane.

Hill Failure Criterion

Assumptions: • Orthotropic materials only • Incompressibility during plastic deformation • Tensile and compressive behavior are identical

At each integration point, MD Nastran Implicit Nonlinear calculates:

CHAPTER 119 Model Generation

σ 12 σ 22 σ 32  1 1 ---1 1 1 1 ------ + ------ + ------ – ------ + ----– 2- σ 1 σ 2 –  -----2- + ----2- – ----2- σ 1 σ 3 2 2 2  2 2 X Y Z X Y Z X Z Y 2 2 2 σ 12 σ 13 σ 23 1 1 1 - + -------- + ------- ⁄F –  -----2 + ----2- – -----2- σ 2 σ 3 + ------2 2 2   S S S Y Z X 12 13 23

(5-175)

For plane stress condition, it becomes 2

2

2

 σ 1 σ 1 σ 2 σ 2 σ 12  - + ------ + -------- ⁄ F  -----2- – ----------2 X2 Y 2 S 12 X 

(5-176)

where

X

is the maximum allowable stress in the 1 direction

Y

is the maximum allowable stress in the 2 direction

Z

is the maximum allowable stress in the 3 direction

S 12, S 23, S 31, F are as before Hoffman Failure Criterion

Note:

Hoffman criterion is essentially Hill criterion modified to allow unequal maximum allowable stresses in tension and compression.

At each integration point, MD Nastran Implicit Nonlinear calculates: 2

2

2

[ C1 ( σ2 – σ3 ) + C2 ( σ3 – σ1 ) + C3 ( σ1 – σ2 ) + C4 σ1 + C5 σ2 2 + C σ2 + C σ2 ] ⁄ F + C 6 σ 3 + C 7 σ 23 8 13 9 12 with

(5-177)

120 Modeling Guide

1 1 1 1 C 1 = ---  ---------- + ---------- – -----------  2 Z t Z c Y t Y c X t X c 1 1 1 1 C 2 = ---  ----------- + ---------- – ----------  2 Xt X c Z t Z c Y t Y c 1 1 1 1 C 3 = ---  ----------- + ---------- – ----------  2 Xt X c Y t Y c Z t Z c 1 1 C 4 = ----- – ----Xt Xc 1 1 C 5 = ---- – ----Yt Yc 1 1 C 6 = ---- – ----Zt Zc 1C 7 = ------2 S 23 1C 8 = ------2 S 13 1C 9 = ------2 S 12

(5-178)

For plane stress condition, it becomes 2

2

2

σ1 σ2 σ 12 σ 1 σ 2   1 1  1- ---1- - – ----- σ 1 +  --------------------------- -----------– σ + + +   ---  Y t Y c 2 X t X c Y t Y c S 2 – X t Xc  ⁄ F  X t Xc  12 where:

Note:

(5-179)

X t, X c, Y t, Y c, Z t, Z c, S 12, S 23, S 31, F are as before.

For small ratios of, for example,

σ1 ------ , the Hoffman criteria can become negative due to the Xt

presence of the linear terms. Tsai-Wu Failure Criterion

Tsai-Wu is a tensor polynomial failure criterion. At each integration point, MD Nastran Implicit Nonlinear calculates:

CHAPTER 121 Model Generation

σ 12 σ 22 σ 32 1- ----1 1- ---1- 1 ---1-  --- -- ----------------------------– σ + – σ + – σ + + +  Xt X c 1  Y t Y c 2  Z t Z c 3 Xt X c Y t Y c Z t Z c 2 2 2 τ 12 τ 23 τ 13 - + ------- + ------- + 2F 12 σ 1 σ 2 + 2F 23 σ 2 σ 3 + 2F13 σ 1 σ 3 ] ⁄ F + ------2 2 2 S 12 S 23 S 13

where

(5-180)

X t, X c, Y t, Y c, Z t, Z c, S 12, S 23, S31, F are as before.

F 12

Interactive strength constant for the 12 plane

F 23

Interactive strength constant for the 23 plane

F 13

Interactive strength constant for the 31 plane For plane stress condition, it becomes 2

2

2

σ1 σ2 σ 12  1 1   1 ---1- - – ----- σ 1 +  -------------- + --------- + -------– σ + + 2F σ σ   ---⁄ F 2 12 1 2   Y 2 Y c X t X c Y t Y c S 12  Xt X c  Note:

(5-181)

In order for the Tsai-Wu failure surface to be closed,

1 - --------12 < ---------F 12 • Xt Xc Yt Yc

1 - --------12 < --------F 23 • Yt Yc Zt Zc

1 - --------12 < ---------F 31 • X t Xc Zt Zc

See Wu, R.Y. and Stachurski, 2, “Evaluation of the Normal Stress Interaction Parameter in the Tensor Polynomial Strength Theory for Anisotropic Materials”, Journal of Composite Materials, Vol. 18, Sept. 1984, pp. 456-463. Interlaminar Shear for Thick Shell and Beam Elements

Calculation of interlaminar shear stress (a parabolic distribution through the thickness direction) for thick shells and beams is available. These interlaminar shears are printed in the local coordinate system above and below each layer selected for printing. These values are also available for postprocessing. PARAM,MRTSHEAR,1 must be used for activating the parabolic shear distribution calculations. In MD Nastran Implicit Nonlinear, the distribution of transverse shear strains through the thickness for thick shell and beam elements was assumed to be constant. From basic strength of materials and the equilibrium of a beam cross section, it is known that the actual distribution is more parabolic in nature. As an additional option, the formulations for certain beam and shell elements have been modified to include a parabolic distribution of transverse shear strain. The formulation is exact for MSC.Marc beam

122 Modeling Guide

element 45, but is approximate for MSC.Marc thick shell elements 22, 75, and 140. Nevertheless, the approximation is expected to give improved results from the previous constant shear distribution. Furthermore, interlaminar shear stresses for composite beams and shells can be easily calculated. With the assumption that the stresses in the condition through the thickness is given by

1

2

V and V direction are uncoupled, the equilibrium

∂τ ( z )- ∂σ (z) -----------+ -------------- = 0 ∂z ∂x where

σ ( z ) is the layer axial stress; τ ( t ) is the layer shear stress. From beam theory, we have

∂M V + -------- = 0 ∂x where

(5-182)

(5-183)

M is the section bending moment and V is the shear force. Assuming that

σ ( z ) = f ( z )M

(5-184)

by taking the derivative of Equation (5-184) with respect to x, substituting the result into Equation (5-182), using Equation (5-183) and integrating, we obtain

τ(z) =

 f ( z )dz • V

(5-185)

z

The function

f ( z ) is given from beam theory as

E0 ( z ) f ( z ) = ------------- ( z – z ) EI where

E0 ( z )

Mz σ ( z ) = – ------I

(5-186)

is the layer initial Young’s modulus, z is the location of the neutral axis and EI is the section bending moment of inertia. Equation (5-186) and Equation (5-184) express the usual bending relation (5-187)

except that these two equations are written so that the z = 0 axis is not necessarily the neutral axis of bending. With respect to this axis, membrane and bending action is, in general, coupled. Note that

CHAPTER 123 Model Generation

 z E ( z )dz z z = -------------------- E ( z )dz

(5-188)

z

and stress

τ ( z ) = 0 at the top and bottom surface of the shell.

Interlaminar Stresses for Continuum Composite Elements

In MD Nastran Implicit Nonlinear, the interlaminar shear and normal stresses are calculated by averaging the stresses in the stacked layers. The stresses are transformed into a component tangent to the interface and a component normal to the interface. The two components, considered as shear stress and normal stress, respectively, are printed out in the output file. Progressive Composite Failure

A model has been put into MD Nastran Implicit Nonlinear to allow the progressive failure of certain types of composite materials. The aspects of this model are defined below: 1. Failure occurs when any one of the failure criteria is satisfied. 2. The behavior up to the failure point is linear elastic. 3. Upon failure, the material moduli for orthotropic materials at the integration points are changed such that all of the moduli have the lowest moduli entered. 4. Upon failure, for isotropic materials, the failed moduli are taken as 10% of the original moduli. 5. If there is only one modulus, such as in a beam or truss problem, the failed modulus is taken as 10% of the original one. 6. There is no healing of the material. Specifying the Failure Criteria

Any of the failure models described above can be selected with the MATF Bulk Data entry. Entry

Description

MATF

Specifies failure model properties for linear elastic materials to be used for static, quasi static or transient dynamic analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

References • MATF in the MD NASTRAN QRG. Defining Failure Models in SimXpert

124 Modeling Guide

To define a Failure Model in MSC SimXpert: 1. From the Materials Application form, select one of the following: • Materials and Properties>Isotropic>Advanced>Add Constitutive Model>Failure • Materials and Properties>2D Orthotropic>Advanced>Add Constitutive Model>Failure • Materials and Properties>2D Anisotropic>Advanced>Add Constitutive Model>Failure

2. Enter parameter values. 3. Click OK.

CHAPTER 125 Model Generation

126 Modeling Guide

Isotropic Material Input Data

Isotropic materials require the following failure model data: Failure Theory : Hill, Hoffman, Tsai-Wu, Maximum Stress

Property Name

Description

Tension Stress Limit

Defines the tension stress (or strain) limits in the element’s coordinate system.

Compression Stress Limit Defines the compression stress (or strain) limits in the element’s coordinate system. Absolute values are used. Shear Stress Limit

Defines the shear stress (or strain) limits.

3-D Orthotropic Material Input Data

3-D orthotropic materials require the following failure model data: Failure Theory : Hill, Hoffman, Tsai-Wu, Maximum Stress, Maximum Strain

Property Name

Description

Tension Stress (Strain) Limit ii

Defines the tension stress (or strain) limits in direction ii.

Compression Stress (Strain) Limit ii

Defines the compression stress (or strain) limits in direction ii.

Shear Stress (Strain) Limit ij

Defines the shear stress (or strain) limits in direction ij.

3-D Anisotropic Material Input Data

3-D anisotropic materials require the following failure model data: Failure Theory : Hill, Hoffman, Tsai-Wu, Maximum Stress

Property Name

Description

Tension Stress (Strain) Limit

Defines the tension stress (or strain) limits.

Compression Stress (Strain) Limit

Defines the compression stress (or strain) limits.

Shear Stress (Strain) Limit

Defines the shear stress (or strain) limits.

Damage Models In many structural applications, the finite element method is used to predict failure. This is often performed by comparing the calculated solution to some failure criteria, or by using classical fracture mechanics. Ductile Metals

CHAPTER 127 Model Generation

In ductile materials given the appropriate loading conditions, voids will form in the material, grow, then coalesce, leading to crack formation and potentially, failure. Experimental studies have shown that these processes are strongly influenced by hydrostatic stress. Gurson studied microscopic voids in materials and derived a set of modified constitutive equations for elastic-plastic materials. Tvergaard and Needleman modified the model with respect to the behavior for small void volume fractions and for void coalescence. In the modified Gurson model, the amount of damage is indicated with a scalar parameter called the void volume fraction f. The yield criterion for the macroscopic assembly of voids and matrix material is given by:

q 2 σ kk σ 2 F =  ----- + 2q 1 f∗ cosh  ------------- – [ 1 + ( q 1 f∗ ) 2 ] =  σ y  2σ y 

(5-189)

as seen in Figure 5-34. σe ⁄ σM 1.0

f*

=

0

f * ⁄ f * = 0.01 u

0.5 0.1 0.6

0.3

0.9 0 0

Figure 5-34

1

2

3

4 σ kk ⁄ 3σ M

Plot of Yield Surfaces in Gurson Model

The parameter q 1 was introduced by Tvergaard to improve the Gurson model at small values of the void volume fraction. For solids with periodically spaced voids, numerical studies [10] showed that the values of

q 1 = 1.5 and q 2 = 1 were quite accurate.

The evolution of damage as measured by the void volume fraction is due to void nucleation and growth. Void nucleation occurs by debonding of second phase particles. The strain for nucleation depends on the particle sizes. Assuming a normal distribution of particle sizes, the nucleation of voids is itself modeled as a normal distribution in the strains, if nucleation is strain controlled. If void nucleation is assumed to be stress controlled in the matrix, a normal distribution is assumed in the stresses. The original Gurson model predicts that ultimate failure occurs when the void volume fraction f, reaches unity. This is too high a value and, hence, the void volume fraction f is replaced by the modified void volume fraction in the yield function.

f∗

128 Modeling Guide

The parameter f∗ is introduced to model the rapid decrease in load carrying capacity if void coalescence occurs.

f∗ = f

if f ≤ fc

f u* – f c f∗ = f c +  -------------- ( f – f c )  f F – f c

if f > fc

(5-190)

where fc is the critical void volume fraction, and f F is the void volume at failure, and f u* safe choice for f F would be a value greater than

= 1 ⁄ q1 . A

( 1 ⁄ q 1 ) namely, f F = 1.1 ⁄ q 1 . Hence, you can

control the void volume fraction, f F , at which the solid loses all stress carrying capability. Numerical studies show that plasticity starts to localize between voids at void volume fractions as low as 0.1 to 0.2. You can control the void volume fraction f c , beyond which void-void interaction is modeled by MD Nastran Implicit Nonlinear. Based on the classical studies, a value of f c

= 0.2 can be chosen.

The existing value of the void volume fraction changes due to the growth of existing voids and due to the nucleation of new voids.

· · · f = f growth + f nucleation

(5-191)

The growth of voids can be determined based upon compressibility of the matrix material surrounding the void.

· ·p f growth = ( 1 – f ) ε kk

(5-192)

As mentioned earlier, the nucleation of new voids can be defined as either strain or stress controlled. Both follow a normal distribution about a mean value. In the case of strain controlled nucleation, this is given by

fN ε mp – ε n 2 · p · - exp – 1---  ---------------f nucleation = ------------m 2 S  ε S 2π

(5-193)

where f N is the volume fraction of void forming particles, ε n the mean strain for void nucleation and

S the standard deviation. In the case of stress controlled nucleation, the rate of nucleation is given by:

CHAPTER 129 Model Generation

· f nucleation

2 1--σ σ + – σ   · 1· kk n fN 1 3 = -------------- exp – ---  --------------------------------- * σ + --- σ kk  3 2 S S 2π  

(5-194)

If the second phase particle sizes in the solid are widely varied in size, the standard deviation would be larger than in the case when the particle sizes are more uniform. The MD Nastran Implicit Nonlinear user can also input the volume fraction of the nucleating second phase void nucleating particles in the input deck, as the variable f N . A typical set of values for an engineering alloy is given by Tvergaard for strain controlled nucleation as

ε n = 0.30 ; f N = 0.04 ; S = 0.01

(5-195)

It must be remarked that the determination of the three above constants from experiments is extremely difficult. The modeling of the debonding process must itself be studied including the effect of differing particle sizes in a matrix. It is safe to say that such an experimental study is not possible. The above three constants must necessarily be obtained by intuition keeping in mind the meaning of the terms. When the material reaches 90 percent of f F , the material is considered to be failed. At this point, the stiffness and the stress at this element are reduced to zero. Elastomers

Under repeated application of loads, elastomers undergo damage by mechanisms involving chain breakage, multi-chain damage, micro-void formation, and micro-structural degradation due to detachment of filler particles from the network entanglement. Two types of phenomenological models namely, discontinuous and continuous, exists to simulate the phenomenon of damage. Discontinuous Damage

The discontinuous damage model simulates the “Mullins’ effect” as shown in Figure 5-35.

Figure 5-35

Discontinuous Damage

130 Modeling Guide

This involves a loss of stiffness below the previously attained maximum strain. The higher the maximum attained strain, the larger is the loss of stiffness. Upon reloading, the uniaxial stress-strain curve remains insensitive to prior behavior at strains above the previously attained maximum in a cyclic test. Hence, there is a progressive stiffness loss with increasing maximum strain amplitude. Also, most of the stiffness loss takes place in the few earliest cycles provided the maximum strain level is not increased. This phenomenon is found in both filled as well as natural rubber although the higher levels of carbon black particles increase the hysteresis and the loss of stiffness. The free energy, W, can be written as:

W = K ( α, β )W where

0

(5-196)

0

W is the nominal strain energy function, and 0

α = max ( W )

(5-197)

determines the evolution of the discontinuous damage. The reduced form of Clausius-Duhem dissipation inequality yields the stress as: 0

∂W S = 2K ( α ,β ) ---------∂C

(5-198)

Mathematically, the discontinuous damage model has a structure very similar to that of strain space plasticity. Hence, if a damage surface is defined as:

Φ = W–α≤0

(5-199)

The loading condition for damage can be expressed in terms of the Kuhn-Tucker conditions:

· α≥0

Φ≤0

· αΦ = 0

(5-200)

The consistent tangent can be derived as: 2

0

0

0

∂ W ∂K ∂W ∂W C = 4 K --------------- + ---------0- ---------- ⊗ ---------∂C∂C ∂W ∂C ∂C

(5-201)

Continuous Damage

The continuous damage model can simulate the damage accumulation for strain cycles for which the values of effective energy is below the maximum attained value of the past history as shown in Figure 5-36.

CHAPTER 131 Model Generation

Figure 5-36

Continuous Damage

This model can be used to simulate fatigue behavior. More realistic modeling of fatigue would require a departure from the phenomenological approach to damage. The evolution of continuous damage parameter is governed by the arc length of the effective strain energy as: t

β =

∂

-W  -----∂s′

0

( s′ ) ds′

(5-202)

0

Hence, β accumulates continuously within the deformation process. The Kachanov factor K ( α, β ) is implemented in MD Nastran Implicit Nonlinear through both an additive as well as a multiplicative decomposition of these two effects as: 2 ∞

K ( α, β ) = d +

 n=1 2

∞

K ( α, β ) = d +

α dn

α exp  – ------ +  η n

2 β

 dn n=1

β exp  – -----  λ n

(5-203)

α + δn β

-  dn exp  – -----------------ηn 

(5-204)

n=1

α

β

You specify the phenomenological parameters d n , d n ,

∞

α and β , the Kachanov factor K = 1 . If, (5-204) the value of K exceeds 1, K is set back to 1.

it is automatically determined such that, at zero values of according to Equation (5-203) or Equation

∞

η n, λ n, d n, δ n and d . If d is not defined,

132 Modeling Guide

The above damage model is available for deviatoric behavior. In addition, viscoelastic behavior can be included. Finally, the user subroutine, UELDAM available starting in version 2005, can be used to define damage functions different from Equation (5-211) to Equation (5-214). The parameters required for the continuous or discontinuous damage model can be obtained using the experimental data fitting option in Mentat. Specifying Hyperelastic Damage Model Entries

The hyperelastic damage model described above can be selected with the MATHED Bulk Data entry. Entry MATHED

Description Specifies damage model properties for hyperelastic materials to be used for static, quasi static or transient dynamic analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

References • MATHED in the MD NASTRAN QRG. SimXpert Materials Application Input Data.

Creep Creep is an important factor in elevated-temperature stress analysis. In MD Nastran Implicit Nonlinear, creep is represented by a Maxwell model. Creep is a time-dependent, inelastic behavior, and can occur at any stress level (that is, either below or above the yield stress of a material). The creep behavior can be characterized as primary, secondary, and tertiary creep, as shown in Figure 5-39. Engineering analysis is often limited to the primary and secondary creep regions. Tertiary creep in a uniaxial specimen is usually associated with geometric instabilities, such as necking. The major difference between the primary and secondary creep is that the creep strain rate is much larger in the primary creep region than it is in the secondary creep region. The creep strain rate is the slope of the creep strain-time curve. The creep strain rate is generally dependent on stress, temperature, and time. The creep data can be specified in either an exponent form or in a piecewise linear curve.

· dε c ε c = ------dt

(5-205)

CHAPTER 133 Model Generation

Creep Strain εC Tertiary Creep Secondary Creep Primary Creep

Time (t)

Note:

Figure 5-37

Primary Creep: Fast decrease in creep strain rate Secondary Creep: Slow decrease in creep strain rate Tertiary Creep: Fast increase in creep strain rate

Creep Strain Versus Time (Uniaxial Test at Constant Stress and Temperature)

Forms of Creep Material Law

There are three possible modes of input for creep constitutive data. 1. Express the dependence of equivalent creep strain rate on any independent parameter through a piecewise linear relationship. The equivalent creep strain rate is then assumed to be a piecewise linear approximation to

· dk ( t ) ε c = A • f ( σ ) • g ( ε c ) • h ( T ) • -----------dt

(5-206)

·c c ε is equivalent creep strain rate; and σ , ε , T , and t are equivalent stress, equivalent creep strain, temperature and time, respectively. The functions f , g , h , and k are piecewise linear. This representation is shown in Figure 5-40. (Any of the functions ( f , g , h , or k ) can be set to unity by setting the number of piecewise linear slopes for that relation to

where A is a constant;

zero on the input data.) 2. The dependence of equivalent creep strain rate on any independent parameter can be given directly in power law form by the appropriate exponent. The equivalent creep strain rate is

· · n ε c = Aσ m • ( ε c ) • T p • ( qt q – 1 )

(5-207)

This is often adequate for engineering metals at constant temperature where Norton’s rule is a good approximation.

· εc = Aσn

(5-208)

134 Modeling Guide

3. Use the MATEP material to activate the ORNL (Oak Ridge National Laboratory rules) capability of the program. Isotropic creep behavior is based on a von Mises creep potential described by the equivalent creep law

· · ε = f ( σ, ε c, T, t )

(5-209) F4 F3

Function F (X) [Such as t ( σ ) , g(ε

c

F2

S3

S2

) , h (T),

k (t)]

S1 F1

X1

X2

X3

X4

Variable X (Such as σ, εC, T, t) (1) Slope-Break Point Data S1X1 S2X2 S3X3 (2) Function-Variable Data F1X1 F2X2 F3X3 F4X4

Figure 5-38

Piecewise Linear Representation of Creep Data

The material creep behavior is described by

· c  ∂σ  ·c ε ij = ε  --------∂σ  

ij 

(5-210)

During creep, the creep strain rate usually decreases. This effect is called creep hardening and can be a function of time or creep strain. The following section discusses the difference between these two types of hardening. Consider a simple power law that illustrates the difference between time and strain-hardening rules for the calculation of the creep strain rate. c

ε = βt n

(5-211)

CHAPTER 135 Model Generation

where

c

ε is the creep strain, β and n are values obtained from experiments and t is time. The creep

rate can be obtained by taking the derivative

c

ε with respect to time

c ·c -------- = nβt n – 1 ε = dε

(5-212)

dt

However,

t being greater than 0, we can compute the time t as

c 1/n

ε t =  ---- β

(5-213)

Substituting Equation (5-209) into Equation (5-212) we have

·c ε = nβt n – 1 = n ( β 1 ⁄ n ( ε c ) ( ( n – 1 ) ⁄ n ) )

(5-214)

Equation (5-213) shows that the creep strain rate is a function of time (time hardening). Equation (5-214) indicates that the creep strain rate is dependent on the creep strain (strain hardening). The creep strain rates calculated from these two hardening rules generally are different. The selection of a hardening rule in creep analysis must be based on data obtained from experimental results. Figure 5-41 and Figure 5-42 show time and strain hardening rules in a variable state of stress. It is assumed that the stress in a structure

varies from

σ 1 to σ 2 to σ 3 ; depending upon the model chosen, different creep strain rates are

calculated accordingly at points 1, 2, 3, and 4. Obviously, creep strain rates obtained from the time hardening rule are quite different from those obtained by the strain hardening rule. εc

σ1 σ2

3

σ3

1 4 2 0

t

Figure 5-39

Time Hardening

136 Modeling Guide

εc

σ1 σ2

3 1 2

σ3 4

0 t

Figure 5-40

Strain Hardening

Oak Ridge National Laboratory Laws Oak Ridge National Laboratory (ORNL) has performed a large number of creep tests on stainless and other alloy steels. It has also set certain rules that characterize creep behavior for application in the nuclear structures. A summary of the ORNL rules on creep is discussed in MSC.Marc Volume A, Theory and User Information. The references listed at the end of this section offer a more detailed discussion of the ORNL rules. Viscoplasticity (Explicit Formulation) The creep (Maxwell) model can be modified to include a plastic element (as shown in Figure 5-43). This plastic element is inactive when the stress ( σ ) is less than the yield stress ( σ y ) of the material. The modified model is an elasto-viscoplasticity model and is capable of producing some observed effects of creep and plasticity. In addition, the viscoplastic model can be used to generate time-independent plasticity solutions when stationary conditions are reached. At the other extreme, the viscoplastic model can reproduce standard creep phenomena. The model allows the treatment of nonassociated flow rules and strain softening which present difficulties in conventional (tangent modulus) plasticity analyses. It is recommended that you use the implicit formulation described in the following paragraphs to model general viscoplastic materials.

CHAPTER 137 Model Generation

σ

ee

evp

p

ε = ε

vp

Figure 5-41

Plastic Element Inactive if σ < σy

Uniaxial Representation of Viscoplastic Material

Creep (Implicit Formulation) This formulation, as opposed to that described in the previous section, is fully implicit. A fully implicit formulation is unconditionally stable for any choice of time step size; hence, allowing a larger time step than permissible using the explicit method. Additionally, this is more accurate than the explicit method. The disadvantage is that each increment may be more computationally expensive. There are two methods for defining the inelastic strain rate. The creep model definition option can be used to define a Maxwell creep model. The back stress must be specified through the field reserved for the yield stress in the MAT1 or other material definitions. There is no creep strain when the stress is less than the back stress. The equivalent creep strain increment is expressed as

·c ·c n m ε = Aσ • ( ε ) • T P • qt q – 1

(5-215)

and the inelastic deviatoric strain components are

3 i σ′ ij Δε iji = --- Δε -------2 σ where

σ′ij is the deviatoric stress at the end of the increment and σ y is the back stress. A is a function

of temperature, time, etc. Creep only occurs if

σ sigma is greater σ y .

One of three tangent matrices may be formed. The first uses an elastic tangent, which requires more iterations, but can be computationally efficient because re-assembly might not be required. The second uses an algorithmic tangent that provides the best behavior for small strain power law creep. The third uses a secant (approximate) tangent that gives the best behavior for general viscoplastic models.

138 Modeling Guide

Specifying Creep Material Entries Each of the creep models described in this section can be selected with the MATVP Bulk Data entry. MATVP is the only form of creep data material input supported by SOL 600, ie.e., no other MD Nastran creep data formats are supported by SOL 600. Entry

Description

MATVP

Specifies viscoplastic or creep material properties to be used for quasi-static analysis in MD Nastran Implicit Nonlinear (SOL 600) only.

References • MATVP in the MD NASTRAN QRG. SimXpert Materials Application Input Data

To define creep behavior in SimXpert: 1. Select Materials and Properties>Isotropic or Orthotropic or Anisotropic>Advanced>Add Constitutive Model>Creep. 2. Enter parameter values. 3. Click OK. Creep material models require the following MATVP material data: Creep

Isotropic/Orthotropic/Anisotropic

Description

Creep Data Input Form

Power Law

Creep Law Type

ID number for the emperical creep law type. The Creep Law Type is defined as three digits, Creep Law Type = ijk, where each is 1 or 2 (Class 1 equation), or all three together specify 300 (Class 2 equation). Class 1 eq.,

c

ε ( σ, t ) = A ( σ ) [ 1 – e

– R ( σ )t

] + K ( σ )t

Terms A(σ), R(σ), and K(σ) are specified as follows: b bσ A(σ) = aσ (i=1), or ae (i=2) dσ d R(σ) = ce (j=1), or cσ (j=2) g fσ K(σ) = e ⋅ sinh ( fσ ) (k=1), or ee (k=2) Class 2 eq.,

c

b d

ε ( σ, t ) = aσ t , where

1.0 < b < 8.0 , and 0.2 < d < 2.0 . Creep Reference Temperature

Reference temperature at which creep characteristics are defined.

CHAPTER 139 Model Generation

Isotropic/Orthotropic/Anisotropic

Description

Temperature Dependent Exp.

Temperature dependent term in the creep rate expression,

e

( – ΔH ) ⁄ ( R ⋅ T0 )

Creep Threshold Stress Limit

Threshold limit for creep process. Threshold stress under which creep does not occur is computed as Creep Threshold Stress Limit times Young’s modulus.

Creep Coefficient i , i = A,...,G

Coefficients of the imperical creep law specified in Creep Law Type

Creep Data Input Form

Table

Creep Reference Temperature

Reference temperature at which creep characteristics are defined.

Temperature Dependent Exp.

Temperature dependent term in the creep rate expression,

e

( – ΔH ) ⁄ ( R ⋅ T0 )

Creep Threshold Stress Limit

Threshold limit for creep process. Threshold stress under which creep does not occur is computed as Creep Threshold Stress Limit times Young’s modulus.

Primary Creep Stiffness

ID number of a TABLES1 entry, which defines the creep model parameter Kp(σ). Creep model parameter Kp(σ) represents a parameter of the uniaxial rheological model shown below.

Primary Creep Damping

ID number of a TABLES1 entry, which defines the creep model parameter Cp(σ). Creep model parameter Cp(σ) represents a parameter of the uniaxial rheological model shown below.

Secondary Creep Damping

ID number of a TABLES1 entry, which defines the creep model parameter Cs(σ). Creep model parameter Cs(σ) represents a parameter of the uniaxial rheological model shown below.

Elastic

Primary Creep

Secondary Creep

Kp ( σ )

σ(t)

Cp ( σ ) Ke

Cs ( σ )

140 Modeling Guide

Composite Composite materials are composed of a mixture of two or more constituents, giving them mechanical and thermal properties which can be significantly better than those of homogeneous metals, polymers and ceramics. Laminate composite materials are based on layering homogeneous materials using one of several methods. In order to define a laminate composite material, you must define the homogeneous materials that form the layers, the thickness of each layer, and the orientation angle of the layers relative to the standard coordinate axis being used for the model. The orientation is particularly important for orthotropic and anisotropic materials, whose properties vary in different directions. The material in each layer may be either linear or nonlinear. Tightly bonded layers (layered materials) are often stacked in the thickness direction of beam, plate, shell structures, or solids.

Each layer is a “ply”, and each ply can have a different material, thickness, or material orientation (angle). Figure 5-42 identifies the locations of integration points through the thickness of beam and shell elements with and without a composite formulation.

Note that when the COMPOSITE option is used, as shown in Figure 5-42, the layer points are positioned midway through each layer. When the COMPOSITE option is not used, the layer points are equidistantly spaced between the top and bottom surfaces. MD Nastran Implicit Nonlinear performs a numerical integration through the thickness. If the COMPOSITE option is used, the trapezoidal method is employed; otherwise, Simpson’s rule is used.

CHAPTER 141 Model Generation

* * * * *

* * * * Beams or Shells with Composite Option

Figure 5-42

Beams or Shells without Composite Option

Integration Points through the Thickness of Beam and Shell Elements

Figure 5-43 shows the location of integration points through the thickness of continuum elements. MD Nastran Implicit Nonlinear forms the element stiffness matrix by performing numerical integration based on the standard isoparametric concept.

* * * * Figure 5-43

* * * * Integration Points through the Thickness of Continuum Elements

Specifying Composite Material Entries MD Nastran provides a property definition specifically for performing composite analysis. You specify the material properties and orientation for each of the layers and MD Nastran produces the equivalent PSHELL and MAT2 entries for shells. This is extended to PSOLID and MATORTH for SOL 600 only. Entry

Description

PCOMP

Defines the properties of an n-ply composite material laminate.

The stacking direction for 3-D composite solids was added with a new entry, MSTACK.

Gasket Engine gaskets are used to seal the metal parts of the engine to prevent steam or gas from escaping. They are complex (often multi-layer) components, usually rather thin and typically made of several different

142 Modeling Guide

materials of varying thickness. The gaskets are carefully designed to have a specific behavior in the thickness direction. This is to ensure that the joints remain sealed when the metal parts are loaded by thermal or mechanical loads. The through-thickness behavior, usually expressed as a relation between the pressure on the gasket and the closure distance of the gasket, is highly nonlinear, often involves large plastic deformations, and is difficult to capture with a standard material model. The alternative of modeling the gasket in detail by taking every individual material into account in the finite element model of the engine is not feasible. It requires a lot of elements which makes the model unacceptably large. Also, determining the material properties of the individual materials might be cumbersome. The gasket material model addresses these problems by allowing gaskets to be modeled with only one element through the thickness, while the experimentally or analytically determined complex pressure-closure relationship in that direction can be used directly as input for the material model. The material must be used together with 2-D or 3-D first-order solid composite element types or 2-D axi-symmetric elements. In that case, these elements consists of one layer and have only one integration point in the thickness direction of the element. Constitutive Model

The behavior in the thickness direction, the transverse shear behavior, and the membrane behavior are fully uncoupled in the gasket material model. In subsequent sections, these three deformation modes are discussed. Local Coordinate System

The material model is most conveniently described in terms of a local coordinate system for the integration points of the element (see Figure 5-44). For three-dimensional elements, the first and second directions of the coordinate system are tangential to the midsurface of the element at the integration point. The third direction is the thickness direction of the gasket and is perpendicular to the midsurface. For two-dimensional elements, the first direction of the coordinate system is the direction of the midsurface at the integration point, the second direction is the thickness direction of the gasket and is perpendicular to the midsurface, and the third direction coincides with the global 3-direction. In a total Lagrange formulation, the orientation of the local coordinate system is determined in the undeformed configuration and is fixed. In an updated Lagrange formulation, the orientation is determined in the current configuration and is updated during the analysis. 2

3 2

1 1

Midsurface Integration Point

Figure 5-44

Integration Point

Midsurface

The Location of the Integration Points and the Local Coordinate Systems in Two- and Three-dimensional Gasket Elements

CHAPTER 143 Model Generation

Thickness Direction - Compression

In the thickness direction, the material exhibits the typical gasket behavior in compression, as depicted in Figure 5-45. After an initial nonlinear elastic response (section AB), the gasket starts to yield if the pressure p on the gasket exceeds the initial yield pressure py0. Upon further loading, plastic deformation increases, accompanied by (possibly nonlinear) hardening, until the gasket is fully compressed (section BD). Unloading occurs in this stage along nonlinear elastic paths (section FG, for example). When the gasket is fully compressed, loading and unloading occurs along a new nonlinear elastic path (section CDE), while retaining the permanent deformation built up during compression. No additional plastic deformation is developed once the gasket is fully compressed. The loading and unloading paths of the gasket are usually established experimentally by compressing the gasket, unloading it again, and repeating this cycle a number of times for increasing pressures. The resulting pressure-closure data can be used as input for the material model. The user must supply the loading path and may specify up to ten unloading paths. In addition, the initial yield pressure py0 must be given. The loading path should consist of both the elastic part of the loading path and the hardening part, if present. If no unloading paths are supplied or if the yield pressure is not reached by the loading path, the gasket is assumed to be elastic. In that case, loading and unloading occurs along the loading path. The loading and unloading paths must be defined using the TABLES1 bulk data entries and must relate the pressure on the gasket to the gasket closure. The unloading paths specify the elastic unloading of the gasket at different amounts of plastic deformation; the closure at zero pressure is taken as the plastic closure on the unloading path. If unloading occurs at an amount of plastic deformation for which no path has been specified, the unloading path is constructed automatically by linear interpolation between the two nearest user supplied paths. The unloading path, supplied by the user, with the largest amount of plastic deformation is taken as the elastic path at full compression of the gasket. For example, in Figure 5-45, the loading path is given by the sections AB (elastic part) and BD (hardening part) and the initial yield pressure is the pressure at point B. The (single) unloading path is curve CDE. The latter is also the elastic path at full compression of the gasket. The amount of plastic closure on the unloading path is cp1. The dashed curve FG is the unloading path at a certain plastic closure cp that is constructed by interpolation from the elastic part of the loading path (section AB) and the unloading path CD.

144 Modeling Guide

E loading path py1

D G

py B

py0 Gasket Pressure p

unloading path

A cp0

F cp

cy0

C cp1

cy

cy1

Gasket Closure Distance c

Figure 5-45

Pressure-closure Relation of a Gasket

The compressive behavior in the thickness direction is implemented by decomposing the gasket closure rate into an elastic and a plastic part:

· ·e ·p c = c +c

(5-216)

Of these two parts, only the elastic part contributes to the pressure. The constitutive equation is given by the following rate equation:

· ·e · ·p p = Dc c = Dc ( c – c )

(5-217)

Here, Dc is the consistent tangent to the pressure-closure curve. Plastic deformation develops when the pressure p equals the current yield pressure py. The latter is a function of the amount of plastic deformation developed so far and is given by the hardening part of the loading path (section BD in Figure 5-45). Initial Gap

The thickness of a gasket can vary considerably throughout the sealing region. Since the gasket is modeled with only one element through the thickness, this can lead to meshing difficulties at the boundaries between thick regions and thin regions. The initial gap parameter can be used to solve this. The parameter basically shifts the loading and unloading curves in the positive closure direction. As long

CHAPTER 145 Model Generation

as the closure distance of the gasket elements is smaller than the initial gap, no pressure is built up in the gasket. The sealing region can thus be modeled as a flat sheet of uniform thickness and the initial gap parameter can be set for those regions where the gasket is actually thinner than the elements of the finite element mesh used to model it. Thickness Direction - Tension

The tensile behavior of the gasket in the thickness direction is linear elastic and is governed by a tensile modulus Dt. The latter is defined as a pressure per unit closure distance (that is, length). Transverse Shear and Membrane Behavior

The transverse shear is defined in the 2-3 and 3-1 planes of the local coordinate system (for threedimensional elements) or the 1-2 plane (for two-dimensional elements). It is linear elastic and characterized by a transverse shear modulus Gt. The membrane behavior is defined in the local 1-2 plane (for three-dimensional elements) or the local 3-1 plane (for two-dimensional elements) and is linear elastic and isotropic. Young’s modulus Em and Poisson’s ratio νm that govern the membrane behavior are taken from an existing material that must be defined using the MAT1 bulk data entry. Multiple gasket material can refer to the same isotropic material for their membrane properties (see also the GASKET model definition option in MSC.Marc Volume C: Program Input). Thermal Expansion

The thermal expansion of the gasket material is isotropic and the thermal expansion coefficient are taken from the isotropic material that also describes the membrane behavior. Constitutive Equations

As mentioned above, the behavior in the thickness direction of the gasket is formulated as a relation between the pressure p on the gasket and the gasket closure distance c. In order to formulate the constitutive equations of the gasket material, this relation must first be written in terms of stresses and strains. This depends heavily on the stress and strain tensor employed in the analysis. For small strain analyses, for example, the engineering stress and strain are used. In that case, the gasket closure rate and the pressure rate are related to the strain rate and the stress rate by

c = – hε and Δp = – Δσ

(5-218)

in which h is the thickness of the gasket. The resulting constitutive equation for three-dimensional elements, expressed in the local coordinate system of the integration, now reads

146 Modeling Guide

σ 11 σ 22 σ 33 σ 12

=

σ 23 σ 31

Em νm Em -------------- --------------- 0 2 2 1 – ν m 1 – νm

0

νm Em Em -------------- --------------- 0 2 2 1 – ν m 1 – νm

0

0 0 ε 11 0 0

ε 22 p

ε 33 – Δε 33

0

0

C

0 0 0 Em - 0 0 0 ----------------------2 ( 1 + νm )

0

0

0

0

0

0

Gt 0

0

0

0

0

0 Gt

γ12

(5-219)

γ23 γ31

in which C = hDc. For two-dimensional elements, the equation is given by

ν m Em Em -------------- 0 -------------- 0 2 2 1 – νm 1 – νm

σ 11 σ 22 σ 33 σ 12

=

0 C 0 0 νm Em Em -------------- 0 -------------- 0 2 2 1 – νm 1 – νm 0

0

0

ε 11 p

ε 22 – Δε 22 ε 33

(5-220)

γ 12

Gt

For large deformations in a total Lagrange formulation, in which the Green-Lagrange strains and the second Piola-Kirchhoff stresses are employed (as well as in an updated Lagrange environment) in which the logarithmic strains and Cauchy stresses are being used, similar but more complex relations can be derived. Specifying Gasket Material Entries The MATG provides specifically for modeling gasket materials. Entry

Description

MATG

Specifies gasket material properties to be used in MD Nastran Implicit Nonlinear (SOL 600) only.

MATTG

Specifies gasket material property temperature variation to be used in MD Nastran Implicit Nonlinear (SOL 600) only.

CHAPTER 147 Model Generation

References • MATG in the MD NASTRAN QRG. • MATTG in the MD NASTRAN QRG.

Material Damping In direct integration analysis, the user very often defines energy dissipation mechanisms as part of the basic model - dashpots, inelastic material behavior, etc. In such cases, there is usually no need to introduce additional “structural” or general damping: it is unimportant compared to these other dissipative effects. However, some models do not have such dissipation sources (an example is a linear system with chattering contact, such as a pipeline in a seismic event). In such cases, it is usually desirable to introduce some general low level of damping. MD Nastran Implicit Nonlinear provides “Rayleigh” damping for this purpose. The user includes the two Rayleigh damping factors, αR for mass proportional damping and βR for stiffness proportional damping on the NLSTRAT Bulk Data entry. In the case of elements the damping values must be used in conjunction with these property references. For a linear problem, these provide a damping matrix [C] as described above: [C]=αR[M]+βR[K]. Since the model may have quite general nonlinear response, the concept of “stiffness proportional damping” must be generalized, since it is possible for the tangent stiffness matrix to have negative eigenvalues (which would imply negative damping). To overcome this problem, βR is interpreted as defining viscous material damping which creates an additional “damping stress,” σd, proportional to the total strain rate: el · σ d = βD 0 ε

(5-221)

Here D0el is the material’s initial (virgin) elastic stiffness. This damping stress is added to the stress caused by the constitutive response at the integration point when the dynamic equilibrium equations are formed, but it is not included in the stress output. This allows damping to be introduced for any nonlinear case, and provides standard Rayleigh damping for linear cases. Since the βR factor introduces damping proportional to the strain rate, this may be thought of as damping associated with the material itself, while the αR factor introduces damping forces caused by the absolute velocities of the model, and so simulates the idea of the model moving through a viscous “ether” (a permeating, still fluid, so that any motion of any point in the model causes damping). The αR factor is applied to all elements that have mass. The βR factor applies to all elastic elements and to beam and shell elements. The βR factor is not applied to spring elements. Discrete dashpot elements should be used as needed for springs.

148 Modeling Guide

Specifying Material Damping Entries Parameters for material damping are input through the NLSTRAT entry. Entry NLSTRAT NLDAMP

Description Defines transient analysis damping parameters BETA, GAMMA, GAMMA1, GAMMA2. Defines damping constants for nonlinear analysis when MSC.Marc is executed from MD Nastran used in SOL 600 only (Not supported in MSC SimXpert 2004).

References • NLSTRAT in the MD NASTRAN QRG. • NLDAMP in the MD NASTRAN QRG. SimXpert Materials Application Input Data

Isotropic

Description

Gamma (Newmark)

Mass proportional damping coefficient.

Beta (Newmark)

Stiffness proportional damping coefficient.

CHAPTER 149 Model Generation

Properties Typical properties include cross-sectional properties of beam elements, thicknesses of plate and shell elements, material IDs, etc. Properties are assigned to the elements of a specified part or element type, either directly to the elements, or indirectly through the part to which the elements belong or the geometry with which the elements are associated. Properties associate materials with elements.

150 Modeling Guide

Tables, Variable LBCs and Properties In some problems, you may need to enter variable data. For example, the plate thickness may vary across a part, or even within an element. Variable loads, boundary conditions, and material and element properties can be generated by creating a Table of XY pairs that describes the variation, by typing in an equation, by creating or importing spreadsheet data, or by extrapolating from results values. A table is a set of XY pairs that can define a function to use in generating variable properties for independent data. For example, tables can be used in generating temperature-dependent material properties, stress-dependent materials, creep parameters, general Hyperelastic material parameters, and variable heat transfer coefficients. Tables can used in defining material properties. They can be created directly from the material form or under the Tables tab in the Tool Ribbon. By using a table, you can enter values for the property behavior with respect to an independent variable.

Variable LBCs and Properties Variable LBCs and properties can define loads, attributes, or coefficients to vary as a function of coordinate components or independent variables. For example, they can be used to define a variable thickness, nonlinear properties, or variable force. Function expressions and tablular inputs are used to generate the data for the variable load, attribute, or coefficient. Variable LBCs and properties can be created directly from the LBC or Material forms by clicking on the drop-down arrow to the right of the desired textbox and selecting New. There are four ways to define Variable LBCs and Properties: Function, Tabular, Discrete FEM, and Continuous FEM. Function Function defines an expression for a scalar, or up to three expressions for vector components. To enter a function , clicking on the drop-down arrow to the right of the desired textbox and select New > Function. You may either type an expression directly on the Create Function form or click on the ellipsis to use the function input form. You may use the following functions in an equation: acos

fmod

asin

log

atan

log10

atan2

sin

cos

sinh

cosh

sqrt

exp

tan

fabs

tanh

CHAPTER 151 Model Generation

Tabular Tabular allows you to manually input or import spreadsheet style data of one or more independent variables vs. a value. To enter tabular data, click on the drop-down arrow to the right of the desired textbox and select New > Tabular. Discrete FEM Discrete FEM defines the variation in a property or load /boundary condition by entering values to be associated with specific nodes or elements. To enter Discrete FEM data, click on the drop-down arrow to the right of the desired textbox and select New > Discrete FEM. Continuous FEM Continuous FEM defines the variation in a property or load /boundary condition by entering data either manually in a spreadsheet, importing data from a file, or by selecting a current Results Plot created using Post Processing tools (Results from one analysis can be used to generate loads for another). To enter Continuous FEM data, click on the drop-down arrow to the right of the desired textbox and select New > Continuous FEM.

152 Modeling Guide

CHAPTER 1 Combining Models

Combining Models

2 Modeling Guide

Replacing Parts SimXpert has part replacement tools which allow you to substitute a new part for an existing part in the database. The part replacement procedure can be performed manually or using a wizard.

Replace Part Wizard The wizard expects incoming parts to have the same Part ID as the part being replaced so you need to prevent SimXpert from offsetting input part Ids. This is accomplished using the Options Editor as follows: Tools > Options. Expand General and Input/Output branches. Highlight Nastran Structures. Uncheck Offset Part IDs in the Input group. Click OK. Part IDs can be identified in the Nastran input file by locating the keyword SXNAME. The following example shows the entry for a part named Ring Inner with ID 28. $23456781234567812345678123456781234567812345678 $SXNAME COMP 28 "Ring Inner" To see Part IDs in SimXpert, click the List tab in the Model Browser. The default listing will be Parts and their corresponding ID numbers. The Replace Part Wizard is accessed through Tools > CAE Wizard > Replace Parts. This script asks for a Nastran file which contains the modified part designs. The procedure operates on the assumption that if two part IDs are the same they are considered to be duplicate. Once duplicate parts are found, you are prompted to be sure you wish to delete the existing part and replace it with the new one. If connections exist in the database SimXpert will go through the process of reconnecting the parts.

Manually Replace Parts You can also manually replace parts in a database. To do so, select Tools > Part > Replace Parts.You will be prompted for name of the part to be replaced and the part with which to replace it. The contents of the two parts will be swapped. The message area reflects the change Unlike the Replace Part Wizard, the Replace Part command does not automatically delete the original part or reconnect the parts if connections exist in the database.

CHAPTER 3 Combining Models

Exporting Combined Input Files After importing multiple MD Nastran files into SimXpert and modifying the models you may want to export the updated model files. This is accomplished using File > Export. The file(s) to be exported may contain only solver entries or they may have either INCLUDE statements or solver entries. To export files after the corresponding models have been modified in SimXpert, use File > Export with any of the following choices: • Nastran Model -- export all the model data under the Model tab to a single file. • Nastran Scene -- export all entities displayed in the graphics window to a single file. • Nastran Multiple -- export files based on SimXpert File Sets. The file names and destination

directories can be changed. Following is an example of the Nastran Multiple method. Shown is an image of the Model tab for two MD Nastran models.

After the two models have been modified, export them to two MD Nastran files using File > Export > Nastran Multiple.

4 Modeling Guide

The Export Multiple form has several parameters that can be specified. • Export -- true: export the corresponding file. • Set Name -- SimXpert file set name. • Job -- select whether to output Nastran analysis job entries. • File -- MD Nastran input file that will be created. • Choose Folder -- Specify a single folder to which all files will be exported.

The two files that were imported were not referenced by a ‘parent’ file with just INCLUDE statements, so when the two files are exported they are not referenced by a parent file. Following is an example of the Nastran Multiple method for models that are referenced by a parent file. Shown is an image of the Model tab for the MD Nastran models. The parent file is named main.dat.

CHAPTER 5 Combining Models

After the models have been modified, export them to MD Nastran files using File > Export > Nastran Multiple. One of the files that will be exported is named main.dat. It will contain only INCLUDE statements. The other files will contain MD Nastran entries.

6 Modeling Guide

CHAPTER 3 Model Display

Model Display For display purposes, SimXpert entities are organized into three major collection types: 1. Parts Parts consist of: • Geometric Entities • Finite Element Entities (not including nodes)

Each part can have its own graphics attributes. 2. LBC Sets LBC Sets consist of: • Loads • Boundary Conditions

3. Connection Groups Connection Groups consist of: • List of Connected Parts • Connection Locations

In this document we will discuss controlling the display of entire collections and also the entities contained therein.

4 SimOffice Workspace 2006

Viewing The View menu and toolbars provide access to the tools for controlling the display of the model graphics window (model orientation, rendering, scenes) as well as the appearance of the SimXpert GUI (toolbars, regions). Also found here are ways to control which entities are displayed. Shown below are the entity display menu and the corresponding Entity Display toolbar. Using these, all entities of a specific type may be displayed or hidden.

Entity Display toolbar

Note:

• Entities turned off using Entity Display can only be turned back on from this

menu. Other display commands described in this document will not redisplay entities turned off using this command. If you would like to fine tune which specific entities, rather than entity types, to display or hide, you can use the Organize command from the Element Render toolbar or the View menu. When the Action is set

CHAPTER 5 Model Display

to Activation, you can Activate or Deactivate (turn on or off) the three major collection types: Parts, LBC Sets, or Connection Groups. They can be selected from the screen or the Model Browser.

When the Action is set to Visibilty you can selectively Hide or Show individual collection members: finite elements, boundary conditions, connections, or geometric entities. If you select to Hide or Show a collection the action is applied to all entities in that collection.

6 SimOffice Workspace 2006

Display Control Using the Model Browser Entity display can be controlled using the context menu. Right click on an item in the Model Browser to display the context menu. You can also right click on parts in the graphics window to display a context menu.

Figure 1

Context Menu from Model Browser

CHAPTER 7 Model Display

Visibility

Visibility controls whether selected entities are displayed in the graphics window. Show Only

Turns off the graphics display of all unselected entities

Show

Turns on graphics display of entities

Hide

Turns off the graphics display of entities

Show All

Turns on the graphics display of any hidden entities

Hide All

Turns off the graphics display of all entities

Reverse All

Shows entities that are currently hidden, and hides those that are currently shown

Entities can not be selected from the graphics area or the Model Browser after they are hidden. Note:

To return all items in your model to the graphics display, • Select the Scenes tab in the Model Browser • Select the Action Show Scene • Click on scene All

8 SimOffice Workspace 2006

Activation

Activation controls whether collections are turned on or off . Activated parts are turned on. Deactivated parts are turned off. Parts can be selected from the graphics area or the Model Browser after they are Deactivated (turned off). The appearance of the part icon in the Model Browser changes to show which parts are displayed.

Displayed Parts

Deactivated Parts

Hidden Parts

CHAPTER 9 Model Display

Parts Part display can be controlled from the context menu. Each part can have its own graphics attributes by selecting Change Graphics.

10 SimOffice Workspace 2006

Scenes

A scene consists of the current contents of the window including parts, connections, and boundary conditions. Current view, graphics, and visibility are also saved with the scene by default. Notice that you can select checkboxes to ignore render style and view angle if you wish to keep your current settings when you display a different scene. If you isolate parts and/or elements that you would like to recall as a group at a future time, you can save them as a scene using View > Scenes > Create Scene or Create Scene from the Scenes tab in the Model Browser and supplying a name. The scene can be recalled at any time by selecting it from the Scenes option of the View menu or the Scenes tab of the Model Browser. Note:

To return all items in your model to the graphics display, • Select the Scenes tab in the Model Browser • Select the Action Show Scene • Click on scene All

CHAPTER 11 Model Display

Viewing Enhancement There are several things that can be done to improve the quality of the display of geometry. There are different tolerances that affect the display of curves and surfaces, and parameters that can be used to control the display of hatch lines for surfaces.

Tolerances The three available tolerances for modifing the quality of the display of geometry are • Surface Planar Tolerance: used to make planar surfaces display more smoothly. Reduce the

tolerance to increase the smoothness. • Curve Chordal Tolerance: used to make curves with curvature display more smoothly. Reduce

the tolerance to increase the smoothness. • Surface Edge Chordal Tolerance: used to make surface edges and faces display more smoothly.

Reduce the tolerance to increase the smoothness. These parameters are accessed using Tools > Options and highlighting Geometry in the tree.

Hatch Lines Hatch lines can be displayed on surfaces to assist visualizing the surface curvature. The three available parameters for modifing hatch line display on surfaces are • Surface Hatch Spacing: used to display hatch lines on surfaces or faces of solids. It has units that

are the model units of length. • Surface Hatch Line Style: used to change the style for displayed hatch lines. • Surface Hatch Line Width: used to specify the line width. The units are pixels.

These parameters are also accessed using Tools > Options and highlighting Geometry in the tree.

12 SimOffice Workspace 2006

CHAPTER 1 Keyboard Shortcuts

Keyboard Shortcuts You can create your own keyboard shortcuts to execute commands from the GUI. You can access the form to modify or create keyboard shortcuts using Tools >Customize > Hot Keys.

To assign a command to a key combination, simply click in the appropriate cell on the form, then select the desired command from a menu or toolbar. Click Save if you would like to use your key assignments in all SimXpert databases.

2 Modeling Guide

CHAPTER 1 Geometry Interfaces

Geometry Interfaces

2 New Template 2005

Parasolid You can directly import a parasolid file generated from your CAD code using File / Import / Parasolid. For the supported formats listed, SimXpert can convert the geometry to parasolid format and open it as such. This is accomplished under File/ Import / Geometry as Parasolid. No CAD license is required when geometry is imported as a parasolid. File Format

Supported Types and Versions

CATIA V5

V5R2 - R18

CATIA V4

.model, .exp, V4.1.9 – 4.2.4

Pro/Engineer

.prt, .asm, Pro/E 16 – Wildfire 2.0 (M250) and Wildfire 3.0 (F000))

ACIS

.sat, to ACIS R16

STEP

.ste, .step, AP203, AP214

IGES

.igs, .iges, to 5.3

CHAPTER 3 Geometry Interfaces

CATIA SimXpert can directly access Native CATIA geometry using File / Import / CATIA. The following file types are supported: CATProduct, CATPart and CATAnalysis. Supported versions of CATIA for direct access are V5R16 through R18. When direct access is used, no geometry translation is involved. The CATIA model itself is opened. You can directly edit CATIA features and parameters in SimXpert and choose to save them back to the original CATIA file. This command uses the local CATIA installation directly and therefore a CATIA license is required. There are several parameters that affect importing CATIA geometry into SimXpert. They are available under Tools: Options, Geometry / CAD Import. The parameters are • Sew Surface: if this is enabled at the time of import, adjacent surfaces whose edges are within

the Sewing Tolerance are stitched (connected topologically). • Generate Mapping File: use this to create a file that identifies the topological relationship

between geometry. • Update Model: use this to update a CATIA model during import into SimXpert. The “Ask user”

option is used to be able to specify if it is desired to update the geometry; if this is not used the model will be updated automatically. The Update Model option was implemented to deal with the case of parametric changes made to the model in CATIA, then without updating, saving the model in CATIA. • Use DGM: If checked, the DGM (Derived Geometry Modeler) represents CAE geometry by

modifying CAD to a form that is suitable for meshing purposes. If unchecked, the SGM (SimXpert Geometry Modeler) algorithms perform suppression and meshing operations.

4 New Template 2005

IGES The IGES (Initial Graphics Exchange Specification) defines a neutral data format that makes possible the digital exchange of information among computer-aided design (CAD) systems. Using IGES, a CAD user can exchange product data models in the form of circuit diagrams, wireframe, freeform surface, or solid modeling representations. Applications supported by IGES include traditional engineering drawings, models for analysis, and other manufacturing functions. For this application the IGES file is used to transmit geometric curves, surfaces, and solids data. Once imported into SimXpert they can be used to create other geometry if needed. Then, they will be meshed, creating 1D, 2D, or 3D elements. There are several parameters that affect importing IGES geometry into SimXpert. They are available under Tools: Options, Geometry / CAD Import. The parameters are • Detect System: used to specify the source of the IGES file, e.g. CATIA. The default is “Auto

Detect”. This option is very useful because there can be subtle differences between IGES files from different sources. • Surface Trimmimg: causes surfaces to be split at intersections during import. • Force Global Precision: tolerance to be used for the entire model, e.g. global model tolerance. • Free Curves: If checked, unconnected curves will be imported. • Free Surfaces: If checked, unconnected surfaces will be imported. • Check Geometry: If checked, the geometry topology will be checked on import.

CHAPTER 5 Geometry Interfaces

FE data import from CATIA V5 and SimDesigner: Unit System and Coordinate Systems are fully supported. Connections are supported with the exception of those between higher order elements. The following tables list specific entity types: Element Type Solid

Shell

1D

SimXpert

Hexa 8

Supported

Hexa 20

Supported

Penta 15

Supported

Pents 6

Supported

Tetra 4

Supported

Tetra 10

Supported

Pyramid

Not Supported

Quad 4

Supported

Quad 8

Supported

Tria 3

Supported

Tria 6

Supported

Bar2 (CBar, CBeam, CBush, CELAS, CGAP, CRod ) Supported Bar3 (CBar, CBeam, CBush, CELAS, CGAP, CRod ) Not Supported

Rigid

RBE 2

Supported

RBE 3

Supported

Property Type

MD Nastran entry

SimXpert

Solid

PSOLID

Supported

Shell

PSHELL

Supported

Bar / Beam

PBAR / PBARL / PBEAM / PBEAML Supported

GAP

PGAP

Supported

Rod

PROD

Supported

Bush

PBUSH

Supported

SPRING

PELAS

Supported

Composite

PCOMP

Supported

WELD

PWELD

Supported

6 New Template 2005

SimDesigner Material

Nastran Entry

Crash Workspace

Structures Workspace

Type

Model

Isotropic Linear

NA

MAT1

NA

Supported

Isotropic Thermal

NA

MAT4

NA

Supported (This material is also supported for the Thermal Workspace as MatIsotropic

Isotropic

Elastic

MAT1+MATEP

NA

Supported

Linear Plastic

MAT1+MATEP

NA

Supported

Plastic-Kinematic MAT1+MATEP

NA

Supported

Power LawPlastic

MAT1+MATVP_POWER

NA

Supported

Elastic-Plastic

MAT1+MATEP / MAT1+MATS1 / MAT1+MATVP_POWER

NA

Supported

Rigid

NA

MAT 20

Supported

Neo-Hookean / Mooney-Rivlin / 3D-OrderInvarient

MATHE_MOONEY

NA

Supported

Gent

MATHE_ABOYCE_GENT NA

Supported

Arruda-Boyce

MATHE_ABOYCE_GENT NA

Supported

Ogden / Foam

MATHE_OGDEN_FOAM

NA

Supported

MAT8

NA

Supported

Isotropic Hyper Elastic

Orthotropic Composites NA

FE Entity

Nastra SimXper n Entry t

Distributed Mass CONM2 Supported Line Mass Densities

CONM2 Supported

Surface Mass Densities

CONM2 Supported

Inertia on Virtual Parts

CONM2 Supported

CHAPTER 7 Geometry Interfaces

STL STL (Stereo Lithography) file can be imported directly in SimXpert.

8 New Template 2005

Geometry Simplification Tools Feature Suppression Suppression is performed to eliminate fine (very small) CAD features. This will give you a better quality mesh as you can eliminate sliver surfaces. You can suppress curves that are not required to define a boundary when meshing. If a manifold curve is suppressed, the two surfaces it connects become one. Similarly suppressing a vertex reduces the number of curves to be dealt with. Curves which are not feature curves (no significant difference in the surface normals on either side of the curve) should be suppressed. Select Suppress/Unsuppress vertex or edges from the Cleanup group under the Geometry tab. You can then select vertices or curves respectively to be ignored when meshing. The Break Angle specified on the (Un)Suppress form will be used to suppress curves at the interface of surfaces whose normals intersect at an angle less than or equal to the break angle. A mesh will not break at that interface -- mesh nodes will not be constrained to be along the entire interface. Force Suppression allows (un)suppression of all selected entities regardless of Break Angle. Suppressed entities are diplayed in blue.

No entities suppressed:

After suppression: Suppressed edges and vertices shown in blue.

Turning on and off the display of suppressed entities is controlled by the Geometry Graphics toolbar.

Turn on/off the display of suppressed edges.

Turn on/off the display of suppressed vertices.

CHAPTER 9 Geometry Interfaces

Stitching This command will take sheet bodies whose boundaries lie within a specified tolerance and create congruent surfaces with aligned normals. Select Stitch Surfaces from the Surface group under the Geometry tab. Select the Sheet Bodies you would like to make continuous. You can modify the stitch tolerance, if desired. Unconnected or free edges are displayed in red. Shared edges are displayed in green. Model before stitching: Unshared edges shown in red.

Model after stitching: No remaining interior free edges.

10 New Template 2005

CHAPTER 1 Mouse Functionality

Mouse Functionality You can customize the functions of each mouse button as it is used in the graphics window using Tools/ Options / Mouse Options.

2 Modeling Guide

Mouse Settings There are four pre-configured mouse settings. They are based on default mouse settings for the codes indicated and cannot be modified. There is a Custom choice that allows you to select your own mouse functionality preferences. The following table shows the Default settings for the mouse buttons

None

Pick

Done

Context Menu

Shift

Polygon Pick Mode

None

Drag Dynamic Rot

Control Pick

Toggle Pick Mode

Drag Zoom

Control View Manip Menu +Shift

Toggle Pick Mode

Drag Pan

The following table shows the Catia setting for the mouse buttons:

None

Pick

Click Pan

Context Menu

Shift

Pick

Drag Dynamic Rot

None

Control Polygon Pick Mode

Drag Zoom

Done

Control View Manip Menu +Shift

Drag Dynamic Rot

Reject Last

Catia settings also support the following mouse button combinations: Left Drag

Rectangular Pick

Middle Drag

Pan

Middle Left Release Drag

Zoom

Middle Right Release Drag

Zoom

Middle Left Drag

Rotate

Middle Right Drag

Rotate

CHAPTER 3 Mouse Functionality

The following table shows the Patran setting for the mouse buttons:

None

Pick

Drag Dynamic Ro

Context Menu

Shift

Pick

Drag Pan

Pick

Control Polygon Pick Mode

Drag Zoom

None

Control None +Shift

Drag Dynamic Rot

Reject Last

The following table shows the Sofy setting for the mouse buttons:

None

Pick

Done

Toggle View Manip.

Shift

Reject Last

None

None

Control Pick Menu

Toggle Pick Mode

View Manip. Menu

Control None +Shift

Toggle Pick Mode

None

Drop-down menu choices If Custom View Manipulation is selected the following actions can be assigned to to mouse buttons + key combinations. These actions are selected from the drop down menus. Fields

Descriptions

None

No action assigned.

Drag Pan

Dragging in the graphics area with the selected key/mouse button combination will translate the image.

Toggle Pan

Turns on pan mode. Image will move as you move the mouse. Click mouse button assigned to Done to finish (default is middle mouse button).

Drag Zoom

Dragging in the graphics area with the selected key/mouse button combination will magnify/shrink the image.

Toggle Zoom

Turns on zoom mode. Image will magnify/shrink as you move the mouse. Click mouse button assigned to Done to finish (default is middle mouse button).

4 Modeling Guide

Fields

Descriptions

Drag Dynamic Rot.

Dragging in the graphics area with the selected key/mouse button combination will rotate the image.

Toggle Dynamic Rot Turns on dynamic rotation mode. Image will rotate as you move the mouse. Click mouse button assigned to Done to finish (default is middle mouse button). Drop

Deselects entities that are clicked on with this key/mouse button combination.

Done

Finalizes the action or selection.

Reject Last

Discards your most recent selection

Toggle Pick Mode

Changes picking action between Select and Deselect.

Pick Menu

Displays the menu that lets you select Single, Polygon, Rectangular Window, or Sketch picking.

View Manip. Menu

Displays the View / Display menu.

Drag View Manip.

Dragging in the graphics area with the selected key/mouse button combination will manipulate the image based on whichever method is currently selected from the View Manipulation toolbar or menu.

Toggle View Manip. Turns on whichever method is currently selected from the View Manipulation toolbar or menu. Image will move as you move the mouse. Click mouse button assigned to Done to finish (default is middle mouse button). Context Menu

Displays a menu related to the currently selected command.

CHAPTER 1 Post Processing

Post Processing

2 Modeling Guide

Freebody plots The function of freebody plots is to display a freebody diagram on a selected portion of the model. The freebody plots are in the form of vector plots, showing either the individual components or resultant values. Individual components that make up the total freebody diagram, such as reaction forces, nodal equivalenced applied forces, internal element forces and other forces from MPCs, rigid bars, or other external influences, can also be plotted separately. To enable the plotting of Freebody diagrams, right click on Output Request in the Model Browser and select Create Grid Point Force Balance Output Request. Freebody results provide an intuitive interface to Nastran’s Grid Point Force Balance data. The data table shows the forces and moments acting on the grid point from each source (element, applied load, etc.) in the Nastran global coordinate system. Grid Point Force and Moment data are stored as nodal and element vector quantities. The data can also be viewed with other Result Plot Types such as Vector. Result Types Freebody plots can be derived in three different plot types: 1. Loads - Which displays a freebody of the structure based on all internal/external loads, just the applied loads, just the constraint loads, etc. 2. Interface - Plots net loads at structure interfaces. 3. Displacement - Shows displacements at the freebody boundary. At each node, the grid point force balance table includes contributions from elements, applied loads, SPCs, and MPCs or

F Total = Σ ( F elms ) + F Applied + F SPC + F MPC These nodal contributions form the basis for the Result Type selections in the Freebody Plot: • Freebody Loads

– Σ ( Felms ) = – Internal Forces • Applied Loads

F Applied • Constraint Forces

FSPC • Internal Forces

Σ ( F elms )

CHAPTER 3 Post Processing

• MPC Forces

F MPC • Summation of Forces

F Total One or more result cases can be used in freebody plots...(slide 71) Freebody Loads are used to display a true freebody showing loads apploed to the structure from all sources, including the applied loads, constraints (SPCs), MPCs/rigid elements, and other sources (Totals).

FreebodyLoads = – Σ ( F elms ) = F Applied + F SPC + F MPC – F Total Freebody Loads, as shown above, are equal to the negative of the Internal (or element) Forces. The summation point is the point about which moments will be summed. Obviously for equilibrium, the sum of forces and moments about any point should be zero. Applied Loads Applied Loads displays the applied loads acting on the target elements. These loads are not true freebodies since they do not include all loading. The spreadsheet Totals row will sum to the total load applied to the freebody elements. Constraint Forces Constraint Forces displays the constraint forces acting on the target elements. Constraint Forces are not true freebodies since they do not include all loading. Force Summation Force summation typically will be all zeros. Force Summation is not a true freebody since it does not include all loading. Display Method It is possible to toggle the display methods in order to show force, moment, or both together. The options will be displayed as either resultant or component. Freebody Plots Within the Freebody tab is a Vector Attributes tab. The Vector Attributes tab controls vector scaling, color and style. There is also an Annotation tab where the label and title options can be adjusted. The Data Transforms tab controls coordinate transformation and scaling. The filter option can be useful for uncluttering the display. On the Spreadsheet tab, it is possible to examine the forces and moments at each

4 Modeling Guide

node. Contained in the spreadsheet is a Node ID, coordinate references for forces/moments, force/moment resultants, and force/moment components. Freebody Interface Plot The interface method is designed to calculate and display net loads at structure interfaces. A common use is to calculate net forces and moments at various stations along a wing or fuselage. The interface method differs from the Loads method in that both elements and nodes must be selected. Results belonging to nodes not associated to the target elements will be ignored. A single net force/moment is calculated at the summation point in the reference system. The summation point can be any node, point, or location in space. Recall that Freebody Loads =

– Σ ( F elm ) Also recall that _ is stored as vector data for the element at its nodes. Therefore, nodes should be selected along the cut edge. Then, the elements that join the cut edge nodes should also be selected. THe nodelist displayed along the cut boundary means that only elements that connect to these nodes will contribute. In every interface plot it is necessary to specify a Summation Point Location as well as to Show Summation Point. Boundary Displacement Plot The Boundary Displacement Plot displays/rotations instead of forces and/or moments.

CHAPTER 1 Customization

Customization

2 Modeling Guide

Window Options Tools > Options, Interface / Window allows you to specify window parameters such as background color or axis display.

CHAPTER 3 Customization

Custom Menus You can create your own custom menus in SimXpert by using: Tools > Customize > Custom Menus. Click on Create when the Custom Menu Creation form appears. After entering your Custom Menu Name, you can simply click on commands you would like included in your menu. You can select from the main menu, the tool ribbon, or from the toolbars. Once you save your menu, the main menu will now have a Custom menu that contains your customized menu

Notice that your custom menu is a tear away menu and can be made to remain displayed by clicking on the dashed line at the top of the menu.

4 Modeling Guide

Tool Ribbon Customization By creating a custom tool ribbon you can add, remove, and rearrange tools, groups, and tabs on the tool ribbon. Tools that you do not need can be removed. All the tools needed for a specific problem can be placed under one tab and in the order each is used.

Creating a New Custom Tool Ribbon To customize a tool ribbon, right-click in the tool ribbon region and select Configurations > Customize.... The Ribbon Editor form allows you to create an entirely new tool ribbon from scratch (Create...) or modify an existing tool ribbon (Clone...). You can customize the cloned tool ribbon using the Ribbon Layout section of the form to rearrange or delete tools, groups, or tabs.

Using a Custom Tool Ribbon To use a customized tool ribbon, right click in the tool ribbon region and select Configurations > customized_tool_ribbon_name.

CHAPTER 5 Customization

Custom Help Documentation You can add your own documentation to the SimXpert Help menu. This allows your organization to provide help for custom macros, templates, and procedures that have been developed. Using an environment variable, one or more entries can be added to the help menu. If the specified entry is a folder, then a cascading menu will be created with each sub folder being a “node” in the cascading tree and each HTML or PDF file a “leaf” (terminating) entry. This functionality supports HTML and PDF file formats. All other file types are ignored. Selecting a document will launch the document in a separate browser window.

Creating a custom Help menu Create an environment variable In Microsoft Windows, this is done in the Control Panel > System. Select the Advanced tab in the Systems Properties dialog box. Click the Environment Variables button, then New. Create a user variable with Variable name: MSC_SX_CUSTOM_HELP_ROOT_DIRS and set the Variable value to be the path(s) to the custom help documentation. Any number and combination of files and folders can be specified. Network locations can also be specified. Each entry in this list will correspond to a “root” item added to the help menu. The format of the locations should be: no quotes with entries separated by a semi-colon. For example: C:\ABC_Corp_SimX_Templates;C:\ABC_Corp_Std_Work_Instructions

Add a script to the SimXpert startup The script to be executed is located at: <SimXpert installation directory>/RADE/SimXpert/CustomHelpDocumentation.rdl

6 Modeling Guide

Execution of this script needs to be added to the SimXpert startup shortcut. Locate the SimXpert startup shortcut desktop icon (or on Start menu). Right-click and open Properties.

On the Shortcut tab, append “-ridl script path” to the existing Target. For example: C:\MSC.Software\SimXpert\R4\WINNT\bin\simxpert32.bat -ridl C:\MSC.Software\SimXpert\R4\RADE\SimXpert\CustomHelpDocumentation.rdl

Click Ok to save the change to the shortcut.

Using a custom Help menu Once a custom help menu has been created, as shown above, start SimXpert using the shortcut, as usual. The customizing of the Help menu will occur as SimXpert starts. The addition of the custom help documentation will be noted in the Messages window.

Upon selecting the Help menu, you will see the additional menu items. Navigate through the folders to view the html and pdf files inside. The Help menu names are the same as the folder and file names in the specified custom help paths.

CHAPTER 7 Customization

8 Modeling Guide

CHAPTER 1 SimXpert Files

SimXpert Files

2 New Template 2005

Basic SimXpert Files Name

File Type

Comments

Model.SimXpert

Database

One per model

Model.SimXpert.bak

Database

Backup database. Allows you to retrieve data up to the previous state.

Model.SimXpert.autosave

Database

Saves a SimXpert database automatically at a particular time interval. Autosave can be disabled.

Model_SimXpert.proc

Process (Macro)

Contains a record of executed commands. Repetitive tasks can be automated using the .proc file. Data can be regenerated by running the .proc file.

Model_recover.proc

Process (Macro)

To recover a file which terminated abnormally, SimXpert writes a _recover.proc file.

SimX_LocalSettings.xml

Custom Settings

SimXpert’s user interface can be customized by the user. The changes made are saved in the SimX_Local_Settings.xml file

SimX_DefaultSettings.xml

Default Settings

Contains all the factory default settings provide by MSC. Resetting to factory defaults loads the settings from this file.

SimXpert.log

Text

Record of all messages SimXpert reports to the message region. One per session.

SimXpert.err

Text

Status file showing code versions and database entities.

Backup Databases .bak The .bak file is created from an existing .SimXpert database. An existing .SimXpert file is renamed .SimXpert.bak when the save command is executed. It can be opened by removing the .bak extension and opening the renamed file in SimXpert. .autosave The .autosave file is created at regular time intervals. The settings for the .autosave file can be edited by going to Tools > Options > General and scrolling down to Automatic Backup. From the User Options form: • automatic backup can be enabled or disabled

CHAPTER 3 SimXpert Files

• the number of backups to save can be specified • the backup time interval at which an automatic save is taken can be changed • the file extension for the backup file can be changed • the log file that keeps track of SimXpert’s autosave activity can be renamed

Automation Files .proc The .proc process file is created every time SimXpert is executed. It contains a record of executed commands. The process file is an XML file. It can be executed to repeat the actions performed. It can be edited in the SimXpert Template Builder Workspace. When SimXpert is first executed a text file named SimXResLog.txt is created. After a workspace is selected a procedure file named UNTITLED.proc is created. This file is used to record all actions that occur. During the execution of SimXpert a log file, simx_backup.log, and a backup database, UNTITLED.autosave01, are created. When a database is saved using File > Save a name must be specified. SimXpert creates the database with the suffix .SimXpert, e.g. model.SimXpert. The original procedure file’s name is changed from UNTITLED.proc to the user specified name, with the suffix _SimXpert.proc, e.g. model_SimXpert.proc. When an existing SimXpert database is opened all subsequent steps performed are appended to the end of the existing procedure file.

4 New Template 2005

_recover.proc The _recover.proc file is written when a database has exited abnormally. When SimXpert is re-started it will prompt whether to recover the database. By executing the recover process file, SimXpert will rebuild the database.

Custom Settings SimXpert’s user interface can be customized using the User Options form found under to Tools > Options. When the user interface is customized, the changes are written to the SimX_LocalSettings.xml file. If this file exists, it is read whenever SimXpert is started and will determine settings and appearance in the user interface. This file is specific to the user.

Default Settings The default factory settings can be recovered by clicking on the Restore Factory Defaults button on the User Options form. The default file locations can be accessed using Tools > Options / General / Locations. They can be modified.