Finite Element Methods Of Structural Analysis

Finite element methods of structural analysis

1

1.0 Introduction With the development of finite element methods and availability of fast and cheap computers the cycle time and cost of development of a product has comedown substantially. The concept of concurrent and collaborative engineering is widely used now to cut the cycle time for realizing the product from configuration finalization to proto development. The following figures illustrates the traditional and current process that are being followed for the design and development of a product

2

Concept

Detailed design Prototype Verification Optimum/near optimum design within time and resources

Production

Traditional development process 3

Concept

Analysis ‘Software prototyping’

Optimal design Detailed design Prototype Verification Production

Product development using predictive engineering

4

1.1 Finite Element Method Defined • Many problems in engineering and applied science are governed by differential or integral equations. • The solutions to these equations would provide an exact, closedform solution to the particular problem being studied. • However, complexities in the geometry, properties and in the boundary conditions that are seen in most real-world problems usually means that an exact solution cannot be obtained or obtained in a reasonable amount of time.

5

Finite Element Method Defined (cont.) • Current product design cycle times imply that engineers must obtain design solutions in a ‘short’ amount of time. • They are content to obtain approximate solutions that can be readily obtained in a reasonable time frame, and with reasonable effort. The FEM is one such approximate solution technique. • The FEM is a numerical procedure for obtaining approximate solutions to many of the problems encountered in engineering analysis with reasonable accuracy.

6

Finite Element Method Defined (cont.) • In the FEM, a complex region defining a continuum is discretized into simple geometric shapes called elements. • The properties and the governing relationships are assumed over these elements and expressed mathematically in terms of unknown values at specific points in the elements called nodes. • An assembly process is used to link the individual elements to the given system. When the effects of loads and boundary conditions are considered, a set of linear or nonlinear algebraic equations is usually obtained. • Solution of these equations gives the approximate behavior of the continuum or system. 7

Finite Element Method Defined (cont.) • The continuum has an infinite number of degrees-of-freedom (DOF), while the discretized model has a finite number of DOF. This is the origin of the name, finite element method. • The number of equations is usually rather large for most realworld applications of the FEM, and requires the computational power of the digital computer. The FEM has little practical value if the digital computer were not available. • Advances in and ready availability of computers and software has brought the FEM within reach of engineers working in small industries, and even students. 8

Finite Element Method Defined (cont.) Two features of the finite element method are worth noting. • The piecewise approximation of the physical field (continuum) on finite elements provides good precision even with simple approximating functions. Simply increasing the number of elements can achieve increasing precision. • The locality of the approximation leads to sparse equation systems for a discretized problem. This helps to ease the solution of problems having very large numbers of nodal unknowns. It is not uncommon today to solve systems containing a million primary unknowns. 9

1.2 How can the FEM Help the Design Engineer? • The FEM offers many important advantages to the design engineer:

• Easily applied to complex, irregular-shaped objects composed of several different materials and having complex boundary conditions. • Applicable to steady-state, time dependent and eigenvalue problems. • Applicable to linear and nonlinear problems. • One method can solve a wide variety of problems, including problems in solid mechanics, fluid mechanics, chemical reactions, electromagnetics, biomechanics, heat transfer and acoustics, to name a few. 10

How can the FEM Help the Design Engineer? (cont.) • General-purpose FEM software packages are available at

reasonable cost, and can be readily executed on microcomputers, including workstations and PCs. • The FEM can be coupled to CAD programs to facilitate solid modeling and mesh generation. • Many FEM software packages feature GUI interfaces, auto-meshers, and sophisticated postprocessors and graphics to speed the analysis and make pre and postprocessing more user-friendly.

11

How can the FEM Help the Design Organization? • Simulation using

the FEM also offers important business advantages to the design organization: • Reduced testing and redesign costs thereby shortening the product development time. • Identify issues in designs before tooling is committed. • Refine components before dependencies to other components prohibit changes. • Optimize performance before prototyping. • Discover design problems before litigation. • Allow more time for designers to use engineering judgment, and less time “turning the crank.” 12

1.3 Theoretical Basis: Formulating Element Equations • Several approaches can be used to transform the physical formulation of a problem to its finite element discrete analogue. • If the physical formulation of the problem is described as a differential equation, then the most popular solution method is the Method of Weighted Residuals. • If the physical problem can be formulated as the minimization of a functional, then the Variational Formulation is usually used.

13

Theoretical Basis: Variational • The variational method involves Method the integral of a function that produces a number. Each new function produces a new number. • The function that produces the lowest number has the additional property of satisfying a specific differential equation. • Consider the integral π = ∫ [D/2 (y’(x))2 - Qy]dx = 0. (1) The numerical value of π can be calculated given a specific equation y = f(x). Variational calculus shows that the particular equation y = g(x) which yields the lowest numerical value for π is the solution to the differential equation Dy’’(x) + Q = 0. (2) 14

Theoretical Basis: Variational Method (cont.) • In solid mechanics, the so-called Rayeigh-Ritz technique uses the theorem of Minimum Potential Energy (with the potential energy being the functional, π ) to develop the element equations. • The trial solution that gives the minimum value of π is the approximate solution. • In other specialty areas, a variational principle can usually be found. •Principle of minimum potential energy: For conservative systems, of all the kinematically admissible displacement fields, those corresponding to equilibrium extremize the total potential energy. If the extremum condition is a minimum, the equilibrium state is stable.

15

1.4 Advantages of the Finite Element Method • Can readily handle complex geometry: • The heart and power of the FEM. • Can handle complex analysis types: • Vibration • Transients • Nonlinear • Heat transfer • Fluids • Can handle complex loading: • Node-based loading (point loads). • Element-based loading (pressure, thermal, inertial forces). • Time or frequency dependent loading. • Can handle complex restraints: • Indeterminate structures can be analyzed.

16

Advantages of the Finite Element Method (cont.) • Can handle bodies comprised of nonhomogeneous materials: • Every element in the model could be assigned a different set of material properties. • Can handle bodies comprised of nonisotropic materials: • Orthotropic • Anisotropic • Special material effects are handled: • Temperature dependent properties. • Plasticity • Creep • Swelling • Special geometric effects can be modeled: • Large displacements. • Large rotations. • Contact (gap) condition.

17

1.5 Limitations of the Finite Element Method • A specific numerical result is obtained for a specific problem. A general closed-form solution, which would permit one to examine system response to changes in various parameters, is not produced. • The FEM is applied to an approximation of the mathematical model of a system (the source of so-called inherited errors.) • Experience, judgment and knowledge of structural theory are needed in order to construct a good finite element model. • A powerful computer and reliable FEM software are essential. • Input and output data may be large and tedious to prepare and interpret. 18

Limitations of the Finite Element Method (cont.) • Numerical problems: • Computers only carry a finite number of significant digits. • Can help the situation by not attaching stiff (small) elements to flexible (large) elements. • Susceptible to user-introduced modeling errors: • Poor choice of element types. • Distorted elements. • Geometry not adequately modeled. • Certain effects not automatically included: • Buckling • Large deflections and rotations. • Material nonlinearities . • Other nonlinearities. 19

2. FEM Applied to Solid Mechanics Problems (Displacement Method) 2.1 BASIC STRUCTURAL PRINCIPLES •Statically determinate structural problems can be solved by equilibrium equations •For redundant structures the equilibrium equations are insufficient •Additional equations are needed from consideration of the geometry of structural deformation •Continuity/ Compatibility of deformation leads to the additional required equations •Further more introducing the compatibility in terms of consistent deformation of the structure requires that a force displacement law is specified(stress strain relationships) 20

Thus the three important conditions needed are •Equilibrium of forces •Compatibility of deformation •Stress-strain relations(relating forces and deformations) These three principles are applied in developing the both the force method and the displacement methods of finite element methods of structural analysis

21

2.2 Assumptions

• If we do not understand the various assumptions properly, we would be wasting our time and resources. • Qualification of assumptions is a key to successful use of FEA in product design. To be capable of qualifying assumptions, we need to understand • Mechanics of materials being modeled. • Failure modes the product can encounter. • Manufacturing and operating environments the product might encounter, • Capabilities and limitations of element types and solution methods. •

You need to understand that there is an assumption behind every decision you make in FEA.

22

Mesh • • • • • •

Quality of mesh characterizes the convergence of the problem Global displacements should converge to a stable value, Other results should converge locally. A bad looking mesh always indicate a problem. A good looking mesh need not be a best mesh. Equilateral Triangles and squares shaped elements are ideal. Transition between densities should be smooth and gradual with out skinny distorted elements. When we use beams and shells, we are making assumptions that these can adequately represent the geometry and that they can capture the structural response of the system.

23

Static Analysis Assumptions •Loads are gradually applied to their full magnitude. •Vibratory or sinusoidal loads are not static. •Loads generated by Impact or collisions with another body is not static •Generally it takes some time for the load to get applied and reach final steady state value. Steady state implies loads of constant magnitude.

24

Geometry •Supplied CAD geometry adequately represent the physical part. •Only internal fillets in the area of interest will be included in the solution. •Thickness of the part is small enough relative to its width and length, such that shell idealization is valid. •If the dimensions of a particular part are not critical and will not affect the analysis results, some approximations can be made in modeling the particular part •Thickness of the walls are sufficiently constant to justify constant thickness shell elements •Primary members of structure are long and thin such that a beam idealization is required. •Local behavior at the joints of beams or other discontinuities are not of primary interest such that no special modeling of these area is required. •Decorative or external features will be assumed insignificant to the stiffness and the performance of the part and will be omitted from the model 25

Material Property. •Material remain in the linear regime. It is understood that either stress levels exceeding yield or excessive displacements will constitute a component failure. That is non linear behavior cannot be accepted. •Nominal material properties adequately represent the physical system. •Material properties are not affected by load rate. •Material properties can be assumed isotropic (Orthotropic) and homogeneous. •Part is free of voids or surface imperfections that can produce stress risers and skew local results. •Actual non linear behavior of the system can be extrapolated from the linear material results. •Weld material and the heat affected zone will be assumed to have same material properties as the base material. •Temperature variations may have a significant impact on the properties of the materials used. Change in material properties is neglected. 26

Boundary conditions •Choosing proper BC’s require experience. •Using BC’s to represent parts and effects that are not or cannot be modeled leads to the assumption that the effects of these un-modeled entities can truly be simulated or has no effect on the model being analyzed. •For a given situation there would be many ways of applying boundary conditions. But these various alternatives can be wrong if the user does not understand the assumptions they represent. •Symmetry/ anti-symmetry/ reflective symmetry/ cyclic symmetry conditions if exists can be used to minimize the model size and complexity.. •Displacements may be lower than they would have been had the boundary conditions been more appropriate. Stress magnitudes may be higher or lower depending on the constraint used 27

Fasteners •Residual stress due to fabrication , preloading of bolts, welding and/or other manufacturing or assembly processes are neglected. •Bolt loading is primarily axial in nature. •Bolt head or washer surface torque loading is primarily axial in nature. Surface torque loading due to friction will produce only local effects. •Bolts, spot welds, welds, rivets, and/or fasteners which connect two components are considered perfect and acts as rigid joint •Stress relaxation of fasteners or other assembly components will not be considered. Load on threaded portion of the part is evenly distributed on engaged threads •Failure of fasteners will not be reflected in the analysis

28

Assumptions. General. •If the results in the particular area are of interest, then mesh convergence will be limited to this area •No slippage between interfacing components will be assumed. •Any sliding contact interfaces will be assumed frictionless. •System damping will be normally small and assumed constant across all frequencies of interest unless otherwise available from published literature or actual tests. •Stiffness of bearings in radial or axial directions will be considered infinite •Elements with poor or less than optimal geometry are only allowed in areas that are not of concern and do not affect the overall performance of the model

29

2.3 Linear/Nonlinear Analysis •A linear approximation is a fast and efficient solution for many engineering problems. For design engineer it is a first step. The variance between a nonlinear solution and a linear approximation will determine how valid the linear results are. •Understanding the effects of the nonlinearity can enable a design engineer to make sound decisions on linear results. Working knowledge of nonlinear concepts and terminology will help in understanding the effects of nonlinearity. •It is important to understand the underlying assumptions of linear analysis. Once they are understood, it is possible to examine the real world problem and decide on the mode of analysis- nonlinear linear analysis •or Nonlinear material. behavior, plasticity, large displacements, or nonlinear buckling are some of the causes to go for nonlinear analysis •Nonlinear analysis is an iterative method requiring large amount of time and effort and should be carried out only if absolutely 30 necessary

2.3.1 Why Nonlinear Analysis Some common reasons to use nonlinear analysis are •Exact performance required - In the last stage of design process before proto type realization, it may be desirable to know the exact behavior of the product , which may necessitate a nonlinear analysis. - Another reason for obtaining exact performance data is a postmortem study. In case a system or a part of a system fails during operation, the need to know the exact cause of failure may necessitate a nonlinear analysis

•Contact analysis While part-to-part interfaces can be modeled with linear conditions and tricks to approximate contact, there are many instances that simply require the ability for the parts contacting surfaces to impact, slide, and/or lift off one another. This is most common when the loading on the system causes a portion of the contact interface to be in a compressive stage while the rest wants to 31 disengage.

•Large displacements In many thin-walled plastic parts, geometric or stress stiffening Plays a critical roll in the final response. The linear analysis may give displacements much more than the actual values. Nonlinear analysis can only give correct displacements.

•Fatigue analysis Fatigue analysis requires a sequence of maximum principal stresses structured by the loading history of the system, and calculate damage or life estimates. Precise stress estimates are required.

•Manufacturing and forming simulation Finite element analysis is being used to simulate the manufacturing process. The most common are metal forming or forging and plastic or casting filling simulations. In these tools the event of interest is nonlinear by definition.

32

2.3.2 Linearity Analysis Conditions Stress-strain •The relationship of stress to strain over the strains being studied must be linear and elastic. The part or system must return to its initial state elastically when all the external loads are removed.

Strain displacement •The displacements should be small, such that the relationship of strain to displacement are linear

Load continuity •The magnitude, orientation, and distribution of loads must not change between the unloaded and deformed conditions

33

2.3.4 Common Symptoms of Nonlinear Behavior Stress levels approach the yield point •Most materials will exhibit a significant range of nonlinear elastic behavior long before the yield stress is reached. •Another point to remember is reported yield stress is typically an estimated quantity (obtained by 0.2% offset method). The actual point where permanent set occurs may be appreciably lower than the reported yield stress. Take yield stress as a guide •Do not simply look at the reported maximum stress in the linear analysis results and assume that a nonlinear analysis is required. •Look at the area of high stress, the distribution of the stress approaching and exceeding yield, and determine the cause of these stresses. If the cause is a point load/constraint or a Poisson effect, a nonlinear run is probably not warranted, although remodeling may be. •If the high stress region is highly localized, there is a possibility of redistribution 34

Coupled displacements are restrained •End constraints may generate in-plane tensile stresses and stiffen the structure. Ex.: A long plate is supported at its ends and subjected to a pressure load. •While large displacements should prompt you to examine the system more closely, the degree of nonlinearity due to these displacements will be small in a lightly constrained case and larger as the constraints restrict the natural flow of the material •Consider the entire system before opting for a nonlinear solution

Larger displacements are expected In many cases, the system may undergo large displacements when in service as a part of desired performance. It is best to assume That a nonlinear solution is desired

35

Unreasonably high deflections are observed •A part is designed using sound engineering judgment and based on some historical experience of similar parts. In spite of this, large displacements are observed in the linear analysis- a nonlinear analysis will be required to confirm whether such displacements are real.

Two surfaces or curves penetrate •Contact is a nonlinear problem and its solution is time consuming. It is common practice to model the system with potential contact as a non-contact linear approximation and study these results before going for a nonlinear solution. If penetration occurs in one or more of the suspect regions, a contact condition should be modeled and a nonlinear solution employed •Linear analysis also helps in estimating the reaction forces at the contact surfaces, which could be applied as loads for the purpose of debugging and converging the mesh in case of large models..

36

2.4 Common Types of Nonlinear behavior •Most nonlinear behavior in product design can be categorized into one of three common types: Material, geometric, and boundary nonlinearity. •Material nonlinearity is the type most commonly thought of when the topic of nonlinear is suggested. A stress strain curve is typically known to be nonlinear; therefore it requires a nonlinear analysis. The other two types are more common in design analysis •In many cases , if material nonlinearity is present, one or both of the other two types will be required as well

37

2.4.1 Material Nonlinearity •If a nonlinear material model is required to provide the data necessary to verify or improve the design, test data or the generic data found in data sheets or a vendor’s reference data base after careful examination should be used. •A key feature of a nonlinear solution is the need to continually reevaluate the strain state to determine which modulus , or stiffness, should be applied to an element at any given load step. •In the nonlinear world there are many types of modulii you should be familiar. Some of these names are tangent modulus, secant modulus, elastic modulus, plastic modulus, hardening modulus •The name of the modulus used is dependent upon the material model chosen. The success and efficiency of a nonlinear material solution are dependent on the choice of the material model

38

Yield Criteria When plastic behavior is desired or expected, you will need to tell the server which criteria to seek to initiate yielding. Some of the more common yield criteria are •Tresca, which looks at the maximum shear stress in the model and provides a reasonable calculation of the brief plasticity in more brittle materials. •Von Mises looks to the von Mises stress to determine yielding and is the best criterion for crystalline plastics and ductile materials •Mohr-Coulomb, which evaluates a combination of maximum and minimum principal stresses to determine yielding , is some what more accurate for plasticity in moderately brittle materials Drucker-prager combines data from the first and second stress invariants and is better for problems involving materials such as soil and concrete. It provides the best model for yielding i.e. , first invariant dependent such as at crack tips and in amorphous plastics. The above criteria are primarily the same as the failure criteria 39

Hardening Rules •A hardening rule determines how the material model responds to repeated stress reversals, or switching between tension and compression. •In ductile material that has never experienced plasticity, the yield point in tension can be expected to equal the opposite of the yield stress in compression. •However once tensile yielding has occurred, some materials experience a phenomenon known as the Bauschinger Effect, which causes the yield point in compression to be somewhat less than the compressive equivalent of the initial yield stress. Consequently nonlinear solutions have implemented hardening rules to allow for adjustment of the yield point in stress reversals •An isotropic hardening model does not take the Bauschinger Effect, into account. •A kinematic hardening model will take into account the reduction in the compressive yield point after a stress reversal 40

Commonly Used Material Models •An important decision to be made when considering a nonlinear analysis is the material model selection. Various material approximations are available. The common material models are - Bilinear Material Model - Tri-linear Material Model - Multi-linear stress-strain curve - Stress-strain curves- offset by temperature and strain rate •Regardless of your choice of models, three pieces of data must be specified: yield stress, yield criteria, and hardening rule •In a bilinear material model, there are two required modulii: the elastic modulus and the plastic modulus. The plastic modulus is activated when a stress in an element exceeds the specified yield criterion. As in a linear analysis, the plastic modulus is interpolated for all strains in excess of yield. 41

•Many materials experience noticeable hardening after the onset of plasticity. In these materials, the response of the system to large strains will diverge in a bilinear model. Therefore, a tri-linear model contains a third, hardening modulus to account for this. •For tri-linear material models, you need to specify three modulii (E1, E2 and E3 ) and two transition stresses (yield and a hardening transition strain). •All material models with more than two modulus transitions are lumped into multi-linear classification. A multi-linear model is input using pairs of stress-strain (S-S) values. The data should be extracted from a standard tensile test.

42

B ilinear M aterial M odel

Stress

4

Slope =E , Plastic m odulus 2

Slope=E , Y oungs m odulus, E lastic m odulus 1

0 0

6

Strain

43

T rilinear M aterial M odel 4

Slope, E = 3

Stress

H ardening M odulus

Slope =E , Plastic m odulus 2

Slope=E , Y oungs m odulus, E lastic m odulus 1

0 0

11

Strain

44

M ultilinear Stress Strain C urve

Stress

5

0 0

25

Strain

45

•For ferrous materials, the stress-strain (S-S) curve is relatively independent of temperature and strain rate. •However, most other materials, especially plastics, will show a shift resulting from strain rate and temperature. •As a general rule, stiffness increases as strain rate increases. This will result in an upward shift of the curve. Similarly, as the testing temperature increases, the material tends to soften and this is illustrated by downward shift in the S-S curve. This is illustrated in the following figure •To obtain the above data, material testing under conditions similar to actual problem is ideal. If this is not possible the data base supplied by material supplier should be used.

46

Stress strain curves offset by tem perature and strain rate 80

60

Stress

Increased strain rate 40

20

Increased temperature 0 0

1

2

Strain

3

4

47

2.4.2 Geometric Nonlinearity •Geometric nonlinearity primarily refers to stiffness changes that are independent of material properties. The stiffness change can be related to geometry constraints and/or the magnitude of strain. •The large in-plane stress induced by the deformation is the one common characteristic of geometric nonlinearity. This may happen due to boundary constraints. •Strain- displacement relations used for linear analysis assumes small displacements and higher order terms are neglected . If the structural deformations are large linear analysis will not give correct results. nonlinear analysis has to carried out. •It is difficult to decide on the need for nonlinear analysis. The general guide line is that if the observed displacement through linear analysis is about one third to one times the wall thickness, then you may have to go for nonlinear analysis. •Geometric nonlinearity is ease to handle. Need to give the option with few defined load steps 48

2.4.3 Boundary Nonlinearity •Boundary nonlinearity is the change in boundary conditions due to resultant deformation. There are two common occurrences of boundary nonlinearity : Contact and follower forces

Contact •Contact conditions allow parts or portions of the same part to touch or lift of each other. This capability may be necessary to model the interaction of certain systems

Follower forces •Follower forces represent loads that are dependent on the orientation of the features to which they are applied. If a feature deflects so much that the orientation of the load becomes of interest , geometric nonlinearity should probably be considered. •Nonlinear forces can be defined as displacement or velocity based; they can be defined to follow the orientation of a feature or scale with displacement or velocity magnitudes in a particular degree of freedom. 49

2.4.4 Other types of Nonlinearities Hyperelastic Hyperelastic materials, such as rubber, silicone, and other elastomers, behave differently than standard engineering materials. Their strain displacement relationship is nonlinear even at small strains, and they are nearly incompressible. The Poisson’s ratio of hyperelastic materials may be near to 0.5.

Nonlinear Transients A nonlinear transient analysis is used to calculate the response of a part or a system in which properties or boundary conditions vary withtime. A good example is crash or impact analysis.

Creep Creep is the term used to define time varying permanent strain due To long-term application of a constant or near-constant stress level. When the material creeps, it effectively relaxes and the stress levels in the part reduce. 50

Nonlinear Buckling Analysis A linear buckling analysis gives the critical buckling load and the Initial buckled shape based on the orientation of an existing load set. The linear analysis will not give the post-buckling behavior of the structure. To determine the post collapse response of a structure, a nonlinear buckling analysis is required

Bulk Metal Forming Bulk metal forming analysis, such as sheet metal folding, forging, And cold heading usually require a special software configuration that will automatically cleanup elements that become overly distorted by the excessive deformations of the mesh.

51

2.5 FEM Applied to Solid Mechanics Problems

Create elements of the beam

Nodal displacement and forces dxi 1

dyi 1

dxi 2

1

2

4

3

dyi 2

• A FEM model in solid mechanics can be thought of as a system of assembled springs. When a load is applied, all elements deform until all forces balance. • F = Kd • K is dependant upon Young’s modulus and Poisson’s ratio, as well as the geometry. • Equations from discrete elements are assembled together to form the global stiffness matrix. • Deflections are obtained by solving the assembled set of linear equations. • Stresses and strains are calculated from the deflections. 52

Classification of Solid-Mechanics Modal analysis AnalysisProblems of solids Static Elementary

Response transient/ harmonic/random

Dynamic s

Advanced Behavior of Solids

Linea r

Skeletal Systems 1D Elements Trusses Cables Pipes

Nonlinea r

Geometric Classification of solids Plates and Shells 2D Elements

Stress Stiffening Large Displacement

Geometri c Fractur e Materia l

Plane Stress/Plane Strain Axisymmetric Plate Bending Shells with flat elements Shells with curved elements

Instability Plasticity Viscoplasticity

Solid Blocks 3D Elements Brick Elements (Hexahedral)) Tetrahedral Elements General Elements 53

Governing Equation for Solid Mechanics Problems • Basic equation for a static analysis is as follows:

[K] {u} = {Fapp } + {Fth } + {Fpr } + {Fma } + {Fpl } + {Fcr } + {Fsw } + {Fld } (1) [K]

= total stiffness matrix

{u}

= nodal displacement

{Fapp } = applied nodal force load vector {Fth } =applied element thermal load vector {Fpr } =applied element pressure load vector {Fma } =applied element body force vector Loads related to Nonlinear analysis {Fpl } =element plastic strain load vector {Fcr } =element creep strain load vector {Fsw } =element swelling strain load vector {Fld } = element large deflection load vector

54

2.5.1 Six Steps in the Finite Element Method • Step 1 - Discretization: The problem domain is discretized into a collection of simple shapes, or elements. • Step 2 – Selection of elements- depends on the type of structure • Step 3 - Assembly: The element equations for each element in the FEM mesh are assembled into a set of global equations that model the properties of the entire system. • Step 4 - Application of Boundary Conditions: Solution cannot be obtained unless boundary conditions are applied. They reflect the known values for certain primary unknowns. Imposing the boundary conditions modifies the global equations. • Step 5 - Solve for Primary Unknowns: The modified global equations are solved for the primary unknowns at the nodes. • Step 6 - Calculate Derived Variables: Calculated using the nodal values of the primary variables.

55

Process Flow in a Typical FEM Analysis Start

Analysis and design decisions

Problem Definition

Stop

Processor Pre-processor • Reads or generates nodes and elements (ex: ANSYS) • Reads or generates material property data. • Reads or generates boundary conditions (loads and constraints.) Step 1, Step 4

• Generates element shape functions • Calculates master element equations • Calculates transformation matrices • Maps element equations into global system • Assembles element equations • Introduces boundary conditions • Performs solution procedures

Post-processor • Prints or plots contours of stress components. • Prints or plots contours of displacements. • Evaluates and prints error bounds. Step 6

Steps 2, 3, 5 56

Discretization - Mesh Generation surface model airfoil geometry (from CAD program)

3 1 12 14 13

4

5 11

2

mesh generator ET,1,SOLID45 N, 1, 183.894081 N, 2, 183.893935 . . TYPE, 1 E, 1, 2, 80, E, 2, 3, 81, . . .

, -.770218637 , -.838009645

79, 80,

4, 5,

5, 6,

, ,

5.30522740 5.29452965

83, 84,

82 83

meshed model 57

Boundary Conditions and Loads • Displacements ⇒ DOF constraints usually specified at model boundaries to define rigid supports. • Forces and Moments ⇒ Concentrated loads on nodes usually specified on the model exterior. • Pressures ⇒ Surface loads usually specified on the model exterior. • Temperatures ⇒ Input at nodes to study the effect of thermal expansion or contraction. • Inertia Loads ⇒ Loads that affect the entire structure (ex: acceleration, rotation). 58

2.5.2 Development of element stiffness matrix Variation principle spring-mass example A spring of stiffness k subjected to load P has deflected to a displacement of u The internal strain energy U = ½ (Force in the spring X Displacement = ½ (k u) (u)= ½ k u2 Potential energy of the external load P is Wp = (Load) X Displacement from zero potential state = -P u Total potential π =U + Wp = ½ k u2 – P u The minimum of π can be obtained by differentiating with respect to u and equating it to zero

∂π = ku − P = 0 ∂u ku = P

is the equilibrium equation for the spring mass system

59

Overview of stiffness and loads evaluation Analysis steps

Generalized coordinate method

Interpolation model method

1.Element configuration 2.Displacement model

-

-

u =φ α q=Aα α = A- q

u=Nq

3.element strains and stresses

ε = Bα α σ = CBα α

ε =Bq σ =CBq

4.Element stiffness and loads

kα = ∫ ∫ ∫ Bα T C Bα dv

kα = ∫ ∫ ∫ BT C B dv

Qα = ∫ ∫ ∫ φ T X dv +∫ ∫ φ T ds k= A- T kα A

T

Q = ∫ ∫ ∫ NT X dv + ∫ ∫ NT T ds

Q= A- T Qα 5. Equilibrium equation

[k] {q} =Q

[k] {q} =Q 60

Stiffness matrix of a 2 node axial element Consider an element of length L and cross sectional area, A A load P is applied at node 1 and node 2 is constrained.

Stress

u1

P σ= A

Stress strain relationship

ε=

σ E

1

2

du P Strain-displacement relationship ε = dx = EA P PL dx = The displacement u at node 1 = ε = EA EA L ∫ 0

P EA The stiffness is defined as force for unit displacement = = u L

61

u2

Stiffness Matrix

ku = P

 k11 k  21

k12   u1    = { P} (3)  k 22  u2 

K11 is the force required at node 1 to cause unit displacement at node 1 with displacement at node 2 zero. K21 is the force at node 2 due to unit displacement at node 1 with displacement at node 2 zero Similarly K22 is the force required at node 2 to cause unit displacement at node 2 with displacement at node 1 zero. K21 is the force at node 1 due to unit displacement at node 2 with displacement at node 1 zero Thus

EA  1 − 1 [k] =  L − 1 1 

(4)

K11 , k12 , k22 , k21 are called stiffness influence coefficients 62

Stiffness matrix of a bar element Method 1: Generalized coordinate method Number of Nodes 2 DOF per node: 1 , Displacement u1 Element displacements: u1 u2 Length l C/S area A Displacement function( polynomial) Y’ Modulus E u = a0 +a1 x Where a0 and a1are generalized coordinates a0 (1) a } u= {φ }T{α }= [1 x]{

u2 x

1

u1 = a0 u2 = a0 +a1 l 1

u1

{q}=

0

= [A] {α } = u2

1

l

a0 a1

(2) 63

1

0

{α }= [A]-1 {q}=

u1 u2

(3)

-1/l 1/l ao ε =∂u/ ∂x =Bα α = 0 1 

a1

(4)

σ =[c] ε =[E] ε [kα ]= A ∫ [Bα ]T[E] [Bα ] dx Though the above integral is volume integral the strain is constant across width and depth so dv=A dx 64

[k]= A ∫ [A-1 ]T [Bα ]T[E] [Bα ] [A-1 ] dx Substituting for [A]-1 and [Bα ] from equations 3 and 4 gives 2  E /l [ k ] = A∫0  2 − E / l  l

− E /l2 dx 2  E /l 

The element stiffness matrix is EA  1 − 1 [k] =  l − 1 1 

65

Example 1:Two Degrees of Freedom System – Static analysis

F1

k1

F2

k3

k2

x1 k 2 ( x2 − x1 )

k1 x1 F1 Equations of motion

x2

k 2 ( x2 − x1 )

k1 x1 + k 2 ( x1 − x2 ) − F1 = 0

k 2 ( x2 − x1 ) + k3 x2 − F2 = 0

k 3 x2 F2

(a)

66

Rearranging the equations in matrix form

− k 2   x1   F1  (k1 + k 2 )  =   −k  (k 2 + k3 )  x2   F2   2 or

[ K ]{x} = {F }

(b)

©

Where x1 and x2 are the displacements at nodes 1 and 2 respectively. K is the stiffness matrix, x is the displacement matrix and F is the force matrix Spring stiffness and applied forces are known. The displacements have to be found. The solution is

{x} = [ K ]−1{F }

(d)

Example: assume k1 = k 2 = k3 = k 67

 2k [K ] =  − k

− k 2k 

Or

1 2 1 [K ] =  3k 1 2 −1

The solution (Eq. (d) is  x1  1 2 1   F1   =   F  x 3 k 1 2   2   2 Let F1 = F2 = 10000.N and k = 200000 N/M  x1  2 1 1000 0.005 1  =  =     x2  3 X 200000 1 2 1000 0.005

68

Example 2:A uniform rod of length 3L is fixed at both ends and axial load applied at location L and 2L as shown. 1

F1 2

F2 3

1 2 3 4 Idealized as 3 elements of equal length. The element stiffness is EA  1 − 1 [k] =  L − 1 1 

The stiffness matrix, displacement vector and force vector for complete structure is  x1   1 −1 0 0  0 x    F   2 EA − 1 2 − 1 0   1 { X} =   [K] = { F } =   x L  0 − 1 2 − 1 F2   3   0 0 −1 1   x4   0    69

The equilibrium equation is  1 − 1 0 0   x1   0       EA − 1 2 − 1 0   x2   F1   =  L  0 − 1 2 − 1  x3   F2   0 0 −1 1 x   0    4   

(a)

Applying boundary conditions ( fixed at both ends)  1 − 1 0 0   x1   0       EA − 1 2 − 1 0   x2   F1   =  L  0 − 1 2 − 1  x3   F2   0 0 −1 1 x   0    4   

(b)

 2 − 1  x2   F1  k   =   © Where k=EA/L  − 1 2   x3   F2  70

The solution of equation © is  x2  1 2 1   F1   =   F  (d) x 3 k 1 2   2   3 Let F1 = F2 = 10000.N and k = 200000 N/M  x2  2 1 1000 0.005 1  =  =     x3  3 X 200000 1 2 1000 0.005

(e)

The result is same as the previous example Substituting for the displacements from Eq. (e) in (a)  1 − 1 0 0   0  − 1000 − 1 2 − 1 0  .005  1000       200000  =     0 − 1 2 − 1 .005  1000   0 0 − 1 1   0  − 1000      The reactions at the fixed end (nodes 1 & 4) = -1000N

71

2.6 Dynamic analysis Free vibration (Modal analysis): •Natural frequencies and mode shapes •The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. They are also required to do a spectrum analysis or a mode superposition harmonic or transient analysis.

Response: •Steady state response •Transient response- Example: crash/impact •Response to random excitation

72

Equation of motion

[ M ]{ x} + [ C ]{ x } + [ K ]{ x} = { Q} Is the equation of motion for a structure undergoing vibration under external load. Where [M], [C], [K], and {Q} are the mass, damping, stiffness and load matrices respectively. •The load matrix {Q} is function of time and can be steady state, transient, or random • x, x  , x are the displacement, velocity, and acceleration vectors respectively

73

3.0 Element selection & application 3.1 Selection of element The selection of element depends on type of structure •Type of structure: simple column,beam,plate,shell or stiffened structure. Stiffened structure could be plane or curved • The structure could be a truss with hinged or welded joints •Plate or shell type of structures could be thin or thick •The structure could be pressure vessel of complex shape, non-uniform thickness and made of orthotropic material. It could be axisymmetric • The structure could be solid body of irregular shape and of orthotropic material 74

Modeling types The most common modeling types are •Planar simulations •Plane stress •Plane strain •Axisymmetric •3D simulation and modeling •Beam simulation •Symmetry or anti-symmetry •Plate or shell models •Solid models

75

3.2 Discretization •Subdivision process is essentially an exercise of engineering judgments •The number, the shape,size and configuration of the elements has to be decided in such a way that the original body is simulated as closely as possible •The general objective of a such discretization is to divide the body in to elements sufficiently small so that the simple element can approximate the true solution as close as possible

3.3 Subdivision at discontinuities: •Nodes to be located at places where abrupt changes in geometry, loading and material properties •Refined mesh for steep gradients. One example where steep gradients of the variable occurs are at which stress concentration exists 76

3.4 Geometric approximation: If straight sided elements are employed, curved boundaries are approximated by piecewise linear. To idealize as closely as possible to the curved boundary refined mesh may be necessary.

3.5 Element quality parameters Aspect ratio : For two dimensional elements aspect ratio is defined as ratio of the largest dimension to the smallest dimension. Aspect ratio of 1 is ideal. However in unavoidable circumstances aspect ratio of about 3 is acceptable. Jacobian and warping are other quality parameters

77

3.6 Analysis of large structures •To circumvent large computer facility and time two approaches are followed. One is course to fine sub division method and the other is substructure method Course- to- fine subdivision method The large structure is subdivided in to course mesh and finite element analysis is carried out to obtain displacements and stresses. Zone of specific interest is selected and subdivided in to finer meshes. The stresses and displacements obtained from course analysis are applied along the boundary of the specific zone and analysis is carried out to obtain better results. 78

Substructure method The large structure is subdivided in to convenient small components/substructures •The stiffness matrix for each substructure is determined by subdividing the structure into a number of smaller, simple finite elements •Obtain the overall stiffness of the substructure •Condense the substructure stiffness to eliminate the internal degrees of freedom which do not participate in the inter connections of the different structures •Assemble/add the stiffness of individual substructure and obtain the overall equilibrium equation. Carryout the analysis for the given loads on the overall structure

79

•The detailed solution for the individual substructure are then obtained by performing finite element analysis for each one of them with input loads and/or displacements derived from the analysis of parent structure Finite representation of infinite bodies •It is not possible to model an infinite body.we must limit it or make it finite. •One case is where loading is on part of the body. The effect of loading decreases with increasing distance from the point of application. By trail and error the significant extent of the structure to be modeled can be found out. •Some infinite bodies can be analyzed by plain strain idealization. One such example is gravity dam. 80

H-element Vs. P-element (higher order element ) •Two choices are, use of simple lower order element (H-element) with finer mesh or use of higher order element which may need less number of elements to get same result •If the discretization is such that the final number of algebraic equations to be solved are same in both cases,then the higher order model gives more accurate solution. Due to higher band width the computation effort is higher in second case. It also to be noted that the trade off between mesh refinement and higher order model also depends on the type of problem •The basic philosophy of the FEM is that simple but relatively complete models are used to get approximate solution to complicated problem 81

3.7 Sources of Error in the FEM • The three main sources of error in a typical FEM solution are discretization errors, formulation errors and numerical errors. • Discretization error results from transforming the physical system (continuum) into a finite element model, and can be related to modeling the boundary shape, the boundary conditions, etc.

Discretization error due to poor geometry representation.

Discretization error effectively eliminated.82

Sources of Error in the FEM (cont.)

• Formulation error results from the use of elements that don't precisely describe the behavior of the physical problem. • Elements which are used to model physical problems for which they are not suited are sometimes referred to as ill-conditioned or mathematically unsuitable elements. • For example a particular finite element might be formulated on the assumption that displacements vary in a linear manner over the domain. Such an element will produce no formulation error when it is used to model a linearly varying physical problem (linear varying displacement field in this example), but would create a significant formulation error if it used to represent a quadratic or cubic varying displacement field.

83

Sources of Error in the FEM (cont.) • Numerical error occurs as a result of numerical calculation procedures, and includes truncation errors and round off errors. • Numerical error is therefore a problem mainly concerning the FEM vendors and developers. • The user can also contribute to the numerical accuracy, for example, by specifying a physical quantity, say Young’s modulus, E, to an inadequate number of decimal places.

84

3.8 Problems in structural mechanics Topic

Typical application

I. 2-D stress analysis a. Plane strain -Gravity dam, Buried pipes b. Plane stress -Stretching of plates with holes, notches etc. bending of deep beams c. Axisymmetric -Axisymmetric thin/ thick shells; Nuclear containment vessels, rocket motors etc. II 3-D stress analysis -Machine parts, Thick shells, Nuclear containment vessels, arch dams III Bending of plates -Automotive floor slabs, ship decks, hulls, aircraft panels,

85

Problems in structural mechanics Topic

Typical application

IV Bending/ stretching of shells a. Axisymmetric -Roof domes, pressure vessels b.

General

-Thin arch dams, Shell roofs, ship hulls, curved panels

V Stability (Buckling)

-Beams, columns, frames, plates, shells, stiffened panels VI Stiffened structures -Commercial vehicles body, stiffened panels, Bridge decks, aircraft wing and fuselage 86

4.0 Boundary Conditions Simply supported/ Hinged: Displacement is zero and rotations allowed Clamped : Both displacements and rotations suppressed Free- Free : Structure is free from any restrained Partially restrained :Displacement or rotations or both of them constrained by spring supports

87

Boundary conditions - Beams w

o ooo o ///////////

o



θ u

Movable hinge w=0 Immovable hinge Simply supported u=0 , w=0 Only lateral movement Allowed. u= 0, θ y=0

///////////

Clamped u= w = θ y= 0 Supported on lateral spring u= 0

o

u = w = 0 Rotation constrained by torsional spring

•Boundary conditions could be specified displacements

88

Symmetry/ Antisymmetry •A symmetrical system of loads is a system of forces and/or moments in which there exists, for each load, another load, equal in magnitude and symmetrical in sense placed symmetrically to the first load with respect to the axis of symmetry of the system •An antisymmetrical system of loads is a system of forces and/or moments in which there exists, for each load, another load, equal in magnitude and antisymmetrical in sense placed symmetrically to the first load with respect to the axis of symmetry of the system •By the use of symmetry and antisymmetry boundary conditions computation effort can be reduced substantially.

89

Symmetry/ Antisymmetry •If a structure and applied load is symmetric about an axis, analysis of half of the structure is sufficient with appropriate symmetric boundary conditions along the axis of symmetry •If a structure is symmetric and applied load is antisymmetric about an axis, analysis of half of the structure is sufficient with appropriate antisymmetric boundary conditions along the axis of symmetry. •If a two dimensional structure and applied load is symmetric about two axes, analysis of quarter of the structure is sufficient with appropriate symmetric boundary conditions along the two axes of symmetry.Similarly a three dimensional structure is symmetric about 3 axes, one eighth of structure can be analyzed

90

Boundary conditions - Beams Plane of symmetry u= 0, θ y= 0

z(w)

y(v) x(u) DOF:u w θ

y

Plane of anti-symmetry w=0

91

Boundary conditions - Beams z(w) Case A

P

Plane of symmetry u= 0, θ y= 0 Case B

P/2

y(v) x(u) DOF:u w θ

y

P/2

Case A= Case B+Case C

Case C

Plane of anti-symmetry w=0 P/2 P/2

92

Boundary conditions- Plates y (v, θ y) B

A Nodal DOF: u v w θ xθ y θ

z (w, θ z)

z

x (u, θ x)

o

D Edge boundary conditions:

C

Clamped: u v w θ x θ y θ z are zero Simply supported:u v w are zero along all edges θ x θ z are zero along edges AD & BC θ y θ z are zero along edges AB & DC

93

Boundary conditions- Plates Along Symmetrical axis y (v, θ y)

Nodal DOF: u v w θ xθ y θ

z (w, θ z)

z

o

x (u, θ x)

Symmetric : Along ox v, θ x , θ z are zero Along oy u, θ y , θ z are zero Anti-symmetric: Along ox u, w , θ y are zero Along oy v, w , θ x are zero 94

Boundary conditions Axi-symmetric shell y (v, θ y)

y (v, θ y) z (w,θ z)

DOF: u v w θ x θ

y

θ

x (u, θ x)

z

Sym. BC: Along xz plane v = θ x= θ z = 0 Along yz plane u = θ y= θ z = 0 Along xy plane w = θ x= θ y = 0 Anti-sym. BC: Along xz plane u = w= θ y = 0 Along yz plane v = w= θ x = 0 Along xy plane u = v= θ z = 0

95

•If an axisymmetric structure is subjected to a concentrated antisymmetric load it is still possible to do an axisymmetric analysis by expressing the load as a function of fourier series. The radial and the tangential displacements also expressed in terms of fourier series. •If the concentrated or line load is acting on the line of symmetry and the analysis is carried out for half structure due to symmetry the load also is to be taken half only for analysis •If the plate type of structures is having two plane symmetry the free vibration analysis can be carried out for one fourth of the Structure four times with sym-sym, sym-antisym, antisym-sym, and antisym.-antisym boundary conditions and obtain all frequencies and mode shapes. 96

Near-symmetry •In many cases, slightly asymmetric geometry can be initially modeled as symmetric by analyzing the less rigid half under the assumption that if the weaker half is acceptable, the stronger half will be also acceptable. •Analyst engineering judgment is critical, because the assumption of near-symmetry may not be valid in all cases

97

Cyclic symmetry •Cyclic symmetry is a more specialized condition where features that are repeated about an axis can be modeled by a single instance of that feature. Common applications of cyclic symmetry are fan blades, turbine blades, flywheels, and motor rotors. •In addition to the geometric definition, which is subjected to the near-symmetric assumptions made earlier, constraints and loading must fit the cyclic symmetry requirements. •In Cyclic symmetry, each instance of the feature must see the same boundary conditions in its respective frame of reference •Acceptable loading might be centrifugal forces, radial displacements due to a press-fit, or uniform wind or fluid resistance due to spinning 98