FINITE ELEMENT METHODS FOR MECHANICAL ENGINEERING MME3360b Winter2012 Prof. Paul M. Kurowski

MME3360b web site http://www.eng.uwo.ca/MME3360b/2012/

Design Center web site http://www.eng.uwo.ca/designcentre/

SOFTWARE INSTALLATION Questions? Ask Yara Hosein your TA

LAB THIS WEEK Download and read it for Thursday lab if you don’t have the book Download for Thursday lab

3% BONUS http://www.solidworks.com/sw/support/810_ENU_HTML.htm

MONKEY CLIMBING TWO ROPES

TWO ROPES

TEXT BOOKS Recommended Required

FUNDAMENTAL CONCEPTS OF FINITE ELEMENT ANALYSIS

TOOLS OF DESIGN ANALYSIS REAL OBJECTS MODELS PHYSICAL MODELS MATHEMATICAL MODELS ANALYTICAL NUMERICAL FINITE ELEMENT METHOD FINITE DIFFERENCE METHOD BOUNDARY ELEMENT METHOD

NUMERICAL TOOLS OF DESIGN ANALYSIS Structural design analysis problems are described by a set of partial differential equations and belong to the class called boundary value field problems. Such problems can be solved approximately by different numerical methods. Finite Element Method Based on the variational formulation of a boundary value problem. In the FEM the unknowns are approximated by functions generated from polynomials. The polynomials are defined on standard elements (such as triangles and rectangles) which are then mapped onto elements with (possibly) curved sides or faces and the continuity of the mapped polynomials is enforced. These functions are effective for the reasons of numerical efficiency. The solution domain must be divided (meshed) into elements that can be mapped from the standard elements using mapping functions. For reasons of numerical efficiency and versatility, most commercial analysis systems are based on the Finite Element Method commonly called Finite Element Analysis (FEA) Finite Difference Method Based on the differential formulation of a boundary value problem. This results in a densely populated, often ill-conditioned matrix leading to numerical difficulties. Boundary Element Method Based on the integral equation formulation of a boundary value problem. This also results in densely populated, non-symmetric matrix. Boundary Element Methods are efficient only for “compact” 3D shapes.

BASIC STEPS IN THE FINITE ELEMENT ANALYSIS Step 1 Creation of a mathematical model An idealization of a real object accounting for geometry, loads, supports and material properties leads to a formulation of a boundary value problem described by a set of governing partial differential equations. Most often these equations are impossible to solve analytically and an approximate numerical method must be used. Step 2 Deciding on the solution method For reasons of numerical efficiency and generality we select the Finite Element Method. Step 3 Approximating solution with piecewise polynomials In order to represent solution with piecewise polynomials, we divide the body into simple shape sub domains (elements) and define our polynomials (also called shape functions), with yet unknown factors ai , bi ,ci (also called nodal degrees of freedom) in each of element separately. In the finite element method, nodal degrees of freedom are nodal displacements or temperatures. Notice that by selecting certain polynomial order, we impose displacement pattern in each element. Working with the first order polynomial (linear) we agree on linear displacement field, while second order polynomial will return second order displacement field etc.

BASIC STEPS IN THE FINITE ELEMENT ANALYSIS Continuous body - mathematical model Discretized body – finite element model Step 4 Finding nodal displacements Now we use the principle of minimum total potential energy (the state of minimum total potential energy is also the state of equilibrium) to find this set of ai , bi ,ci factors that minimizes the total potential energy of the body. This is also the new state of equilibrium under load. Knowing ai , bi ,ci we can now calculate discertized displacement anywhere in the body. Notice that displacements are primary unknowns and are calculated first. Of course the accuracy of the results will depend on how well the exact solution can be approximated by the particular design of the mesh and selection of the polynomial degrees. Step 5 Finding strains and stresses Once displacements have been found, we calculate strains as derivatives of displacements. Knowing strains and material properties we can now find stresses.

BASIC STEPS IN THE FINITE ELEMENT ANALYSIS Idealization of geometry (if necessary) Type of analysis Material properties Restraints Loads MATHEMATICAL MODEL CAD geometry Simplified geometry CAD FEA Pre-processing

BASIC STEPS IN THE FINITE ELEMENT ANALYSIS Discretization Numerical solver MATHEMATICAL MODEL FEA model FEA results FEA Pre-processing FEA Solution FEA Post-processing

[ F ] = [ K ] * [ d ] FEA EQUATIONS [ F ] vector of nodal loads known [ K ] stiffness matrix known [ d ] vector of nodal displacements unknown

CAD GEOMETRY AND FINITE ELEMENTS GEOMETRIC ENTITY MESHED ELEMENTS CREATED GEOMETRY Volume Solids 3D Surface Shells Curve Beams 2D Plane Beams

DEGREES OF FREEDOM, SHAPE FUNCTIONS 1st order tetrahedral element Before deformation After deformation 2nd order tetrahedral element Before deformation After deformation Degrees of freedom Everything there is to know about the behaviour of this element under load can be calculated as soon as x, y and z displacements of all nodes defining that element are found. x, y and z displacements components fully describe node displacement for these 3D tetrahedral elements. x, y and z displacements are the three degrees of freedom of each node. Shape functions The displacement at any point within the element is a function of nodal displacements. This function is called shape function. In the first order element the shape function is a linear combination of nodal displacement, in the second order element this a second order function etc.

Nodes of solid elements do not have rotational degrees of freedom. With only one node restrained the element spins in three directions. With two nodes restrained the element spins about the line connecting two nodes. With three nodes restrained the element won’t move. Nodes of solid elements do not have rotational degrees of freedom. DOF.SLDASM

Most often used element DEGREES OF FREEDOM Tetrahedral solid element 3 D.O.F. per node Triangular shell element 6 D.O.F. per node First order elements Linear displacement Constant stress Second order elements Second order displacement Linear stress Most often used element

TYPES OF ELEMENTS AND DEGREES OF FREEDOM Solids x, y and z nodal displacement components fully describe behavior of each node. Each node has 3 D.O.F Shells and beams x, y and z displacements are not sufficient to describe what is happening to each node while element deforms. Also needed are rotations about x, y and z axis so each node has 6 D.O.F. 2D plane stress, plane strain, axi-symmetric x and y displacement fully describe behavior of each node. Each node has two degrees of freedom.

TYPICAL ANALYSIS ASSUMPTIONS: LINEAR MATERIAL MODEL STRESS Linear material model Non-linear material model Linear range STRAIN The linear material behavior complies with Hooke’s law:  =  E in tension =  G in shear

TYPICAL ANALYSIS ASSUMPTIONS: SMALL DISPLACEMENTS To comply with assumptions of small displacements theory, the displacement must not change the stiffness in a significant way. Note that displacements don’t have to be large to significantly change the stiffness.

3D STATE OF STRESS State of stress expressed by six stress components. State of stress expressed by three principal stresses.

VON MISES STRESS CRITERION The maximum von Mises stress criterion is based on the von Mises-Hencky theory, also known as the shear-energy theory or the maximum distortion energy theory. The theory states that a ductile material starts to yield at a location when the von Mises stress becomes equal to the stress limit. In most cases, the yield strength is used as the stress limit. Factor of safety (FOS) = slimit  / svon Mises  

THE MAXIMUM SHEAR STRESS CRITERION Also known as Tresca yield criterion, is based on the Maximum Shear stress theory. This theory predicts failure of a material to occur when the absolute maximum shear stress (tmax) reaches the stress that causes the material to yield in a simple tension test. The Maximum shear stress criterion is used for ductile materials.   tmax is the greatest of t12, t23 , t13 Where: t12 = (s1 – s2)/2; t23 = (s2- s3)/2; t13 = (s1- s3)/2 Hence: Factor of safety (FOS) =  slimit /(2*tmax)

THE MAXIMUM NORMAL STRESS CRITERION Also known as Coulomb’s criterion is based on the Maximum normal stress theory. According to this theory failure occurs when the maximum principal stress reaches the ultimate strength of the material for simple tension. This criterion is used for brittle materials. It assumes that the ultimate strength of the material in tension and compression is the same. This assumption is not valid in all cases. For example, cracks decrease the strength of the material in tension considerably while their effect is smaller in compression because the cracks tend to close. Brittle materials do not have a specific yield point and hence it is not recommended to use the yield strength to define the limit stress for this criterion. This theory predicts failure to occur when:   s1 ≥ slimit where s1 is the maximum principal stress. Hence: Factor of safety (FOS) = slimit  / s1

THE MOHR-COULOMB STRESS CRITERION Is based on the Mohr-Coulomb theory also known as the Internal Friction theory. This criterion is used for brittle materials with different tensile and compressive properties. Brittle materials do not have a specific yield point and hence it is not recommended to use the yield strength to define the limit stress for this criterion. This theory predicts failure to occur when:   s1 ≥ sTensileLimit  if s1 > 0 and s3 > 0 s3  ≥ - sCompressiveLimit  if s1  < 0 and s3 < 0 s1  / sTensileLimit + s3  / sCompressiveLimit < 1  if s1 ≥ 0 and s3  ≤ 0 The factor of safety is given by: Factor of Safety (FOS) = {s1 / sTensileLimit + s3  / sCompressiveLimit }(-1)

COMMON TYPES OF ANALYSES STRUCTURAL Linear static Nonlinear static Modal (frequency) Linear buckling THERMAL Steady state thermal Transient thermal

FINITE ELEMENT MESH

MESH COMPATIBILITY There is only one node here Compatible elements The same displacement shape function along edge 1 and edge 2 Incompatible elements Different displacement shape function along edge 1 and edge 2

MESH COMPATIBILITY Model of flat bar under tension. There is a mesh incompatibility along the mid-line between left and right side of the model. The same model after analysis. Due to mesh incompatibility a gap has formed along the mid-line.

Shell elements and solid elements combined in one model. MESH COMPATIBILITY Hinge Solid elements Shell elements Shell elements and solid elements combined in one model. Shell elements are attached to solid elements by links constraining their translational D.O.F. to D.O.F. of solid elements and suppressing their rotational D.O.F. This way nodal rotations of shells are eliminated and nodal translations have to follow nodal translations of solids. Unintentional hinge will form along connection to solids if rotational D.O.F. of shells are not suppressed.

MESH QUALITY Elements before mapping Elements after mapping

MESH QUALITY aspect ratio angular distortion ( skew ) angular distortion ( taper ) curvature distortion midsize node position warpage

MESH QUALITY Element distortion: aspect ratio Element distortion: warping

Element distortion: tangent edges MESH QUALITY Element distortion: tangent edges

MESH ADEQUACY Support Load This stress distribution needs to be modeled This stress distribution is modeled with one layer of first order elements

MESH ADEQUACY cantilever beam size: 10" x 1" x 0.1" modulus of elasticity: 30,000,000psi load: 150 lbf beam theory maximal deflection: f = 0.2" beam theory maximal stress:  = 90,000psi our definition of the discretization error : ( beam theory result - FEA result ) / beam theory result

Shell elements adequately model bending. MESH ADEQUACY Two layers of second order solid elements are generally recommended for modeling bending. Shell elements adequately model bending.

CONTROL OF DISCRETIZATION ERROR CONVERGENCE PROCESS CONTROL OF DISCRETIZATION ERROR

DISCRETIZATION OF STRESS DISTRIBUTION Mesh built with first order triangular elements called constant stress triangles Discrete stress distribution in constant stress triangles First order element assumes linear distribution of displacements within each element. Strain, being derivative of displacement, is constant within each element. Stress is also constant because it is calculated based on strain.

DISCRETIZATION OF STRESS DISTRIBUTION An isometric view of von Mises effective stress distribution in the upper right quarter of the model shown above. The height of bars represents the magnitude of stress. Notice that stresses are constant within each element. Tensile hollow strip modelled with a coarse mesh of 2D plate elements.

CONVERGENCE ANALYSIS BY MESH REFINEMENT The same tensile strip modelled three times with increasingly refined meshes. The process of progressive mesh refinement is called h convergence.

CHARACTERISTIC ELEMENT SIZE The process of progressive mesh refinement is called h convergence because characteristic element size h is modified during this process

CONVERGENCE CURVE Discretization errors Solution of the hypothetical “infinite” Finite element model (unknown) Solution error for model # 3 Convergence criterion Convergence error for model # 3 # of D.O.F. 1 2 3 Mesh refinement and / or element order upgrade number Discretization errors Discretization error is an inherent part of FEA. It is the price we pay for discretization of a continuous structure. Discretization error can be defined either as solution error or convergence error. Convergence error Convergence error is the difference between two consecutive mesh refinements and/or element order upgrade. Let’s say convergence error is 10%. If convergence takes place, then the next refinement and/or element order upgrade will produce results that will be different from the current one by less than 10%. Solution error The solution error is the difference between the results produced by a discrete model with a finite number of elements and the results that would be produced by a hypothetical model with an infinite number of infinitesimal elements. To estimate the solution error, one has to assess the rate of convergence and predict changes in results within the next few iterations as if they were performed.

COMPARISON BETWEEN h ELEMENTS AND p ELEMENTS The name h comes from characteristic element size usually denoted as h. That characteristic element size is reduced during h convergence process. p - elements The name p comes from polynomial function describing displacement field in the element. The order of polynomial function is increased during p convergence process.

COMPARISON BETWEEN h ELEMENTS AND p ELEMENTS Only tetrahedral elements can be reliably created with the available auto-meshers Only tetrahedral elements can be reliably created with the available auto-meshers Element shape: tetrahedral, wedge, hexahedral Element shape: tetrahedral, wedge, hexahedral Mapping allows for only little deviation from the ideal shape. Mapping allows for higher deviation from the ideal shape but may introduce errors on highly curved edges and surfaces Displacement field mapped by lower order polynomials (1st or 2nd), polynomial order does not change during solution Displacement field described by mapped higher order polynomials, polynomial order adjusted automatically to meet user’s accuracy requirements. results are produced in one single run with unknown accuracy results are produced in the iterative process that continues until the known, user specified accuracy, has been obtained many small elements typically 5,000 – 500,000 fewer large elements typically 500 – 10,000

HOLLOW PLATE Model file HOLLOW PLATE.sldprt Model type solid Material Alloy Steel Restraints fixed to left end face Load 100000N tensile load to right end face Objectives meshing solid CAD geometry using solid elements demonstrating h convergence process Fixed restraint 100,000 N tensile load