Chapter 2 Nonlinear Structural.

Chapter 2 Nonlinear Structural

Chapter Overview The following will be covered in this Chapter:
General Background on Nonlinear Theory Setting Up Nonlinear Analyses Metal Plasticity Solving Nonlinear Models Reviewing Results The capabilities described in this section are generally applicable to ANSYS Structural licenses and above. Exceptions will be noted accordingly February 4, 2005 Inventory #002177 2-2

A. Background on Linear Analysis
In Chapter 4 of the Workbench – Simulation Intro course, the assumptions and restrictions related to performing linear static structural analysis were covered: The matrix equation solved for is Hooke’s Law: Because [K] is assumed to be constant, essentially only linear behavior is allowed As shown on the figure on the right, if the force doubles, the displacement (and stresses) are assumed to double in linear analysis In many real-world situations, however, this small-displacement theory may not be valid. In these situations, nonlinear analysis may be required. K F x February 4, 2005 Inventory #002177 2-3

… Background on Nonlinear Analysis
There are three main sources of nonlinearities: Geometric nonlinearities: If a structure experiences large deformations, its changing geometric configuration can cause nonlinear behavior. Material nonlinearities: A nonlinear stress-strain relationship, such as metal plasticity shown on the right, is another source of nonlinearities. Contact: Include effects of contact is a type of “changing status” nonlinearity, where an abrupt change in stiffness may occur when bodies come into or out of contact with each other. February 4, 2005 Inventory #002177 2-4

In a nonlinear static analysis, the stiffness [K] is dependent on the displacement {x}: The resulting force vs. displacement curve may be nonlinear, as shown on the right, so doubling the force does not necessarily result in doubling of the displacements and stresses A nonlinear analysis is an iterative solution because this relationship between load (F) and response (x) is not known beforehand No time-dependent effects are considered. It is important to remember these assumptions related to performing nonlinear static analyses in Simulation. F x February 4, 2005 Inventory #002177 2-5

… Newton-Raphson Method
Nonlinear solutions require several iterations The actual relationship between load and displacement (shown with a yellow dotted line) is not known beforehand Consequently, a series of linear approximations with corrections is performed. This is a simplified explanation of the Newton-Raphson method (shown as solid red lines) In the Newton-Raphson Method, the total load Fa is applied in iteration 1. The result is x1. From the displacements, the internal forces F1 can be calculated. If Fa  F1, then the system is not in equilibrium. Hence, a new stiffness matrix (slope of red line) is calculated based on the current conditions. The difference of Fa - F1 is the out-of-balance or residual forces. The residual forces must be ‘small’ enough for the solution to converge. This process is repeated until Fa = Fi. In this example, after iteration 4, the system achieves equilibrium and the solution is said to be converged. Fa x 1 2 3 4 Newton-Raphson Method F1 x1 February 4, 2005 Inventory #002177 2-6

… Nonlinear Solution It is useful to understand how loads are managed
Load steps are changes in general loading. Simulation usually solves all nonlinear models with one load step, but, in the case of Pretension Bolt Loads, this is done in two load steps. The bolt preload is applied first, then all other loads are applied next. These load steps can be thought of as Fa and Fb. Substeps apply the loads in an incremental fashion Because of the complex response, it may be necessary to apply the load incrementally. For example, Fa1 may be near 50% of the Fa load. After the load for Fa1 is converged, then the full Fa load is applied. Fa has 2 substeps while Fb has 3 substeps in this example Equilibrium iterations are the corrective solutions to obtain a converged substep In the example on right, the iterations between the dotted white lines indicate equilibrium iterations. Fa xa Fb xb Fa1 Fb2 Fb1 February 4, 2005 Inventory #002177 2-7

In Simulation, the following types of nonlinear static structural analyses are directly available via the GUI: Large deflection effects Nonlinear contact (I.e. frictionless, frictional, no separation) Metal plasticity (Bi-linear or Multi-linear Isotropic Hardening). Many more advanced nonlinear features are not available directly in the Simulation interface. These items can be added with Command Objects Advanced Nonlinear material models (i.e. Creep, Hyperelasticity…) Nonlinear solution options, element formulations, and advanced contact options Advanced time-history postprocessing February 4, 2005 Inventory #002177 2-8

B. Nonlinear Analysis Setup
The procedure for nonlinear static analysis is very similar to performing a linear static analysis, so not all steps will be covered in detail. The steps in yellow italics include options that are specific to nonlinear analyses. Attach Geometry Assign Material Properties (with metal plasticity, if applicable) This will be covered in detail in Section C Define Contact Options (if applicable) Define Mesh Controls (optional) Include Loads and Supports Request Results Set Nonlinear Solution Options Solve the Model Review Results February 4, 2005 Inventory #002177 2-9

… Geometry (Solid Bodies)
Solid bodies are supported for large-deflection analyses with ANSYS Structural licenses and above. Advanced users can change the “Brick Integration Scheme” from “Full” to “Reduced,” which may be useful for large-deformation problems. ANSYS Details: In Simulation, the following elements are used: Solid bodies are meshed with 10-node tetrahedral or 20-node hexahedral elements SOLID187 and SOLID186 SOLID186 has KEYOPT(3)=2 by default in Simulation. If “Brick Integration Scheme” under the part Details view is changed from “Full” to “Reduced,” then KEYOPT(3)=0 is used. The latter is the default option in ANSYS, and is useful to alleviate volumetric locking. Surface bodies are meshed with 4-node quad shell elements SHELL181 using real constants Section definition (and offsets) are not used Line bodies are meshed with 2-node beam elements BEAM188 (with 3rd orientation node) Section definition and offsets are supported February 4, 2005 Inventory #002177 2-10

… Geometry (Line/Surface Bodies)
ANSYS Professional licenses and above support large- deformation analyses with surface or line bodies. Note that ANSYS Professional does not support a combination of line and surface bodies. ANSYS Structural and above must be used in these cases. February 4, 2005 Inventory #002177 2-11

… Solid Body Contact Options
All of the contact options available in linear static analyses are also available for nonlinear, large-deflection analyses in ANSYS Structural licenses and above: In general, face-to-face contact for solid bodies is the only type of contact which supports advanced nonlinear options Most other contact involving surface bodies or solid edges support bonded (and no separation) contact only February 4, 2005 Inventory #002177 2-12

… Meshing Controls Meshing considerations are usually the same in nonlinear analyses. However, if large strains are expected, the shape checking option may be changed to “Aggressive” For large-deflection analyses, if elements may undergo some change in shape, this may reduce the fidelity of the solution By using “Aggressive” shape checking, Simulation will ensure that the element quality is much better prior to solution in order to anticipate distortion of the element in the course of a large-strain analysis. The quality of the “Standard” shape checking is suitable for linear analyses, so it does not need to be changed in linear analyses With “aggressive” shape checking set, some mesh failures may be more likely. See Ch. 3 from the Workbench Simulation - Intro course for some ways to detect and remedy mesh failures. Simulation meshes in ANSYS: The “Shape Checking” toggle is SHPP,LSTET,ON Use of Jacobian tests at integration points is the “Standard” or SHPP,LSTET,ON method, suitable for linear analyses Use of Jacobian tests at corner nodes is the “Aggressive” or SHPP,LSTET,OFF method. This is generally a more conservative approach and may be preferred for nonlinear analyses. This is because elements which undergo distortion during solution should have a good quality shape to begin with. Because Simulation uses its own criteria for shape tests, SHPP,OFF is set when exporting a mesh to ANSYS. Also, even if SHPP,ON is set, the criteria used for warning/error elements differs between Simulation and ANSYS February 4, 2005 Inventory #002177 2-13

… Loads and Supports Most loads and supports used in linear analyses may also be used in large-deflection analyses Thermal-stress analyses are supported for large-deflection analyses. See Chapter 6 of the Workbench – Simulation Intro course on details of performing thermal analyses ANSYS Structural licenses do not support any thermal loads Recall that ANSYS Professional does not support large-deflection analyses for solid bodies Two unique items for loads and supports in large-deflection analyses will be covered next Orientation of loads for large-deflection Pretension Bolt Load February 4, 2005 Inventory #002177 2-14

Direction Before Deflection Direction After Deflection
… Load Orientation It is important to note the orientation of loads and its effect on the structure in large-deflection analyses: Load Direction Before Deflection Direction After Deflection Acceleration (constant direction) Force, Moment, Bolt Load (constant direction) Pressure (always normal to surface) February 4, 2005 Inventory #002177 2-15

… Pretension Bolt Load A Pretension Bolt Load is available in ANSYS Structural Pretension Bolt Load is applied on a single cylindrical surface Each load must be applied to only one set of cylindrical surface(s) For multiple loads, add separate Pretension Bolt Loads branches Usually, a preload value is input in the Details view If the torque is known, this can be converted to a preload force If known, an initial adjustment can be directly applied Internally, preloads are applied in two steps The preload value is applied first, which shortens the grip length The grip length is then fixed, and any other loads are then applied February 4, 2005 Inventory #002177 2-16

… Pretension Bolt Load A Pretension Bolt Load is useful to account for the effect of the preload in bolts, which is caused by their tightening The loss of preload and the effect the preload has on contact regions can be included in this manner, enabling for more complex simulation of real-world assemblies. Contact options for parts connected with fasteners should be set separately in the Contact branch. The Pretension Bolt Load only controls the load on the cylindrical surface representing the bolt. The adjustment or preload is applied in two steps. In real life, if the fastener is tightened, its grip length changes. Simulation mimics this the same way by first applying only the preload or adjustment. If the preload is defined, the adjustment (shortening of the grip length) is calculated. The given or calculated adjustment shortens the grip length of the bolt. All other external loads are then applied in the second load step, once the grip length is shortened. ANSYS Details: The Pretension Bolt Load is modeled with PRETS179 The solid mesh is split near the centroid of the solid body representing the bolt with the PSMESH command. A local coordinate system 11 is temporarily created to aid in automatically generating the PRETS179 elements based on the elements of the selected cylindrical surface. If user-defined Coordinate Systems are present, these will still be translated properly, as local coordinate systems are defined after the PRETS179 elements are generated. Visually verify that the mesh has nodes near the centroid of the body. Otherwise, the PRETS179 elements may be created too far above or below and may be affected by other contact or boundary conditions (see example below): February 4, 2005 Inventory #002177 2-17 In this example, if the nut is bonded to the bolt, the generated PRETS179 elements (solid lines) will not work as expected.

… Pretension Bolt Load In large-deflection analyses, the orientation of the Pretension Bolt Load is not updated The Pretension Bolt Load should not be applied on any part that undergoes large rotation The Pretension Bolt Load is applied in the center of the solid body containing the cylindrical surface Verify the mesh, and ensure that no constraints or bonded contact is present near the center of the ‘bolt’ solid body. Otherwise, the preload may be overconstrained. The Adjustment and Working Load can be reviewed After the solution, in the Details view, the adjustment caused by the preload is shown. Also, the working load is provided, so the user can determine how much preload was lost. ANSYS Details: Adjustments are directly applied to PRETS179 node K with the D command while loads are applied with the F command The SLOAD command is not used when applying loads to the PRETS179 element. Definition of a multiple pretension loading sequence is not possible. All pretension elements are loaded in the first load step. External loads (except for temperatures) are applied in the first load step. However, they are scaled with FSCALE and SFSCALE commands to 1e-12 of their value. After the preload/adjustment is applied and solved for in the first load step, the external loads are scaled back by 1e12. If present, the pretension force is removed, and the current adjustment is step-applied with the D command (using %_FIX% value). Temperature loading, if present, is applied with BF command Although a known adjustment requires only one load step, two load steps are still used when any Pretension Bolt Load is present The Adjustment and Working Load information is also available in the Worksheet tab of the Environment branch February 4, 2005 Inventory #002177 2-18

C. Metal Plasticity What is plasticity?
When a ductile material experiences stresses beyond the elastic limit, it will yield, acquiring large permanent deformations. Plasticity refers to the material response beyond yield. Plastic response is important for metal forming operations. Plasticity is also important as an energy-absorbing mechanism for structures in service. Materials that fail with little plastic deformation are said to be brittle. Ductile response is safer in many respects than is brittle response. This section will review some basics of plasticity by defining certain terminology. February 4, 2005 Inventory #002177 2-19

… Elasticity Review of Elasticity:
Before proceeding to a discussion on plasticity, it may be useful to review elasticity of metals. In elastic response, if the induced stresses are below the material’s yield strength, the material can fully recover its original shape upon unloading. From a standpoint of metals, this behavior is due to the stretching but not breaking of chemical bonds between atoms. Because elasticity is due to this stretching of atomic bonds, it is fully recoverable. Moreover, these elastic strains tend to be small. Elastic behavior of metals is most commonly described by the stress-strain relationship of Hooke’s Law: February 4, 2005 Inventory #002177 2-20

… Plasticity Review of Plasticity:
Plastic deformation results from slip between planes of atoms due to shear stresses (deviatoric stresses). This dislocation motion is essentially atoms in the crystal structure rearranging themselves to have new neighbors results in unrecoverable strains or permanent deformation after load is removed. slipping does not generally result in any volumetric strains (condition of incompressibility), unlike elasticity   Yield Strength sy Elastic Plastic Unloading February 4, 2005 Inventory #002177 2-21

… Rate-Independent Plasticity
If the material response is not dependent on the rate of loading or deformation, the material is said to be rate- independent. Most metals exhibit rate-independent behavior at low temperatures (< 1/4 or 1/3 melting temperature) and low strain rates. Engineering vs. True Stress-Strain: While engineering stress-strain can be used for small-strain analyses, true stress-strain must be used for plasticity, as they are more representative measures of the state of the material. February 4, 2005 Inventory #002177 2-22

… True Stress and Strain
Engineering vs. True Stress-Strain (cont’d): If presented with engineering stress-strain data, one can convert these values to true stress-strain with the following approximations: Up until twice the strain at which yielding occurs: Up until the point at which necking occurs: Note that, only for stress conversion, the following is assumed: Material is incompressible (acceptable approximation for large strains) Stress distribution across cross-section of specimen is assumed to be uniform. Beyond necking: There is no conversion equation relating engineering to true stress-strain at necking. The instantaneous cross-section must be measured. February 4, 2005 Inventory #002177 2-23

… Yield Criterion (Yield Point)
The yield criteria is used to relate multiaxial stress state with the uniaxial case. Tensile testing on specimens provide uniaxial data, which can easily be plotted on one-dimensional stress-strain curves, such as those presented earlier in this section. The actual structure usually exhibits multiaxial stress state. The yield criterion provides a scalar invariant measure of the stress state of the material which can be compared with the uniaxial case. A common yield criterion is the von Mises yield criterion (also known as the octahedral shear stress or distortion energy criterion). The von Mises equivalent stress is defined as: February 4, 2005 Inventory #002177 2-24

… Mises Yield Criterion
If plotted in principal stress space, the von Mises yield surface is a cylinder. Inside the yield surface, as noted earlier, behavior is elastic. Note that the multiaxial stress state can exist anywhere inside of the cylinder. At the edge of the cylinder (circle), yielding will occur. No stress state can exist outside of the cylinder. Instead, hardening rules will describe how the cylinder changes with respect to yielding. e Elastic Plastic 3 2 1  sy Principal Stress Space Uniaxial Stress-Strain February 4, 2005 Inventory #002177 2-25

… Hardening Rules Hardening Rules:
The hardening rule describes how the yield surface changes (size, center,shape) as the result of plastic deformation. The hardening rule determines when the material will yield again if the loading is continued or reversed. This is in contrast to elastic-perfectly-plastic materials which exhibit no hardening -- i.e., the yield surface remains fixed. Elastic Plastic Yield Surface after Loading Initial Yield Surface February 4, 2005 Inventory #002177 2-26

… Isotropic Hardening Isotropic Hardening:
Isotropic hardening states that the yield surface expands uniformly during plastic flow. The term ‘isotropic’ refers to the uniform dilatation of the yield surface and is different from an ‘isotropic’ yield criterion (i.e., material orientation). e 3 2 1  2s' sy s' Initial Yield Surface Subsequent Yield Surface February 4, 2005 Inventory #002177 2-27

… Isotropic Hardening  ’ y 2s’ 
Plotting the stress-strain curve enables an understanding of what occurs during a loading and reverse loading cycle:  ’ y 2s’  Note that the subsequent yield in compression is equal to the highest stress attained during the tensile phase. Isotropic hardening is often used for large strain or proportional loading simulations. It is usually not applicable cyclic loading. February 4, 2005 Inventory #002177 2-28

… Stress-Strain Curve Representation
Curve shapes Two different type of stress-strain curve representations are possible:   Bilinear Multilinear February 4, 2005 Inventory #002177 2-29

… Summary of Plasticity in Simulation
In Simulation, metal plasticity can be included as part of the model. The following points should be remembered: Metal plasticity deals with elastic and inelastic (permanent) deformation. Inelastic or plastic deformation occurs when the stress is higher than the yield strength. There will always be some recoverable strain (elastic strain) upon unloading. A stress-strain curve is based on scalar data, usually from a uniaxial test. A system may undergo a multiaxial stress state, so Simulation uses the Mises yield criterion to relate a multiaxial stress state with scalar test data. In this situation, true stress vs. strain data should be supplied. After yielding occurs, the yield point may increase due to strain hardening. This changes the yield surface, and the way in which it evolves in Simulation is determined by isotropic hardening assumption. The stress-strain curve can be represented by a bilinear or multilinear curve. February 4, 2005 Inventory #002177 2-30

… Material Properties Linear elastic material properties must be supplied The same requirements exist for linear static structural analyses, namely that Young’s Modulus and Poisson’s Ratio must be defined as a minimum. Metal plasticity is available as a nonlinear material model. This will be discussed next. Other nonlinear constitutive models may be added with the Preprocessing Command Builder However, note that only ANSYS Structural licenses and above support nonlinear material laws. ANSYS Professional supports large-deflection analyses of surface or line bodies, but it does not support any material nonlinearities February 4, 2005 Inventory #002177 2-31

… Metal Plasticity To add metal plasticity, first navigate to the specific part or parts under the geometry branch. In the Details window, highlight the material you wish to modify February 4, 2005 Inventory #002177 2-32

… Metal Plasticity Right side of the Engineering Data application shows the currently defined properties. Choose “Add/Remove Properties” to continue. February 4, 2005 Inventory #002177 2-33

… Metal Plasticity Select either “Bilinear” or “Multilinear Isotropic Hardening” under “Nonlinear > Plasticity”. Multilinear representation usually provides a more accurate description of stress-strain curve than Bilinear. February 4, 2005 Inventory #002177 2-34

… Metal Plasticity To enter or modify the plasticity definition click either chart icons for the property. Chart Icons To return to the general material property display use the “Close Curve” icon. February 4, 2005 Inventory #002177 2-35

… Bilinear Stress-Strain
The Bilinear Stress-Strain requires two input values: The “Yield Strength” and “Tangent Modulus” is input in the Details view. The yield strength is the value at which plastic straining occurs. The tangent modulus is the slope of the stress-strain curve after yielding. As the name implies, the “Bilinear Stress-Strain” provides a simple representation of metal plasticity February 4, 2005 Inventory #002177 2-36

… Multilinear Stress-Strain
The Multilinear Stress-Strain allows stress-strain input: Right-click on the spreadsheet to add rows Input as many Strain and Stress values as needed The stress-strain plot will be displayed dynamically The origin (0,0) should be the first point. Also, ensure that the second point has the same slope as the Young’s modulus. Simulation assumes perfect plasticity (zero slope) beyond the defined stress-strain values. February 4, 2005 Inventory #002177 2-37

Large Deflection with Metal Plasticity
Workshop 2A Large Deflection with Metal Plasticity

D. Workshop 2A – Metal Plasticity
Goal Compare and contrast results using small deflection, large deflection and large deflection with metal plasticity on a model with identical loads and boundary conditions. Model Description 3D large deflection of spring plate Spring plate Ductile steel Loads and Boundary Conditions: Fixed support 3 Mpa Pressure load at opposite end February 4, 2005 Inventory #002177 2-39

… Workshop 2A – Metal Plasticity
Steps to Follow: Start an ANSYS Workbench session. Browse for and open “Spring_ws01.wbdb” project file. This project contains a Design Modeler (DM) geometry file “Spring_ws01.agdb” and a Simulation (S) file “Spring_ws01.dsdb”. Highlight the the Model, Small Deflection-Linear Mat’l (Spring_ws01.dsdb) file and open a Simulation Session. February 4, 2005 Inventory #002177 2-40

Review the contents of the model Highlight geometry “Solid” branch and examine the Details of “Solid ”Window (lower left corner of screen). Note we will start with a structure steel and Nonlinear Material Effects off. The boundary conditions and load (3Mpa Pressure) have already been defined. Highlight the “Solution” branch. Note: We accept the default settings, including Large Deflection “Off” February 4, 2005 Inventory #002177 2-41

Add a Solution Information Folder to the Solution Branch Run the Solution Solution, RMB SOLVE After solution run is complete, open the Solution Information folder and scroll to near the bottom of the output. As expected, this solves in one iteration. February 4, 2005 Inventory #002177 2-42

Review the displacement and stress results from this first run. February 4, 2005 Inventory #002177 2-43

Highlight the “Small Deflection- Linear Mat’l” Branch at the top of the Project Tree, and duplicate this Branch with RMB=> Duplicate. Change the new branch name to “Large Deflection - Linear Mat’l” Highlight Solution Branch and turn Large Deflection “ON” The Project tree should look as shown in figure to the right. Execute a Solve on this new Solution… February 4, 2005 Inventory #002177 2-44

After solution run is complete, open the Solution Information folder and scroll to near the bottom of the output. Note the solution still solves in one substep, but 9 iterations were made on the stiffness matrix during the run to account for large deflection effects. Change Solution Output to Force Convergence to review the Newton-Raphson History. February 4, 2005 Inventory #002177 2-45

Review the large deflection analysis displacement and stress results and compare with the first run. Note: Total Deformation is larger, but max equivalent stress is actually slightly lower and in a different location then the linear run. Extra Credit: To better understand the differences, try post processing x and y deflections and equivalent strains separately for both runs. Note the dramatic increase in the y deflections especially and the different distributions of strain energies. February 4, 2005 Inventory #002177 2-46

Highlight the “Large Deflection- Linear Mat’l” Branch and duplicate this Branch with RMB=> Duplicate. Change the new branch name to “Large Deflection-NonLinear Mat’l” Add metal plasticity: Highlight Geometry “Solid” branch Activate Nonlinear material effects (YES) RMB on Structural Steel Select Edit Structural Steel… Select “Add/Remove Properties” Activate Bilinear Isotropic Hardening Plasticity [OK] February 4, 2005 Inventory #002177 2-47

Click on the ICON to the right of Bilinear Isotropic Hardening Define Yield Strength of 250Mpa and a Tangent Modulus of 10000Mpa. Select “Close Curve” Return to project tree and execute a solve on this latest Solution February 4, 2005 Inventory #002177 2-48

This last solution run can take up to two minutes depending on machine. Review the Solution Convergence History as before. It now takes 42 iterations in eight substeps, including two bisections. February 4, 2005 Inventory #002177 2-49

Review the displacement and stress results and compare with the large deflection run. Note: Total Deformation is considerably larger and stresses come down due to the dramatic loss of stiffness as part goes plastic. February 4, 2005 Inventory #002177 2-50

Add Equivalent Plastic Strain to the solution branch for a better picture of where most of the yielding occurs. February 4, 2005 Inventory #002177 2-51

E. Solving Nonlinear Models
The solution options for nonlinear analyses are the same for linear analyses. However, for large-deflection problems, the user has an additional option of turning on “Large Deflection” Use of the Large Deflection option accounts for changes in the geometry during the course of the analysis. ANSYS Professional only supports large-deflection analyses for surface or line bodies. The Newton-Raphson method is employed in nonlinear solutions (see next slides) February 4, 2005 Inventory #002177 2-52

… Nonlinear Solution Simulation automates nonlinear solutions by automatically determining the number of load steps, substeps, and equilibrium iterations In this way, the user does not have to worry about these settings. However, as will be shown later, it is very useful to understand these concepts in dealing with nonlinear solutions During the course of the analysis, if Simulation has trouble converging, it will bisect the solution. This means that Simulation will apply the load in smaller increments (more substeps). This usually helps for difficult problems since the response will be easier to converge if a smaller load is applied. The final, total load will be solved for in the end. February 4, 2005 Inventory #002177 2-53

… Nonlinear Solution The number of load steps is usually set to 1
If Pretension Bolt Loads are present, there will be 2 load steps For thermal-stress analyses, the thermal analysis is performed first as a separate analysis. Hence, this part is not considered a load step since it is a different type of analysis. The initial number of substeps is usually set to 1 If frictional contact with a Friction Coefficient  0.2 is present, this results in 5 initial substeps The max number of equilibrium iterations is usually around 20 The type of contact will dictate the maximum number of equilibrium iterations If a substep cannot be converged within the specified number of equilibrium iterations, Simulation will bisect the solution. It will apply half of the current load and run equilibrium iterations again to converge. Usually, this is repeated until 10% of the load is applied. If the solution still does not converge, Simulation will stop and produce an error message. February 4, 2005 Inventory #002177 2-54

… Nonlinear Solution Auto Time Stepping specifications can be changed within Simulation in the Details of Solution Window: Change Auto Time Stepping from “Program Controlled” to “On” Manually define the initial, minimum and maximum values. February 4, 2005 Inventory #002177 2-55

… Nonlinear Solution Output
Nonlinear solution output from the ANSYS solver is requested with the “Solution Information” branch When requested, the “Solution Information” branch may be used to display Solver Output or Force Convergence progress, among a number of other options from the pull-down menu The “Update Interval” allows users to specify (in seconds) how frequency this output is updated The “Solver Output” and “Force Convergence” provide details on the nonlinear solution progress. February 4, 2005 Inventory #002177 2-56

… Nonlinear Solver Output
Nonlinear solutions, especially those dealing with frictionless or frictional contact, can be difficult to solve During the solution, it is useful to become familiar with reading the ANSYS solver output In the “Solution Information” branch, informative messages about the solution, solver, and contact settings are usually printed first when solution is initiated It may be useful to browse through the contact information (sample below) to ensure that initial gaps or initial penetration is not very large. If an initial gap is automatically closed, this will also be printed in the output. In this example, the initial penetration 7e-5 may be very small compared to the dimensions of the model, so it can be ignored. These small values of penetration or gaps may be caused by the mesh discretization. February 4, 2005 Inventory #002177 2-57

As the nonlinear solution progresses, the equilibrium iteration information is shown (sample below) Note that for each equilibrium iteration, the residual forces (FORCE CONVERGENCE VALUE) must be lower than the CRITERION Ideally, the residual or out-of-balance forces should be zero for a system to be in equilibrium. However, because of machine precision and practical concerns, Simulation determines a value small enough to result in negligible error. This value is the CRITERION, and the FORCE CONVERGENCE VALUE must be smaller than the CRITERION for the substep to be converged. In the example below, after 3 equilibrium iterations, the residual forces are lower than the criterion, so the solution is converged. Informative messages (such as convergence or bisection) are noted with “>>>” and “<<<“ in the output. February 4, 2005 Inventory #002177 2-58

By understanding how to read the solution output, potential problems can be detected early on In the contact output below, there are notes of initial penetration and initial gaps. One should always verify automatically-generated contact regions The improper specification of contact may cause convergence difficulties, so reading the contact output would be helpful in determining if any contact region is problematic Initial penetration/gaps are reported in active length units February 4, 2005 Inventory #002177 2-59

During the equilibrium iterations, reviewing the pattern of the residual forces will help determine if a solution is diverging In the example below, the residual forces (FORCE CONVERGENCE VALUE) initially decreases but then starts to increase dramatically. In this situation, the user can abort the solution and check his/her model to see what caused the high residual forces. Otherwise, Simulation may continue for several more iterations (and even bisect the solution) until it diverges, which would take longer. Some causes of high residual forces include excessively large loading (verify units), high contact stiffness (especially for thin, bending-dominated behavior), or high friction coefficient values. February 4, 2005 Inventory #002177 2-60

Warning and error messages will also be printed in the output When contact status changes abruptly, this is just a warning indicating that the contact elements enter or exit the ‘pinball region’ drastically. This may be due to parts sliding or separating drastically if the load is too high. Simulation may automatically bisect the solution, if necessary. Element distortion messages are usually severe problems due to excessive loading or over-constraints. Bisection of the load is automatically performed, but sometimes corrective measures may need to be taken to fix the problem. February 4, 2005 Inventory #002177 2-61

… Nonlinear Force Convergence
The Solver Output option shows detailed text information. If “Solution Output” is changed to “Force Convergence,” the force convergence behavior is shown graphically: Text Output Graphical Output February 4, 2005 Inventory #002177 2-62

… Nonlinear Force Convergence
The Force Convergence view shows what the force criterion and residual forces (“force convergence”) are. When the residual forces are less than the criterion, the substep is assumed to be converged. Additional useful features include the fact that converged substeps and loadsteps are also indicated on the chart with a green and blue dotted line, respectively. For this model, because Pretension Bolt Loads are present, it is a two-load step analysis. “Time” is the same as load step number in this case. The current “time” is 1.2, so it is 20% complete with the second load step. February 4, 2005 Inventory #002177 2-63

… Results Tracker Besides monitoring the out-of-balance forces, a Results Tracker is available from the “Solution Information” branch The Results Tracker enables users to monitor deformation at a vertex and/or contact region information during the solution. For “Results Tracker > Deformation,” select a vertex of interest and specify whether x, y, or z deformation is to be monitored. For “Results Tracker > Contact,” a pull-down menu enables users to select a contact region. Then, the quantity to track (such as number of contacting elements) can be displayed. February 4, 2005 Inventory #002177 2-64

… Results Tracker After the Results Tracker items are requested and solution initiated, users may “track” the deformation or contact results during the course of the solution. In this example, the number of contacting elements is monitored for a particular contact region. As is apparent in the graph on right, between Time=1.4 and 1.7, the number of contacting elements jumps from zero to 29. Since “Time” is a “placeholder” in a nonlinear static analysis, this means that, after the first load step (Time=1.0), between 40% and 70% of the load, contact is established. February 4, 2005 Inventory #002177 2-65

… Nonlinear Solution It is the user’s responsibility to determine whether or not large deformation effects are significant and need to be considered. Simulation has some basic checks after the solution, where if the deformation is large compared to the overall geometry size, the warning below will appear: This, however, occurs for obvious, exaggerated cases. It does not mean that if the warning does not appear in a linear analysis that large deformation effects may not be significant. February 4, 2005 Inventory #002177 2-66

… Newton-Raphson Residuals
As emphasized earlier, the Newton-Raphson method employs multiple iterations until force equilibrium is achieved. For debugging purposes, it may be useful to request the Newton-Raphson Residuals (i.e., residual forces) to see what locations have high residuals which may be the cause of force equilibrium not being satisfied. In the “Solution Information” details view, enter the number of equilibrium iterations to retrieve Newton-Raphson Residuals. For example, if “3” is entered, the residual forces from the last three iterations will be returned if the solution is aborted or does not converge. February 4, 2005 Inventory #002177 2-67

… Newton-Raphson Residuals
After solution is stopped or fails to converge, residuals will be available under the “Solution Information” branch, as shown below. If a solution fails to converge or is aborted by the user, the requested number of residuals will be available. By looking at the residuals, one can example at which locations out-of-balance forces are high. This helps users identify possible problematic locations, so that corrective action may be taken. February 4, 2005 Inventory #002177 2-68

F. Reviewing Results Requesting and reviewing results are similar to linear static structural analyses In large deformation problems, one usually should view the deformation with “Actual” scaling from the Result toolbar Any of the structural results may be requested, such as Equivalent Stress, shown below February 4, 2005 Inventory #002177 2-69 Model shown is from a sample Unigraphics assembly.

… Reviewing Results - Equivalent Plastic Strain
If plasticity is defined, equivalent plastic strain can be requested as output (example shown below) Total equivalent strain is the sum of equivalent elastic and equivalent plastic strain. Total equivalent strain is used to correlate to the stress-strain curve. February 4, 2005 Inventory #002177 2-70

… Reviewing Results Animations of nonlinear solutions linearly increase from zero to the final value The actual load history is not accounted for in the animation If Pretension Bolt Loads are present, only the second load step (externally applied loads after adjustment) is animated, as shown in the example below This model has Pretension Bolt Loads applied on the three bolts. Although the solution consisted of two load steps simulating the assembly and loading processes, only the final result is animated. This final result is animated in a linear fashion from zero to the final value. The actual load history is not contained in the animation (i.e., if multiple substeps were solved for, they are not included in the animation) February 4, 2005 Inventory #002177 2-71

Bolt Pretension with Contact
Workshop 2B Bolt Pretension with Contact

G. Workshop 2B – Goals Goal:
In this workshop our goal is to investigate the behavior of the pipe clamp assembly (Pipe_clamp.x_t) shown here. Specifically we wish to determine the crushing stress and deformation in a copper pipe section when the bolt in the clamp is torqued down. February 4, 2005 Inventory #002177 2-73

. . . Workshop 2B – Assumptions
We will assume the material used for the pipe is a copper alloy while all other parts are steel. It is assumed the clamp is torqued to 1000 N when placed in service. We’ll assume the coefficient of friction between the clamp and pipe is The other contact regions will be treated as either bonded or no separation as shown in the accompanying figures. February 4, 2005 Inventory #002177 2-74

. . . Workshop 2B - Start Page From the launcher start Simulation.
Choose “Geometry > From File “ and browse to the file “Pipe_clamp.x_t”. When Workbench Simulation starts, close the Template menu by clicking the ‘X’ in the corner of the window. February 4, 2005 Inventory #002177 2-75

. . . Workshop 2B – Preprocessing
Change the working unit system to metric mm. “Units > Metric (mm, kg, MPa, C, s)” Insert the material “Copper Alloy” from the material library. Highlight the “Part 2” in the geometry branch (pipe). Click in the “Material” field and “Import…”. 1. 2. 3. February 4, 2005 Inventory #002177 2-76

Select “Copper Alloy” material. 4. February 4, 2005 Inventory #002177 2-77

Expand the “Contact” branch and use the shift key to highlight all contact definitions. In the details window change the Formulation to “Augmented Lagrange. 5. 6. February 4, 2005 Inventory #002177 2-78

Highlight the first contact branch. This is the definition for the pipe to clamp contact. In the detail for the definition change the Type to “Frictional”. Enter a value for “Friction Coefficient” of 0.4. 7. 8. 9. February 4, 2005 Inventory #002177 2-79

Highlight the second contact branch. This is the definition for the bolt shaft to clamp hole contact. From the details window change the Type to “No Separation”. The remaining 2 contact regions will be modeled using the default bonded type of contact. 10. 11. February 4, 2005 Inventory #002177 2-80

Create a local coordinate system along the pipe’s axis. Note, we will use the local coordinate system for post processing later. Highlight the Model branch. “RMB > Insert > Coordinate Systems”. Notice the result is a new branch “Coordinate Systems” appears in the tree. Also, the “Global Coordinate System” is automatically placed in the branch. 12. 13. February 4, 2005 Inventory #002177 2-81

With the Coordinate system branch highlighted: Select the inside surface of the cylinder. “RMB > Insert > Coordinate System”. 14. 15. February 4, 2005 Inventory #002177 2-82

From the detail for the new coordinate system change “Type” to “Cylindrical”. “Click to Change” in the “Z Direction” field to change the system’s orientation. Select the inner surface of the pipe. “Apply” in the detail window. 16. 17. 18. 19. February 4, 2005 Inventory #002177 2-83

. . . Workshop 2B - Environment
Highlight the Environment branch. Select one of the end surfaces of the pipe. RMB > Insert > Fixed Support. 20. 21. 22. February 4, 2005 Inventory #002177 2-84

. . . Workshop 2B - Environment
Select the cylindrical face of the bolt part. “RMB > Insert > “Bolt” In the detail for the pretension bolt load enter a “Preload” value of 1000. 23. 25. February 4, 2005 Inventory #002177 2-85

. . . Workshop 2B – Solution Setup
Highlight the solution branch. RMB > Insert > Stress > Equivalent (von Mises). RMB > Insert > Deformation > Total. 26. 27. 28. February 4, 2005 Inventory #002177 2-86

Switch to “Body” select mode. Select the pipe part. 29. 30. February 4, 2005 Inventory #002177 2-87

“RMB > Insert > Deformation > Directional”. From the detail for the “Directional Deformation” change to “Coordinate System”. Note we allowed the default name “Coordinate System” to be used when the local system was created. We could easily change the name to a more meaningful one. 31. 32. February 4, 2005 Inventory #002177 2-88

Switch to face select mode. Highlight the outer surface of the pipe. “RMB > Insert > Contact Tool > “Pressure”. Repeat steps 34 and 35 inserting contact “Frictional Stress”. Solve 33. 34. February 4, 2005 Inventory #002177 2-89

. . . Workshop 2B – Solution Notes
The solution for this workshop will take several minutes or more depending on the available hardware. The use of frictional contact triggers a nonlinear solution requiring equilibrium iterations. The solution progress can be viewed by inserting the “Solution Information” object. The use of the pretension bolt load also causes 2 solutions to be run. The first applies the pretension load and locks it down. The second applies any remaining loads. February 4, 2005 Inventory #002177 2-90

. . . Workshop 2B - Results Recall that the solution triggered the use of “Weak Spring” stabilization. To insure that the weak springs are not the result of rigid body motion, highlight the Environment branch and inspect the weak spring reaction forces. Here we can see that the reaction in the weak springs is of the order e-5, a negligible value. February 4, 2005 Inventory #002177 2-91

. . . Workshop 2B - Results Highlighting and plotting the “Total Deformation” for the assembly shows the plot is not particularly useful for our goal (investigation of pipe’s behavior). The “scoped” result we placed in the solution branch will be more instructive. February 4, 2005 Inventory #002177 2-92

. . . Workshop 2B - Results Highlight and plot the result “Directional Deformation”. In this case the result is scoped only to the pipe section. Also, since we employed a local cylindrical system at the pipe axis, the X direction here is displayed in the radial sense. February 4, 2005 Inventory #002177 2-93

. . . Workshop 2B - Results Similarly, the behavior of the contact region can be view by highlighting the contact result objects. Again the use of scoped results allows a more intuitive plot of the quantity displayed. February 4, 2005 Inventory #002177 2-94

Chapter 2 Nonlinear Structural.

Similar presentations

Presentation on theme: "Chapter 2 Nonlinear Structural."— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

Chapter 2 Nonlinear Structural.

Similar presentations

Presentation on theme: "Chapter 2 Nonlinear Structural."— Presentation transcript:

Similar presentations

About project

Feedback