1 / 94

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

susanhenderson
Download Presentation

Nonlinear Structural

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Chapter 2 Nonlinear Structural

  2. 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

  3. F K x 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 theforce 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. February 4, 2005 Inventory #002177 2-3

  4. … 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 onthe right, is another source of nonlinearities. • Contact: Include effects of contact is a typeof “changing status” nonlinearity, where anabrupt change in stiffness may occur whenbodies come into or out of contact with eachother. February 4, 2005 Inventory #002177 2-4

  5. F x … Background on Nonlinear Analysis • In a nonlinear static analysis, the stiffness [K] is dependent on the displacement {x}: • The resulting force vs. displacement curvemay be nonlinear, as shown on the right, sodoubling the force does not necessarilyresult in doubling of the displacementsand stresses • A nonlinear analysis is an iterative solutionbecause 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 staticanalyses in Simulation. February 4, 2005 Inventory #002177 2-5

  6. Newton-Raphson Method Fa 4 3 2 F1 1 x1 x … 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 totalload Fa is applied in iteration 1. The resultis x1. From the displacements, the internalforces F1 can be calculated. If Fa F1, thenthe system is not in equilibrium. Hence,a new stiffness matrix (slope of red line) iscalculated based on the current conditions.The difference of Fa- F1 is the out-of-balanceor residual forces. The residual forces mustbe ‘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. February 4, 2005 Inventory #002177 2-6

  7. Fb Fb2 Fb1 Fa Fa1 xa xb … 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, itmay be necessary to apply the loadincrementally. For example, Fa1 may benear 50% of the Fa load. After the loadfor Fa1 is converged, then the full Fa loadis applied. Fa has 2 substeps while Fbhas 3 substeps in this example • Equilibrium iterations are the correctivesolutions to obtain a converged substep • In the example on right, the iterations between the dotted white lines indicate equilibrium iterations. February 4, 2005 Inventory #002177 2-7

  8. … Background on Nonlinear Analysis • 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

  9. 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

  10. … 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. February 4, 2005 Inventory #002177 2-10

  11. … 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

  12. … 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

  13. … 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 andremedy mesh failures. February 4, 2005 Inventory #002177 2-13

  14. … 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

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

  16. … 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

  17. … 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. February 4, 2005 Inventory #002177 2-17

  18. … 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. The Adjustment and Working Load information is also available in the Worksheet tab of the Environment branch February 4, 2005 Inventory #002177 2-18

  19. 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

  20. … 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

  21. Yield Strength sy Unloading  Elastic Plastic … 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 February 4, 2005 Inventory #002177 2-21

  22. … Rate-Independent Plasticity 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

  23. … 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

  24. … Yield Criterion (Yield Point) Yield Criterion: • 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

  25. 1  Plastic sy e Elastic 2 3 Principal Stress Space Uniaxial Stress-Strain … 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. February 4, 2005 Inventory #002177 2-25

  26. Plastic Yield Surface after Loading Elastic Initial Yield Surface … 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. February 4, 2005 Inventory #002177 2-26

  27. Subsequent Yield Surface 1  s' Initial Yield Surface e sy 2s' 2 3 … 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). February 4, 2005 Inventory #002177 2-27

  28. ’ y 2s’  … Isotropic Hardening • Plotting the stress-strain curve enables an understanding of what occurs during a loading and reverse loading cycle: 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 strainorproportional loading simulations. It is usually not applicable cyclic loading. February 4, 2005 Inventory #002177 2-28

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

  30. … 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

  31. … 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

  32. … 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

  33. … 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

  34. … 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

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

  36. … 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

  37. … 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

  38. Workshop 2A Large Deflection with Metal Plasticity

  39. 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

  40. … 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

  41. … Workshop 2A – Metal Plasticity • 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

  42. … Workshop 2A – Metal Plasticity • 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

  43. … Workshop 2A – Metal Plasticity • Review the displacement and stress results from this first run. February 4, 2005 Inventory #002177 2-43

  44. … Workshop 2A – Metal Plasticity • 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

  45. … Workshop 2A – Metal Plasticity • 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

  46. … Workshop 2A – Metal Plasticity • 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

  47. … Workshop 2A – Metal Plasticity • 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

  48. … Workshop 2A – Metal Plasticity • 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

  49. … Workshop 2A – Metal Plasticity • 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

  50. … Workshop 2A – Metal Plasticity • 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

More Related