NECKING OF A TEST SPECIMEN WORKSHOP 3 NECKING OF A TEST SPECIMEN Symmetry Plane Symmetry Plane

Model Description In this lesson, you will stretch an 8 inch long planar steel bar by 1.65 inch (i.e. more than 20% of its length). This elastic-plastic problem will demonstrate the importance of the concept of true stress (or Cauchy stress) in non-linear analysis. This test specimen will be modeled using a quarter symmetry model.

Objective Large Deflections/Strains analysis Elastic-Plastic material model using isotropic hardening Required A file named necking.bdf in your working directory (Ask your instructor for it if you don’t see it before starting) Proceed to the next page.

Suggested Steps for Exercise: Import the meshed model (necking.bdf)to SimXpert Set MAT1 & MATTEP material cards Set Plane stress elements for this model Fix the vertical and horizontal lines of symmetry of the bar and pull the other end by 1.65 inches. Create a Sol600 job

Step 1. Open a New Database Structures Workspace. Launch SimXpert. Select Structures.

Step 2. Set Unit b c a f d e Set the units to English. Select Tools / Options Select Units Manager. Click Standard Units. Select the line containing English Units (in, lb, s…) Click OK Click OK. a f d e

Step 3. Import the necking.bdf a Import the required geometry. Select File / Import / Nastran Select necking.bdf as the File name. Click Apply. In order to use Plain Strain 2D Solid elements, the geometry must be in the X-Y Plane at Z=0. The normals of the elements must point in the +Z Direction.

Step 4. Input the Stress vs. Strain Curve Define the Plastic Strain vs. Stress Curve. In Materials and Properties tab, select Table \ StructPhysical \ Stress-Strain. Enter Stress-Strain_1 as Table name Click + icon to add rows Key in all data as we provide Click OK a b c d e

Step 5. Define Plastic Material Modify the material aluminum with elastic properties. In Model Brower, double click Material / Aluminum Click Advanced icon. Click Add Constitutive Model / Elasto Plastic. b a c

Step 5. Define Plastic Material (cont.) Create the material aluminum_1100, with elastic properties. Select Nonlinear Data Input: Stress-Strain Data. Stress-Strain Data: select the Stress-Strain_1 curve which you created in step16. Click OK. d e f

Step 6. Define the Element Properties-convert to plane stress Convert plane strain elements to plane stress. On the LBC’s tab, select PARAM from the Parameter group Enter MREL1103 in N filed Enter 3 in V1 field Click Create. b c d This step is for SOL600 to set plane stress element property. For more info, please check Nastran qrg document.

Step 7. LBC: symmetric_vertical Create the three required Displacement Boundary Conditions. Here we create symmetric_vertical. On LBC’s tab, select General from the Constraint group Enter symmetry_vertical as Name. Check only Tx Pick nodes along the symmetric edge Click Apply b d c e

Step 8. LBC: pull_at_end a d b c e Create the pull_at_end Displacement Boundary Conditions. Enter pull_at_end as Name. Check Tx and enter 1.65 Check Ty and enter 0 Pick nodes along the right edge Click Apply a d b c e

Step 9. LBC: symmetric_horiz Create the symmetric_horiz Displacement Boundary Conditions. Enter symmetric_horiz as the New Set Name. Check only Ty Pick nodes along the upper edge Click OK a c b d

Step 10. Display LBC Change display mode: Request plotting of Loads/BCs markers on FEM entities. Click Render On/Off to show LBCs a

Step 11. Create a New Job a c b c d e Create a new job. Right-click FileSet and select Create new Nastran Job Enter Necking for the Job Name. Select Implicit Nonlinear Analysis (SOL 600) for the Solution Type. Click the ellipses on the Solver Input file. Select the file path Enter Necking for the File Name.. Click OK.. a c b c d e

Step 12. Select Load/BCs b c a Select Load/BCs. In Model Browser, right click Simulation / Necking / Load Cases / DefaultLoadCase / Load/Boundaries / Select Lbc Set Select DufaultLbcSet Click OK.. b c a

Step 13. Subcase Properties Open Model Browser, double click Necking \ Load Cases \ Loadcase Control Check on DefineLoadIncrementParameters option Switch Increment Type from Fixed to Adaptive Enter Trial Time Step Size as 0.01 Enter 1 as Total Time. Click on Apply b c d e a f

Step 13. Subcase Properties (cont.) Switch to Sol600SubcaseIterationParameters dialog Enter 0.01 as in Residual Tolerances / Relative Residual Force Click Apply. a b c d

Step 13. Subcase Properties (cont.) Setup the Analysis Parameter Select SOL600SubcaseNonlinearGeomParameter dialog Switch Nonlinear Geometric Effects option to Large Displacement/Large Strains Click Apply Click Close a b c d e

Step 14. Output Requests-Element Results Right Click on Output Requests to add the following output Total Strain Tensor (301) Plastic Strain Tensor (321) Cauchy Stress Tensor (341) a

Step 15. Run this job a Run this job Open Model Browser, click right mouse button at Necking, Select Run. a

Step 16. Attach result file Attach results files, *.t16 File \ Attach Results\ Result Entities… Choose necking.marc.t16 Click OK b a c

Step 17. Plot the Deformation Results c b d e Plot the deformation & stress results. On the Results tab, select Deformation Result Cases: select the Increment with Time=1.0 Result type: Displacement, Translation Click Display setting tab, change Deformed display scaling to “True :1”. Choose Update

Step 21. Plot the Stress Results a e d b c Plot the deformation & stress results. Plot type: Fringe Result Cases: select the Increment with Time=1.0 Result type: Result Type: Stress,Cauchy Derivation: von Mises Choose Update

Congratulation!