BREAK FORMING

1. BREAK FORMING MAR 120 - Break Forming Exercise

2. Model Description: A flat sheet is formed into an angled bracket by punching it through a hole in a table using the contact option. The cylindrical punch drives the sheet down into the hole of the table to a total stroke of 0.3 inches. The material is elastic-plastic with some work-hardening. At the bottom of the stroke, the total strain is nearly 60%. The vertical force rises quickly, hardens through about half of the stroke, then softens near the end of the stroke.

3. Objectives: • Large displacement / large strain analysis. • Contact analysis using rigid-deformable contact. • Elastic-plastic material model. • Define multiple load cases. • Investigate convergence criteria effects. • Required: • A file named break_forming.igs in your working directory.

4. Exercise Overview: • Import the geometry. • Mesh the deformable body. • Model the rigid and deformable contact curves and surfaces. • Define the materials and properties. • Define the load cases. • Submit the job to analysis. • Evaluate the results. • Modify the convergence criteria. • Re-submit the analysis. • Compare the results.

5. Step 1. Create a New Database a d • Create a new database. Name it Break_Forming.db. • Select File / New. • Enter Break_Forming as the file name. • Click OK. • Select MSC.Marc as the Analysis Code. • Click OK. e c b

6. Step 2. Import the Geometry a Import the required geometry. • Select File / Import. • Switch the Source to IGES. • Select break_forming.igs as the File name. • Click Apply. b c d

7. Step 2. Import the Geometry (Cont.) • Click OK on the Import Summary Page. e 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. The ‘Import Summary’ Page show what types of entities were imported into the MSC.Patran database. After clicking OK, the geometry should look like the image to the left.

8. Step 3. Define the Mesh Seeds • Create the finite element mesh seeds. • Elements: Create / Mesh Seed / Uniform. • Enter 6 as the Number. • Pick the rightedge of the surface. • Enter 80 as the Number. • Pick the topedge of the surface. a b d e c

9. Step 4. Create the Mesh • Create the finite element mesh. • Elements:Create / Mesh / Surface. • Verify that Quad4 elements are selected. • Select the plate surface in view port. • Click Apply. a b c d After meshing, the viewport should look like the image to the left.

10. Step 5. Hold the Plate in the X-Direction Create the Boundary Condition fixing the plate from moving in the X-Direction. • Loads/BCs: Create / Displacement / Nodal. • Enter Fixed-X as the New Set Name. • Click on Input Data. • Enter <0,, > for the Translation. • Click OK. a d e b c

11. Step 5. Hold the Plate in the X-Direction (Cont.) • Click on Select Application Region. • Switch the Geometry Filter to FEM. • Select the center nodes of the plate. • Click Add. • Click OK. • Click Apply. g i j h f k We are fixing these center nodes as a type of symmetry condition. This constraint will remove the Rigid Body motion in the X-Direction.

12. Step 6. Apply a Gravity Load Create the Boundary Condition for Gravity in the –Y Direction. • Loads/BCs: Create / Inertial Load / Element Uniform. • Enter Gravity as the New Set Name. • Switch to 2D Element Type. • Click on Input Data. • Enter <,-386.4, > for the Trans Accel. • Click OK. a e f b c d

13. Step 6. Apply a Gravity Load (Cont.) • Click on Select Application Region. • Switch to Geometry as the Geometry Filter. • Select the plate surface. • Click Add. • Click OK. • Click Apply. h j k i g l We are adding a gravity load to force the plate to remain on the table after the forming operation. This constraint will remove the Rigid Body motion in the Y-Direction during the Release.

14. Step 7. Define the Deformable Contact Body for the Plate Create the deformable contact object. • Loads/BCs: Create / Contact / Element Uniform. • Confirm Deformable Body as the Option. • Enter Plate as the New Set Name. • Select 2D as the Target Element Type. • Click on Select Application Region form. • Confirm that the Geometry option is selected for the Geometry Filter. • Select the plate surface. • Click Add. • Click OK. • Click Apply. a f b h i c d e g j After you click Apply, you will see the contact markers(pink circles) in the viewport. e

15. Step 8. Define the Rigid Contact Body for the Table Create the rigid contact object for the Table. • Loads/BCs: Create / Contact / Element Uniform. • Select Rigid Body as the Option. • Enter Table as the New Set Name. • Select 1D as the Target Element Type. • Click on Select Application Region form. • Confirm the Geometry Filter is set to Geometry. • Select all of the table curves. Be sure not to include any of the surface edges. • Click Add. • Click OK. a f b h i c d Curve 3 Curve 5 Curve 8 Curve 7 e Curve 2 Curve 4 Curve 1 g

16. Step 8. Define the Rigid Contact Body for the Table (Cont.) The rigid contact markers point toward the inside of the rigid body –think of them as tick marks representing a wall. If the tick marks are reversed, Modify the Contact Body and flip the contact side on the Modify Data Form. • Click Apply. j

17. Step 9. Define the Rigid Contact Body for the Punch Create the rigid contact object for the Punch. • Loads/BCs: Create / Contact / Element Uniform. • Select Rigid Body as the Option. • Enter Punch as the New Set Name. • Select 1D as the Target Element Type. • Click on Input Data. • Enter <0., -0.3, 0.> for the Velocity. • Click OK. • Click on Select Application Region form. a b f c d e h g

18. Step 9. Define the Rigid Contact Body for the Punch (Cont.) • Confirm the Geometry Filter is set to Geometry. • Select the punchcurve. • Click Add. • Click OK. • Click Apply. i k j l m The tick-marks should be on the inside of the circle for the Punch.

19. Step 10. Preview the Rigid Body Motion Preview the Rigid Body Motion. • Loads/BCs: Create / Contact / Element Uniform. • Select Preview Motion. • Select Punch. • Select Preview Motion. • The Rigid Body should display the prescribed motion that was entered on the Input Data form. • Click OK when finished examining the motion. a c d f e b

20. Step 11. Input the Stress vs. Plastic Strain Curve Define the Plastic Strain vs. Stress Curve. • Fields: Create / Mat. Prop. / Tabular Input. • Enter Plasticity as the Field Name. • Un-check the Temperature Variable. • Check the Strain Variable. • Click on Input Data. • Click in the Top Left Cell. • Enter the Strain Data. • Click in the Top Right Cell. • Enter the Stress Data. • Click OK. • Click Apply. a To quickly enter this data, Enter the top value and press Enter. The table will automatically tab down. f b c h d g e i k j

21. Step 12. Verify the Stress vs. Plastic Strain Data a b Check the Field Input by plotting the data. • Fields: Show. • Select the Plasticity field. • Click the Specify Range Panel. • Select Use Existing Points. • Click OK. • Click Apply. • Click Cancel on the Data Form. • Click Unpost Current XYWindow. c h f g d The XY Plot should look like the one on the left. e

22. Step 13. Define the Elastic Material Properties Define the Elastic portion of the Steel material. • Materials: Create / Isotropic / Manual Input. • Enter Steel as the Material Name. • Click on Input Properties. • Confirm Elastic as the Constitutive Model. • Enter 30e6 as the Elastic Modulus. • Enter 0.3 as the Poisson Ratio. • Enter 0.00074 for the Density. • Click OK. • Click Apply. d a e f g b h c In order to define Elastic-Plastic material properties in MSC.Marc, we first have to define the Elastic Portion of the Stress-Strain curve (Step 10) and then define the Plastic portion of the curve (Step 11). i

23. Step 14. Define the Plastic Material Properties Define the Plastic portion of the Steel material. • Materials: Create / Isotropic / Manual Input. • Select Steel in the Existing Materials. • Select Plastic as the Constitutive Model. • Click in the Stress vs. Plastic Strain data box. • Select Plasticity in the Fields list. • Click OK. • Click Apply. c a b d e g f

24. Step 15. Show the Material Model Confirm that the Steel material has Elastic and Plastic constitutive models. • Materials: Show / Isotropic / Tabular. • Select Steel in the Existing Materials. • Confirm that there are two constitutive models (Elastic and Plastic) in the Current Constitutive Models list. • Click Cancel. a b c d

25. Step 16. Define the Element Properties a Define the Element Properties. • Properties: Create / 2D / 2D Solid. • Enter Plate as the Property Set Name. • Confirm Plane Strain as the Option. • Confirm Standard Formulation. • Click on Input Properties. • Click on Mat Prop Name icon. • Choose Steel from the Existing Material list. • Click OK. g f b c d e h

26. Step 16. Define the Element Properties (Cont.) • Click in Select Members panel. • Select the plate surface. • Click Add. • Click Apply. i k j l

27. Step 17. Create a Forming Load Case Define the Forming Load Case. • Load Cases: Create. • Enter Form as the Load Case Name. • Click on the Assign/Prioritize Loads/BCs Panel. • Select each of the available Loads/BCs in the top left corner of the window. a d b After selecting the loads from the available list in the top right corner, they should appear here. c

28. Step 17. Create a Forming Load Case (Cont.) • Click OK. • Click Apply. This is a list of all the Loads/BCs that are defined in the MSC.Patran Database. Only the Loads/BCs listed in this section are assign to this Load case. f This column lists the type of Load/BC. e This column defines the Scale Factor to be used as a multiplier for the Load/BC. This is an easy way to have multiple load magnitudes without having to define each one individually.

29. Step 18. Create a Release Load Case Define the Release Load Case. • Load Cases: Create. • Enter Release as the Load Case Name. • Click on the Assign/Prioritize Loads/BCs Panel. • Select each of the available Loads/BCs in the top left corner of the window. a d b After selecting the loads from the available list in the top right corner, they should appear here. c

30. Step 18. Create a Release Load Case (Cont.) • Click on the Scale Factor cell for the Punch. • Click in the Scale Factor Entry Box. • Enter -1.0 and press Enter. f g e f e

31. Step 18. Create a Release Load Case (Cont.) • Click OK. • Click Apply. For the Release Load Case, we are using a Scale Factor of -1.0 to change the direction of the velocity vector that we assigned to the Punch when we made the Rigid Contact Body. The Punch originally had a velocity of 0.3 in/sec in the –Y Direction. For this Release Load Case, it will be 0.3 in/sec in the +Y Direction. i h

32. Step 19. Analyze the Model Setup and launch the Analysis. • Analysis: Analyze / Entire Model / Full Run. • Enter Break_Forming_Job1 as the Job Name. • Click on Job Parameters. • Click on Solver Options. • Check the Non-Positive Definite option. • Click OK. • Check the Assumed Strain option. • Click OK. • Click on the Load Step Creation form. e a d f The Non-Positive Definite option is needed in this problem due to the existence of Rigid Body Modes. Without this option, the analysis would end in a 2004 Exit Number in the middle of the analysis. We are turning on the Assumed Strain option because we are using Standard Formulation Plain Strain elements and the Assumed Strain option will provide more accurate results. It is recommended to use the Assumed Strain option for Standard Plain Strain, Plane Stress, and Hex Elements. b g c i h

33. Step 19. Analyze the Model (Cont.) • Enter Form in the Job Step Name. • Click on the Select Load Case form. • Select the Form Load Case from the list. • Click OK. • Click Apply. j l k m n

34. Step 19. Analyze the Model (Cont.) • Enter Release in the Job Step Name. • Click on Solution Parameters. • Click on Load Increment Params. • Enter 10 for the [# of Steps of Output]. • Click OK. • Click OK. • Click on Select Load Case. • Select the Release Load Case from the list. • Click OK. • Click Apply. • Click Cancel. • Click Load Step Selection. o q p t u z x y We are changing the number of Output steps saved to the results file to save time and disk space. Entering a ’10’ in the [# of Steps of Output] box will force the solver to save 10 evenly spaced results over the total time of the step. In this case, there will be results for every 0.1 seconds. v r s w

35. Step 19. Analyze the Model (Cont.) • Select the Form Job Step from the top section. • Select the Release Job Step from the top section. • De-select the Default Static Step from the bottom section. • Click OK. • Click Apply. a b When setting up jobs with multiple Load Steps, the order of the load cases in the ‘Selected Job Steps’ section will be the order that the Load Steps will be solved. In non-linear analyses, the state of the structure at the beginning of the second load step will be taken from the end of the first load step. This allows us to simulate complex multi-step manufacturing processes in one analysis job. c e The resulting Job Step form should look like the one to the right. d

36. Step 20. Monitor the Job Monitor the job. • Analysis: Monitor / Job. • Select Break_Forming_Job1 as the Job Name. • Click Apply. • Click Cancel when the job is complete. • Click on View Status File. • Close the Status File Window. a b f e c d

37. Step 21. Attach the Results Read (Attach) results. • Analysis: Read Results / Result Entities / Attach. • Click on Select Results File form. • Select file Break_Forming_Job1.t16. • Click OK. • Click Apply. a c d b e

38. Step 22. Plot the Stress Results Post-process results. • Results: Create / Quick Plot. • Select all of the result cases. • Select Stress, Global System as the Fringe Result. • Select Displacement, Translation as the Deformation Result. • Click Apply. a b c d Notice the Spring-back as the punch is first released. The final shape will open slightly due to the elastic strain still in the structure. e

39. Step 23. Create a Load vs. Displacement Plot Post-process results – Rigid Body Force. • Results: Create / Graph / Y vs X. • Click on the Results Tree button to view all of the result cases. • Select all of the result cases. • Select Global Variable for the Y. • Select Body Punch, Force Y for the Y Variable. • Select Global Variable for the X. • Select Time for the X Variable. • Click Apply. a b c d e The plot is shown on the next page. f g h

40. Step 23. Create a Load vs. Displacement Plot (Cont.) • The plot shows the total body force required to form the plate. i This force plot shows a typical outcome when the convergence tolerance is too large: the force curve is not very smooth. Finding the maximum required Punch Force from this plot would be difficult. In the next section, we will tighten the convergence tolerance and see its effect on the plot.

41. Step 24. Un-Post the Results Unpost the Results Plots. • Results: Post / Plots. • Click on the Select None button. • Click -Apply-. a b c

42. Step 25. Re-Analyze the Model With More Accuracy Setup and launch the second analysis. • Analysis: Analyze / Entire Model / Full Run. • Click on Break_Forming_Job1 in the Available Jobs list. • Enter Break_Forming_Job2 as the Job Name. • Click on the Load Step Creation form. • Click on the Form Job Step. • Click on the Select Load Case panel. • Confirm that the Form Load case is selected. • Click OK. a e g b h c f d

43. Step 25. Re-Analyze the Model With More Accuracy (Cont.) • Click on Solution Parameters. • Click on Iteration Parameters. • Enter 0.01 for the Relative Residual Force. • Click OK. • Click OK. • Click Apply. (Yes to Overwrite) • Click Cancel. • Click Load Step Selection. j i m n o p k l

44. Step 25. Re-Analyze the Model With More Accuracy (Cont.) • Select the Form Job Step from the top section. • Select the Release Job Step from the top section. • De-select the Default Static Step from the bottom section. • Click OK. • Click Apply. q r s u t

45. Step 26. Monitor the Second Job Monitor the job. • Analysis: Monitor / Job. • Select Break_Forming_Job2 as the Job Name. • Click Apply. • Click Cancel when the job is complete. • Click on View Status File. • Close the Status File Window. a b f e c d

46. Step 27. Attach the Second Results Read (Attach) results. • Analysis: Read Results / Result Entities / Attach. • Click on Select Results File form. • Select file Break_Forming_Job2.t16. • Click OK. • Click Apply. a c d b e

47. Step 28. Plot the New Stress Results Post-process results. • Results: Create / Quick Plot. • Select all of the result cases with an A2 in the name. (Note: Use the CTRL key to select multiple results that are not in a continuous series.) • Select Stress, Global System as the Fringe Result. • Select Displacement, Translation as the Deformation Result. • Click Apply. a b c d e

48. Step 29. Create a Second Load vs. Displacement Plot Post-process results – Rigid Body Force. • Results: Create / Graph / Y vs X. • Click the Results Tree icon. • Select all of the result cases with an A2 in the name. • Select Global Variable for the Y. • Select Body Punch, Force Y for the Y Variable. • Select Global Variable for the X. • Select Time for the X Variable. • Click the Attributes Page. • Check the Append Curves in XY Window option. • Click Apply. a h b c d e The plot is shown on the next page. f i The Append Curves in XY Window option will save the original curve from the previous run and add a second curve that can be posted. Step 30 will show you how to see both curves in the same window. Without this option turned on, the previous curve would be overwritten by the new curve. g j

49. Step 29. Create a Second Load vs. Displacement Plot (Cont.) • The plot shows the total body force required to form the plate. k This force plot appears much smoother than the original curve. By tightening the convergence tolerance from 0.1 to 0.01, the force balance became more accurate. However, there is a trade-off with run-times. The tighter tolerance will usually result in more cycles in the analysis. In this case, the CPU and wall times were between 3 and 4 times longer with the tighter tolerance.

50. Step 30. Show Both Plots Together Post both Body Force curves for comparison. • XY Plot: Post / Curve. • Select both default_Graph## curves in the Post/Unpost section. • Click Apply. a b We can now see the difference in the curves. c