HM-4330: Define *STEP using Abaqus Step Manager

In this step you will load the Abaqus user profile and model file.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, set the user profile to Abaqus, Standard 3D.
3. Open a model file by clicking File > Open > Model from the menu bar, or by clicking on the Standard toolbar.
4. In the Open Model dialog, open the abaqus_StepManager_tutorial.hm file.
   Note: The abaqus_StepManager_tutorial.hm file contains pre-defined model data. Use this file in the following steps to define the history data portion of this model.

In this step you will create a *STEP card with the *STATIC analysis procedure.

1. From the menu bar, click Tools > Loadsteps Browser.
   The Step Manager opens.
2. Click New.
   The Create New Step dialog opens.
3. In the Name field, type step1.
4. Click Create.
   A step labeled step1 opens the Load Step dialog.
5. In the first pane, select Title.
   The Step Heading option with a disabled field is displayed.

   
   
   Figure 1.

6. Select the Step heading checkbox and type 100kN in the text field.

   
   
   Figure 2.

7. Click Update to store the heading information in step1.
8. In the first pane, select Parameter.
9. Select the Name and Perturbation checkboxes.
   Note: Notice that Name is already set to step1.

   
   
   Figure 3.

10. Click Update.
11. In the first pane, select Analysis procedure.
12. Set Analysis type to static.

    
    
    Figure 4.

13. Click Update.
14. Click the Dataline tab.
15. Select the Optional dataline checkbox to add an additional dataline.
16. Add individual data, such as Initial increment, by selecting the appropriate checkbox and entering a value.
    Note: When a checkbox is disabled, a space will be added in the ASCII file, and the Abaqus solver will use the default value.

    
    
    Figure 5.

17. Click Update.

In this step you will create constraints.

1. In the first pane, select Boundary.
2. Click New.
   The Create Load Collector dialog opens.
3. In the Name field, type loads_and_constraints.
4. Click Create.
5. Optional: In the Load collector table, Display column, click the color icon to select a color for the load collector.
6. Verify that the Status checkbox for loads_and_constraints is selected.
   Note: By selecting this checkbox, you are adding this load collector into the loadstep.
7. Click the loads_and_constraints load collector.
   New tabs display.
8. From the Define tab, verify that Type is set to default(disp).

   
   
   Figure 6.

9. Click Define from 'Constraints' panel.
   The Constraints panel opens, from which you will create constraints.

In this step you will create constraints from the Constraints panel.

1. On the Standard Views toolbar, click (XZ Right Plane View).
2. In the Constraints panel, click nodes >> by window.
3. With the exception of nodes at the ends of the cradle, draw a rectangle around all of the displayed nodes.

   
   
   Figure 7.

4. Select the exterior checkbox.
5. Click select entities.
   HyperMesh selects all nodes outside the window your drew.

   
   
   Figure 8.

6. Verify that all six dof checkboxes are selected.

   
   
   Figure 9.

7. Click create.
   HyperMesh creates constraints at the selected nodes.

   
   
   Figure 10.

8. Click return to go back to the Load Step dialog.
9. At the bottom of the Load Step dialog, look at the Load type line.
   Bc (short for BOUNDARY) appears on this line, which indicates step1 is a load type created in the load_and_constraints load collector. The corresponding load type in the first pane is also highlighted.

   
   
   Figure 11.

In this step you will create forces (*CLOAD).

1. In the first pane of the Load Step dialog, expand Concentrated loads, and select CLOAD-FORCE. New tabs display.

   
   
   Figure 12.

2. From the Define tab, click Define from 'Forces' Panel.
   The Forces panel opens from which you will create forces.

In this step you will create forces from the Forces panel.

1. Select the central node on the top side of the bracket arm.

   
   
   Figure 13.

2. In the Forces panel, magnitude= field, type -100.
3. Set the orientation selector to z-axis.

   
   
   Figure 14.

4. Click create.

   
   
   Figure 15.

5. Click return to go back to the Load Step dialog.
6. At the bottom of the Load Step dialog, notice the Load type now reads Cload-f, which indicates CLOAD-force as another load type created in the loads_and_constraints load collector. The corresponding load type in the first pane is highlighted.

   
   
   Figure 16.

7. Click Review/Reset.
   The constraints and forces that belong to the loads_and_constraints load collector highlight.

   
   
   Figure 17.

8. Revert the highlighted constraints and forces to the load collector color by right-clicking on Review.

In this step you will create a *DLOAD pressure load and add it to the current load collector with an element set.

1. In the first pane of the Load Step dialog, expand Distributed loads, and select DLOAD.
   A new set of tabs displays.
2. From the Define tab, set Define DLOAD on to Element sets.
   The elements sets table displays.
3. Rotate the model to the view as shown in the following image.

   
   
   Figure 18.

4. From the Load Step dialog, set Type to default (Pressure).
5. Set Element sets to pressure_set.
   Note: To view the entire list of element sets, click . Use Fileter and Sort to narrow your search.
6. Click the right arrow to add the selected set to the element sets table.

   
   
   Figure 19.

7. Under Element sets, click Review | Reset Set. The element set highlights.

   
   
   Figure 20.

8. Revert the load collector back to its original color by right-clicking on Review | Reset Set.
9. In the element sets table, Label column, select P for the newly added pressure_set.

   
   
   Figure 21.

10. Because the pressure_set contains shell elements, the direction of normal to the elements must be known to determine the sign of the magnitude. Find the direction of the normal by selecting the pressure_set element from the table and clicking Show faces.

    
    
    Figure 22.

11. Clear the display by right-clicking on Show faces.
12. In the element sets table, Magnitude column, type -10 for pressure_set.
    Note: The negative magnitude means pressure load in the opposite direction of the underlying shell element normals.
13. Click Update.
    The HyperMesh database updates. The Load type line, at the bottom of the dialog, now displays Dload, which indicates DLOAD as another load type created in the loads_and_constraints load collector. The corresponding load type is the first pane is also highlighted.

    
    
    Figure 23.

14. In the element sets table, Elset column, click pressure_set.
15. Click Review | Reset Set to review the loads.

    
    
    Figure 24.

16. Revert back to the standard view by right-clicking on Review | Reset Set.

    
    
    Figure 25.

    In this exercise, you constrained and applied distributed loads on the model using HyperMesh panels. The loads (*DLOAD) information is automatically stored in step1. Next, you will specify the output requests for this step.

In this step you will specify several output requests for step1.

1. In the first pane of the Load Step dialog, expand Output request and click ODB file.

   
   
   Figure 26.

2. Click New.
3. In the Create Output block dialog, Name field, type step1.
4. Click Create.
5. In the Output block table, click step1.
   New tabs appear.

   
   
   Figure 27.

6. In the Output tab, select the Output checkbox. Leave Output set to field.
7. Select the Node output and Element output checkboxes.
   the Node Output and Element Output tabs become active.

   
   
   Figure 28.

8. Click the Node Output tab.
9. Expand Displacement and select U.
   The Data lines table now displays "U", which allows you to request displacement results obd in the file.

   Note: You can manually type output request into the Data lines table, including unsupported requests. They will be written just as they are entered in the table.

   
   
   Figure 29.

10. Click Update.
11. Click the Element Output tab.
12. Select the Position checkbox and set it to Nodes.
13. Expand Stress and select S.
    The Data lines table now displays "S" which allows you to request stress results in the .obd file.

    
    
    Figure 30.

14. Click Update.

In this step you will request results file (.fil) outputs.

1. In the first pane of the Load Step dialog, expand Output request and click Result file (.fil).

   
   
   Figure 31.

2. In the Define tab, select the Node file and Element file checkboxes.
   The Node File and Element File tabs become active.

   Figure 32.
   
   

3. Click the Node File tab.
4. Expand Displacement and select "U."
   The Data lines table displays "U," which allows you to request displacement result in the .fil file.
5. Click Update.
6. Click the Element File tab.
7. Select the Position checkbox and set it to averaged at nodes.
8. Expand Stress and select S.
   The Data Line table displays "S," which allows you to request str4ess results in the .fil file.

   
   
   Figure 33.

9. Click Update.
10. Under the Output block table, click Review | Reset.
    The Review output block dialog opens and displays the output requests you made.

    Note: This is the format used in the Abaqus input file (.inp).

    
    
    Figure 34.

11. Click Close to exit the Review output block dialog.
12. In the first pane of the Load Step dialog, click Unsupported cards.
13. Optional: Select the Unsupported cards checkbox to add any unsupported card.
14. Click Close to exit the Load Step dialog and return to the Step Manager.
    The Step Manager dialog displays all information you defined for step1.

    
    
    Figure 35.

15. Click Close to exit the Step Manager dialog.

In this step you will export the .inp file.

1. From the menu bar, click File > Export > Solver Deck.
2. In the File: field, type job1.inp.
3. To the left of Export Options, click .
4. Set Export to all.
5. Click Export.

In this step you will save the .hm file.

1. From the menu bar, click File > Save as > Model.
2. In the Save Model As dialog, type job1.hm as the file name.
3. Click Save.
   Notes:

   • After you quit HyperMesh, you can run the Abaqus solver using the job1.inp file that was written from HyperMesh.
   • At your site, you can use the Abaqus license to run this model.
   • If the batch mode option is being used, then enter the name of the .inp file exported in the previous step as the input file.
   • After you have successfully completed the analysis, the result file will be available in your working directory with the name <jobname.odb>.
   • Use HvTrans to translate the Abaqus solver result file to an H3D file.

In this step you will open HyperView from the application menu.

1. On the Client Selector toolbar, select HyperView. HyperView opens.

   
   
   Figure 36.

2. In the panel area, load the model and results files.
   Note: Load *.h3d files for both the model and result files.

   
   
   Figure 37.

3. Click Apply.
4. On the Results toolbar, click to open the Contour panel.
5. Review displacement (v) results by setting the Result type to Displacement (v).

   
   
   Figure 38.

6. Click Apply.

   
   
   Figure 39.

7. In the Results Browser, review steps and increments.

   
   
   Figure 40.

8. On the Animation toolbar, set the animation mode to linear.

   
   
   Figure 41.

9. Review the animation by clicking .
10. Review UR-Rotational displacement (v) results by setting the Result type to UR-Rotational displacement (v) in the Contour panel.

    
    
    Figure 42.

11. Click Apply.

    
    
    Figure 43.