Exercise 2: Introduction to ANSYS Load Steps

In this exercise you will: create constraint load collectors; apply the constraints to the model; apply the force on mass elements with force1, force2, and force3 load collectors; create multiple load steps; add /SOLU and LSSOLVE in control cards; and export the deck to ANSYS *cdb format.

This exercise introduces the concept of ANSYS load steps in HyperMesh. In HyperMesh, you need to have each load or constraints in a separate load collector (load cols). With the help of these load collectors, you can create multiple load steps depending on the requirement. The combination of loads with constraints, form a load step. If you have created load steps in your model, the exported *.cdb file will have all of the load step information. This *.cdb file when imported into ANSYS, automatically creates the *.so files in the working directory which can be used later if needed.

Retrieve the HyperMesh Model File

In this step, you will retrieve and open the model file.

Only complete this step if you did not complete Exercise 1: Define Elements, Real Constants, Materials, Properties, and Components.
  1. From the menu bar, click File > Open > Model.
  2. In the Open Model dialog, open the chapter2_2.hm file.
  3. Optional: If you model's elements and mesh lines are not shaded, click on the Visualization toolbar.


    Figure 1.

Create a Constraints Load Collector

In this step you will learn how to create load collectors within HyperMesh.

  1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
    HyperMesh creates and opens a load collector in the Entity Editor.
  2. For Name, enter constraints.
  3. Click the Color icon, and select a new color for the load collector.
  4. Repeat steps 1 through 3 to create three more load collectors named force1, force2, and force3.
Four load collectors display in the Model Browser as indicated in Figure 2.


Figure 2.

Apply the Constraints to the Model

In this step, you will apply the constraints you created to the model.

  1. In the Load Collectors folder of the Model Browser, right-click on constraints and select Make Current from the context menu.
    Note: When new loads are created, HyperMesh will place them in this collector.
  2. From the menu bar, click BCs > Create > Constraints.
    The Constraints panel opens.
  3. Select the dof (degree of freedom) checkboxes as indicated in Figure 3.


    Figure 3.
  4. Click nodes > by path.
  5. Select a start node and an end node on the left side of the model as indicated in Figure 4.


    Figure 4.
  6. Click Create.


    Figure 5.
  7. Repeat steps 4 and 5 to select a start node and an end node on the right side of the model as indicated in Figure 6.


    Figure 6.
  8. Click Create.


    Figure 7.
  9. Click return to exit the Constraints panel.


    Figure 8.

Apply the Force on Mass Elements with the Force1 Load Collector

In this step, you will apply the force on mass elements with the force1 load collector.

  1. In the Load Collector folder of the Model Browser, right-click on force1 and select Make Current from the context menu.
  2. From the menu bar, click BCs > Create > Forces.
    The Forces panel opens.
  3. Verify the entity selector is set to nodes.
  4. Select the two nodes in the center of the two bolt holes as indicated in Figure 9.


    Figure 9.
  5. In the magnitude= field, enter 500.
  6. Set the orientation selector to z-axis for the direction of application of the force.
  7. In the uniform size= field, enter 20.
  8. Click Create.


    Figure 10.
  9. Click return to exit the Forces panel.


    Figure 11.

Apply the Force on Mass Elements with the Force2 Load Collector

In this step, you will apply the force on mass elements with the force2 load collector.

  1. In the Load Collector folder of the Model Browser, right-click on force2 and select Make Current from the context menu.
  2. For better visualization, press F5 to open the Mask panel.
  3. Set the entity selector to loads.
  4. Select the two forces you created in step 8 of Apply the Force on Mass Elements with the Force1 Load Collector.
  5. Click mask.
  6. Click return.
  7. From the menu bar, click BCs > Create > Forces.
    The Forces panel opens.
  8. Verify the entity selector is set to nodes.
  9. On the Standard Views toolbar, click .
  10. Select the left side node in the center of the bolt hole as indicated in Figure 12.


    Figure 12.
  11. In the magnitude= field, enter 500.
  12. Set the orientation selector to z-axis for the direction of application of the force.
  13. Click create.
  14. Select the right side node in the center of the bolt hole as indicated in Figure 13.


    Figure 13.
  15. In the magnitude= field, enter -500.
  16. Set the orientation selector to z-axis for the direction of application of the force.
  17. Click create.


    Figure 14.
  18. Click return to exit the Forces panel.

Apply the Force on Mass Elements with the Force3 Load Collector

In this step, you will apply the force on mass elements with the force3 load collector.

  1. In the Load Collector folder of the Model Browser, right-click on force3 and select Make Current from the context menu.
  2. Open the Mask panel.
  3. Verify the entity selector is set to loads.
  4. Select the two forces you created in steps 13 and 17 of Apply the Force on Mass Elements with the Force2 Load Collector.
  5. Click mask.
  6. Click return.
  7. From the menu bar, click BCs > Create > Forces.
    The Forces panel opens.
  8. Verify the entity selector is set to nodes.
  9. Select the two nodes in the center of the two bolt holes as indicated in Figure 15.


    Figure 15.
  10. In the magnitude= field, enter -500.
  11. Set the orientation selector to z-axis for the direction of application of the force.
  12. Click create.


    Figure 16.
  13. Click return to exit the Forces panel.


    Figure 17.

Create Multiple Load Steps

In this step, you will create multiple load steps.

  1. In the Model Browser, right-click and select Create > Load Step from the context menu.


    Figure 18.
    HyperMesh creates and opens a load step in the Entity Editor.
  2. For Name, enter Step1.
  3. For Loadcol IDs, click 0 Loadcols > Loadcols.


    Figure 19.
  4. In the Select Loadcols dialog, select constraints and force1.


    Figure 20.
  5. Click OK.
  6. Repeat steps 1 through 5 to create a second load step named Step2 with the load collectors constraints and force2.
  7. Repeat steps 1 through 5 to create a third load step named Step3 with the load collectors constraints and force3.
  8. In the Model Browser, review the Load Collectors and Load Steps you created.


    Figure 21.
  9. Optional: If necessary, click View > Browsers > HyperMesh > Solver from the menu bar to open the Solver Browser.
  10. In the Solver Browser, review the Load Collectors and Load Steps you created.

Add /SOLU, ANTYPE, and LSSOLVE in the Control Cards

In this step, you will add the following Control Cards.

  1. From the menu bar, click Setup > Create > Control Cards.
    The Control Cards panel opens.
  2. In the card image, click /SOLU to exit the PREP7 preprocessor and enter the SOLU preprocessor.


    Figure 22.
  3. Click return.


    Figure 23.
  4. Because you are solving the model for static analysis, click ANTYPE.


    Figure 24.
  5. Set type to STATIC and status to NEW.


    Figure 25.
  6. Click return.
  7. Click LSSOLVE.


    Figure 26.
    Tip: If you do not see the LSSOLVE Control Card, click next.
  8. Enter 1 in the LSMIN field as indicated in Figure 27.
    The minimum number of load steps is set.
  9. Enter 3 in the LSMAX field as indicated in Figure 27.
    The maximum number of load steps is set.
  10. Enter 1 in the LSINC field as indicated in Figure 27.
    The load step increment is set.


    Figure 27.
  11. Click return to exit the card image.
  12. Click return to exit the Control Cards panel.

Export the Deck

In this step, you will export the deck to ANSYS *.cdb format.

  1. From the menu bar, click File > Export > Solver Deck.
    The Export tab opens.
  2. Set File type to Ansys.
    Note: If you are in the ANSYS user profile, HyperMesh automatically sets the File type to Ansys and loads ANSYS as the default Template.
  3. In the File field, navigate to your working directory and save the file as 4410_export.cdb.
  4. Click Export.