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 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 > HyperMesh Model.
  2. In the Open File dialog, select the chapter2_2.hm.
  3. Optional: If your model's elements and mesh lines are not shaded, click on the View Controls toolbar then select .


    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.


Figure 2.

Apply the Constraints to the Model

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

  1. In the Model Browser, right-click on Load Collectors and select Open.
  2. Right-click on constraints and select Make Current.
  3. From the Analyze ribbon, click BCs > Constraints tool.


    Figure 3.
    The Constraints panel opens.
  4. Select the dof (degree of freedom) checkboxes as indicated in Figure 4.


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


    Figure 5.
  7. Click Create.


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


    Figure 7.
  9. Click Create.


    Figure 8.
  10. Click return to exit the Constraints panel.


    Figure 9.

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 Model Browser, right-click on Load Collectors and select Open.
  2. Right-click on Force1 and select Make Current.
  3. From the Analyze ribbon, Loads tool group, click the Apply Forces tool.


    Figure 10.
    The Forces panel opens.
  4. Verify the entity selector is set to nodes.
  5. Select the two nodes in the center of the two bolt holes as indicated in Figure 11.


    Figure 11.
  6. In the magnitude= field, enter 500.
  7. Set the orientation selector to z-axis for the direction of application of the force.
  8. In the uniform size= field, enter 20.
  9. Click Create.


    Figure 12.
  10. Click return to exit the Forces panel.


    Figure 13.

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 Model Browser, right-click on Load Collectors and select Open.
  2. Right-click on Force2 and select Make Current.
  3. For better visualization, press F5 to open the Mask panel.
  4. Set the entity selector to loads.
  5. Select the two forces you created in step 9 of Apply the Force on Mass Elements with the Force1 Load Collector.
  6. Click mask.
  7. Click return.
  8. From the Analyze ribbon, Loads tool group, click the Apply Forces tool.


    Figure 14.
    The Forces panel opens.
  9. Verify the entity selector is set to nodes.
  10. Select the left side node in the center of the bolt hole as indicated in Figure 15.


    Figure 15.
  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 16.


    Figure 16.
  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 17.
  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 Model Browser, right-click on Load Collectors and select Open.
  2. Right-click on Force3 and select Make Current.
  3. For better visualization, press F5 to open the Mask panel.
  4. Set the entity selector is set to loads.
  5. Select the two forces you created in steps 13 and 17 of Apply the Force on Mass Elements with the Force2 Load Collector.
  6. Click mask.
  7. Click return.
  8. From the Analyze ribbon, Loads tool group, click the Apply Forces tool.


    Figure 18.
    The Forces panel opens.
  9. Verify the entity selector is set to nodes.
  10. Select the two nodes in the center of the two bolt holes as indicated in Figure 19.


    Figure 19.
  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.


    Figure 20.
  14. Click return to exit the Forces panel.


    Figure 21.

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 22.
  2. For Name, enter Step1.
  3. For Loadcol IDs, click the three dots.


    Figure 23.
  4. In the Advanced Selection dialog, select constraints and force1.


    Figure 24.
  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. Review the Load Collectors and Load Steps you created.


    Figure 25.
  9. Optional: If necessary, click View > Solver Browser 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. In the panel area, click Analysis > 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 26.
  3. Click return.


    Figure 27.
  4. Because you are solving the model for static analysis, click ANTYPE.


    Figure 28.
  5. Set type to STATIC and status to NEW.


    Figure 29.
  6. Click return.
  7. Click LSSOLVE.


    Figure 30.
    Tip: If you do not see the LSSOLVE Control Card, click next.
  8. Enter 1 in the LSMIN field as indicated in Figure 31.
    The minimum number of load steps is set.
  9. Enter 3 in the LSMAX field as indicated in Figure 31.
    The maximum number of load steps is set.
  10. Enter 1 in the LSINC field as indicated in Figure 31.
    The load step increment is set.


    Figure 31.
  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. Navigate to your working directory and save the file as 4410_export.cdb.
  3. In the Solver Export Options dialog, click Export.