HM-4010: Format Model for Analysis

In this step you will load the OptiStruct user profile.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, select OptiStruct.
3. Click OK.

In this step you will open and view the file, channel_brkt_assem_analysis.hm.

1. Open the model file by clicking File Open Model from the menu bar, or clicking on the Standard toolbar.
2. In the Open Model dialog, open the channel_brkt_assem_analysis.hm file.
   The model appears in the graphics area.

In this step you will review a bracket element to identify what type of OptiStruct element it is, and to see how it will be formatted in the OptiStruct input file.

1. Open the Card Edit panel by clicking on the Collectors toolbar.
2. Set the entity selector to elems.
3. In the graphics area, select an element on the bracket component. The bracket component is blue.
4. Click edit.
   The Card Image opens, and indicates that the selected element is an OptiStruct CQUAD4 or CTRIA3, depending on whether you selected a quad or tria element.

   Note: EID is the element’s ID, PID is the ID of the element’s property, and G(X) is the grid (node) ID that makes up the element. Options specific to the CQUAD4 or CTRIA3 appear in the menu panel area.
5. Close the Card Image by clicking return.
6. Exit the Card Edit panel by clicking return.

In this step you will review and edit the existing steel material’s card image by accessing the card editor from the Model Browser.

1. In the Model Browser, Material folder, click steel.
   The Entity Editor opens and displays the material's corresponding data.

   Note: The card image indicates the material is of OptiStruct type MAT1.

   
   
   Figure 2.

2. In the Entity Editor, NU (Poisson's Ratio) field, change the value from 0.3 to 0.28.

   
   
   Figure 3.

In this step you will define a material collector named aluminum for the bracket.

1. In the OptiStruct, right-click and select Create > Material from the context menu.
   The material opens in the Entity Editor.
2. For Name, type aluminum.
3. Set Card Image to MAT1.
4. For E (Young's Modulus), type 7.0e4.
5. For NU (Poisson's Ratio), type 0.33.

   
   
   Figure 4.

In this step you will define a property collector (PSHELL card image) that will be assigned to the channel component collector.

1. In the Model Browser, right-click and select Create > Property from the context menu.
   HyperMesh creates and opens a property in the Entity Editor.

   
   
   Figure 5.

2. For Name, type channel.
3. Set ard Image to PSHELL.
4. For Material, click Unspecified >> Material.

   
   
   Figure 6.

5. In the Select Material dialog, select steel and then click OK. The material is assigned.

   
   
   Figure 7.

6. For T (thickness), type 3.0.

   
   
   Figure 8.

In this step you will assign the channel property to the channel component.

1. In the Model Browser, Component folder, click channel.
   The Entity Editor open and displays the component's corresponding data.

   
   
   Figure 9.

2. For Property, click Unspecified >> Property.

   
   
   Figure 10.

3. In the Select Property dialog, select channel and then click OK.
   HyperMesh assigns the property channel to the component channel.

   
   
   Figure 11.

In this step you will update the bracket property to have a PSHELL card image, a thickness of 2.0, and the aluminum material.

1. In the Model Browser, Property folder, click bracket.
   The Entity Editor opes and displays the properties' corresponding data.

   
   
   Figure 12.

2. Set Card Image to PSHELL.
3. For Material, click Unspecified >> Material.
4. In the Select Material dialog, select aluminum and then click OK.
   HyperMesh assigns the material aluminum to the property bracket.
5. For T (thickness), type 2.0.

   
   
   Figure 13.

In this step you will calculate the section properties for the bar elements (OptiStruct CBEAM) by using HyperBeam.

1. Open the HyperBeam panel by clicking Properties > HyperBeam from the menu bar.
2. Go to the standard section subpanel.
3. Set the standard section library to HyperBeam.
4. Set the standard section type to solid circle.
5. Click create.
   HyperMesh opens the HyperBeam module.

   Note: The solid, green circle represents the cross section. Under the local coordinate system you should see the number, 10.0000, which is the circle’s radius.

   
   
   Figure 14.

6. Under Parameter Definition, click the Value field next to Radius (r) and change the value from 10 to 3.
   HyperMesh updates the values in the Data pane to reflect the circle's new diameter.
7. In the Model Browser, right-click on circle_section.1 and select Rename from the context menu.
8. In the editable field, rename the section 6mm_Beam_Sect.
9. Close the HyperBeam module and return to your HyperMesh session by clicking File > Exit from the menu bar.
10. Return to the main menu by clicking return.

In this step you will create a property collector named bars_prop for the bar elements (OptiStruct).

1. In the Model Browser, right-click and select Create > Property from the context menu.
   HyperMesh creates and opens a property in the Entity Editor.

   
   
   Figure 15.

2. For Name, type bars_prop.
3. Set Card Image to PBEAM.
4. For Material, click Unspecified >> Material.
5. In the Select Material dialog, select steel and then click OK.
   HyperMesh assigns the material steel to the property bars_prop.
6. For Beam Section, click Unspecified >> Beamsection.

   
   
   Figure 16.

7. In the Select Beam Section dialog, select 6mm_Beam_Sect and then click OK.
   HyperMesh assigns the beam section and populates the parameter fields in the PBEAM card with the data in the 6mm_Beam_Sect beam section.

   
   
   Figure 17.

In this step you will update the CBEAM elements in the bolts component to use the PBEAM property.

1. In the Model Browser, Component folder, click bolts.
   The Entity Editor opens and displays the component's corresponding data.

   
   
   Figure 18.

2. For Property, click Unspecified >> Property.
3. In the Select Property dialog, select bars_prop and then click OK.
   HyperMesh assigns the property bars_prop to the component bolts.

   
   
   Figure 19.

In this step you will define an H3D file to be output from OptiStruct by using the control cards panel.

1. Open the Control Cards panel by clicking Setup > Create > Control Cards from the menu bar.
2. In the Card Image, select the control card FORMAT.
   Note: In the card image, the FORMAT line is set to H3D. This specifies OptiStruct to output results to a Hyper3D (H3D) file, which can be viewed in the HyperView Player. A HTML report file will be output and the H3D file will be embedded in it.

   
   
   Figure 20.

3. In the number_of_formats= field, type 2. A second FORMAT line appears in the card image.
4. In the second FORMAT line, click H3D and then select HM.
   Note: This option specifies OptiStruct to output the results to a HyperMesh binary results file, allowing the results to be post-processed within HyperMesh.

   
   
   Figure 21.

5. Exit to the Control Cards panel by clicking return.
   The FORMAT button is now green, which indicates that the card will be exported to the OptiStruct input file.
6. Return to the main menu by clicking return.

In this step you will export the model to an OptiStruct input file.

1. From the menu bar, click File > Export > Solver Deck.
2. In the File field, click .
3. In the Select OptiStruct File dialog, navigate to your working directory and save the file as channel_brkt_assem_loading.fem.
4. Click Export.
   HyperMesh exports the model as an OptiStruct .fem input file for the solver specified by the current user profile.

In this step you will review the contents of the channel_brkt_assem_loading.fem file.

1. In any text editor, such as Notepad and Wordpad, open the file channel_brkt_assem_loading.fem.
2. Near the top of the file, note the following:
   • The line FORMAT HM, which you specified in HyperMesh
   • The load step (OptiStruct SUBCASE) named pressing_step, which you defined in HyperMesh
   • Under the load step, the load collector IDs (OptiStruct load and constraint set identification numbers)

     
     
     Figure 22.

3. Search for "FORCE."
4. Note the load set identification number for each force (OptiStruct FORCE). It is either 1 or 2 as shown below. These numbers correspond to the numbers under the load steps in the file.

   
   
   Figure 23.

5. Search for "SPC" (HyperMesh constraint).
6. Note the constraint set identification number for each constraint (OptiStruct SPC). It is 2 as shown below, which lists a few of the constraints. This number corresponds to the number under the load steps in the file.

   
   
   Figure 24.

7. Search for the load collector name "pressing_load."
8. Note the load collectors, pressing_load and constraints. Also, note their collector ID and color ID. When the model is imported into HyperMesh, the loads are organized into these load collectors and have these IDs and colors.

   
   
   Figure 25.

9. Close the file.

In this optional step you will save your work.