HM-4450: Introduction to HyperBeam

In this tutorial, you will learn how to:

•	Assign a standard beam section using the Section panel.

•	Assign the arbitrary beam section using the HyperBeam panel.

•	Couple degrees of freedom.

The steps involved include:

•	Loading the ANSYS user profile

•	Retrieving the HyperMesh model files for this tutorial

•	Adding element types

•	Creating collectors

•	Creating beam elements

•	Coupling DOF – Rigid elements creation

•	Creating standard circular beam sections

•	Creating arbitrary beam sections

•	Updating component collectors with respective beam section collectors

The following images are a pictorial representation of the original model. The model can be simplified in such a way that you can extract represent the entire model with a set of shell elements representing the plate part of the model and two lines indicating the beam.

hm-4450-5b

hm-4450-5

Model Files

This exercise uses the chapter3.hm file, which can be found in <hm.zip>/interfaces/ansys/. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Load the ANSYS User Profile

1.	Start HyperMesh Desktop.

2.	In the User Profile dialog, set the user profile to Ansys.

Step 2: Retrieve the HyperMesh Model File

1.	From the menu bar, click File > Open > Model.

2.	In the Open Model dialog, open the chapter3.hm file. The model shown above displays in the graphics area.

This model contains a plate collector containing shell elements. The plate component is updated with the necessary element type, real constant, and material properties.

hm-4450-6

3.	If your model's elements and mesh lines are not shaded, click on the Visualization toolbar.

Step 3: Create Collectors and Attach Element Types and Materials to Them

1.	In the Model browser, right-click and select Create > Component from the context menu. HyperMesh creates and opens a component in the Entity Editor.

hm-4450-7

2.	For Name, enter beam_std.

3.	Click the Color icon, and select a color.

4.	Right-click on Type and select Create from the context menu. The Create Sensors dialog opens.

hm-4550-8

5.	Set Element Type to BEAM188.

hm-4450-8

6.	Click Close.

7.	For Material, click Unspecified >> Material.

8.	In the Select Material dialog, select Steel and then click OK.

hm-4450-10

9.	In the Model browser, right-click and select Create > Component from the context menu. HyperMesh creates and opens a component in the Entity Editor.

10.	For Name, enter beam_asec.

11.	Click the Color icon, and select a new color.

12.	For Type, click Unspecified >> Sensor.

hm-4450-2

13.	In the Select Sensor dialog, select sensor1 (BEAM188) and then click OK.

hm-4450-9

14.	For Material, click Unspecified >> Material.

15.	In the Select Material dialog, select Steel and then click OK.

Step 4: Create a Beam Element

In the Model browser, notice that the current component is beam_asec.

hm-4450-13

1.	Opens the Bars panel by clicking Mesh > Create > 1D Elements > Bars from the menu bar.

2.	Go to the bar2 subpanel.

3.	Set orientation to plane.

4.	Set Beam Y Axis to parallel to XY.

hm-4450-14

5.	Using the node A and node B selectors, select the two nodes that form the ends of the Arbitary_Beam_Section line as indicated in the following image. HyperMesh creates a BEAM188 element.

Note:

Arbitary_Beam_Section is shown as a tag in the graphics area.

hm-4450-15

6.	In the Model browser, Component folder, right-click on beam_std and select Make Current from the context menu.

7.	Using the node A and node B selectors, select the two nodes that form the ends of the Std_circular_Beam_sec line as indicated in the following image. HyperMesh creates a BEAM188 element.

hm-4450-16

8.	Click return to exit the bar2 panel.

Step 5: Create Coupled DOF - Rigid Elements

1.	Open the Rigids panel by clicking Mesh > Create > 1D Elements > Rigids from the menu bar.

2.	Set the dependent selector to multiple nodes.

3.	Select all of the dof checkboxes.

hm-4450-18

4.	Set elem types to CERIG.

5.	In the Model browser, Component folder, right-click on beam_asec and select Make Current from the context menu.

6.	Activate the independent selector set to node.

7.	On Arbitary_Beam_Section, select the independent node at the end of the beam element as indicated in the following image.

hm-4450-19

8.	Click dependent: nodes >> by path.

9.	On the plate component, select the dependent nodes indicated in the following image.

hm-4450-20

10.	Click create.

hm-4450-21

11.	In the Model browser, Component folder, right-click on beam_std and select Make Current from the context menu.

12.	Activate the independent selector set to node.

13.	On Std_circular_Beam_sec, select the independent node at the end of the beam element as indicated in the following image.

hm-4450-22

14.	Click dependent: nodes >> by path.

15.	On the plate component, select the dependent nodes indicated in the following image.

hm-4450-23

16.	Click create.

hm-4450-24

17.	Click return to exit the Rigids panel.

Step 6: Create and Attach a Standard Circle Property to a Component

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

2.	Right-click on property and select Create from the context menu. The Create Properties dialog opens.

3.	For Name, enter Circular_Sec.

4.	Set SUBTYPE to CSOLID.

5.	Under SECDATA, enter 15 for R.

6.	Click Close. HyperMesh assigns the property Circular_Sec to the component beam_std.

Step 7: Create an Arbitrary Property

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.

2.	For Name, enter arbi_sec.

3.	Set Card Image to SECTYPE.

4.	In the Model browser, Component folder, click next to beam_std, beam_asec, and Plate to turn off the display of their elements.

Note:

You should only see geometric entities in the graphics area.

hm-4450-27

5.	Open the HyperBeam panel by clicking Properties > HyperBeam from the menu bar.

6.	Go to the solid section subpanel.

7.	Set the entity selector to lines.

8.	Select all of the lines (displayed in gray in the following image) that form the Arbitrary_Beam_Section.

hm-4450-28

9.	Set section base node to centroid.

hm-4450-29

10.	Click create. The HyperBeam Data Model dialog opens, meshes the area enclosed by the selected lines with quadrilateral elements, and calculates the properties using these elements.

hm-4450-30

11.	Return to HyperMesh by clicking File > Exit from the menu bar.

12.	Click return to exit the HyperBeam panel.

13.	In the Model browser, Properties folder, click arbi_sec. The Entity Editor opens and displays the beam section's corresponding data.

14.	For Hyper beam section [OPTIONAL], click Unspecified >> Beamsection.

hm-4450-4

15.	In the Select Beamsection dialog, select solid_section.0 and then click OK.

Step 8: Update the Component Collector with the Beam Section

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

2.	For Property, click Unspecified >> Property.

3.	In the Select Property dialog, select arbi_sec and then click OK. HyperMesh attaches this property to the component.

4.	In the Model browser, click to display all of the entities in the graphics area.

hm-4450-35

Step 9: Save you Work

1.	From the menu bar, click File > Save As > Model.

2.	In the Save Model As dialog, navigate to your working directory and save your file.

Step 10: Export the Deck to ANSYS *.cdb Format.

1.	Open the Export tab by clicking File > Export > Solver Deck from the menu bar.

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 4450_export.cdb.

4.	Click Export.

HM-4450: Introduction to HyperBeam

HM-4450: Introduction to HyperBeam

HM-4450: Introduction to HyperBeam

The steps involved include:

Model Files

Exercise

See Also: