ANSYS Contact Manager

The Contact Manager enables you to manage existing contact pairs and surface elements, and create new contact pairs and ANSYS thermal and structural surface elements.

In the Contacts tab you can review a list of existing contact pairs, and in the Surface Elements tab you can review a list of existing surface element components. Contact pairs are listed according to their target and master components, color, assigned ET type, property cards, material, and pilot node name. You can update the data in any of these columns, as well as modify the element key options, properties, and materials of the contact pairs and surface components. You can view the contact normal and reverse it with the buttons provided in the Contacts table. These features are also available for surface elements.

contact_manager_ansys

You can create 2D and 3D contact pairs with the Surface to Surface and Point to Surface options. You can also define contacts using the Pilot Node option.

1.	From the Utility menu, click Contact Manager. The Ansys Contact Manager opens and the Contact tab is displayed by default.

2.	Click New to create a new contact pair. The Create New Contact Pair dialog opens.

contact_mgr_01

3.	Under Creation method, select Flexible or Pilot node.

4.	In the Contact type field, select 2D or 3D.

5.	Under Create from, select whether to create a surface to surface contact pair or a point to surface contact pair.

6.	Under Symmetric Contact, select Yes or No.

To create two pairs of symmetry contacts, click Yes. In order to create a symmetry pair, the selected elements must meet all of the element configuration requirements.

•	Contact elements in the first pair will be target elements in the second pair.

•	Target elements in first pair will be contact elements in the second pair.

•	Different properties and ET types will be created for the second pair. You can update the contact pair with desired properties and contact options later.

7.	Click Pick Target to select the target body components.

8.	From the panel area, click the comps selector.

9.	Select the components that belong to the target component elements.

10.	Click select.

11.	Click proceed.

12.	In the Target Elements Selection dialog, click the Elements selector.

ansys_auto_contact_02

13.	In the panel area, verify that the elems selector is active, then select the target elements of the contact pair.

14.	Click proceed.

15.	In the Target Elements Selection dialog, click Next. The Target Component Details dialog opens.

This dialog displays a default name and color for the target component, which can both be modified. You can also modify the ET Type name and the ID of the target component, as well as the values of the key options. Once Save Keyopts is clicked, all of your changes will be applied to the target element. The next time you create a new contact pair, the options you selected in the dialog will be saved and you will not need to apply them again.

ansys_auto_contact_03

16.	Click Next.

17.	In the Contact Components Selection dialog, click the Components selector.

18.	In the panel area, click the comps selector.

19.	Select the components to assign as the target body.

20.	Click select.

21.	Click proceed.

22.	Click Next.

23.	In the Select Contact Elements dialog, click the Elements selector.

24.	In the panel area, verify that the elems selector is active, then select the elements to assign as the contact surface elements.

25.	Click proceed.

26.	Click Next. The Contact Component Details dialog opens.

This dialog displays a default name and color for the contact component, which can be modified if desired. The ET type and the ID of the contact component can also be modified.

27.	Click Next.

28.

In the Contact Property dialog, enter the values for items shown. You can create a new property, or create a new one based on an existing property, which helps expedite the process. Click Save real constants to save the property values you entered. In the future, when the Contact Property dialog opens, the values you saved will appear by default.

ansys_auto_contact_04

29.	Click Next.

30.	In the Contact Material dialog, click New to define a new material or select None to skip defining a material.

ansys_auto_contact_05

31.	Click Next. The Ansys Contact Manager dialog opens and displays a summary of the target and contact elements. The contact pair you created is displayed.

32.	To exit the Contact Manager, click Close.

33.	To repeat this process, click Restart.

Surface elements can be created on the edges of plane elements (2D) or on faces of solid elements (3D). Using the Contact Manager, you can create the thermal surface elements SURF151 and SURF152, the structural surface elements SURF153 and SURF154, and the radiosity elements SURF251 and SURF252.

1.	From the Utility menu, click Contact Manager.

2.	In the Ansys Contact Manager, click the Surface Elements tab. A list of existing surface element components displays.

3.	Click New to create new surface elements. The Surface Effect Elements dialog opens.

contact_mgr_surface_elements

4.	From the Element Type field, select the type of surface elements to create.

5.	Select whether to create 2D Surface or 3D Surface elements.

Note:

2D Surface creates surface elements on the edges of a plane element, and 3D Surface creates surface elements on the faces of solid elements.

6.	To create surface elements with extra nodes, select the With Extra Nodes check box.

Note:

With Extra Nodes is only available for thermal surface elements.

7.	If you selected Radiosity Elements as the Element type, you must specify an Emissivity and Enclosure number value to apply to the edges and faces of base elements.

Note:

Radiosity elements require radiation loads to be applied on the faces of the elements over which the skin elements are created. The Contact Manager automatically creates these loads with the emissivity and enclosure values that you specify.

8.	Click Pick Components.

9.	In the panel area, click the comps selector.

10.	Select components on which surface elements will be created.

11.	Click select.

12.	Click proceed.

13.	In the Elements Selection dialog, click the Elements selector.

14.	In the panel area, verify that the elems selector is active, then select elements on which surface elements will be created.

15.	Click proceed.

16.	In the Elements Selection dialog, click Next.

contact_mgr_surface_elements_2

17.	In the Nodes Selection dialog, click the Nodes selector.

Note:

The Nodes Selection dialog only appears if you selected the With Extra Nodes check box.

18.	In the panel area, verify that the Nodes selector is active, then select extra nodes to create surface elements with.

Note:

A maximum of two nodes can be selected.

19.	Click proceed.

20.	In the Nodes Selection dialog, click Next.

21.	In the Surface Element Component Details dialog, select the appropriate key options.

contact_mgr_surface_elements_3

22.	Click Next.

23.	In the Contact Property dialog, define values for the element real sets (properties).

contact_mgr_surface_elements_4

24.	Click Next.

25.	In the Surf Material dialog, click New to create and define a new material or select None to skip defining a material.

Note:

The Surf Material dialog only appears if the surface elements being created needs material properties defined.

contact_mgr_surface_elements_5

26.	Click Next. The Ansys Contact Manager dialog opens and displays the surface elements you created.

1.	To exit the Contact Manager, click Close.

2.	To repeat this process, click Restart.