Element Based Surface: Define Tab

3D Solid or Gasket Elements

Use the 3D solid or gasket elements option to define the *SURFACE card by specifying face identifiers for individual solid and gasket elements.

These faces are displayed by special face elements.

In order to create surface, you need to select the underlying solid or gasket elements first.

Click Elements to open the Element Selector panel, and then select the underlying 3D solid or gasket elements from the graphic area. Selected elements are highlighted. Click Reset to resets the selected elements.

You can then define the face identifiers for the selected solids in two ways: (a) by creating a solid skin and manually picking the faces from the skin, (b) by picking nodes on a specific face and sweeping through a break angle. Under Select faces by, select Solid skin for (a) and Nodes on face for (b).

(a) Solid skin enables the following:

Table 1.
Button	Action
Faces	Creates a temporary skin of the selected solids. Opens the Element Selector panel, from which you can select face elements from this skin. The selected faces are highlighted. Click Reset to reset the selected faces and delete the skin. Note: by face on the element selector panel can be used to find all faces within a feature angle of the selected face. The feature angle setting can be accessed by clicking Preferences > Geometry Options. The skin will initially have the same color as the current surface. You can change the skin color using Solid skin color button.
Add	Adds the selected faces to the current surface and creates special face elements for display. It also checks for duplicate faces and displays a message if any are found. Note: The Delete Face tab contains tools to find and delete duplicate faces in the current surface.
Reject	Rejects the recently added faces.

(b) Nodes on face enables the following:

Table 2.
Button	Action
Nodes	Opens the Node Selector panel, from which you can select nodes from the graphic area. Three nodes (or two corner nodes) from the same solid element must be picked to define a face of that solid. The selected nodes are highlighted. The corresponding Reset button resets the selected nodes. Note: Several three-node or two-corner-node sets can be selected at the same time to define faces in different solids.
Add	Finds all faces from the selected solids that fall within a specified break angle of the face(s) defined by nodes. These faces are then added to the current surface and create special face elements for display. It also checks for duplicate faces and displays a message if any are found. Note: The Delete Face tab contains tools to find and delete duplicate faces in the current surface.
Reject	Rejects the recently added faces.

3D Shell, Membrane or Rigid Elements

Use the 3D shell, membrane, and rigid elements option to define the *SURFACE card by specifying face identifiers for individual shell, membrane, and rigid elements.

In the graphics area, these faces are displayed by special face elements. These face elements have their own normals to define the SPOS and SNEG faces. The face with normals along the underlying element normals define the SPOS faces. In contrast, the face with opposing normals define the SNEG face.

The 3D shell, membrane, or rigid elements enable the following:

Table 3.
Button	Action
Elements	Opens the Element Selector panel, from which you can select underlying 3D shell, membrane, or rigid elements from the graphic area. The selected elements are highlighted and their normals are displayed. The corresponding Reset button resets the selected elements and hides the normals.
Add	Adds the selected elements to the current surface and creates special face elements for display. It also checks for duplicate faces and displays a message if any are found. By default, SPOS faces are created. In order to create SNEG faces, activate the Reverse checkbox and click Add.
Reject	Rejects the recently added faces.

3D Solid Coated with Shell

Use the 3D solid coated with shell option to define the *SURFACE card by specifying face identifiers for these 3D solid or gasket elements.

In HyperMesh, surfaces on 3D solid or gasket elements that are coated with shell, membrane, or rigid elements are treated differently from surfaces on regular solids.

The faces are displayed by special contactsurface elements. Unlike, regular solids, there is only one way to define the face identifiers for solids with shell coating: by picking nodes on a specific face and sweeping through a break angle. Therefore, the Nodes on face option is always selected. This option is valid for Standard.3D template or 3D models in Explicit template only.

3D solid coated with shell enables the following:

Table 4.
Button	Action
Elements	Opens the Element Selector panel, from which you can select underlying 3D solid and gasket elements from the graphic area. The selected elements are highlighted. The corresponding Reset button resets the selected elements.
Nodes	Opens the Node Selector panel, from which you can select nodes from the graphic area. Three nodes (or two corner nodes) from the same solid element must be picked to define a face of that solid. The selected nodes are highlighted. The corresponding Reset button resets the selected nodes. Note: Several three-node or two-corner-node sets can be selected at the same time to define faces in different elements.
Add	Finds all faces from the selected 3D solids that fall within a specified break angle of the face(s) defined by nodes. These faces are then added to the current surface and special contactsurface elements are created for display. Note: You cannot add duplicate contactsurfaces for the same element in HyperMesh. Therefore, the Add button does not check for duplicates and there is no Reject button.

3D Shell - Edge Based

Use the 3D shell – edge based option to define the *SURFACE card by specifying edge identifiers for 3D shell elements.

The edges are displayed by special contactsurface elements. Face identifiers for solids with shell coating are defined by picking nodes on a specific edge and sweeping through a break angle. Therefore, the Nodes on edge option is always selected.

3D shell – edge based enables the following:

Table 5.
Button	Action
Elements	Opens the Element Selector panel, from which you can select underlying 3D shell elements from the graphic area. The selected elements are highlighted. The corresponding Reset button resets the selected elements.
Nodes	Opens the Node Selector panel, from which you can select nodes from the graphic area. Two nodes from the same solid element must be picked to define a edge of that shell. The selected nodes are highlighted. The corresponding Reset button resets the selected nodes. Note: Several two-node sets can be selected at the same time to define edges in different elements.
Add	Finds all edges from the selected 3D shells that fall within a specified break angle of the edge(s) defined by nodes. These edges are then added to the current surface and special contactsurface elements are created for display. Note: You cannot add duplicate contactsurfaces for the same element in HyperMesh. Therefore, the Add button does not check for duplicates and there is no Reject button.

2D Solid, Axisymmetric or Gasket Elements

The 2D solid, axisymmetric or gasket elements option is valid for Standard.2D template or 2D models in Explicit template only.

Use it to define the *SURFACE card by specifying edge identifiers for individual 2D solid, axisymmetric, and gasket elements. In the graphic area, these edges are displayed by special contactsurface edge elements. Unlike, 3D solids, there is only one way to define the face identifiers for 2D solids: by picking nodes on a specific edge and sweeping through a break angle. Therefore, the Nodes on edge option is always selected.

2D solid, axisymmetric, or gasket elements enable the following:

Table 6.
Button	Action
Elements	Opens the Element Selector panel, from which you can select underlying 2D solid, axisymmetric, and gasket elements from the graphic area. The selected elements are highlighted. The corresponding Reset button resets the selected elements.
Nodes	Opens the Node Selector panel, from which you can select nodes from the graphic area. Two nodes from the same element must be picked to define an edge of that element. The selected nodes are highlighted. The corresponding Reset button resets the selected nodes. Note: Several node pairs can be selected at the same time to define edges in different element.
Add	Finds all edges from the selected 2D solids that fall within a specified break angle of the edge(s) defined by nodes. These edges are then added to the current surface and special contactsurface edge elements are created for display. Note: You cannot add duplicate contactsurface edges for the same element in HyperMesh. Therefore, the Add button does not check for duplicates and there is no Reject button.

Beam, Pipe or Truss Elements

Use the Beam, pipe or truss elements option to define the *SURFACE card for individual beam, pipe and truss elements.

In the graphic area, these faces are displayed by special contactsurface elements. These contactsurface elements have their own normals to define the SPOS and SNEG faces. The contactsurface with normals along the underlying element normals define the SPOS faces. In contrast, the face with opposing normals defines the SNEG face.

Note: For 3D beam, pipe and truss elements, the SPOS and SNEG faces do not have any meaning. Therefore, these face identifiers will be ignored by the Standard.3d template.

Beam, pipe, or truss elements enables the following:

Table 7.
Button	Action
Elements	Opens the Element Selector panel, from which you can select underlying beam, pipe or truss elements from the graphic area. The selected elements are highlighted. The corresponding Reset button resets the selected elements.
Add	Adds the selected elements to the current surface and creates special contactsurface elements for display. By default, SPOS faces are created. In order to create SNEG faces, activate the Reverse check box and click Add. Note: You cannot add duplicate contactsurfaces for the same element in HyperMesh. The Add button does not check for duplicates and there is no Reject button.

Element Set

Use the Element set option to define the *SURFACE card for element sets.

Only one elset is allowed in a surface. It does not support a combination of elsets and individual elements in the same *SURFACE data line.

The Element set menu contains a list of the existing elsets. You can also use the … button to open the Entity Browser to select an elset. There are two types of elsets in HyperMesh: Components and Entity sets. The Abaqus elsets that are linked to sectional property cards, such as *SOLID SECTION and *SHELL SECTION, become components in HyperMesh. Others become entity sets. To differentiate between these two types, there is a divider line "- - - - -" in the elset lists that pops up if you click the Element set menu. The elsets listed below the divider line are components.

Element set option enables the following:

Table 8.
Button	Action
Review Set	Reviews the selected elsets set by highlighting them in the the graphic area. Right-click on Review to clear the review selections.
Create/Edit Sets...	Opens the Entity Sets panel. When you finish creating/editing the set, click return. The Element Based Surface tab is updated with the new set appearing in the element set list.
Show Faces	Creates a temporary skin of the selected elset, opens the element selector panel, from which you can select face elements from this skin. When you return from the Element Selector panel, the selected faces will display color coded face identifier tags. In the graphic area, these tags are sometimes blocked by the solid mesh. You may need to rotate the model a little to view the tags.
Update	Adds the selected elset into the current surface. By default, HyperMesh does not create a display for surfaces defined with elsets. However, if you check the Display option before clicking Update, it creates a special display using contactsurface elements. Note: The special display created with contactsurface elements does not have links to the elset in the HyperMesh database. Therefore, if you edit the elset later on, the display will not automatically reflect your changes. In this case, check the Display option and click Update again.

After selecting an element set, click the arrow keys to move the set into table on the right. Once an elset has been added to the table, the face column becomes activated and you can manually define the appropriate face identifier for the selected elset. Select None if you do not want to define a face identifier for the set. In this case, Abaqus will create a surface with the free faces for the selected element set.