Load Step: Boundary

Load Step: Boundary: Define Tab

In the Define tab, define *BOUNDARY cards on individual nodes or geometry (surfaces, points, lines). You can also define the boundary on node sets.

There are five different types of boundary conditions available:

Table 1.
Boundary Types	Abaqus Keyword
Default (disp)	*BOUNDARY
Velocity	*BOUNDARY, TYPE = VELOCITY
Acceleration	*BOUNDARY, TYPE = ACCELERATION
Temperature	*BOUNDARY on dof 11
Electric potential	*BOUNDARY on dof 9

It is recommended that you use only one boundary type per load collector in HyperMesh. If you need to use multiple boundary types in the same STEP, define each type in a separate load collector and add them to the same load step.

You can define a *BOUNDARY card on nodes/geometry or on node sets. For Define Boundary on:, the following options are available:

Nodes or geometry
Node sets

The layout of the Define tab changes, based on your selection.

Define Boundary On: Nodes or Geometry

Use the Define Boundary on: Nodes or geometry option to define various types of boundaries on individual nodes or geometry.

Boundaries created on nodes have a special graphical display in HyperMesh. Loads created on geometric entities like surfaces, lines or points are automatically mapped to FEA mesh on export. You can also map them using the Map Loads on Geometry button.

The Define tab for Define Boundary on: Nodes or geometry has the following buttons:

Table 2.
Button	Action
Define from 'Contraints' panels	Opens the Constraints panel to create/update boundary conditions. To create a boundary on nodes, go to the create subpanel, select the nodes button, pick the desired nodes from HyperMesh graphics, check the constrained degrees of freedoms, and click create. To create a boundary on geometry, go to the create subpanel, select surfs, points, or lines using the switch, pick the desired geometry from the HyperMesh graphics, check the constrained degrees of freedom, and click create. Note: Loads created on geometric entities are automatically mapped to FEA mesh on export. You can also map them using the Map Loads on Geometry button. An existing boundary can be updated from the updatesubpanel. While you are in the constraints panel, press the H key to view panel-specific help. When you are finished creating or updating boundary conditions, click return to update the Step Manager with the new loads.
Map Loads on Geometry	Opens the HyperMesh loads on geom panel to map loads on geometry to FEA mesh entities. Click Map loads to map all geometric loads in the current load collector to FEA entities. Note: You can also pick other load collectors by clicking the loadcols button and map loads in all of them together. While you are in the loads on geom panel, press the H key to view panel-specific help. When you are finished, click return to update the Step Manager with the new loads.

Define Boundary On: Node Sets

The Define Boundary on: Node sets option defines various types of boundaries on node sets.

The node set names are used in the *BOUNDARY data lines instead of the individual nodes. Unlike Abaqus surfaces in HyperMesh, you can combine node sets with individual node IDs in the same *BOUNDARY card.

Note: HyperMesh does not graphically display loads created on sets. Therefore, when you review a load collector in the Step Manager, only loads created on individual entities are highlighted. For loads defined on sets, the underlying nodes or elements are highlighted.

This dialog contains a Node sets menu with a list of the existing node sets. It also has a table for data line input containing the following columns:

Table 3.
Column	Description
Nset	The name of the node sets. Node sets can only be added or deleted from this column using the → or ← buttons, respectively.
1st dof	The first degree of freedom. You can input any integer or any of the following types in this column: XSYMM, YSYMM, ZSYMM, ENCASTRE, PINNED, XASYMM, YASYMM, ZASYMM, NOWARP, NOOVAL, NODEFORM
Last dof	The last degree of freedom
Magnitude	The magnitude
Load ID	The ID of the load collector

The Define tab for Define Boundary on: Node sets contains the following buttons:

Table 4.
Button	Action
Review Set	Reviews the selected node sets by highlighting them in the HyperMesh graphics. Right-click the Review button to clear the review selections.
Create/Edit Set	Opens the Entity Sets panel in HyperMesh. When you finish creating/editing the set, click return. The Step Manager is updated with the new set appearing in the element set list.
→	Add the selected node set from the pull down menu to the data line table on the right.
←	Delete the selected node set from the data line table.
Review	Reviews the selected node set in the data line table. Right-click Review to clear the highlighted selections.
Update	Updates the HyperMesh database with the data lines defined in the table. By default, HyperMesh does not create a display for loads defined with sets.
Display/Review from panel	Opens the appropriate HyperMesh panel. Use the Review button to expand the loads and constraints on the sets for visualization purposes.

For tips on entering information and navigating in the Define tab, see Step Manager Tab Environment.

Load Step: Boundary: Delete Tab

In the Delete tab, delete boundaries and other loads from HyperMesh.

There are three options:

Table 5.
Option	Description
All loads in current collector	The Delete button deletes all the loads from the current load collector.
All 'Boundary' in current collector	The Delete button deletes only *BOUNDARY loads from the current load collector.
By selection	The Pick Loads button opens the HyperMesh load selector panel. Pick the loads you want to delete and click proceed. The corresponding Reset button resets the selected loads. The Delete button deletes the selected loads.

Load Step: Boundary: Parameter Tab

In the Parameter tab, define optional parameters for the *BOUNDARY card.

The supported parameters are: Amplitude, OP, Load Case, Fixed, and Region Type.

Click Update to activate the optional parameter selection in the HyperMesh database.