When you create a boundary condition, you must specify the name of the boundary condition, the step in which to activate the boundary condition, the type of boundary condition, and the region of the assembly to which you want to apply the boundary condition.
To create a boundary condition:
From the main menu bar, select BC
Create.
A Create Boundary Condition dialog box appears with a default name displayed in the Name text field.
Tip:
You can also create a boundary condition using the 
tool in the Load module toolbox.
Type a name for the boundary condition. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select the step in which to activate the boundary condition. Click the arrow next to the Step text field, and select from the list that appears.
From the Category list on the left side of the dialog box, choose the desired category. The Category choices available are dependent upon the type of analysis procedures you are performing.
The Types for Selected Step list on the right side of the dialog box changes to a list of all the available boundary condition types.
From the Types for Selected Step list, select the boundary condition type and click Continue.
If you are creating a connector boundary condition using assembled fasteners, you can click Done in the prompt area to select a wire set from the template model.
The boundary condition editor appears.
Click the arrow next to the Assembled fastener field, and select from the list that appears.
The template model name associated with the assembled fastener is displayed in the editor. The Template set list is populated with the wire sets that are associated with the referenced template model.
Select a wire set from the Template set list. You must ensure that the wire set has a section assignment that has the available components of relative motion for which you want to define velocity.
The appropriate fields for the available components of relative motion are displayed.
For all other boundary condition types, select the region to which you want to apply the boundary condition.
If you are creating a connector displacement, connector velocity, or connector acceleration boundary condition, you must select wires that are associated with a connector section assignment. The best approach for selecting wires is to use the default geometry set name for the wire feature (see “Creating or modifying wire features for multiple connectors,” Section 15.12.9, for more information). If you select multiple wires, you must ensure that the connector sections assigned to the wires in the connector section assignments have the available components of relative motion for which you want to define displacement, velocity, or acceleration. If there are insufficient available components of relative motion for the connector boundary condition, a message appears asking you to select different wires or to change the connection type.
If you are creating a connector material flow boundary condition, you must select endpoints of wires that are associated with a connector section assignment.
If you are creating an Eulerian mesh motion boundary condition, select an Eulerian part instance in the viewport. Otherwise, use one of the following methods to select the region for the boundary condition:
Select a region in the viewport. You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see “Using the angle and feature edge method to select multiple objects,” Section 6.2.3. When you have finished selecting, click mouse button 2.
Tip: You can limit the types of objects that you can select in the viewport by specifying filtering options in the Selection toolbar. See “Using the selection options,” Section 6.3, for more information.
If the model contains a combination of mesh and geometry, you must choose the type of region to which you want to apply the boundary condition. From the prompt area, select one of the following:
Click Geometry to apply the boundary condition to geometry or to a reference point.
Click Mesh to apply the boundary condition to a native or orphan mesh selection.
By default, a set or surface is created that contains the selected objects. You can change this behavior by toggling off the option to create a set or surface in the prompt area. A default name is provided in the prompt area, but you can enter a new name.
To select from a list of existing sets or surfaces, do the following:
Click Sets or Surfaces on the right side of the prompt area. (The name of the button depends on the type of object you are creating. For example, if you are creating a pressure load, a Surfaces button appears.)
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets or surfaces.
Select the set or surface of interest and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets or Surfaces on the right side of the prompt area.
The boundary condition editor appears. The region to which you are applying the boundary condition is highlighted in the viewport.
Enter all of the data necessary to define the boundary condition and click OK.
Note: If you create a connector displacement boundary condition that exceeds the failure criteria for a connector, the connector displacement will be ignored.
On Context from the main menu bar and then click the feature of interest or see “Using the boundary condition editors,” Section 16.10.Symbols appear in the viewport that represent the boundary condition that you just created. For more information, see “Understanding symbols that represent prescribed conditions,” Section 16.5.
