Using , you can apply a displacement to an individual node or a set of nodes. You must create a node based named selection before you can apply a .
is available for the following analysis types:
Eigenvalue Buckling (for Nonlinear-based Eigenvalue Buckling Analysis only)
The following section outlines the common boundary condition characteristics that include application requirements of the boundary condition, support limitations, as well as loading definitions and values.
Dimensional Types
3D Simulation: Supported.
2D Simulation: Supported.
Geometry Types: Geometry types supported for the boundary condition include:
Solid: Supported.
Surface/Shell: Supported.
Wire Body/Line Body/Beam: Supported.
Topology: The boundary condition is scoped via node-based Named Selections only. See the Specifying Named Selections by Direct Node Selection Help section for more information.
Note: The boundary condition supports spatially varying loading on the scoped nodes for Static and Transient analyses only. For Eigenvalue Buckling, Harmonic Response, and Modal analyses, only constant loading conditions are supported.
To apply a :
On the Environment toolbar, click >. Or, right-click the Environment tree object or right-click within the Geometry window and select >.
Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the Nodal Displacement.
Define loads in the X, Y, and/or Z directions.
Tip: Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System.
The Details View selections are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method: read-only field that displays scoping method - Named Selection . Named Selection: drop-down list of available node-based Named Selections. |
| Definition |
Type: read-only field that displays boundary condition type - . Coordinate System: read-only field that displays the coordinate system - Nodal Coordinate System. X Component: specify a displacement value in the X direction. The default value is (no Displacement constraint applied). Y Component: specify a displacement value in the Y direction. The default value is (no Displacement constraint applied). Z Component: specify a displacement value in the Z direction. The default value is (no Displacement constraint applied). You can define the Component values as a , in form as a function of varying Time or varying Step (Static Structural only), or as a . Suppressed: includes or excludes the boundary condition in the analysis. |
Solution Restarts are only supported for Tabular data modifications.
If a Component property is set to , all other Components properties automatically default to the setting and become read-only.
Two Nodal Displacement objects that have same scoping do not produce a cumulative loading effect. The Nodal Displacement object that was specified last takes priority and is applied, and as a result, the other Nodal Displacement object is ignored. For Explicit Dynamics analyses, the compatibility of multiple Nodal Displacements applied to a node must be respected. The solver will attempt to combine the constraints, but if this is not possible, the solve will fail with an appropriate error message.