Using Nodal Displacement, 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 Nodal Displacement.
This page includes the following sections:
| Analysis Types |
| Dimensional Types |
| Geometry Types |
| Topology Selection Options |
| Applying a Nodal Displacement Boundary Condition |
| Details Pane Properties |
| API Reference |
Analysis Types
Nodal Displacement is available for the following analysis types:
|
Dimensional Types
The supported dimensional types for the Nodal Displacement boundary condition include:
3D Simulation
2D Simulation
Geometry Types
The supported geometry types for the Nodal Displacement boundary condition include:
Solid
Surface/Shell
Wire Body/Line Body/Beam
Topology Selection Options
The Nodal Displacement boundary condition is scoped via node-based Named Selections only. For more information, see the Specifying Named Selections by Direct Node Selection Help section.
Note: The Nodal Displacement 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.
Applying a Nodal Displacement Boundary Condition
To apply a Nodal Displacement:
On the Environment Context tab, click >. Alternatively, 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.
As needed, set the Rev Dir for Inv Steps property to . See the description below for requirements.
Tip: Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System.
Details Pane Properties
The Details pane selections are described below.
| Category | Property/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 . Rev Dir for Inv Steps: This property is only available when the following Advanced Analysis Settings properties are defined:
Options include (default) and . Setting this property to inverts the direction of your specified Nodal Displacement. Suppressed: Includes or excludes the boundary condition in the analysis. |
Note:
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 the 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.
API Reference
For specific scripting information, see the Nodal Displacement section of the ACT API Reference Guide.