Nodal Displacement

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.

Analysis Types

Nodal Displacement is available for the following analysis types:

Common Characteristics

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

Geometry Types: Geometry types supported for the Nodal Displacement boundary condition include:

Topology: The Nodal Displacement 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 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.


Boundary Condition Application

To apply a Nodal Displacement:

  1. On the Environment toolbar, click Direct FE>Nodal Displacement. Or, right-click the Environment tree object or right-click within the Geometry window and select Insert>Nodal Displacement.

  2. Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the Nodal Displacement.

  3. 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.


Details View Properties

The Details View selections are described below.

CategoryFields/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 - Displacement.

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 Free (no Displacement constraint applied).

Y Component: specify a displacement value in the Y direction. The default value is Free (no Displacement constraint applied).

Z Component: specify a displacement value in the Z direction. The default value is Free (no Displacement constraint applied).

You can define the Component values as a Constant, in Tabular form as a function of varying Time or varying Step (Static Structural only), or as a Function.

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 Function, all other Components properties automatically default to the Free 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.



Release 18.2 - © ANSYS, Inc. All rights reserved.