17.6.3.9. Fixed Rotation

You can apply a Fixed Rotation boundary condition to faces, edges, and vertices of a surface body. When you only apply a Fixed Rotation support to a surface body, the geometry is free in all translational directions. However, by default, the rotation of the geometry is fixed about the axes of the corresponding coordinate system.

Note:  

  • Rotation constraints are combined with other constraints that produce rotational DOF assignments to determine which values to apply. They are combined with all other constraints to determine the Nodal Coordinate System orientation (frictionless supports, cylindrical supports, given displacements, etc.).

  • There may be circumstances in which the rotational support and other constraints cannot resolve a discrepancy for preference of a particular node’s coordinate system.

This page includes the following sections:

Analysis Types

Fixed Rotation is available for the following analysis types:

Dimensional Types

The supported dimensional types for the Fixed Rotation boundary condition include:

  • 3D Simulation

Geometry Types

The supported geometry types for the Fixed Rotation boundary condition include:

  • Surface/Shell: Supported for Surface Body only.

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Fixed Rotation include:

  • Face

  • Edge

  • Vertex

    • A fixed vertex rotation support is not realistic and leads to singular stresses (that is, stresses that approach infinity near the fixed vertex rotation support). You should disregard stress and elastic strain values in the vicinity of the fixed vertex rotation support.

    • This boundary condition cannot be applied to a vertex scoped to an end release.

Applying a Fixed Rotation Boundary Condition

To apply a Fixed Rotation:

  • In the Details pane, select Free or Fixed for Rotation X, Rotation Y, and Rotation Z to define the Fixed Rotation support.

  1. On the Environment Context tab: click Supports>Fixed Rotation. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Fixed Rotation.

  2. Specify Scoping Method and Geometry or Named Selection.

  3. As needed, specify the coordinate system for the corresponding rotational constraint.

  4. Define the rotational axes as Fixed (default) or Free.

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: Options include:

  • Geometry Selection - Default setting, indicating that the boundary condition is applied to a geometry or geometries, which are chosen using a graphical selection tool.

    • Geometry - Visible when the Scoping Method is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) and the number of geometric entities (for example: 1 Body, 2 Edges) to which the boundary has been applied using the selection tools.

  • Named Selection - Indicates that the geometry selection is defined by a Named Selection.

    • Named Selection - Visible when the Scoping Method is set to Named Selection. This field provides a drop-down list of available user-defined Named Selections.

Definition

Type - Read-only field that describes the object - Fixed Rotation.

Coordinate System - Drop-down list of available coordinate systems. Global Coordinate System is the default.

Rotation X - Fixed (default) or Free.

Rotation Y - Fixed (default) or Free.

Rotation Z - Fixed (default) or Free.

Suppressed - Include (No - default) or exclude (Yes) the boundary condition.

Caution:  When parameterizing this boundary condition, a Free axis of rotation is represented by a one (1) and Fixed with a value of zero (0) inside the Parameter tab in Ansys Workbench (outside of Mechanical). Entering any value other than 0 or 1 causes the application to produce unexpected results.

API Reference

For specific scripting information, see the Fixed Rotation section of the ACT API Reference Guide.