End Releases

For line body models, the End Release feature enables you to free the degrees of freedom (translation and rotation) at a vertex that is shared by two or more edges. You can free the constraint of multiple edges at the vertex’s location, however, you must always keep at least one edge from being released.

Deformation results for a pin-jointed beam-based truss are shown in the following illustrations. The loading is standard earth gravity. These examples illustrate some basic scoping scenarios.

Here is the Deformation with no End Release applied to the truss.

This illustration depicts the Deformation of the truss with an End Release applied to the vertex and one edge.

Here is the Deformation with an End Release applied to two independent edges.

Here is the Deformation with an End Release applied to the same two edges except that they are not independent.

To add an End Release:

  1. Add a Connections folder if one is not already in the tree, by highlighting the Model object and selecting Connections from the Model Context Toolbar or by choosing Insert >Connections from the context menu (right-click).

  2. Add an End Release object by highlighting the Connections folder and selecting End Release from the Connections Context Toolbar or by choosing Insert >End Release from the context menu (right-click).

  3. Specify the Scoping Method as Geometry Selection (default) or Named Selection.

  4. Specify the Vertex Geometry and the Edge Geometry, respectively. The vertex must be one of the end points of the selected edge or edges.

  5. If you specified more than one edge for the Edge Geometry property, use the Independent Edges property to specify whether the edges are independent of one another (Yes - default) or fixed together (No).

  6. Specify the Coordinate System as the Global Coordinate System or a local user-defined coordinate system.

  7. Specify the translational and/or rotational degrees of freedoms in X, Y and Z directions by changing axial properties from Fixed to Free.

  8. Based upon the configuration of your model, specify the connection Behavior property as either Coupled (default) or Joint. This property uses coupling or a general joint, respectively.

Notes


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