17.6.3.6. Compression Only Support

Applies a compression only constraint normal to one or more faces. It is modeled internally using Asymmetric rigid-flexible contact. A rigid target surface is constructed and/or mirrored from the scoped faces/edges of the Compression Only Support. Therefore, the following points should be kept in mind:

  • The underlying technology is using penalty-based formulations. As a result, normal contact stiffness can be an important parameter if nonlinear convergence issues arise. Control normal contact stiffness using the Normal Stiffness property of the Compression Only Support object.

  • Because source and target topologies are perfect mirrors of one another, be careful during nonlinear analyses to make that contact doesn't "fall off" the target face. Be sure that the contact area on the rigid body is large enough to accommodate any potential sliding taking place during the analysis. To avoid this, consider using a fully fixed rigid body and a nonlinear contact to replace the Compression Only Support.

Consider the following model with a bearing load and supports as shown.

 

Note the effect of the Compression Only Support in the animation of total deformation.

The following demo is presented as an animated GIF. View online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product.

 

Since the region of the face in compression is not initially known, a nonlinear solution is required and may involve a substantial increase in solution time.

This page includes the following sections:

Analysis Types

Compression Only Support is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Compression Only Support boundary condition include:

  • 3D Simulation

  • 2D Simulation

Geometry Types

The supported geometry types for the Compression Only Support boundary condition include:

  • Solid

Topology Selection Options

The supported topology selection options for Compression Only Support include:

  • Face: Supported for 3D only.

  • Edge: Supported for 2D only.

Applying a Compression Only Support Boundary Condition

To apply a Compression Only Support:

  1. On the Environment Context tab, click Supports>Compression Only Support. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Compression Only Support.

  2. Specify Scoping Method and Geometry or Named Selection.

  3. Specify Normal Stiffness property. If set to Manual, enter a Normal Stiffness Factor value.

  4. Specify Update Stiffness property.

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 - Compression Only Support.

Normal Stiffness: Defines a contact Normal Stiffness factor. Options include:

  • Program Controlled: This is the default setting. The Normal Stiffness Factor is calculated by the program.

  • Manual: The Normal Stiffness Factor is input directly by the user. The Normal Stiffness Factor property displays for this setting.

Update Stiffness: Specify if the program should update (change) the contact stiffness during the solution. Options include:

  • Never: This is the default setting. Turns off the program's automatic Update Stiffness feature.

  • Each Iteration: Sets the program to update stiffness at the end of each equilibrium iteration.

  • Each Iteration, Aggressive: Sets the program to update stiffness at the end of each equilibrium iteration, but compared to the option, Each Iteration, this option allows for a more aggressive changing of the value range.

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

API Reference

For specific scripting information, see the Compression Only Support section of the ACT API Reference Guide.