Introduction

All geometry Bodies have an associated Stiffness Behavior property in Ansys Mechanical that you can modify during an analysis. The available behavior options can be accessed from within the Mechanical tree under the details of the geometry body, as shown in the image below.

Four behavior options are available : Flexible, Rigid, Gasket, Flexible Beam and Rigid Beam. Note that the last two are beta options and will only be visible if you turn on workbench beta options (You can turn on beta options by going to Workbench, Tools, Appearance and check beta options).

In this article, we will briefly explain what each of the stiffness option represents.

Flexible Behavior

This is the default behavior option in Ansys Mechanical. This implies that the body can deform during the analysis and stresses and strains can develop within the body.

Rigid Behavior

When you define a body’s Stiffness Behavior as Rigid, you are telling to the application to not allow the body to deform during the solution process. This feature is useful if a mechanism has only rigid body motion or, if in an assembly, only some of the parts experience most of the strains. It is also useful if you are not concerned about the stress/strain of that component and wish to reduce CPU requirements during meshing or solve operations.

The application does not mesh a rigid body and the solver represents the body as a single mass element. However, the system maintains the mass element’s mass and inertial properties. The Mass, Centroid, and Moments Of Inertia properties for the body are available in the Details view of the body object.

The following restrictions apply to rigid bodies:

1. Rigid bodies are only valid in Static Structural, Transient Structural, Harmonic Response, Modal, Rigid Dynamics, Random Vibration, and Response Spectrum analyses for the objects listed below:

• Point Mass
• Joint
• Spring
• Remote Displacement
• Remote Force
• Moment
• Contact

2. Rigid bodies are valid when scoped to solid bodies, surface bodies, or line bodies in an Explicit Dynamics analysis for the following objects:

• Fixed Support
• Displacement
• Velocity
• Spring
• Remote Displacement

3. The following outputs are available for rigid bodies, and are reported at the centroid of the rigid body:

• Results: Displacement, Velocity, and Acceleration.
• Probes: Deformation, Position, Rotation, Velocity, Acceleration, Angular Velocity, and Angular Acceleration.

Note:

• If you highlight Deformation results in the tree that are scoped to rigid bodies, the corresponding rigid bodies in the Geometry window are not highlighted.
• You cannot define a line body, 2D plane strain body, or 2D axisymmetric body as rigid, except that in an Explicit Dynamics analysis, 2D plane strain and 2D axisymmetric bodies may be defined as rigid.
• All bodies in a body group (of a multibody part) must have the same Stiffness Behavior. When Stiffness Behavior is Rigid, the body group acts as one rigid mass regardless of whether or not the underlying bodies are topologically connected (via shared topology).

Gasket Behavior

Gasket joints are essential components in most structural assemblies. Gaskets as sealing components between structural components are usually very thin and made of various materials, such as steel, rubber and composites. From a mechanics perspective, gaskets act to transfer force between components. The primary deformation of a gasket is usually confined to one direction, namely, through thickness. The stiffness contribution from membrane (in-plane) and transverse shear are much smaller, and are neglected.

When a body is defined as a gasket, only one element is meshed through its thickness and the through thickness deformation is decoupled from the in plane deformation. The gasket material is usually under compression. The material under compression is highly nonlinear and must be defined appropriately in Engineering Data.

The following restrictions apply to Gasket bodies:

• Gasket bodies are valid only in Static Structural analyses.
• Gasket bodies are valid for 3D solids only, that is, 2D gasket bodies cannot be specified.
• A valid gasket material model must be specified.
• In addition to gasket bodies, a multibody part may also include flexible bodies but not rigid bodies.
• Gasket bodies are not supported for cyclic symmetry analyses.

Meshing a gasket body

A Gasket body is meshed with the INTER194 elements (if using Element Order = Quadratic, in such cases a single layer of elements are generated with midside nodes on top and bottom faces, but linear edges across thickness) or INTER195 elements (if using Element Order = Linear).

Upon setting the Stiffness Behavior as Gasket, a Gasket Mesh Control object is added beneath the Body object in the tree. The Mesh Method property for the object is automatically set to Sweep and is read-only. By default, this property instructs the application to drop mid-side nodes on gasket element edges that are parallel (Normal To) to the scoped sweep direction.

Flexible Beam (Beta)

This is only supported for line bodies. Ansys meshes the line body using 1-D beam elements.

Rigid Beam (Beta)

This is essentially the same as a stiff beam behavior and it is supported for line bodies only

• Only structural analyses support this feature. For example, thermal or electrical analyses are unaffected.
• The application approximates a rigid beam by making the Young’s modulus 1e4 times higher than defined in the Engineering Data Workspace.