When performing analysis using Mechanical, there is an option called Stiffness Behavior in the geometry properties panel, as shown below:
There are five options available in the dropdown: Flexible, Rigid, Gasket, Flexible Beam, and Rigid Beam. Some options may only appear in certain versions with beta features enabled.
This article provides a brief explanation of each option.
1. Flexible
This behavior is the software’s default setting. Selecting this behavior means the object will deform during the analysis process, and stress and strain will be generated inside the geometry.
2. Rigid
When you set a geometry body to Rigid, this typically means the geometry body is not allowed to deform in subsequent structural analysis. Common scenarios for setting this include:
1. When the mechanism only undergoes rigid body motion;
2. In an assembly, only some parts bear most of the load;
3. Users do not care about the stress and strain of a certain part and want to reduce meshing to improve solving efficiency.
Once a geometry body is set to rigid, the software will not mesh the rigid body. The underlying operation converts it into a mass element that has all the physical properties of this geometry body, such as mass, center of mass, and moment of inertia. These data can be obtained by checking the detailed properties of the geometry body object.
Rigid bodies typically follow these limitations:
1. Applicable analysis range for rigid bodies: Static Structural, Transient Structural, Harmonic Response, Modal, Rigid Body Dynamics, Random Vibration, Response Spectrum
2. Valid object types for rigid bodies include: Point Mass, Joints, Springs, Remote Displacement, Remote Force, Moment, Contact
3. In explicit dynamics analysis, when a geometry body is set as rigid, it is only valid for: Fixed Support, Displacement, Velocity, Springs, Remote Displacement
4. Output contents for rigid bodies include: Displacement, Velocity, Acceleration.
Additionally, when selecting as rigid body, note the following:
1) In implicit analysis, line bodies, 2D plane strain bodies, or 2D axisymmetric bodies cannot be defined as rigid. However, in explicit analysis, 2D plane strain bodies or 2D axisymmetric bodies can be defined as rigid;
2) All geometry bodies in a multi-body part must have the same stiffness behavior. That is, when users set a certain geometry component as rigid, regardless of whether the underlying parts are connected through shared topology, the entire geometry group will act as a single rigid mass block.
3. Gasket
Gasket joints are key components in most structural assemblies. As sealing elements between structural components, gaskets are typically very thin and made from various materials such as steel, rubber, and composite materials. From a mechanical perspective, the function of gaskets is to transfer forces between components. The primary deformation of gaskets is usually limited to one direction—the thickness direction. Stiffness contributions from membrane (in-plane) and transverse shear are much smaller and are usually ignored.
When users specify the geometry property as Gasket, only one layer of elements is meshed in the thickness direction, and the deformation in the thickness direction is decoupled from in-plane deformation. Gasket materials are usually in a compressed state. Materials under compression have high nonlinearity, which must be correctly defined in the material properties.
This behavior type follows these limitations:
1) This behavior type is only valid in Static Structural analysis;
2) Only for 3D solid structures;
3) A valid gasket material model must be specified;
4) In addition to gasket bodies, a multi-part can also contain flexible bodies, but cannot contain rigid bodies;
5) Cyclic symmetry analysis is not supported.
The underlying element types in the software are INTER194 and INTER195 elements, where 195 is the low-order element and 194 is the high-order element, depending on the order selected by users during meshing.
When a certain geometry body property is set to gasket, a gasket-related mesh control object is usually added under the geometry body object in the structural tree. The meshing method property of this object is automatically set to Sweep and is read-only.
4. Flexible Beam
This option only applies to line bodies. If it is a 3D solid, the software uses one-dimensional beam elements to mesh the line body.
5. Rigid Beam
The analysis method and objects are basically the same as the flexible beam mentioned above. When rigid beam is selected, the software will by default enlarge the structural material’s elastic modulus by 10,000 times to simulate a rigid beam. Of course, users can also customize a very large elastic modulus value to equivalently replace it.
The above is the explanation of stiffness behavior. Thank you for reading.
For simulation business cooperation, please click: Business Services
For more original courses by Shuige, please click: Shuige’s Original Course List – Up to September 2025
For more finite element learning resources, please visit Shuige’s blog: FSCAE.COM
Best regards,
ANSYS Structural Institute
October 27, 2025
No comments yet