Creating ANSYS rigid bodies

In ANSYS, you can use rigid bodies to simulate multi-body dynamics analyses. In ANSYS, a rigid body consists of a set of rigid body nodes, defined by contact elements, and a single pilot node, defined by a target element. A rigid body cannot exist by itself. It must be in contact or connection with other bodies through contact elements.

In a finite element model, you can use a rigid body to represent certain relatively stiff parts when stress distributions and wave propagation in such parts are not critical. Rigid bodies offer the advantage of computational efficiency over deformable finite elements.

• Elements that belong to the rigid body have no associated internal forces or stiffness.

• The motion of the rigid body is controlled by the degrees-of-freedom at the pilot node.

In Pre/Post, you can use options in the Region dialog box to define rigid bodies that you can then use within a Structural Contact definition to define a contact pair.

For more information, see Modeling Rigid Bodies in a Multibody Analysis in the ANSYS Multibody Analysis Guide.

Defining rigid bodies for a linear statics solution

For Linear Statics solutions, ANSYS requires one Structural Contact definition. The Structural Contact definition must contain two rigid bodies: one in the Source Region and one in the Target Region.

• The Type of the Source Region must be Flexible.

• The Type of the Target Region must be Rigid. Additionally, you must use the Master Grid Point option to specify a pilot node.

Defining rigid bodies for dynamics solutions

For Transient Dynamics solutions, two Structural Contact pair definitions are recommended, although ANSYS only requires one.

• Pair 1 is the contact definition which represents the connection between the rigid body and the adjacent flexible body.

• Pair 2 represents the rigid body itself, which is defined by the enclosed boundary surfaces of the body as specified in the Region definition and by the selected Pilot Node in the target region.

For example, you could create two Structural Contact pair definitions as follows:

• Structural Contact Pair 1, which contains the contacting surfaces in the flexible body (1). Source (SF1) is the specified Source Region and Target (TF1) as the target region. The Type of both regions is Flexible.

• Structural Contact Pair 2 , which contains the contacting surfaces in the rigid body (2). Source (SF2) is the specified Source Region and Target (TF2) as the target region. Source (SF2) is a Rigid region and contains all the boundary surfaces of the rigid body. These surfaces include the interface surface TF1 as well as the other three faces on the rigid body (3). Target (TF2) is the Pilot Node. Because rigid regions require that you specify a pilot node, use the Master Grid Point option to re-select TF2 as the pilot node.

ANSYS ignores any loads or boundary conditions defined on the surfaces in the (rigid) target region, except for those defined on the pilot node. The pilot node controls all degrees-of-freedom for the entire rigid body.

Specifying the mass of the rigid body

In a multi-body dynamics analysis, the mass and rotational inertia of the rigid body are important to the dynamic response of the model. In ANSYS, the contact and target elements that define the rigid bodies do not contribute to the mass of the system. To add mass, use the 0D Mesh command to create a MASS21 element at the center of gravity of the rigid body. You can use the MASS21 ET modeling object to specify the rigid body mass and rotary inertia for the element.

The node of the MASS21 element has the following characteristics:

• It is usually connected to the specified pilot node, although you can also connect it to any of the nodes on the rigid body.

• It is generally defined in a local coordinate system that is parallel to the rotary principal axes.

Specifying the KEYOPTs for the target elements

Use the TARGE170 KEYOPTs options in the CONTA174ET modeling object dialog box. Use these options to specify options for the target elements, such as whether ANSYS should automatically constrain the target nodes.

Exporting or importing solutions that contain rigid bodies

When you export or solve a solution that contains a Flexible or Rigid region, the software modifies the input file syntax to meet the ANSYS requirements for rigid bodies.

• For Rigid regions, ANSYS requires that their target shape is specified in the input file with the TSHAP command. The software automatically writes out the TSHAP command as follows:For elements on the surface of the selected region (TARGE170), the software generates TSHAP= 6, 7, 8, or 9 for TRI3, QUAD4, TRI6, or QUAD8 elements. For elements on the edge of the selected region (TARGE169), the software generates TSHAP= 1 or 2 for 2-node or 3-node elements on edge, respectively.For the element generated from the pilot node (TARGE169 or TARGE170), the software generates TSHAP=99.The value for the TSHAP command displays in column 8 of the EBLOCK section of the input file. Other settings for the TSHAP command, such as TSHAP=ARC, CIRC, SPHE, are not supported.

• For Flexible regions, ANSYS does not require that their target shape is specified in the input file. The software writes out the appropriate TARGE170 or TARGE169 elements instead. Additionally, TSHAP = 0 is written to column 8 of the EBLOCK section of the input file.

• For Rigid regions that are used as a target surface in a Structural Contact definition, ANSYS does not allow underlying elements to be included in the solution. However, in Linear Statics solutions in the ANSYS environment in Pre/Post, the model must have underlying elements, such as SHELL181 or SOLID185 elements. In this case, when you export or solve the solution, the software removes those underlying elements and replaces them with TARGE170 elements.As a best practice, you should not create 2D elements, such as SHELL181 elements, on top of 3D elements, such as SOLID185 elements. Instead, use 2D elements to define the enclosed volume.Note: If there are 3D elements underneath the region, the software only removes the solid elements connected to the TARGET170 elements from the input file. It does not remove any other solid elements in the volume.

When you import an ANSYS input file that contains a rigid body definition, if the TARGE170 elements on the rigid body to not have underlying elements that share the same nodes, the software creates the appropriate SHELL281 or SHELL181 elements during the import process.

Where do I find it?

Simulation Region

Application	Pre/Post
Prerequisite	A Simulation file as the displayed part and the work partANSYS as the specified solverStructural as the specified analysis type
Command Finder	Simulation Region

CONTA174ET modeling object

Application	Pre/Post
Prerequisite	A Simulation file as the displayed part and the work partANSYS as the specified solverStructural as the specified analysis type
Command Finder	Modeling Objects
Location in dialog box	Type→ list CONTA174ET

How do I

Define surface-to-surface contact

Learn more

Surface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS)

Structural Contact (ANSYS)

Thermal Contact (ANSYS)

Automatic face pairing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Creating ANSYS rigid bodies, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });