March 17, 2023 at 8:59 amFAQParticipant
Typical solid elements do not have nodal rotational degrees of freedom, therefore, there are no nodal rotations to output. The following approaches can be followed to output the rotations of a deformable body. 1) An approach to output the rotation of a region of a solid part is to define a small rigid patch using *CONSTRAINED_NODAL_RIGID_BODY. Then, the rotations of the nodal rigid body will be available in the RBDOUT file. 2) A second approach is to use the functions AX2(n1,n2), AY2(n1,n2), AZ2(n1,n2) of *DEFINE_CURVE_FUNCTION. These require that a local coordinate system is attached to node n1 and another one to n2. The local coordinate system should be defined with *DEFINE_COORDINATE_NODES and FLAG=1. Also, node n2 should not be omitted from the function arguments. The *DEFINE_CURVE_FUNCTION value with respect to the time is written to the output file CURVOUT, which is triggered by *DATABASE_CURVOUT. 3) A third approach is to add a new node and constrain it to a node set of the solid elements using *CONSTRAINED_INTERPOLATION. The rotations at this dependent node are written in NODOUT. However, to activate the rotation slots in NODOUT, you also need to add at least one shell or beam element in the model. This approach will not affect the stiffness of the deformable part.
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- The LS-DYNA equivalent of *MODEL_CHANGE card (in ABAQUS). Which keywords can be used to introduce(activate)/delete(deactivate) elements in the middle of a calculation (at user-specific time/load steps).
- The warning message is: “The maximum contact stiffness is too big. This may affect the accuracy of the results.” Why does large contact stiffness affect results accuracy?
- Contact Definitions in ANSYS Workbench Mechanical
- How to deal with “”Problem terminated — energy error too large””?”
- After Workbench crashes, how can I recover the project from a .mechdb file?
- How to display the color of each body based on the material in Mechanical?
- How to resolve “Error: Invalid Geometry”?
- Model has a large number of contacts – how to reduce them?
- Please explain the difference between Point Mass and Distributed Mass.
- How to locate an element of a particular ID number in Mechanical?