Tagged: ls-dyna, LS-DYNA Suite, lsdyna, R13.x, structural-mechanics
-
-
March 17, 2023 at 8:59 am
FAQ
ParticipantIn LS-DYNA, parts assigned the material *MAT_RIGID are treated as rigid bodies. *BOUNDARY_PRESCRIBED_MOTION_RIGID is used for prescribing translational or rotational motion to a rigid body. By default, the motion is prescribed to the center of mass of the rigid body. DOF=8 can be used to prescribe rotational motion about an axis that is parallel to vector VID but that is still passing through the body’s center of mass. Special care should be given so that the constraints specified with the fields CMO, CON1, and CON2 in *MAT_RIGID are not in conflict with the prescribed motion. To prescribe rotation about an axis that is away from the body’s center of mass, one of the following two workarounds can be used. 1) *PART_INERTIA can be used instead of *PART for defining the rigid body. In *PART_INERTIA, the location of the center of mass can be specified by NODEID or by the coordinates XC, YC, ZC. By doing so *BOUNDARY_PRESCRIBED_MOTION_RIGID will apply the rotation about the location of NODEID or the location (XC, YC, ZC). The downside is that the translational mass TM and the inertia tensor terms should be also specified in *PART_INERTIA. Nonetheless, if all six degrees of freedom of the rigid body are prescribed or constrained, the mass and inertia terms can be arbitrary. Note that if a diagonal inertia tensor is specified, the terms in the diagonal should not be all equal. Otherwise, the analysis will terminate with an error. NODEID can be added as an extra node to the rigid body by using *CONSTRAINED_EXTRA_NODES while the coordinates XC, YC, ZC are ignored in NODEID is specified. 2) An alternative approach is to add a dummy rigid body whose center of mass is at the location about which the rotation needs to be prescribed. The dummy rigid body can be constrained to the original rigid body through an appropriate *CONSTRAINED_JOINT option, such as a LOCKING joint. Then, the rotation can be applied to the dummy rigid body using *BOUNDARY_PRESCRIBED_MOTION_RIGID.
-

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?
© 2023 Copyright ANSYS, Inc. All rights reserved.