Tagged: ls-dyna, LS-DYNA Suite, lsdyna, R13.x, structural-mechanics
-
-
March 17, 2023 at 8:59 amFAQParticipant
To define a cross section and output the cross-sectional resultant forces in the updated cross-sectional coordinate system, two alternative approaches can be followed. 1) Define the cross section in the input file using the keyword *DATABASE_CROSS_SECTION_PLANE. Select ITYPE=2 and use ID to reference the section’s coordinate system. The coordinate system should be defined using *DEFINE_COORDINATE_NODES with FLAG=1 so that the local coordinate system is updated at every time step based on the position of three nodes. The resultant cross-sectional forces are calculated by LS-DYNA in the updated local coordinate system and are written in the output file secforc which can be loaded in LS-PrePost. 2) Define a cross section in LS-PrePost after loading d3plot. This can be done by selecting FEM > Model and Part > Section Plane. In the Section Plane window, select “3Nds†for defining the cross-sectional plane using three nodes. Also, select “FixM†for the cross section to be fixed to the model and be updated based on the position of the three nodes. Then press “Cut†and then “Forceâ€. Next, check the option “Plane coordinate systemâ€, select the section force component to be plotted, and press “Plotâ€. This will plot the section forces with respect to the updated local coordinate system. With this approach the calculation of the element forces is done by LS-PrePost, independently of LS-DYNA, using the element stress data written in d3plot.
-
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.
- How to deal with “”Problem terminated — energy error too large””?”
- 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).
- Contact Definitions in ANSYS Workbench Mechanical
- How do I request ANSYS Mechanical to use more number of cores for solution?
- There is a unit systems mismatch between the environments involved in the solution.
- How to restore the corrupted project in ANSYS Workbench?
- After Workbench crashes, how can I recover the project from a .mechdb file?
- 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.
© 2024 Copyright ANSYS, Inc. All rights reserved.