Can ANSYS nCode DesignLife be used with a mode-superposition transient analysis if residual vectors are calculated?
April 5, 2023 at 2:32 pmFAQParticipant
Not directly. Mechanical includes residual vectors by performing a modal restart just before doing the transient analysis that calculates the residual vectors. Thus, the residual vectors are not included in the original modal analysis system or in its results. There are 2 methods that might enable you to use a mode-supe transient analysis with ANSYS nCode DesignLife. Method 1: Insert Command Object in the Modal analysis system and issue MAPDL commands to define the loads and invoke RESVEC to include the residual vectors. If those commands are issued, the modal .rst file should contain the modal stresses associated with the residual vector. Method 2: 1. In the Transient analysis system, in the Details Window of the “Analysis Settings” branch, change “Analysis Data Management > Delete Unneeded Files to “No” 2. Insert a Command Object under the Transient folder/branch with the single command “/EOF”. This end of file command will stop the analysis. Also, ensure that, in the Details Window, “Definition > Step Selection is set to “Zero”. 3. Solve the transient system. It will not be a complete solve, as the /EOF command will stop the solution after the modal restart. However, since Mechanical was instructed to keep all unneeded files, the file.rst should contain the modal stresses (if requested) for all of the modes, including the residual vector.
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?
- How to deal with “”Problem terminated — energy error too large””?”
- Contact Definitions in ANSYS Workbench Mechanical
- How to display the color of each body based on the material in Mechanical?
- After Workbench crashes, how can I recover the project from a .mechdb file?
- How do I request ANSYS Mechanical to use more number of cores for solution?
- 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.