When trying to use submodeling in Workbench with an .rst file created by a solve that was done totally in MAPDL and map the results across why one gets a ‘General Error’?
June 5, 2023 at 7:04 amFAQParticipant
The workflow uses External model to read in the .cdb file and then Tools>Read Results in Mechanical to read the results in to Mechanical. A dummy command object under the Static Structural branch will be needed in order to ‘trick’ Mechanical into showing up as complete. For submodelling to work the .rst file will need to contain the information about the units used during the solve. For models solved from Mechanical the /UNITS command is used to record this information. By default models set up in MAPDL from scratch will not include this. This will lead to a message something similar to this “Since the result file does not indicate the unit system, the following file unit system is assumed: Metric (m, kg, N, s, V, A)” This will then lead to the ‘General Error’ when the results are mapped across. In order to overcome this one can resume the database in MAPDL, read in the results set of interest and then issue /UNITS to define the set of units used. Then use the RESWRITE to recreate the existing results set onto a new file with the units recorded. Note the SI and User cannot be used on the /UNITS command for this to work. Everything else is fine.
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?