Tagged: cfx, fluid-dynamics, General - CFX
-
-
March 17, 2023 at 8:58 amFAQParticipant
There are 2 ways for performing a restart in a case with only a slightly modified mesh: 1. The standard approach is to use the interpolator a) If the meshes have a different mesh topology, then this is the only alternative. The restart will not be smooth, e.g. residuals show a jump, as the solution fields have to be interpolated on the new mesh. b) If the mesh topology is identical for mesh1 and mesh2, i.e. only changes in vertex co-ordinates, then the solution fields can just be copied onto the new mesh file. This is done by the interpolator when setting the following environment variable. CFX_INTERP_NOCRDVX_CHECK = 1 The restart will be smoother than case a), but will still show some jumps in residuals, as boundary IP flows (such as wall shear and wall heat flux) and hybrid values are not interpolated onto the new mesh. 2. If the mesh topology is identical, the def-file of the new mesh can just be appended to the result-file of mesh1 by the following command: cat mesh1.res mesh2.def > mesh2_restart.def cfx5solve –def mesh2_restart.def The order of the files in the cat-command is important. Restarting with this method will be smooth, depending on the changes in the mesh co-ordinates.
-
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 1Â 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 overcome the model information incompatible with incoming mesh error?
- How to create and execute a FLUENT journal file?
- What are the requirements for an axisymmetric analysis?
- How can I Export and import boxes / Systems from one Workbench Project to another?
- How can I select interior faces and other entities that are inside the model?
- What is a .wbpz file and how can I use it?
- Skewness in ANSYS Meshing
- Left-handed faces troubleshooting
- Error: Update failed for the Mesh component in Fluid Flow (Fluent). Error updating cell Mesh in system Fluid Flow (Fluent). View the messages in the Meshing editor for more details.
- Running Python Script from Workbench
© 2024 Copyright ANSYS, Inc. All rights reserved.