January 25, 2023 at 7:16 amFAQParticipant
The mesh check report will indicate if the mesh contains left-handed faces and/or faces that have the wrong node order. If you have left handed cells and you are continuing the simulation without correcting it solver will calculate the face normal wrongly and that will result in wrong flux calculation. This may some time leads to divergence. You must take steps to repair such meshes, since you cannot obtain a flow solution until all of the faces are right handed and have the proper node order. 1. The left-handed faces mostly occur at locations where the surfaces that are non-conformally connected have sharp corners or contortions. When you get the left-handed faces, you can fix it in Fluent by the TUI commands: mesh/repair-improve/repair-face-handedness mesh/repair-improve/repair-face-node-order 2. When you fix the left handed faces you may get cells with negative volume. You will need to repair these cells manually. It’s best to fix the problematic geometry at the grid generation stage. To identify the problematic geometry, read the case file again and create an adaption register using the IsoValue Adaption panel with the category Grid and the subcategory Face-Handedness as follows: (a) Go to Adapt–>Iso-values (b) Select mesh in the Iso-value of drop down menu (c) Select Face handedness from the drop down menu below that (d) Enter 1 for Max as well as Min value in the Iso-min and Iso-max input box (e) Press mark (f) Go to manage in the same panel (g) Click on the display button to see where the negative volumes are forming This may give you an idea of the location of problematic geometry which you may then fix in the grid generation software.
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.
- ANSYS Fluent: Introduction to the GEKO Turbulence Model Part I
- Delete or Deactivate Zone in Fluent
- What is meant by Warning: Flow boundary zone 18 is adjacent to a solid zone?
- ANSYS Polyflow: Adaptive Meshing Based on Contact
- Aero-Mechanical Simulation of Turbomachinery Blading
- Apply Custom Material Properties in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- Predict Gearbox Lubrication, Oil Temperature and Churning Losses using CFD Simulation
- Check CPU Time in ANSYS FLUENT
- How to Predict Performance of Bioreactors and Mixing Tanks