-
-
September 27, 2017 at 11:19 am
admin
Ansys EmployeeHow can I locate and fix left handed cells?
-
September 27, 2017 at 11:19 am
admin
Ansys EmployeeThe 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.
-
- You must be logged in to reply to this topic.

Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.

Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
-
2656
-
2120
-
1345
-
1118
-
461
© 2023 Copyright ANSYS, Inc. All rights reserved.