CFD Online Discussion Forums - [ANSYS Meshing] Model Information is incompatible with incoming mesh

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)

- - [ANSYS Meshing] Model Information is incompatible with incoming mesh (https://www.cfd-online.com/Forums/ansys-meshing/162493-model-information-incompatible-incoming-mesh.html)

Model Information is incompatible with incoming mesh

Dear all,
I faced to this msg in setup, but i can not find the following steps, which described below. ( ansys 16), can any one help me.
Found some missing and new zones in the mesh. To make mesh compatible with settings, please visit "Match Zone Names" panel

(Mesh->Recorded Mesh Operations->Edit Incoming Zones... -> Match Zone Names...).

Thank you in advance

i am facing the same problem

Model Information is incompatible with incoming mesh

It occur because the meshing cannot detect the face at the setup option, hence i suggest to match the missing surface for the same name item.

If I may add my own observations, this error message usually occurs when one has linked an existing geometry and mesh to a Fluent case initially, but changes something in the geometry/mesh later on, hence requiring the link between the Fluent case file and the mesh to be updated.

For my case, I'm performing a parametric study in Workbench, and for simplicity & reduced skewness in tetrahedral meshing, I have set No Shared Topology for some bodies, leading to Contact Regions generated in Ansys Meshing.

When running the parametric analysis, an upstream change in geometry will eventually lead to a change in the auto-generated "wall" surfaces that represent the Contact Regions between the discrete bodies. These wall surfaces can usually be identified with some obscure naming that you didn't create:

wall-32
wall-25
etc.

You'll know it's not a real wall surface when you attempt to Display the selected mesh in Fluent and you get the following error message:

"Note: zone-surface: cannot create surface from sliding interface zone.
Creating empty surface."

In addition to that, Ansys Meshing would rename your Contact Regions to have the string "contact_region" in it every time a geometry parameter is changed and the cells are refreshed.

So yes,

1. You can attempt to match the zone names through the main menu toolbar "File>Recorded Mesh Operations" function.
2. For myself, as I can't afford to manually match zone names every time my geometry is modified, I learnt how to use Workbench Scripting to
a. Reset the Setup cell from Workbench's Project Schematic
b. Run a Fluent TUI-based Journal file that loads in all my case settings

It was a little difficult to find some of these handy commands and format to interface the Workbench Script with the Fluent TUI Journal, I found it in AnsysHelp (Ansys AIM and Workbench Scripting Guide --> Data Containers --> Fluent --> Fluent Setup --> Send Command section). Here is a copy of my code for your reference:

Code:

# encoding: utf-8

# Release 19.2

SetScriptVersion(Version="19.2.120")

system1 = GetSystem(Name="FFF 2")

setupComponent1 = system1.GetComponent(Name="Setup")

setupComponent1.Refresh()

setup1 = system1.GetContainer(ComponentName="Setup")

fluentLauncherSettings1 = setup1.GetFluentLauncherSettings()

fluentLauncherSettings1.SetEntityProperties(Properties=Set(DisplayText="Fluent Launcher Settings", Precision="Double", EnvPath={}, RunParallel=True, NumberOfProcessors=22))

setup1.Edit()

setup1.SendCommand(Command="/file/read-journal \"W:\folder1\folder2\workbenchfilename_files\dp0\FFF-2\Fluent\journalname.jou\" " )

Another discovery is that you can actually run Fluent TUI commands from Workbench Scripts. As an example:

Code:

setup1.SendCommand(Command="/define/operating-conditions/gravity y 0 -9.81 0")

setup1.SendCommand(Command="/define/models/viscous kw-sst y")

Best of luck to anyone reading this.

Cheers
John

Quote:

Originally Posted by abtin (Post 572916)

Yeah I think it happens because u changed ur geometry after using setup you just went back to either SpaceClaim or Meshing and made some name selection or geometry changes.

It worked for me when I linked mesh to a stand alone Fluent, instead of using same Fluent I linked before

After the geometry is imported into icem, it is severely deformed

After I imported the geometry into icem, serious deformation occurred in the place with a small size, and the end face was severely deformed, which made it impossible to create part.
The overall size is mm, where the deformed end face is 0.1mm, the end face of 0.1mm is very narrow. But there is no problem with drawing the grid, and there is no problem with the line display, that is, the surface is greatly deformed when it is displayed.

This thing usually occurs when you go back to design modeler/mesh to edit something like, changing name selection or any silly things.

Solution: RESET the Fluent and UPDATE it again. you will no longer see that error message.

Mesh->Recorded Mesh Operations->Edit Incoming Zones... -> Match Zone Names...) .

Sur ANSYS 2022R1

Merci d'avance