CFD Online Discussion Forums - [ICEM] Problems with export 2D mesh from ICEM to FLUENT

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

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

- - [ICEM] Problems with export 2D mesh from ICEM to FLUENT (https://www.cfd-online.com/Forums/ansys-meshing/83958-problems-export-2d-mesh-icem-fluent.html)

Hi guys,

I've been working on the 3D case of the flat plate. I've made a structured mesh, checked it and smooth it 3 times and everything went okay. The issue is that in fluent it shows non-positive volumes, left-handed faces and high skewness elements. How can I fix all that stuff?
Btw I don't know what left-handed faces means.

I upload the icem files here:
https://www.dropbox.com/sh/er8eqcqh617rrt9/Xjq2PuE0DQ

Thanks!

Hi every one,

I am a new member of this community so I don't know exactly if this is the right place to write my question...
Anyway, I have a problem to export a 2D mesh from ICEM CFD to Fluent in batch mode. I am using icem and fluent with Linux.When I do the operation using the graphique interface, all is OK, a file mesh.msh is created and consistant for fluent. To make icem run in batch mode, the only solution I have found is to make a script file (.rpl) saving all the steps of the mesh designing using the option Replay scripts and then replaying this script (with the linux command: icemcfd -batch script.rpl). This solution is functionning for all the steps except the one exporting the mesh to fluent.
When I am recording the steps to export the mesh, icem write in the script.rpl the following lines:
ic_undo_group_begin
ic_uns_create_diagnostic_edgelist 1
ic_uns_diagnostic subset all diag_type uncovered fix_fam FIX_UNCOVERED diag_verb {Uncovered faces} fams {} busy_off 1 quiet 1
ic_uns_create_diagnostic_edgelist 0
ic_undo_group_end

When Icem execute this script, it said:
Saved replay log to /panfs/storage/p003858/optim/output.rpl
Starting at command 1, going to end
Current Coordinate system is global
5 command lines replayed.
Replay complete.

Instead of :
Select an unstructured domain.
Running: "/panfs/storage/local/commercial/ansys_inc/v140/icemcfd/linux64_amd/icemcfd/output-interfaces/fluent6" -dom "/panfs/storage/p003858/optim/mesh.uns" -b "mesh.fbc" -dim2d "./mesh"

Running FLUENT V6 Interface Vers. 14.0.3

Creating a Fluent 2D mesh.
Computing connectivity for 198431 cells.
100000 cells
200000 cells
Creating cell sections for 198431 cells.
Checking mesh:
interior faces : 395685
interior walls : 0
boundary faces : 2354
Creating face section for 398039 faces.

FLUENT V6 input file written (file: ./mesh.msh)
... done
When I do it manually using the graphique interface.

Clearly, ICEM is reading the code in the script but it does not understand it and so not it doesn't execute it.

Is anybody has a idea of what should I do to fix this ?

Thank you so much !!!

Hi marylou,

I have exactly the same problem. I'm making a script on Matlab to adapt automatically my mesh when the geometry change and my only problem is when i need to export the mesh.
It's like we can't export the mesh using the replay script.

Did you find a solution about that ?

Regards,

Antoine.

Oh yea,

There is a bug if you select "Fluent V6" while generating the output script command... Instead, select "ANSYS Fluent" and it works.

Hi,

Indeed, to export the file.msh, I use this function :

ic_create_output Fluent_V6 filename.uns dim2d 1 bocofile filename.fbc outfile test1.msh

It works but ICEM open two windows : save as file.fbc and save as project.prj
I don't know why but I don't want to interfer manually during the mesh making.

If someone know a function to cancel the saving of these files, it would be grate.

Regards,

Antoine.

It only pops those up in interactive mode.

It will need to have those files saved in order to generate the output file (since it works from saved files rather than in memory files), so create and save the boco file and save the project in the script just before you output.

When you run it later in batch mode, it won't try to call any popups.

Simon

Hello guys,

I was having the same problem and could solve it with the hint of PSYMN. Thank for that one.
However, the resulting fluent.msh file is broken. I can neither import it into ICEM (GUI) again, nor into my solver or EnSight. If I process the same replay script using the GUI, the resulting Fluent mesh is perfectly O.K.
Is anybody having this issue also or can anybody support a tip to fix this problem? Unfortunately, I have to process the meshing in batch mode for some memory reasons and can therefore not just use the GUI.

Cheers,
Daniel

ICEM-to-FLUENT 3D Mesh

When trying to compute an input-file for FLUENT, I get the following warning:

WARNING: Mesh has uncovered edges. Fluent needs a complete boundary (lines in 2D) or it will give a variety of errors and not read in the mesh! If this was 2D Hexa, perhaps your edges are not associated with perimeter curves

For my mesh, I've followed the steps of the DLR F6 tutorial as have been performed by turbo engineer on Youtube as well. However, I've been using my own geometry this time.

I've added my mesh online at:
https://www.dropbox.com/s/twwfjj9xqw1x1t6/ICM.uns

Check Mesh in ICEM shows various erros. The flap mesh is degenerated. Further your mesh has no volume elements. Check some basic ICEM tutorials first to get a better idea of meshing. ICEM has some build in tutorials to start with.

Thanks for the quick response Kad! I just wanted to pull off a quick mesh and then run it through FLUENT for a first test.

I did do some of the tutorials and I thought I had some idea of generating a basic mesh. However I also noted the problems with the FLAP and I couldn't figure out how to solve them.

I guess that's back to the drawing board then.

The problem with the tutorials is that those are 'perfect' geometries with a tailored approach. Once I'm building a grid around my own geometry I have no feeling for the scaling, sizing and refining that are required.

You can preview mesh sizes (global, surfaces, curves, densities) by activating the corresponding switch. Surface, curve and density sizes can be activated via right click on display tree. In the pop menu activate "show tetra sizes". For curve sizes click on "show node spacing". Global max size can be previewed in Global Mesh Setup.

ICEMCFD: Fluent output in batch mode on win7

Dear All,

I believe that I have very much related problem. I operate Icemcfd v14.0 on windows 7. I created a replay_script and it is successfully executed in GUI mode, yet it fails in batch mode.

Problem description:
While batch execution an error 'signal 11: segmentation violation' is reported:

Signal 11 caught!
segmentation violation - exiting after doing an emergency save

I recognised that error occurs at the command for mesh export:

ic_create_output Fluent_V6 $directory/$name/$name.uns dim2d 1 bocofile $directory/$name/$name.fbc $directory/$name/$name.msh

In GUI there are two pop-up windows to save files. It is a default setting to save attributes and project files. Those files were saved before in the script. So this pop-up is completely useless, and script performs well even if cancel option is chosen in GUI.

My questions:

-Has anyone found a solution to create Fluent output using batch on windows?

-Am I correctly recognising that the signal11 is a graphical interface problem linked to pop-up windows in GUI?

-Is there a way to disable those pop-up windows in batch mode in windows, so that the script executes without error 'signal 11'?

I have spent more than a week reading forums and looking for answers for this problem only. Any help will be appreciated.

Kind regards,
Tomasz

Hi Tomasz,

to export the premesh to fluent in batch mode i use the following script (for 2d mesh). It's working with windows and linux.

Code:

     

# Set boundary conditions (replaces the first pop up menu to set BCs)

  ic_boco_set WALL {{1 WALL 0}}

  ic_boco_set INLET {{1 VELI 0}}

  ic_boco_set FLUID {{1 FLUID 0}}

  #...... as many as needed



# Premesh

   ic_hex_create_mesh $allfamilies proj 2 dim_to_mesh 2 nproc 2;  # nprocs according to your capacities



# Convert to Unstruct

  cmd_rm "hex.uns"; # don't use if meshes are merged

  ic_hex_write_file hex.uns $allfamilies proj 2 dim_to_mesh 2 -family_boco family_boco.fbc



# Mesh writing

  exec "$icemenv/icemcfd/output-interfaces/fluent6" -dom "hex.uns" -b "family_boco.fbc" -dim2d -scale 1,1,1 "$whereToSave/fluent.msh"

Some explanations:

I usually set a working directory to use relative paths.

Usually i copy the ic_boco_sets from the recorded replay script. Another option is to prepare a *.fbc file to skip those settings.

For $allfamilies put all the part names you need (for example: set $allfamilies "SYM WALL INLET OUTLET FLUID") Those parts should have a boundary condition defined by ic_boco_set.

the $icemenv variable can be set in batch mode by

Code:

global env

set icemenv $env(ICEM_ACN)

the whole exec command is usually copied in the command window of icem if you export the mesh by hand.

In case of a 3D mesh use "dim_to_mesh 3" instead of "dim_to_mesh 2" for the commands ic_hex_create_mesh and ic_hex_write_file. And remove the -dim2d option in the fluent export command

With regards,
Sebastian

ICEMCFD: Fluent output in batch mode on win7

Dear Sebastian,

It worked well. The exec command for fluent output did the trick. Also, I've tried other commands and I find them useful.

Thank you for help. Vielen Dank.

Kind regards,
Tomasz

Very helpful thread!