|
[Sponsors] |
[ICEM] Problems with export 2D mesh from ICEM to FLUENT |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 22, 2013, 17:23 |
|
#41 |
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 273
Rep Power: 15 |
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! |
|
February 4, 2013, 07:38 |
|
#42 |
New Member
Join Date: Feb 2013
Posts: 2
Rep Power: 0 |
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 !!! |
|
May 22, 2013, 16:45 |
|
#43 |
New Member
Antoine
Join Date: Mar 2013
Location: Montreal
Posts: 6
Rep Power: 13 |
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. |
|
May 23, 2013, 11:10 |
|
#44 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
Oh yea,
There is a bug if you select "Fluent V6" while generating the output script command... Instead, select "ANSYS Fluent" and it works.
__________________
----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey |
|
May 23, 2013, 12:13 |
|
#45 |
New Member
Antoine
Join Date: Mar 2013
Location: Montreal
Posts: 6
Rep Power: 13 |
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. Last edited by Sandro23; May 23, 2013 at 14:35. |
|
May 24, 2013, 11:12 |
|
#46 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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
__________________
----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey |
|
May 27, 2013, 11:01 |
|
#47 |
New Member
Daniel
Join Date: Oct 2010
Posts: 1
Rep Power: 0 |
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 |
|
July 4, 2014, 06:41 |
ICEM-to-FLUENT 3D Mesh
|
#48 |
New Member
Robert
Join Date: Jul 2014
Location: Delft, The Netherlands
Posts: 12
Rep Power: 12 |
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 |
|
July 4, 2014, 08:12 |
|
#49 |
Senior Member
Join Date: Feb 2013
Location: Germany
Posts: 200
Rep Power: 24 |
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.
|
|
July 4, 2014, 08:45 |
|
#50 |
New Member
Robert
Join Date: Jul 2014
Location: Delft, The Netherlands
Posts: 12
Rep Power: 12 |
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. |
|
July 6, 2014, 12:32 |
|
#51 |
Senior Member
Join Date: Feb 2013
Location: Germany
Posts: 200
Rep Power: 24 |
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.
|
|
August 13, 2014, 09:51 |
ICEMCFD: Fluent output in batch mode on win7
|
#52 |
New Member
Tomasz Stankowski
Join Date: Aug 2014
Location: Cranfield, United Kingdom
Posts: 2
Rep Power: 0 |
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 |
|
August 13, 2014, 12:57 |
|
#53 |
Senior Member
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 567
Rep Power: 21 |
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" 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) 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 Last edited by bluebase; September 1, 2014 at 16:14. |
|
August 18, 2014, 06:17 |
ICEMCFD: Fluent output in batch mode on win7
|
#54 |
New Member
Tomasz Stankowski
Join Date: Aug 2014
Location: Cranfield, United Kingdom
Posts: 2
Rep Power: 0 |
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 |
|
September 20, 2014, 13:40 |
|
#55 |
New Member
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
Very helpful thread!
|
|
Tags |
batch mode, flat plate, fluent, icem |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
ICEM - problems with prism mesh | João Lourenço | CFX | 2 | September 18, 2019 04:07 |
Moving mesh | Niklas Wikstrom (Wikstrom) | OpenFOAM Running, Solving & CFD | 122 | June 15, 2014 07:20 |
Transport mesh from ICEM CFD, to Fluent, to Sysnoise | Wieland | FLUENT | 2 | April 15, 2012 07:28 |
[ICEM] Export refined mesh to fluent | Heleen | ANSYS Meshing & Geometry | 8 | March 26, 2012 09:33 |
Export mesh from ICEM to Fluent 6.3 (3D) | bigbang | ANSYS | 0 | June 8, 2010 00:05 |