|
[Sponsors] |
Problems while exporting .cgns mesh files from Salome |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 11, 2022, 08:03 |
Problems while exporting .cgns mesh files from Salome
|
#1 |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Hello everybody,
I am trying to export mesh files from the Salome in .cgns format but I have some errors while running the simulation. When I run SU2_CFD this error pops up: Code:
The configuration file doesn't have any definition for marker BAR_21-1100 I also exported file as .unv and opened it in GMSH so I can export it as .su2 but this time error was: Code:
Could not find the keyword "NMARK=". Check the SU2 ASCII file format. I read this post as well but I guess plug-in doesn't work anymore. Salome cgns format mesh to SU2 How can I export a mesh file from Salome? Last edited by CleverBoy; October 16, 2022 at 09:21. |
|
October 11, 2022, 09:38 |
|
#2 |
New Member
Jay Wee
Join Date: Oct 2022
Posts: 6
Rep Power: 4 |
Could you post the cgns mesh here? Because the cgnsconvert fails, it is possible that the cgns mesh is either broken or based on tool old cgns library, which is incompatible with the su2.
|
|
October 11, 2022, 09:56 |
|
#3 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Yes of course. I added Salome file at the attachment too. I am using Salome 9.8. https://1drv.ms/u/s!AhBDg13OQn2zhA4Z...Zr_tE?e=e4UrEH |
||
October 11, 2022, 15:00 |
|
#4 | |
New Member
Jay Wee
Join Date: Oct 2022
Posts: 6
Rep Power: 4 |
Quote:
I checked the Mesh1.cgns, which is built on v4.1 CGNS lib. I checked the latest master of SU2, which is built on v4.2 CGNS lib, so the mesh is not the problem. From your post, I see one boundary is missing in the configuration file, please check your config file. |
||
October 11, 2022, 16:30 |
|
#5 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Thank you so much for validation. I checked my .cfg file but as far as I can see, there is no problem with boundary conditions. I am attaching .cfg file with a picture from Salome so you can check it as well. Could it be exporting group names wrong? |
||
October 12, 2022, 09:43 |
|
#6 |
New Member
Jay Wee
Join Date: Oct 2022
Posts: 6
Rep Power: 4 |
Could you post following things here? I want to duplicate your error:
1. all input files to SU2: mesh file, configuration file, etc. 2. the command to generate the error you posted in the first thread: "The configuration file doesn't have any definition for marker BAR_21-1100" |
|
October 12, 2022, 09:44 |
|
#7 | |
New Member
Jay Wee
Join Date: Oct 2022
Posts: 6
Rep Power: 4 |
Quote:
The mesh looks good to me. The SU2 seems like fail to read the correct boundary conditions. |
||
October 12, 2022, 11:04 |
|
#8 | ||
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Yes of course. https://1drv.ms/u/s!AhBDg13OQn2zhA-G...XAT37?e=NPc9ex The code and output: Code:
SU2_CFD fire_II.cfg . . . . Error in "short unsigned int CConfig::GetMarker_CfgFile_TagBound(std::string) const": ------------------------------------------------------------------------- The configuration file doesn't have any definition for marker BAR_21-1100 ------------------------------ Error Exit ------------------------------- -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD with errorcode 1. Quote:
I didn't put a lot of work on mesh because I am just trying the simulation to work. |
|||
October 13, 2022, 10:17 |
|
#9 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
I tried the .cgns Mesh file with a configuration file from the tutorials but the outcome is same. I tried a different geometry and a mesh with different cfg files but error was same with different marker numbers. Were you able to look at the files? |
||
October 13, 2022, 10:53 |
|
#10 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
When I use the marker name in the Error in my cfg file for a boundary condition, it works. I can't say which boundary is it though, so it is not a solution for this problem. |
||
October 13, 2022, 11:37 |
|
#11 |
New Member
Jay Wee
Join Date: Oct 2022
Posts: 6
Rep Power: 4 |
too busy period.... I will try to investigate later today or tomorrow....
|
|
October 13, 2022, 17:39 |
|
#12 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 672
Rep Power: 21 |
Save your result after 1 iteration in su2 as a paraview multiblock file. You can then view the mesh and all the boundaries in paraview.
|
|
October 13, 2022, 18:37 |
|
#13 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Yes, I did that. I guess Salome exports the BCs not the way I wanted. As you can see from the picture, all the edges of domain are selected as surface and groups I defined on Salome are not shown. I imported geometry to Salome as STEP at first. Could it be related with this? |
||
October 14, 2022, 05:54 |
|
#14 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 672
Rep Power: 21 |
use this in su2:
Code:
OUTPUT_FILES= PARAVIEW_MULTIBLOCK Code:
cgnsconvert |
|
October 15, 2022, 10:12 |
|
#15 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Thank you for explanation. I tried "cgnsconvert" before as I mentioned above, output doesn't change. I viewed the output in .vtm format and saw that there is only 1 boundary defined as "BAR_21-1100" and nothing else. It seems as the outer edge of the full domain. I guess I am doing something wrong or there is something wrong with Salome but I couldnt figured it out yet. |
||
October 15, 2022, 10:16 |
|
#16 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 672
Rep Power: 21 |
Did you give the outer boundary a name in salome, like FarField or something? Is the outer boundary somehow taken into account twice in the mesh?
If it is just salome giving the outer boundary some default name, then everything should work as expected. |
|
October 15, 2022, 10:42 |
|
#17 | |
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Yes, I named boundaries as farfield, symmetry and wall. I guess Salome doesn't export boundaries as individuals but sees them as one and names it itself. I uploaded the file if you'd like to check it out. |
||
October 15, 2022, 11:58 |
Solution
|
#18 | ||
Member
Ercan Umut
Join Date: Aug 2022
Posts: 51
Rep Power: 4 |
Quote:
Quote:
I guess it means when we create groups under the mesh module and export it in a format any other than MED, they don't include the groups that was either created or transferred from the geometry module. I exported the mesh as MED, then opened it up with GMSH and exported it again as .su2 file. After these everything seem to worked out. Thanks for your time and help! bigfootedrockmidget, jaywee Last edited by CleverBoy; October 15, 2022 at 15:28. |
|||
October 15, 2022, 12:16 |
|
#19 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 672
Rep Power: 21 |
ok, after some googling it looks like it is a known export problem in salome.
It looks like the solution is indeed to export it to another format and then try to convert it to cgns or su2 with another tool. |
|
November 21, 2022, 16:32 |
|
#20 | |
Member
Giovanni Medici
Join Date: Mar 2014
Posts: 48
Rep Power: 12 |
Quote:
I'm happy to see that you found a way out, I'll definitely worth a try. As for now I've always used a small python routine that I found online and ad-hoc modified, which natively exports in su2 from salome (ASCII). You may give it a try here |
||
Tags |
cgns, mesh, salome |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 08:38 |
decomposePar problem: Cell 0contains face labels out of range | vaina74 | OpenFOAM Pre-Processing | 37 | July 20, 2020 06:38 |
UDF issue | MASOUD | Fluent UDF and Scheme Programming | 14 | December 6, 2012 14:39 |
[Gmsh] 2D Mesh Generation Tutorial for GMSH | aeroslacker | OpenFOAM Meshing & Mesh Conversion | 12 | January 19, 2012 04:52 |
critical error during installation of openfoam | Fabio88 | OpenFOAM Installation | 21 | June 2, 2010 04:01 |