|
[Sponsors] |
Mismatch between NPOIN and number of points listed in mesh file - Export Gmsh to SU2 |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 5, 2023, 05:37 |
Mismatch between NPOIN and number of points listed in mesh file - Export Gmsh to SU2
|
#1 |
New Member
Rafael Gomes Batista
Join Date: Apr 2023
Posts: 12
Rep Power: 3 |
Dear someone who might be able to help,
I have recently started using SU2 for compressible CFD analysis, and I have encountered an issue while replicating a 2D compressible flow over an unsteady NACA 0012 from a SU2 tutorial, using structured or unstructured grids that I created in GMSH. When I use the input mesh (unsteady_naca0012_mesh.su2) from the tutorial website (https://su2code.github.io/tutorials/Unsteady_NACA0012/), I have no trouble running the simulation. However, when I use both structured and unstructuredgrids I created in GMSH, I get this error. During the simulation, I received the following error message: Error in "void CPhysicalGeometry:istributeColoring(const CConfig*, CGeometry*)": ------------------------------------------------------------------------- Mismatch between NPOIN and number of points listed in mesh file. Please check the mesh file for correctness. ------------------------------ Error Exit ------------------------------- I am attempting this tutorial because I plan to analyze a 2D compressible flow over NACA 0012 in the future with a personalized configuration file. This situation seems strange because I have created meshes for other SU2 tutorials, such as the laminar cylinder (https://su2code.github.io/tutorials/Laminar_Cylinder/) and the oblique shock (https://su2code.github.io/tutorials/Inviscid_Wedge/), both in GMSH, and I was able to run the cases in SU2 with no issues. I have tried adding a physical group as a physical surface in GMSH, as suggested by several individuals, and I have tried both checking and unchecking the box that says "Save all elements". However, I encountered a new error message, which seems to be caused by adding a new marker that isn't present in the configuration file: Error in "short unsigned int CConfig::GetMarker_CfgFile_TagBound(std::string) const": ------------------------------------------------------------------------- The configuration file doesn't have any definition for marker fluid_domain ------------------------------ Error Exit ------------------------------- I have checked to ensure that there are no unused points, construction lines, or geometries in the mesh and it doesn't seems to have. Initially I have defined only the two boundary conditions necessary for the tutorial, which are: % BOUNDARY CONDITIONS % MARKER_HEATFLUX= ( airfoil, 0.0 ) MARKER_FAR= ( farfield ) MARKER_PLOTTING= ( airfoil ) MARKER_MONITORING= ( airfoil ) I have defined a physical curve "airfoil" for the airfoil and another physical curve for the "farfield" in GMSH. So what could be causing this error? I couldn't understand the issue here. Here is the link to the tutorial on the official website: https://su2code.github.io/tutorials/Unsteady_NACA0012/ I have attached the geometry mesh file in GMSH (.geo), the SU2 mesh file (.su2) and also the configuration file (.cfg). If someone could help, I would be extremely grateful! Thank you so much to whoever can help me. Last edited by rgbatista; May 5, 2023 at 05:41. Reason: grammar error in the text |
|
May 5, 2023, 07:56 |
|
#2 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 633
Rep Power: 18 |
There was a bug in gmsh in the su2 writer that was introduced 8 months ago and was fixed last month,. It might be related to this. I think the issue is restricted to gmsh 4.11.*
In any case, I opened your .geo with my old gmsh, clicked "mesh ->2D" to generate the mesh, exported to su2 format, keeping the option 'save all elements' deselected, and I got an su2 file which worked on your configuration. Your .su2 file did not have the element connectivity information saved (at the start of the su2 file, it says NELEM=0) |
|
May 9, 2023, 07:01 |
|
#3 | |
New Member
Rafael Gomes Batista
Join Date: Apr 2023
Posts: 12
Rep Power: 3 |
Quote:
Just to confirm if I understood correctly, were you able to run the simulation with my GMSH file? Or were you unable to run it? I ask this because when I run the simulation after exporting the GMSH file into a .su2 format, with the "Save all elements" option deselected, I encounter an error related to the fluid_marker, created by the physical surface "fluid_domain". This marker appears in the error message: Error in "short unsigned int CConfig::GetMarker_CfgFile_TagBound(std::string) const": ------------------------------------------------------------------------- The configuration file doesn't have any definition for marker fluid_domain ------------------------------ Error Exit ------------------------------- I believe this error occurs because the marker "fluid_domain" was not defined in the configuration file. I checked the markers on the SU2 website (https://su2code.github.io/docs_v7/Ma...x-no-slip-wall), and I did not find a specific marker for the general fluid domain of the mesh. So I would like to ask if you were able to run the simulation? If so, did it run without any problems or did you encounter this error message? If there were no errors, could you please let me know which versions of SU2 and GMSH you used? I have tried with an older version of GMSH (4.8.0), and I encountered the same error. Thank you very much for your help! |
||
May 9, 2023, 07:54 |
|
#4 |
Senior Member
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 633
Rep Power: 18 |
I have gmsh 4.8.4 and I could start an SU2 simulation with your cfg and the mesh that I've made from your .geo file. The fluid domain is not written to the su2 file in my case.
Are you sure that you were using an older gmsh version, because it sounds exactly like the bug that was introduced. I downloaded gmsh 4.11.1 and that version writes the fluid_domain marker to the file and gives the error that you mention. |
|
May 9, 2023, 11:18 |
|
#5 | |
New Member
Rafael Gomes Batista
Join Date: Apr 2023
Posts: 12
Rep Power: 3 |
Quote:
After downloading GMSH version 4.8.0, I realized that even though I thought I had opened the older version by right-clicking and selecting "Open with..." and choosing the GMSH application from the 4.8.0 folder, it actually opened the newer version. So, after removing the newer version from my laptop, I tried again and confirmed the version in GMSH by going to "Help » About Gmsh." Then, I exported to .su2 without any problems, and the fluid_domain marker, which was created by the Physical Surface function, did not appear in the file as expected. In summary, as you mentioned, the problem or bug is likely related to this particular version of GMSH. Thank you so much for your help. I am very grateful for your assistance and contribution. Best regards, Rafael Batista |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Gmsh to SU2: NPOIN | mhollander | SU2 | 3 | May 17, 2023 08:13 |
NPOIN Mismatch Mesh Error | Shruti Arumbakkam | SU2 | 16 | February 10, 2023 19:02 |
GMSH and SU2 NPOIN/NELEM Errors | djpicho | SU2 | 5 | March 9, 2021 16:12 |