CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

Mismatch between NPOIN and number of points listed in mesh file - Export Gmsh to SU2

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By rgbatista

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 5, 2023, 04:37
Default 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: 3
Rep Power: 2
rgbatista is on a distinguished road
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.
Attached Files
File Type: zip CFD_Online.zip (13.3 KB, 5 views)

Last edited by rgbatista; May 5, 2023 at 04:41. Reason: grammar error in the text
rgbatista is offline   Reply With Quote

Old   May 5, 2023, 06:56
Default
  #2
Senior Member
 
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 341
Rep Power: 15
bigfootedrockmidget is on a distinguished road
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)
bigfootedrockmidget is offline   Reply With Quote

Old   May 9, 2023, 06:01
Default
  #3
New Member
 
Rafael Gomes Batista
Join Date: Apr 2023
Posts: 3
Rep Power: 2
rgbatista is on a distinguished road
Quote:
Originally Posted by bigfootedrockmidget View Post
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)
First of all, I would like to thank you for your availability and effort in helping me, as well as for the quick reply.

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!
rgbatista is offline   Reply With Quote

Old   May 9, 2023, 06:54
Default
  #4
Senior Member
 
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 341
Rep Power: 15
bigfootedrockmidget is on a distinguished road
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.
bigfootedrockmidget is offline   Reply With Quote

Old   May 9, 2023, 10:18
Default
  #5
New Member
 
Rafael Gomes Batista
Join Date: Apr 2023
Posts: 3
Rep Power: 2
rgbatista is on a distinguished road
Quote:
Originally Posted by bigfootedrockmidget View Post
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.
You were correct when you mentioned that the issue was related to the GMSH version.


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
rgbatista is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Gmsh to SU2: NPOIN mhollander SU2 3 May 17, 2023 07:13
NPOIN Mismatch Mesh Error Shruti Arumbakkam SU2 16 February 10, 2023 18:02
GMSH and SU2 NPOIN/NELEM Errors djpicho SU2 5 March 9, 2021 15:12


All times are GMT -4. The time now is 11:52.