Mesh Import Issues

#1 · August 7, 2026, 6:46 am

Quote from Kunal Bhatia on August 7, 2026, 6:46 am
Hello BARAM Team,

First of all, I'd like to appreciate the work you've done with BARAM. I've been evaluating the software extensively, and I believe it is one of the most advanced GUIs built on top of an optimized OpenFOAM solver. The solver itself has been performing exceptionally well in our testing.

We have benchmarked numerous cases against ANSYS Fluent and STAR-CCM+, and the CFD results are on par with both commercial solvers. Overall, the simulation capabilities are very impressive.

However, I have encountered one major bottleneck.

The problem occurs while importing complex multi-region meshes, specifically:

Fluent .msh files

OpenFOAM meshes (constant/polyMesh along with multi-region case files)

For relatively simple geometries, mesh import works correctly.

The issue appears only for complex industrial models containing approximately 10–100 regions (multi-region CHT cases). In these cases:

Importing a Fluent .msh file causes BARAM to become unresponsive or appear to hang indefinitely.

Importing the equivalent OpenFOAM case does not read the mesh at all.

An additional observation is that many of these meshes are polyhedral meshes generated and exported from third-party meshing software. These tools export meshes in an OpenFOAM-compatible constant/polyMesh format, and the meshes can be used successfully in OpenFOAM itself. However, BARAM is currently unable to read these exported meshes.

Could you please advise whether there are any specific compatibility requirements or preprocessing steps needed before importing such meshes into BARAM? If not, is this a known limitation of the current mesh importer, and are there any plans to improve compatibility with third-party OpenFOAM mesh formats?

I have attached a pipe flow cht & complex multi-region cht mesh files that reproduces the issue. I would greatly appreciate it if your team could investigate this case and help identify the root cause.

https://drive.google.com/drive/folders/1y7fBc2FF4_k0dtVEdnuMMU44gvSK6njA?usp=drive_link

Over the past year, I have been independently testing BARAM on more than 100 CFD cases, including many extremely complex industrial models, while benchmarking against ANSYS Fluent and STAR-CCM+. Through this process, I've identified several strengths as well as areas where the workflow could be further improved.

If it would be helpful, I would be happy to discuss my findings with your team or arrange a meeting. I believe the feedback from these benchmark studies and real-world industrial cases could help improve BARAM, particularly in terms of robustness and usability for complex engineering applications.

From my evaluation so far, this mesh import capability is the significant bottleneck I have found. Once support for importing large, complex multi-region meshes and third-party OpenFOAM mesh formats is more robust, I believe BARAM will become an even stronger platform for industrial CFD workflows.

Thank you for your excellent work on BARAM. I look forward to your guidance and any possible solution to this issue.

Hello BARAM Team,

First of all, I'd like to appreciate the work you've done with BARAM. I've been evaluating the software extensively, and I believe it is one of the most advanced GUIs built on top of an optimized OpenFOAM solver. The solver itself has been performing exceptionally well in our testing.

We have benchmarked numerous cases against ANSYS Fluent and STAR-CCM+, and the CFD results are on par with both commercial solvers. Overall, the simulation capabilities are very impressive.

However, I have encountered one major bottleneck.

The problem occurs while importing complex multi-region meshes, specifically:

Fluent .msh files
OpenFOAM meshes (constant/polyMesh along with multi-region case files)

For relatively simple geometries, mesh import works correctly.

The issue appears only for complex industrial models containing approximately 10–100 regions (multi-region CHT cases). In these cases:

Importing a Fluent .msh file causes BARAM to become unresponsive or appear to hang indefinitely.
Importing the equivalent OpenFOAM case does not read the mesh at all.

An additional observation is that many of these meshes are polyhedral meshes generated and exported from third-party meshing software. These tools export meshes in an OpenFOAM-compatible constant/polyMesh format, and the meshes can be used successfully in OpenFOAM itself. However, BARAM is currently unable to read these exported meshes.

Could you please advise whether there are any specific compatibility requirements or preprocessing steps needed before importing such meshes into BARAM? If not, is this a known limitation of the current mesh importer, and are there any plans to improve compatibility with third-party OpenFOAM mesh formats?

I have attached a pipe flow cht & complex multi-region cht mesh files that reproduces the issue. I would greatly appreciate it if your team could investigate this case and help identify the root cause.

https://drive.google.com/drive/folders/1y7fBc2FF4_k0dtVEdnuMMU44gvSK6njA?usp=drive_link

Over the past year, I have been independently testing BARAM on more than 100 CFD cases, including many extremely complex industrial models, while benchmarking against ANSYS Fluent and STAR-CCM+. Through this process, I've identified several strengths as well as areas where the workflow could be further improved.

If it would be helpful, I would be happy to discuss my findings with your team or arrange a meeting. I believe the feedback from these benchmark studies and real-world industrial cases could help improve BARAM, particularly in terms of robustness and usability for complex engineering applications.

From my evaluation so far, this mesh import capability is the significant bottleneck I have found. Once support for importing large, complex multi-region meshes and third-party OpenFOAM mesh formats is more robust, I believe BARAM will become an even stronger platform for industrial CFD workflows.

Thank you for your excellent work on BARAM. I look forward to your guidance and any possible solution to this issue.

#2 · August 8, 2026, 9:59 am

Hi Mr. Bhatia,

Thank you for the kind words, and for taking the time to share such detailed feedback.

We have received the mesh files you shared, one Fluent mesh file and three OpenFOAM cases:

Electronics.msh
pipe-flow-cht-reference-mesh-1
pipe-flow-cht-reference-mesh-2
pipe-flow-cht-reference-mesh-3

Regarding the OpenFOAM cases, I found that they use a rather old file format. There are two points in particular:

1. constant/regionProperties

The files are written in the legacy style:

fluidRegionNames    ( fluid-mid fluid-outlet fluid-Inlet );
solidRegionNames    ( solid-pipe );
fluidBasicThermo    (basicPsiThermo);

In the current format, it should be written as follows:

regions
(
    fluid
    (
        fluid-mid
        fluid-outlet
        fluid-Inlet
    )
    solid
    (
        solid-pipe
    )
);

2. polyPatch types

The directMappedWall type has been deprecated and replaced by mappedWall in modern standard OpenFOAM:

interface-f-in-to-f-mid
{
    type            directMappedWall;
    startFace       349830;
    nFaces          626;
    sampleMode      nearestPatchFace;
    sampleRegion    fluid-mid;
    samplePatch     interface-f-in-to-f-mid;
}

After updating these two items, I confirmed that the cases could be imported into BARAM without any problem.

As for the Fluent mesh file, I have reproduced the issue you reported, but identifying the root cause will take a little more time. I will get back to you as soon as I have something to share.

I'm also very glad to hear that you are willing to share your findings with us. Feedback from over 100 benchmark cases would be a great boost for BARAM. Once I have identified the root cause of the Fluent mesh issue, I would be happy to arrange a meeting at your convenience.

Thank you again.

-- Jake

#3 · August 12, 2026, 4:22 pm

Quote from bykima5230416a7 on August 12, 2026, 4:22 pm
Hi Kunal Bhatia,

I tested fluent msh file convert in baramFlow.

When converting fluent msh file in baramFlow, the conversion itself completes successfully, but it appears that a problem occurs while loading the converted mesh.

Although the exact cause of this issue is unknown, it may be due to mesh quality issues. Several regions contain serious problems, such as negative volume and open cells. I suspect this problem may have originated when the mesh was converted to an msh file in EnnovaCFD.

Until now, there have been no conversion issues like this with various meshes containing a large number of regions.

Thanks,

The following is a portion of the checkMesh results of converted mesh.

----------------

Checking geometry...
Overall domain bounding box (-3970.59139393 -0.323555698042 -4873.25617158) (8906.76649053 10460.8516488 8592.15236139)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
***Boundary openness (1.58439539679e-05 1.26210164743e-15 -1.36263527843e-05) possible hole in boundary description.
***Open cells found, max cell openness: 0.333130295509, number of open cells 4
<<Writing 4 non closed cells to set nonClosedCells
<<Writing 95 cells with high aspect ratio to set highAspectRatioCells
***Zero or negative face area detected. Minimum area: 0
<<Writing 1 zero area faces to set zeroAreaFaces
Min volume = -7.01194110232e-24. Max volume = 3.762337389e-09. Total volume = 4.80320921632e-06
***Zero or negative cell volume detected. Minimum negative volume: -7.01194110232e-24, Number of negative volume cells: 46
<<Writing 46 zero volume cells to set zeroVolumeCells
Mesh non-orthogonality Max: 90 average: 5.75812658528
*Number of severely non-orthogonal (> 70 degrees) faces: 10.
***Number of non-orthogonality errors: 11.
<<Writing 21 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 4 faces are incorrectly oriented.
<<Writing 4 faces with incorrect orientation to set wrongOrientedFaces
***Max skewness = 4.17369163786e+126, 79 highly skew faces detected which may impair the quality of the results
<<Writing 79 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 8 mesh checks.

Hi Kunal Bhatia,

I tested fluent msh file convert in baramFlow.

When converting fluent msh file in baramFlow, the conversion itself completes successfully, but it appears that a problem occurs while loading the converted mesh.

Although the exact cause of this issue is unknown, it may be due to mesh quality issues. Several regions contain serious problems, such as negative volume and open cells. I suspect this problem may have originated when the mesh was converted to an msh file in EnnovaCFD.

Until now, there have been no conversion issues like this with various meshes containing a large number of regions.

Thanks,

The following is a portion of the checkMesh results of converted mesh.

----------------

Checking geometry...
Overall domain bounding box (-3970.59139393 -0.323555698042 -4873.25617158) (8906.76649053 10460.8516488 8592.15236139)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
***Boundary openness (1.58439539679e-05 1.26210164743e-15 -1.36263527843e-05) possible hole in boundary description.
***Open cells found, max cell openness: 0.333130295509, number of open cells 4
<<Writing 4 non closed cells to set nonClosedCells
<<Writing 95 cells with high aspect ratio to set highAspectRatioCells
***Zero or negative face area detected. Minimum area: 0
<<Writing 1 zero area faces to set zeroAreaFaces
Min volume = -7.01194110232e-24. Max volume = 3.762337389e-09. Total volume = 4.80320921632e-06
***Zero or negative cell volume detected. Minimum negative volume: -7.01194110232e-24, Number of negative volume cells: 46
<<Writing 46 zero volume cells to set zeroVolumeCells
Mesh non-orthogonality Max: 90 average: 5.75812658528
*Number of severely non-orthogonal (> 70 degrees) faces: 10.
***Number of non-orthogonality errors: 11.
<<Writing 21 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 4 faces are incorrectly oriented.
<<Writing 4 faces with incorrect orientation to set wrongOrientedFaces
***Max skewness = 4.17369163786e+126, 79 highly skew faces detected which may impair the quality of the results
<<Writing 79 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 8 mesh checks.