[skuznet]

Hello!

I'm trying to generate a mesh for conjugate heat transfer using snappyHexMesh utility.
I have two stl files for fluid and solid geometries where various patches including fluid_to_solid and solid_to_fluid are defined.

When I run snappyHexMesh I get a number of domains called
domain1
domain2
...
etc

instead of just two domain solid and fluid.

Does anyone have an idea what is going wrong?

Thank you!

************************************************** **********
it looks like there are some problems with the surface, the surfaceCheck utility says that

sergkuznet@ubuntu:/media/ubuntu/run/UCcases/UCsideOptShort_run/constant/triSurface$ surfaceCheck fluid.stl
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.x-37940e0cd1ae
Exec   : surfaceCheck fluid.stl
Date   : May 27 2014
Time   : 23:30:17
Host   : "ubuntu"
PID    : 5557
Case   : /media/ubuntu/run/UCcases/UCsideOptShort_run/constant/triSurface
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Reading surface from "fluid.stl" ...

Statistics:
Triangles    : 5270
Vertices     : 2491
Bounding Box : (-0.002424 -0.00101 -0.000606) (0.004848 0.001414 0.003838)

Region	Size
------	----
fluid_to_solid	4878
maxX	2
minX	2
maxY	168
minY	12
maxZ	96
minZ	112


Surface has no illegal triangles.

Triangle quality (equilateral=1, collapsed=0):
    0 .. 0.05  : 0.232827
    0.05 .. 0.1  : 0.0757116
    0.1 .. 0.15  : 0.0538899
    0.15 .. 0.2  : 0.0724858
    0.2 .. 0.25  : 0.103226
    0.25 .. 0.3  : 0.0242884
    0.3 .. 0.35  : 0.0616698
    0.35 .. 0.4  : 0.0390892
    0.4 .. 0.45  : 0.0180266
    0.45 .. 0.5  : 0.0242884
    0.5 .. 0.55  : 0.059203
    0.55 .. 0.6  : 0.0440228
    0.6 .. 0.65  : 0.027704
    0.65 .. 0.7  : 0.0163188
    0.7 .. 0.75  : 0.0129032
    0.75 .. 0.8  : 0.0178368
    0.8 .. 0.85  : 0.00227704
    0.85 .. 0.9  : 0.0366224
    0.9 .. 0.95  : 0.0377609
    0.95 .. 1  : 0.0398482

    min 3.65063e-05 for triangle 3175
    max 0.999997 for triangle 1354

Edges:
    min 5.32471e-05 for edge 192 points (0.001616 -0.00101 0.00277059)(0.00159507 -0.00101 0.00272163)
    max 0.00506211 for edge 7488 points (0.004848 0.001414 0.003838)(0.004848 -0.00101 -0.000606)

Checking for points less than 1e-6 of bounding box ((0.007272 0.002424 0.004444) meter) apart.
Found 0 nearby points.

Surface is not closed since not all edges connected to two faces:
    connected to one face : 18
    connected to >2 faces : 0
Conflicting face labels:18
Dumping conflicting face labels to "problemFaces"
Paste this into the input for surfaceSubset

Number of unconnected parts : 1

Number of zones (connected area with consistent normal) : 1


End

I prepared parts of this surface in salome and then named them and joined together manually and they looked ok visually. I did open surface in HelyxOS and surface looked ok, but when I open it in meshlab i can see several large holes in my surface (if I open separate parts, before they were joined, there are no holes).
I guess it might be due to intersecting surfaces?
What do I do with this? Any suggestions?

I tried to run surfaceClean but it didn't help and I'm not sure which parameters to use - minlength, min quality/


************************************************** ************************************************** ************
I used
https://netfabb.azurewebsites.net/
to fix my surfaces.


no surfaceCheck says

sergkuznet@ubuntu:/media/ubuntu/run/UCcases/UCsideOptShort_run/constant/triSurface$ surfaceCheck solid.stl
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.x-37940e0cd1ae
Exec   : surfaceCheck solid.stl
Date   : May 28 2014
Time   : 10:52:13
Host   : "ubuntu"
PID    : 9647
Case   : /media/ubuntu/run/UCcases/UCsideOptShort_run/constant/triSurface
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Reading surface from "solid.stl" ...

Statistics:
Triangles    : 4776
Vertices     : 2234
Bounding Box : (-2e-06 -0.00201 -0.000606) (0.002424 0.001414 0.003836)

Region	Size
------	----
patch0	4776


Surface has no illegal triangles.

Triangle quality (equilateral=1, collapsed=0):
    0 .. 0.05  : 0.210008
    0.05 .. 0.1  : 0.0822864
    0.1 .. 0.15  : 0.0527638
    0.15 .. 0.2  : 0.0728643
    0.2 .. 0.25  : 0.0768425
    0.25 .. 0.3  : 0.0249162
    0.3 .. 0.35  : 0.0464824
    0.35 .. 0.4  : 0.0456449
    0.4 .. 0.45  : 0.0303601
    0.45 .. 0.5  : 0.0276382
    0.5 .. 0.55  : 0.0406198
    0.55 .. 0.6  : 0.0406198
    0.6 .. 0.65  : 0.0372697
    0.65 .. 0.7  : 0.00942211
    0.7 .. 0.75  : 0.0247069
    0.75 .. 0.8  : 0.0500419
    0.8 .. 0.85  : 0.00439698
    0.85 .. 0.9  : 0.0316164
    0.9 .. 0.95  : 0.0450168
    0.95 .. 1  : 0.0464824

    min 4.18994e-06 for triangle 2236
    max 0.99973 for triangle 4741

Edges:
    min 1.99996e-06 for edge 3492 points (0.000404 0.000808 -0.000534)(0.000404 0.000806 -0.000534)
    max 0.00185613 for edge 3582 points (0.002114 -0.00101 0.000222)(0.000258 -0.00101 0.0002)

Checking for points less than 1e-6 of bounding box ((0.002426 0.003424 0.004442) meter) apart.
Found 0 nearby points.

Surface is closed. All edges connected to two faces.

Number of unconnected parts : 1

Number of zones (connected area with consistent normal) : 1


End

so looks that my surface is ok now, however, I lost all my surface definitions, so can't apply BC, and
when I run snappyHexMesh it still creates a number of spurious domains
domain1
domain2
....

[Quin404]

Hello!

Sorry I understand this thread is a little old now, however did you manage to find a solution to the problem, as I have been having the same issue?

Thank you

[Quin404]

Thought it would best to let people know that I did find the issue to my problem some time ago...

I had multiple components under the same part name in the same ".stl" file.

For example, I had 10 Heat pads all in different locations, essentially having 10 different solid domains, but had defined them under the same part - "HeatPads".

So I had to rename them as individual parts, e.g. HeatPad1, HeatPad2 etc and export them as individual ".stl" files.

This then removed the random domain names

(Sorry, I do understand this was a very basic mistake!)

[wyldckat]

To add to Quin404's answer, I'll quote from openfoamwiki.net: http://openfoamwiki.net/index.php/Sn...-region_meshes

Instructions on how to remove an external unwanted region: Background Mesh in snappy with multi domain (CHT) post #3

• Note: this happens whenever the base mesh doesn't coincide with the outer limits of the target surface geometry. The tutorial heatTransfer/chtMultiRegionFoam/snappyMultiRegionHeater is such an example where the outside of the original STL files coincides with the base mesh.