[bmikuz]

Hello everyone,

I run out of ideas how to solve my problem, so I decided to ask for your help here.

I have a mesh made with ICEM and I'd like to import this mesh in OpenFOAM. The mesh has cca 13e6 points and contains solid & fluid regions (it is a model of nuclear reactor fuel assembly with spacer grids and mixing vanes...). I want to simulate the water flow through such geometry and I don't need to calculate heat transfer, so I need only mesh for fluid regions.

The ICEM mesh is saved in fluent format and converted with fluent3DMeshToFoam to OpenFOAM format. If checkMesh is run after that, I get an error:

checkMesh: malloc.c:3551: munmap_chunk: Assertion `ret == 0' failed.
Aborted

I get the same error also when I run decomposePar (or also simpleFoam, potentialFoam,...) on this mesh. If the mesh contains solid and fluid regions, it doesn't have any holes and I don't get any error. The problem arises only if the solid regions are excluded from mesh (in ICEM) and then this mesh with holes is converted in OpenFOAM.

Please help me out! I already tried to increase vm.max_map_count on the system, but it didn't help.

Thanks a lot!

[bmikuz]

I didn't mentioned that the mesh was converted on computer cluster where the older version of OpenFOAM 1.7.1 is installed and used. I also attached log1.txt to this post, where it can be seen the log of command fluent3DMeshToFoam.
Then I did the same conversion in latest OpenFOAM 2.1.1, but on desktop computer. The log file is attached (log2.txt). It can be seen that the process is killed before the end. Do you have any idea what could be the problem? Did I skipped any important step in conversion of fluent to OpenFOAM mesh?

[jhoepken]

Maybe you have too little memory available on the machine, you try to run decomposePar etc. on? The tutorials work correctly?

[bmikuz]

Thank you for your respond, Jens. I didn't mention that I ran this on computer cluster, which has cca 74 GB of ram on main node, so ram was not a problem...
Tutorials worked without problem and also the bigger mesh (cca 18e6 points), which contains solid&fluid regions was "successfully" converted into OpenFoam.

After second thought I think that this problem belongs to the topic OpenFOAM\Meshing & Mesh Conversion\Other Meshers:ICEM, Star, Ansys,... , so I posted my question also on this site:
http://www.cfd-online.com/Forums/ope...-openfoam.html

In order not to duplicate this debate I kindly ask you to post me on the latter site, where I also attached some log files. I apologize for confusion.

[bmikuz]

Here I also appended checkMesh log for bigger mesh (cca 18e6 points), which contains solid&fluid regions and was "successfully" converted in OpenFOAM. As one can see, the non-orthogonality is quite high, although this mesh converge very good in CFX.
To summarize: the attached checkMesh_log has been done on bigger mesh, which contains solid&fluid regions. I need only mesh for fluid region, but such mesh has holes in regions, where solid used to be and this mesh is useless after conversion to OpenFoam. Useless means that whenever I run checkMesh, decomposePar, simpleFoam, potentialFoam on mesh (which do not contains solid regions) I get the error mentioned above.

[wyldckat]

Greetings to all!

Originally Posted by bmikuz

After second thought I think that this problem belongs to the topic OpenFOAM\Meshing & Mesh Conversion\Other Meshers:ICEM, Star, Ansys,... , so I posted my question also on this site:
http://www.cfd-online.com/Forums/ope...-openfoam.html

In order not to duplicate this debate I kindly ask you to post me on the latter site, where I also attached some log files. I apologize for confusion.

I've moved the two posts from the other thread and removed that thread, since you've made this one in the right place Next time you can PM one of the moderators to move the thread for you


As for the question at hand: I'm not sure I understand the differences between the bigger mesh and this smaller one. Are both being exported with both fluid+solid regions, or at least one of them doesn't have the solid region?

Are you able to get a statistics reading in ICEM as you do with checkMesh? There might be some cells that are so complex that cannot be converted to OpenFOAM.
The other possibility is if you've removed the solid region in ICEM and are trying to convert that fluid only mesh to OpenFOAM. In this case, you'll have to somehow patch up first the missing solid interfaces. Which reminds me of this page: http://openfoamwiki.net/index.php/Ho...internal_walls

Best regards,
Bruno

[JanL]

Hi All,

I wanted to convert a very decent hexa mesh created in ICEM to OpenFoam. The quality-checks in ICEM were fine! Conversion with fluentMeshToFoam or fluent3DMeshToFoam went well, without any problems. Running checkMesh resulted in no serious errors. However running checkMesh -allGeometry reported the following two errors:

***Error in face tets: 81 faces with low quality or negative volume decomposition tets.

***Cells with small determinant found, number of cells: 13161

If I run the case, OF aborts after a few hours of calculation without any clear indication of the error

Courant Number mean: 0.000411233 max: 0.445354
Interface Courant Number mean: 2.04923e-05 max: 0.445354
deltaT = 0.000495591
Time = 2

MULES: Solving for alpha1
Liquid phase volume fraction = 0.781159  Min(alpha1) = -1.30355e-18  Max(alpha1) = 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.000408614, Final residual = 5.90198e-10, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 3.99949e-05, Final residual = 1.16145e-10, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 5.59624e-06, Final residual = 1.00657e-10, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 0.000904118, Final residual = 9.74192e-08, No Iterations 17
GAMG:  Solving for p_rgh, Initial residual = 1.35873e-05, Final residual = 8.34209e-08, No Iterations 6
time step continuity errors : sum local = 4.27077e-12, global = -5.66935e-15, cumulative = -2.2038e-10
GAMG:  Solving for p_rgh, Initial residual = 7.67956e-06, Final residual = 8.0873e-08, No Iterations 3
GAMG:  Solving for p_rgh, Initial residual = 5.80541e-07, Final residual = 9.34415e-08, No Iterations 1
time step continuity errors : sum local = 4.78379e-12, global = -1.03453e-13, cumulative = -2.20483e-10
GAMG:  Solving for p_rgh, Initial residual = 2.48911e-07, Final residual = 6.42141e-08, No Iterations 1
GAMG:  Solving for p_rgh, Initial residual = 1.06364e-07, Final residual = 9.29553e-09, No Iterations 16
time step continuity errors : sum local = 4.7589e-13, global = -1.45762e-15, cumulative = -2.20485e-10
ExecutionTime = 56329.6 s  ClockTime = 57288 s

7 additional processes aborted (not shown)

Has this problem occurred to anybody else?
Any suggestions how to convert the fluent mesh differently?

Any comments are highly appreciated.

Regards
Jan

[wyldckat]

Greetings Jan,

I know I've seen a thread that explains a conversion trick for meshes that came for ICEM, Gambit or Fluent, but I can't find it right now

Closest I got was this thread, which addresses also the issue of negative volumes: http://www.cfd-online.com/Forums/ope...me-gambit.html


Although, maybe I've finally found the one I was looking for: http://www.cfd-online.com/Forums/ope...sed-cells.html - says something about ICEM, TGrid and Tpoly...

Best regards,
Bruno

[waiter120]

Hello, for everyone. I want share my solution of converting ICEM CFD hex mesh to OpenFOAM mesh.
This was found thanks to this amazing forum and all of its users.

So my recipe is like that.

1. Prepare mesh in ICEM CFD with all name selections
2. Export it to FLUENT_V6 (for my present experience, you don’t need specify BC in Output -> Boundary Condition (If I am wrong, please correct me))
3. Read mesh in FLUENT
4. Modify names of BC
4a. If you case is multi region (like chtMultiregionFoam). In FLUENT change type of coupled wall. From Wall to Interior (+ add interior- prefix to its name)
5. Change write-type to ascii “file/ binary-files? no”
6. Write .cas file
7. In OpenFOAM work directory
7a. fluentMeshToFoam –wrireZones fluent.cas
7b. splitMeshRegions -cellZones -overwrite

That’s ALL )))

[nb977]

HI everyone !

i am new in openfoam ... i am actually working with a converted mesh from icem to foam to solve for a problem .. the setFields and decomposePar worked just fine but once i used interfoam to solve in parallel i got bunch of error message telling that

keyword nu is undefined in dictionary "/work/nb977/dropletQuad/processor15/constant/transportProperties"

i checked all the files , there is no transportProperties directory , and the one existing in constant/tranportProperties actually has nu defined as you can see below :

FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

phases (water air);

water
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1e-06;
rho rho [ 1 -3 0 0 0 0 0 ] 1000;
CrossPowerLawCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
m m [ 0 0 1 0 0 0 0 ] 1;
n n [ 0 0 0 0 0 0 0 ] 0;
}

BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
k k [ 0 0 1 0 0 0 0 ] 99.6;
n n [ 0 0 0 0 0 0 0 ] 0.1003;
}
}

air
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.48e-05;
rho rho [ 1 -3 0 0 0 0 0 ] 1;
CrossPowerLawCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
m m [ 0 0 1 0 0 0 0 ] 1;
n n [ 0 0 0 0 0 0 0 ] 0;
}

BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
k k [ 0 0 1 0 0 0 0 ] 99.6;
n n [ 0 0 0 0 0 0 0 ] 0.1003;
}
}

sigma sigma [ 1 0 -2 0 0 0 0 ] 0.07;








I am really stuck, please help me !