[Jordan.]

I'm trying (and failing) to run a chtMultiRegionFoam case with an imported mesh. In paraview I am getting these weird reds boxes (see photo) they normally appear on mesh boundary's but here they we all over the shop!

boxes.jpg

[wyldckat]

Greetings Jordan,

That usually happens to me when I mess up a step that involved renumberMesh.
Essentially, the problem was that even though the mesh seemed OK, the point/face/cell identification was torn apart by something else, leading to the field values to be incorrectly associated to the mesh cells.

My advice is that you review carefully all of the steps you've taken to convert the mesh and to prepare the simulation. If the mesh is considerably heavy (1 million cells or more), then start over with something more simple, so that you can review all of the steps more quickly and do some trial-and-error attempts.

Best regards,
Bruno

[Jordan.]

Thank-you very much for the reply Bruno! I am quite confused to how I messed up the Mesh, all I am trying to do is demonstrate heat transfer from a solid-solid, solid-fluid and fluid-solid for a Mesh from fluent (my Mesh is essentially a column of different regions of mesh that I have defined as different solids and a fluid). My instructions followed are as follows:

fluentMeshToFoam constant/polyFoam/thermo9FL.msh -writeSets
setsToZones -noFlipMap
splitMeshRegions -cellZones -overwrite

Then delete all 0/region/files that are not applicable to solids/fluids.

ChangeConditions (a bash file I wrote to run changeDictionary for all regions in turn)

Then I renamed all *Zones by adding .bak

StitchMeshes (another bash file that runs stitchMesh -overwrite -perfect on all internal walls)

Then remove the new cellZones and remove the .bak from the old one
Then delete all boundary's with 0 in nFaces in constant/polyMesh/boundarys

checkMesh (says its ok)

Then change all boundary's in constant/region/polyMesh/boundarys to mappedwall for the internal walls to match the 0 condition of compressible::turbulentTemperatureCoupledBaffleMix ed that is set up.

Then move meshPhi form the 0 folder to 0/topRegionInTheFolder (otherwise I get an error)

chtMultiRegionFoam
paraFoam

----------end

Additionally: why does there need to be a small velocity passing though a fluid to make the fluid allow heat to flow from one of its boundary's e.g. use 'fixedValue' and set a wall surrounding a fluid to 500K, it only heats up the fluid if there is a small velocity running though it. I have the same problem with a solid however have no solution to make the heat move throughout it.

I am currently using OpenFOAM V2.1

I have attached my working folders but note that I had to upload the constant folder separately and had to delete some of its files so it would upload (eg faces, the mesh, sets, ...)

Thanks again

Jordan Salmon

[wyldckat]

Hi Jordan,

I took a very quick look at the files you attached and didn't see anything out of the ordinary... but I might have been too quick. Well, there was one detail: the ones of type "zeroGradient" do not need a "value" entry.

Nonetheless, there are a couple of details I can see right now from your description and point out:

1. Do not manually remove regions from the folder/file structure. OpenFOAM might get confused in numbering the mesh. The correct way to do this is explained here: http://www.cfd-online.com/Forums/ope...tml#post341623 - post #3
2. Moving "meshPhi" is very likely the real reason why you're getting some really strange data. If I remember correctly, that file pretty much defines any mesh morphing that has occurred on the mesh from the previous iteration (in this case, the one in "constant").

My usual suggestion in these kinds of scenario where the person is still not familiar enough with everything associated to a simulation to be performed, is to take a few steps back and first try to create a working work-flow by using a simpler case. One such example can be found here: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D - try reproducing this simple case using a mesh created with Fluent.


I'll try this coming weekend to look into the other detail you mentioned, regarding there not being any heat being exchanged when the fluid is stopped... that's really odd... either conduction is not accounted for in the fluid region or there is a small detail missing in the boundary conditions.

Best regards,
Bruno

[Jordan.]

Hi Bruno,

Thank you very much again for your helpful reply, I have had a quick look at the example you mentioned, the mesh I am trying above is equally simply but just in 3D, I have attached my starting folder setup as it may be easier to see where I am going wrong. I have modelled it on the multiRegionHeater example. The only place I have to use different bash commands is when they use topoSet (in the Allrun file) (I also assume this creates the mappedPatchBase boundary for the tutorial case as I have to type mine manually in the boundary files). I understand setSet is another way of doing this and I have followed the link you posted.

From the folder attached I typed:

fluentMeshToFoam constant/polyMesh/thermo9FL.msh -writeSets
setsToZones -noFlipMap

Then I created a file called batch.setSet containing:

 
cellSet isolation new zoneToCell solid-1
cellSet isolation add zoneToCell solid-2
cellSet isolation add zoneToCell fluid-3
cellSet isolation add zoneToCell solid-4
cellSet isolation subset

Then:
setSet -batch batch.setSet (This created a VTK folder.)
subsetMesh -overwrite isolation

Then I get multiple Foam Warnings to do with the U folder expecting uniform or non-uniform - even though it has got uniform and non uniform.
Then:

splitMeshRegions -cellZones -overwrite
Tidy0
ChangeConditions
Change all constant/'region'/polyMesh/boundary files to include mapped walls.
Apply an initial condition of solid-1 = 400K at the start (internalFeild uniform 400)
chtMultiRegionFoam

Then I get an error, after it calculates 0.7s of time:

No Iterations 27

--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded
    From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
    in file /home/bmss/OpenFOAM/OpenFOAM-2.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69.
FOAM aborting
 
Backtrace:
        ZN10StackTraceC1Ev [0x6c5815c0+80]
                 module: C:\PROGRA~2\BLUECF~1.1\OpenFOAM-2.1\platforms\linuxmingw-w64DPOpt\lib\libstack_trace.dll
        (No symbol) [0x2eed610]
        RtlCaptureContext [0x7711baa0+0]
                 module: C:\Windows\system32\kernel32.dll
        ZNK4Foam12hConstThermoINS_14incompressibleEE5limitEd [0x620396c0+0]
                 module: C:\PROGRA~2\BLUECF~1.1\OpenFOAM-2.1\platforms\linuxmingw-w64DPOpt\lib\libbasicThermophysicalModels.dll
        (No symbol) [0x550278]
        RtlNtdllName [0x77405430+32]
                 module: C:\Windows\SYSTEM32\ntdll.dll
        (No symbol) [0x2b6fac0]
        (No symbol) [0x10]
        (No symbol) [0x540000]
        (No symbol) [0x8]
        (No symbol) [0x54026c]
        (No symbol) [0x19200010000f]
        (No symbol) [0x53002b002b0033]
        (No symbol) [0x206002b002b]
        (No symbol) [0x7205a0]
        (No symbol) [0x773c800250006]
        (No symbol) [0x540230]
This application has requested the Runtime to terminate it in an unusual way.
Please contact the application's support team for more information.

The 0.7s it does calculate there is no heat transfer...?? but at least the weird red boxes are gone.

Thank you again for all the help you are giving me you are a life saver!
NOTE: I have not attached the mesh as it is too large to upload - do you want me to try and dropbox it??

Best Regards,
Jordan

[Jordan.]

I halved the value of delta T and now it does not come up with this error - however I still get no heat transfer. I have tried setting the walls hot - doesn't even spread though the solid/fluid it is part of. And I have tried having whole regions starting hot but no temperature crosses region boundary's!!

I'm so confused, my case looks just like the multiRegionHeater...

Thanks again for all the help,

Best Regards,

Jordan

[Jordan.]

Dear Bruno,

I was just wandering whether you have any further ideas on what might help me to get this case to work.

Best Regards,

Jordan Salmon.

[Jordan.]

I managed to sort this!!! I wasn't sharing the topology in Design Modeller - opps!

thanks a lot for all your help

Jordan

[wyldckat]

Hi Jordan,

I'm sorry, I wasn't able to find enough time to help here on the forum

But I'm very glad you've managed to solve this yourself and many thanks for sharing the solution!

Best regards,
Bruno