[Talaat]

I have a geometry where I have a cylinder and inside it I have many smaller cylinders made of different materials. Is there a way I could define a mappedWall condition for the big cylinder's inner wall with each of the smaller cylinders' walls?

It's impractical to divide the big cylinder into the same number of regions. I have more than 50 cylinders inside.

Edit: I apologize about the typo in the title.

[pete20r2]

I had a similar problem to this.
I found if I blockMesh the entire mesh, then use topSet to make cellZones, then used splitMeshRegions -cellZones the boundaries are automatically created in the form:

FoamFile
{
    version     0.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/cell_1/polyMesh";
    object      boundary;
}

    cell_1_to_channelT
    {
        type            mappedWall;
        inGroups        1 ( wall );
        nFaces          1600;
        startFace       445600;
        sampleMode      nearestPatchFace;
        sampleRegion    channelT;
        samplePatch     channelT_to_cell_1;
    }

There are 16 cells in my case all with contacts to the "channel" region.

By doing this and having default p,T,U fields in 0 when doing the split, I can control all of the patches in the similar regions by using a linux trick.
I create a system folder for cell_1 and then link the system folder for cell_2-16 to cell_1
I have this script in the system folder to make it quickly:

#!/bin/bash
cd ${0%/*} || exit 1    # run from this directory

for i in cell_2 cell_3 cell_4 cell_5 cell_6 cell_7 cell_8 cell_9 cell_10 cell_11 cell_12 cell_13 cell_14 cell_15 cell_16
do
   ln -s cell_1 $i
done

Then I setup a changeDictionaryDict file in system\cell_1 (which will now apply to all regions cell_x)
It's written using widcards for the region numbers so it can run on all regions:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
T
    {
        internalField   uniform 300;

		boundaryField
		{
    		"cell_.*_to_channel.*"
    		{
        		type            compressible::turbulentTemperatureCoupledBaffleMixed;
        		Tnbr            T;
        		thicknessLayers ( 1.5e-05 );
        		kappaLayers     ( 2 );
        		kappaMethod     solidThermo;
        		value           uniform 300;

Then just run changeDict on all regions and you should be good to go

[Talaat]

Originally Posted by pete20r2

I had a similar problem to this.
I found if I blockMesh the entire mesh, then use topSet to make cellZones, then used splitMeshRegions -cellZones the boundaries are automatically created in the form:

FoamFile
{
    version     0.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/cell_1/polyMesh";
    object      boundary;
}

    cell_1_to_channelT
    {
        type            mappedWall;
        inGroups        1 ( wall );
        nFaces          1600;
        startFace       445600;
        sampleMode      nearestPatchFace;
        sampleRegion    channelT;
        samplePatch     channelT_to_cell_1;
    }

There are 16 cells in my case all with contacts to the "channel" region.

By doing this and having default p,T,U fields in 0 when doing the split, I can control all of the patches in the similar regions by using a linux trick.
I create a system folder for cell_1 and then link the system folder for cell_2-16 to cell_1
I have this script in the system folder to make it quickly:

#!/bin/bash
cd ${0%/*} || exit 1    # run from this directory

for i in cell_2 cell_3 cell_4 cell_5 cell_6 cell_7 cell_8 cell_9 cell_10 cell_11 cell_12 cell_13 cell_14 cell_15 cell_16
do
   ln -s cell_1 $i
done

Then I setup a changeDictionaryDict file in system\cell_1 (which will now apply to all regions cell_x)
It's written using widcards for the region numbers so it can run on all regions:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
T
    {
        internalField   uniform 300;

		boundaryField
		{
    		"cell_.*_to_channel.*"
    		{
        		type            compressible::turbulentTemperatureCoupledBaffleMixed;
        		Tnbr            T;
        		thicknessLayers ( 1.5e-05 );
        		kappaLayers     ( 2 );
        		kappaMethod     solidThermo;
        		value           uniform 300;

Then just run changeDict on all regions and you should be good to go

Thanks for your help. Did you have 16 channel.* regions? If so, did you use inletOutlet boundary condition for the velocity at the region interfaces or what condition did you use?

[pete20r2]

I'm using a mapped inlet to develop the inlet velocity profile.
U is zeroGradient on outlet.
p is zeroGradient on inlet, fixedMean 0 on the outlet.
I know there are no flow reversals across my boudaries so I'm getting away with it, inletOutlet is a good idea to start with to improve the chances of getting a converged solution. Might not be accurate but will get you running.
There are 2 fluid channels contacting 16 solid regions, each solid region has a patch to each fluid region.

[suoCFD]

I wrote this with something misunderstanding.