CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Coupling patches in chtMultiRegionSimpleFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 2 Post By Bloerb

Reply
 
LinkBack Thread Tools Display Modes
Old   May 27, 2016, 13:23
Default Coupling patches in chtMultiRegionSimpleFoam
  #1
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
Hello to everyone!

I am running a case with chtMultiRegionSimpleFoam in which i have 4 different regions: 3 are solid and 1 is fluid.
I've created a mesh for each region separately - each region has its own polyMesh - and generated the meshes by means of blockMesh -region.

I've assigned a compressible::turbulentHeatFluxTemperature boundary condition on the external wall of a solid region - which is a boundary patch - and now i am wandering what should i assign to the internal wall of the same region and to the corresponding patch of the fluid region (the 2 patches that sould be coupled).
I see that i cannot use compressible::turbulentTemperatureCoupledBaffleMix ed since it requires mapping - i went through the planeWall2D tutorial, but as i said i generated 4 different meshes instead of mapping one.

What should i assign to the fluid/solid patches in the 0/T file?

Thanks in advance!
Nkl is offline   Reply With Quote

Old   May 31, 2016, 05:59
Default
  #2
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
No one can help?
Nkl is offline   Reply With Quote

Old   May 31, 2016, 09:06
Default
  #3
New Member
 
flanel
Join Date: Apr 2016
Posts: 8
Rep Power: 2
flanel1988 is on a distinguished road
Hey! First of all: What OF-Version do you use? I had similar problems in the past, but then I detected gmsh and I created one big mesh with all regions. I assigned all relevant patches to physical surfaces; except for the boundary patches. If you assign physical volumes, in OF with
Code:
splitMeshRegions -cellZones -overwrite
the program detects the boundaries by itself and adds patches like solid1_to_solid2 or something like that.
flanel1988 is offline   Reply With Quote

Old   May 31, 2016, 09:11
Default
  #4
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
Hi! I use the 3.0.1 version.
I know there is that possibility, but since i already modelled the different regions i wanted to figure out if there is a possibility of coupling the patches in another way.
Nkl is offline   Reply With Quote

Old   May 31, 2016, 10:43
Default
  #5
New Member
 
flanel
Join Date: Apr 2016
Posts: 8
Rep Power: 2
flanel1988 is on a distinguished road
But i do not understand, why you cannot use
Code:
compressible::turbulentTemperatureCoupledBaffleMix  ed
flanel1988 is offline   Reply With Quote

Old   May 31, 2016, 10:48
Default
  #6
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
I've tried to apply that patch to both the solid and fluid region as in the planeWall2D case, but i receive the following error:

Code:
--> FOAM FATAL ERROR: 

    patch type 'wall' not type 'mappedPatchBase'
Nkl is offline   Reply With Quote

Old   May 31, 2016, 11:09
Default
  #7
Senior Member
 
Join Date: Aug 2013
Posts: 227
Rep Power: 6
Antimony is on a distinguished road
Hi,

This error means that in the boundary file under constant/polyMesh, the highlighted patch has been specified as 'wall', while the compressible::turbulentTemperatureBaffleMixed is only available (again from the error message) if the type is 'mappedPatchBase'.

So change the type to 'mappedPatchBase' in the boundary file and at the very least, this error message will be removed.

Hope this helps.

Cheers,
Antimony
Antimony is offline   Reply With Quote

Old   May 31, 2016, 11:25
Default
  #8
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
Hello and thanks for the suggestion. Unfortunately it is the first thing i did but then i receive the following error:

Code:
--> FOAM FATAL ERROR: 

    patch type 'genericPatch' not type 'mappedPatchBase'
    for patch walls of field T in file "/home/nikola/OpenFOAM/nikola-3.0.1/PhD/receiverMultiRegion4/0/moltenSalt/T"
I supposed that i cannot use compressible::turbulentTemperatureCoupledBaffleMix ed when different regions have a separate mesh. Any suggestions about this error?
Nkl is offline   Reply With Quote

Old   June 1, 2016, 03:30
Default
  #9
New Member
 
flanel
Join Date: Apr 2016
Posts: 8
Rep Power: 2
flanel1988 is on a distinguished road
Do you have different Meshes in your constant/ folder? So chance the "mapped" in the constant/meshXX/boundary to "mappedWall". This has to be done for all meshes involved!
flanel1988 is offline   Reply With Quote

Old   June 8, 2016, 06:48
Default
  #10
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
Sorry for the late answer.

I tried to change to mappedWall in the various constant/regionX/polyMesh/boundary files, but now I receive the following error:

Code:
--> FOAM FATAL IO ERROR: 
keyword sampleMode is undefined in dictionary ".walls"

file: .walls from line 34 to line 37.
Should I map the fields using the mapFields utility?
Nkl is offline   Reply With Quote

Old   June 21, 2016, 11:42
Default
  #11
Nkl
Member
 
Nikola
Join Date: Sep 2013
Location: Madrid, Spain
Posts: 60
Rep Power: 5
Nkl is on a distinguished road
Some one can help please?
Nkl is offline   Reply With Quote

Old   July 12, 2016, 03:50
Default Same issue
  #12
New Member
 
Sing
Join Date: Jan 2016
Posts: 24
Rep Power: 2
Struggle_Achieve is on a distinguished road
Hello Nikola,
I also created a very complex geometry of a ladle which is used in Steel operations.
I already made different regions using blockMesh. Then I saw the plane2D wall case example for chtMultiRegionSimpleFoam. Then I tried to modify my mesh files so the format matches with the example. But when I run this case I too get the same error:

patch type 'genericPatch' not type 'mappedPatchBase'

in the T file for the mappedWall zone1_to_zone2. I used

type compressible::turbulentTemperatureCoupledBaffleMix ed;
Tnbr T;
kappa fluidThermo;
kappaName none;
value uniform 1873;

for the same.

I am clueless. One possible solution I can think is to recreate the whole geometry using snappyhex and let splitMeshRegions -cellZones -owerwrite define all the boundaries between the different regions. ie (zone0_to_zone1, etc)

Any help would be greatly appreciated!

Thanks and regards,
Singh.
Struggle_Achieve is offline   Reply With Quote

Old   July 15, 2016, 14:47
Default
  #13
Member
 
Join Date: Sep 2013
Posts: 88
Rep Power: 5
Bloerb is on a distinguished road
The answer has already been given. Change your patch type in all constant/meshXX/boundary files from wall to mappedWall.

As for Nkl issue. Here is an example from the tutorials:

Code:
bottomAir_to_leftSolid
{
    type            mappedWall;
    nFaces          130;
    startFace       4680;
    sampleMode      nearestPatchFace;
    sampleRegion    leftSolid;
    samplePatch     leftSolid_to_bottomAir;
}
You have to set this accordingly. The sample region is the neighbour region and the samplePatch the neighboring patch to this one. You need to add these lines since you meshed with different meshes instead of splitting one mesh into different domains. The splitmeshregions command automatically adds these lines. For many industrial applications meshing your domains separately is of course more convenient.
Nkl and Struggle_Achieve like this.
Bloerb is offline   Reply With Quote

Old   July 19, 2016, 02:24
Default Problem still persists
  #14
New Member
 
Sing
Join Date: Jan 2016
Posts: 24
Rep Power: 2
Struggle_Achieve is on a distinguished road
Quote:
Originally Posted by Bloerb View Post
The answer has already been given. Change your patch type in all constant/meshXX/boundary files from wall to mappedWall.

As for Nkl issue. Here is an example from the tutorials:

Code:
bottomAir_to_leftSolid
{
    type            mappedWall;
    nFaces          130;
    startFace       4680;
    sampleMode      nearestPatchFace;
    sampleRegion    leftSolid;
    samplePatch     leftSolid_to_bottomAir;
}
You have to set this accordingly. The sample region is the neighbour region and the samplePatch the neighboring patch to this one. You need to add these lines since you meshed with different meshes instead of splitting one mesh into different domains. The splitmeshregions command automatically adds these lines. For many industrial applications meshing your domains separately is of course more convenient.
Hello Bloerb,
First of all my gratitude for your answer.
Yes I have already modified the wall type to mappedWall; I have tried a number of things here but still same error appears.

I have used a format like this for all the boundaries:
Code:
domain1_to_domain0
    {
        type            mappedwall;
        inGroups        1(wall);
        nFaces          4000;
        startFace       236000;
    sampleMode      nearestPatchFace;
        sampleRegion    domain0;
        samplePatch     domain0_to_domain1;
    }
I am certainly new to openFOAM and I guess I must be wrong somewhere.
I would be very grateful if you may please point that out.

I have also posted the whole problem, it might be useful to understand the whole case.
Please take a look:
chtMultiRegionSimpleFoam: Confusion in geometry creation using blockMesh

My deepest thanks and regards,
Prateek Singh.
Struggle_Achieve is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Foam::error::PrintStack almir OpenFOAM Running, Solving & CFD 66 November 23, 2016 15:42
Possible bug with stitchMesh and cyclics in OpenFoam Jack001 OpenFOAM Pre-Processing 0 May 21, 2016 08:00
Problems setting up case for running with chtMultiRegionFoam (mesh is from Salome) esujby OpenFOAM Pre-Processing 29 January 31, 2016 14:09
Merging edge patches Yosmcer OpenFOAM Native Meshers: blockMesh 11 November 16, 2014 15:51
groovyBC for coupling of patches deniggo OpenFOAM Running, Solving & CFD 20 October 2, 2014 18:04


All times are GMT -4. The time now is 04:09.