CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Other] splitMeshRegions does not create interface patch between regions

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

Like Tree2Likes
  • 1 Post By fsan
  • 1 Post By mwaqas

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 16, 2019, 10:34
Default splitMeshRegions does not create interface patch between regions
  #1
New Member
 
Join Date: May 2019
Location: Paris, France
Posts: 7
Rep Power: 3
fsan is on a distinguished road
Hello,

Here's my problem, I'm trying to do a simulation with chtMultiRegionFoam to check the thermal evolution in the surface of a pipe.
The geometry contain a fluid region with relatitive cold methan, around it a solid region for the pipe and arounnd the pipe a fluid region for hot air.

The mesh was created on the Ansys Workbench (spaceClaim and fluent meshing) and was import to openFoam with the "fluent3DMeshToFoam" command.

Then when I try to split the mesh into different region by typing
in the terminal:

Code:
splitMeshRegions -cellZones -overwrite
The three different region are well recognize but no interface patch are created (like "fluidToSolid" and "solidToofluid") as you can see in the output given in the terminal:

Code:
Create time

Create mesh for time = 0

Creating single patch per inter-region interface.

Trying to match regions to existing cell zones.


Number of regions:3

Writing region per cell file (for manual decomposition) to "/media/ubuntu/DATAS/Run/Coude/Coudemsh3/constant/cellToRegion"

Writing region per cell as volScalarField to "/media/ubuntu/DATAS/Run/Coude/Coudemsh3/0/cellToRegion"

Region	Cells
------	-----
0	6867
1	37308
2	142547

Region	Zone	Name
------	----	----
0	0	fff-solid-pipe
1	1	fff-fluid-pipe
2	2	fff-fluid-air

Sizes of interfaces between regions:

Interface	Region	Region	Faces
---------	------	------	-----

Reading geometric fields

Reading volScalarField cellToRegion


Adding patches


Adding patches


Region 0
-------- 
Creating mesh for region 0 fff-solid-pipe
Testing:"/media/ubuntu/DATAS/Run/Coude/Coudemsh3/system/fff-solid-pipe/fvSchemes"
Mapping fields
Mapping field cellToRegion
Deleting empty patches
Writing new mesh
Writing addressing to base mesh
Writing map pointRegionAddressing from region0 points back to base mesh.
Writing map faceRegionAddressing from region0 faces back to base mesh.
Writing map cellRegionAddressing from region0 cells back to base mesh.
Writing map boundaryRegionAddressing from region0 boundary back to base mesh.

Region 1
-------- 
Creating mesh for region 1 fff-fluid-pipe
Testing:"/media/ubuntu/DATAS/Run/Coude/Coudemsh3/system/fff-fluid-pipe/fvSchemes"
Mapping fields
Mapping field cellToRegion
Deleting empty patches
Writing new mesh
Writing addressing to base mesh
Writing map pointRegionAddressing from region1 points back to base mesh.
Writing map faceRegionAddressing from region1 faces back to base mesh.
Writing map cellRegionAddressing from region1 cells back to base mesh.
Writing map boundaryRegionAddressing from region1 boundary back to base mesh.

Region 2
-------- 
Creating mesh for region 2 fff-fluid-air
Testing:"/media/ubuntu/DATAS/Run/Coude/Coudemsh3/system/fff-fluid-air/fvSchemes"
Mapping fields
Mapping field cellToRegion
Deleting empty patches
Writing new mesh
Writing addressing to base mesh
Writing map pointRegionAddressing from region2 points back to base mesh.
Writing map faceRegionAddressing from region2 faces back to base mesh.
Writing map cellRegionAddressing from region2 cells back to base mesh.
Writing map boundaryRegionAddressing from region2 boundary back to base mesh.
End
The problem is that I can't use the "compressible::TurbulentTemperatureCoupledBaffleMi xed" or the "compressible::TurbulentTemperatureRadCoupledMixed " boundary condition, this mean that I have one same patch contained in two different region.

Even if I try to launch my simulation, I have the folowing fatal error: " not type 'mappedPatchBase' ".
I tried to replace in the polymesh the 'wall' by 'mappedWall' but it's still not working.

I would like to ask if some of you know how I can create those interface patch? If there is a command that can help to separate the patch shared by two region in two or any other clue.

Thank you
fsan is offline   Reply With Quote

Old   August 22, 2019, 04:54
Default
  #2
Senior Member
 
Muhammad Waqas
Join Date: Jul 2014
Location: Germany
Posts: 123
Rep Power: 8
mwaqas is on a distinguished road
Send a message via Skype™ to mwaqas
Hello Fsan,


This problem occurs when you have non-conformal mesh in Ansys. Make a conformal mesh in Ansys and you will get a mappedWall.


Regards
mwaqas is offline   Reply With Quote

Old   August 23, 2019, 05:20
Default
  #3
New Member
 
Join Date: May 2019
Location: Paris, France
Posts: 7
Rep Power: 3
fsan is on a distinguished road
Hello Muhammad,
Thank you for you reply, I did check if the mesh was non-conformal or not but it look like a conformal mesh for me.

I upload some screen of the different region separation so you can all tell me what you think about it. The green and red region are fluid while the white region is a solid.
I can also upload the msh file if needed.

Thank you
Attached Images
File Type: png outlet_gas&air.png (70.5 KB, 16 views)
File Type: png inlet_gas.png (101.5 KB, 17 views)
fsan is offline   Reply With Quote

Old   August 23, 2019, 05:37
Default
  #4
Senior Member
 
Muhammad Waqas
Join Date: Jul 2014
Location: Germany
Posts: 123
Rep Power: 8
mwaqas is on a distinguished road
Send a message via Skype™ to mwaqas
The mesh is conformal.

Then, there might be a problem with your BC.



Can you please upload your BC file (0/P or U, wherever is the problem) as well as your polyMesh/boundary file of problematic regions.


Probably, you are not giving correct BC.


Regards
mwaqas is offline   Reply With Quote

Old   August 23, 2019, 08:39
Default
  #5
New Member
 
Join Date: May 2019
Location: Paris, France
Posts: 7
Rep Power: 3
fsan is on a distinguished road
Alright I upload the boundary files for each of the region (fluidAir, fluidNG and solid). And I'll post just below the boundary condition for U:

For the fluid air region:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0/fff-fluid-air";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 1 -1 0 0 0 0 ];

internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet-air
    {
        type            fixedValue;
        value           uniform (-0.15 0 0);
    }
    outlet-air
    {
        type            pressureInletOutletVelocity;
        value           $internalField;
    }
    wall-fff-fluid-air
    {
        type            noSlip;
    }

    wall-fff-fluid-air-fff-solid-pipe
    {
        type            noSlip;
    }

}

// ************************************************************************* //
And for the fluid Natural Gas region:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0/fff-fluid-pipe";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 1 -1 0 0 0 0 ];

internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet-gas
    {
        type            fixedValue;
        value           uniform (0 0.15 0);
    }
    outlet-gas
    {
        type            pressureInletOutletVelocity;
        value           $internalField;
    }
    wall-fff-fluid-pipe-fff-solid-pipe
    {
        type            noSlip;
    }
}

The main problem I think is during the generation of the interface patch (solid_to_fluid and fluid_to_liquid) when i execute:

Code:
splitMeshRegions -cellZones -overwrite
As I don't get the mappedWall boundary condition for my T field where I need to use it, I can't use it afterward.
And I don't know what other BC I could use for the T fields instead of the coupled BC.

Thank you for your help.
Attached Files
File Type: txt boundary(fluidAir).txt (1.3 KB, 6 views)
File Type: txt boundary(fluidNG).txt (1.1 KB, 2 views)
File Type: txt boundary(solid).txt (1.2 KB, 11 views)
fsan is offline   Reply With Quote

Old   August 23, 2019, 10:09
Default
  #6
Senior Member
 
Muhammad Waqas
Join Date: Jul 2014
Location: Germany
Posts: 123
Rep Power: 8
mwaqas is on a distinguished road
Send a message via Skype™ to mwaqas
You are not getting any coupled wall during mesh conversion. I had this problem once when I had exported Ansys mesh to Openfoam. It was due to the non-conformal mesh. As I wasn't having any coupled wall in Ansys meshing.
It is looking like to me that you don't have coupled wall in Ansys meshing (because if there would be a coupled wall, you would have automatically got in OpenFOAM ).
You can do these things:


1) Check in fluent if your interface type is coupled or not. I suspect, it wont be.
2) Create coupled interface and then export to OpenFOAM.


Regards
fsan likes this.
mwaqas is offline   Reply With Quote

Old   August 23, 2019, 10:35
Default
  #7
New Member
 
Join Date: May 2019
Location: Paris, France
Posts: 7
Rep Power: 3
fsan is on a distinguished road
Thank you again for your reply.

I can't have acces to fluent now but when I will, I'll tell here if it would work or not.

Regards
fsan is offline   Reply With Quote

Old   August 27, 2019, 11:18
Default
  #8
New Member
 
Join Date: May 2019
Location: Paris, France
Posts: 7
Rep Power: 3
fsan is on a distinguished road
Hi Muhammad,

Naming each side of the interface in fluent did make the job, openFoam now recognize my interface and patch them. Thank you for the help.

Unfortunately, right now my simulation is not working as I wish, certaintly because of the BC, the scheme or the thermophysical model I don't know yet.

Regards
fsan is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, mappedpatchbase error, splitmeshregions

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 18:57
createPatch Segmentation Fault (CORE DUMPED) sam.ho OpenFOAM Pre-Processing 2 April 21, 2014 02:01
Radiation interface hinca CFX 15 January 26, 2014 17:11
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 02:34
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55


All times are GMT -4. The time now is 08:55.