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

[blockMesh] mergePatchPairs with blockMesh

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

Like Tree12Likes
  • 1 Post By Ivanet
  • 9 Post By aeroGeek
  • 1 Post By fakekarma
  • 1 Post By ziemowitzima

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 7, 2011, 13:23
Default mergePatchPairs with blockMesh
  #1
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 13
Ivanet is on a distinguished road
Dear Foamers,
I have done a mesh with blockMesh consisting of 6 blocks. Now I want to merge all the blocks and I am using for it mergePatchPairs. It works for some patches but not for all of them. I have attached my blockMeshDict so that you can check it.
Any idea or suggestion will be highly appreciated.
Thanks a lot in advance
Ivan
Attached Files
File Type: txt blockMeshDict.txt (4.5 KB, 1180 views)
ordinary likes this.

Last edited by Ivanet; July 8, 2011 at 02:00.
Ivanet is offline   Reply With Quote

Old   July 8, 2011, 11:35
Default Problem solved
  #2
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 13
Ivanet is on a distinguished road
I have just solved the problem using face matching instead of face merging!
I guess it must work also with face merging, but I am happy so far with the mentioned solution.
Many greetings
Ivan
Ivanet is offline   Reply With Quote

Old   November 24, 2011, 23:51
Smile mergePatchPairs with blockMesh
  #3
Member
 
张德胜
Join Date: Oct 2011
Posts: 71
Rep Power: 12
hei@ge is on a distinguished road
can you tell me how to edit mergepatchpairs?My case is cut the windfarm into two blocks.Thaks a lots.
hei@ge is offline   Reply With Quote

Old   November 25, 2011, 03:05
Default
  #4
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 13
Ivanet is on a distinguished road
Hi hei@ge
at the end of your blockMeshDict there is a mergePatchPairs entry. You only have to write there which patch pairs you want to merge.
If you have 2 different meshes that you want to merge, you can use the utility mergeMeshes for that.
I hope this helps...
Ivan
Ivanet is offline   Reply With Quote

Old   November 26, 2011, 21:34
Smile
  #5
Member
 
张德胜
Join Date: Oct 2011
Posts: 71
Rep Power: 12
hei@ge is on a distinguished road
Hi,thread,thank you for your reply.but i can not solve my problem.please see my blockmeshdict for me.
vertices
(
( 581321 4.78537e+06 930)
( 582290 4.78537e+06 930)
( 582290 4.78624e+06 930)
( 581321 4.78624e+06 930)
( 581321 4.78537e+06 1030)
( 582290 4.78537e+06 1030)
( 582290 4.78624e+06 1030)
( 581321 4.78624e+06 1030)
( 581321 4.78537e+06 2000)
( 582290 4.78537e+06 2000)
( 582290 4.78624e+06 2000)
( 581321 4.78624e+06 2000)

);

blocks
(
hex (0 1 2 3 4 5 6 7) (30 30 25) simpleGrading (1 1 1)
hex (4 5 6 7 8 9 10 11) (30 30 30) simpleGrading (1 1 1)
);

edges
(
);

patches
(
patch outlet
(
(2 6 5 1)
(6 10 9 5)

)
patch sides
(
(1 5 4 0)
(5 9 8 4)
(3 7 6 2)
(7 11 10 6)
)
patch inlet
(
(0 4 7 3)
(4 8 11 7)
)
wall ground
(
(0 3 2 1)
)
patch top
(
(8 9 10 11)
)
patch interface1
(
(4 5 6 7)
)
patch interface2
(
(4 7 6 5)
)
);

mergePatchPairs
(
(<interface1> <interface2>)
);
my model is a Hex,i turn it into 2 blocks in the near bottom.
hei@ge is offline   Reply With Quote

Old   December 20, 2011, 00:22
Default
  #6
New Member
 
Jacob Crabill
Join Date: Nov 2011
Posts: 1
Rep Power: 0
aeroGeek is on a distinguished road
Hi hei@ge,

You've probably figured it out by now, but just in case (and because unanswered threads bug me), here's your answer:

Internal faces between blocks (which won't be receiving boundary conditions) don't get assigned as patches - they are simply ignored, and OpenFoam will recognize them as simply being an interface between two blocks.

The exception is when the two blocks use separate vertices to define overlapping faces - say, if you were to copy vertices 4, 5, 6, & 7 to vertices 12, 13, 14, & 15. THEN you would use mergePatchPairs to merge the faces (4 5 6 7) and (15 14 13 12)

Hope this helps someone!

Regards,
Jacob
guin, nasa55, curiosity and 6 others like this.
aeroGeek is offline   Reply With Quote

Old   January 16, 2012, 09:57
Default
  #7
New Member
 
Elia Daniele
Join Date: Mar 2010
Location: Oldenburg
Posts: 21
Rep Power: 14
fakekarma is on a distinguished road
@ Hei@ge,

I don't if it is just a mistake in copy and paste but you should in matchPatchPairs write

(interface1 interface2)

instead of

(<interface1> <interface2>)

Cheers,

Elia
sourav90 likes this.
fakekarma is offline   Reply With Quote

Old   November 19, 2015, 11:22
Default
  #8
Senior Member
 
Mieszko Młody
Join Date: Mar 2009
Location: POLAND, USA
Posts: 144
Rep Power: 15
ziemowitzima is on a distinguished road
Hi,
Do you know how to specify BC at the interface patches ?
thx
ZMM
jaimeff likes this.
ziemowitzima is offline   Reply With Quote

Old   June 27, 2017, 12:47
Default
  #9
New Member
 
Join Date: Apr 2017
Location: Germany
Posts: 5
Rep Power: 7
marv91 is on a distinguished road
hey

in case I can't connect my blocks because they don't have the same vertices at their interface how should I proceed. As aeroGeek described I need to define two patches and merge them with mergePatchPairs. The problem is than that I need boundaries in the 0 directory for the two new internal patches.
Or are these two patches automatically formed to an internal face?

Thanks a lot!

Marvin
marv91 is offline   Reply With Quote

Old   January 17, 2018, 22:02
Default
  #10
Member
 
Join Date: Jan 2018
Location: Malaysia
Posts: 58
Rep Power: 6
jiahui_93 is on a distinguished road
Hi, I am a totally newbie in CFD. I am facing the problem that openfoam doesnt accept the block with internal faces. But i need that to build a hollow cavity within the center of a rectangular box. What should I do? i hope can get some advice and will be very grateful on that. thanks

Creating topology blocks
--> FOAM Warning :
From function Foam::vector Foam::cellModel::centre(const labelList&, const Foam::UList<Foam::Vector<double> >&) const
in file meshes/meshShapes/cellModel/cellModel.C at line 70
zero or negative pyramid volume: -10.12 for face 0
--> FOAM Warning :
From function Foam::vector Foam::cellModel::centre(const labelList&, const Foam::UList<Foam::Vector<double> >&) const
in file meshes/meshShapes/cellModel/cellModel.C at line 70
zero or negative pyramid volume: -10.12 for face 1
--> FOAM Warning :
From function Foam::vector Foam::cellModel::centre(const labelList&, const Foam::UList<Foam::Vector<double> >&) const
in file meshes/meshShapes/cellModel/cellModel.C at line 70
zero or negative pyramid volume: -23.76 for face 3
--> FOAM Warning :
From function Foam::vector Foam::cellModel::centre(const labelList&, const Foam::UList<Foam::Vector<double> >&) const
in file meshes/meshShapes/cellModel/cellModel.C at line 70
zero or negative pyramid volume: -10.12 for face 4
--> FOAM Warning :
From function Foam::vector Foam::cellModel::centre(const labelList&, const Foam::UList<Foam::Vector<double> >&) const
in file meshes/meshShapes/cellModel/cellModel.C at line 70
zero or negative pyramid volume: -10.12 for face 5


--> FOAM FATAL IO ERROR:
Block hex (37 38 46 45 53 54 62 61) (16 339 4) simpleGrading (1(1) 1(1) 1(1)) has inward-pointing faces
4(37 53 61 45) 4(38 46 62 54) 4(45 61 62 46) 4(37 45 46 38) 4(53 54 62 61)

file: /mnt/c/Users/User/OpenFOAM/jhTutorial/pimpleDyMfoam/elevator/system/blockMeshDict.blocks at line 91.

From function void Foam::blockDescriptor::check(const Foam::Istream&)
in file blockDescriptor/blockDescriptor.C at line 89.

FOAM exiting
jiahui_93 is offline   Reply With Quote

Old   February 23, 2018, 09:42
Default
  #11
Member
 
Anurag
Join Date: Aug 2014
Location: Germany
Posts: 57
Rep Power: 9
anuragm is on a distinguished road
Were you able to solve this problem? blockMesh does not like internal faces, but a cavity inside is not usually a problem because this is external to the mesh. If you post the geometry or blockMeshDict file, I can help you with it.

In any case, you can take a look at the createBaffles utility if you want internal walls.
anuragm is offline   Reply With Quote

Old   February 23, 2018, 10:27
Default
  #12
Member
 
Join Date: Jan 2018
Location: Malaysia
Posts: 58
Rep Power: 6
jiahui_93 is on a distinguished road
Quote:
Originally Posted by anuragm View Post
Were you able to solve this problem? blockMesh does not like internal faces, but a cavity inside is not usually a problem because this is external to the mesh. If you post the geometry or blockMeshDict file, I can help you with it.

In any case, you can take a look at the createBaffles utility if you want internal walls.
Thanks for your suggestion. I will try it now. Is it something like splitMeshRegions?

previously, by using setSet, I got my hollow box within the domain. But i faced another problem, the deleted cell zone left a hole there when it moved up. The mesh seems not replaced automatically.

I am trying the moving Cone topo method which is topo changer. As it seems limited, so i was trying to modify it to suit my case which has vertical translation motion.

thanks again for your help.
jiahui_93 is offline   Reply With Quote

Old   February 23, 2018, 10:53
Default
  #13
Member
 
Anurag
Join Date: Aug 2014
Location: Germany
Posts: 57
Rep Power: 9
anuragm is on a distinguished road
No, splitMeshRegions splits the mesh into different regions, which I achieve in my case through meticulous blocking and naming. createBaffles on the other hand is capable of generating internal walls using previously defined cell sets or regions. Here is an example image of my mesh with internal walls and cavity, note that I define internal walls explicitly in the blockMeshDict using duplicate vertices instead of using the createBaffles utility:

https://www.cfd-online.com/Forums/op...evolution.html

Again, it is difficult to say what exactly is the problem in your case without any details but it seems to me like you are trying to transform your mesh to create a cavity instead of deleting it. To me, this seems a little strange way to do things.
anuragm is offline   Reply With Quote

Old   February 23, 2018, 11:16
Default
  #14
Member
 
Join Date: Jan 2018
Location: Malaysia
Posts: 58
Rep Power: 6
jiahui_93 is on a distinguished road
Quote:
Originally Posted by anuragm View Post
No, splitMeshRegions splits the mesh into different regions, which I achieve in my case through meticulous blocking and naming. createBaffles on the other hand is capable of generating internal walls using previously defined cell sets or regions. Here is an example image of my mesh with internal walls and cavity, note that I define internal walls explicitly in the blockMeshDict using duplicate vertices instead of using the createBaffles utility:

https://www.cfd-online.com/Forums/op...evolution.html

Again, it is difficult to say what exactly is the problem in your case without any details but it seems to me like you are trying to transform your mesh to create a cavity instead of deleting it. To me, this seems a little strange way to do things.
Thanks for reply. Sry for not providing sufficient info. Here is my post with more details.
Linear motion of a solid inside a fluid

Actually i am trying to build a 3D hollow box moving in a rectangular tube (domain), and i aim to mesh the space btwn hollow box and rectangular tube to study the external airflow and pressure and turbulence parameters. This is my starting step to learn the simulation of aerodynamic outside a vehicles or body within a domain. Is it correct for me to delete the cells within the box to make it hollow? i am sry for my dummy questions. Thanks a lot
jiahui_93 is offline   Reply With Quote

Old   February 23, 2018, 14:23
Default
  #15
Member
 
Anurag
Join Date: Aug 2014
Location: Germany
Posts: 57
Rep Power: 9
anuragm is on a distinguished road
Quote:
Originally Posted by jiahui_93 View Post
Thanks for reply. Sry for not providing sufficient info. Here is my post with more details.
Linear motion of a solid inside a fluid

Actually i am trying to build a 3D hollow box moving in a rectangular tube (domain), and i aim to mesh the space btwn hollow box and rectangular tube to study the external airflow and pressure and turbulence parameters. This is my starting step to learn the simulation of aerodynamic outside a vehicles or body within a domain. Is it correct for me to delete the cells within the box to make it hollow? i am sry for my dummy questions. Thanks a lot
I read your post now, and I want to make it clear that I do not have extensive experience with moving meshes. I took the movingCone case and modified it a little to get something similar to what you want. But first, I would like to say a couple of things:

  1. In case you are only working with simple shapes like block or cylinder, blockMesh is a perfectly capable tool. However, it is very difficult to work with if you are working with a complex geometry (a car or motorbike, for example)
  2. In complex cases, snappyHexMesh is good but it has some problems with boundary layers. There is another open-source tool called cfMesh which supposedly gives better results as compared to snappyHexMesh
  3. In case you are working with blockMesh, then just be careful when defining blocks and faces. Keep in mind that you can assign a boundary condition to a block face and not to part of it (unless you make use of an additional utility).
Anyway, here is an example blockMeshDict that you can adapt for your case. I have made it based on the movingCone case so you can test this case with pimpleDymFoam (remember to change the boundary conditions from wedge to empty):
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

vertices
(
    (-7.5 0 0)     //0
    (-7 0 0)       //1
    (-3.5 0 0)     //2
    (0 0 0)        //3
    (-7.5 1.75 0)  //4
    (-7 1.75 0)    //5
    (-3.5 2 0)     //6
    (0 2 0)        //7
    (-7.5 2.5 0)   //8
    (-7 2.5 0)     //9
    (-3.5 2.5 0)   //10
    (0 2.5 0)      //11
    (-7.5 1.75 1)  //12
    (-7 1.75 1)    //13
    (-3.5 2 1)     //14
    (0 2 1)        //15
    (-7.5 2.5 1)   //16
    (-7 2.5 1)     //17
    (-3.5 2.5 1)   //18
    (0 2.5 1)      //19
    (-7.5 0 1)     //20
    (-7 0 1)       //21
    (-3.5 0 1)     //22
    (0 0 1)        //23
    (-7 0.75 0)    //24
    (-7 0.75 1)    //25
    (-3.5 0.75 0)  //26
    (-3.5 0.75 1)  //27
    (-7.5 0.75 0)  //28
    (-7.5 0.75 1)  //29
    (0 0.75 0)     //30
    (0 0.75 1)     //31
);

blocks
(
    hex (0 1 24 28 20 21 25 29) (15 20 1) simpleGrading (2 0.25 1)
    hex (28 24 5 4 29 25 13 12) (15 20 1) simpleGrading (2 0.25 1)
    hex (2 3 30 26 22 23 31 27) (20 20 1) simpleGrading (2 0.25 1)
    hex (26 30 7 6 27 31 15 14) (20 20 1) simpleGrading (2 0.25 1)
    hex (4 5 9 8 12 13 17 16) (15 20 1) simpleGrading (2 0.25 1)
    hex (5 6 10 9 13 14 18 17) (50 20 1) simpleGrading (2 0.25 1)
    hex (6 7 11 10 14 15 19 18) (20 20 1) simpleGrading (2 0.25 1)
    hex (1 2 26 24 21 22 27 25) (50 20 1) simpleGrading (2 0.25 1)
);

edges
(
);

boundary
(
    movingWall
    {
        type wall;
        faces
        (
            (24 5 13 25)
            (5 6 14 13)
            (26 6 14 27)
            (24 26 27 25)
        );
    }
    farFieldMoving
    {
        type patch;
        faces
        (
            (9 17 18 10)
            (1 21 22 2)
        );
    }
    fixedWall
    {
        type wall;
        faces
        (
            (3 30 31 23)
            (30 7 15 31)
            (7 11 19 15)
        );
    }
    axis
    {
        type empty;
        faces
        (
            //(0 1 1 0)
            //(2 3 3 2)
        );
    }
    left
    {
        type patch;
        faces
        (
            (0 20 29 28)
            (28 29 12 4)
            (4 12 16 8)
        );
    }
    farField
    {
        type patch;
        faces
        (
            (8 16 17 9)
            (0 20 21 1)
            (10 18 19 11)
            (2 22 23 3)
        );
    }
    back
    {
        type empty;
        faces
        (
            (0 28 24 1)
            (28 4 5 24)
            (2 26 30 3)
            (26 6 7 30)
            (4 8 9 5)
            (5 9 10 6)
            (6 10 11 7)
        );
    }
    front
    {
        type empty;
        faces
        (
            (20 21 25 29)
            (29 25 13 12)
            (22 23 31 27)
            (27 31 15 14)
            (12 13 17 16)
            (13 14 18 17)
            (14 15 19 18)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //
anuragm is offline   Reply With Quote

Old   February 23, 2018, 20:21
Default
  #16
Member
 
Join Date: Jan 2018
Location: Malaysia
Posts: 58
Rep Power: 6
jiahui_93 is on a distinguished road
Quote:
Originally Posted by anuragm View Post
I read your post now, and I want to make it clear that I do not have extensive experience with moving meshes. I took the movingCone case and modified it a little to get something similar to what you want. But first, I would like to say a couple of things:

  1. In case you are only working with simple shapes like block or cylinder, blockMesh is a perfectly capable tool. However, it is very difficult to work with if you are working with a complex geometry (a car or motorbike, for example)
  2. In complex cases, snappyHexMesh is good but it has some problems with boundary layers. There is another open-source tool called cfMesh which supposedly gives better results as compared to snappyHexMesh
  3. In case you are working with blockMesh, then just be careful when defining blocks and faces. Keep in mind that you can assign a boundary condition to a block face and not to part of it (unless you make use of an additional utility).
Anyway, here is an example blockMeshDict that you can adapt for your case. I have made it based on the movingCone case so you can test this case with pimpleDymFoam (remember to change the boundary conditions from wedge to empty):
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

vertices
(
    (-7.5 0 0)     //0
    (-7 0 0)       //1
    (-3.5 0 0)     //2
    (0 0 0)        //3
    (-7.5 1.75 0)  //4
    (-7 1.75 0)    //5
    (-3.5 2 0)     //6
    (0 2 0)        //7
    (-7.5 2.5 0)   //8
    (-7 2.5 0)     //9
    (-3.5 2.5 0)   //10
    (0 2.5 0)      //11
    (-7.5 1.75 1)  //12
    (-7 1.75 1)    //13
    (-3.5 2 1)     //14
    (0 2 1)        //15
    (-7.5 2.5 1)   //16
    (-7 2.5 1)     //17
    (-3.5 2.5 1)   //18
    (0 2.5 1)      //19
    (-7.5 0 1)     //20
    (-7 0 1)       //21
    (-3.5 0 1)     //22
    (0 0 1)        //23
    (-7 0.75 0)    //24
    (-7 0.75 1)    //25
    (-3.5 0.75 0)  //26
    (-3.5 0.75 1)  //27
    (-7.5 0.75 0)  //28
    (-7.5 0.75 1)  //29
    (0 0.75 0)     //30
    (0 0.75 1)     //31
);

blocks
(
    hex (0 1 24 28 20 21 25 29) (15 20 1) simpleGrading (2 0.25 1)
    hex (28 24 5 4 29 25 13 12) (15 20 1) simpleGrading (2 0.25 1)
    hex (2 3 30 26 22 23 31 27) (20 20 1) simpleGrading (2 0.25 1)
    hex (26 30 7 6 27 31 15 14) (20 20 1) simpleGrading (2 0.25 1)
    hex (4 5 9 8 12 13 17 16) (15 20 1) simpleGrading (2 0.25 1)
    hex (5 6 10 9 13 14 18 17) (50 20 1) simpleGrading (2 0.25 1)
    hex (6 7 11 10 14 15 19 18) (20 20 1) simpleGrading (2 0.25 1)
    hex (1 2 26 24 21 22 27 25) (50 20 1) simpleGrading (2 0.25 1)
);

edges
(
);

boundary
(
    movingWall
    {
        type wall;
        faces
        (
            (24 5 13 25)
            (5 6 14 13)
            (26 6 14 27)
            (24 26 27 25)
        );
    }
    farFieldMoving
    {
        type patch;
        faces
        (
            (9 17 18 10)
            (1 21 22 2)
        );
    }
    fixedWall
    {
        type wall;
        faces
        (
            (3 30 31 23)
            (30 7 15 31)
            (7 11 19 15)
        );
    }
    axis
    {
        type empty;
        faces
        (
            //(0 1 1 0)
            //(2 3 3 2)
        );
    }
    left
    {
        type patch;
        faces
        (
            (0 20 29 28)
            (28 29 12 4)
            (4 12 16 8)
        );
    }
    farField
    {
        type patch;
        faces
        (
            (8 16 17 9)
            (0 20 21 1)
            (10 18 19 11)
            (2 22 23 3)
        );
    }
    back
    {
        type empty;
        faces
        (
            (0 28 24 1)
            (28 4 5 24)
            (2 26 30 3)
            (26 6 7 30)
            (4 8 9 5)
            (5 9 10 6)
            (6 10 11 7)
        );
    }
    front
    {
        type empty;
        faces
        (
            (20 21 25 29)
            (29 25 13 12)
            (22 23 31 27)
            (27 31 15 14)
            (12 13 17 16)
            (13 14 18 17)
            (14 15 19 18)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //
I had tried snappyHexMesh, Salome, gmesh, etc.. and agree that blockMesh is the best for my simple geometry.
But i still cnt figure out if there's the function for me to choose where i wan to mesh, something like locationInMesh in snappyHexM. So that i can choose only to mesh the space between my hollow box and the rectangular domain. And most importantly, when the hollow car moved up, its original location won't left a hole there.

HTML Code:
Keep in mind that you can assign a boundary condition to a block face and not to part of it (unless you make use of an additional utility).
Yes, I use setSet, toposet and changeDictionary.

HTML Code:
 here is an example blockMeshDict that you can adapt for your case. I have made it based on the movingCone case so you can test this case with pimpleDymFoam (remember to change the boundary conditions from wedge to empty)
I tried it before. It is very useful for me to understand pimpleDyM. Thanks for suggestion

Thanks again for your help. I very appreciate your help

Thanks
jiahui_93 is offline   Reply With Quote

Old   May 4, 2021, 06:48
Default
  #17
Member
 
Bushra Rasheed
Join Date: Dec 2020
Posts: 97
Rep Power: 3
B_R_Khan is on a distinguished road
Does anyone know how to give boundary condition to internal faces that you have merged through merge patch pairs? I had different size blocks and merged them through mergePatchPairs. Now it's giving me error that interface boundary condition is not defined in 0 folder.
B_R_Khan is offline   Reply With Quote

Old   May 4, 2021, 10:32
Default
  #18
jmt
Member
 
Julian
Join Date: Sep 2019
Posts: 31
Rep Power: 4
jmt is on a distinguished road
Quote:
Originally Posted by B_R_Khan View Post
Does anyone know how to give boundary condition to internal faces that you have merged through merge patch pairs? I had different size blocks and merged them through mergePatchPairs. Now it's giving me error that interface boundary condition is not defined in 0 folder.
I can speak for multi-region, conjugate heat transfer simulations in which the internal face is a fluid-solid interface. In this case, there is a mechanism in OpenFOAM for this type of internal face which is shared by two regions.

If you are not using multi-region CHT, I think you might need to create a baffle out of the internal face using createBafflesDict or something similar.

If you are using CHT, in your blockMeshDict, specify the two interface boundaries as type `patch` in the `boundary` group as shown below.

Code:
...
boundary
(
...
    bottomWall
    {
        type patch; 
        faces
        (
            (12 13 15 14)
        );
    }
...
    solidInterface
    {
        type patch;
        faces
        (
            (16 18 19 17)
        );
    }
...
);

mergePatchPairs
(
    (bottomWall solidInterface)
);
Then when you split the blockMesh into multiple regions, OpenFOAM will automatically rename the interface boundary based on the fluid and solid region names. You can then specify boundary conditions for these on a per-region basis.
jmt is offline   Reply With Quote

Reply

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
[blockMesh] blockMesh | MergePatchPairs | snappyHexMesh |Different number of cells in divisions pythag0ra5 OpenFOAM Meshing & Mesh Conversion 1 September 19, 2020 14:38
[mesh manipulation] mergePatchPairs after running blockMesh ashishmagar600 OpenFOAM Meshing & Mesh Conversion 2 March 8, 2019 04:15
[blockMesh] mergePatchPairs reducing a face to less than 3 points aow OpenFOAM Meshing & Mesh Conversion 2 June 1, 2018 17:37
[blockMesh] Error running blockMesh with mergePatchPairs on OF2.4.0 deepbandivadekar OpenFOAM Meshing & Mesh Conversion 1 November 25, 2017 14:50
[blockMesh] BlockMesh documentation User Guide clearance of mergePatchPairs proposals benru OpenFOAM Meshing & Mesh Conversion 0 June 9, 2008 02:22


All times are GMT -4. The time now is 19:07.