[Mahdi2010]

Hi All

I am trying to create a thin wall film mesh by extruding the intersection of 2 zones. I mean I have a simple mesh split into 2 zones (one fluid and one solid zone) using " splitMeshRegions". The intersection of these two zones is of course an internal patch which is automatically considered in blockMesh. (actually not possible to specify any BC in blockMeshDict because it is an internal patch)

Now I want to extrude this internal patch (which should be considered as a wall over the solid zone) into a thin film region. According to the tutorial cases I need a "faceSet" and "faceSetZones" over this patch to be able to extrude from. But I cannot create this faceSet using topoSet, because this is an internal patch and cannot be named, while I would need a patch name as the "reference" in the topoSet file.

Does anybody have experience in creating a faceSetZone over the intersection of two zones (i.e. an internal patch)?

[Mojtaba.a]

Originally Posted by Mahdi2010

Hi All

I am trying to create a thin wall film mesh by extruding the intersection of 2 zones. I mean I have a simple mesh split into 2 zones (one fluid and one solid zone) using " splitMeshRegions". The intersection of these two zones is of course an internal patch which is automatically considered in blockMesh. (actually not possible to specify any BC in blockMeshDict because it is an internal patch)

Now I want to extrude this internal patch (which should be considered as a wall over the solid zone) into a thin film region. According to the tutorial cases I need a "faceSet" and "faceSetZones" over this patch to be able to extrude from. But I cannot create this faceSet using topoSet, because this is an internal patch and cannot be named, while I would need a patch name as the "reference" in the topoSet file.

Does anybody have experience in creating a faceSetZone over the intersection of two zones (i.e. an internal patch)?

Hi,
How would you extrude a faceSet, when you already have some cells in your solid or fluid regions?

[Mahdi2010]

Originally Posted by Mojtaba.a

Hi,
How would you extrude a faceSet, when you already have some cells in your solid or fluid regions?

Actually I am trying to extrude a faceSetZone into a new "mesh region" which is a film. So if I had two regions (i.e fluid and solid), this would be the third region. But in contrast to fluid and solid regions, this new region is a film region (surface mesh). So at the end there will be three regions:
1) solid
2) fluid
3) wall film

This will be done using "extrudeToRegionMesh" .

[Mojtaba.a]

Originally Posted by Mahdi2010

Actually I am trying to extrude a faceSetZone into a new "mesh region" which is a film. So if I had two regions (i.e fluid and solid), this would be the third region. But in contrast to fluid and solid regions, this new region is a film region (surface mesh). So at the end there will be three regions:
1) solid
2) fluid
3) wall film

This will be done using "extrudeToRegionMesh" .

So there is a gap between the regions you are calling fluid and solid?

[Mahdi2010]

Originally Posted by Mojtaba.a

So there is a gap between the regions you are calling fluid and solid?

Actually I wouldn't call it a gap because there is no gap between solid and fluid zones. The solid and fluid are "cellSetZone"s while this film surface mesh is a "faceSetZone". This is similar to the strategy used in tutorial cases of solvers like "reactingParcelFilmFoam". If for instance you want to run a tutorial case of such solver (which solves 2D film model within the flow), you would see in the "Allrun" file that first a wallFilm faceSetZone is created using "topoSet" over one of the walls. and then "extrudeToRegionMesh" is used to extrude that wall film faceSetZone into a surface (2D) mesh. briefly as follows:

1- defining wallFilmFaces to create a faceSet.(called wallFilmFaces)
2- changing this faceSet to a faceSetZone (called wallFilmRegion)
3- extruding the wallFilm surface mesh from the faceSetZone created in step No. 2.

I should mention that the first two steps are done by "topoSet" (or wallFilm.topoSet) and the last one is done by "extrudeToRegionMesh"

So you can see this is not a gap, this is only a one single layer surface mesh.
What I am trying to do is exactly the same procedure except that before step 1, I would do another step in which I split the mesh into solid and fluid zones. then I am trying to do the above-mentioned steps on the inter-section patch of the fluid and solid.

[Mojtaba.a]

Originally Posted by Mahdi2010

Actually I wouldn't call it a gap because there is no gap between solid and fluid zones. The solid and fluid are "cellSetZone"s while this film surface mesh is a "faceSetZone". This is similar to the strategy used in tutorial cases of solvers like "reactingParcelFilmFoam". If for instance you want to run a tutorial case of such solver (which solves 2D film model within the flow), you would see in the "Allrun" file that first a wallFilm faceSetZone is created using "topoSet" over one of the walls. and then "extrudeToRegionMesh" is used to extrude that wall film faceSetZone into a surface (2D) mesh. briefly as follows:

1- defining wallFilmFaces to create a faceSet.(called wallFilmFaces)
2- changing this faceSet to a faceSetZone (called wallFilmRegion)
3- extruding the wallFilm surface mesh from the faceSetZone created in step No. 2.

I should mention that the first two steps are done by "topoSet" (or wallFilm.topoSet) and the last one is done by "extrudeToRegionMesh"

So you can see this is not a gap, this is only a one single layer surface mesh.
What I am trying to do is exactly the same procedure except that before step 1, I would do another step in which I split the mesh into solid and fluid zones. then I am trying to do the above-mentioned steps on the inter-section patch of the fluid and solid.

I see,
Well how about using createBaffles utility?
https://openfoamwiki.net/index.php/CreateBaffles

As the definition says: "Makes internal faces into boundary faces. Does not duplicate points, unlike mergeOrSplitBaffles."

Then you may use topoSet to define the faceZone.

However if you want to split the mesh and therefore have two separate boundaries on each side (so-called fluid and solid), you may use SplitMeshRegions.

[Mahdi2010]

Originally Posted by Mojtaba.a

I see,
Well how about using createBaffles utility?
https://openfoamwiki.net/index.php/CreateBaffles

As the definition says: "Makes internal faces into boundary faces. Does not duplicate points, unlike mergeOrSplitBaffles."

Then you may use topoSet to define the faceZone.

However if you want to split the mesh and therefore have two separate boundaries on each side (so-called fluid and solid), you may use SplitMeshRegions.

In fact I am using "splitMeshRegions" because it can split the cellZoneSets into two regions (with everything split up automatically)

But about the baffles I will try if this is possible for my case. Then will come back to this post

[Mojtaba.a]

Originally Posted by Mahdi2010

In fact I am using "splitMeshRegions" because it can split the cellZoneSets into two regions (with everything split up automatically)

But about the baffles I will try if this is possible for my case. Then will come back to this post

Well I didn't mention you have used splitMeshRegions at first. By this utility you won't have any internal faces actually, but instead there would be two external boundaries each belongs to a zone (fluid and solid).
In this case, the "CreateBaffles" utility will have no use. After splitMeshRegions you actually have to see the boundaries in there. Share your boundary file to see what is going on in there, before and after splitMeshRegions.

[Mahdi2010]

Originally Posted by Mojtaba.a

Well I didn't mention you have used splitMeshRegions at first. By this utility you won't have any internal faces actually, but instead there would be two external boundaries each belongs to a zone (fluid and solid).
In this case, the "CreateBaffles" utility will have no use. After splitMeshRegions you actually have to see the boundaries in there. Share your boundary file to see what is going on in there, before and after splitMeshRegions.

You are right. I also noticed the same when I checked CreateBaffles utility. When we use splitMeshRegions, there will be two automatically created patch belong to the fluid and solid zones each, as you also said. The point is that I was trying to extrude the face Mesh from the the one belongs to fluid (because then the film model is going to be solved within the fluid zone). I was aware of this fact.

Lets get back to the previous post where I wrote the 3 steps. Actually in the first step when I am going to create faceSet, I would have the following:

actions
(

{
name wallFilmSet;
type faceSet;
action new;
source patchToFace;
sourceInfo
{

INTERSECTION!!!;
}
}
)

So, the source is "patchToFace" and the sourceInfo should be this intersection. I mean if
can find a correct source info for this part, then I can proceed with step 2 and 3...
but the problem is that when I use splitMeshRegions, this intersection is defined but cannot be referred as an independent patch (like what we usually make and name in blockMesh). do you get what I am mentioning? after splitMeshRegions, of course there will be 2 patches in each zone, but these patches cannot be adressed here in the "sourceInfo"

[Mojtaba.a]

Originally Posted by Mahdi2010

You are right. I also noticed the same when I checked CreateBaffles utility. When we use splitMeshRegions, there will be two automatically created patch belong to the fluid and solid zones each, as you also said. The point is that I was trying to extrude the face Mesh from the the one belongs to fluid (because then the film model is going to be solved within the fluid zone). I was aware of this fact.

Lets get back to the previous post where I wrote the 3 steps. Actually in the first step when I am going to create faceSet, I would have the following:

actions
(

{
name wallFilmSet;
type faceSet;
action new;
source patchToFace;
sourceInfo
{

INTERSECTION!!!;
}
}
)

So, the source is "patchToFace" and the sourceInfo should be this intersection. I mean if
can find a correct source info for this part, then I can proceed with step 2 and 3...
but the problem is that when I use splitMeshRegions, this intersection is defined but cannot be referred as an independent patch (like what we usually make and name in blockMesh). do you get what I am mentioning? after splitMeshRegions, of course there will be 2 patches in each zone, but these patches cannot be adressed here in the "sourceInfo"

If there exists a patch then it should have been put in the boundary file by OF, then you will be use it. Otherwise you can't use it as patch. Share polyMesh/boundary to see the name of the patches. It is likely a name problem.

[Mahdi2010]

Originally Posted by Mojtaba.a

If there exists a patch then it should have been put in the boundary file by OF, then you will be use it. Otherwise you can't use it as patch. Share polyMesh/boundary to see the name of the patches. It is likely a name problem.

I already checked. My geometry consists of two zones and the names are: topFluid and bottomSolid. so the boundary file in "constants/topFluid/polyMesh" is:

2
(
walls
{
type wall;
inGroups 1(wall);
nFaces 17500;
startFace 552500;
}
topFluid_to_bottomSolid
{
type mappedWall;
inGroups 1(wall);
nFaces 2500;
startFace 570000;
sampleMode nearestPatchFace;
sampleRegion bottomSolid;
samplePatch bottomSolid_to_topFluid;
}
)

and the boundary file in "constants/bottomSolid/polyMesh" is:


2
(
walls
{
type wall;
inGroups 1(wall);
nFaces 5000;
startFace 182500;
}

bottomSolid_to_topFluid
{
type mappedWall;
inGroups 1(wall);
nFaces 2500;
startFace 190000;
sampleMode nearestPatchFace;
sampleRegion topFluid;
samplePatch topFluid_to_bottomSolid;
}
)


I defined all the surrounding walls as "walls", so the only thing which both zones share
is this intersection. I also tried to use the name "topFluid_to_bottomSolid" or "bottomSolid_to_topFluid"
as sourceInfo but it didn't work.

[Mojtaba.a]

Originally Posted by Mahdi2010

I already checked. My geometry consists of two zones and the names are: topFluid and bottomSolid. so the boundary file in "constants/topFluid/polyMesh" is:

2
(
walls
{
type wall;
inGroups 1(wall);
nFaces 17500;
startFace 552500;
}
topFluid_to_bottomSolid
{
type mappedWall;
inGroups 1(wall);
nFaces 2500;
startFace 570000;
sampleMode nearestPatchFace;
sampleRegion bottomSolid;
samplePatch bottomSolid_to_topFluid;
}
)

and the boundary file in "constants/bottomSolid/polyMesh" is:


2
(
walls
{
type wall;
inGroups 1(wall);
nFaces 5000;
startFace 182500;
}

bottomSolid_to_topFluid
{
type mappedWall;
inGroups 1(wall);
nFaces 2500;
startFace 190000;
sampleMode nearestPatchFace;
sampleRegion topFluid;
samplePatch topFluid_to_bottomSolid;
}
)


I defined all the surrounding walls as "walls", so the only thing which both zones share
is this intersection. I also tried to use the name "topFluid_to_bottomSolid" or "bottomSolid_to_topFluid"
as sourceInfo but it didn't work.

Well of course in this case you would have problems. You have two separate regions saved into two separate polyMesh folders. This is what splitMeshRegions does.
First you have to use mergeMeshes to merge both meshes in a single polyMesh folder and then do the rest. Note that mergeing meshes would not combine two boundaries into one.

So here is what you do:

1. Define two different problems, each contains its own OF folders, i.e: constant, system.

2. Copy each polyMesh folders to the above created constant directories. So until here you have two separate cases each containing a zone (one fluid and the other solid)

3. Now try mergeMeshes utility in one of those cases to make it one. for example if you are running the command in fluid's directory:

mergeMeshes "./" "../solid/"

This would make a new folder depending on your time step (You can even use overwrite option, but I don't suggest it since it removes the old fluid mesh). In this time step you have a single mesh (polyMesh) which is a combination of the last two. In the boundary of of this newly combined Mesh, you would have 3 total boundaries including: walls, topFluid_to_bottomSolid and bottomSolid_to_topFluid.
Now copy this combined polyMesh file into a newly constructed case and continue with your other preferred steps.

[Mahdi2010]

Originally Posted by Mojtaba.a

Well of course in this case you would have problems. You have two separate regions saved into two separate polyMesh folders. This is what splitMeshRegions does.
First you have to use mergeMeshes to merge both meshes in a single polyMesh folder and then do the rest. Note that mergeing meshes would not combine two boundaries into one.

So here is what you do:

1. Define two different problems, each contains its own OF folders, i.e: constant, system.

2. Copy each polyMesh folders to the above created constant directories. So until here you have two separate cases each containing a zone (one fluid and the other solid)

3. Now try mergeMeshes utility in one of those cases to make it one. for example if you are running the command in fluid's directory:

mergeMeshes "./" "../solid/"

This would make a new folder depending on your time step (You can even use overwrite option, but I don't suggest it since it removes the old fluid mesh). In this time step you have a single mesh (polyMesh) which is a combination of the last two. In the boundary of of this newly combined Mesh, you would have 3 total boundaries including: walls, topFluid_to_bottomSolid and bottomSolid_to_topFluid.
Now copy this combined polyMesh file into a newly constructed case and continue with your other preferred steps.

Thanks for the hint, I will try to see if it works. but before that let me ask a question.
Actually from the beginning I have one single geometry and mesh created in blockMesh, and I split it by splitMesh. Do you mean I should avoid that or you mean first splitMesh and then mergeMesh? what if I don't use the splitMesh at all? I could not get that.

[Mojtaba.a]

Originally Posted by Mahdi2010

Thanks for the hint, I will try to see if it works. but before that let me ask a question.
Actually from the beginning I have one single geometry and mesh created in blockMesh, and I split it by splitMesh. Do you mean I should avoid that or you mean first splitMesh and then mergeMesh? what if I don't use the splitMesh at all? I could not get that.

Well the procedure I just mentioned above is after which you have used spliMeshRegions, however now I have a much more easier procedure for doing this. You can do these all only using blockMesh.
The point is that, when editing the blockMeshDict file, at the intersection boundary of the two zones try defining duplicate vertices each blonging to a block (which they would be defined as cellzones later in blockMesh). By this procedure you can easily have two separate faces in the intersection and you can define boundaries on them.
Next, you have to define cellzones for each block. I assume you know how to do that in blockMeshDict.

[Mahdi2010]

Originally Posted by Mojtaba.a

Well the procedure I just mentioned above is after which you have used spliMeshRegions, however now I have a much more easier procedure for doing this. You can do these all only using blockMesh.
The point is that, when editing the blockMeshDict file, at the intersection boundary of the two zones try defining duplicate vertices each blonging to a block (which they would be defined as cellzones later in blockMesh). By this procedure you can easily have two separate faces in the intersection and you can define boundaries on them.
Next, you have to define cellzones for each block. I assume you know how to do that in blockMeshDict.

I applied what you suggested. Thanks. Seems that problem is solved. But afterward when physical model for film motion is called, suddenly the error below arose:

--> FOAM FATAL ERROR:

request for polyMesh region0 from objectRegistry BOX_SolidFluidFilmRegions failed
available objects of type polyMesh are

3
(
bottomSolid
topFluid
wallFilmRegion
)


I tried to find out where we had something like region0 ( I guess this usually is the case when you leave some zones without specified name, right?). but I couldn't find it in the case. Do you have any suggestion?

[Mojtaba.a]

Originally Posted by Mahdi2010

I applied what you suggested. Thanks. Seems that problem is solved. But afterward when physical model for film motion is called, suddenly the error below arose:

--> FOAM FATAL ERROR:

request for polyMesh region0 from objectRegistry BOX_SolidFluidFilmRegions failed
available objects of type polyMesh are

3
(
bottomSolid
topFluid
wallFilmRegion
)


I tried to find out where we had something like region0 ( I guess this usually is the case when you leave some zones without specified name, right?). but I couldn't find it in the case. Do you have any suggestion?

Well I am not very familiar with film models, but as I guess I have seen this error in some other threads, too.
Out of curiosity, you have defined the sets or zones using blockMesh, right? Something like this: http://www.cfd-online.com/Forums/ope...tml#post373467

[Mahdi2010]

Originally Posted by Mojtaba.a

Well I am not very familiar with film models, but as I guess I have seen this error in some other threads, too.
Out of curiosity, you have defined the sets or zones using blockMesh, right? Something like this: http://www.cfd-online.com/Forums/ope...tml#post373467

No. I used topoSet to define cell zones (one step before splitMesh) but the link you put here seems also a nice way I haven't seen before.
However seems not useful in my case because there are only two regions (except the film) and I intentionally want to make them split unless
I define different zones like this:

hex (0 1 3 2 6 7 9 8) topFluid (200 100 1) simpleGrading (1.0 1.0 1.0)
hex (2 3 5 4 8 9 11 10) bottomSolid (200 100 1) simpleGrading (1.0 1.0 1.0)

and then no need to splitMesh command? but what would be the benefit?

[Mojtaba.a]

Originally Posted by Mahdi2010

No. I used topoSet to define cell zones (one step before splitMesh) but the link you put here seems also a nice way I haven't seen before.
However seems not useful in my case because there are only two regions (except the film) and I intentionally want to make them split unless
I define different zones like this:

hex (0 1 3 2 6 7 9 8) topFluid (200 100 1) simpleGrading (1.0 1.0 1.0)
hex (2 3 5 4 8 9 11 10) bottomSolid (200 100 1) simpleGrading (1.0 1.0 1.0)

and then no need to splitMesh command? but what would be the benefit?

Well I am not sure but doesn't splitMesh command results in multiple polyMesh directories? My whole effort was to eliminate the actions of splitting and topoSet and the merging them into one polyMesh. Because you can do all of them using blockMesh.
On the other hand the name of the boundaries are in your hands while editing blockMesh. Of course the alternative is to change the names in the boundary file.

[Mahdi2010]

Originally Posted by Mojtaba.a

Well I am not sure but doesn't splitMesh command results in multiple polyMesh directories? My whole effort was to eliminate the actions of splitting and topoSet and the merging them into one polyMesh. Because you can do all of them using blockMesh.
On the other hand the name of the boundaries are in your hands while editing blockMesh. Of course the alternative is to change the names in the boundary file.

Yes you are right. This way works well for putting the topoSet for cellzones aside. But anyway I need splitMesh because it creates the multiple directories. I also tested it right now, I faced the same error (saying that the intersection is not defined although it is written in the boundary file!!). So I can conclude in my case, the way you suggested is still an important step to be done (the mergeMesh command).
But let's get back to the alternative you said, by duplicating vertices in blockMesh. What do you exactly mean? because I did the same but at the end I had two boxes with no connection, so blockMesh failed to build the geometry. It is probably a misunderstanding of what you say.

[Mojtaba.a]

Originally Posted by Mahdi2010

Yes you are right. This way works well for putting the topoSet for cellzones aside. But anyway I need splitMesh because it creates the multiple directories. I also tested it right now, I faced the same error (saying that the intersection is not defined although it is written in the boundary file!!). So I can conclude in my case, the way you suggested is still an important step to be done (the mergeMesh command).
But let's get back to the alternative you said, by duplicating vertices in blockMesh. What do you exactly mean? because I did the same but at the end I had two boxes with no connection, so blockMesh failed to build the geometry. It is probably a misunderstanding of what you say.

How about re-asking your question in here and maybe sharing a sample case, since I would feel more convenient answering in there.