[cosimobianchini]

Hi all,
I have such a problem:
I'm using PatchToPatchInterpolation.faceInterpolate() to map boundary conditions on a patch from the coincident patch on another mesh (imposing heat flux and temperature continuity on a solid-fluid interface in a conjugate solver).
In a single-processor run it is working perfectly even if the two meshes are not conformal (the global geometry is the same).
If I run the case in parallel, with the processor patch normal to the interface, the two sides (solid & fluid) of the interface on processorn are not conformal and have different geometry (there is no way of decomposing the meshes in order to obtain coincident geometry: no shared vertex).
In this case PatchToPatchInterpolation.faceInterpolate() is not giving good results in the zone near processor patch, read where the two sides of the interface differ in geometry.
Any hint on how to still use PatchToPatchInterpolation.faceInterpolate() is very appreciated.
(I use default choices for algorithm and direction)
Thanks a lot
Cosimo

[bigphil]

Hi,

I realise this is quite an old thread but did you ever get the patchToPatchInterpolation class to work correctly in parallel?

Philip

[feymark]

Hi,

I'm also interested in knowing the answer!

/FEYMARK

[cosimobianchini]

It actually is a quite old thread but to my knowledge patchToPatchInterpolation is not working in parallel in the latest versions too. In order to make it work in parallel you can try one of the following ways:

• use GGIInterpolation only in the ext version
• use some tricks to decompose the patch on the same processor
• implement your own parallel communication and recostruct the full patch and patchField locally and then perform the interpolation

Hope this is still useful,
Cosimo

[bigphil]

Hi,


I was able to get my code with patchToPatchInterpolation to work in parallel.

The way I did it was:

In the case,
for the patches of interest define faceZones, using the setSet utility

faceSet <patchName>FaceZone new patchToFace <patchName>
quit

then the command

setsToZones -noFlipMap

Then in your decomposeParDict, add the line:

globalFaceZones ( <faceZoneName1> <faceZoneName2>)

then when you decompose your case the full faceZone meshes will be included on each processor.

In your code, you can create a zoneToZoneInterpolation

label faceZone1ID = cp_.mesh().faceZones().findZoneID(facezoneName1);
label faceZone2ID = mesh.faceZones().findZoneID(faceZoneName2);

zoneToZoneInterpolation faceZoneInterpolator
        (
         mesh.faceZones()[faceZone1ID](), // from                                                                                          
         mesh.faceZones()[FaceZone2ID](), // to zone                                                                                        
         );

then you can use this interpolator just like a patchToPatch interpolator and it works in parallel.

However be careful when you have a moving mesh as the faceZone meshes might not be moved correctly, you might have to correct them and keep them consistent across the processors.


Hope it helps,
Philip

[mcdonalds]

I am trying to use patchtopatchinterpolation.H and I ID'd my patches and declared the pointtopointinterpolation. How do I do the last step, use the interpolator to map one patch to another?

Benjamin

Here is my code:

1) Set findID codes.

label cathodeID = mesh.boundaryMesh(). findPatchID("bottomcathode");


label electrodeID = mesh.boundaryMesh().findPatchID("topelectrode");

2) Declare patchtopatchinterpolation.

const polyPatch& electrodePatch = mesh.boundaryMesh()[electrodeID];
const polyPatch& cathodePatch = mesh.boundaryMesh()[cathodeID];

patchToPatchInterpolation cathodeToElectrode
(
cathodePatch,
electrodePatch
);

[bigphil]

Hi Benjamin,

From your email, you need to specify the template parameter for the faceInterpolate function i.e:

scalarField interpolatedQuantity = cathodeToElectrode.faceInterpolate<scalar>
(
         H2O.boundaryField()[cathodePatch]
);

Best regards,
Philip

[mcdonalds]

Originally Posted by bigphil

Hi Benjamin,

From your email, you need to specify the template parameter for the faceInterpolate function i.e:

scalarField interpolatedQuantity = cathodeToElectrode.faceInterpolate<scalar>
(
         H2O.boundaryField()[cathodePatch]
);

Best regards,
Philip

Yes I have done so and I am still getting errors. In your code you have:

vectorField interpolatedQuantity = fromPatch_To_toPatch_Interpolate.faceInterpolate<vector> ( quantity.boundaryField()[fromPatchIndex] );

Firstly, what is the interpolatedQuantity refer to? When I compile it says that it is an unused variable. So how do I use it?

Second, what does quantity refer to in your "quantity.boundaryField()[fromPatchIndex]? I am putting my scalarfield (H2O) there but I do not think that is correct.

Sincerely,

Benjamin

[bigphil]

Originally Posted by mcdonalds

Yes I have done so and I am still getting errors. In your code you have:

vectorField interpolatedQuantity = fromPatch_To_toPatch_Interpolate.faceInterpolate<vector> ( quantity.boundaryField()[fromPatchIndex] );

Firstly, what is the interpolatedQuantity refer to? When I compile it says that it is an unused variable. So how do I use it?

Could you post your code that does not compile here?
The quantities mentioned in my previous post are just generic and are to be replaced with your specific scalar/vector/tensor fields.

I will try give a more clear example:

If I want to copy my temperature field T from the boundary patch called "left" to the boundary patch called "right":

label leftID = mesh.boundaryMesh().findPatchID("left");
label rightID = mesh.boundaryMesh().findPatchID("left");
patchToPatchInterpolation interpolator
(
 mesh.boundaryMesh()[leftID],    // from patch
 mesh.boundaryMesh()[rightID],     // to patch
 intersection::FULL_RAY,
 intersection::CONTACT_SPHERE
 );
scalarField TRightPatch = interpolator.faceInterpolate<scalar>(T.boundaryField()[leftID]);

regards,
Philip

[mcdonalds]

Here is my code, pretty much an exact replica of yours:

label bottomID = mesh.boundaryMesh().findPatchID("bottomcathode");
label topID = mesh.boundaryMesh().findPatchID("topelectrode");

patchToPatchInterpolation interpolator
(
 mesh.boundaryMesh()[bottomID],    // from patch
 mesh.boundaryMesh()[topID],     // to patch
 intersection::FULL_RAY,
 intersection::CONTACT_SPHERE

 );
scalarField H2ObottomcathodePatch = interpolator.faceInterpolate<scalar>

(
    H2O.boundaryField()[bottomID]

);

Now it is compiling, which is great. What I'm unsure about is the intersection piece? What is Full_ray and Contact_sphere? a set? region?

Also, what should my case/0/H2O file look like? Specifically, what type do I use for the patches I'm connecting?

Lastly, just to double check, I place this code within the time loop of my solver, right?

Sincerely,


Benjamin

[bigphil]

Originally Posted by mcdonalds

Here is my code, pretty much an exact replica of yours:

label bottomID = mesh.boundaryMesh().findPatchID("bottomcathode");
label topID = mesh.boundaryMesh().findPatchID("topelectrode");

patchToPatchInterpolation interpolator
(
 mesh.boundaryMesh()[bottomID],    // from patch
 mesh.boundaryMesh()[topID],     // to patch
 intersection::FULL_RAY,
 intersection::CONTACT_SPHERE

 );
scalarField H2ObottomcathodePatch = interpolator.faceInterpolate<scalar>

(
    H2O.boundaryField()[bottomID]

);

Now it is compiling, which is great. The only thing I have a question on is what is my intersection? What is Full_ray and Contact_sphere? a set? region?

Benjamin

The intersection options define how the projection is performed from one patch to another. The direction can be in the normal direction (HALF_RAY), in both directions (FULL_RAY) or in the normal direction to the visible portion of the surface (VISIBLE).
The distances are then calculated by either fitting spheres between the surfaces (CONTACT_SPHERE) or using a normal vector (VECTOR).
To find out more, you can read through the patchToPatchInterpolation class.

Best regards,
Philip

[mcdonalds]

Originally Posted by bigphil

The intersection options define how the projection is performed from one patch to another. The direction can be in the normal direction (HALF_RAY), in both directions (FULL_RAY) or in the normal direction to the visible portion of the surface (VISIBLE).
The distances are then calculated by either fitting spheres between the surfaces (CONTACT_SPHERE) or using a normal vector (VECTOR).
To find out more, you can read through the patchToPatchInterpolation class.

Best regards,
Philip

Everything seems to be working. Solver is compiling and the solver runs in my case. However, when i look at the results the two patches aren't passing the information. Two quick questions:

What should my case/0/H2O file look like? Specifically, what type do I use for the patches I'm connecting?

Lastly, just to double check, I place this code within the time loop of my solver, right?

Sincerely,

Benjamin

[mcdonalds]

Originally Posted by bigphil

The intersection options define how the projection is performed from one patch to another. The direction can be in the normal direction (HALF_RAY), in both directions (FULL_RAY) or in the normal direction to the visible portion of the surface (VISIBLE).
The distances are then calculated by either fitting spheres between the surfaces (CONTACT_SPHERE) or using a normal vector (VECTOR).
To find out more, you can read through the patchToPatchInterpolation class.

Best regards,
Philip

Originally Posted by mcdonalds

Everything seems to be working. Solver is compiling and the solver runs in my case. However, when i look at the results the two patches aren't passing the information. Two quick questions:

What should my case/0/H2O file look like? Specifically, what type do I use for the patches I'm connecting?

Lastly, just to double check, I place this code within the time loop of my solver, right?

Sincerely,

Benjamin

Also, it seems like in your code:

label leftID = mesh.boundaryMesh().findPatchID("left"); label rightID = mesh.boundaryMesh().findPatchID("left"); patchToPatchInterpolation interpolator (  mesh.boundaryMesh()[leftID],    // from patch  mesh.boundaryMesh()[rightID],     // to patch  intersection::FULL_RAY,  intersection::CONTACT_SPHERE  ); scalarField TRightPatch = interpolator.faceInterpolate<scalar>(T.boundaryField()[leftID]);

There is a dangling label in the last line, namely, "TRightPatch". How do I use this label and associate it with the "to patch"?

Benjamin

[mcdonalds]

So this is what I have so far:

label bottomID = mesh.boundaryMesh().findPatchID("bottomcathode");
label topID = mesh.boundaryMesh().findPatchID("topelectrode");

patchToPatchInterpolation interpolator
(
 mesh.boundaryMesh()[bottomID],    // from patch
 mesh.boundaryMesh()[topID],     // to patch
 intersection::FULL_RAY,
 intersection::VECTOR

 );

H2O.boundaryField()[topID] = interpolator.faceInterpolate <scalar>


(
    H2O.boundaryField()[bottomID]

);

I think everything here is good and should work. Now I don't know how to insert what I've done in my solver to my case. Specifically, how do I assign the patches in my case/0/H2O boundary file? What I have in my solver isn't connecting to my case.

Benjamin

[bigphil]

Hi Benjamin,

The patchToPatch interpolation explicitly passes a field from one patch to another,
so it allows explicit coupling of patches.
Depending on the system, you may need a loop within each time-step where you solve the governing equation then explicitly update the boundaries and iterate until convergence.

Alternatively if you could use implicitly coupled boundaries it would probably be faster and more stable.

Best regards,
Philip

[mcdonalds]

Originally Posted by bigphil

Hi Benjamin,

The patchToPatch interpolation explicitly passes a field from one patch to another,
so it allows explicit coupling of patches.
Depending on the system, you may need a loop within each time-step where you solve the governing equation then explicitly update the boundaries and iterate until convergence.

Alternatively if you could use implicitly coupled boundaries it would probably be faster and more stable.

Best regards,
Philip

How would I go about using implicitly coupled boundaries? Is there information where I can find out more about implicitly coupled boundaries?

Sincerely,

Benjamin

[mcdonalds]

Originally Posted by mcdonalds

How would I go about using implicitly coupled boundaries? Is there information where I can find out more about implicitly coupled boundaries?

Sincerely,

Benjamin

Hey BigPhil,

So I read through your posts that you got patchtopatch coupling working in parallel. And you had already been able to work it in serial. Do you have the code in serial where you get patchtopatch coupling working? Would you be able to share that code?

Sincerely,

Benjamin

[bigphil]

Hi Benjamin,

I used patchToPatchInterpolation in the elasticContactSolidFoam solver (actually in the contactPatchPatch class) which is in the solidMechanics branch of OpenFOAM-1.6-ext.

As regards implicit boundary coupling, I am not that familiar with it, I would recommend google and the forum search.

Best regards,
Philip

[mcdonalds]

Originally Posted by mcdonalds

How would I go about using implicitly coupled boundaries? Is there information where I can find out more about implicitly coupled boundaries?

Sincerely,

Benjamin

Originally Posted by bigphil

Hi Benjamin,

I used patchToPatchInterpolation in the elasticContactSolidFoam solver (actually in the contactPatchPatch class) which is in the solidMechanics branch of OpenFOAM-1.6-ext.

As regards implicit boundary coupling, I am not that familiar with it, I would recommend google and the forum search.

Best regards,
Philip

Hello Phil,

I downloaded the open extension 1.6 and the solidmechanics files. It is extremely complex but I've filtered through it and it seems that I am on the right track. When you do use the interpolator you definitely do use a forall loop. So, I've tried modifying my code. I was hoping you could take a quick look at it to see where I have gone wrong. It just doesn't seem to be picking up those mapped patches when I run the case.

It is of a really simple case so very basic.

Sincerely,

Benjamin

[bigphil]

Benjamin,

I downloaded waterFoam2.tar.gz and looked at the '.C' file,
there is a lot of code commented out and it is not clear what exactly you are trying to do and where your problem is.
If you tidy up the solver and add descriptive comments pointing out exactly what code is not doing what you expect, then I may be able to help.

Best regards,
Philip