CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   PatchToPatchInterpolationfaceInterpolate (http://www.cfd-online.com/Forums/openfoam-solving/59868-patchtopatchinterpolationfaceinterpolate.html)

cosimobianchini January 8, 2007 13:04

Hi all, I have such a problem
 
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 April 12, 2011 07:20

Hi,

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

Philip

feymark April 12, 2011 08:38

Hi,

I'm also interested in knowing the answer! :)

/FEYMARK

cosimobianchini April 30, 2011 13:52

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 June 3, 2011 09:50

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
Code:

faceSet <patchName>FaceZone new patchToFace <patchName>
quit

then the command
Code:

setsToZones -noFlipMap
Then in your decomposeParDict, add the line:
Code:

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
Code:

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 March 7, 2013 16:30

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 March 7, 2013 16:37

Hi Benjamin,

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

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

Best regards,
Philip

mcdonalds March 7, 2013 17:30

Quote:

Originally Posted by bigphil (Post 412387)
Hi Benjamin,

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

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:

HTML Code:

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 March 8, 2013 05:38

Quote:

Originally Posted by mcdonalds (Post 412404)
Yes I have done so and I am still getting errors. In your code you have:

HTML Code:

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":
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]);

regards,
Philip

mcdonalds March 8, 2013 13:55

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

HTML Code:

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 March 8, 2013 14:02

Quote:

Originally Posted by mcdonalds (Post 412616)
Here is my code, pretty much an exact replica of yours:

HTML Code:

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 March 8, 2013 14:56

Quote:

Originally Posted by bigphil (Post 412617)
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 March 8, 2013 15:42

Quote:

Originally Posted by bigphil (Post 412617)
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

Quote:

Originally Posted by mcdonalds (Post 412622)
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:

HTML 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 March 8, 2013 16:58

Update
 
So this is what I have so far:

HTML Code:

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 March 11, 2013 06:44

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 March 11, 2013 13:13

Quote:

Originally Posted by bigphil (Post 413085)
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 March 11, 2013 14:19

Quote:

Originally Posted by mcdonalds (Post 413173)
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 March 12, 2013 13:05

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 March 12, 2013 17:07

2 Attachment(s)
Quote:

Originally Posted by mcdonalds (Post 413173)
How would I go about using implicitly coupled boundaries? Is there information where I can find out more about implicitly coupled boundaries?

Sincerely,

Benjamin

Quote:

Originally Posted by bigphil (Post 413497)
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 March 12, 2013 18:24

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


All times are GMT -4. The time now is 09:15.