CFD Online Discussion Forums - Access boundaryMesh / boundaryField on cellZone

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)

- - Access boundaryMesh / boundaryField on cellZone (https://www.cfd-online.com/Forums/openfoam-programming-development/140381-access-boundarymesh-boundaryfield-cellzone.html)

Access boundaryMesh / boundaryField on cellZone

Hi all:

I have a question similar to one posed in an earlier thread regarding the manipulation of cellZones.

I would like to calculate the wall shear stress on the boundary of a cellZone which I have created using topoSet. I think this would be something like:

Code:

            const label cellZoneID = mesh.cellZones().findZoneID("myCellZone");

            if (cellZoneID < 0)

            {

                FatalError

                    << "Unable to find cell zone " << "myCellZone" << endl

                    << exit(FatalError);

            }

            const cellZone& zone = mesh.cellZones()[cellZoneID];

            const cellZoneMesh& zoneMesh = zone.zoneMesh();

            const labelList& cellsZone = zoneMesh[cellZoneID];



           // Calculate WSS as in 'wallShearStress' utility:

            autoPtr<incompressible::RASModel> model

            (

                incompressible::RASModel::New(U, phi, laminarTransport)

            );

            const volSymmTensorField Reff(model->devReff());



            // Perform this calculation over the cell set only - how?

            scalarField zoneWSS = mag( (-mesh.Sf().boundaryField()[cellZoneID]/mesh.magSf().boundaryField()[cellZoneID]) & Reff.boundaryField()[cellZoneID] )

But I don't think "mesh.Sf().boundaryField()[cellZoneID]" is correct (this would access the patch corresponding to cellZoneID, not the cellZone, right?).

Can anyone give me some guidance on how to proceed? Thanks!

-Nuc

P.S.
Relevant thread:
http://www.cfd-online.com/Forums/ope...ne-volume.html

Quote:

Originally Posted by rob3rt (Post 267069)

... I know there is a function like mag(mesh.Sf().boundaryField()[cellZoneID][cI]) ... <-- This is what I'm looking for, but I'm not sure about the syntax

Just a short question: Are there multiple boundary patches in the cellZone?

Quote:

Originally Posted by jhoepken (Post 505970)

Just a short question: Are there multiple boundary patches in the cellZone?

In this case, there is only one boundary patch (a wall) and then some exposed internal faces.

Is it possible to query a patch within a cellZone?

Why don't you create a faceZone that solely contains the boundary faces and just loop over them?

Quote:

Originally Posted by jhoepken (Post 506002)

Why don't you create a faceZone that solely contains the boundary faces and just loop over them?

jhoepken,

I tried this, but the faceSet I created included internal faces in my bounding box.If I can create a faceSet from a patch, that would work, so I'll look into that.

Thanks!

*EDIT: I got it - see bottom

Okay, I was able to create a faceSet of boundary faces only via the following topoSetDict code (the key - use of "action subSet"):

Code:

    {

        name   myFaceSet;

        type    faceSet;

        action  new;

        source  patchToFace;

        sourceInfo

        {

            name myPatch;

        }

    }

    {

        name  myFaceSet;

        type    faceSet;

        action  subset;

        source boxToFace;

        sourceInfo

        {

            box   (-0.045 -0.0123 -0.02) (-0.00209 0.0105 0.015);

        }

    }

    {



        name     myFaceZone;

        type      faceZoneSet;

        action    new;

        source   setToFaceZone;

        sourceInfo

        {

            faceSet myFaceSet;

        }

    }

So, now I have a faceZone containing global indices to the faces in my region of interest. However, I am having trouble querying these faces. For example, mesh.magSf() allows for accessing faces using their global index, but it only includes internal faces, not boundary faces.

Meanwhile, mesh.magSf().boundaryField() allows for accessing boundary faces by patch ID and local face ID, not global face ID.

How would I instead query the face area of the faces in my faceZone, which are boundary faces? Thanks again!

Code:

           // Example Code:

           scalar zoneFaceArea(0);



           forAll (facesZone, faceI)

           {

                // mesh.magSf() addresses internal faces only, while the indices from facesZone[faceI] address boundary faces...

                zoneFaceArea += mesh.magSf()[facesZone[faceI]]; 

           }

*SOLUTION:
To convert between global faceID and local, patch-based faceID, you can use the 'whichPatch' and 'whichFace' functions. So, something like the following:

Code:

           scalar zoneFaceArea(0);



           forAll (facesZone, faceI)

           {

                label facePatchID = mesh.boundaryMesh().whichPatch(faceI);

                label faceID = mesh.boundaryMesh()[facePatchID].whichFace(facesZone[faceI]);                 



                zoneFaceArea += mesh.magSf().boundaryField()[facePatchID][faceID];

                // etc... 

           }

I found references to these functions in "src/fvOptions/sources/derived/effectivenessHeatExchangerSource/effectivenessHeatExchangerSource.C"

Thanks for the help jhoepken! I hope your book is coming along well - it looks interesting.

Great that you've figured it out! I was busy and could not answer, sorry :).

I am interested of this topic.

I made faceZone with snappyHexMesh using stl file like:

Code:

faceZone1

{

level (1 1);

cellZone  cz1;

faceZone fz1;

...

}

And I want get access to pressure and U fields on this surface (fz1) during calculation. How it can be implemented? I tried to use code from this topic but has no effect.

Andy,

Can you post your code so we can see what's going on? You need to setup a few things before you can access faceZone data.

It not easy because there is no way to see it in my project now. I tried different variants.

Code:

label zID = mesh.facesZone().findZoneID(zName);

const faceZone& facesZone = mesh.faceZone()[zID];

 

forAll(facesZone, I)

{

Here I want get access to pressure field. If I try code as

p.boundaryField()[zID][i]; 

I get acces to patch field with ID=zID

 

If I try 

facePatchID = mesh.boundaryMesh().whichPatch(zID);

fID = mesh.boundaryMesh[facePatchID].whichFace(facezZone[zID])

I get error during calculation.

}

Sorry, may be errors because I entered the code as I remember.

Do you have any idea?

Can you post your error message too? I'll dig up my code later and see how the syntax differs.

BTW: you have a typo in your code:
facezZone[zID]

facesZone[zID]

PrintStack error. I think it is because faceZone length array and numder iteration in cycle is different

Code:

facezZone[zID]

facesZone[zID]

It's my mistake. All right in code

Maybe there is function in mesh which get faceID and return cellID?

I solved this problem but it is not work in parallel. Because there are boundaryfaces on processor and faces are duplicate. How can I delete duplicate faces on processor?

Hi to all,

I'm also interested to the topic.
How did you solve the PrintStack error?

Thanks
Giacomo

Spanwise averaging fields within a cellSet.

Ken
Are you ware of the spanwise averaging utility "postSpanwiseAverage" posted by some one on this forum. I need to use it, but wish to calculate the spanwise average of a field in particular cellSet. Do know how to do that

Hi Nucleophobe,

I managed to follow all your steps successfully to loop over all faces of a facezone which was created as a subset. However, I cant seem to be able to run in parallel (edit: or series) even though im using the reduce(facesum, sunOp<scalar>()) .The solver crashes with the following error:

[1] #0 Foam::error::printStack(Foam::Ostream&) at ??:?
[1] #1 Foam::sigSegv::sigHandler(int) at ??:?
[1] #2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3 Foam::OutputInfoFunctionObject::execute() at ~/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude/polyPatch.H:392
[1] #4 Foam::functionObjectList::execute() at ??:?
[1] #5 Foam::Time::run() const at ??:?
[1] #6 ? at ??:?
[1] #7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #8 ? at ??:?
[mne-alra12:22426] *** Process received signal ***
[mne-alra12:22426] Signal: Segmentation fault (11)
[mne-alra12:22426] Signal code: (-6)
[mne-alra12:22426] Failing at address: 0x3ea0000579a

My code:
const label stagID = mesh().faceZones().findZoneID("StagZone");
const faceZone& zone = mesh().faceZones()[stagID];
const faceZoneMesh& zonemesh = zone.zoneMesh();
const labelList& stagcells = zonemesh[stagID];

forAll( stagcells, facei)
{

label facePatchID = mesh().boundaryMesh().whichPatch(facei);
label faceID = mesh().boundaryMesh()[facePatchID].whichFace(stagcells[facei]);

faceArea += (mesh().magSf().boundaryField()[facePatchID][faceID]);

}

reduce(faceArea,sumOp<scalar>());