|
[Sponsors] |
December 30, 2007, 20:05 |
Dear OpenFOAMers
Greetings
|
#1 |
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 18 |
Dear OpenFOAMers
Greetings I need the face list of faces belonging to a boundary patch. This is what I am doing: label patchID = mesh.boundaryMesh().findPatchID("cylinder"); const polyPatch& cPatch = mesh.boundaryMesh()[patchID]; With the above code lines I can create a polyPatch and assign it equal to the boundary patch i need. Please give me a clue on how to access the faces of this patch as I need to loop over these faces. Thanks in advance Best Regards Jaswinder PS: I am searching the posts simultaneously |
|
December 30, 2007, 22:16 |
Hi Forum
Good Evening once
|
#2 |
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 18 |
Hi Forum
Good Evening once again I wanted to calculate the surface area of a patch. This is how I achieved the result : label patchID = mesh.boundaryMesh().findPatchID("walls"); const polyPatch& cPatch = mesh.boundaryMesh()[patchID]; const surfaceScalarField& magSf = mesh.magSf(); scalar patchArea = 0.0; forAll(cPatch, facei) { patchArea += magSf.boundaryField()[patchID][facei]; } Info << "Patch Area " << patchArea << endl; I checked it for a cylinder and it gives accurate result. I am sure that it can be done in a more elegant way. Experts please suggest. Now the next step is to iterate over the faces of this patch and sum the area of only those faces where value of volume fraction gamma is positive. Any suggestions are highly appreciated. Wish you all a successful year ahead Best Regards Jaswinder |
|
December 30, 2007, 22:19 |
Jaswinder,
you can access e
|
#3 |
New Member
Shivasubramanian Gopalakrishnan
Join Date: Mar 2009
Location: Amherst, Massachusetts, USA
Posts: 15
Rep Power: 17 |
Jaswinder,
you can access each of the faces in this manner after getting specific patch. forAll(cPatch, faceI) { //whatever you need to access here } regards Shiva |
|
December 30, 2007, 22:55 |
Thanks Shiva
Your profile s
|
#4 |
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 18 |
Thanks Shiva
Your profile shows that you work with Multiphase Flows. That's a good news for me as I am a novice in this field and have been looking out for people who are experienced, especially within OpenFOAM community. Kind Regards Jaswinder |
|
December 31, 2007, 13:14 |
Hi Jaswinder,
good to know
|
#5 |
New Member
Shivasubramanian Gopalakrishnan
Join Date: Mar 2009
Location: Amherst, Massachusetts, USA
Posts: 15
Rep Power: 17 |
Hi Jaswinder,
good to know you are working in multiphase flows as well. I am still learning a lot about this. you can use an if test in the for loop for checking faces with gamma > 0 . forAll(cPatch,faceI) { if (gamma.boundaryField()[patchID][faceI] > 0) //whatever you need to do. } This works, but am not sure how efficient this is and whether there is any other elegant workaround. regards Shiva |
|
January 6, 2008, 07:04 |
Thanks Shiva
It works.
|
#6 |
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 18 |
Thanks Shiva
It works. Happy New year Jaswinder |
|
March 2, 2013, 22:43 |
sum of areas of all faces of a cell
|
#7 |
New Member
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
I have a similar problem to solve. I want to calculate, for each given cell in the domain :
Length= cell Volume / sum of areas of all faces of a cell Can you kindly help me how can I code this. |
|
March 3, 2013, 02:59 |
How to loop over cell faces
|
#8 |
Senior Member
Fumiya Nozaki
Join Date: Jun 2010
Location: Yokohama, Japan
Posts: 266
Blog Entries: 1
Rep Power: 19 |
Hi Marshak,
I think it is better to start another thread for being easy to search later. Regarding your question, the following is my sample code: Code:
scalar sumA = 0.0; //Sum of areas of all faces of a cell const cell& cFaces = mesh.cells()[yourCellIndex]; forAll(cFaces, i) { sumA += mag(mesh.Sf()[cFaces[i]]); //cFaces[i]: face label of a cell } scalar Length = mesh.V()[yourCellIndex]/sumA; Fumiya |
|
September 28, 2013, 16:34 |
|
#9 |
New Member
David
Join Date: Mar 2010
Location: Vancouver, Canada
Posts: 13
Rep Power: 16 |
label patchID = mesh.boundaryMesh().findPatchID("NAME OF PATCH");
Info << "patchID = " << patchID << endl; const polyPatch& cPatch = mesh.boundaryMesh()[patchID]; Info << "cPATCH = " << nl << cPatch << endl; const surfaceScalarField& magSf = mesh.magSf(); scalar AREA = gSum(magSf.boundaryField()[patchID]); Info << "AREA = " << nl << AREA << endl; You might find it more efficient to do the following, it will avoid the need for additional looping. There is also the Foam::max and Foam::min function when needed to only sum more or less than a given value. Cheers DH |
|
October 1, 2013, 06:06 |
|
#10 |
New Member
Join Date: Feb 2012
Posts: 25
Rep Power: 14 |
Is this the procedure for boundary patches only? if yes then how about finding surface area of each internal mesh cell?
|
|
December 4, 2013, 05:37 |
|
#11 |
Member
Ye Zhang
Join Date: Dec 2009
Location: Delft,Netherland
Posts: 92
Rep Power: 16 |
Dear DH,
should I add this code into controlDict file? or the solver code? |
|
December 4, 2013, 15:01 |
Faces... faces... everywhere...
|
#12 |
New Member
David
Join Date: Mar 2010
Location: Vancouver, Canada
Posts: 13
Rep Power: 16 |
The routine above works for addressable patches, i.e. ones that have been created in blockmesh or are created upon splitting a mesh for multi-region. This code would be included in the solver, not in controlDict.
If you wanted to do a loop over all faces in a domain, there are examples of this in the grad calc function in OpenFoam's source guide. I do have code for this and will try to post a "how" later on today. Cheers, DH |
|
September 19, 2014, 06:20 |
surface area of boundary
|
#13 |
New Member
Caro
Join Date: Jul 2014
Posts: 15
Rep Power: 12 |
I solved my problem below. It is working.
Hello, I am using the coldEngine solver and I wanted to get the area of the cylinderwalls. The walls of the cylinder are definded as walls in a boundary patch called 'liner'. The mesh is changing over time and so is the surface of the liner. This is the code I used: #include "fvCFD.H" #include "fvCFD.H" #include "wallFvPatch.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Main program: int main(int argc, char *argv[]) { // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // timeSelector::addOptions(); #include "addRegionOption.H" #include "setRootCase.H" #include "createTime.H" instantList timeDirs = timeSelector::select0(runTime, args); #include "createNamedMesh.H" forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; mesh.readUpdate(); label patchID = mesh.boundaryMesh().findPatchID("liner"); Info<<"\nsurface of liner " << gSum(mesh.magSf().boundaryField()[patchID]) << endl; } Info<< "\nEnd\n" << endl; return 0; }; my problem now is that the results are wrong. They are much smaller than if I calculate the surface myself. I have checked everything I could think of, but haven't found the problem. I have checked the dimension of my cylinder in paraView and there the geometry is correct. Does anyone know what the problem could be? I would appreciate any help. Ca Last edited by will_ca; September 19, 2014 at 06:53. Reason: solved |
|
September 23, 2015, 06:25 |
|
#14 |
Member
Xinguang Wang
Join Date: Feb 2015
Posts: 45
Rep Power: 11 |
Hi Will
Do you know how to access all faces that are parallel to a wall? I am using the code: label cellI = patch.faceCells()[faceI]; to access the cells next to a wall. Jason |
|
August 24, 2016, 08:52 |
|
#15 | |
Member
Peng Liang
Join Date: Mar 2014
Posts: 60
Rep Power: 12 |
Quote:
do you know how to access patch field value for example temperature? Thanks in advance, Peng |
||
November 10, 2019, 10:35 |
A question on how to execute the codes mentioned?
|
#16 |
New Member
Ravi
Join Date: Nov 2019
Posts: 1
Rep Power: 0 |
Dear all,
I am very new to OpenFOAM and sorry for this stupid question. This is my concern here for writing. @jaswi and @shivasub seem to have suggested that we should run a given code or line of codes to be able to get the data required. However, I do not understand how do we execute that code. Any help would be much appreciated? |
|
May 4, 2020, 08:33 |
|
#17 | |
Senior Member
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 366
Rep Power: 8 |
Quote:
you should first start with tutorials on openfoam wiki. things will make sense soon. |
||
October 7, 2020, 11:30 |
|
#18 |
New Member
Tian Jin
Join Date: Aug 2020
Posts: 10
Rep Power: 6 |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
HELP NEEDED HOW TO MAP VALUES FROM PATCH OF ONE MESH TO PATCH OF ANOTHER MESH | mkraposhin | OpenFOAM Running, Solving & CFD | 3 | September 4, 2011 10:42 |
how to access a variable in DPM within a UDF | patrick | FLUENT | 13 | September 15, 2010 09:38 |
Gradients on surfaces or how to find neighbour faces for face on a patch | tehache | OpenFOAM Running, Solving & CFD | 21 | May 25, 2010 08:08 |
How to access the number of faces on a boundary | jam | OpenFOAM Running, Solving & CFD | 1 | January 20, 2008 14:13 |
[Technical] Mapping cell faces to other cell faces | doug | OpenFOAM Meshing & Mesh Conversion | 5 | March 30, 2007 03:43 |