# surface and volume fields multiplication

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 2, 2011, 20:10 surface and volume fields multiplication #1 New Member   Ivan Join Date: Sep 2010 Location: Russia , Moscow. Posts: 14 Rep Power: 9 Greetings ! I have two fields: volVectorField X and surfaceScalarField M. Is there any method to multiply them to get volume field on new time step like that : X(n+1,i) = X(n,i-1)*M(n,1-1/2)-X(n,i+1)*M(n,i+1/2) there n timestep index and i index of a cell. i+1/2 - right face of a cell i-1/2 - left face. I assumed that this will look like interpolate(interpolate(X)*M) with upwind interpolation schemes, but as i know there is no method for interpolating face field onto cell volumes. Is there any way to make such construction in solver ? Best regards !

 March 7, 2011, 13:10 #2 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Something along these lines should do the trick. You're going to have to sort out the the discretization and mathematical correctness of it all. Since the mesh is unstructured you'll probably need to use the face normal vector or something to get the direction. Also take a look at finiteVolume/finiteVolume/fvc/fvcReconstruct.C, which does something similar. Code: ``` vectorField& Xi = X.internalField(); const vectorField& X0i = X.oldTime().internalField(); const scalarField& M0i = M.oldTime().internalField(); const unallocLabelList& owner = mesh.owner(); const unallocLabelList& neighbour = mesh.neighbour(); Xi = vector::zero; forAll(owner, faceI) { label P = owner[faceI]; label N = neighbour[faceI]; // You're gonna have to sort out the sign issue here // This will probably need the face normal Xi[P] += X0i[N]*M0i[faceI]; Xi[N] -= X0i[P]*M0i[faceI]; } forAll(mesh.boundaryMesh(), patchI) { fvPatchVectorField& pf = X.boundaryField()[patchI]; const fvPatchVectorField& pf0 = X.oldTime().boundaryField()[patchI]; const fvsPatchScalarField& psf = M.oldTime().boundaryField()[patchI]; const unallocLabelList& faceCells = mesh.boundaryMesh()[patchI].faceCells(); if (pf.coupled()) { // I'm going to leave this one up to you } else { forAll(pf, faceI) { Xi[faceCells[faceI]] += pf0[faceI]*psf[faceI]; } } } X.correctBoundaryConditions();``` Last edited by cliffoi; March 7, 2011 at 13:21. Reason: Forgot the boundaries

 March 7, 2011, 13:25 #3 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 This might be a much simpler alternative. Again, you need to sort out the discretization and mathematical correctness. X = fvc::surfaceSum(fvc::interpolate(X.oldTime())*M.ol dTime())

 March 7, 2011, 18:44 #4 New Member   Ivan Join Date: Sep 2010 Location: Russia , Moscow. Posts: 14 Rep Power: 9 Hi Ivor , thank you very much for your reply ! It was really helpful for me. I'm trying to add some another algorithms in OpenFoam like FLIC or Big particles method, but there is a very little information about classes and methods in OpenFoam and tutorials for their usage, except Doxygen documentation. Construction proposed by you in your second post looks to be that i need. I used it for coding 3rd step in FLIC method and solver is compiling well now. I will try to solve some test cases and work out correctness issue. Best regards !

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mjoelnir Open Source Meshers: Gmsh, Netgen, CGNS, ... 8 March 30, 2017 08:52 velan Open Source Meshers: Gmsh, Netgen, CGNS, ... 3 October 22, 2015 11:05 nishant_hull Open Source Meshers: Gmsh, Netgen, CGNS, ... 23 August 5, 2015 02:09 ouafa Open Source Meshers: Gmsh, Netgen, CGNS, ... 7 May 21, 2010 12:43 t42 OpenFOAM Meshing & Mesh Conversion 6 July 10, 2008 07:51

All times are GMT -4. The time now is 14:51.