# Evaluate phi from a areaVectorField

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

 December 2, 2010, 18:10 Evaluate phi from a areaVectorField #1 New Member   Diego Villa Join Date: Mar 2010 Location: Genova Italy Posts: 28 Rep Power: 7 Hi all, I'm using OF1.5-dev to use the Finite Area Method. I have evaluate from the Volume velocity U the areaVectorField Us though a volSurfaceMapping vsm(aMesh), in the following way: Us.internalField() = vsm.mapToSurface(U.boundaryField()); Now I need to find the phi from the Us How I can do that? Thank to everybody Diego

 December 3, 2010, 05:11 #2 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,620 Rep Power: 25 Hi Diego I suspect you would like to compute the edgeScalarField such as: edgeScalarField phiS = linearEdgeInterpolate(Us) & aMesh.Le(); Best regards, Niels

 December 3, 2010, 11:09 #3 New Member   Diego Villa Join Date: Mar 2010 Location: Genova Italy Posts: 28 Rep Power: 7 Yes exactly. Thank youvery much Niels An other question, how does the code compute the Le() function? I don't find the code, is it a vector orthogonal to the edge and contained in the mean plan of the surface mesh evaluate for each edge? Sorry for the confuse question, but I hope you understand. But I need to understand witch vector Le() gives! Diego

 December 7, 2010, 06:15 #4 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,620 Rep Power: 25 Hi Diego Yes, I understand what you mean. The edge normal is normal to the edge and is tangential to the the curved surface. The computation of the normal is found in ~/OpenFOAM/OpenFOAM-1.5-dev/src/finiteArea/faMesh/faMeshDemandDrivenData.C in the function void faMesh::calcLe() const The documentation on the FAM method is rather scarce, however there exist a Ph.D. thesis (in Croatian) [1], however the figures are neat and rather self-explanatory. Look for chapter 5, pp. 137-156. I have also given the bib-file as I understand it to be written, if any comments on that, please do not hesitate to correct me. Best regards, Niels [1]: http://powerlab.fsb.hr/ped/kturbo/Op...vicPhD2005.pdf [Bib]: Code: ```@phdthesis{tukovic2005, Author = {Tukovi\'{c}, {\v{Z}}}, Title = {{Metoda Kontrolnih Volumena Na Domenama Promjenjivog Oblika (Finite Volume Method on Domains of Variable Shape)}}, School = {University of Zagreb}, Year = {2005}, Note = {(In Croatian)}, }```

 December 7, 2010, 11:23 #5 New Member   Diego Villa Join Date: Mar 2010 Location: Genova Italy Posts: 28 Rep Power: 7 Thank you very much, I have a lot of problem with the Croatian language but I have understand the meaning. An other problem. I have create a mesh with Star and I have convert it with ccm26ToFoam. All seams good, if I use a normal fvSolver the solution have no problem. But in some case, not always if I change some parameters that change very few the mesh generated, the faSolver don't works. I particular I have an Floating point exception on all the part that use the something about the surface mesh. For example when I compute the edge phi for the areaVelocity and use: edgeScalarField phiS = linearEdgeInterpolate(Us) & aMesh.Le(); In the run I have the error. Have you any idea on which could be the problem? Diego

 December 8, 2010, 06:11 #6 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,620 Rep Power: 25 I have not had any problems using faMesh, but if I have changed the mesh and have forgotten to do makeFaMesh, I receive a run-time error. It is the only explanation I can think of. Best regards and good luck Niels

 February 11, 2015, 14:03 Correcting phiS #7 New Member   frederik stoll Join Date: Aug 2014 Location: Hannover Posts: 3 Rep Power: 3 Dear Fomers, i do also want to solve the Exner-equation. Since i obtain some spirious oscillations i want to smooth the flux phiS. Therefore i will use a additional diffusion term which is dependant on the cells slope. (see the following paper:FORTUNATO, A.B. and OLIVEIRA, A., 2007. Improving the Stability of a Morphodynamic Modeling System. Journal of Coastal Research, SI 50 (Proceedings of the 9th International Coastal Symposium), 486 – 490. Gold Coast, Australia, ISSN 0749.0208) I want to implement a loop over all edges. To clarify which two cells are owner and neighbour of which edge. All i need is the name of the List, where the edges are stored. I hope you can get my point. Something like an edgeList, Best regards frederik

 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 peterwy OpenFOAM Programming & Development 4 August 4, 2010 16:36 doug OpenFOAM Running, Solving & CFD 4 November 10, 2009 05:33 ehsan_vaghefi OpenFOAM Running, Solving & CFD 0 October 24, 2008 19:56 kar OpenFOAM Running, Solving & CFD 3 February 20, 2008 06:20 A Mitt Phoenics 1 August 8, 2002 07:29

All times are GMT -4. The time now is 13:33.