CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

Evaluate phi from a areaVectorField

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2010, 18:10
Default Evaluate phi from a areaVectorField
  #1
New Member
 
Diego Villa
Join Date: Mar 2010
Location: Genova Italy
Posts: 28
Rep Power: 7
DiegoNaval is on a distinguished road
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
DiegoNaval is offline   Reply With Quote

Old   December 3, 2010, 05:11
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,620
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Diego

I suspect you would like to compute the edgeScalarField such as:

edgeScalarField phiS = linearEdgeInterpolate(Us) & aMesh.Le();

Best regards,

Niels
ngj is offline   Reply With Quote

Old   December 3, 2010, 11:09
Default
  #3
New Member
 
Diego Villa
Join Date: Mar 2010
Location: Genova Italy
Posts: 28
Rep Power: 7
DiegoNaval is on a distinguished road
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
DiegoNaval is offline   Reply With Quote

Old   December 7, 2010, 06:15
Default
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,620
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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)},
}
ngj is offline   Reply With Quote

Old   December 7, 2010, 11:23
Default
  #5
New Member
 
Diego Villa
Join Date: Mar 2010
Location: Genova Italy
Posts: 28
Rep Power: 7
DiegoNaval is on a distinguished road
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
DiegoNaval is offline   Reply With Quote

Old   December 8, 2010, 06:11
Default
  #6
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,620
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is offline   Reply With Quote

Old   February 11, 2015, 14:03
Default Correcting phiS
  #7
New Member
 
frederik stoll
Join Date: Aug 2014
Location: Hannover
Posts: 3
Rep Power: 3
frederik is on a distinguished road
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
frederik is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
read scalar field phi, get flux through faces peterwy OpenFOAM Programming & Development 4 August 4, 2010 16:36
Turbulence Model phi vs phi_ doug OpenFOAM Running, Solving & CFD 4 November 10, 2009 05:33
Another phi question ehsan_vaghefi OpenFOAM Running, Solving & CFD 0 October 24, 2008 19:56
About phi in icoFoam kar OpenFOAM Running, Solving & CFD 3 February 20, 2008 06:20
Processing PHI A Mitt Phoenics 1 August 8, 2002 07:29


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