# Interpolation in OpenFoam

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

 July 27, 2008, 01:51 Interpolation in OpenFoam #1 Member   srinath Join Date: Mar 2009 Location: Champaign, USA Posts: 90 Rep Power: 8 Hello I was reading Hrv's thesis and have a couple of doubts on the interpolation routine in OpenFoam For the NVD schemes, there is an expression on page 109, which gives \phi c \tilda = 1 - (gradphi)f.d/(2*grad phi)c.d And a nice algorithm to give the value of phi on the face, using blended/gamma differencing. But how do we calculate (grad phi)c? Suppose i had rho at cell centers and wanted to obtain a limited value of rho on the surface, what would i do? Should i use a least squared approach to find (grad phi)c? Also i can't seem to find a formulation of TVD using slope limiters on unstructured grids. Could someone please help me on this? Thanks Srinath

 July 30, 2008, 08:08 Thanks for the reference Profe #3 Member   srinath Join Date: Mar 2009 Location: Champaign, USA Posts: 90 Rep Power: 8 Thanks for the reference Professor Jasak, this scheme seems so much better computationally than something like ENO. For the cell gradient, when you say Gauss gradient, do you mean integral(grad (phi)dV) = \sigma dS * phi_face Where dS is the outward pointing Area vector? But in that case how do we get phi_face? Is it ok to use the cell centre averages of the 2 cells sharing that face? Regards Srinath

 July 30, 2008, 10:44 Yes, correct: you interpolate #4 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,758 Rep Power: 21 Yes, correct: you interpolate from the cell centre values. Remember how the scheme says Gauss linear - it is the linear that tells you how to interpolate (=linear interpolation}. You could of course do Gauss harmonic as well, you can guess what that does. Enjoy, Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 July 31, 2008, 02:42 Thanks Professor Jasak That #5 Member   srinath Join Date: Mar 2009 Location: Champaign, USA Posts: 90 Rep Power: 8 Thanks Professor Jasak That clears up this issue totally Regards Srinath

 September 4, 2008, 07:01 Hi, I'm testing discretiza #6 Member   ville vuorinen Join Date: Mar 2009 Posts: 63 Rep Power: 8 Hi, I'm testing discretization schemes for LES and have come up with the following picture on a scalar pulse that is originally: c = 1, when 0.2m < x < 0.7m c = 0, elsewhere and the pulse is advected to the right with velocity 1m/s. The Courant number is 0.1 and time integration is backward. The Gamma scheme is the Gamma01 scheme. A couple of questions about Gamma schemes in OpenFOAM in general: 1) I've noted that the smaller I make the value 0<= psi <= 1, the larger overshoots I make. What is the connection between psi and the parameter beta given in the above-mentioned paper (Jasak et al.)? I seached the code (as given above and related files) but could not find a connection... The paper tells us that typically beta = 0.1 is the lower limit. 2) What is the difference between the GammaV scheme and the Gamma scheme? I can use both for velocity.. So, where does the "V" come into play? Regards, Ville

May 26, 2014, 02:26
#7
Senior Member

Tushar Chourushi
Join Date: Jul 2009
Location: IIT-Indore, India
Posts: 318
Blog Entries: 1
Rep Power: 9
Quote:
 Originally Posted by ville Hi, A couple of questions about Gamma schemes in OpenFOAM in general: 1) I've noted that the smaller I make the value 0<= psi <= 1, the larger overshoots I make. What is the connection between psi and the parameter beta given in the above-mentioned paper (Jasak et al.)? I seached the code (as given above and related files) but could not find a connection... The paper tells us that typically beta = 0.1 is the lower limit. 2) What is the difference between the GammaV scheme and the Gamma scheme? I can use both for velocity.. So, where does the "V" come into play? Regards, Ville