Interpolation in OpenFoam
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 
Yes. Both TVD and NVD are cal
Yes. Both TVD and NVD are calculated the way I described in the original Gamma paper:
@Article{Jasak:GAMMAPAPER, author = {Jasak, H. and Weller, H.G. and Gosman, A.D.}, title = {High resolution NVD differencing scheme for arbitrarily unstructured meshes}, journal = {Int. J. Numer. Meth. Fluids}, year = 1999, volume = 31, pages = {431449} } Here's the code (below). As you can see, it uses the cell gradient and a face gradient (actually a difference across the face). For the cell gradient, you can use whatever you like: Gauss gradient will do. The code implements phict for the NVD and r for TVD. Enjoy, Hrv scalar phict ( const scalar faceFlux, const vector& phiP, const vector& phiN, const tensor& gradcP, const tensor& gradcN, const vector& d ) const { vector gradfV = phiN  phiP; scalar gradf = gradfV & gradfV; scalar gradcf; if (faceFlux > 0) { gradcf = gradfV & (d & gradcP); else { gradcf = gradfV & (d & gradcN); } // Stabilise for division gradcf = stabilise(gradcf, VSMALL); return 1  0.5*gradf/gradcf; } scalar r ( const scalar faceFlux, const vector& phiP, const vector& phiN, const tensor& gradcP, const tensor& gradcN, const vector& d ) const { vector gradfV = phiN  phiP; scalar gradf = gradfV & gradfV; scalar gradcf; if (faceFlux > 0) { gradcf = gradfV & (d & gradcP); } else { gradcf = gradfV & (d & gradcN); } // Stabilise for division gradf = stabilise(gradf, VSMALL); return 2*(gradcf/gradf)  1; } } 
Thanks for the reference Profe
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 
Yes, correct: you interpolate
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 
Thanks Professor Jasak
That
Thanks Professor Jasak
That clears up this issue totally Regards Srinath 
Hi,
I'm testing discretiza
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. http://www.cfdonline.com/OpenFOAM_D...ges/1/9040.jpg 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 abovementioned 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 http://www.cfdonline.com/OpenFOAM_D...ges/1/9041.jpg 
Quote:

All times are GMT 4. The time now is 23:17. 