non zero divergence for incompressible flow!
Hi all,
I'm simulating wake vortices in ground effect. I use icoFoam (incompressible) solver. But when I compute the divergence of U, I find non zero divergence (~0.5 to 0.5). I compute the divergence with : foamCalc div U and my own utility (using Gauss linear scheme). Both way I got the same results (with a difference less then 1%). Can somebody explain me why I have such high divergence (I'm not expecting to have div(U) = 0 but more like div(U) ~= 0.01) Thank you, Pascal 
Hey Pascal,
Have you checked for convergence at each timestep (like looking at the initial residuals)? Maybe you need to increase your nCorr (number of PISO corrector steps)? Just guessing... 
You must check div(phi), using the phi coming out from the pressure equation, not div(U).
Actually the code does that for you when it prints the local and global continuity error. Search for the file continuityErrs.H to check. Best, 
Thank you for your help
But can you explain me why it is better to check div(phi) than to check div(U) both should be near zero? And by the way what is a good value for div(U) and div(phi) for an incompressible flow (I know that in theory it should be div(U) = 0 ...) Pascal 
Hi Pascal,
Quote:
Short answer: you impose div(phi) = 0, meaning div(U_f) = 0, being U_f the velocity on the cell faces, not div(U) = 0, being U the velocity in cell centers. Long answer: If you go through the derivation, you can think to semidiscretize the momentum equation as A*U = H  grad(p)/rho so that U = (H/A)  grad(p)/(A*rho) At this point you use the continuity equation div(phi) = div(Uf) = 0 The continuity equation tells you the divergence of the flux is zero, and the flux is computed at cell faces, not at cell centres. By interpolating the predicted U, obtained from the semidiscrete momentum equation, you get (S is the surface area vector, and S its norm) phi = Uf = (H/A)_f  snGrad(p)/(rho*A)_f S and, replacing this in the continuity equation div((H/A)_f)  laplacian(1/(rho*A)_f S, p) = 0 Note that in OpenFOAM phi is computed as phi = fvc::interpolate(U) + ddtPhiCorr(rUA, U, phi) where U = H/A, and rUA = 1/A. The term ddtPhiCorr originates from the collocated grid arrangement. Quote:
time step continuity errors : sum local = 8.06059e09, global = 9.28097e19, cumulative = 9.00754e18 Best, 
Thank you Alberto!
I really appreciate the short and long answer! It really helps me. Regards, Pascal 
But U_f and U should the same velocity distributions (or almost since U_f is just the interpolated U at cell surfaces) so why should the divergence be different for each of them?

Hi Pavan:
icoFoam solves for the integral form of NavierStokes equations. Therefore, you should compute the mass imbalance (in the computational cell) as the integral of div(U) in the cell volume V_P. Subsequently, you should apply Gauss theorem to transform the volumetric integral of div(U) as the sum of phi on the face. Do you know what does div(phi) mean? 
Thanks Patricio, I forgot about the way it's calculating div in the discrete space.

Maybe we should put this in the wiki FAQ :D

Hi Alberto,
Do you have an idea how to compute the vorticity based on the flux phi like this : curl(phi) When I tried to compiled I got this error message : Code:
zVorticityPhi.C:82: error: no matching function for call to ‘curl(Foam::surfaceScalarField&)’ Code:
IOobject phiheader Pascal 
Hello, phi is a scalarField, so curl(phi) is not defined. You have to use a vectorField to compute the curl.
Best, 
Thanks for your reply,
So are you saying that I can't compute vorticity directly from the flux? Because phi must be a surfaceScalar and the vorticity must a volVector. What are you suggesting me to do since div(phi) is more accurate than div(U) I guess that curl based on phi would be more accurate than the curl based on U? What do you think? Pascal 
What do you use the vorticity for?

I use the vorticity for tracking the position of wake vortices and for stability analysis.

What I said is phi is a scalar quantity (it is the U_f \cdot surface), while the curl operation is only defined for vectors.
The U in cell centres, which is what you visualize in paraview is not "inaccurate". It does not satisfy the continuity equation strictly, since the continuity constraint is applied to the flux. Best, 
Quote:
that is a good question. But how can you relate phi with curl(U)? May be I am wrong, but I think that Gauss theorem cannot be applied to curl operator in order to express a volume integral as surface integrals. So I have difficulties to figure out a way of implementing a "conservative" discretization of curl. I think that it is usually treated as a source term. To visualize vortex shedding you can just employ the "vorticity" command implemented by default in OF, and select the component to visualize in paraView. In the presence of nonorthogonal cells you may find jumps at element boundaries, as discussed in Tomboulides and Orszag (JFM, 2000, 416:4573), so take care of them. I will post a nice picture showing vortex sheding in the near future. Best wishes, Patricio 
Hi Patricio,
I think you're totally right. I was just wondering what was the most efficient way to compute the vorticity. In my case the mesh is orthogonal :) so I will keep using the vorticity utility. Thanks Pascal 
All times are GMT 4. The time now is 02:30. 