
[Sponsors] 
June 17, 2010, 16:16 
non zero divergence for incompressible flow!

#1 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
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 

June 18, 2010, 08:06 

#2 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 10 
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... 

June 18, 2010, 10:36 

#3 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
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,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 18, 2010, 18:46 

#4 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
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 

June 18, 2010, 19:16 

#5  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
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,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 18, 2010, 19:52 

#6 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
Thank you Alberto!
I really appreciate the short and long answer! It really helps me. Regards, Pascal 

June 18, 2010, 23:00 

#7 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 10 
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?


June 19, 2010, 11:00 

#8 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 95
Rep Power: 10 
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? 

June 19, 2010, 21:42 

#9 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 10 
Thanks Patricio, I forgot about the way it's calculating div in the discrete space.


June 20, 2010, 15:31 

#10 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Maybe we should put this in the wiki FAQ
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 20, 2010, 16:17 

#11 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
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&)’ make: *** [Make/linux64GccDPOpt/zVorticityPhi.o] Error 1 Code:
IOobject phiheader ( "phi", runTime.timeName(), mesh, IOobject::MUST_READ ); if (phiheader.headerOk()) { Info<< " Lecture de phi" << endl; surfaceScalarField phi(phiheader, mesh); // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< " Calcul de vorticity" << endl; volVectorField vorticity ( IOobject ( "vorticity", runTime.timeName(), mesh, IOobject::NO_READ ), fvc::curl(phi) ); } Pascal 

September 20, 2010, 16:38 

#12 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hello, phi is a scalarField, so curl(phi) is not defined. You have to use a vectorField to compute the curl.
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 20, 2010, 17:18 

#13 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
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 

September 20, 2010, 17:23 

#14 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
What do you use the vorticity for?
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 20, 2010, 17:27 

#15 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
I use the vorticity for tracking the position of wake vortices and for stability analysis.


September 20, 2010, 17:36 

#16 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
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,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 21, 2010, 05:09 

#17  
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 95
Rep Power: 10 
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 

September 21, 2010, 10:22 

#18 
Member
Pascal
Join Date: Jun 2009
Location: Montreal
Posts: 65
Rep Power: 9 
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 

Tags 
incompressible divergence 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
multiphase flow, quick divergence of contuinity eq  violet  FLUENT  8  February 16, 2016 06:32 
Flow meter Design  CD adapco Group Marketing  CDadapco  3  June 21, 2011 08:33 
flow past a missle: how to solve divergence?  xiaofish  FLUENT  0  September 9, 2007 22:53 
reversed flow at velocity inlet / mass flow inlet  ib  FLUENT  1  March 26, 2007 13:11 
transform navierstokes eq. to eulereq.  pxyz  Main CFD Forum  37  July 7, 2006 08:42 