# non zero divergence for incompressible flow!

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

 June 17, 2010, 16:16 non zero divergence for incompressible flow! #1 Member   Pascal Join Date: Jun 2009 Location: Montreal Posts: 65 Rep Power: 10 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 time-step (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 open-source implementation of quadrature-based 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: 10 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:
 Originally Posted by Pascal_doran 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?
It is a question of consistency with how you discretise and solve the equations.

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 semi-discretize the momentum equation as

so that

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 semi-discrete 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:
 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 ...)
Very small. Take a look at icoFoam tutorials for the cavity case, which return something like:

time step continuity errors : sum local = 8.06059e-09, global = 9.28097e-19, cumulative = 9.00754e-18

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 open-source implementation of quadrature-based 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: 10 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 Navier-Stokes 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 open-source implementation of quadrature-based 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: 10 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 Here the main part of my code: 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) ); } Thank you, 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 open-source implementation of quadrature-based 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: 10 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 open-source implementation of quadrature-based 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: 10 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 open-source implementation of quadrature-based 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:
 Originally Posted by Pascal_doran 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
Hi Pascal,

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 non-orthogonal cells you may find jumps at element boundaries, as discussed in Tomboulides and Orszag (JFM, 2000, 416:45-73), 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: 10 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 Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post violet FLUENT 8 February 16, 2016 06:32 CD adapco Group Marketing Siemens 3 June 21, 2011 08:33 xiaofish FLUENT 0 September 9, 2007 22:53 ib FLUENT 1 March 26, 2007 13:11 pxyz Main CFD Forum 37 July 7, 2006 08:42

All times are GMT -4. The time now is 09:06.