phi = pEqn.flux() vs. linearInterpolate(U) & mesh.Sf()
Hi all FOAMers, I'm wondering why final phi at the end of each timestep in icoFoam is calculated as:
a) Code:
phi = pEqn.flux(); b) Code:
phi=linearInterpolate(U) & mesh.Sf(); I've checked the values of both methods and they are slightly different, maybe with a difference of 1030%. It's interesting that, if you are running continued, phi for the next timestep is calculated like a), but if you stop running and then restart phi for the next timestep then phi is calculated following b). It should be equal? If not, What is correct and why? Why one is used for continued runnings and the other one for restarting? Thx in advance. 
Hi Santiago,
please keep in mind that = means subtraction. So, in step a phi is not completely recalculated, but subtracted with pEqn.flux(); For a complete understanding of the procedure for solving the NavierStokes equation I suggest you read pages 143 till and with 146 of Jasak's thesis: http://powerlab.fsb.hr/ped/kturbo/Op...jeJasakPhD.pdf Cheers, Steven 
I was wondering the same question. In my own experiment the method with linearInterpolate(U)&mesh.Sf() can yields in very erroneous results...
Regards, Cyp 
Quote:
My advisor is implementing icoFoam in MatLab and is assembling phi at the beginning of each timestep by method b), things aren't going well that way. Regards. 
Hi Santiago,
Ok, but why do you think method a) is used in continued running and method b) in restart? If I look in icoFoam I don't see any differences for restarting or not. at line 72: Code:
phi = (fvc::interpolate(U) & mesh.Sf()) Code:
phi = pEqn.flux(); 
Steven, thanks for the interest in the topic. When you restart or start from /0 UEqn is assembled using phi calculated by createFields.H line 43 of icoFoam.C. This is calculated using method b). This phi surfaceScalarField affects the values of H operator, U predictor, etc. used afterwards. In case of continued running UEqn is assembled using phi calculated at the end of previous timestep using method a).
That's the question. Regards. 
Hi Santiago,
Ok, at start method b is used in createFields.H indeed. This is just to get the simulation started. The nonlinearity of the momentum equation is lagged using phi from the previous timestep. But since phi is usually not available at start this is created in createFields.H. But if phi is available (usual in a restart unless you delete phi) phi is read from the timefolder. See line 46 of createFields.H: Code:
IOobject::READ_IF_PRESENT and then: So this is what your advisor should do as well. This set of equations is not easy to understand. Especially if you compare to the original paper of Issa describing the PISO method. Reading the four pages in Jasak's thesis helped me a lot so I really urge you to do the same. Steven 
Aha, it's true, phi is read if it is present, I had forgotten this point, and as you said if you delete this file and approximated phi is assembled to restarting.
Respect of using both methods while running it's true too, but the phi stored for the next time is what was calculated using method a). This method resembles Eqn. 144 from Jasak thesis, which comes from Eqn.140 & Sf. Eqn. 140 is the same of Eqn. 139 but interpolated at faces. Checking the notation is worthy to note that Eqn. 140 is written as: a) U_f=[H(U)/a_P]_f(1/a_P)_f (\nabla p)_f (the last has each factor previously interpolated) and not b) U_f=[H(U)/a_P]_f[(1/a_P) (\nabla p)]_f which one would obtain applying the interpolation the each term of the RHS in Eqn. 129. Checking the code in laplacianScheme.C we have: Code:
00108 return fvmLaplacian(tinterpGammaScheme_().interpolate(gamma)(), vf); phi=U_f & S.f leads to phi=(U_f=[H(U)/a_P]_f[(1/a_P) (\nabla p)]_f)&Sf which uses b) and not a), this explains the differences we've found, but it's not clear for me and my advisor why a) is correct and not b). Regards. 
Quote:
Code:
phi = (fvc::interpolate(U) & mesh.Sf()) Concerning the difference between: [(1/a_P) (\nabla p)]_f and (1/a_P)_f (\nabla p)_f This is the way OpenFoam discretizes a laplacian operator (see equation 3.24 in Jasak): (1/a_P)_f (\nabla p)_f: What about: [(1/a_P) (\nabla p)]_f How would you discretize this? Since now you need [(1/a_P) (\nabla p)]_f. The program would need to use 3.26 of Jasak instead of 3.25 of Jasak. This method is thus not incorrect, but undesirable. Read section 3.3.1.3 of Jasak. 
Quote:
You use pEqn.flux() to obtain the exact term you have to subtract from the matrix of the pEqn, in order not to introduce conservation errors. Best, 
Quote:
(a*b*c)_f = a_f * b_f * c_f This is not true in general, and it holds only for a smooth functional. However it often simplifies the development of the solution procedure. For example, if you take a look at compressible solvers, you find phi = rho_f*U_f while from the theory it should be phi = (rho*U)_f In practice, in many applications, the approximation is acceptable. Best, 
Hi,
Quote:
Code:
00088 if (nonOrth == nNonOrthCorr) phi = {3.4645991399177079e06, 3.4646001127746356e06, 6.3903343759551748e06, 2.9257355721740963e06, ...} and for phi by method b) $62 = {3.531581793505539e06, 4.1013330984044824e06, 5.9540249950781068e06, 3.2691627424804398e06, ...} values are slightly different. I think the answer is was given by Alberto in #10. My advisor pointed me in the necessity of have a look at fluxes conservation. Respect of: Quote:
Quote:
Thanks to you guys, discussion was really useful. 
I have seen the approximation (a*b)_f = a_f*b_f used quite often in Issa papers (I have in mind a paper on multiphase flows (Oliveira & Issa, 2003, Int. J. Num. Meth. Fluids), but also elsewhere), and in extension to the RhieChow formula (S. Zhang, X. Zhao, General formulation for RhieChow Interpolation, ASME Heat Transfer/FLuids Engineering Summer Conference, HTFED0456274, Charlotte, North Carolina, July 1115 2004).
Keep in mind that this assumption is absolutely arbitrary. If you want to be picky, you should not make that assumption, since it introduces an approximation. I have to say it is a very convenient approximation however, and I have used it myself in multiphase codes for a simple reason. Just consider the case where you have a phase fraction 0 < alpha < 1, and you define phi = (alpha*rho*U)_f In this case, if you use a reconstruction procedure when correcting the velocity, you must divide by alpha_f*rho_f. This forces you to do something (typically not very clean) when alpha is small. If you define phi as the velocity flux: phi = (U)_f and then consider alpha_f*rho_f*(U)_f where you need it, like in the pressure equation, your correction step is clean, and does not have any problem when alpha tends to zero. Of course if your fields are strongly nonuniforms (shocks), you need the first approach, but in incompressible solvers or slightly compressible ones, you probably won't see a significant difference. Finally, b) does not enforce the conservation principle because you do not enforce it on U exactly, but on phi. Your pressure equation is div(phi) = div(U_f) = 0 not div(U_c) = 0 being U_c the cellcentered velocity. For the same reason, in transport equations you use div(phi, T). Best, 
Excellent!!

variable porosity
Hi
I, simulating flow in a channel with variable porosity. so I need to change some thing in correction of flux. it means I have to multiply porosity to pressure. the flux in updated by pEqn.flux() could anyone let me know how I can use porosity*pressure instead of pressure in correction of flux? 
Hello,
I also had the problem about the pEqn.flux(). In these equations in your post, is pEqn.flux() returns the value [(1/a_P) (\nabla p)]_f&Sf? In rhoPimpleFoam, there are two regimes for pressure: transonic and subsonic. In Transonic, the correcpsonding flux correction is: phi == pEqn.flux() while in subsonic regime, it is as follows phi +=pEqn.flux So from the above the sign is opposite. How can we justify this difference? I also check other solvers and found that some use "==" while some use "+=" . Does anybody know something about this? Thanks. Quote:

Hi
I have this problem, too. this function (pEqn.flux() ) works based on which relation in jasak's thesis? thanks 
Hi!
You can find in the following link a presentation I made regarding the details of icoFoam. I sure you will find all your answers there. http://www.scribd.com/doc/143414962/...oninOpenFOAM The slides are in French, but you could easily understand the mathematical and programming part ;) Enjoy! Cyp 
Quote:
But there is no any note about pEqn.flux() overthere. I know this module return a surfaceScalarField type that must be subtracted form phi. But I don't Know Why? phi = pEqn.flux(); 
Hello,
Quote:
I think some time ago there was some explanation regarding this topic, but lets do it from the top. A nice explanation of the way NS is solved in OpenFOAM is presented in the OFwiki about SIMPLE algo: http://openfoamwiki.net/index.php/Th...hm_in_OpenFOAM PISO algo is very similar: http://openfoamwiki.net/index.php/Th...hm_in_OpenFOAM Of course check also subtopics. Now for some notes. As we all know, OF uses Eulerial approach with nonstaggered meshes. This can introduce some significant numerical errors (especially while using 2nd order central difference schemes). For that reason in OF we "do not" solve directly for velocity (U), but for the fluxes (phi). If you check the divergence of U, you will almost always find that there is a notnegligible error. At the same time phi is guaranteed to be divergence free. Now lets take a look into the PISO algo itself. I will not cite the code but it should be easy to follow. 1) create the UEqn using the last known phi. Note that any "XEqn" is like a black box, with a void space for the unknown. The imporatant stuff are the coeffs. 2) if you like, solve momentum predictor (this is unnecessary and can be dropped for time saving). 3) extract the semicentral coeffs from the UEqn, reverse them and call rAU. This is the famous "operator splitting". 4) pressure loop: 4.1) recalculate velocity: U = rAU * H(); 4.2) recalculate fluxes: phi = interpolate(U) * S; note that the flux field is NOT divergence free; 4.3) solve for pressure using the non divergence free flux 4.4) solve it several times... 5) now, we solved for pressure with nondivfree phi. But the literature (Jasak's thesis, Issa et al.) tells us, that we can correct the fluxes using the pressure field and this way ensure divfree condition. This is the famous phi = pEqn.flux(); 6) Finally, we correct the velocity field, acquiring a good approximation of the velocity field. Note that the solution are the three fields: U, p and phi. And the imporatant one is in fact phi not U. Hope I managed to clear the things a bit. Best, Pawel 
All times are GMT 4. The time now is 01:07. 