Hi all,
I'd like to know mo
Hi all,
I'd like to know more about DdtPhicorr term. I have not clear in mind the theoretical derivation of this operator. It's similar to RhieChow interpolation for Colocated variable arrangement?! Moreover, it's possible to use it in steady simulations?! Thanks in advance Luca 
This term accounts for the div
This term accounts for the divergence of the face velocity field by taking out the difference between the interpolated velocity and the flux. Have a look at:
finiteVolume/ddtSchemes/EulerDdtScheme/EulerDdtScheme.C in the main library: rDeltaT*fvcDdtPhiCoeff(U.oldTime(), phi.oldTime())* ( fvc::interpolate(rA)*phi.oldTime()  (fvc::interpolate(rA*U.oldTime()) & mesh().Sf()) ) Unfortunately, I don't think there's anything written about it. Enjoy, Hrv 
Does this add more numeric dis
Does this add more numeric dissipation to the scheme?
What should I expect if I remove this from the oodles main code? Can I live without it? Or what were you guys trying to achieve when you come up with this? (I m running incompr LES) Thanks a lot! luiz 
Hello everyone,
I detected so
Hello everyone,
I detected some inconsistency, while experimenting with the term "fvcDdtPhiCoeff" in "ddtPhiCorr". Probing the pressure signal of a LES yielded different results depending on using the present calculation of "fvcDdtPhiCoeff" or using a constant value, as was done in FOAM version 1.1. If I use the present version the signal looks a bit wavy (f~1/deltaT) with small amplitude. If I use a constant value then the signal looks smoother. I´m not sure, if it is numerical noise in the one case or a wrongly smoothed signal in the other case. Can anyone give me a hint? Thanks in advance Rolando 
ddtPhiCorr meaning
Could you explane me why in turbDyMFoam (OF 1.5dev) I have:
phi = (fvc::interpolate(U) & mesh.Sf()); //+ fvc::ddtPhiCorr(rUA, U, phi); Can you explane me better the meaning of ddtPhiCorr term? why in some solvers is commented and in other (es. pisoFoam) is not? thanks Aldo 
Quote:
phi = (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rAU, U, phi); In lid driven cavity and turbulent channel flow (DNS) this calculation of phi works very well. However, for a laminar, inviscid TaylorGreen vortex the term + fvc::ddtPhiCorr(rAU, U, phi); turned out to dissipate kinetic energy very strongly. On fine grids about 10% of the initial energy within a few eddy turnaround times. When I removed the + fvc::ddtPhiCorr(rAU, U, phi) term things seemed to work much better. My solution: RungeKutta 4 and the projection method  I implemented the solver. I would very much appreciate comments regarding the necessity of + fvc::ddtPhiCorr(rAU, U, phi) in PISO! Best, Ville 
I have been investigating this issue too.
I think ddtPhiCorr is approximately equal to : UfaceOld*Area  phiOld, (if we assume that this difference is close to zero, for the simplest case). You can look at this link which sums it up : http://www.scribd.com/doc/48195039/ddtPhiCorr So why would we need to carry this difference in the computation of phi ? My guess is that in the piso algortihm you correct for the non orthogonalities and do not have phi = Uface*Surface anymore after the correction. Forcing phi to be equal to this on the next iteration would be a bit silly so you want to keep that correction. This is the ddtPhiCorr. Thus it should not appear where no correction that we want to keep is done. However this doesn't explain why Ville found an excessive dissipation of kinetic energy when ddtPhiCorr is there. Could you give more details about how you figure this out ? During your simulation did you correct non orthogonalities ? Was your grid non orthogonal ? Regards, 
Hello everyone ,
I am new to OpenFOAM , and I am working on a melting problem , but I can understand the following code Quote:
Thanks Zhipeng 
Quote:
I think you may read through this to have some basic idea. http://openfoamwiki.net/index.php/Op...hm_in_OpenFOAM and also go through how governing equations(especially pressure equation, in OF, we solve "real pressure equation" instead of "pressure correction equation") discretization is realized in jasak's PhD theis. http://www.h.jasak.dial.pipex.com/ for the buoyancy approximation, you may read through any material found online. Best., 
Hi,
in this paper some OpenFOAM related matters are discussed including syntax. Also the adhoc ddtPhiCorr term is discussed from effect point of view although its origin remains unclear. I noted that the extra term has actually been removed in some newer solvers. On the implementation of lowdissipative Runge–Kutta projection methods for time dependent flows using OpenFOAM®, Computers & Fluids, Volume 93, 10 April 2014, Pages 153163, V. Vuorinen, J.P. Keskinen, C. Duwig, B.J. Boersma 
ddtPhiCorr is a form of Choi correction and was originally intended to remove time step size dependency from RhieChow interpolation.
http://nht.xjtu.edu.cn/paper/en/2002206.pdf In FOAM there is however an additional adhoc component fvcDdtPhiCoeff that appears to be purely empirical in nature. The Choi correction is dissipative in nature, but it is consistent. There appears to be an issue with the FOAM implementation in that setting fvcDdtPhiCoeff to 1 (full Choi correction) results in instabilities. So it might very well be the case that the implementation is flawed in some way. Investigations are ongoing. 
Quote:
Thank you very much for answer. 
Since this thread dates back to previous version of OF, which one do we talk about, since in the bugreport someone has pointed out the Uf to be an issue and DPhiDtCorr involves this variable? I am not an expert on this subject so I am looking forward the outcome of this "investigation".

Dear All,
I am also confused with the additional term "fvc::ddtPhiCorr(rUA, U, phi)" for the phi formulation. Did anyone dig into it? What is the actual significance of it?  Best Regards! 
It is an ad hoc term which is probably added to stabilize some certain flow situations.
Sometimes it does not matter, sometimes it has a strong effect. There are more questions than answers but please see On the implementation of lowdissipative Runge–Kutta projection methods for time dependent flows using OpenFOAM®, Computers & Fluids, Volume 93, 10 April 2014, Pages 153163, V. Vuorinen, J.P. Keskinen, C. Duwig, B.J. Boersma where we demonstrated what happens if it is there and what if it is not. Best,Ville 
Quote:
 Best Regards! 
All times are GMT 4. The time now is 06:58. 