
[Sponsors] 
Suggested unsteady, implicit solver stable with arbitrarily large time steps 

LinkBack  Thread Tools  Display Modes 
May 12, 2010, 10:11 

#41 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27 
Is the Courant number actually 10000, or is this the value you read by OpenFOAM? If so, are you using an unstructured grid? Does the mesh pass checkMesh (skewness?)?
If you use Euler or CN schemes, you're already using an implicit scheme. 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 15, 2010, 11:26 

#42 
New Member
Join Date: Sep 2010
Posts: 3
Rep Power: 8 
Dear all,
I am very interested in this topic. Actually, I also met the same problem in my unsteady computation. My unsteady computation is unstable if I don't use a relaxation factor. To my point of view, it is not correct to use relaxation factor in an unsteady simulation. In OpenFoam, the momentum equations are probably (I didn't read the code very deeply) solved by A . U = H  grad (p) + rhok . g  (Predictor) I printed the A values at different relaxation factor and they are different. That means the equation you solve becomes A' . U = H  grad (p) + rhok . g + R(f)  (Predictor) where R(f) is related to relaxation factor. These A values are also used in pressure correction step. So the solutions will be different no matter how many subiterations you use in the pressure correction step. The equation becomes more explicit with increasing relaxation factor. I think the solution will be the same only when the time step is small enough. Best regards, Y. J. 

September 19, 2010, 15:51 
... use coefficients without relaxation!

#43 
Member
Ulf Bunge
Join Date: Mar 2009
Location: Wolfsburg, Germany
Posts: 34
Rep Power: 9 
Hi,
thanks for you post and you are right. That is the reason why I suggested to use coefficients without relaxation for the pressure equation in post #26 in this thread you are reading here: http://www.cfdonline.com/Forums/ope...tml#post247123. You have to do that in order to achieve an unsteady, implicit solver stable with arbitrarily large time steps as my thread title implies. However, on reaching convergence, this does not play a role, at least if you do not omit some parts of the coefficients. So, your "problem" is already solved. Best regards, Ulf. 

September 19, 2010, 18:01 

#44 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27 
Hello,
elegant solutions to this problem have been published (literature search helps ), which do not rely on modifications of the iterative procedure (they are not related to it, so why should you change that?), but simply fix the problem at its root, the RhieChow interpolation formula. For example, following Zhang and Zhao (Proceedings of HTFED04, 2004 ASME Heat Transfer/Fluid Engineering Summer Conference, July 1115, 2004, Charlotte, North Carolina, USA), you can write (for what possible on a forum ) the face velocity as: u_(i+1/2) = H + B_(i+1/2) DeltaP where H = f*H_(i+1) + (1f)*H_i and f the interpolation factor. At this point, you can think to apply relaxation as follows: u_(i+1/2) = URF*(H + B_(i+1/2) * DeltaP) + (1URF)*U0_(i+1/2) with U0_(i+1/2) value of U_(i+1/2) at the previous iteration. Now, with some algebra, substituting the definition of H, you find u_(i+1/2) = u#_(i+1/2) + URF*DeltaX*B_(i+1/2)*DeltaP + (1URF)*(u0_(i+1/2)  u0#_(i+1/2)) with u#_(i+1/2) = f*u_(i+1) + (1f)*u_i u0#_(i+1/2) = f*u0_(i+1) + (1f)*u0_i which ensures the face velocity converges to the correct value, independently from the applied relaxation. P.S. The dependency on URF is not related to the time step. It is always there, if you use the standard RhieChow formula. Such a formula introduces also a dependency on time step, and the same paper cited above shows how to deal with it (and some treatment should be implemented in ddtPhiCorr, if my understanding is correct). 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. 

May 1, 2013, 22:32 

#45 
New Member
Hansjoerg Seybold
Join Date: Mar 2009
Posts: 16
Rep Power: 9 
Hi,
I enjoyed reading this discussion and I'd like to ask if there is any final conclusion on the implementation? 

March 23, 2015, 05:14 

#46 
Senior Member
M. Montero
Join Date: Mar 2009
Location: Madrid
Posts: 122
Rep Power: 9 
I am also interested in this topic.
How to deal with extremely high CFL using pimpleDyMFoam? 

Tags 
implicit, pimple, relaxation, simple, unsteady 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Implicit versus Explicit  Deepak  Main CFD Forum  17  November 7, 2015 14:14 
Working directory via command line  Luiz  CFX  4  March 6, 2011 21:02 
Doubt on Implicit Methods  analyse In India  Main CFD Forum  10  March 9, 2007 04:01 
Time scales and Fluent's unsteady solver issue  Freeman  FLUENT  6  December 13, 2005 15:30 
Convergence with coupled implicit solver  Henrik StrĂ¶m  FLUENT  1  October 29, 2005 03:57 