CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

Suggested unsteady, implicit solver stable with arbitrarily large time steps

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

Like Tree6Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 12, 2010, 10:11
Default
  #41
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   September 15, 2010, 11:26
Default
  #42
New Member
 
Join Date: Sep 2010
Posts: 3
Rep Power: 6
CpCaniggia is on a distinguished road
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 sub-iterations 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.
CpCaniggia is offline   Reply With Quote

Old   September 19, 2010, 15:51
Default ... use coefficients without relaxation!
  #43
Member
 
djbungee's Avatar
 
Ulf Bunge
Join Date: Mar 2009
Location: Wolfsburg, Germany
Posts: 34
Rep Power: 8
djbungee is on a distinguished road
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: Suggested unsteady, implicit solver stable with arbitrarily large time steps. 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.
djbungee is offline   Reply With Quote

Old   September 19, 2010, 18:01
Default
  #44
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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 Rhie-Chow interpolation formula.

For example, following Zhang and Zhao (Proceedings of HT-FED04, 2004 ASME Heat Transfer/Fluid Engineering Summer Conference, July 11-15, 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) + (1-f)*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) + (1-URF)*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 + (1-URF)*(u0_(i+1/2) - u0#_(i+1/2))

with

u#_(i+1/2) = f*u_(i+1) + (1-f)*u_i

u0#_(i+1/2) = f*u0_(i+1) + (1-f)*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 Rhie-Chow 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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 1, 2013, 22:32
Default
  #45
New Member
 
Hansjoerg Seybold
Join Date: Mar 2009
Posts: 16
Rep Power: 8
hansjoerg is on a distinguished road
Hi,
I enjoyed reading this discussion and I'd like to ask if there is any final conclusion
on the implementation?
hansjoerg is offline   Reply With Quote

Old   March 23, 2015, 05:14
Default
  #46
Senior Member
 
M. Montero
Join Date: Mar 2009
Location: Madrid
Posts: 110
Rep Power: 8
be_inspired is on a distinguished road
I am also interested in this topic.
How to deal with extremely high CFL using pimpleDyMFoam?
be_inspired is offline   Reply With Quote

Reply

Tags
implicit, pimple, relaxation, simple, unsteady

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Implicit versus Explicit Deepak Main CFD Forum 16 November 29, 2014 21:54
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 Ström FLUENT 1 October 29, 2005 03:57


All times are GMT -4. The time now is 05:37.