CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Question on transient simulation in OpenFOAM and FLUENT

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2014, 23:13
Question Question on transient simulation in OpenFOAM and FLUENT
  #1
New Member
 
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 3
nicklj is on a distinguished road
Dear all:
Recently I'm trying to use OpenFOAM to simulate transient incompressible flow, and have some questions to inquire.

I know that in FLUENT, for transient flow, iterations are required within each time step, to confirm the result can converge at the end of the current time step. The default value is 20, which means if the result cannot converge within 20 iterations, the solver will march into next time step. This is normally how the transient solver works in my mind.

However, when perform transient simulation in OpenFOAM, using either PISO or PIMPLE, it seems that no iteration is required within one time step (Of course iterations are still required when solving equations, that's not my question). This can be seen clearly from one section of the log file:

Code:
Courant Number mean: 0.279317 max: 0.999569
deltaT = 0.00175747
Time = 5.92794

DILUPBiCG:  Solving for Ux, Initial residual = 8.03872e-05, Final residual = 3.01259e-10, No Iterations 4
DILUPBiCG:  Solving for Uy, Initial residual = 7.47932e-05, Final residual = 2.18265e-10, No Iterations 4
DILUPBiCG:  Solving for Uz, Initial residual = 5.96536e-05, Final residual = 1.09994e-10, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.000123055, Final residual = 4.66822e-10, No Iterations 10
time step continuity errors : sum local = 1.54552e-12, global = 2.47586e-13, cumulative = -4.13283e-11
GAMG:  Solving for p, Initial residual = 2.08618e-05, Final residual = 6.33155e-10, No Iterations 8
time step continuity errors : sum local = 2.09623e-12, global = -2.88986e-13, cumulative = -4.16173e-11
DILUPBiCG:  Solving for epsilon, Initial residual = 2.95649e-05, Final residual = 9.94966e-11, No Iterations 4
DILUPBiCG:  Solving for k, Initial residual = 4.52894e-05, Final residual = 6.86864e-10, No Iterations 4
ExecutionTime = 3449.02 s  ClockTime = 3453 s

Courant Number mean: 0.279319 max: 0.999571
deltaT = 0.00175747
Time = 5.9297

DILUPBiCG:  Solving for Ux, Initial residual = 8.04511e-05, Final residual = 2.77023e-10, No Iterations 4
DILUPBiCG:  Solving for Uy, Initial residual = 7.47824e-05, Final residual = 2.18558e-10, No Iterations 4
DILUPBiCG:  Solving for Uz, Initial residual = 5.97415e-05, Final residual = 1.09586e-10, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.000123775, Final residual = 5.54077e-10, No Iterations 10
time step continuity errors : sum local = 1.83445e-12, global = 2.88968e-13, cumulative = -4.13283e-11
GAMG:  Solving for p, Initial residual = 2.07948e-05, Final residual = 5.90437e-10, No Iterations 8
time step continuity errors : sum local = 1.95485e-12, global = -2.66983e-13, cumulative = -4.15953e-11
DILUPBiCG:  Solving for epsilon, Initial residual = 2.95488e-05, Final residual = 9.23568e-11, No Iterations 4
DILUPBiCG:  Solving for k, Initial residual = 4.52872e-05, Final residual = 4.31262e-10, No Iterations 4
ExecutionTime = 3449.6 s  ClockTime = 3453 s
It is clear that between time 5.92794 and 5.9297, only one standard PIMPLE step is performed, and no iteration occurs to confirm convergence at the end of this time step. In "fvSchemes", I've already assign "ddtSchemes" to be "Euler", so I think it should be an implicit time discretization.

May I ask why this happens? Actually the same situation happens in the "pitzDaily" case in the tutorial pimpleFoam directory, so I think maybe this is some mechanism exist in OpenFOAM. Can anyone help me to explain it?

Thank you very much!
nicklj is offline   Reply With Quote

Old   May 7, 2014, 17:12
Default
  #2
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I don't know about how Fluent handles things I'm afraid. However, to solve the entire problem several times at one time step using PIMPLE you may increase the nOuterCorrectors in fvSolution to whatever value you wish. If you set it to 1 the solver will operate in PISO mode which, as you've pointed out, only iterates over each equation a number of times.

There is a substantial amount of discussion on this forum as to how the two algorithms differ, see for instance these threads:

On the PIMPLE algorithm

How does PIMPLE work?

Peace,

A
Artur is offline   Reply With Quote

Old   May 8, 2014, 01:29
Default
  #3
New Member
 
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 3
nicklj is on a distinguished road
Quote:
Originally Posted by Artur View Post
I don't know about how Fluent handles things I'm afraid. However, to solve the entire problem several times at one time step using PIMPLE you may increase the nOuterCorrectors in fvSolution to whatever value you wish. If you set it to 1 the solver will operate in PISO mode which, as you've pointed out, only iterates over each equation a number of times.

There is a substantial amount of discussion on this forum as to how the two algorithms differ, see for instance these threads:

On the PIMPLE algorithm

How does PIMPLE work?

Peace,

A
Dear Artur,
Thank you very much for your reply and the information. It is very helpful. According to the references and CFD books, PISO is a kind of non-iterative method for transient problem.

I also found in this thread:
On the pimpleFoam solution algorithm
It seems that if the nOuterCorrectors is set to 1, the PIMPLE becomes identical to PISO.

Therefore, if I am not wrong, maybe the pisoFoam corresponds to the non-iterative PISO scheme in FLUENT, and pimpleFoam correspdons to the iterative PISO scheme in FLUENT, which providing the capability to perform outer iterations.


Regards,
Nick
nicklj is offline   Reply With Quote

Old   May 8, 2014, 03:22
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
RodriguezFatz will become famous soon enough
I was wondering the same things when switching from Fluent to OpenFoam, but you are right.
pisoFoam is the same as if you set (in Fluent) the maximum number of iterations per time step to 1. PimpleFoam with any number of outer iterations is the same as a regular transient simulation in Fluent.
I did not check, whether piso=piso and simple=simple in Fluent and OpenFoam, but what you write is generally right.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is online now   Reply With Quote

Old   May 8, 2014, 22:30
Default
  #5
New Member
 
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 3
nicklj is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
I was wondering the same things when switching from Fluent to OpenFoam, but you are right.
pisoFoam is the same as if you set (in Fluent) the maximum number of iterations per time step to 1. PimpleFoam with any number of outer iterations is the same as a regular transient simulation in Fluent.
I did not check, whether piso=piso and simple=simple in Fluent and OpenFoam, but what you write is generally right.
Thank you very much. I'm so happy to hear that
nicklj is offline   Reply With Quote

Reply

Tags
fluent, iteration, transient

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
Possible Bug in pimpleFoam (or createPatch) (or fluent3DMeshToFoam) cfdonline2mohsen OpenFOAM 3 October 21, 2013 09:28
FLUENT or OpenFoam for Particle-surface intercation simulation? Amir1 Main CFD Forum 0 May 10, 2013 17:15
Question: BC openFOAM vs. FLUENT oehmu OpenFOAM 2 December 14, 2010 17:14
Fluent elbow in Openfoam chemeng OpenFOAM 1 January 21, 2010 04:52
OpenFOAM vs Fluent for cylinder at Re%3d150 lr103476 OpenFOAM Running, Solving & CFD 40 December 18, 2008 10:09


All times are GMT -4. The time now is 12:57.