
[Sponsors] 
December 25, 2017, 07:45 
min time step in transient CFD

#1 
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Hi all
The maximum of time step is calculated by Courant Number. Is there any limitation for min time step in transient CFD simulations? I have a transient problem that it will be solved for Cr=0.8 . Now I want to investigate the independence of my problem from time step. so I increased my Cr from 0.8 to 0.3. Every thing is good and exact until 50% of the total time. after that suddenly residuals become in order of 10^20 and time step in order of 10^10 !!! pressure and velocity become unbounded and the problem become diverged! Thanks 

December 25, 2017, 09:07 

#2 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 
The best what you can do is to write results in between and look which of the field get strange.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

December 25, 2017, 09:26 

#3  
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Quote:
I did what you said. Pressure is increasing in every time step strongly! So I increased the number of loops of solution of pressure correction equation from 1 to 200!! but again the problem became diverged! 

December 25, 2017, 11:02 

#4 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 
Looks like a problem with the boundary conditions.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

December 25, 2017, 11:27 

#5 
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 

December 25, 2017, 11:48 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 
Your problem can be due likely to a bug in your code. But if it is not, you have to consider that a small time step requires to work with smaller residuals in your iterative methods to avoid false convergence of the solutions.
And if you want to check the independence of the solution by changing only the time step you need to work on a spatial grid very fine since from the large time step. In practice, the value h has to be evaluated from the smallest time step you use. 

December 25, 2017, 12:20 

#7 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 
It is easy to construct something what is not physical. At least this is valid for me.
If pressure increases it may be you have a closed volume, incompressible medium and "generate" mass somehow. This may happen if you have an inflow but no outflow. Or if you generate mass by density changings or chemical reactions. I don't know your case, so I can only guess what may be the reason.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

December 25, 2017, 12:23 

#8  
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Quote:
Thanks 

December 25, 2017, 12:27 

#9  
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Quote:
the code is for openFoam. my residuals are set to 10^6 . is it enough? what is h in? ( In practice, the value h has to be evaluated from the smallest time step you use) 

December 25, 2017, 12:31 

#10 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 

December 25, 2017, 15:44 

#11 
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 

December 25, 2017, 16:15 

#12 
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 502
Rep Power: 20 
You could be a bit more specific with the description of your flow problem and also OpenFOAM can be anything from financialFoam to potentialFoam ...
Some of our "normal" compressible solvers show a strange behaviour, when we combine shock waves with small time steps. 

December 26, 2017, 05:38 

#13 
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 

December 26, 2017, 05:51 

#14 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 
you should provide all the details of your simulation


December 26, 2017, 06:05 

#15 
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
steady 2D flow of viscoelastic fluid around a circular cylinder
Re=100 (rho = D = U_inf = 1, mu=0.01) viscoelastic properties: FENECR model Wi(wisenberg number) = 80 numerical aspects: div scheme: upwind (with central will be diverged!) residuals = 10^6 PISO algorithm relaxations: U: 0.5 , p,tau: 0.3 Grid: thank you 

December 26, 2017, 06:10 

#16 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 
First of all, I suggest to do the test without the viscoelastic coupling to check if you still have the same problem. At such a low Re number, the main stability constraint is for the viscous part, not for the convective part.
Then consider also the relaxation factors in this simplified test. 

December 27, 2017, 23:53 

#17  
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Quote:
I solved this problem for Newtonian case (with viscoelastic solver) by Cr=0.3 . It works good, and give me the results close to Cr=0.8 results. I think as we increase the viscoelastisity, because of nonlinear nature of viscoelastic constitutive equation, we cant decrease the time step much more! Of course I hear that (this is a experience of some of friends) if we decrease time step from a critical value, the problem will be diverged! Maybe for these nonlinear equations this limitation is very stronger! Whats your idea? 

December 28, 2017, 05:12 

#18  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,278
Rep Power: 34 
Quote:
This is what is possibly happening here. Also, as he pointed out as viscosity becomes dominant term, convective part stop playing critical part. In your case what it means is that you are solving diffusion or Poisson problem for momentum equation. What it in turn means is that you can not use implicit under relaxation anymore that modern solvers apply. You need explicit under relaxation. In numerical point of view implicit urf is used to divide Ap of the matrix and that increases diagonal of matrix. It is well known that this approach does not work for Poisson equation. 

December 28, 2017, 06:01 

#19  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71 
Quote:
For an explicit timemarching scheme, the numerical stability region is determined by the curve (in the 1D case) cfl=f(Re_h), being Re_h the cell Reynolds number. Only for Re_h >>1 you can recover the constraint due to only the cfl value. In your case, at Re=100 I suppose you are working at Re_h=O(1) so that the max cfl value for the stability is much lower than it would be for the inviscid case. 

December 29, 2017, 03:43 

#20  
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 
Quote:
1 dissipation (physical or numerical?). especially what is Rhie Chow dissipation? 2 what are implicit and explicit under relaxations? what is the difference between them? why did you think that in my problem, viscosity becomes dominant term? 

Tags 
time step size, transient 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field  lakeat  OpenFOAM Community Contributions  58  December 23, 2021 02:36 
p_rgh initial residual no change with different settings  manuc  OpenFOAM Running, Solving & CFD  3  June 26, 2018 15:53 
pimpleDyMFoam computation randomly stops  babapeti  OpenFOAM Running, Solving & CFD  5  January 24, 2018 05:28 
simpleFoam error  "Floating point exception"  mbcx4jc2  OpenFOAM Running, Solving & CFD  12  August 4, 2015 02:20 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 