|
[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: 6,776
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, 12:27 |
|
#7 | |
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 |
|
#8 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,776
Rep Power: 71 |
||
December 25, 2017, 15:44 |
|
#9 |
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 |
||
December 25, 2017, 16:15 |
|
#10 |
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 501
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 |
|
#11 |
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 |
||
December 26, 2017, 05:51 |
|
#12 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,776
Rep Power: 71 |
you should provide all the details of your simulation
|
|
December 26, 2017, 06:05 |
|
#13 |
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: FENE-CR 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 |
|
#14 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,776
Rep Power: 71 |
First of all, I suggest to do the test without the visco-elastic 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 |
|
#15 | |
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 non-linear 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 non-linear equations this limitation is very stronger! Whats your idea? |
||
December 28, 2017, 05:12 |
|
#16 | |
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
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 29, 2017, 03:43 |
|
#17 | |
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? |
||
December 29, 2017, 22:40 |
|
#18 | |
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34 |
Quote:
About the Rhie and Chow term, which is difficult to find from books as to what my comment was talking about here is very short hint. Rhie and chow term is inversely propertional to diagonal of momentum matrix. Diagonal of momentum matrix is inversely propertional to time step size. For euler time stepping it would be ( density * volume / delta_T ). So when delta goes to 0, it shall go to infinity and 1/Ap goes to 0. So basically as delta_T reduces the Rhie and Chow term becomes weaker and weaker. After certain value, it could be too small at some parts of simulation that solution can diverge. |
||
January 9, 2018, 00:36 |
|
#19 |
Senior Member
A. Min
Join Date: Mar 2015
Posts: 305
Rep Power: 12 |
Hi all
I want to solve the flow around the cylinder in viscoelastic fluid. At first I did it for Newtonian fluid in Re= 10 , 40 , 100 and for viscoelastic fluid in Re= 10 , 100 and obtained exact results. But when I change the Re to 40 for viscoelastic fluid, it became diverged! I changed many parameters of solution: urf = from 0.1 to 0.9 --> diverged! corunt Nu. = from 0.1 to 0.9 --> diverged! changing the kind and size of mesh --> diverged! changing the kind and size of mesh --> diverged! increasing the number of solving pressure correction Eqn from 2 to 20 --> diverged! decreasing the min residuals to 1e-8 --> diverged! changing discretization schemes of div terms: Gauss linear (central), Gauss upwind(1st), Gauss upwind(2nd), limitedLinear , QUICK --> diverged! But I have done some ways to solve that: 1- I saw in this page that sb proposed to the other that decrease the residuals to 1e-19 !! I did it and my solution became converged! I can't analyze that! Is it possible? 2- In the other way I increased the number of solving pressure correction Eqn to 20, decreasing the min residuals to 1e-8 3- setting the time step to 0.001 instead of setting Cr=0.3 Now I don't know that my results are reliable or not! Could you please tell me what happend that these solutions are appropriate for solve it? Thanks |
|
December 28, 2017, 06:01 |
|
#20 | |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,776
Rep Power: 71 |
Quote:
For an explicit time-marching 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. |
||
Tags |
time step size, transient |
|
|
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 |