min time step in transient CFD
 

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

The best what you can do is to write results in between and look which of the field get strange.

Thank you
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!

Looks like a problem with the boundary conditions.

I didn't get it! could you please explain your statement?

Thanks

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.

It is easy to construct something what is not physical. At least this is valid for me.:o

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.

As I have gotten result from this problem by Cr=0.8 (it is validated with papers), I'm sure that non of them is happened. Just when I change Cr from 0.8 to 0.3, the problem become diverged.

Thanks

thank you
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)

h is the mesh size and the residuals can be required to be smaller

Ok
Thank you
I will do that

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.

Hi
I set my residuals to 10^-12 but unfortunately again become diverged!

you should provide all the details of your simulation

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:
http://uupload.ir/files/tae8_6-1.png
http://uupload.ir/files/j0hw_6-2.png

thank you

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.

Could you please explain more about your sentence : "At such a low Re number, the main stability constraint is for the viscous part, not for the convective part."
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?

Yes. It is because of the Rhie Chow dissipation which is proportional to time step size and below certain time step size it does not provide enough dissipation to keep velocity and pressure coupled.
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.

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.

Thanks for your nice answer. because it will force me to learn some new concept. could you please explain about these concepts, or give me link or reference to read about them:
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?