CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Convergence problems!!! (http://www.cfd-online.com/Forums/fluent/89278-convergence-problems.html)

king lui June 8, 2011 15:03

Convergence problems!!!
 
Hello everybody,

I investigate a time-dependent two-phase flow with the vof-model and I have some problems with the convergence. I donīt know why but my simulation runs good for the first few time steps (between 2 and 50), but suddenly the continuity residual raises and results in a floating point error.At the beginning I had also the problem with a too high global courant number but this is gone since I am using the variable time step method. Anyway, now the floating point error is the problem, for example the last simulation I did runs very good, at the end the time steps converged quicker and quicker but as I said did the continuity increase suddenly.

I hope someone can help me with this problem as I tried already many things like different solver settings, changing the under-relaxation factors, minimise the time step size, etc.

me3840 June 8, 2011 15:14

The problem may lie with your grid. Check the velocity vectors for discontinuities or weird flow fields, and refine or change the grid in that location.

Trev June 8, 2011 17:42

Depending on the type of flow you could also try initially running the solution as single phase (deactivate the VOF equation) then later patch the other phase into the domain when the solution is stable.

But as me3840 says check the quality of the mesh first. You could try looking for regions where large gradients exist which may not physically occur. But the state of your solution will probably not provide much useful information considering you have only done a handful of time steps and the solver will have barely processed the boundary conditions.

king lui June 9, 2011 02:44

1 Attachment(s)
Hello, at first thank you for your suggestions to solve this problem, I will try now to alter the mesh. About the answer of Trev, how do I kow when the solution is already stable? Yesterday my last try looks quite good for the first 260 time steps, but than the global courant number increases from 2 to 2e8. Another question is, if there is a difference between the "normal" courant number and the global courant number? To display my problem more clearly for you, I attach a picture from the residuals of my last try.
Thank you in advance for your help. Attachment 7948

Trev June 9, 2011 09:38

The solution is generally stable when the residuals are flat (as low as the residual error will go) or at least oscillating by a small amount and your mass flux error is at an acceptable value (I normally use <10-6). From the look of yours I would say that for 1st order discretisation the averaged residual errors are ok but not for anything higher. In which case you should be using 1st order upon the initial run of the solution. You have large oscillations around the magnitude of an order which straight away says that your time step is too large as the solver can't properly resolve the flow. So you will have to drop the CFL number to account for this as a rough estimate i would say set it to something like 0.1 initially just to get the solution going. As well as use a fixed time step but experiment with it too see how the residual oscillations are affected. You can increase both at a later stage as all you want to do initially is get the solution running without the worry of divergence.

I don't know how you have set the solver up but have used these guidelines in the past to do VOF work once you have accepetable convergence values at each stage.

1) Run singlephase as steady-state with 1st order discretisation.
2) Switch to transient solver.
3) Increase to 2nd order.
4) Patch appropriate region with secondary phase.

I'm not too sure on the difference between the standard CFL and global CFL number. But would hazard a guess that the solver uses the standard CFL number as a baseline value and deviates from it accordingly at parts of the mesh where it is having trouble resolving the flow. Then applies a global CFL when things are going wrong to try and prevent divergence. But like I said I'm not sure so hopefully someone else could help you out on that one?

king lui June 11, 2011 08:24

Thank you guys for your help, now my residuals are stable if I use your suggestions but unfortunately with a very small time step so that my simulation needs several months and if I alter the time step size the same problem occurs as I already explained.

So if you have maybe some more ideas please let me know.
But anyway thank you for your help.

Trev June 12, 2011 10:49

Although your time step is small at the moment to keep the solution stable this should only be temporary and you will probably find that you can start to increase it as the solution progresses. So I suggest experimenting with seeing how much you can increase it by every now and again. A good indicator of what you can get away with using is to see how much oscillation it causes in the residuals. If it speeds up the solution you can allow oscillations in the residuals as long as they are not too large or cause divergence.

king lui June 14, 2011 03:21

I try this now, unfortunately I can increase the time steps just with a very small amount. But anyway, thanks a lot for your help.

kbaker June 15, 2011 05:00

What type of flow regime you working with?

king lui June 15, 2011 05:05

Hello,
its a gas-liquid flow regime.

kbaker June 15, 2011 08:38

dude i mean with what type of flow regime is it stratified-annular-slug flows...........etc?

king lui June 15, 2011 10:30

its a stratified annular flow


All times are GMT -4. The time now is 06:25.