[mohamadalimirzaei1994]

I am trying to simulate a cyclone using DDPM and RSM with structured hexahedral mesh. although the mesh quality seems to be fine (Minimum Orthogonal Quality = 0.53), the solution diverges immediately after the start with the following warning:

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in many cells
and then:
reverse flow at the outlet

the turbulent boundary condition is assigned at inlet using intensity and hydraulic diameter.
is there any solution method that might help?
at the moment I am using phase coupled SIMPLE, green-gauss node based, presto!, second-order upwind for momentum, quick for volume fraction and first-order upwind for the rest.

I ran the same simulation using sst-cc and it was fine. I tired converged solution of sst-cc as initial for RSM simulation bit it did not help. can you help find the problem?

[vinerm]

is not a good starting point for RSM; is. But even with to begin with, you should be able to converge. Firstly, when the model is changed, URFs should be very very low, of the order of 0.01, so that the matrix could be developed. Use only first-order numerics and disable volume fraction for a few iterations. If the mesh is hex and structured, node based gradient does not add anything, so, prefer using LSQ.

[mohamadalimirzaei1994]

Originally Posted by vinerm

is not a good starting point for RSM; is. But even with to begin with, you should be able to converge. Firstly, when the model is changed, URFs should be very very low, of the order of 0.01, so that the matrix could be developed. Use only first-order numerics and disable volume fraction for a few iterations. If the mesh is hex and structured, node based gradient does not add anything, so, prefer using LSQ.

thank you so much. so far, it seems that using very low URFs for the transition from one turbulence model to the other is solving the problem. just one question. with these very low UTFs (0.01) residuals are dropped in order of 10e-3 after a very low number of iteration at each time step (meaning that the convergence at each time step is achieved fast enough). so do you think it is ok to continue with these very low UFRs or these values must increase? if they must increase should it be gradually increased?

[vinerm]

You should increase the URFs otherwise there could be conservation issues. You can increase in two to three steps, say, every 10 time-steps.

[mohamadalimirzaei1994]

Originally Posted by vinerm

You should increase the URFs otherwise there could be conservation issues. You can increase in two to three steps, say, every 10 time-steps.

and eventually, work with default values?
I mean, how can we ensure that our URFs are big enough??

[vinerm]

Yes, usually default values are good. However, if convergence is good within each time-step for given values of URF and URFs are not very small, say below 0.1, then its alright. With very small URFs, the changes in the coefficient matrix are so small and numerical solver considers everything converged. What happens in reality is that high frequency errors are reduced but low frequency errors remain. So, using high URFs are required but 0.5 and 0.9 won't make a difference as long as solution is well converged.

[mohamadalimirzaei1994]

Originally Posted by vinerm

Yes, usually default values are good. However, if convergence is good within each time-step for given values of URF and URFs are not very small, say below 0.1, then its alright. With very small URFs, the changes in the coefficient matrix are so small and numerical solver considers everything converged. What happens in reality is that high frequency errors are reduced but low frequency errors remain. So, using high URFs are required but 0.5 and 0.9 won't make a difference as long as solution is well converged.

I started from 0.01 for all URFs and increased them all gradually up to 0.2 and up to there it was ok (residuals were drop enough after 2 or 3 iterations in each time steps), but when I increase them to 0.3, it immediately diverges (warning: very high turbulent viscosity ratio). is it normal?
in general is it ok to continue the simulation with 0.2 for URFs? how can we ensure that the final converged result is not affected by this value?

[vinerm]

If it is diverging with 0.3, then you can continue with 0.2 or 0.25. Once converged, which will take longer due to small URF, solution will be more or less independent of the URF used. Most importantly, you should set up some monitors. If those monitors become constant, then you can consider it converged.

[mahsa asadi]

hi, I am simulating a cyclone separator with DDPM and RSM. I could not converge it. is it possible for you to talk about this problem? this is my email address mahsatorkaman.a@yahoo.com