[GregCFD]

I'm running a simulations of a 2D baffle-vane type mixing cell using the k-omega SST turbulence model and a 2nd order implicit time step method (the Software is ANSYS Fluent 16.2, but I figure this is a general enough question for this Forum). To conduct a time-mesh convergence study I've started with a simple mesh and have then ran the simulation to "steady state" and then collected some data to compare against other time steps, in this case the maximum TKE and TDR, the torque and TKE, TDR and Velocity magnitude at three points through out cell.

I stared with a time step equivalent to the mixer moving at two degrees per timestep and the halved the time step at each iteration. The problem I'm having is that even with the the Courant number at ~0.02 none of the monitors I mentioned above have converged yet, worse the percentage differences are still increasing even after 5 halvings. My reading through the literature before this had most simulations of mixing cells claiming time-convergence with the rotational angle at ~2-3 degrees per timestep while my unconverged is running at 1/16 degree per timestep.

Can anyone offer any sort of advice as to why I'm not seeing convergence even with a (what appears to be a) ridiculously fine time step?

[davidwilcox]

What is your number of iterations per time step?


Sent from my iPhone using CFD Online Forum mobile app

[GregCFD]

Originally Posted by davidwilcox

What is your number of iterations per time step?

10 - 20 iterations per time step to reduce the (absolute) residuals to 1e-6.

[arjun]

Originally Posted by GregCFD

Can anyone offer any sort of advice as to why I'm not seeing convergence even with a (what appears to be a) ridiculously fine time step?

You are possibly seeing what is call decoupling of pressure and velocity. This could happen bacause Ap or diagonal of momentum equation is inversely proportional to timestep size (1/dt) , as dt goes small Ap increases.

The Rhie and Chow coupling is function of inverse of Ap , so its directly proportional to dt or timestep size. As times step goes down this Rhie and Chow flux will become weaker and equations can decouple.


In starccm, we added something to counter this. In fluent there is nothing.

[GregCFD]

Originally Posted by arjun

You are possibly seeing what is call decoupling of pressure and velocity.

In starccm, we added something to counter this. In fluent there is nothing.

Thanks for your reply arjun, I've had a quick look on the internet and I can't find anything about it but do you know of a method to tell if the decoupling has occurred and how, if at all, I can avoid it?

[arjun]

Originally Posted by GregCFD

Thanks for you reply arjun, I've had a quick look on the internet and I can't find anything about it but do you know of a method to tell if the decoupling has occurred and how, if at all, I can avoid it?

Check for checkerboarding on internet. Also check if this type of thing happening. It is difficult to spot in Fluent because the plots are usually made from node values which are interpolated from cell centers. So you have to be careful in spotting it.
In starccm you can make contour plot from cell center values so it is easy to see it happening.

PS: Note that this is one of the possible reasons but until you make sure you are not sure. Based on what you wrote earlier this is best guess.

[GregCFD]

Fortunately you can switch between node and cell centre values in Fluent with a click. I've attached an image of the cell centre values of the static pressure, I'm not seeing anything that looks like checker-boarding unfortunately.

[arjun]

You do have little bit of it in this plot. Interestingly it is at the grid parts where there is skew. Do you see that minus and plus pressure adjacent to each other. That is checkerboarding.

You do have some places where pressure is suddenly changing and not smooth.

What is pressure interpolation scheme? In old Fluent the standard scheme was default one. If I am right now the default one is second order pressure interpolation.

[GregCFD]

Originally Posted by arjun

What is pressure interpolation scheme?

You're correct in that the default is the 2nd order scheme but based on the recommendations in the User Guide I've been running it with the PRESTO! scheme and the coupled method for pressure-velocity coupling.

[arjun]

Originally Posted by GregCFD

You're correct in that the default is the 2nd order scheme but based on the recommendations in the User Guide I've been running it with the PRESTO! scheme and the coupled method for pressure-velocity coupling.

I would try the other schemes like standard, second order and body force weighted too.

I am not aware of details about PRESTO, as they are never mentioned anywhere. The closest information I got was from previous fluent developer, where he said that he can't reveal but I am not missing much. (that just means that it slight rearranging of terms).

PS: Note that it could be one of the reasons, there is no guarantee that this is the reason.


EDITED TO ADD:

I did not notice you said coupled method for coupling. There is that courant criteria, play with it. It could cause divergence in case of coupled system. IT is very sensitive to it.

[GregCFD]

I've tried playing around with some of the settings, on the original mesh PISO (without it's skewness correction) diverges immediately which I thought was a bit odd because the maximum skewness is only ~0.6 but with it switched on PISO like SIMPLE and the coupled method all run fine.

I've also tested changing around the pressure interpolation (to Standard and 2nd Order) but that hasn't helped. I also tried switching over the turbulence models to the realizable k-e method which almost seems to work but returns to diverging results like the SST method at finer time steps.

Any other ideas as to what is stopping the time convergence?