using RNG k-e
 

I used k-e for free surface model the result was converged, but for the same model (same mesh size time scale .... ) I used RNG k-e (for comparison)the simulation does not reach to convergence after 1200 iteration. can anyone tell me the reasons
thanks

have anyone any suggestion for above problem ??????, please

K-e and RNG k-e turbulence models are very similar. If this change in your model makes a difference then you model is obviously on the verge of being numerically unstable.

but I do not change anything in my model, only turbulence model from k-e to RNG k-e, what should I do to the model in order become convergence with RNG K-e??? I reduced time scale but It does not reach convergence :confused:

The standard things to improve numerical stability: Double precision numerics, better mesh quality, smaller time step, better initial condition.

but I did all above parameters for simulation by k-e and successfully reach convergence but for RNG k-e does not reach

Let me repeat post #3:

as I understood from your post , (if changing turbulence model from RNG k-e to standard k-e, makes the solver numericaly unstable then some parameters should be changed such as (time scale, mesh quality ...)) is that Right??

Yes, correct.

But the point I am really trying to say is that your simulation is very unstable anyway. So anything you do to make the RNG simulation converge will help the k-e simulation as well.

After changing mesh to coarse to hide vortex shedding in order to become convergence and increasing time scale the results are, mass flow rate become constant, but highly fluctuation observed in v,u,w equations, I used supercritical B.C at outlet, initial conditions include velocity, pressure and (air and water VoF)
https://drive.google.com/open?id=0B3...0pNRmtnemtQR00
https://drive.google.com/open?id=0B3...W5IUmp1dkJHQTg
while previous residual for fine mesh with lower time step are
https://drive.google.com/open?id=0B3...HctaFA1TkwxeUE

This is normal. But note that your results have probably reduced in accuracy significantly by coarsening the mesh.

In my experience many free surface flow simulations require a transient solution to obtain convergence. This is because surface waves have very low dissipation and they can be resolved in a transient simulation but cause havoc with convergence in steady state simulations. So have you tried a transient simulation? You should be able to get that to converge even with the fine mesh. But it will take significantly longer to run.

I did sensitivity analysis for choosing mesh size, turbulent model, for this reason I used k-e and RNGk-e and compare their result, the third is the comparison between steady and transient simulation type for this reason I wan to simulate with steady stat, yes for transient I want for time step use 1- adaptive time step with 5 loop coeff. 2- Strouhal frequency (fst=St D/V), from this formula strouhal number (St) can be find, time step = St/5, which of them are better???
note: 1-adaptive time step need higher computational time, than specifying time step value, 2-I saw many researches in free surface flow performed by CFX using steady state analysis type !!

For transient simulations I recommend adaptive with 3-5 coeff loops. You can use time step formula you like, but you need to check the time step sensitivity.

If other researchers have got this model to converge steady state then have a look at what they have done and try to figure out why they get it working and you can't.

thanks
If I used time step according to equation, how can I check my result does reach convergence

By defining a convergence criteria and seeing if it is achieved.

ok, I defined residual (10-4), and imbalances 0.01, and a monitor point at outlet to monitor mass flow rate (or any interest variable), if the a above criterion are met, so the convergence was achieved. is it right?

Yes, the convergence tolerance you defined has been achieved. But is the tolerance you defined sufficient to give an accurate enough result? That is an important question as well.

according to residuals and imbalances the results appear that reached convergence, but Courant No. is high (RMS Courant no. = 15 , MAX Courant no. = 286) is the a problem?

Do a sensitivity analysis on your time step size and find out.

I tested three time step (0.05, 0.04, 0.03), the results of (0.03, 0.04) is near to each other and courant No. reduced to 10 at time step 0.03. is that enough?