Need URGENT HELP for convergence problem of a turbine
 

Hello everyone,

I encountered convergence problem when I tried to do simulation of a turbine. I have spent more than two weeks but still can not fix the thing. So hopefully you would help me figure it out or give me some suggestions.

The model is a three-stage turbine. We may call it 'baseline' (Fig. 1 top-left). Then I added endwall contouring on the first rotor (R1), named as 'contoured' (Fig. 1 top-right). For these two case, everything is fine. Usually it takes 300 time steps to get converged. Then I went to 'baseline with purge' (Fig. 1 bottm-left) which has purge flow at upstream of R1. This case also got converged in 500 time steps. After this, I applied purge flow to contoured case 'contoured with purge' (Fig. 1 bottom-right). Then the trouble keeps bothering me. By the way, the turbulence model is SST model.

At the beginning, I used High Resolution for both Advection Scheme and Turbulence Numerics. I got smooth but pretty high residual for Mass (red curve in Fig. 2) and Heat Transfer (Fig. 3), which is much higher (1-2 orders) than what I got from previous cases. This was due to the imbalance within R1. At the same time, the unreasonable result which was not physics was obtained computational domain R1, see temperature distribution in Fig. 4.

Then I tried to enhance the quality of the mesh several times. It never works. So I realized it should not be the problem of mesh, as I used the similar mesh for previous case successfully. I also tried to change the boundary conditions. It did not work either.

Finally, I turned to Timescale. This time I set local timescale factor as 5, using First Order and blender factor 0.75. Although the residual looks better than before (Fig. 5), the residual significantly increased after 500 time steps and became to oscillate. It is quite strange that the high RMS-Mass was found in R3 but not in R1 and thus the temperature distribution in R1 seems reasonable. But I did not see any trend that the residual may drop to less than 1e-6 as previous cases which were all converged. Moreover, after I changed back to physical timescale and high resolution scheme, R1 became my headache again. So my questions are:

1. Does the strong unsteady property of the flow cause this problem?

2. Since the strong unsteady property exists in the 'baseline with purge' too, does the complicated geometry of the endwall contouring lead to instabilities?

3. Could I use the results calculated with local timescale factor as final results?

4. What is the possible solution for this problem if I can not afford to perform transient calculation?

This bothered me a lot, so I eagerly look forward to your solutions or suggestions. Thank you very much.

http://www.cfd-online.com/Forums/cfx...nvergence.html

this might be useful for you

Thank you for your reply. I went to the link and reviewed your discussion. I tried to use double precision, but it runs too slowly that I can not afford it. By the way, I am using 10 cpus with total 66GB memory for the running. Is it because the number of the cpus is not enough or the memory is small or I did not set that correctly?

For the mesh, I am afraid that I can not increase the height of the first grid as I use SST turbulence model.

well, I have no clear solution for this problem, this might be due to mesh, flow might be transient or any thing else you name it.

But what I wanted to say is that, use the default time scheme that is auto time scale and set the time scale factor to 0.1 and then run the solution for the 1000-2000 time steps. During this phase you may occasionally have the some divergence, don't worry, ultimately the solution converge to the required tolerance provided that any steady solution exists. (my last reply in the thread SMC models convergence)

PS.

1. With automatic wall treatment you don't need to have the Y+ to be ~1. Y+~ 10 should do the same magic.
2. Can you tell me (or attach the line plot of Y+) the y+ values at the leading edge of rotor 1 (in other words Y+ in the stagnation region)

Pursuor,

Yes the cause may well be unsteady flow patterns, assuming you are now running frozen rotor or mixing plane simulations. The obvious fix is to do a transient simulation instead.

If you dont need the increased accuracy of a transient calculation or just dont have the time, I would suggest setting a physical timescale to a typical residence time as the CFX manual suggests. For turbomachinery: use 1/(2*pi*rpm [min^-1]) where rpm is ofcourse the speed of your machine.

Hope this helps,

Graham

This looks a FAQ question to me:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria