attene wrote: ↑Tue Sep 25, 2018 10:45 am
Hi everybody,
I would like your opinion regarding the last simulations I have done on my model. you can find attached the two setup.xml I tested as well as the two listing files:
1) steady simulation using the SIMPLEC algorithm.
2)////////////////////////// SIMPLE /////////.
Resuming: The computational domain consists of two parts, one rotating cylindrical fluid zone ( frozen-rotor approach) + one stationary tank domain with rectangular cross-section. The rotating domain is included in the tank domain. No faces joining was done.
All the simulations I carried out so far blew up!
You maximum CFL number is already much too large at the first time step, and only gets worse from there.
The SIMPLE steady algorithm is rarely used, and not robust enough in most cases, so the convergence problem in this case is not so surprisong.
I am not sure even the "frozen rotor" model works well with a local time step (SIMPLEC pseudo-steady comptation), so I recommend checking with a fixed time step first, and then testing with a pseudo-steady algorithm to accelerate conevrgence if that works.
In any case, you at least need to reduce your reference time step first (whether you use a fixed or varying or local time step), so the CFL stays within reasonable bounds (ideally CFL everywhere, in practice if you have a mean CFL areound 1 and a max CFL under 10 or 20, things should be OK).
I did a test with a constant reference time step (0.0001) as you suggested, the simulation diverged after very few time steps.
Please find attached the .xml and listing files.
I was thinking now to try changing the numeric scheme under equation parameters..
I am starting to think as well that both mesh and turbulence set up (reference length, k and omega in my case) may play a role in the stability of the calculation
What can I also try to do..?
Can you try reducing the time step by another factor of 5 or 10 ? The average value is OK at start but the maximum very high, so you probably have a mesh quality issue. You may also try using least-squares gradient (or least squares with partial extended neighborhood). Using upwind or partially upwind scheme in numerical parameters may also help (reducing precision, but increasing stability).
Thank you for your answer!
I will have a look at changing all the numerical parameters you mentioned!
Meanwhile I have realized something strange in my set-up: Having refined the mesh to solve the boundary layer, I do not need any wall functions in my kw-SST model but although I tried to impose no wall function in the advanced options, the
latter option is not selected!!( 2 scales model (log-law) appeared instead).
In the last test simulation I launched I further reduced the CFL. This time the max CFL looks smaller and below 10 after initialization (please see the listing_0timestep). Even during the first two time steps (listing-calc) it seems ok, but after that goes up and up and the solution diverges.
To better isolate the cause of the process, could you run the same mesh using a transient turbomachinery model (or better, for a start, no turbomachinery model), or do you have a smaller mesh on which you reproduce this issue (and with which I could run my own tests) ?
An easy test would also be to run this case using k-epsilon (linear production) or Rij-SSG model ?
This might be a mesh quality issue, so could you also post the "listing" file for the mesh run in "mesh quality" mode ? In this case we can try additional "mesh robustness" oriented settings. If the problem is not due to mesh quality but choice of options, it should be reproducible on a smaller mesh (I am thinking of the turbulence model here, because in our test suite, k-epsilon is used, and I am not sure about k-omega in this case.
Thank you for your answer!
I will do all the test you suggested.
To change from frozen-rotor to transient simulation do I have to impose a sliding wall BC to the blades although a rotational velocity is imposed to the rotating cylindrical domain(in the turbomachinery module)?
If this is the case: what velocity? ( I can see I can set-up the three components of the velocity U V and W but they should be a function of the radius from the center of rotation..)
To run in "mesh quality" mode I should add the flag --quality one the preprocessing stage?
To run in transient mode you do not need to change anything else than the matching option. Just use the regular wall function (or no-slip condition for wall-resolved meshes). The code should add the rotation terms automatically based on the defined mesh rotation of the matching zone.