[kjetil]

Hello everybody,
I am trying to simulate stall in a diffuser (low liquid flow). Currently both steady state and transient simulations overpredicts by far - stall occurring at over twice the flow rate than what is found in experimental data. Quite a few parameteres have been checked, including mesh quality (y+), timestep and numerical schemes.

I am now experimenting a bit with the turbulence models, as I fear that the SST model might be causing parts of this. I read that SST might not work well in curved geometries, or with secondary flows, and here I have both. I have therefore tried to turn to RSM models, with the obvious difficulties to get this to cooperate at all.

Observing numerous "FINMES" errors, still with even lower timesteps, I conducted a planned near crash, and was able to store the .res file. Highest residuals are then found close to the interface. Mesh is overall good, though not quite uniform across the interface, and aspect ratios a bit on the high side in this area. Could this be causing the errors?

Though, looking at the partially converged RSM simulation, the flow pattern is much more what is expected, that is - without the blockage/stall. I was also trying to find some other differences between these two simulations, and found that the eddy viscosity plots to differ quite a bit. They are attached here. Turbulence numerics are first order, but advection "High resolution". Switching RSM simulation to "High resolution" turbulence cause only eddy dissipation to converge differently, and whole simulation to crash earlier than with first order.

So my questions are:
- should I try to improve the mesh near the interface?
- should I coarsen the mesh?
- other experiences with turbulence models for initial run, before running RSM? My current runs here are initialized from a fairly stable run on higher flow, then flow is gradually reduced in steps by an expression. Though do not converge, possibly due to the mesh problems mentioned. I did not have any good experience with initializing with SST runs on same flow.

[ghorrocks]

Yes, the mesh size jump over the interface is probably contributing to your convergence problems. So making the interface mesh size more uniform will help.

Coarsen the mesh - for development of the model yes, it will help. It will run fast, give you a rough idea of the flow and converge easier. Only refine the mesh once you are happy of the simulation setup (which includes turbulence model).

Flows in stall are not well captured by any RANS turbulence model, including RSM. I would consider SAS, DES and other LES type models.

Also note there are lots of options with the SST turbulence model, including curvature correction models. I would try them too.

[kjetil]

Thanks. Wouldn't it be a risk that SAS-SST fallbacks to URANS with possibly similar effects as the SST currently gives? I know Menter now promotes SAS over DES and LES, but it also seems to rely on a high quality grid. Would it possible in CFD-post to distinguish which regions are treated with what turbulence model?

[ghorrocks]

I do not use these turbulence models so cannot answer detailed questions on them. But I am sure there will be a variable to show which regions are URANS and which are LES.

But I do know that stall is very difficult to predict accurately with RANS models, and that turbulence models from the LES family are much more successful in these applications. Exactly which turbulence model from the LES family I will leave up to you

[kjetil]

Just to clarify myself a bit - just finished reading through the SAS-SST paper; this turbulence model is fairly independent of the grid resolution. Instead the resolved turbulent structures depend on the given timestep. For high resolution time steps the SAS-SST will behave LES-like.

(I intend to try this out specifically for the case mentioned above.)

[ghorrocks]

Sounds good, let us know if it works for you.

[turbo]

For me, "stall occurring at over twice the flow rate than what is found in experimental data" sounds weird. There must be a fundamental reason for the huge gap in somewhere else, not the turbulence models. I do not think the choice of turbulence model will predict the flow rate as much as TWICE.

[D.B]

As an addition to the point made by turbo, you can cross-check your pressure ratio vs mass flow chart at 'normal' points with experimental data and see if they match, if not, then check your problem setup and post-processing.

Cheers,

[kjetil]

I don't have anything conclusive here yet, except from that the SAS-SST alone did not solve this. As expected maybe. Though I have been digging in some historic matter and found simulations from 2009 with far coarser mesh that actually succeeds in simulating this, but then for a different design. I ran these over again in v16.2 and v17, and code seems to produce similar results.

I have scoured the settings and mesh quality, and so far come across the Kato Launder limiter as one of few differences. Reading the documentation in software and the CFD-Wiki it sure seems relevant, though I am uncertain to apply the Kato Launder or the fixed Clip factor. It seems the Clip factor of 10 is set/tuned for aerodymic applications, and my case is for water. Any recommendations here? I will certainly do some experimenting also.