SST turbulence model
 

Hello everyone,

I have two questions concerning the SST turbulence model:

I am analyzing a very complex flow in a compressor.

For my CFD-STAGE-SETUP, I have chosen the BSL- and the SST-model for a comparison because they combine the advantages of the k-eps and the k-omega models. Both models predict totally different flow structures (separation) - and the SST model seems to be wrong (compared to experimental data)! Even more, both models totally overpredict the total pressure ratio.

1.) From an analysis it came out that the limiter of the turbulent eddy viscosity is the reason for the mal-prediction. If I slightly increased the coefficient, the separation is predicted correctly with the SST-model
.
Can anybody refer me to a paper/book etc. where I can read why this -coefficient is set to 0.31?

2.) I do have the impression that the overprediction of the total pressure ratio is due to an overprediction of mach number (close to Ma=1.00) near the stage interface of the rotor. Has anybody an idea what I could change in my setup to decrease the overestimation? (Of course, I have already ensured that my BCs are correct)

Thanks.

You would have to follow up the references listed in the documentation for discussion of constant values.

Why do you think the production of k is the cause of the problem?

Have you looked at all the additional stuff SST can do - curvature correction, turbulence transition? Have you turned these on to see if they help?

I have used curvature corretion already but the impact is very small. Especially the separation does not change.

I have tested transition very shortly since I had huge problems to get it converged. Which approach would you suggest?

Often the turbulence transition model needs a transient approach to get convergence. Did you run transient?

And are you sure of things like surface roughness, inlet turbulence levels and things like that? I would check these before tuning constants.

I didn't use a transient approach. I doubt that this makes much sense due to the blade-numbers. Even if I just tried to resolve the unsteadyness in each domain (no blade passing-phenomena), I have real doubts in this approach.

I am using smooth walls - this is an adequate assumption. yes, I am sure about the BCs.

I see. Do I understand you correctly in that you have assumed a frozen rotor approach, so does not include transient flow effects or blade passing effects in a complete fashion.

same problem
 

Hi PCFD,

I'm working on a compressor too, and using SST model. In my simulations, there is a huge separation starting form the trailing edge of the impeller. I assume, that it's not a real phenomenon. Can you please describe your problems with SST and these separations more detailed? Maybe we can help each other:D.

Best Regards,
Attesz

Hi,

I have a separation too but this one is within the stator.

I am using a stage-interface for modelling the rotor-stator-coupling. The interface is very !!close!! to the trailing edges of the rotor. Generally I would prefer to put the mixing-plane in the middle (between rotor and stator) but in my case this is not possible. The mixing plane type is: Constant Total Pressure + STATIONARY, Implicit Stage Averaging = On, Pressure Profile Decay = 0.05.

The SST-model predicts the separation in the stator on the wrong side (default settings!). The k-omega model predicts the separation on the right side but totally overestimates the stage total pressure ratio and efficiency.
I have the impression that this is due to an overprediction of the mach number within the rotor. By the way, the outlet mach number of the rotor (in stn frame) is very close to Ma=1.0.

An overprediction (~2%) of the mach number level easily leads to an overprediction of the total pressure
. Assuming that the static pressure is correct (and I have compared it with measurements --> very good match), you can easily see that high mach numbers lead to significant total pressure differences (~0.1 bar).

So, for my case the k-omega model is definetly preferable. Anyway, I am asking myself what could be the reason for the over-pressuring within the impeller.
My first guess was the mixing-plane. Do you have any other suggestions?

Hi,

the next week I will write you detailed answer. But I think, the overestimate is not wrong, because we don't calculate with the losses (friction loss etc.)...
Attesz

Hi,

I am excited to hear your explanation but I would like to add something in advance.

The stage which I am analyzing numerically is investigated experimentally too. We have static pressure measurements on the casing (in streamwise direction) of the rotor and these data fit nicely with the numerics. The total pressure is measured very close behind the rotor - and there I can see big differences (in total pressure distributions). This leads to my conclusion that the mach number level is not correctly predicted. Within the stator the deltas between CFD and experimental data are more or less constant.

I would like to ask two more questions about the CFX-mixing plane model:
1. What is the idea behind the pressure profile decay? The explanation from the manual does not help me at all. Is there a paper which explains the approach?

2. CFX 12.X supports a feature which is called "Iteratively implicit pressure averaging at stage interfaces and outlets". This feature is really unstable in my case because all simulations with this option did diverge. Is there a certain way how I should use it? In which cases does it make sense/is is necessary to use this option?
(By the way, I have to use "implicit stage averaging at stage interfaces" - otherwise I do see massive fluctuations on the stage interface in the total temperature average.)

Thanks

In the release notes for V12.0 or V12.1 it should describe a method to turn this feature off and revert the previous behaviour. Is this what you are doing to obtain convergence?

Hi ghorrocks,

I do not understand your last post.

Up to now, I did _not_ us the option "implicit pressure averaging" because my stage simulations became instabile with it (in v12.0). Right now, I am testing "implicit pressure averaging" in v12.1 with a rotor and an "artificial stator". As far as I can judge, the implicit pressure averaging option does not negatively impact the convergence. The next step for me will be to switch this option in the stage-simulation on.

I am already using "implicit stage averaging" since v12.0. This option is really helpful for tightly coupled rows. Before I could use this feature, I have seen strong oscillations in the massflow-averaged total temperatures on the stage interface.

Hi PCFD,

I could read your post detailed, at least. It's very interesting what you say(write), because I think, we have a similar problem since half a year. We have tried stationary and transient simulations, stage, frozen rotor and TRS interfaces. We moved the interface close or far from the leading edge, used fine and coarse mesh, 5 or 12 element in boundary layer...without results. In our problem, the compressor stage seems to have a lower performance, so lower pressure ratio, efficiencies etc. We reach the surge at lower PR than the operating one. There are also measurements, but in our case, the simulation underestimates the performances. Theere is a huge separation at the leading edge, and by overestimating its size can occour this phenomenon.

Now we want to change the turbulence model, or its constants also, because we have not any more idea. We try k-E and RNG k-E models. Ramping up the rotating velocity and pressure ratios had not results also.

Are you using periodic model? If yes, how about the pitch ratios? I have a pitch ratio=2 between the rotor and the stator, i think, frozen rotor is invalid, but stage can work.

An other idea. If there is a big separation in the flow field, it is a transient phenomenon. But, If we run stationary simulation, this separation will be averaged, so mostly overpredicted. Bigger separation means lower flow areas, lower performance, which appears in my work. Has anybody any idea how to avoid it? Maybe should change the timescale values?

Thanks for any advice.

Best regards,
Attesz

Not necessarily. But it can be.

Why do you say this? I can't see a justification for this.

For a steady run, once the residuals are converging nicely you should increase the physical time scale to quite large compared to the fluid timescales. This should still converge quickly, but should allow the flow to "average" as best as possible.

Hi Glenn! Thank you for your answer!

I think it can be, because if the separation fluctuates than its a transient phenomenon, but If I run in stationary, the separation "stays there always". We get this result by comparing a transient and a steady simulation, and in trans. we get 30% higher mass flows than in steady. But of course, it can caused by anything else...

I don't know how to do this. Do you mean the fluid timescales which displayed in out files, or for example displayed in post, on a streamline by setting variable to "Time on streamline". How to compare these timescales? If I have 1.6e-4 timescale value, I should set the physical timescale to 3e^-4 or higher, as you write it?

Moreover we started simulations with SST, k-e, RNG k-e turbulence models, in the same operation point. I will send the results.

Regards,
Attesz
Attachment 2756

Hi Attesz,

what you call "separation" is the wake-region of an impeller. This region contains low-momentum fluid but it is not necessarily seperated. This flow-structure is well known phenomena in radial compressors.

You will find a good explanation of it in Ziegler's measrurements/diss.

Regards, PCFD

What I mean by fluid time scale is the time taken for the fluid to go from the inlet to the outlet. So if you fluid time scale is of the order of 1e-4s then you should be able to run physical time scales of 1e-2s. If you go too large it will diverge but you want to run a time scale several orders of magnitude higher, not just a little bit higher.

PCFD's comment is important - the different turbulence models will capture this wake region differently as they all have different accuracy in shear layers.

Yes I know the wake-jet regions in impellers, but this weak is on the wrong side, i think. The operation is at PR1, low RPM, so it's very strange.

What do you think, can we capture this phenomenon with steady simulation, or is it fully transient? Or we need more studies to decide it? On the operation point, most of the compressors can be simulated in steady state, as I read it in literature...

I'm sorry, but I don't know what is this...:rolleyes: Thank you!

Thanks Glenn again!

Regards,
Attesz

Could you post a S3-plot of the relative mach number near or behind the impeller trailing edges. this will help me to understand your jet-wake structure. The position of your wake-region strongly depends on the intensity of your secondary flows (within the impeller).

I was talking about the PhD-work of Ziegler. He analysed the testcase RADIVER which is (to my mind) a very good work! He explains several phenomena in a radial compressor in details, so you should look at his papers.

It is hard to say if steady methods will help to analyse your case. As far as I can see on your picture, the radial gap between impeller and diffuser is not very small. So, steady CFD should be able to handle this. (By the way, in my case the mixing plane is even _much_ closer to the rotor-trailing edges).

What about your residuals and Yplus-values?

As ghorrocks mentioned, I would be very careful with changing turbulence model parameters. If you really think that you have to do it, contact an ANSYS-turbulence-expert and discuss the issue with them!!!
Generally speaking, I think that the SST-model, which is implemented in CFX, is a very powerful model. But in my case it does not converge too. Have you been using the k-omega model for your case (with curvature correction v12.1!!)? In this case, check your eddy viscosity ratio near the impeller outlet (a circumferentially averaged plot would be representative). I would not wonder if the SST-model showed much lower ratios in comparison to the k-omega model.

I don't know exactly what is this S3 plot. However, I've attached some contour plot about Mach numbers.

The solution is well converged, as you can see on the pictures.

But there is an error in temperatures at the interfaces (picture4). Can it caused by the mesh difference between the sides (picture5, green highlited mesh), or the GGI method can handle this, so caused by for example the pitch ratio? High pitch ratio (in my case this is 2 between rotor and stator) can cause big numerical errors?