Overpredicting Total-Total Pressure Ratio in Centrifugal Compressor
 

Hello,


I'm running a steady-state simulation for a centrifugal compressor using air. It's an openly available test case, the "MTU Radiver" compressor. The issue is two-fold, I'm getting higher pressure ratios than experimental values by about 0.5 even at different performance points (speeds/mass flows). So, boundary conditions that should produce a total pressure ratio of 2.5 according to the experimental results actually result in a 3.0 ratio. The second issue is that the total-total isentropic efficiency is around 88% when it should be around 75%.



I'm using the SST turbulence model. The boundary conditions are total pressure and total temperature at the inlet and mass flow rate at the outlet. The interfaces between the rotor and inlet/outlet are all frozen rotor interfaces. The simulations seem to be converging well, imbalances are within 1%, and there's no oscillation or anything. But, the final results are clearly off. I've attached the outfile, a screenshot of the run monitors, and the turbo macro "Gas Compressor Performance" report results.


Please let me know if any more info is required and thank you!

What fluid was used for the experiments? Air or a refrigerant?

What speed was used for the experiments? What speed are you using? Since you are way above compared to other published Ansys CFX results, you seem to be running at higher speeds.

Also, what Radiver use case are you validating Radiver, or Radiver 2?

Hi,


The fluid used is Air. The compressor is running at 28160 which is 80% speed. This is what most published results use as far as I can tell. Finally, it's the Radiver 1 case.



I have suspected that it could be an issue with the corrected values. The experiments were conducted with inlet conditions of 296K and 0.6 bar and then corrected to 288K and 1.013 bar. The operating maps are then all made in corrected values (speed and mass flow). For the simulations, I've used the actual conditions and found the actual mass flow using the typical formula. Am I missing something here? My supervisor seems convinced this is the problem area but I can't find the issue as I've double and triple checked the formula.



Thanks!

Have you done all the basic checks listed here: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

I did check all of these. The turbulence model I'm using is SST which I've from what I've read in several published papers is the best/among the best for centrifugal compressors. I've tried several different meshes, and I've spent most of my time checking the boundary conditions and they seem perfectly fine.



However, I did keep the turbulence intensity at medium (5%). Could that have a significant impact? I wasn't sure what to set it as so I kept the default. Also, how would you recommend checking the grid quality? I used TurboGrid to make the ones I've used and I tried to check the statistics it provides to make sure it's of a decent quality.



Thank you for the help, any advice would be really appreciated!

The critical checks which many forget is mesh size, convergence criteria and time step size (if transient).

The easiest way to see if your 5% incoming turbulence intensity is significant is to do a sensitivity check on it - run low (1% I think) and/or high (10%?) and compare. If it does not affect the results significantly then it does not matter and you can use anything. If it does affect results then you need to find out what the correct incoming turbulence is as it is a critical parameter.

If your grid is from TurboGrid then it is probably pretty good quality. Again, the best way to check if grid quality is important is to do a mesh with a very different grid (either much worse or much better quality - and I am guessing much better will be challenging, so I would do a much worse quality grid) and compare the results.

I am a bit confused by your setup. You said the experiments were conducted using Air, but your setup uses an RGP file for some kind of refrigerant.

Which one is it?

The Radiver 1 case has been simulated by several authors using Ansys CFX, and the results are within expectations; therefore, something is off in the setup. Secondly, your results are not even close which points to more than mesh resolution, or convergence (which yours is very good).

Either the wrong fluid, boundary conditions, or machine speed (direction).

Hi,


I'm sorry, I realise the confusion. I posted two questions which are for two different cases. Part of my thesis project is validating certain results on different compressors. This one is the Radiver compressor running on Air. My question from a few days ago is on an in-house compressor that uses R1233zd which is the one I was using an rgp file for.

And yes, I agree, the results being so far off speaks to a more fundamental issue, I just haven't been able to find it. I guess it could be the rotation direction, that is the only thing I haven't looked at. I spent a lot of time testing the boundary conditions so I don't think that's it. As for the fluid for this case I'm just using Air at 25C from the built-in materials so I haven't edited that at all.



Again, sorry for the confusion, I should've clarified. I'm trying to simultaneously fix the issues with both of these test cases on a tight deadline. Thank you both for your comments! I'll explore the rotation direction and the turbulence intensity, but any other ideas are greatly appreciated.

Sorry, that is your problem.

You MUST use Air Ideal Gas. Air at 25 C is an INCOMPRESSIBLE material

Ok, then we've found the problem area. Thanks a lot. The issue is that I've tried to use Air Ideal Gas just to check but I immediately get errors within the first few iterations and the run stops. I'll run it using Air Ideal Gas and report back with the specific error code. Thank you!!

Hi,



Indeed the run errored out after 28 iterations. I've attached the run monitors and the outfile. You're right of course. Air at 25C is incompressible and it was a big mistake to use it without learning more about it. When this error occured last time I just assumed that Air Ideal Gas was the wrong choice and switched the fluid.


The main thing I notice with this run is that the Mach Number is increasing rapidly. The error occurs when it suddenly spikes to e08 magnitude which is clearly problematic. Why this is happening though I can't say. Please advise, thank you very much!

A few things from the output file:

1 - Based on node count, without real mesh scaling/metrics, information, the mesh seems way too coarse. Perhaps it is good, but just a warning
2 - I am not familiar with the Radiver operating range; therefore, it is important to know if the setup is about the choke point, design point, or stall/surge point.
3 - I am a bit surprised the automatic time scale including the Timescale Factor is so small compared to the Advection Time scale reported. How does it compare to the rotation speed timescale, usually @ 0.1/omega (in rad/s)?
4 - How uniform/flat is the region around the selected operating point?

Compressor modeling is tricky when the performance curve is fairly flat and only drops near choke. The guidelines for Ansys CFX is to use the exit corrected mass flow option since it is more robust unless you have a better insight into the machine behavior.

Hello,


1- I did make a 2.5M node mesh (this one is 1.42M) but it didn't make a real difference so I used the smaller one to speed things up a bit. But considering all those runs were using Air at 25C it is certainly worth looking into again.

2- It is rather flat at this part of the curve and far from the choke and the stall points but I'll try to play around with it and see if that could have an effect.

3- I might be using a too small timescale factor (starting at 0.1). The rotation speed is 28541 RPM = 2989 rad/s so the rotation timescale would be 3.35e-5. I don't think this could be causing any issues, right?

4- See 2


Finally, I haven't used the exit corrected mass flow option before as I've been using the actual mass flow as my outlet boundary condition, but it definitely sounds interesting. Could you please tell me where to find it?

I really can't thank you enough. You've been a great help!!

When doing turbomachinery modeling, I use a timescale of around 1/omega unless there is another more restrictive timescale.

Going smaller is good when the convergence is unstable; however, going smaller when it is not needed will start capturing useless pseudo-transient you are not interested in and will require more iterations to obtain the converged solution.

Exit-corrected mass flow is available at the outlet for compressible material. If it is not available in the UI, either you are using a very old release of the software, or your material is not compressible.

Hello,


I'm happy to report that the simulation was successful. I achieved a pressure ratio (which is the main result I'm looking to compare) within 4% of experimental results. With a stable convergence. I still have to perform high-resolution runs, and the residuals weren't as low as I'd like but all the important monitors were stable at good values.

Thank you very much for all your help. You diagnosed the issues well at every stage. The final hurdle was indeed the timestep, the high mach numbers stopped being an issue afterwards, I imagine they could have been psuedo transient effects that were affecting the solution somehow. In any case, 0.1/omega was the right call. Thanks again and have a good weekend!