Rotor 37

[kemmerch]

Hello,

I am trying to run a simulation of NASA Rotor 37, using the frozen rotor model of Code_Saturne’s turbomachinery model. There is a picture attached to this post which shows a section of the whole geometry as the model for the numerical simulation.

The geometry was meshed with approximately 1.6 million tetrahedrons. The rotational speed of the rotor equals 1800 rad/s (Axis direction: –z).
I defined the blade together with the bottom surface of the rotating part of hub (light blue colored block of the geometry) as the rotating faces of the model.
Inlet conditions are:

Total pressure: 101325 Pa
Total enthalpy: 289850 J/kg

The static pressure at the outlet equals 90000 Pa.

Unfortunately so far I couldn’t produce any realistic results of the total pressure or total temperature ratios at the outlet face. The calculation starts and finishes after the predefined number of iterations without any warnings or error messages.

My question is, if this setup is appropriate for Code_Saturne? Especially when it comes to the boundary conditions and the selection criteria of the rotor definition for the frozen rotor model.

I appreciate your help.

Best regards,
Chris

[Yvan Fournier]

Hello,

We're missing many detail which could help answer you here:

- I am not familiar with this case. What type of flow Regime is this (Reynolds number, Mach number, ...) ?
- How do you test for convergence ?
- How far from expected results are the results you obtain ?
- How do you postprocess things ?

From your description, I assume this is a compressible case. I am not sure the compressible algorithm is compatible with the froze rotor (or even transient) model. It migh be compatible, but I am not sure this has ben checked for, and am not familiar enough with the compressible model to know whether no modifications, minor changes, or major changes might be required.

Best regards,

Yvan

[AndrewH]

Hi,

I wanted to make the comment that the compressible module (cfmspr/cfmsfp) assumes that the continuity equation is in an absolute velocity formulation and will only give the absolute mass flux. You need to re-write the code to calculate relative mass flux within the rotating domain and add a term into the total energy equation to allow for the compressible module to work with the turbomachinery module. Furthermore, the base code for the compressible module is limited to first order upwind for the convective terms.

From my experience with modelling the Rotor 67, 1e-9 s is also a very small step and it will take many iterations with a transient or pseudo-transient solver to reach a solution.

Best Regards,
Andrew

[kemmerch]

Hello,

Thank you very much for answering.

At Yvan:

Yes, indeed this case represents a transonic compressor with the following aerodynamic design parameters:

• Number of blades: 36
• Tip diameter at leading edge: 0.5074 m
• Hub diameter at leading edge: 0-3576 m
• Rotational speed: 17188.7 rpm (1800 rad/s)
• Tip clearance: 0.356 mm
• Tip speed: 454.14 m/s
• Pressure ratio: 2.106
• Mass flow rate: 20.19 kg/s

I am trying to model the flow through the Rotor and compare the results of the total pressure ratio and the total temperature ratio at plane location 'Stn 4' (which represents the Outlet of my geometry) with the measured data published by NASA Lewis Research Center.

So far I have monitored the listing file for convergence check and interrupt the calculation at time step number 2365 because of the unrealistic velocity values. I haven’t used the turbomachinery model before, so this is the reason why I am not sure how to properly setup a case in Code_Saturne.
I tried to get a first impression by checking the XML-File ‘radial_flow_frozen.xml’ which was uploaded by you earlier.
But for example I am not certain if this case requires a face joining and how to do this. Furthermore, does the Selection criteria among Rotor definition require faces or volumes to set the Rotational velocity?
Postprocessing will be done with ParaView 5.2.0.

At Andrew:

Thank you for your comment. Is there any chance that you can tell me how and where these changes have to be made? Did your setup showed good agreement with the test data? I am very interested in your work and would be really grateful if you would share some more details with me. I guess you are the author of the abstract 'Study of Rotating Stall in Centrifugal Compressor'?

Best regards,
Chris

[AndrewH]

Hi Chris,

For centrifugal compressors, I got decent results. For Rotor 67, I haven't been able to get any good results yet. The last attempt I made a few weeks ago was with a high CFL number and the solution diverged after a few ten's of thousand time iterations. I have been wanting to try again with a much lower CFL number but haven't had the time due to writing my PhD thesis.

If you want to make the turbomachinery module compatible with the compressible module, you need to make the velocity flux in cfmsfp relative for cells that are in a rotating frame. And you need to insert the term -grad((omega x r) P) into the RHS of the energy equation (cfener). These changes aren't too difficult to make but you need to make many other changes to get 2nd-order accuracy in space and not to be restricted to a CFL less than 0.8, like writing a MUSCL scheme and rewriting the algorithm into a pressure-correction algorithm. Although Code_Saturne is great open-source for most applications, Fluent/CFX might be worth a look if you have access to it and your're only needing a steady-state solution for Rotor 37. To get transient results for a single operating point with the NASA LSCC/CC3 took several weeks unless I was running a very coarse mesh. I don't want to discourage you from trying to model with Rotor 37 with Code_Saturne but I want to make you aware of all the headaches that are involved to get a good solution for a transonic compressor.

Regards,
Andrew

[kemmerch]

Hello Andrew,

I just want to give thanks to you for your description and sharing your experience with me.

Best regards,
Chris