[Veronique Pe]

Hi everyone!

I'm looking for an example/tutorial with the use of Transient Blade Models - Fourier Transformation - in a case of Transient Rotor Stator? There is no Ansys Tutorial with Fourier Transformation AND Rotor Stator? (as tutorial #35, with Fourier Transformation instead of Time Transformation).

Thanks,

Have a nice day

Véronique

[Thomas MADELEINE]

I am not sure of what I am saying but I think that there is no example of a rotor-stator simulation with TBR-FT because it's not really the best choice for this kind of simulation.

TBR-FT needs 2 blades of a rotor (or stator) and can expand the domain for the whole rotor (or stator) after that. In fact the TBR-FT method will be usefull to simulate periodical disturbance in the flow (for example inlet or blade flutter)

But the fact that you need 2 blades (no more no less) is very painfull to simulate a rotor-stator (you can't choose your pitch ratio)

So that is why the TBR-TT is here for that, this method will allow to have a pitch ratio much worse than usual.

And I don't think it's possible to mix the both methods.

If you really want to have a stator-rotor simulation with TBR-FT, best thing to do is maybe to simulate your rotor first and later your stator with the inlet from your previous simulation.

Again I am not sure of what I am saying.

[Veronique Pe]

Thanks Thomas!

I need a TBR-FT because of my incompressible fluid. So, I can't use the traditional "time transformation". In any cases, with my configuration, I prefer simulate 2 rotor blades and 2 stator blades instead of the correct number of blades to obtain a pitch ratio near 1.
And simulate all the channels with a 360° calculation will be too long because of the number of cases I have to study.
Ansys support informed me yesterday that I need to activate the beta feature to access all options of Fourier Transformation, in particular Rotor-stator (without the beta fetaure, only "rotor flow boundary disturbance" and "blade flutter). This option is in CFX-Pre / Edit / Options / General / Enable Beta Features.

Yesterday, my CFX-pre was ok, I just need now correct some mistakes (about the initial value of R1 Velocity).

I keep in mind your idea to simulate rotor flow, and then the stator flow. Good Idea!!!

Thanks again,
Véronique

[Veronique Pe]

Hello,

With your solution, Thomas, I think I can't catch all the rotor stator interaction effect, for example the upstream potential effect which comes from the downstream row to the upstream row.
Maybe with successive calculations, one with rotor distubance as inlet stator disturbance, then with stator disturbance as outlet rotor disturbance, and so long...

This solution seems boring...

Have a nice day,

Véronique

[Thomas MADELEINE]

yep, if you separate the two domain in two different cases, you can expand the results of one domain to the other but can't go in the other way... you will miss some interactions.
I don't think the solution of coupling the runs one by one will take less time than simulate the whole rotor and stator...
It is kind of desesperate solution if nothing else works

[sfotovati]

I am doing the same approach to predict flutter in a gas turbine. There is a strong wake coming from the upstream stator to the rotor. to include that, I ran a steady state rotor-stator model. This runs quite fast. Then I extracted the total pressure, temperature, and velocities form the interface on the stator side. Then used them as an inlet profile for my TBR-FT case. It seems it is working.

Good luck

[Veronique Pe]

Thanks Shawn!

But in my case I need all the rotor-stator interactions, upstream and downstream.
At this day, no good solution purposed by my ANSYS-CFX support. Maybe in CFX 16.0....

[tonyOdili]

Good day every one,

Please I am new to simulation and I need help in carrying out a simulation work.

I am working on "The Effect of varrying blade angles of an impeller in a multage stage centrifugal pump". I am to varry the exit blade angles of a three stage centrifugal pump to see the effect it has on the output discharge, pressure and efficiency of the pump.

Anyone who is willing to help should mail me "odilianthony24@gmail.com" and we can discuss more on the topic and how much I will pay to get the work done.

Thank you.

[Thomas MADELEINE]

hi
the problem with the TBR-FT is that you need two blade for each stage...
in a radial compressor the volute chamber can't be simulated in the same time, I think.

If someone has a idea how to make it possible, I will be pleased to know it.

For me, it is really hard to use a TBR method to create a run with all your stage to catch all the effects of the blade angle of the impeller.

[Thomas MADELEINE]

By the way, how does your case work, Veronique ?
With the beta solution of TBR-FT in rotor/stator, I think you can have a really nice domain of your stage with only four blades (2 for the rotor and 2 for the stator).

I think you can do quite the same case than the tutorial #35 but with two passages of each blade domain in order to have the sampling interface...

if your run doesn't converge well, don't hesitate to extend the domain in the outlet: the waves of your blades can bounce on the outlet and decrease the convergence of your run...
if your outlet is pressure based, you can also use a radius averaged pressure in the outlet rather than a whole average outlet by default (not sure of its name)

[tonyOdili]

Hi Thomas MADELEINE ,

I will be glad if you can help me build a model and simulate my work with the analysis and we discuss a price.

Thank you

[Thomas MADELEINE]

Hi Anthony
if you can describe a little more your case I am sure than it is possible to make something not too complicated to simulate.
If you are new in TBR methods you will need to use the tutorials to make an idea of how it works.
If you create a new topic with your case, you will find easily people to help you in your analysis.