[Sasquatch]

Dear fellow CFX users,

I am simulating the flow over small-scale (10cm long) Radial Outflow Turbine which consists of 3 stages.

1stator: 12 blades
1rotor: 24 blades

2stator: 31 blades
2rotor: 37 blades

3stator: 30 blades
3rotor: 29 blades

I have of course simulated first a mixing plane model for the full machine but the early results show strong unphysical effects at the 1st stator/rotor interface. I contacted ANSYS twice about why my Mixing Plane model yields strong shock exaggeration but I have not received any reply for two weeks.

Thanks to Opaque's hint, I have easily found a workaround and a transient sim. for 1 stator and 2 rotor blades gave a smooth, physical result.

For now my conclusion is that: SS simulation for such small 1[mm] gaps fails to predict strong unsteady effects due to neglecting higher order terms.

I have also performed a successful Time Transformation method for the 1st stage as a check. Now, after adding the 2nd stator, analogically to the previous case, my model fails. My pitch ratio is 0.77 thus within the acceptable range.

Te solver expects one outlet which can be specified as:
TRANSIENT BLADE ROW MODELS: Inflow Boundary = <main inlet name> Outflow Boundary = <main outlet name> Option = Time Transformation . . . END

but I cannot find where I can modify it.
The previous 1stage case involved indeed 2 outlets from each rotor blade, and worked well...

I am puzzled by the boundary conditions.
Nr. of blades for S2 is 31, I need at least 2 passages per model.

The solver does not give any specific hints - just crashes which means that it is a 'fatal error'.

I am attaching the picture of the domain:

https://s31.postimg.org/grotk9x7f/Ti...rm_problem.png

or



Could you please help me track the source of my mistake?

Best regards,

[Sasquatch]

I have managed to make it run after initialization from a different file, I also added a rotor but the time transformation seems to fail for further stages and I am not sure whether for the 1st one too...

Here is the video of the static temperature:
http://sendvid.com/o0gegvn7

I have seen in the guide that between rotor and stator I could use profile transformation but CFX 16.0 does not allow for using time and profile transf. at the same time anyway....

Does anyone know what is the cause for such flow behavior here?

Kind regards!

[Thomas MADELEINE]

Hi Sasquatch,

first of all, TBR methods are quite old to me i will try to help you with what i remember (not as much as I would like).
And since english is not my native language, i hope that I have understood your problem and that there is not too much error in my answer.

I have look a little bit at your posts on the three threads (turbine stage, multistage and transient blade row), first tell me if i have miss something.

My first question is about the "small gap of 1 [mm]", is it the dimension of your domain in the span wise direction ?
The aim is to create a quasi 2D model ? if it is the case what is you boundary conditions for the hub and he shroud ?

For me the small dimension in span wise is no cause for bad result unless you have define no slip walls here.


In my opinion, I would use the frozen rotor option as initialisation instead of the mixing plane. Since you simulate the air flow at a certain rotational position, it works well for turbomachinery initialisation.

Other point (i have learned it the hard way), whenever you change your model (for example: by adding a passage in rotor or in stator, or adding a new stage), you have to remake an initialisation result (with frozen rotor for example). I do not know if you have done that or not, so if you did sorry...


I have not totally understood what you did qhat which simulation worked or not :
steady-state with mixing plane => converged but with non physical results
TBR-TT only the first stage => converged
TBR-TT for 1.5 stage => crashed and then converged with another initialisation
TBR-TT for 2 stages => converged but strange results (are you sure this isn't just a rotational offset problem ? look not that weird to me)


Normally TBR-TT works with only one passage for each rotor and stator. The easiest way for me to solve your problem is to merge the mesh of two blade into one domain.
However, I can not assure you that it will work for the odd number of passages (15.5 for the 31 blades stator).

If this doesn't work, the other proper way to simulate will be :
- from the first stage simulation, get the total pressure at the interface between S1 and R1 (in the R1 domain)
- create a simulation with the other stages (R1, S2, R2, S3, R3) with only one passage and implement a TBR-TT for a periodic profile at the inlet with the previous data

this could be quite time consuming, so see also what is the precision you want for this...

My knowledge on this is from R15 it could have change a little bit (before adding different type of TBR wasn't really good)

I hope I helped and didn't say too much crap.

I will follow what you do so please keep us updated of your results ^^

thnaks

Thomas

[Sasquatch]

Hello Thomas,

Thank you for your time. Answering your questions:

1. The small, 1 mm gap concerns the distance between the tip of one blade and the nose of another one. Therefore, it is the gap between the stages. The aim was indeed to create a quasi 2D mesh first. The spanwise thickness is 1E-04 [m] and of course free-slip condition has been applied.

2. I agree. Frozen rotor can be also used for the initialization, however, this is a matter of which option stabilizes faster. Once the simulation set-up is correct, I will study this issue but I think it was not the source of error now.

3. Initialization is of course respectively done from each SS model separately - I have also learned it after some hours of troubleshooting :P

4. Regarding the simulations, I have tried to read this forum and documentation cerefully before shooting questions but I obtained the following:

Steady state:

a) Mixing plane model for the first stage showed unphysical shock. I reckon this has to do with the numerical reflectivity and beta nonreflective BC is of little help here, since it is a stage interface, not outlet. Simulating the 1st stator only, proved that the shock is slighly smaller (probably because stator/rotor interaction does not occur) but more importantly - the shock is physical, even for the short outlet domain.

b) Mixing plane model for the machine proved similar issues.



Transient:

c) Transient simulation of the 1st stage was easy: 12 and 24 blades - no time transformation - the result gave a proof that a shock from the 1st stator spills over a rotor too a little - quite an unsteady flow - i was afraid that although it is the last resort, this is the only way to go.

d) Time transformation of the 1st stage also went well, but it was not needed - I wanted to check the correctness of my model.

e) Adding the 2nd stator and later 2nd rotor resulted in INFO: "only some combinations of disturbances are alowed, please refer to documentation"

-> This clearly means that my TBR Time transformation cannot be done for such config. and I cannot find why, I have read the documentation and it is still not clear.

Even though I obtained results for 1.5 and 2 stages, they are not valid and they converged only because I created only one disturbance because only this did not result an error of time transformation "combination". Even the one created, seemed not accurate, the offset, or angle shift you spoke about seems happening but why? E.g. the wake is translated too often. I am puzzled...

Regarding your last option: Thank you very much, it sounds complicated as I do not know yet how can I obtain such profile but this will be my next step if merging the domains fails.

Right now I work on the Ansys 17.1 - so quite up to date and there have been some breakthroughs there so maybe it will also make a difference.

Mixing plane is based on a circumferential averaging and I am wondering why my model yields slightly different results depending on whether between the repetitive passages I put "General Connection, None, None" or just leave it merged as it is without applying anything.

Both converge, at least for a 10k test meshes:

With GC interface between repetitive passages:


Without:


If someone is able to explain these phenomena, or at least some of them, I will be very happy if he/she could share them.

Best regards,

[Sasquatch]

Although I have received the following warning:

"In Analysis 'Flow Analysis 1': Multiple Time Transformations have been set up for Transient Blade Row Models. Only certain combinations of disturbances and domain interfaces are supported. Please refer to the documentation for details."

I have managed to run it with the following set-up:

TRANSIENT BLADE ROW MODELS:
Option = Time Transformation
TIME TRANSFORMATION: R1S2 Time
Domain Interface = R1S2
Option = Rotor Stator
TIME TRANSFORMATION SIDE 1:
Option = None
END
TIME TRANSFORMATION SIDE 2:
Domain Name = S2
Option = Domain List
END
END
TIME TRANSFORMATION: S1R1 Time
Domain Interface = S1R1
Option = Rotor Stator
TIME TRANSFORMATION SIDE 1:
Domain Name = S1
Option = Domain List
END
TIME TRANSFORMATION SIDE 2:
Domain Name = R1
Option = Domain List
END
END
TIME TRANSFORMATION: S2R2 Time
Domain Interface = S2R2
Option = Rotor Stator
TIME TRANSFORMATION SIDE 1:
Domain Name = S2
Option = Domain List
END
TIME TRANSFORMATION SIDE 2:
Domain Name = R2
Option = Domain List
END
END
TRANSIENT METHOD:
Option = Time Integration
TIME DURATION:
Number of Periods per Run = 1
Option = Number of Periods per Run
END
TIME PERIOD:
Option = Value
Period = 1.1603E-04 [s]
END
TIME STEPS:
Computed Timestep = 1.1603e-006[s]
Number of Timesteps per Period = 100
Option = Number of Timesteps per Period
END
END
END

The obtained result has a shifted wake, I can't find out why...:

http://sendvid.com/j98t2rw6

Regards,

[Sasquatch]

For those who were interested,

I have finally spoken to Ansys support and for now, Transient Blade Row, as a beta feature is still under development and multistage transient simulation might not work as expected, apart from some special cases (probably easy ones, like in the tutorials). I will have a webex session too and maybe sth more will clear out.

A big surprise, it is a very expensive package but maybe this will help sb to make a decision in the future.

[Thomas MADELEINE]

The Transient Blade Row method is a global method for harmonic simulation.

At the begining the only available features were for blade flutter and periodic disturbation inlet (both with fourier transformation if i remember correctly).

I am not surprised it is stilll under development but it could have been great that you can add different form of TBR method to adjust to your model...

and that centrifugal turbine/compressor would have been supported (with obvious big pitch ratio).

I hope it will be implemented in the near future ^^


And the option to merge the 2 passages in 1 to adapt to the "normal" TBR-TT didn't work ?

[Sasquatch]

Dear Thomas,

Yes, I have tried it, all the blade rows had their own passage (2 stages => 4 passages). Pitch close to 1.0. I managed to run, I iterated until 2 passing periods (maybe too little(?)).

I obtained the result, for the first stage, as always, good result (pitch ratio is exactly 1.0 so it is easy), but the interface R1S2 and S2R2 have faulty wakes in wrong places...

Best regards,