Surge simulation
 

Hi !
I am going to perform surge simulation of centrifugal impeller with vaneless diffuser. I managed to calculate steady case and noticed big turbulance inside impeller. I also tried harmonics unsteady model, however it seems to be just for rotor/stator interaction (correct me if i am wrong) - results don't change with time. Is it possible to model surge in NUMECA turbo ? Which unsteady model should I use ? Does anybody have tutorial of such case ?
Best regards,
Piotr

Hi Piotr,
you are right, non-linear harmonics unsteady method does not work in your case, because you have no rotor-stator or rotor-rotor combination(s) in your machine.
Besides the NLH-method you can use the standard unsteady method.

Hi,

Thank you for your sharing.
Do you by any chance know if the NLH-method could work in a compressor with a volute, or it may only work in blade rows?

It works in a volute, too (compressor and turbine). But make sure to mesh just one blade passage of each row. The blade passage of each row needs periodic boundaries in circumferential direction. If you are interested in the background of this please ask, I could try to draw a sketch to explain the reason.

Daryl,
Should I use domain scalling method or phased-lagged one ?

Hi Piotr,
the advantage of the phase lagged method is a reduced CPU time needed for unsteady computations. But it is only allowed for one-stage machines (stator-rotor) or 1.5-stage machines with the same number of stators.

Domain scaling is the only available unsteady method for you then.

Daryl,
I am really grateful for your advices. I haven't checked Rotating Boundary Condition in Boundary Condition option. I used steady result for initial solution. In control variables i have to input physical time step. In NUMECA manual i found following formula:
http://www.cfd-online.com/Forums/dat...BJRU5ErkJggg==
As i understand omega is rotational speed (in my case 9000RPM), Nperiods (number of blades=21).
Could you please tell me how to calculate NOFROT ?

Hi Piotr,
you are right, because you have no rotor-stator interface you have to calculate the physical timestep size manually. The following questions lead to the desired duration of the physical time step.

1. What is your rotational speed in [rad/s]?
2. How far in [rad] must one blade rotate for one blade passage?
3. How long does this take?
4. With how many time steps do you want to resolve one blade passage?

If you are lazy have a look at the attached file. ;)

Hi Daryl,


All you have explained works good.
Further I would like to know few more things for an unsteady simulation:
1. How does dual time stepping method helps for solution convergence ? What actually does it do? I have gone through manual. It says for each iteration, dual time stepping method performs internal calculation to meet set residual level. I couldn't actually get all from this.

Also how many iteration steps to be defined for this(default 100 seems large to me).
Or Does it have to do with number of computations performed for one instantaneous position of rotor and stator(please correct me)?



2. In the control variables menu under time step, two buttons are available:
a. Number of angular positions(default value 30)- Does this number represent, for one passage sector total number of rotations or for the given mesh the total number of rotations. e.g. say row 1 has periodicity of 21, so will this number be = (360/(21*30)) deg or if the mesh is full annuls, the number will be = 360/30 deg rotation in each time step.

b. Number of time steps : As I could get, this means total number of iterations which will be performed, correct me if I am wrong.


Also I am not sure, where to specify number of iterations for an instantaneous position of rotor and stator.


Please clarify my doubts.
Also I would to know, are there expert parameters in fine turbo to tweak to get good near stall experimental validation(in my case, numerical stall mass flow rate is almost 5% earlier than experimental data).


Thanks alot!!


Kind Regards
Vishwas

Dear Vishwas,

Dual time stepping isn’t a NUMECA specific idea to accelerate convergence. You can search this forum and will get a thread with a lot of information and dual time stepping papers.

The maximum number of inner iterations = 100 is too large for most turbomachinery applications. From my experience 20 is enough, use 25 if you are very conservative. You can check the convergence of the iterations during your computation in the monitor (accessible at the top bar). In the monitor, in an unsteady simulation not the iterations, but the inner iterations convergence is plotted. This means if you compute 1.000 time steps with 20 inner iterations you will see 20.000 “work units” on the x-axis. This makes it possible to check the convergence of each iteration (check mass flow, efficiency and pressure ratio). You should focus on regions with high gradients between the time steps. As a rule of thumb the maximum number of inner iterations need to have a higher value the larger your physical time step size is, as the difference of the flow field between two iterations is bigger then.

Number Of Angular Positions refers to your mesh! An example: 36 blades and one meshed passage means your mesh contains of 10° (360°/36). If you choose a number of angular positions = 10 you will get an unsteady result every 1°. On the other hand, if you have meshed all passages (36 blades) you will need to define a number of angular positions = 360 to get the same time resolution, as your mesh now contains of 360°.

The Number of time steps is the total number of time steps for your computation. If one period contains of 360 angular positions and you define 3600 Number of time steps you will compute 10 full periods of your application. You should start from a converged steady computation and do at least 3 or 4 full periods, but you will post-process only the last one. The reason is that unsteady fluctuations at the beginning vanish during the first full periods. If everything goes right you will see a periodic behavior of the flow quantities after 2 or 3 full periods.

Unfortunately, there are no expert parameters to get the same numerical results in comparison with experimental data in stall region in general. But as a general recommendation you can define inlet profiles for the velocity components or total pressure/temperature or even the turbulent quantities, if they are available from experiments. Usually, profiles yield a more realistic flow field than using constant values.
Secondly, especially in the stall region a lot of flow separation takes place, which amount and behavior can highly depend on the chosen turbulence model. Please keep in mind that you can use the numerically efficient turbulence model EARSM (Explicit Algebraic Reyolds-Stress Model), which assumes an anisotropic behavior of turbulence in contrary to one- or two-equation turbulence models like SA, SST or k-epsilon. This can lead to a more realistic flow prediction.
Thirdly, a high-quality mesh with y+ values around 1 (if you use a low-reynolds turbulence model) can help to achieve more realistic results, as the boundary layer flow is well predicted then.

Hint: Once the unsteady computation has started you can open the .std file in the computation folder. Search for the string “TIME STEP”. This is the physical time step size, which is computed by FINE/Turbo. You should check if this value is as expected.

Kind regards,
Holger

Dear Holger,


Thankyou very much!!


Kind Regards,
Vishwas