Nonlinear Harmonic (NLH) method in Numeca
 

I want to do NLH analysis using Fine/TURBO for contra rotating fan ( two rotors rotating in opposite direction ) and I need some one to send me step by step procedure of NLH approach with some tutorial .
thank you in advance

Of course we can assist you to guide you through the process. At what point of your project are you exactly? I will see if I can get a helpful tutorial tomorrow.

Dear DarylMusashi

thank you so much for ur fast response; For my contra rotating fan case mesh is done using AutoGrid5 and steady analysis is also performed and now I want to switch to unsteady analysis using NLH. For instance if I choose Basic NLH then how I can determine 1) No. of frequencies per perturbation
2)max no. of perturbations per blade row
in reconstruction
how we determine
1)no. of harmonics per perturbation used
2)no. of time steps
in Rotated rows and number of channels
how we determine
1) no. of channels represented
2) displacement of the pitch
for ur information
In my case number of blades of rotor-1 is 19 and that of rotor-2 is 17 and both rotors have the same design RPM.

thanks

Hello Tegegn,

a) The maximum number of perturbations per blade row is 1 in your case. You have a machine with 2 rotors. Each rotor is affected by the other rotor.

b) You can leave the number of harmonics to resolve the perturbation at its standard value 3 to get good results. You may increase it to five, but that needs more computational time. In CFView for reconstruction you should use the highest value you defined in FINE/Turbo.

For reconstruction you need to set two things: time steps and the number of periods, which is 1 by default. The number of periods can be interpreted as the ratio of your lowest frequency (minimum blade number*rotation speed) and the frequency of your blade you are interested in. The frequency you want to resolve is in your case (blade number of row 1* rotation speed) + (blade number of row 2 * rotation speed) because both rotors are rotating in the opposite direction. In short terms I would try p = (17 blades * rotation speed [rad/s]) / ((17 blades * rotation speed [rad/s])+(19 blades * rotation speed [rad/s])). As you said both rotors have the same magnitude of rotation speed, so it can be canceled out. You have 17 / (17+19) which is approximately p = 0.5.

The number of time steps depends on how fine (in time) you want to resolve the flow field. This leads to the question how long one time step should be. Unfortunately the duration of a time step cannot be defined during reconstruction (only the number of time steps). At my actual project I resolved the rotation of the rotor of interest with a resolution of 0.15 rad/time step. As you know your rotation speed in rad/s it is 0.15 [rad/time step] / rotation speed [rad/s].
One hint: After reconstruction you should load the second reconstructed time step, go to "quantity, time label". Now the duration between timestep 2 and timestep 1 is shown. This is your actual timestep size. You can increase your duration of your time steps by increasing p and/or reducing the number of time steps. You can reduce the duration of your time steps by increasing the number of time steps and/or decreasing p. To keep the time step size fixed and simulate a longer time period keep the ratio of p and number of time steps fixed (multiply both with the same factor).

If you set the "number of repeated blade channels" to 0 only ONE passage is reconstructed. The flow field is identically in every passage in your machine. On the opposite set it to "max" to let CFView calculate the flow field separately for every passage. This is the most realistic way, but consumes very much disk space.

I would recommend to do some "slim" reconstructions at first until you are sure you have the desired time step lenght. Therefore choose only one variable (e.g. static pressure) for reconstruction. Reconstruct only 2 timesteps and set the number of repeated blade channels to 0.

If anything is fine until here you can check how large the CGNS files for every timestep become, when you reconstruct all other variables. Finally you may increase the number of repeated blade channels to its maximum (the limit is your disk space). Of course it depends on your mesh, but it is not uncommon to get CGNS files for every time step, which are several GB large. You should also check if your machine is able to handle this (the RAM will be the limiting factor).

NLH method in Numeca
 

Dear DarylMusashi

Great thanks and appreciation for your kind help and guidance

I will try according your suggestions;in mean time I have some more queries:

1. minimum size of mesh in stream-wise,pitch-wise and span-wise direction;is there any restriction on lower limit?
2. Max no. of interaction of harmonics between the upstream row and the downstream row of the reference row in Multi harmonic method. is the default no interaction is works fine for my case? or can I choose interaction option?
3.In the Harmonics page of the Outputs/Computed Variables page,can I tick both real and imaginary part and amplitude part or only real and imaginary part of a given variable like pressure,velocity etc?

thanks

Dear Tegegn,

did you read it in the FINE/Turbo handbook, or why do you want to use multi-rank method? The handbook mentions exactly your case I think?
"For a contra-rotating open rotors (CROR) case, if the pylon of the CROR mounted on the fuselage is taken into account, then the reproduction of its unsteady effects on the flow in the rotor that is not adjacent to the pylon cannot be performed by the basic/clocking harmonic methods."

1.
Do you use Autogrid for meshing?
If so, you can consider the grid quality report after generating your 3D mesh (min. skewness, max. aspect ratio, max expansion ratio). The skewness should not be below 20 in every row, the aspect ratio should be below 10000 (roughly) and the expansion factor should be definitely below 2.0). Very generally spoken a good boundary layer mesh then has approximately 1 million cells per row. If you use Autogrid during the "row wizard" process you are asked for the number of flowpaths in every row. Here a value between 50 and 70 are advised. I think 57 is the default value.

2.
"The maximum order in interaction is set by default to the number of harmonics of rank 1. This number can be reduced but cannot be lower than 1 or larger than the number of harmonics of rank 1. For example, a max order in interaction of 3 will introduce the interaction of the first three harmonics from the upstream row and the downstream row into the reference row." (FINE/Turbo handbook)
I would use the maximum possible number of harmonics in your case.

3.
"If a box is checked, the Real & Imaginary parts and/or the norm (Amplitude) of the complex amplitude of the harmonics of the variable, can be stored in the output ".cgns" file." You can tick both, but please keep in mind that your CGNS files get larger and larger the more ticks you set here. But I don't know how much the size of the CGNS files is affected by adding additional harmonic outputs.

Dear DarylMusashi

Yes I have gone through FINE/Turbo user manual and still I am referring it. My case is not CROR, mine is ducted Contra rotating fan proposed to be used in turbo fan engine. So my confusion is either to use basic Harmonic method or multi-rank harmonic method?. " The basic harmonic method deals with rotor/stator interaction of only adjacent rows". My case is rotor/rotor interaction, not rotor/stator interaction. " The multi-rank harmonic method considers not only the perturbation from the adjacent successive N rows of the reference row, but also the interaction of harmonics between the adjacent successive N rows". I am thinking to use multi rank harmonic method with rank-1 but the manual says multi rank harmonic method with rank-1 is similar to basic harmonic method. which one to use is my confusion.

I will apply other comments you have mentioned.

Thanks a lot

Dear Tegegn,

to clarify:
Basic NLH is a rank 1 method: In a multistage machine only the interactions of the neighboring rows are simulated.

Clocking NLH is a simplified rank 2 method, which means the interactions of row 1 and row 3 (row 2 and row 4) are simulated, too. The limitation is a same rotation speed of the rows.

Multi-rank NLH is a generalized method, the rows can have different rotation speeds. At the moment the multi-rank NLH is limited to rank 2, but will be surely further developed in upcoming versions.

----

In the handbook at the multi-rank NLH chapter it is referred to CROR. It is mentioned, that the effect of the pylon to the rotors cannot be simulated by basic NLH or clocking NLH. If you understand the pylon as a stator you have the following machine: row 1 (pylon, stator), row 2 (rotor I), row 3 (rotor II). In short terms it is mentioned, that with basic (rank 1) method the effect of row 1 is only transported to row 2. The effect of row 1 to row 3 is not simulated (because of rank 1). Clocking method does not improve this situation of course, because row 1 and row 3 have different rotation speeds. Therefore it is advised to use multi-rank method, rank 2.

BUT... you said you dont have a CROR but a ducted fan in your case, so I strongly suppose you dont have pylon. But you may have an IGV?? Then it would be the same situation as described above and in the multi-rank NLH chapter in the handbook.

If you have an inlet guide vane or any other kind of stator before your rotors you need to use multi-rank NLH, rank 2. Only now the effects of the stator on the second rotor can be simulated.

If you dont have a stator (IGV, pylon) before your both rotors you can use basic harmonic method, rank 1. Now row 1 effects only the neighboring row 2 and the other way around. As you dont have any other rotors or stators in your machine this is sufficient.


You struggled about the sentence "The basic harmonic method deals with rotor/stator interaction of only adjacent rows" and mentioned, that you dont have a rotor/stator but a rotor/rotor machine. It is not important if it is a rotor/stator or rotor/rotor combination. What they wanted to point out is the fact, that with basic rank 1 NLH only the neighboring rows effect each other.

I think the handbook was just written for standard turbomachinery with alternating rotors and stators.

Best regards,
Holger

Dear Holger

Thank you so much for clarifying my doubt,I will inform you the out come of my simulation .

thanks,

Tegegn

post processing in NLH method
 

Dear Holger

I have successfully reconstructed both Basic NLH and Multi-rank NLH with 1-rank simulation. Now I am facing how to post process the simulation;for example how can I do contour plot of say static pressure or axial velocity for at some location of the blade span say 95% of the blade span for the given time step. I have tried the way we do for steady analysis :go to quantity-field-basic quantity-static pressure and then representation-colour contour-smooth/strip. The contour value of static pressure it displays is some thing which is difficult to understand.so I need some guide lines for post processing NLH simulation results.

thanks
Tegegn

Dear Tegegn,
to generate a contour plot of the flow variable of interest at span 95% do the following, (please have a look at the figure):
1. Click blade-to-blade under the Surface tab
2. Set S=0.95 for 95% span position
3. Click Apply, click Save

Now in the surface tab a new cutplane "CUT1" is generated. You may switch to turbo machinery mode (File-> TurboMachinery), and enlarge the blade-to-blade view (lower left) by pressing "f". Click update -> delete all. Now only select CUT1, choose the quantity of interest (static pressure) and click Representations "Strip contour".

In the upper right part of the GUI you can use the "Next Time Step" button to browse through the different time steps you loaded in during the loading process. The camera position is fixed and by printing every time step finally you have pictures of every time step, which you can combine to an animation (with external programs).
To automatize this you can use the "Animate" Button in the upper right part of the GUI. Everything you did in your actual time step (setting camera position, choosing quantity and representations, printing pictures) is repeated now for all following time steps.

A more advanced method for more complex post processing is programming a macro with a loop to load each time step and do your operations.

Did this answer your question? Besides the static pressure the distribution of entropy, relative Mach number or turbulent viscosity might reveal interesting insights in your machine. But that depends on what you are interested in, in particular of course. Additionally you may create a C_p plot animation for example by print the plot for every time step.

If you have further questions please feel free to contact me.


Best regards,
Holger

NLH post processing
 

Dear Holger

I have generated the contours plot of static pressure for each time step based on the procedure you have given but the results totally nonphysical;I have tried for other variables like relative Mach number,entropy etc and the values are totally out of the range which it is expected to be. I don't know what is wrong with reconstruction;would you suggest some thing to do? I have attached the static pressure contour.

best regards,

Dear Tegegn,

I think it is not a problem of the reconstruction, but a problem of your boundary conditions. Please carefully check them. If you want you can share the .mf and .std file of your solution with me, I sent you a private message with my email address.

Best regards
Holger

Dear Tegegn,

during reconstruction you seem to have selected "Represent perturbation only". This outputs the perturbation of the quantities only and not the space averaged value with the perturbation.

When I look at the picture you posted it makes sense. Only the perturbations (disturbances, fluctuations) are calculated. You have a static pressure of approximately 100.000 Pa, but this value is not plotted here.

What you see is only the fluctuation of static pressure (-420 Pa to 479 Pa). If you deactivate "Represent perturbation only" the absolute values are calculated, which you are interested in (100.000 Pa - 420 Pa to 100.000 Pa + 479 Pa).

Best regards
Holger

NLH post processing
 

Dear Holger

Thank you so much, what you have explained is very correct and now I understood the NLH reconstruction in time output with when "Represent perturbation only" option is activated and and deactivated.

Thanks,
Tegegn