[Prak_32]

Hi,

I created a single passage mesh for a centrifugal compressor in Turbo grid. Now I am trying to model as a full 360 degree domain in CFX Turbo mode. In order to do so I did follow the following steps:

1. In the regions and passages option I changed the number of passages to model to 6 from 1. (There are 6 passages in the domain)

Is the above method correct?

There is another problem, when I do this I have some periodic surfaces from the single passage mesh that remain undefined. How should I model them ? should i make them interfaces?

Regards
Prakhar

[Thomas MADELEINE]

if you want to model the whole compressor in order to run it the easiest way from my point of view (to save time in meshing) is to duplicate the domain in CFX-Pre:
- right-click on your domain and go to transform mesh
- use the rotation with multiple copy
etc...

after that you will have the copies of your domain in the right place so you need some interfaces to connect them (I would use GGI since you don't know if your mesh is perfectly 1:1).

if you only want to see the whole compressor in CFD-Post you can do it with the turbo mode or a simple transformation

[Prak_32]

Originally Posted by Thomas MADELEINE

if you want to model the whole compressor in order to run it the easiest way from my point of view (to save time in meshing) is to duplicate the domain in CFX-Pre:
- right-click on your domain and go to transform mesh
- use the rotation with multiple copy
etc...

after that you will have the copies of your domain in the right place so you need some interfaces to connect them (I would use GGI since you don't know if your mesh is perfectly 1:1).

if you only want to see the whole compressor in CFD-Post you can do it with the turbo mode or a simple transformation

Hi Thomas,

Thanks for your reply,

I did manage to make a full 360 domain using cfx pre, however I am still concerned about the periodic surfaces I got from turbo grid.

I am including an image to elaborate my question:-

If you see the image 1 , I have a single blade passage with periodic boundaries. However, when I transform the mesh I get multiple copies of these periodic boundary.

When I see the turbo mode, it automatically identifies it as periodic. However, I am just curious to know that should I specify them as a interface with general connection ?

Regards
Prakhar

1.jpg

2.jpg

[Thomas MADELEINE]

The periodic interface will "simulate the same model of blade" in both side
since you have them in your domain you should connect them with an interface with general connection and conservative interface flux.
after it is up to you to see if you can use 1:1 connection (mesh of your both face are the same) or only GGI.

[Prak_32]

Thanks a lot !! Solves my doubt

[Prak_32]

Originally Posted by Thomas MADELEINE

The periodic interface will "simulate the same model of blade" in both side
since you have them in your domain you should connect them with an interface with general connection and conservative interface flux.
after it is up to you to see if you can use 1:1 connection (mesh of your both face are the same) or only GGI.

Hi!!,

I Have been trying to simulate a centrifugal compressor. I have made the mesh using bladegen and turbogrid. And the mesh seems to decent.

I am able to simulate the single passage domain without any trouble and the solution converges well. However, when I copy the mesh in CFX to obtain a full 360 mesh, i have convergence issues.

The thing is for the full 360 mesh, the solution converges when I impose pressure boundary conditions ( ie Pressure inlet and Static Pressure outlet). However, when I impose mass flow at the outlet my solution diverges and I get an FINMES ERROR. I am enclosing my mesh images here for both the single passage and complete domain.

I would be really grateful if you could assist me in this.

PS:- When I convert the single passage mesh to full 360 domain, I make an interface (GGI connection ) between the repeating periodic boundaries obtained as a result of copying the single passage mesh.

Regards
Prakhar

[Thomas MADELEINE]

Hi,
I am sorry it did not work.
One thing before to be sure when you say Pressure at Inlet it is Total Pressure, isn't it ?

Also I don't know if you already did it or not but you need to create one interface per inter-blade region (so 6 in your case):
1st interface between blade 1 and blade 2
2nd interface between blade 2 and blade 3
etc

For me you does not have to create 6 volumes as inlet before your compressor... but it should not bother your convergence

What are the conditions between each stage of your compressor ?

[Prak_32]

Originally Posted by Thomas MADELEINE

Hi,
I am sorry it did not work.
One thing before to be sure when you say Pressure at Inlet it is Total Pressure, isn't it ?

Also I don't know if you already did it or not but you need to create one interface per inter-blade region (so 6 in your case):
1st interface between blade 1 and blade 2
2nd interface between blade 2 and blade 3
etc

For me you does not have to create 6 volumes as inlet before your compressor... but it should not bother your convergence

What are the conditions between each stage of your compressor ?

Hi !!

Thank you for your feedback.

Yes it is Total Pressure inlet and static pressure outlet.

Yes I do create 6 interfaces( GGI connection ) for each domain ie 6 for the rotor, 6 for diffuser and also 6 for inlet.

I connect the stationary domains ( inlet and diffuser) to the rotating domain ( rotor) using a mixing plane approach ( stage interface).

Another thing, the convergence issue only seems to occur near the peak efficiency point of the compressor map

Regards
Prakhar

[Thomas MADELEINE]

Personally I would set the inlet domain rotating with the shroud wall moving backward (like in the compressor). Best case will be with inlet and blade in the same domain.
But again this should not lead to convergence problem, so I doubt this is the cause of your problem.

Moreover, I suppose it is just some training because without any stator or other perturbation, you don't need to use the stage interface: frozen rotor interface is enough or create only one domain (inlet and outlet included in the rotor).

How it doesn't converge ? Do you have some high residuals ? if yes you can set them active in cfx-pre and plot them to see where is your problem exactly...

Can you try a quick simulation with frozen rotor please ?
Maybe the fact that your interfaces between each stage are quite close of your blades makes the averaging process hard to control.

[Prak_32]

Originally Posted by Thomas MADELEINE

Personally I would set the inlet domain rotating with the shroud wall moving backward (like in the compressor). Best case will be with inlet and blade in the same domain.
But again this should not lead to convergence problem, so I doubt this is the cause of your problem.

Moreover, I suppose it is just some training because without any stator or other perturbation, you don't need to use the stage interface: frozen rotor interface is enough or create only one domain (inlet and outlet included in the rotor).

How it doesn't converge ? Do you have some high residuals ? if yes you can set them active in cfx-pre and plot them to see where is your problem exactly...

Can you try a quick simulation with frozen rotor please ?
Maybe the fact that your interfaces between each stage are quite close of your blades makes the averaging process hard to control.

Hi !!!

Thanks again for your swift reply.

I already tried the frozen rotor approach and I have the same issue.

I have also made sure my interfaces are not exactly close to the blades. However, it is the same setting as the single passage mesh and that works. I just copy it around 360 and it creates the convergence issue.

Also, i get high mach number notifications.

Yes, I suddenly get divergence in my w momentum and p mass.

Maybe I can share my domain with you? Can you please private message me your email address so that i can share the file with you ?

Thanks again

Prakhar

[Thomas MADELEINE]

Sadly I can't really help you directly since I am on CFX while working.

I will search for other possibilities and stay in touch if anything comes to my mind.
Maybe some other people in the forum can also have an idea.

Sorry for not helping more.

[Thomas MADELEINE]

another try : do you use the first simulation (with one blade) to initialize the second simulation (with full compressor) ?

[Prak_32]

No, I havent tried using the solution of single passage as the initial condition for the whole mesh. However, I do use the solution obtained using the pressure conditions as my initial solution to simulate the domain ( with mass flow specified at outlet) but them my solution residuals oscillate.

Any ways thanks for your feedback and help.