CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

centrifugal compressor

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 7, 2008, 17:54
Default centrifugal compressor
  #1
Marek
Guest
 
Posts: n/a
Hi!

I want to simulate centrifugla compressor in CFX-10.0. First I made hand calculations. I used total pressure on inlet and mass flow on outlet for BC. Although I calculated that Mach number at outlet is 0.77 solver crashed because of high Mach number. For timescale I set 1/omega. I also try to gradually increase mass flow. First I set half final mass flow. Solution almost converged. Than I set 10% bigger mass flow. Solution did't converged. Does anybody has any practical advice?! This is my first compressor simulation except tutorial.

Best regards! Marek

  Reply With Quote

Old   December 13, 2008, 11:25
Default Re: centrifugal compressor
  #2
Georg
Guest
 
Posts: n/a
Perhaps you get high Mach number near blade surface (leading edge). I recommend you to check mesh quality of whole model and especially in this zone. May be your elements are too big. In CFX Post you can verify 1) shape of elements " several criterions (you'll find information about in CFX Help); 2) Y+ variable on walls (it should be less then 200 if you use default k-epsilon turbulence model).
  Reply With Quote

Old   December 13, 2008, 20:15
Default Re: centrifugal compressor
  #3
Marek
Guest
 
Posts: n/a
Georg, thanks for reply

Actually the high Mach number is on outlet. I changed BC to mass flow on inlet and total pressure on outlet. But minimum MAX residual I can get is 5E-4. First I used timescale 1/omega and than I reduced them to 1/(2*omega).
  Reply With Quote

Old   December 15, 2008, 10:52
Default Re: centrifugal compressor
  #4
CycLone
Guest
 
Posts: n/a
Hi Marek,

You can't specify total pressure at an outlet, did you mean static pressure?

Go back to having a total pressure at the inlet and set the relative pressure at the outlet to zero (i.e. equal to your inlet). This should run fine and return the choke mass flow rate. Compare this to your desired mass flow rate to see if it is indeed achievable.

Some common mistakes to check: 1. Geometry scale; it's not uncommon to have created the mesh in the wrong units. 2. Direction of rotation; use right-hand rule. 3. Component vs. full machine; did you apply the full machine mass flow on a single component? 4. Initial guess; if you entered an initial guess, try deleting it and letting the solver do it automatically. Good intentions can lead to undesirable results.

Generally good advice: If the flow is near choke, use a pressure outlet. Away from choke, use mass flow rate. See the turbomachinery best practices guide in the documentation for more help.

-CycLone
  Reply With Quote

Old   December 16, 2008, 07:47
Default Re: centrifugal compressor
  #5
Marek
Guest
 
Posts: n/a
CycLone, thanks for useful reply!

Yes, it was mistake (late hour). I set static pressure at an outlet.

I will set pressures as you said.

Thanks also for common mistakes list. I checked all the things (except No.4) and everything is OK.

best regards Marek

  Reply With Quote

Old   December 17, 2008, 10:04
Default Re: centrifugal compressor
  #6
Marek
Guest
 
Posts: n/a
I set total pressure (relative pressure to 0Pa) at an inlet and Average static pressure (relative pressure 0Pa)at an outlet. I set reference pressure to 1atm. The mass flow I get is the choke mass flow. Is this correct?

Now I have new question. I made three meshes. Compressor inlet, compressor and difusor. I am not sure how to make domain interface between the inlet and compressor and between compressor and difusor. Inlet and difusor domain is stationary but compressor is rotating domain.

Any useful advices are welcome!

Thanks in advance! Marek
  Reply With Quote

Old   December 17, 2008, 12:25
Default Re: centrifugal compressor
  #7
Sonja
Guest
 
Posts: n/a
There are 3 different interfaces which you can use to connect stationary to rotating domains. They are called Stage, Frozen Rotor and transient Stator-Rotor Interface. They are described well in the cfx manual. hope this helps you!

  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Centrifugal compressor mass flow error Attesz CFX 18 May 27, 2012 10:17
[ICEM] Meshing a centrifugal compressor impeller Mitpostdoc ANSYS Meshing & Geometry 8 February 25, 2011 11:51
CFD analysis of Centrifugal compressor murthy pnvr CFX 3 November 12, 2010 12:13
The Onset of Surge in a centrifugal compressor Suzzn CFX 4 December 19, 2009 09:49
centrifugal compressor siva appanna Main CFD Forum 5 February 13, 2006 22:07


All times are GMT -4. The time now is 21:18.