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

centrifugal compressor-diffuser simulation : Overflow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 6, 2014, 23:17
Default centrifugal compressor-diffuser simulation : Overflow
  #1
New Member
 
Lutfi
Join Date: Mar 2014
Posts: 3
Rep Power: 3
insisivus is on a distinguished road
hello,
im conducting a centrifugal compressor-diffuser simulation, and i got stuck
when the compressor alone simulated, the results are good, but when it simulated with diffuser, the result is overflow

these are some details :

Compressor
  • 8 blade
  • 8 splitter
  • radial tip
  • currently simulated @73000rpm
  • 1/8 model for simulation

Diffuser
  • flat plate vanned diffuser
  • +/- 55 blades
  • 1/8 model for simulation

gap to shroud : 0,4mm

Quote:
Quote:
ICEM CFD
  • prism layer : 6 (@blade)
Quote:
CFX PRE

Quote:
COMPRESSOR
  • steady state
  • air ideal gas
  • ref. pressure 1 atm
  • heat transfer : total energy
  • turbulence : k-epsilon

INLET
  • 154 m/s (0.88kg/s)
  • stat. frame tot. temp. : 288K
Quote:
DIFFUSER
  • steady state
  • air ideal gas
  • ref. pressure 1 atm
  • heat transfer : total energy
  • turbulence : k-epsilon

OUTLET
  • average static pressure : 386729 Pa
INTERFACE : stage
Pitch change : automatic

max iteration : 5000
residual target : 10^-6
the problem is Overflow, i've tried to refine the mesh (make it smaller), get a better boundary condition, but it jus didnt work

can somebody help me, please ?

thx cfd-online

ps : sorry for my bad english
Attached Images
File Type: jpg cfx pre.jpg (47.3 KB, 32 views)
File Type: jpg diffuser.jpg (41.8 KB, 28 views)
File Type: jpg impeller.jpg (57.7 KB, 26 views)
File Type: jpg run.jpg (62.8 KB, 27 views)
insisivus is offline   Reply With Quote

Old   April 7, 2014, 08:40
Default
  #2
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
It probably has to do with the initial condition you're using. They can be tricky for high speed compressors.

Try using a ramp for the rotor speed. For instance, start with 5000 rpm, then slowly climb your way to 73000 rpm. You can do that automatically using a 1D function such the one below. Also use a timestep in accordance with the angular velocity.

Code:
LIBRARY: 
  CEL: 
    EXPRESSIONS: 
      rot = angVel(Accumulated Iteration Number)
      timestep = 0.1 [rad] / abs(rot)
    END
    FUNCTION: angVel
      Option = Interpolation
      Profile Function = Off
      Argument Units = []
      Result Units = [rev/min]
      INTERPOLATION DATA: 
        Data Pairs = 0,5000,25,5000,500,73000
        Extend Max = On
        Extend Min = No
        Option = One Dimensional
      END
    END
  END
END
brunoc is offline   Reply With Quote

Old   April 10, 2014, 03:18
Default
  #3
New Member
 
Lutfi
Join Date: Mar 2014
Posts: 3
Rep Power: 3
insisivus is on a distinguished road
Quote:
Originally Posted by brunoc View Post
It probably has to do with the initial condition you're using. They can be tricky for high speed compressors.

Try using a ramp for the rotor speed. For instance, start with 5000 rpm, then slowly climb your way to 73000 rpm. You can do that automatically using a 1D function such the one below. Also use a timestep in accordance with the angular velocity.

Code:
LIBRARY: 
  CEL: 
    EXPRESSIONS: 
      rot = angVel(Accumulated Iteration Number)
      timestep = 0.1 [rad] / abs(rot)
    END
    FUNCTION: angVel
      Option = Interpolation
      Profile Function = Off
      Argument Units = []
      Result Units = [rev/min]
      INTERPOLATION DATA: 
        Data Pairs = 0,5000,25,5000,500,73000
        Extend Max = On
        Extend Min = No
        Option = One Dimensional
      END
    END
  END
END
thx bruno
can you help me with the CEL ?
I tried to put the code in the expression box, but it says "syntax error"

thx again
insisivus is offline   Reply With Quote

Old   April 10, 2014, 05:20
Default
  #4
Member
 
Join Date: Feb 2011
Posts: 85
Rep Power: 6
Antanas is on a distinguished road
Quote:
Originally Posted by insisivus View Post
thx bruno
can you help me with the CEL ?
I tried to put the code in the expression box, but it says "syntax error"

thx again
Tools -> Command editor, then past code there -> Process
Antanas is offline   Reply With Quote

Old   April 10, 2014, 06:31
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,669
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This question is an FAQ:

Residuals flatlining:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Overflow error:
http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
ghorrocks is online now   Reply With Quote

Old   April 15, 2014, 15:50
Default
  #6
Member
 
Kevin Hoopes
Join Date: Oct 2010
Posts: 40
Rep Power: 7
khoopes is on a distinguished road
I would recommend using the equivalent mass flow rate boundary condition on the exit if you have access to CFX V15. I have seen this help a lot with stability as it can run anywhere on the compressor map without issue. Often time these high mach number warnings like you are seeing come from being off the map. Even if you are on the map it may mess up on the way to a steady state answer. The equivalent mass flow boundary condition solves this problem. Also, why are you simulating so many diffuser passages? You are using a stage interface, why not just use one diffuser passage?
khoopes is offline   Reply With Quote

Old   April 22, 2014, 05:14
Default
  #7
New Member
 
Lutfi
Join Date: Mar 2014
Posts: 3
Rep Power: 3
insisivus is on a distinguished road
Quote:
Originally Posted by Antanas View Post
Tools -> Command editor, then past code there -> Process
Quote:
Originally Posted by ghorrocks View Post
Quote:
Originally Posted by khoopes View Post
I would recommend using the equivalent mass flow rate boundary condition on the exit if you have access to CFX V15. I have seen this help a lot with stability as it can run anywhere on the compressor map without issue. Often time these high mach number warnings like you are seeing come from being off the map. Even if you are on the map it may mess up on the way to a steady state answer. The equivalent mass flow boundary condition solves this problem. Also, why are you simulating so many diffuser passages? You are using a stage interface, why not just use one diffuser passage?
hi guys, thx a lot for the answers
i've tried the velocity ramp, and the timescale, but still.. flatlining

i haven't tried the equivalent mass flow rate boundary condition since the version of CFX is v14, but i would like to try when it's possible

i'm modeling the same angle-section for impeller and diffuser (45 deg), 45 deg diffuser contain those number of blades, and i don't know if it's possible anyway
insisivus is offline   Reply With Quote

Old   April 22, 2014, 06:41
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,669
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The FAQ I linked to discusses a lot more than just ramping the velocity and time scales. Have you tried all the other issues the FAQ mentions?
ghorrocks is online now   Reply With Quote

Reply

Tags
compressor diffuser cfx

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 separator simulation RicardoLB OpenFOAM Running, Solving & CFD 2 October 7, 2013 03:40
[Other] simulation of 3 d centrifugal pump yvonne ANSYS Meshing & Geometry 8 March 19, 2013 13:25
3D centrifugal compressor simulation nuimlabib Main CFD Forum 0 April 2, 2010 22:08
Fluent simulation of centrifugal pump yvonne ANSYS 3 January 28, 2010 05:48
3-D Contaminant Dispersal Simulation Apple L S Chan Main CFD Forum 1 December 23, 1998 11:06


All times are GMT -4. The time now is 21:37.