CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   centrifugal compressor-diffuser simulation : Overflow (http://www.cfd-online.com/Forums/cfx/132825-centrifugal-compressor-diffuser-simulation-overflow.html)

insisivus April 6, 2014 23:17

centrifugal compressor-diffuser simulation : Overflow
 
4 Attachment(s)
hello,
im conducting a centrifugal compressor-diffuser simulation, and i got stuck :confused:
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

brunoc April 7, 2014 08:40

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


insisivus April 10, 2014 03:18

Quote:

Originally Posted by brunoc (Post 484390)
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 :)

Antanas April 10, 2014 05:20

Quote:

Originally Posted by insisivus (Post 485132)
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

ghorrocks April 10, 2014 06:31

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

khoopes April 15, 2014 15:50

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?

insisivus April 22, 2014 05:14

Quote:

Originally Posted by Antanas (Post 485161)
Tools -> Command editor, then past code there -> Process

Quote:

Originally Posted by ghorrocks (Post 485179)

Quote:

Originally Posted by khoopes (Post 486338)
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 :confused:

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:D

ghorrocks April 22, 2014 06:41

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?


All times are GMT -4. The time now is 14:07.