[insisivus]

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

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]

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.

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]

Originally Posted by brunoc

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.

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]

Originally Posted by insisivus

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]

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]

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]

Originally Posted by Antanas

Tools -> Command editor, then past code there -> Process

Originally Posted by ghorrocks

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

Originally Posted by khoopes

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

[ghorrocks]

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?