CFD Analysis of a 3D Centrifugal blower

  • Last Post 28 March 2019
prathikshetty posted this 13 March 2019


I am doing a academic project on validation of Centrifugal blower CFD analysis with the experimental data. Here my objective is to match the performance curve (Static pressure versus Volume flow rate) obtained from CFD analysis with that of experimental data.

I am using CFX solver, steady state analysis and SST turbulence model, with pressure inlet (Total pressure) and pressure outlet (Average static pressure) condition and as my interest here is to obtain the volume flow rate.

I have run simulations at different outlet average static pressure conditions, and observed that the CFD is under-predicting the flow at the higher static pressures. The difference between the experimental and CFD performance curve is around 20%. 

How can i reduce this gap?

Would you suggest me to go with a different solver as well as a different Turbulence model?





Order By: Standard | Newest | Votes
rwoolhou posted this 14 March 2019

Have you done a mesh independence study? 

prathikshetty posted this 25 March 2019

Have you done a mesh independence study? 

Yes i have done the mesh independence study! 

Bill Holmes posted this 28 March 2019


Is it a forward or backward curved fan?  Forward curved fans tend to be highly unsteady in nature - maybe trying a transient calculation will help.  In fact if you have a backward curved fan and are only underpredicting at high outlet pressures, running a transient could help as well.

The other thing to look at is if you are only underpredicting at low flow rates (ie. high outlet static pressures) then it's likely the flow is separating from the blade too early.  Trying things like SST with the turbulence transition model and reattachment modification for SST could to better predict the separation point on the blade and improve performance.  

You should also make sure you are reducing the CFD data in a similar manner to how it is obtained on the test bench.  Usually fan test data is corrected to STP or some other pressure/temperature, so make sure you are using the correct density in your simulation and calculations.  Often pressures are measured at discreet locations of sensors or taps, and usually the outlet boundary condition is set to this pressure.  It's wise to double check you indeed are getting those same pressure values at those sensor locations.


Hope this helps,

Bill Holmes





  • Liked by
  • prathikshetty
prathikshetty posted this 28 March 2019

Hi Bill, First of all thanks for your valuable response.

Its basically a backward curved fan. The simulations are done as per the test conditions (I'll cross check again). Since I am using the pressure boundary conditions, I am basically targeting the flow at the outlet. I have also tried the mass flow and total pressure B.C, but in that case too the pressure is under predicted.

I have not checked with the SST with Transition turbulence model and reattachment modification. I will check with this.

And if nothing works, the only option is to run transient case

Thank you once again