centrifugal pump - which solver?
 

Dear OpenFOAMers,

I am running a centrifugal pump case using pimpleDyMFoam solver. The impeller rotates at 4000 rpm. I am mostly interested in impeller rotating at steady state. Which solver is suitable for this besides pimpleDyMFoam? I saw on the forum that some uses MRFSimpleFoam. But, I cannot find this solver on OF-3.0.x.

Suggestion?

Thanks!

Pei-Ying

MRF can by used with most solvers, check out tutorial mixerVessel2D in tutorials/incompressible/simpleFoam. So, use simpleFoam and define MRF in file constant/MRFProperties.

MRF is unsuitable for centrifugal fans.

You can find more on this in the thread below and at several over places.
http://www.cfd-online.com/Forums/ope...tml#post283588

regards,
Sylvester

Well, it's about the only option if you want to do steady state calculations. And regarding the MRF error in that thread, yes it does produce errors if it's misused, but in my opinion MRF works just fine if there is a rotating impeller cellZone. I've used it many times and have no problem with it.

EDIT: And to clarify, with centrifugal pumps the rotation (or spin) axis not perpendicular with the inflow, and the MRF zone is not empty (impeller blades).

Thanks Pekka!

My case has 10 million cells. It will take weeks to complete one revolution on my workstation if I use pimpleDyMFoam. So, the simpleFoam will be my best option for now.

I am thinking taking the results from simpleFoam and run maybe 1000 steps using pimpleDyMFoam to see if the results are still good.

Pei-Ying

Here is a link to a presentation about the subject I did some time ago:

http://www.cleen.fi/en/SitePages/EFE...4_97f1874fe398

It might help you with case setup :)

Hi, Pekka,

Your slides help a lot. My case is similar to yours. I did not specify flow rate at the inlet. I want to know flow rate when the impeller is rotating at 4000 rpm instead.

I am wondering if you can give me more guidance on how you setup BCs for k and omega. I have not been successful with kOmegaSST.

Pei-Ying

You can use pressure only BC too, use totalPressure (p0 = 0) at inlet and for example fixedMean with a reasonable meanValue (use design point pressure for example) at outlet. And remember that incompressible pressure is actually dynamic pressure (p/rho) in openfoam. For velocity use pressureInletOutletVelocity at inlet and outlet. For turbulence parameters I use inletOutlet for inlet and outlet (fixedValue at inlet and zeroGradient at outlet).

For turbulence parameters you should estimate initial values, I used k = 0.4 and omega = 400 for my initial field values. Use wall functions, f.e. kqRWallFunction, omegaWallFunction, nutUSpaldingWallFunction. Increasing initial omega value might help, but it's better to start with upwind differencing and low underrelaxation and then increase from there and change to 2nd order differencing for at least div(phi,U).

Thanks a lot again Pekka!

I will give your suggestion a try. But, can you give me some guidance on how your initial k = 0.4 and omega = 400 were calculated?

Happy New Year!

Pei-Ying

Check for example this link:

http://www.cfd-online.com/Wiki/Turbu...ary_conditions

OpenFOAM uses the Cmu formulation of omega, for length scale you can use for example pipe diameter or half of it. For turbulence intensity you could choose something in the range 1-5 %. All of the initial values are case dependent, so I can't really recommend any absolute values for your case.

If you're not familiar with turbulence modelling, I suggest that you read more about the subject from for example the book "An Introduction to Computational Fluid Dynamics, The Finite Volume Method" by H.K. Versteeg & W. Malalasekera. NASA turbulence modelling resource is also quite useful, but not so user friendly:

http://turbmodels.larc.nasa.gov/

Thanks Pekka!

Pei-Ying