Impellar driven fluid flow in centrifugal pump
 

Is it possible to simulate centrifugal pump just like actual testing.. I mean both inlet and outlet are ambient pressure and when the impeller rotates flow and pressure develops.
From tutorial I understood that we must specify the Pressure difference and/or mass flow rate and we can simulate for the Head. Assume we dont know the mass flow rate and pressure difference and we know only the rpm of the pump. In this case is it possible to simulate for flow and pressure rise, from the rotation of impeller alone?
I have gone through the gear-pump/gerotor-pump cfx tutorial, in which the flow is simulated through rpm alone by using 'Immersed solid' method. Anybody has used this method for centrifugal pump?

Do not use immersed solids to model a centrifugal pump. Use rotating frames of reference. Look at the axial rotor stator tutorial models for how to do this.

Yes, you can model a known rpm with ambient pressure on inlet and outlet reservoirs.

Thanks for the reply GHorrocks :)
Can you please explain why we should not use the immersed solid method?
Also can you please tell in brief that what is the difference between these three methods?
i.e, between default analysis method by specifying mass flow rate, rotating frame of reference method and immersed solid method..
Also which method is more appropriate method for doing transient analysis? that is flow variation with respect to rpm?!
Thanks

Because immersed solids is poor at resolving the boundary layer. Rotating domains will allow you to do a mesh conformal to the impeller wall faces, and with good quality inflation layers. Immersed solid meshes are neither conformal to the impeller wall faces nor allow you to use inflation layers.

The mass flow rate is the boundary condition you specify and that is a different thing.

If you do the tutorials provided with CFX you will have a clearer idea of what these things mean.

Thanks GHorrocks for your inputs :)
I have gone through both the Cavitation of centrifugal pump tutorial and Flow through Axial turbine stage tutorial.
These are the difference i found:
1. In centrifugal pump tutorial, only one domain has been used and the stationary wall is specified as 'counter rotating wall'
2. In Axial turbine tutorial, one stationary domain and one rotating domain is specified. Both the domains are connected by 'Frozen Rotor' Interface.

In your first reply, you mentioned that we can simulate impeller driven fluid flow by specifying atmospheric pressure at both inlet and outlet. But even in the axial turbine tutorial mass flow rate at the outlet is explicitly defined. Please clarify. Thank you :)

in Axial turbine you have a stator (blades that don't move) and a rotor... so you can't model the stator by "cheating" a rotating domain with counter rotating walls...
in the centrifugal pump there is no stator, so you can avoid the tow domains and the interface between. your domain is rotating and you "immobilize" some walls by setting a counter rotating velocity.

for you BC, I will prefer an inlet total pressure if I can. for example if you are working in the atmosphere, you can assume that long time ago the air tank will be at 1 atm (with no velocity, so it is total pressure).
then if you know the exit (the atmosphere by example) you can put (1 atm for example) a static pressure outlet.

I don't know if it will work with two static pressure BCs, if somebody can confirm that i will miss a term to work (like when you put two velocity BCs) ?

Bringing back the old thread.. By setting an expert parameter (unchecking 'artificial boundary wall'), we can analyze by setting static pressure at the both inlet and outlet and the flow will be driven by rotation alone.. But we may face convergence difficulties..