
[Sponsors] 
Rotating or stationary domain in pump/turbine cavity 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 17, 2017, 02:56 
Rotating or stationary domain in pump/turbine cavity

#1 
New Member
Christian Høy
Join Date: Mar 2017
Posts: 2
Rep Power: 0 
Hallo,
I am doing a CFD analysis in ANSYS CFX of a cavity between a rotating impeller (3600rpm) and turbine wheel (6000rpm), see attached figure, for obtaining velocity, internal pressure and thrust forces on the impeller and turbine. There will be a leakage radially inward or outward in/out of the domain depending on P1, P2 and rotating speeds. I am struggeling with setting the correct setup for this domain. I can choose between rotating and stationary domain. As I see it, the cavity it self is stationary, and the walls are inducing a spin to the fluid in the cavity. Some colleagues of mine suggest using a rotating domain, and setting the rotation of the domain equal to the pump impeller speed and the turbine speed to 60003600. My question is, how does CFX treat the rotating domain? In reality the cavity will not rotate, and I am struggeling with understanding how the velocity profile between the two rotating walls will become representative. A rotating domain will include a "pumping effect" on the domain with Coriolis and centripital effect? Hope someone has experience on this and can help me explain the difference between the two setups and what I should choose. Thank you. Christian 

March 17, 2017, 04:05 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
Make sure you know what you are talking about here. It is a "rotating frame of reference" model. So it is the frame of reference which rotates  what the fluid and bodies inside it do is another matter. It is useful when the motion of things is simpler when described in a rotating frame of reference.
So any flow can be described in a stationary frame of reference, or a rotating frame of reference (or translating, or accelerating etc). The flow is the same in all cases, but the velocities in each case are different as they are measured against a different frame of reference. So the answer to your question is: whichever makes it easier to model. It could be either the impeller speed or the turbine speed. One important thing you have not mentioned is that sometimes the choice of reference frame affects convergence. For instance if a straight pipe flow goes through a rotating frame of reference and remains straight, convergence can be compromised because there are large velocities in the rotating reference frame (which only counteract the reference frame rotation). To assist in these cases there is a "alternate rotation model", which is recommended to be used when the flow in a rotating frame of reference is pretty straight in the stationary frame of reference. 

March 17, 2017, 05:30 

#3 
New Member
Christian Høy
Join Date: Mar 2017
Posts: 2
Rep Power: 0 
Thank you Glenn,
if the rotating domain is just a "rotating frame of reference" model, then I understand. But as I can see through CFX documentation: the CFXsolver computes the appropriate Coriolis and centrifugal momentum terms. If you set the domain velocity equal to the pump speed, are you not then solving the Coriolis and centrifugal momentum term with that speed? I am not sure if the velocity profile will be realistic using a rotating domain. The pump impeller wall and turbine wheel wall will induce a spin to the fluid, and the velocity profile in the cavity, will as far as I understand it look like as shown in my figure attached. The velocity profile will affect the local spin and pressure, hence thrust forces, so it is important that I get correct/realistic pressure and velocities. Christian 

March 17, 2017, 06:03 

#4  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
As a rotating frame of reference is an accelerating reference frame then you need to add additional terms to handle that  coriolis and centripetal forces. That is an implication of using an accelerating frame of reference.
Quote:
Quote:
https://en.wikipedia.org/wiki/Rotating_reference_frame https://en.wikipedia.org/wiki/Inerti...e_of_reference This image from https://en.wikipedia.org/wiki/Inerti...e_of_reference explains it nicely (you will need to view it on wikipedia, I can't get the animation to work on the forum): Corioliskraftanimation.jpg The top image is a rolling ball viewed in a stationary frame of reference. It moves in a straight line as there are no XY plane forces acting on it to accelerate it off a straight line. The bottom image is the same rolling ball viewed in a rotating frame of reference. The ball appears to move in curve. There are no forces in the XY plane so what pushes it off a straight line? The answer is that the "fictitious" coriolis and centripetal forces are introduced when you are observing in a rotating frame of reference. Quote:


Tags 
cavity flow, cfx, impeller, rotating domain, stationary domain 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
sliding mesh problem in CFX  Saima  CFX  46  September 11, 2021 07:38 
Sudden increase the residual of Maxwell's equations  hsezsz  CFX  2  October 13, 2016 06:58 
Monte Carlo Simulation: HEnergy is not convergating & high Incident Radiation  volleyHC  CFX  5  April 3, 2016 05:41 
Pressure distribution on a wall  darazsbence  CFX  17  October 6, 2015 10:38 
Rotating Domain + Stationary Domain + Interface Acusolve  bench  Main CFD Forum  3  July 7, 2015 11:34 