CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Rotating or stationary domain in pump/turbine cavity

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 17, 2017, 03:56
Smile Rotating or stationary domain in pump/turbine cavity
  #1
New Member
 
Christian Hy
Join Date: Mar 2017
Posts: 2
Rep Power: 0
Christian Hy is on a distinguished road
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 set-up 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 6000-3600.

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 set-ups and what I should choose. Thank you.


Christian
Attached Images
File Type: png CFD_cavitydomain.PNG (33.1 KB, 15 views)
Christian Hy is offline   Reply With Quote

Old   March 17, 2017, 05:05
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,544
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   March 17, 2017, 06:30
Default
  #3
New Member
 
Christian Hy
Join Date: Mar 2017
Posts: 2
Rep Power: 0
Christian Hy is on a distinguished road
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 CFX-solver 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
Attached Images
File Type: png CFD_cavitydomain2.PNG (18.9 KB, 5 views)
Christian Hy is offline   Reply With Quote

Old   March 17, 2017, 07:03
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,544
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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:
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?
Yes, that is correct. My previous paragraph explains why.

Quote:
I am not sure if the velocity profile will be realistic using a rotating domain.
You appear to be confused between the motion of the device and/or the fluid, against the motion of the rotating frame of reference. The frame of reference is simply what the velocities are measured against. It says nothing about what the velocities are actually doing.

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:
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.
Of course. You need to understand what rotating frame of reference means before you understand what it is doing, however.
ghorrocks is offline   Reply With Quote

Reply

Tags
cavity flow, cfx, impeller, rotating domain, stationary domain

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Sudden increase the residual of Maxwell's equations hsezsz CFX 2 October 13, 2016 06:58
Monte Carlo Simulation: H-Energy 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
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Rotating Domain + Stationary Domain + Interface Acusolve bench Main CFD Forum 3 July 7, 2015 11:34


All times are GMT -4. The time now is 09:00.