CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

pump outlet pressure higher than inlet pressure

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

Like Tree2Likes
  • 1 Post By macfly
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 7, 2014, 12:07
Default pump outlet pressure higher than inlet pressure
  #1
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
Hi,

I am currently simulating flow in a pump.

The inlet i am using is a 'mass flow rate' inlet and the outlet i am using is a 'pressure outlet' and i require the total pressure information at the inlet and outlet. So i created surface monitors at the inlet and outlet surfaces.

However, when i am running the calculation, i realise that the inlet has a higher total pressure than the outlet, which doesnt really make much sense to me.

i'm still in the mids of learning this software. Can someone advise me on what went wrong?

thanks.

Last edited by jstan3; February 8, 2014 at 22:01.
jstan3 is offline   Reply With Quote

Old   February 7, 2014, 16:12
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 531
Rep Power: 21
stumpy is on a distinguished road
A pump is supposed to raise the pressure.
stumpy is offline   Reply With Quote

Old   February 7, 2014, 20:18
Default
  #3
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
Please correct me if i am wrong. Shouldn't the correct case be: Higher pressure at outlet than inlet?
jstan3 is offline   Reply With Quote

Old   February 8, 2014, 15:13
Default
  #4
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Canada
Posts: 392
Rep Power: 17
macfly is on a distinguished road
I can at least tell you that you inversed 'inlet' and 'outlet' in your thread title
Ming Darcy likes this.
macfly is offline   Reply With Quote

Old   February 8, 2014, 22:10
Default
  #5
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
oh. my bad. i meant it the other way around.

Would really appreciate it if someone could give me some advice on this.
jstan3 is offline   Reply With Quote

Old   February 9, 2014, 15:59
Default
  #6
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,406
Rep Power: 48
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
If the mass flow rate you enforce at the inlet is higher than the flow rate of the pump at its current operating point you could actually get a pressure drop from the pump.
Your setup corresponds to a bigger pump feeding fluid through the smaller pump.
As a first remedy, you could decrease the mass flow rate at the inlet.
richujbabu likes this.
flotus1 is offline   Reply With Quote

Old   February 10, 2014, 01:06
Default
  #7
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
i see. tyvm.
jstan3 is offline   Reply With Quote

Old   February 10, 2014, 16:19
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 531
Rep Power: 21
stumpy is on a distinguished road
check the torque on the blades too. A pump should be adding work to the fluid to raise its pressure. In your case it must be extracting work since you are getting a pressure drop. Like Alex said, this means your rotation rate and your flow rate are not consistent.
Just to check... you have a rotating domain around the blades right (and haven't just imposed a wall velocity)?
stumpy is offline   Reply With Quote

Old   February 10, 2014, 21:09
Default
  #9
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
i have created interfaces(which i converted to wall) around the rotating impeller, which are rotating at a speed of 2000rpm around the rotating impeller. On top of that, for the fluid component (wall) that is residing in the impeller, i have also set it to rotate at 2000rpm. This are the only components in my model that is rotating. thx.
jstan3 is offline   Reply With Quote

Old   February 11, 2014, 13:24
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 531
Rep Power: 21
stumpy is on a distinguished road
I didn't really follow that, but it doesn't sound correct. You need a rotating reference frame for your zone. The walls (blades) would be stationary in that zone, since their motion is relative to the zone.
stumpy is offline   Reply With Quote

Old   February 11, 2014, 13:37
Default
  #11
Member
 
David
Join Date: Aug 2012
Posts: 48
Rep Power: 13
GM_XIII is on a distinguished road
Are you monitoring total or static pressure? I assume your geometry ends in the exit of the blades or does it contain the diffusor?
GM_XIII is offline   Reply With Quote

Old   February 11, 2014, 21:10
Default
  #12
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
@stumpy: i didn't realise it could be done that way. I will give it a try. But i have 7 zones in my fluid model. So do you mind explaining in more detail which zone requires a reference frame? and also which zone should be stationary?

Zones:
-the back leakage gap of the centrifugal pump (the leakage from the outer volute back into the inner volute)
-the front leakage gap of the centrifugal pump (the leakage from the outer volute back into the inner volute)
-impeller
-inner volute
-outer volute
-inlet
-outlet

@GM_XIII: i am currently monitoring the total pressure. The geometry ends at the outlet after the fluid exits the pump, which is about 0.1m from the outer volute exit.
jstan3 is offline   Reply With Quote

Old   February 13, 2014, 09:24
Default
  #13
Senior Member
 
ghost82's Avatar
 
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26
ghost82 will become famous soon enough
Also make sure you are rotating the blades in the right direction for your rotating reference frame/dynamic mesh case; remember that fluent uses a right-handed coordinate system.

Daniele
ghost82 is offline   Reply With Quote

Old   February 13, 2014, 11:39
Default
  #14
Senior Member
 
Join Date: Apr 2009
Posts: 531
Rep Power: 21
stumpy is on a distinguished road
If you set a velocity on a wall boundary then it's only valid if the velocity vector is tangential to the boundary. In other words you can't "push" the flow using this method, but you can introduce a shear force. Any boundary that "pushes" the flow (i.e. has a velocity vector with a component in the normal direction) should be modeled by placing it in a rotating reference frame and setting the wall velocity to zero. So this means all your blades need to be in a rotating reference frame with stationary walls. The shroud wall in the rotating reference frame will need to be counter-rotating, and it must be a surface of revolution so that it only has tangential motion. Generally any components upstream or downstream of the blades with non-rotating components are placed into a stationary reference frame.
stumpy is offline   Reply With Quote

Old   February 13, 2014, 23:44
Default
  #15
New Member
 
jason tan
Join Date: Feb 2014
Posts: 7
Rep Power: 12
jstan3 is on a distinguished road
i see. tyvm for the advice.
jstan3 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Why we normally provide velocity at inlet and pressure at outlet for pipe flow? p07ip705 Main CFD Forum 3 August 3, 2012 05:53
Pressure Inlet Boundary Condition Issue zoeburton1987 FLUENT 0 May 15, 2012 09:20
How to set up the inlet boundary condition for a low pressure case? beastieboys6 FLUENT 3 April 10, 2012 22:46
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 10:27.