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

Flow rate restriction simulation set-up

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 11, 2015, 09:13
Default Flow rate restriction simulation set-up
  #1
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 630
Rep Power: 22
siw will become famous soon enough
Hi,

Can anyone suggest a suitable set-up for modelling this scenario?

I have an internal system upstream of a centrifugal fan and when the fan is operating it pulls a volumetric flow rate of 346 litres/second through the system. My CFD model is of the system upstream of the fan only and I would use an outlet mass flow rate and a total pressure inlet (the air is drawn in from the atmosphere) to model this condition - so far so good. However, I need to include a restrictor, e.g. orifice plate, into the system so that the volumetric flow rate is reduced to 250 litres/second. There would be a corresponding pressure loss across the restrictor.

I could simply alter the outlet flow rate boundary condition to the new value of 250 L/s then let CFX calculate the restrictor pressure loss. But this would not produce the reduction in flow rate as part of the calculation because it is the restrictor which reduces the flow rate and not the boundary conditions. Since CFD works on mass conservation then specifying 346 L/s at the outlet and having CFX alter the flow rate through the model does not seem possible to me.

Thanks.
siw is offline   Reply With Quote

Old   November 11, 2015, 12:22
Default
  #2
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 139
Rep Power: 8
shivasluzz is on a distinguished road
2 methods..
1. model the orifice plate also...

2. analyse the orifice plate separately and develop the del P vs mass flow characteristics..
create function in cfx-pre using that relation
create 2 domains from your single domain (by splitting at the place of orifice; no need to model orifice)
create domain interface and use that function for interface model..
shivasluzz is offline   Reply With Quote

Old   November 11, 2015, 18:37
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,467
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The fan has a performance curve (dP vs flow rate), and the system has a performance curve (dP vs flow rate). The system will run at equilibrium when at a given flow rate the pressure rise over the fan equals the pressure loss through the system. So:

If you like pen and paper solutions, draw the two performance curves and where they intersect is the operating point.

But if you want to implement this into CFX so the model finds its own operating point - then make the inlet a CEL function of pressure versus flow rate which describes the fan performance curve and then CFX will find the equilibrium with what ever you model. If you decide to not model the oriface plate (and I recommend you do not model it if you know its effect and don't care about the details) then include its effect in the inlet boundary performance curve.

What I am describing is essentially sluzzer's option 2.
ghorrocks is online now   Reply With Quote

Old   November 12, 2015, 07:59
Default
  #4
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 139
Rep Power: 8
shivasluzz is on a distinguished road
thats a good explanation... and this was the point i was getting confused for months...

basically thr r two things
1. component analysis
2. system analysis (combination of components)

often it is complicated to do system analysis in cfd...
so develop characteristics for components using cfd and do component matching to find the operating point...

system softwares like Amesim, Simulink etc., does this job for you
https://en.wikipedia.org/wiki/LMS_Imagine.Lab_Amesim
(it will be too complicated to match by hand when the variables and components are more)

there is a nasa system engineering handbook regarding component matchings... other than that so far i didnt find good resource regarding system principles.. if any body knows any good material, then please recommend (i put this question in system analysis forum and i got no response :P)
shivasluzz is offline   Reply With Quote

Old   February 16, 2016, 13:15
Default
  #5
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 139
Rep Power: 8
shivasluzz is on a distinguished road
Like to bring back this old thread with a new doubt...
If there is single input and single output for a component in a system, then we can characterise that component using an expression or relation like dp vs flow rate for an orifice... But what if the component we have to characterise by expression or relation has 'Multiple input and Multiple output' ?!

Somebody please give some explanation
shivasluzz 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
rotor 37 choking mass flow rate fluent simulation sehs15 FLUENT 1 January 15, 2015 07:07
two fluid, volumetric/mass flow rate at different volume fractions Veronique Pe CFX 2 November 26, 2014 06:30
Mass flow rate prediction of Purge control valve using set pressure drop enr_venkat CFX 11 February 27, 2014 12:30
mass flow rate... sanjar OpenFOAM Running, Solving & CFD 1 December 2, 2013 01:09
[snappyHexMesh] determining displacement for added points CFDnewbie147 OpenFOAM Meshing & Mesh Conversion 1 October 22, 2013 10:53


All times are GMT -4. The time now is 17:52.