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

Constant flow rate through a small area inside the fluid domain.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 22, 2010, 20:55
Default Constant flow rate through a small area inside the fluid domain.
  #1
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 7
robingilbert is on a distinguished road
Hi,

I want to force a fluid at a constant flow rate through a small area inside the fluid domain. I know about the cyclic boundary condition but i do not know how to set it up so that it will give a constant flow rate. I looked into channelFoam and i know how to modify the simpleFoam solver so that it can fix the flowrate. but i just cant figure out how to make it so that the forcing is only through a small area inside the fluid domain.
I considered adding a forcing term to the UEqn which is something like:

(v/A-U)*alpha

where v is volume flow rate
A-area of the surface
U- current velocity at the surface
alpha- a term which has dimensions 1/time which can drive down the solution to required flow rate.
is this approach right?

Please give me some pointers.
robingilbert is offline   Reply With Quote

Old   September 23, 2010, 11:37
Default
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
The only way to do what you want, is literally to have a fixed mass flow outlet adjacent to a fixed flow inlet that maps the velocity from the adjacent outlet (and vice-versa for pressure). You can do this by starting from the low level coupled patches (cyclics), but it isn't trivial unless you know what you are doing and the resulting system probably wont be very stable. Unfortunately I don't think there is an easy solution for this particular aspect of the problem.

A different approach is to put in something like an actuator disc from 1.7 wind solver and adjust the driving force such that the flow rate approximates your target value.
eugene is offline   Reply With Quote

Old   September 23, 2010, 17:45
Default
  #3
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 7
robingilbert is on a distinguished road
Thank you Eugene,

I will try the actuator disk and see if that works.
So according to ur first suggestion, do i need to make a hollow volume without any meshes and has an inlet (into the fluid domain) and an outlet (into the hollow volume) and map the velocity from inlet to the outlet?
robingilbert is offline   Reply With Quote

Old   September 23, 2010, 18:48
Default
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Quote:
Originally Posted by robingilbert View Post
Thank you Eugene,

I will try the actuator disk and see if that works.
So according to ur first suggestion, do i need to make a hollow volume without any meshes and has an inlet (into the fluid domain) and an outlet (into the hollow volume) and map the velocity from inlet to the outlet?
No, no - no holes required. You take your basic cyclic boundary (which can act just like an internal boundary) and start chopping and changing. For U you want one side of the cyclic patch pair to be a scaled "zero gradient" outlet such that the total flux matches your specification. The other side is an inlet that simply gets its value from the outlet side, just like a normal cyclic. For pressure, you want the reverse, the inlet side is zero gradient and this value is mapped to the outlet side and treated as fixed. The switching is done based on flux direction. I did something like this at my previous job and remember that it was a bit tricky. Unfortunately I don't have the code any more, but it is certainly possible.
eugene is offline   Reply With Quote

Old   September 23, 2010, 21:05
Default
  #5
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 7
robingilbert is on a distinguished road
Thanks once again Eugene.
one more question. forgive me if its a stupid question, can I add a source term in the momentum eqn so that it will force the fluid at a particular flow rate?
robingilbert is offline   Reply With Quote

Old   September 24, 2010, 04:49
Default
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Of course. I pointed you toward the actuator disk because this is exactly the framework you need to implement the source term you need. An example usage can be found here: OpenFOAM-1.7.x/tutorials/incompressible/simpleWindFoam and the source code for the actuator disk and base class can be found here: OpenFOAM-1.7.x/src/finiteVolume/cfdTools/general/fieldSources/basicSource
eugene is offline   Reply With Quote

Old   September 24, 2010, 05:35
Default
  #7
Member
 
Robin Gilbert
Join Date: Jan 2010
Posts: 66
Rep Power: 7
robingilbert is on a distinguished road
Thank you soooooooooo much Eugene. I will try that out!! thank you once again.
robingilbert is offline   Reply With Quote

Old   October 4, 2010, 16:19
Default
  #8
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hi Robin,
I probably need something similar for this kind of problem: How to model a fan fixing the mass flow rate?. Eugene suggested me to modify the actuator disk model as well. Have you made any progress on the subject? Shall we collaborate?
Regards

mad
maddalena is offline   Reply With Quote

Reply

Tags
simplefoam, source, source term, ueqn

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
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
flow simulation across a small fan jane luo Main CFD Forum 15 April 12, 2004 17:49
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
CFD Modeling of Two-phase Flow in Small Dia.Tubes Eric Poindexter Main CFD Forum 2 September 22, 2000 09:21
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 22:09.