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

Volume flow rate (l/s) as boundary

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

Like Tree3Likes
  • 1 Post By macfly
  • 1 Post By macfly
  • 1 Post By macfly

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2013, 10:32
Default Volume flow rate (l/s) as boundary
  #1
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
Hello!

I have two question:

1- Is it possible in FLUENT to set the boundary as volume flow rate (liter/Sec) for inlet and outlet?
2- Is it possible in Fluent to measure a surface area or curve length? for instance I want to measure the area of the inlet.
Thanks.
asal is offline   Reply With Quote

Old   March 14, 2013, 12:22
Default
  #2
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Volume flow inlet is not available in the boundary conditions. Here is how you measure the inlet area:
1. Read mesh: File\Read\Mesh...
2. Initialize without setting anything: Solution\Solution Initialization\Initialize
3. Measure inlet area: Results\Reports\Surface Integrals => Report Type : Area => Surfaces : the inlet
macfly is offline   Reply With Quote

Old   March 14, 2013, 12:49
Default
  #3
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
Thanks for your reply!

I have the values just as Liter/Sec for my inlet ans outlets. If l/s is not available, since my fluid is ideal gas, how can I handle it?
thanks.
asal is offline   Reply With Quote

Old   March 14, 2013, 12:55
Default
  #4
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Divide volume flow rate by inlet area, what units do you get?
stuart23 likes this.
macfly is offline   Reply With Quote

Old   March 14, 2013, 14:10
Default
  #5
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
Sorry, I am new in the fluent, so sorry about my questions

I mean about the outlet, I have now the volume flow rate which I convert to velocity. which type of boundary condition available in Fluent I should choose?
Should I choose Velocity-int but assign opposite direction?
thanks.
asal is offline   Reply With Quote

Old   March 14, 2013, 14:16
Default
  #6
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
typical outlet boundary condition : pressure outlet, leave Gauge Pressure to 0 Pascal (keep default settings)

after simulation, verify mass balance : Results\Reports\Mass Flow Rate => choose inlet and outlet under 'Boundaries' => Compute
macfly is offline   Reply With Quote

Old   March 14, 2013, 15:33
Default
  #7
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
I think you become misunderstood!!!!
I should assign a value for the outlet. Is is not a pressure-outlet type. a known amount of flow should extract from the outlet.
asal is offline   Reply With Quote

Old   March 14, 2013, 15:48
Default
  #8
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Yes, exactly, I'm misunderstood.

You have 1 or multiple outlet(s)? Infiltration, exfiltration? If there is only 1 outlet, why impose a mass outflow, it's necessarily the same amount than the inflow in steady-state.

Steady-state or transient?
stuart23 likes this.
macfly is offline   Reply With Quote

Old   March 14, 2013, 15:55
Default
  #9
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
Yes, Multi outlet and Steady.
asal is offline   Reply With Quote

Old   March 14, 2013, 16:12
Default
  #10
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Then use Outflow boundary condition and adjust the Flow Rate Weightings

or

Use Pressure Outlet or Outlet Vent boundary condition, turn on Target Mass Flow Rate and enter targeted values.

You should compare the results and the mass balance in order to choose the most appropriate for your problem.
asal likes this.
macfly is offline   Reply With Quote

Old   March 16, 2013, 09:44
Default
  #11
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 156
Rep Power: 5
asal is on a distinguished road
Hello again.

I try two method in last couple of days, First Out-Vent and second Velocity outlet. Since for both, the same amount of flow extracted from the outlets, but I got totally different results! and I have no any experiment to compare. what should I do? Any suggestion?

Additionally, there is another problem!!
The whole amount of flow (kg/s) extracted from the all outlets are a bit smaller than the flow impose to the inlet (kg/s). this additional flow should be extracted from one leakage boundary (Pressure outlet). But fluent reported:
"reversed flow in ** faces on pressure-outlet **. "
I don't know what is the problem?!!!
Any idea/solution?

Thanks

Last edited by asal; March 17, 2013 at 06:01.
asal is offline   Reply With Quote

Old   March 17, 2013, 19:07
Default
  #12
New Member
 
amin masumi
Join Date: Jul 2012
Posts: 16
Rep Power: 5
aminepoxnet is on a distinguished road
hi dear,
I think you should learn some experimental problems that usually occur in modelling
1. usually we can not extract the exact data from modelling and ''a bit'' is not so important
2. back flow in fluent modeling is not so important and usually we have this note bye fluent, I had a piston pump modelling that we got the best results but every time got a note about back flow
In fluent help articles, you can read about this note
3. you should use mechanics fundamentals to know if your data extract by modelling is correct or not and don't forget every time they are not exactly correct but they should be near by correct.
aminepoxnet is offline   Reply With Quote

Old   March 17, 2013, 22:44
Default
  #13
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8
macfly is on a distinguished road
Asal, maybe you could try to refine the mesh and see if the different boundary conditions eventually produce the same results. You will find tons of information about how to perform grid independency study on the forum.

Here's some tips in order to avoid backflow: Reversed Flow in Outlet
And there is probably tons of other threads about backflow.
macfly is offline   Reply With Quote

Old   April 30, 2015, 09:49
Post Reversed flow at the pump outlet
  #14
New Member
 
Binama Aladin Maxime
Join Date: Mar 2015
Posts: 3
Rep Power: 2
Aladinos05 is on a distinguished road
Hi everybody!
I have a problem and I ' ll appreciate any help ! I am simulating the fluid flow through a centrifugal pump but I am having a reversed flow at the outlet !this problem appears Right after starting the calculation, ! My BC is velocity in-pressure out ! I am wondering if this can't affect the results in a way or another! Another question is about the pressure prediction at the inlet ! it is always negative (-) ! I think this can't allow me to calculate the total developed Head and all other head related parameters! Is there any method I can use to have positive values of pressure at the inlet ! I just started using this software so I do not know much about it !! thank u
Aladinos05 is offline   Reply With Quote

Reply

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
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
How to change from mass flow to volume flow rate stanley FLUENT 1 February 2, 2007 07:44
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18
Please help with flow around car modelling! Tudor Miron CFX 17 March 19, 2004 20:23
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 15:55.