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

Setting mass flow rate boundary condition

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

Like Tree12Likes
  • 6 Post By philippose
  • 1 Post By maysmech
  • 2 Post By philippose
  • 1 Post By linnemann
  • 2 Post By Dadou

Reply
 
LinkBack Thread Tools Display Modes
Old   October 26, 2010, 11:24
Question Setting mass flow rate boundary condition
  #1
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Dear Foamers,

How can i define mass flow rate boundary instead of velocity for a case simulation in OpenFOAM?
maysmech is offline   Reply With Quote

Old   October 26, 2010, 13:41
Default
  #2
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello there,

A Good Evening to you :-)!

To specify a flow rate instead of a velocity, you can use the boundary condition:

flowRateInletVelocity

For an example of how to use it, check the following file in the tutorials folder of OpenFOAM:

/compressible/rhoPimpleFoam/angledDuct/0/U


Hope this helps.

Have a nice day ahead!

Philippose
koooje, pfhan, m_mousavi88 and 3 others like this.
philippose is offline   Reply With Quote

Old   October 26, 2010, 14:53
Default
  #3
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Dear Philippose,
Thank you very much for your answer.
two questions:

i think it is suitable for inlet patches, isn't it? i need sth for outlet patch.

if i use it for inlet, in tutorial file P type is set to zeroGradient. can we suppose it in flow which comes from a duct as zeroGradient when (as you know) it has pressure drop across the duct?

Best regards,
Maysam
koooje likes this.

Last edited by maysmech; October 26, 2010 at 15:32.
maysmech is offline   Reply With Quote

Old   October 26, 2010, 14:55
Default
  #4
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
And 3rd question:

How can i calculate mass flow rate of a patch by using paraView?
maysmech is offline   Reply With Quote

Old   October 26, 2010, 18:10
Default
  #5
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hi again,

* If I remember right, you can use the flowRateInletVelocity patch as an output simply by changing the sign of the flow rate value, to indicate that it is flowing out of the domain.

* Normally, you cannot specify a fixed velocity (flow rate) and a pressure on the same boundary..... this is why, you need to provide a zeroGradient boundary condition for the pressure when you supply the flow rate as an input parameter. .... I am not sure what you imply by a pressure drop across the input boundary in a duct.

* Paraview has a filter which lets you integrate a variable over a surface (I think the filter is called Surface Flow).... this should give you the flow rate, however, I remember that I had an issue trying to interpret the output of this filter..... try it out anyway.... it basically calculates the dot product of a flow field and the normal vectors of the surface.

Philippose
mwaqas and wmrlak like this.
philippose is offline   Reply With Quote

Old   November 4, 2010, 01:55
Default
  #6
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
As i understand, the flow rate boundary is same as setting a fixed value velocity in the boundary and this is not useful for cases which our velocity profile is not uniform.
maysmech is offline   Reply With Quote

Old   November 4, 2010, 02:20
Default
  #7
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hi,

The question then is, what exactly did you want to do?

a. Specify a uniform flow rate at the input
b. Specify a uniform velocity at the input
c. Specify a non-uniform velocity profile at the input (spatially non-uniform across the input patch)
d. Specify a non-uniform flow rate at the input (spatially non-uniform across the input patch)

In case it was (d), how would you specify the flow rate? would it be the flow rate through each patch element face?

In which case it would be something like specifying a non-uniform velocity profile where v_face = Q_face / A_face

For specifying a parabolic Inlet velocity, you have the boundary condition: "parabolicVelocity"

In addition, you could try to create a customised non-uniform velocity / flow inlet using the "groovyBC" library.

Have a nice day ahead!

Philippose
philippose is offline   Reply With Quote

Old   November 4, 2010, 02:58
Default
  #8
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Thanks Philippose,
I want it for an outlet patch that is not uniform velocity. for example a T-junction geometry with two different outputs and i want control rate as 20% and 80% in outlets by setting mass flow rate.

Best,
maysmech is offline   Reply With Quote

Old   December 16, 2011, 04:53
Default
  #9
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Hi Maysam,

Did you ever get this to work? I am also interested in such a boundary condition with a mass flow rate that is dictated, but also keeps in some way the zero gradient condition there.
Bernhard is offline   Reply With Quote

Old   August 21, 2013, 03:23
Default
  #10
New Member
 
H.Martens
Join Date: Feb 2013
Posts: 2
Rep Power: 0
Spidermohaa is on a distinguished road
I am, too!
Spidermohaa is offline   Reply With Quote

Old   August 21, 2013, 03:39
Default
  #11
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

you can use something lige this (OF22)

for inlet use zeroGradient for outlet use this

Code:
   outlet
    {
        type            flowRateInletVelocity;
        volumetricFlowRate    constant -0.1; // m3/s, negative sign means out of the domain
        value           uniform (0 0 0);
    }
mwaqas likes this.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   February 6, 2014, 03:37
Default
  #12
Member
 
Mehdi GHOZALI
Join Date: May 2013
Location: Dubai, UAE
Posts: 65
Rep Power: 4
Dadou is on a distinguished road
Hi,

Quote:
Originally Posted by linnemann View Post
Hi

you can use something lige this (OF22)

for inlet use zeroGradient for outlet use this

Code:
   outlet
    {
        type            flowRateInletVelocity;
        volumetricFlowRate    constant -0.1; // m3/s, negative sign means out of the domain
        value           uniform (0 0 0);
    }
So if I understood well, if we have a flow in the inlet and outlet (going out of the domain) we need to set inlet = zeroGradient and then put a flow in the outlet ??!!

Thank you
mwaqas and wmrlak like this.
Dadou is offline   Reply With Quote

Old   May 28, 2015, 09:49
Default
  #13
New Member
 
James F.
Join Date: May 2015
Posts: 20
Rep Power: 1
NoradFirst2 is an unknown quantity at this point
I have a quite similar problem and I cannot find the answer.

I am using buoyantPimpleFoam currently.

I have

inlet : U is fixedValue / P is zeroGradient / T is fixedValue

suction_outlet : U is zeroGradient / P is fixedValue (0.995e5) / T is zeroGradient

secondary_outlet (actually, suction_outlet sucks air from this patch in addition to air from the inlet) : U is zeroGradient / P is fixedValue (1e5) / T is inletOutlet (calculated with internalField - to prevent air coming inside the domain from this patch being at 0K).

I'd like to change my suction BC to have a given volumicFlowRate rather than fixed pression which is causing instability. I tryed something like :

Code:
   U
 
suction
    {
        type            flowRateInletVelocity;
        volumetricFlowRate    constant -130; // m3/s, negative sign means out of the domain
        value           uniform (0 0 0);
    }
 
P
 
suction {type     zeroGradient}
But then, the velocity field is 0 nearby, suction is behaving like the outlet...

Do you have any advice? Thanks!!

PS : What does the line " value uniform (0 0 0);" in flowRateInletVelocity stands for?

EDIT - PB SOLVED: I had a unit problem.

Last edited by NoradFirst2; June 9, 2015 at 07:52. Reason: Problem solved
NoradFirst2 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
inlet velocity boundary condition murali CFX 5 August 3, 2012 08:56
How to change from mass flow to volume flow rate stanley FLUENT 1 February 2, 2007 07:44
Target mass flow rate Saturn FLUENT 0 December 10, 2004 05:18
Mass flow boundary condition Síle FLUENT 0 June 12, 2003 07:30
Constant mass flow rate / choking outlet bounardy condition Min Zhu Main CFD Forum 1 September 29, 1998 15:33


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