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

OpenFoam Pressure Inlet Oulet

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2015, 06:51
Question OpenFoam Pressure Inlet Oulet
  #1
New Member
 
Jorge Lobera
Join Date: Jun 2015
Posts: 6
Rep Power: 3
jlobera is on a distinguished road
Hi all,

I'm new in CFD world; I have been working for three months with OpenFoam doing tutorials and some simple cases.
Now Im working in my first real case. Im trying to simulate flow and temperatura in the interior of a wind turbine using buoyantSimpleFoam solver.

The problem is that we have one outlet where we know the pressure but we don't know if the flow is going to enter or to go out. We have tried several BC but we don't find the correct one.

There are some InletOutlet Bc where you have to specify the velocity in the case of the flow entering; and we dont know this value.

Anyone knows any solution or suggest to my problem? There are any BC where you shouldnt specify the velocity value?

Thank you so much
jlobera is offline   Reply With Quote

Old   June 17, 2015, 04:56
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 328
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

It would probably be best ot use a combination of totalPressure for the pressure (equal to your environment pressure) and a pressureInletOutletVelocity boundary condition on the velocity.

Regards,
Tom
tomf is offline   Reply With Quote

Old   June 17, 2015, 07:02
Default
  #3
New Member
 
Jorge Lobera
Join Date: Jun 2015
Posts: 6
Rep Power: 3
jlobera is on a distinguished road
Thanks Tom,

pressureInletOutletVelocity is one of the BC that i have already tested, but I have used it with fixedFluxPressure for 0/p_rgh.

The problem with pressureInletOutletVelocity is that you should specify the value for the velocity if the flow is entering:

myPatch
{
type pressureInletOutletVelocity;
phi phi;
tangentialVelocity uniform (0 0 0);
value uniform 0;
}


When i have used this BC with this values, the flow is not able to enter. I know that there are zones in my surface where the flow should enter and other zones where the flow should go out.

Thanks
jlobera is offline   Reply With Quote

Old   June 17, 2015, 08:04
Default
  #4
New Member
 
Al_th
Join Date: Apr 2015
Posts: 19
Rep Power: 3
al_th is on a distinguished road
Hi jlobera,

I am currently doing a simulation where I have an outlet that can let flow in or out.

If I remember correctly I am using the following BC at inlet and outlet (I specify fixed pressure at inlet/outlet)

Quote:
Inlet
{
type pressureInletVelocity;
value uniform (0 0 0);
}

Outlet
{
type pressureInletVelocity;
value uniform (0 0 0);
}
I do not have any problem so far and flow looks physically correct.

You could also look at the BC "pressureInletOutletVelocityFvPatchVectorField " :
https://github.com/OpenFOAM/OpenFOAM...hVectorField.H
Quote:
Velocity inlet/outlet boundary condition patches for where the pressure is
specified. zero-gradient is applied for outflow (as defined by the flux)
and for inflow the velocity is obtained from the patch-face normal
component of the internal-cell value.
al_th is offline   Reply With Quote

Old   June 17, 2015, 08:12
Default
  #5
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 328
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi jlobera,

You do not have to specify the tangential velocity part and the "value" entry is just a placeholder for the first time-step. I agree with al_th, it should work. I do believe the fixedFluxPressure would mess things up since that one would need the flux over your patch, which you do not know.

Regards,
Tom
tomf is offline   Reply With Quote

Old   June 17, 2015, 09:48
Default
  #6
New Member
 
Jorge Lobera
Join Date: Jun 2015
Posts: 6
Rep Power: 3
jlobera is on a distinguished road
Thank you so much tomf and al_th,

You are right, the problem was the fixedFluxPressure BC. I have tried using inletOutlet BC for velocity and fixedValue for pressure and it works well.

Can you explain me what's the difference between inletOutlet and pressureInletOutlet? And what is more correct to use in this case?

Regards
jlobera is offline   Reply With Quote

Old   June 17, 2015, 09:55
Default
  #7
New Member
 
Al_th
Join Date: Apr 2015
Posts: 19
Rep Power: 3
al_th is on a distinguished road
As far as I can tell with my (poor) understanding of Openfoam :

- inletOutlet BC : You either have zero-gradient (when flow goes out) or a user specified velocity value (when flow goes in)
- pressureInletOutlet BC : You either have zero-gradient (when flow goes out) or a value that depends on the user specified pressure

If you want to set the pressure at the boundary, then using pressureInletOutlet can let you have a velocity vectorfield that is well defined according to the specified pressure.

Edit : This link can maybe give you additional insight into the pressureInletOutlet BC : pressureInletOutletVelocity
al_th is offline   Reply With Quote

Reply

Tags
air flow simulation, outlet bc, pressure bc, pressure boundary

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
Assign static pressure at inlet Tanjina FLUENT 0 November 3, 2013 12:34
Unsteady pressure differential between inlet and outlet of the pipe for single phase joshi20h FLUENT 0 September 26, 2012 12:41
How to set up the inlet boundary condition for a low pressure case? beastieboys6 FLUENT 3 April 10, 2012 22:46
Question about pressure inlet boundary condition. Alina FLUENT 1 November 30, 2007 08:39
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15


All times are GMT -4. The time now is 23:53.