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

backflow with pressureInletOutletVelocity BC

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

Like Tree3Likes
  • 1 Post By Yann
  • 1 Post By geth03
  • 1 Post By Yann

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 15, 2024, 11:41
Default backflow with pressureInletOutletVelocity BC
  #1
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 366
Rep Power: 8
geth03 is on a distinguished road
hi all,

despite declaring the outlet as pressureInletOutletVelocity with zero inflow velocity:

"outlet.*"
{
type pressureInletOutletVelocity;
phi phi;
inletValue uniform (0 0 0);
value uniform (0 0 0);
}

i am having backflow from the outlet patch. (see atached screenshot)

i thought that inletValue -> 0 would prevent backflow in the domain, am i missing something?

any help is appreciated, kind regards
Attached Images
File Type: jpg backflow.jpg (57.4 KB, 15 views)
geth03 is offline   Reply With Quote

Old   February 15, 2024, 12:03
Default
  #2
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
Hello,

I think there is a confusion about the BC name: if you want to avoid backflow you should use an inletOutlet BC with inletValue set to 0.

The whole point of pressureInletOutletVelocity BC is to be able to compute a velocity if there is back flow. (And there is no inletValue parameter for pressureInletOutletVelocity )

Regards,
Yann
geth03 likes this.
Yann is offline   Reply With Quote

Old   February 15, 2024, 12:25
Default
  #3
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 366
Rep Power: 8
geth03 is on a distinguished road
hi Yann,

thanks for your fast response.

HTML Code:
https://github.com/OpenFOAM/OpenFOAM-10/blob/master/tutorials/lagrangian/denseParticleFoam/cyclone/0/U.air
here, however the BC is used like my post above, actually i copied my BC from this tutorial. it is kind of misleading that this appears in a tutorial if it is not even used.
Yann likes this.
geth03 is offline   Reply With Quote

Old   February 15, 2024, 12:44
Default
  #4
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
Yes it often happens in tutorials and it can be quite misleading indeed.

Since you are using OpenFOAM-10, foamInfo is pretty handy to get information about boundary conditions. (and other things!)

Code:
foamInfo pressureInletOutletVelocity
geth03 likes this.
Yann is offline   Reply With Quote

Old   March 16, 2024, 10:40
Default
  #5
Member
 
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 84
Rep Power: 6
2538sukham is on a distinguished road
The outflow boundary condition for velocity in some paper in this case attached is kept as zeroGradient. I am confused about the pressure boundary condition? For now I am following the damBreak atmosphere boundary condition totalPressure with p0 as 0. Whereas somewhere I found that they have specified a pressure value at the outlet. Although the simulation runs, I am skeptic of the fixed pressure with zeroGradient of velocity at outlet. Any suggestions? @Yann
Attached Images
File Type: png shotSleeve.png (17.8 KB, 6 views)
2538sukham is offline   Reply With Quote

Old   March 18, 2024, 05:07
Default
  #6
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
Hello Michael,

I am not sure to understand your question.
Whether you use totalPressure or fixedValue at the outlet, you're still defining a fixed pressure (either fixing static or total pressure).

For the velocity, zeroGradient is fine as long as there is no backflow, otherwise it might be unstable.
PressureInletOutletVelocity is useful if you do expect backflow and you want a BC able to handle it.
Another common BC is to use inletOutlet on the velocity at the outlet, with an inletValue of (0 0 0). This is a way to forbid backflow as you specify a 0 velocity on it.

I hope this helps,
Yann
Yann is offline   Reply With Quote

Old   March 18, 2024, 09:05
Smile
  #7
Member
 
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 84
Rep Power: 6
2538sukham is on a distinguished road
Velocity:
outlet
{
type inletOutlet;
phi phi; //Don't know since its optional
inletValue uniform 0; // No backFlow or velocity (0 0 0)
value uniform 0; // Isn't it suppose to give me zeroGradient?
}
Pressure: p_rgh

outlet
{
type totalPressure;
value uniform 0; // Setting a fixed pressure 0 Pa.
}
Apart from some doubts which let me look into the src I think considering no backFlow, the U and p_rgh bc works with this combination. Thank you Yann.
2538sukham is offline   Reply With Quote

Old   March 18, 2024, 09:37
Default
  #8
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,193
Rep Power: 27
Yann will become famous soon enough
This should be the proper syntax, as U expect a vector instead of a scalar:
Code:
outlet
{
	type		inletOutlet;
	inletValue	uniform (0 0 0);
	value		uniform (0 0 0);
}
And for totalPressure, the total pressure you want to fix is defined by the p0 parameter which is missing in your example.

Code:
outlet
{
	type	totalPressure;
	p0	uniform 0;
	value	uniform 0;
}
On both boundary conditions, the value parameter is just a placeholder, it won't affect the behavior of your boundary condition (and I think you should be able to remove it in recent openfoam versions).
(more details here: What is the difference between the parameters 'value' and 'p0' in totalPressure BC?)
Yann is offline   Reply With Quote

Old   March 18, 2024, 09:45
Default
  #9
Member
 
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 84
Rep Power: 6
2538sukham is on a distinguished road
Sorry forgot about the volVectorField. Yes it should be (0 0 0). I messed up the syntax about p0 as well. If I get into the more technical stuff, I would post here so that others could follow. Thanks!!
P.S: Since there is no inlet pressure in this case (i.e. moving wall - fixedFluxPressure) I think the value of pressure p0 wouldn't matter as the simulation is incompressible and its the pressure difference which is the driving force and not the absolute pressure.
2538sukham is offline   Reply With Quote

Old   March 18, 2024, 17:00
Default
  #10
Member
 
Ching Liu
Join Date: Sep 2017
Posts: 52
Rep Power: 9
qingqingliu is on a distinguished road
Quote:
Originally Posted by geth03 View Post
hi all,

despite declaring the outlet as pressureInletOutletVelocity with zero inflow velocity:

"outlet.*"
{
type pressureInletOutletVelocity;
phi phi;
inletValue uniform (0 0 0);
value uniform (0 0 0);
}

i am having backflow from the outlet patch. (see atached screenshot)

i thought that inletValue -> 0 would prevent backflow in the domain, am i missing something?

any help is appreciated, kind regards
The backflow may not be related to your outlet boundary condition setup, instead, it could be caused by the setup of your problem. It is better to describe your whole geometry and problem.
qingqingliu 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
UDF to simulate one-way valves in ANSYS Fluent to prevent backflow viliam_kacerik Fluent UDF and Scheme Programming 1 August 26, 2021 15:05
backflow chirag.palan1987@yahoo.in FLUENT 0 June 1, 2015 03:42
Inducing backflow restrictions in domain interface for multiphase flow DarrenC CFX 4 August 6, 2014 22:17
Modeling Backflow for a 3D Airfoil (Wing of Finite Span) Josh CFX 9 August 18, 2009 12:31
Swirl in backflow on pressure outlets Jonas Larsson FLUENT 17 February 3, 2000 03:14


All times are GMT -4. The time now is 19:49.