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

Questions about the inletOutlet and outletInlet boundary conditions

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

Like Tree73Likes
  • 6 Post By brooksmoses
  • 5 Post By brooksmoses
  • 2 Post By mcamps
  • 53 Post By Fransje
  • 4 Post By Ahmed Khattab
  • 2 Post By iamed18
  • 1 Post By vonboett

Reply
 
LinkBack Thread Tools Display Modes
Old   February 1, 2006, 03:38
Default I'm working on a rather simple
  #1
brooksmoses
Guest
 
Posts: n/a
I'm working on a rather simple calculation -- a polar-mesh simulation of flow around a cylinder. On the outer boundary, I want to use a boundary condition that specifies the velocity if it's an inflow, and the pressure if it's an outflow. Page U-148 of the user manual makes it pretty clear that I can do this with the inletOutlet (and possibly the outletInlet) boundary conditions, but beyond that I'm confused.

The first source of my confusion is thus: the inletOutlet boundary condition for the velocity requires two values: "value" and "inletValue". However, I can't see why it would need more than one: it needs the inlet velocity for when it's doing fixedValue on the inlet regions, and doesn't need anything to do zeroGradient on the outlet regions. Thus, my confusion: do I set "value" or "inletValue" to this desired inlet velocity? What do I set the other one to?

The second source of my confusion is that I am uncertain which of the boundary conditions I should use for the pressure. Are they coupled such that I'm expected to use the same one for both U and p, or do I use outletInlet for the pressure since I want it specified at the outlet? And, again, which of "value" or "outletValue" should contain my desired outlet pressure, and what should the other one contain?

Finally: Is this explained in the manual anywhere? What did I miss when I was looking for it?

Thanks much!
  Reply With Quote

Old   February 1, 2006, 05:30
Default Actually, now that I've poked
  #2
brooksmoses
Guest
 
Posts: n/a
Actually, now that I've poked around at this a bit more, I think I've figured most of it out:

* I should use inletOutlet for the velocity, and outletInlet for the pressure.

* The "inletValue" and "outletValue" values are what I should put my desired constraints in.

* The "value" values are where OpenFOAM will put the actual boundary values (which may or may not match the constraints) in the files for the later timesteps.

Is this correct?

Also, I'd still like to know if this is explained anywhere in the manual, so that I'll know where to look when I have a similar question.
lth, solefire, yesaswi92 and 2 others like this.
  Reply With Quote

Old   February 1, 2006, 05:59
Default I am very interested at the re
  #3
Senior Member
 
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 338
Rep Power: 9
lr103476 is on a distinguished road
I am very interested at the results of your cylinder flow. Which Reynolds number are you using? I simulated static cylinders at Re=150, which resulted in certain 'strange' results. Check my thread:

http://www.cfd-online.com/OpenFOAM_D...tml?1138207958

Please post your results.....
Frank
__________________
Frank Bos
lr103476 is offline   Reply With Quote

Old   February 1, 2006, 15:45
Default I saw that thread, yes. I'm d
  #4
brooksmoses
Guest
 
Posts: n/a
I saw that thread, yes. I'm doing steady flow, so my Reynolds numbers are in the range of 10 to 30 or so.

I will indeed post a new thread once I get some results -- right now, I'm still having some convergence problems (due to starting out on a very fine mesh, rather than solving on a coarse mesh and then interpolating the results as an initial condition for the fine mesh).
  Reply With Quote

Old   July 2, 2010, 05:27
Default
  #5
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
Hi, brooksmoses. I'm also confused about inletOutlet and outletInlet boundary conditions. I'm involved in external flows simulations and I need them becouse I can't always know a priori inlet or outlet faces. I agree with the meaning of inletValue, but what about value? You wrote this thread in 2006, maybe you know about that now ;-)
vaina74 is offline   Reply With Quote

Old   September 27, 2010, 04:33
Default
  #6
New Member
 
Marta Camps Santasmasas
Join Date: Feb 2010
Posts: 2
Rep Power: 0
mcamps is on a distinguished road
The value entry is the actual value of the field at the boundary.

At time 0 it is the initial value of the boundary condition. At the first iteration OpenFoam doesn't know if the boundary is an inlet or an outlet, so it needs some initial value to start the simulation.
m_mousavi88 and wenxu like this.
mcamps is offline   Reply With Quote

Old   September 27, 2010, 04:53
Default
  #7
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
thanks, marta. a light in the darkness :-)
vaina74 is offline   Reply With Quote

Old   September 27, 2010, 18:14
Default
  #8
Senior Member
 
Francois
Join Date: Jun 2010
Posts: 107
Rep Power: 7
Fransje is on a distinguished road
Ok.

Let's try to explain inflowOutflot and outflowInflow simply. Let's consider the following code:
Code:
U:
outlet 
{ 
    type inletOutlet;
    inletValue uniform (-2 0 0);
    value (0 0 0);
}
With this boundary condition, we have that:
  • If the velocity vector at the outlet points out of the domain, then the boundary condition will be of the Neumann type, ie, zeroGradient.
  • If the velocity vector points into the domain, then we can imagine that the outflow is no longer an outflow, but an inflow, and that we therefore would like to specify a Dirichlet boundary condition, ie, with constant value. In our case the boundary condition would take the value (-2 0 0), ie, Ux = -2, Uy = 0, Uz = 0.
From what I've read, the value (0 0 0) option is a dummy option needed for paraFoam/paraview and should not further be considered. Please correct me if I'm wrong.

Similarly, if, for some reason, we were to specify:
Code:
k:
outlet 
{ 
    type outletInlet;
    outletValue uniform 5;
    value 0;
}
we would have that
  • If the velocity vector at the outlet was to point out of the domain, then the boundary condition would be of the Dirichlet type, with value 5.
  • If the velocity vector at the outlet was to point into the domain, then the outflow conditions would switch from fixedValue to zeroGradient, and become a Neumann boundary condition.

I hope this was helpful!
Fransje is offline   Reply With Quote

Old   September 28, 2010, 08:13
Default
  #9
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
Another light in the darkness :-)
I notice that everyone has a different theory about the value parameter. The only common thing is its probably irrelevant 'initial value'.
I was interested in this boundary condition becouse I'm involved with external flows, inside spherical or similar domains. So i have a single external boundary - with no inlet or outlet patches - and use so far
Code:
boundaries
    {
        type            inletOutlet;
        inletValue   $internalField;
        value          $internalField;
    }
If I'm wrong, tell me.
Anyway, thanks for your help.
vaina74 is offline   Reply With Quote

Old   November 19, 2010, 15:59
Default Undefined inletValue error
  #10
New Member
 
James Briscoe
Join Date: Nov 2010
Posts: 3
Rep Power: 6
jamessbriscoe is on a distinguished road
Hello everyone,

I'm using the inletOutlet boundary condition to model a bubble collapse problem. I have specified both the inletValue and value keywords for all boundaries, but for some reason OpenFOAM gives me an error that inletValue is undefined.

Any assistance would be greatly appreciated. Below you can see my 0/U file. I set the initial values to correspond to an outlet, and specified inletValues which point towards the center of the domain:

boundaryField
{
inletOutletTop
{
type inletOutlet
inletValue uniform (0 -1 0);
value uniform (0 1 0);
}
inletOutletBottom
{
type inletOutlet;
inletValue uniform (0 1 0);
value uniform (0 -1 0);
}
inletOutletLeft
{
type inletOutlet;
inletValue uniform (1 0 0);
value uniform (-1 0 0);
}
inletOutletRight
{
type inletOutlet;
inletValue uniform (-1 0 0);
value uniform (1 0 0);
}
frontAndBack
{
type empty;
}
}
jamessbriscoe is offline   Reply With Quote

Old   November 19, 2010, 16:14
Default Sorry ignore previous post
  #11
New Member
 
James Briscoe
Join Date: Nov 2010
Posts: 3
Rep Power: 6
jamessbriscoe is on a distinguished road
Sorry everyone, somehow stared at that forever and didn't notice a missing semicolon.

Love looking like an idiot...
jamessbriscoe is offline   Reply With Quote

Old   March 4, 2012, 15:30
Default how is value evaluated at outlet in case of neumann?
  #12
Senior Member
 
Ahmed Khattab's Avatar
 
ahmed
Join Date: Feb 2010
Posts: 161
Blog Entries: 1
Rep Power: 7
Ahmed Khattab is on a distinguished road
Quote:
Originally Posted by Fransje View Post
Ok.

Let's try to explain inflowOutflot and outflowInflow simply. Let's consider the following code:
Code:
U:
outlet 
{ 
    type inletOutlet;
    inletValue uniform (-2 0 0);
    value (0 0 0);
}
With this boundary condition, we have that:
  • If the velocity vector at the outlet points out of the domain, then the boundary condition will be of the Neumann type, ie, zeroGradient.
  • If the velocity vector points into the domain, then we can imagine that the outflow is no longer an outflow, but an inflow, and that we therefore would like to specify a Dirichlet boundary condition, ie, with constant value. In our case the boundary condition would take the value (-2 0 0), ie, Ux = -2, Uy = 0, Uz = 0.
From what I've read, the value (0 0 0) option is a dummy option needed for paraFoam/paraview and should not further be considered. Please correct me if I'm wrong.

Similarly, if, for some reason, we were to specify:
Code:
k:
outlet 
{ 
    type outletInlet;
    outletValue uniform 5;
    value 0;
}
we would have that
  • If the velocity vector at the outlet was to point out of the domain, then the boundary condition would be of the Dirichlet type, with value 5.
  • If the velocity vector at the outlet was to point into the domain, then the outflow conditions would switch from fixedValue to zeroGradient, and become a Neumann boundary condition.

I hope this was helpful!
how is value evaluated at outlet in case of neumann?, and what is the gradient in this case?
Ahmed Khattab is offline   Reply With Quote

Old   May 16, 2012, 11:57
Default Moving a Wall Through Air
  #13
Member
 
Edward Leonard
Join Date: May 2012
Location: Calumet, MI
Posts: 31
Rep Power: 5
iamed18 is on a distinguished road
Hey All,

I have a problem along these same lines, and I just want to make sure that my boundary conditions make sense before I move to my next step. The goal of my simulation is to have the moving wall "move" through open atmosphere (i.e. take the three walls out of the cavity tutorial in favor of inlets/outlets).

So what I did, after reading through these posts, was set the following.

U:
Code:
internalField   uniform (0 0 0);

boundaryField
{
    movingWall
    {
        type            fixedValue;
        value           uniform (10 0 0);
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           (0 0 0);
    }

    frontAndBack
    {
        type            empty;
    }
}
p:
Code:
internalField   uniform 0;

boundaryField
{
    movingWall
    {
        type            zeroGradient;
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           0;
    }

    frontAndBack
    {
        type            empty;
    }
}
icoFoam runs, and when I visualize the velocity field with ParaView, I get the following:


It appears as though the boundary on the left is working more/less correctly, but the boundary on the right almost looks to be acting more like a wall than anything else.

I'd love to hear feedback about this. In the meantime, I'm going to mess around with it a little more.

Thanks!
iamed18 is offline   Reply With Quote

Old   May 17, 2012, 09:06
Default Figured that Out
  #14
Member
 
Edward Leonard
Join Date: May 2012
Location: Calumet, MI
Posts: 31
Rep Power: 5
iamed18 is on a distinguished road
Alas, it has been resolved. I was able to simulate the wall moving through air with the following:

U:
Code:
boundaryField
{
    movingWall
    {
        type            fixedValue;
        value           uniform (10 0 0);
    }

    leftWall
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    rightWall
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    bottomWall
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    frontAndBack
    {
        type            empty;
    }
}
p:
Code:
boundaryField
{
    movingWall
    {
        type            zeroGradient;
    }

    rightWall
    {
        type            fixedValue;
        value           uniform 0;
    }

    leftWall
    {
        type            fixedValue;
        value           uniform 0;
    }

    bottomWall
    {
        type            fixedValue;
        value           uniform 0;
    }

    frontAndBack
    {
        type            empty;
    }
}
Hope this helps someone else!
caduqued and eRzBeNgEl like this.
iamed18 is offline   Reply With Quote

Old   March 20, 2013, 06:23
Default
  #15
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 183
Rep Power: 7
vonboett is on a distinguished road
totalPressure for p at left / right / bottom wall would probably work well, too
nisha likes this.
vonboett is offline   Reply With Quote

Old   August 25, 2013, 09:11
Default
  #16
New Member
 
JAY
Join Date: Jul 2013
Posts: 10
Rep Power: 4
JAY ADHVARYU is on a distinguished road
I have some problem with my boundary condition that how i utilize the neumann condition(∂φ/∂x = 0) at outlet. Can i select pressure outlet at outlet?
my inlet condition is :
flat velocity profile =40m/s
Re=1.916*10^5
turbulent intensity=4.5%
And Inlet height of duct=5mm


I select velocity inlet at inlet because my flow is incompresible.
And axis boundary condition applied along the centerline.
and no slip condition at wall.

pls help me.
JAY ADHVARYU is offline   Reply With Quote

Old   October 4, 2013, 10:42
Question
  #17
Senior Member
 
Join Date: Jan 2013
Posts: 202
Rep Power: 5
openfoammaofnepo is on a distinguished road
Hi All,

It is very interesting about this kind of boundary condition. For inletOutlet, in most cases, if the flux is pointed into the flow domain, then this corresponds to the reverse flow. For this situation, Openfoam will ask us to input the inletValue, however, how can we the velocity when the flow direction is into the domain? In other words, how to specify the inletValue for it?

Any comments? Thank you so much!

Quote:
Originally Posted by rebel ahmed View Post
how is value evaluated at outlet in case of neumann?, and what is the gradient in this case?
openfoammaofnepo is offline   Reply With Quote

Old   October 4, 2013, 12:56
Default
  #18
New Member
 
JAY
Join Date: Jul 2013
Posts: 10
Rep Power: 4
JAY ADHVARYU is on a distinguished road
Generally Neumann condition or Drichlate condition at outlet or inlet improve the stability of your result that conditions specify the behaviour of the flow and thats so tricky in my case i used neumann condition at outlet as(∂φ/∂x = 0) where φ=U,V but how it useful in openform that i don't know because i use Fluent & CFX.
JAY ADHVARYU 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
Inletoutlet rengu OpenFOAM Running, Solving & CFD 7 June 8, 2015 03:02
Burgerbs equation non constant Boundary Conditions Initial Conditions arkangel OpenFOAM Running, Solving & CFD 1 October 2, 2008 14:48
questions in initial conditions and inlet boundary nick CFX 2 April 19, 2008 09:26
TwoPhaseEulerFoam and InletOutlet boundary condition hemph OpenFOAM Running, Solving & CFD 10 January 29, 2007 10:47
Integral boundary conditions turbulent intensitylength boundary conditions olesen OpenFOAM Running, Solving & CFD 0 July 27, 2006 07:18


All times are GMT -4. The time now is 17:32.