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

Outlet pressure boundary condition in interFoam

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 4, 2013, 18:25
Default Outlet pressure boundary condition in interFoam
  #1
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
I am running an interFoam case with inlet and outlet and I don't know how to define the pressure (p_rgh) boundary condition in the outlet. I tried to use the same as the patch "sky" in the damBreak tutorial, but I got a physical no-sense (see attached screenshot).

I also tried several solutions, such as that of this link and several of CFD-online, but my simulations either didn't run or diverged after a few iterations. I know it's some tiny detail I'm missing, but I don't know what to do. I also tried a "zeroGradient" type of boundary condition for pressure and "fixedValue" of zero, but it didn't work.

Thank you very much!
Attached Images
File Type: jpg screenshot_outlet_interfoam.jpg (71.1 KB, 121 views)
arnau1985 is offline   Reply With Quote

Old   July 9, 2013, 11:27
Default
  #2
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
You didn't say exactly what your simulation is and the picture didn't help me much.

I use LTSInterFoam for ship hydrodynamic calculations and typically go for zeroGradient or fixedValue uniform 0 for the dynamic pressure term at the outlet. I suppose you could also use something like inletOutlet too.
Artur is offline   Reply With Quote

Old   July 10, 2013, 04:19
Default Details on "Outlet pressure boundary condition in interFoam"
  #3
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Hi Artur,

You're right, I gave very scarce information. I've attached a new picture with some more details on the pressure boundary conditions (henceforth B.C.) of my simulations.

As regards the outlet, as you suggested, I've used a zeroGradient as well as a fixedValue uniform 0 and it didn't work. I also copied the B.C. settings of the "atmosphere" patch in damBreak (inletOutlet type in "boundary" and totalPressure for "p_rgh") and I always get the same result.

However, I've recently observed that at higher inlet velocities, the jet leaves the domain though the right-hand outlet instead of through the bottom and everything works perfectly. I've also run the damBreak case changing one of the side walls to an outlet B.C. and this "spurious" bubbles didn't appear either. Is it possible that this problem only arises when the outlet is horizontal (i.e. perpendicular to the gravity direction)? Maybe it's due to the use of "p_rgh" (gravity corrected pressure) instead of "p".

Thank you very much for your help.

Regards,

Arnau.
Attached Images
File Type: jpg screenshot_outlet_interfoam.jpg (85.0 KB, 71 views)
arnau1985 is offline   Reply With Quote

Old   July 10, 2013, 04:30
Default
  #4
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Ok, I see what you mean now. Unfortunately I don't know much about gravity driven flow simulations as I use interFoam only to calculate the free surface of moving ships so hopefully someone more experienced will have a look at your post. In the meantime, your mesh seems fairly coarse in the outlet region, have you tried refining it a bit to see if it makes a difference?

P.S. I don't think that the horizontal orientation of the outlet should make any difference because it seems like it should be (by enlarge) perpendicular to the flow of the jet.
Artur is offline   Reply With Quote

Old   July 10, 2013, 04:43
Default
  #5
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Posts: 233
Rep Power: 7
Phicau is on a distinguished road
Hi Arnau,

I think the problem may be caused by the bottom outlet, as I guess it is located below Z = 0 plane.

Try making all your outlet patchs be located in the first quadrant (x,y,z>0) and use the same BCs as for the atmosphere and let us know if it gets better.

Best,

Pablo
Phicau is offline   Reply With Quote

Old   July 10, 2013, 08:26
Default
  #6
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
@Artur:

Maybe you're right about the mesh, I haven't had the time to try more refined meshes (I'm running some simulations as I write). However, the damBreak case run perfectly with a coarser mesh and with an outlet instead of one of the side walls, as I described in my previous post.

@Pablo:

You're right, the outlet was below the Z=0 plane. Indeed, in previous simulations I've observed that everything started going bad when the jet crossed this plane (that sounds kind of esoteric, doesn't it?). Nevertheless, I've run the same simulation as you said: in the first quadrant and with the same BC as the atmosphere but I still get the same result (I've attached a video). I'm trying finer meshes to see what happens, I'll let you know about the results.

Video: https://www.dropbox.com/s/corgjwhem1...let_as_sky.avi

BTW, these are the dictionaries of my outlet patch:

Code:
// boundary

        outlet
        {
            type            wall;
        }

// U

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


// alpha1, k, epsilon

    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }


// p_rgh

    outlet
    {
        type            totalPressure;
        p0              uniform 0;
        U               U;
        phi             phi;
        rho             rho;
        psi             none;
        gamma           1;
        value           uniform 0;
    }
Thank you very much for your help!

Best,


Arnau.
arnau1985 is offline   Reply With Quote

Old   July 10, 2013, 08:37
Default
  #7
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I noticed you defined the outlet as a wall in your boundary file. Maybe try changing it to patch? On the video it appears as if the flow is not passing through the outlet so perhaps this is the reason.
Artur is offline   Reply With Quote

Old   July 10, 2013, 08:48
Default
  #8
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Posts: 233
Rep Power: 7
Phicau is on a distinguished road
Hi,

try this:

Code:
// alpha1

    outlet
    {
        type            inletOutlet;
        inletValue      0;
        value           $internalField;
    }
Phicau is offline   Reply With Quote

Old   July 10, 2013, 10:28
Default
  #9
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
@Artur:

I used "wall" as B.C. because is the type to which the patch "atmosphere" belongs. I also tried the generic "patch" and I got the same result.

@Pablo:

Since my alpha1 "internalField" is assigned "uniform 0", what you suggest is what I have been trying.

Any idea? This is exhausting... I'll let you know what happens with the finer-mesh simulations.

Best,

Arnau.
arnau1985 is offline   Reply With Quote

Old   July 11, 2013, 03:16
Default
  #10
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Here are the results with a finer mesh and the problem persists:

https://www.dropbox.com/s/t8ekfxdm20...resolution.avi

I've zipped the entire simulated case (before running), in case somebody wanted to check it out:

https://www.dropbox.com/s/fnc8nuu1iwp4h5e/dam.zip

I don't know what else I should try...
arnau1985 is offline   Reply With Quote

Old   July 11, 2013, 03:28
Default
  #11
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Posts: 233
Rep Power: 7
Phicau is on a distinguished road
Well, actually in this case you provided the bottom outlet is actually included in patch "wall" instead of being part of "outlet"...
Artur likes this.
Phicau is offline   Reply With Quote

Old   July 11, 2013, 03:46
Default
  #12
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Yes, Pablo, this is the last case I run, but as I told you I tried with "patch" as well. Anyway, the patch "atmosphere" in damBreak is defined as "wall", that's why this was my first option.
arnau1985 is offline   Reply With Quote

Old   July 11, 2013, 03:54
Default
  #13
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Posts: 233
Rep Power: 7
Phicau is on a distinguished road
What I mean is that the bottom portion you intend to use as an outlet is actually a part of the boundary called "wall" instead of the one called "outlet" (disregarding if they are either a patch or a wall type), so the boundary conditions of "wall" apply instead of the boundary conditions of "outlet". See the attached picture ("wall" in red and "outlet" in blue)
Attached Images
File Type: jpg patches.jpg (37.4 KB, 50 views)
Phicau is offline   Reply With Quote

Old   July 11, 2013, 03:57
Default Random question
  #14
New Member
 
Bryan
Join Date: Jul 2013
Posts: 3
Rep Power: 3
Missileman is on a distinguished road
Hi, I'm new to this forum. I'm trying to create a new post but I can't find the "New Post" or "New Thread" button. Help?
Missileman is offline   Reply With Quote

Old   July 11, 2013, 04:02
Default
  #15
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Yes, since I thought the horizontal outlet may have been the cause of my troubles, I tried to define as outlet only the vertical patches (again, I tried both cases, but the one I uploaded was the last one). Anyway, the result is the same: the water keeps on blocking at the outlet.

Thanks for your time, Pablo!
arnau1985 is offline   Reply With Quote

Old   July 11, 2013, 04:02
Default
  #16
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Quote:
Originally Posted by Missileman View Post
Hi, I'm new to this forum. I'm trying to create a new post but I can't find the "New Post" or "New Thread" button. Help?
Here, below the sub-forum list:

http://www.cfd-online.com/Forums/openfoam/
Artur is offline   Reply With Quote

Old   July 11, 2013, 04:05
Default
  #17
New Member
 
Bryan
Join Date: Jul 2013
Posts: 3
Rep Power: 3
Missileman is on a distinguished road
Quote:
Originally Posted by Artur View Post
Here, below the sub-forum list:

http://www.cfd-online.com/Forums/openfoam/
Many thanks!
Missileman is offline   Reply With Quote

Old   July 11, 2013, 04:12
Default
  #18
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Quote:
Originally Posted by arnau1985 View Post
Yes, since I thought the horizontal outlet may have been the cause of my troubles, I tried to define as outlet only the vertical patches (again, I tried both cases, but the one I uploaded was the last one). Anyway, the result is the same: the water keeps on blocking at the outlet.

Thanks for your time, Pablo!
Have you tried pure zeroGradient BC at the outlet for alpha1? From the description given here:

Inletoutlet

I thought that maybe if your outflow is not strong enough it will not actually leave the domain? This would tie in with what you said earlier that with increased inlet velocity the problem disappears. Just a thought...
Artur is offline   Reply With Quote

Old   November 26, 2013, 09:57
Default BC located at z=0 => rho*g*h = 0
  #19
New Member
 
Thibault Pringuey
Join Date: Mar 2009
Posts: 17
Rep Power: 8
thibault_pringuey is on a distinguished road
Hello Arnau,

I am sort of looking at the similar issues. As you suggested, I believe that the issue related to the setting of a static pressure BC with p_rgh.

Have you tried setting your outlet BC to z=0 such that by setting fixed value of p_rgh = p_outlet_static + rho*g*0 = p_outlet_static?

Anyway, have you solved your problem?

Regards,


Thibault
thibault_pringuey is offline   Reply With Quote

Old   November 26, 2013, 11:00
Default
  #20
New Member
 
arnau1985's Avatar
 
Arnau
Join Date: Jan 2012
Posts: 17
Rep Power: 5
arnau1985 is on a distinguished road
Hi Thibault,

I solved the problem to a certain extent. What I did is the following: I realized that supercritical flow outlets in OpenFOAM behave as expected as long as there is no flow separation (I got the idea from this tutorial). So I replaced the spill of my model with a descending slope (see attached picture), set all the variables at the outlet to zeroGradient (except for pressure, which I set to buoyantPressure) and everything ran smoothly.

I am still trying to do all this in a more elegant way without spills, slopes and so on: just directly imposing a given water depth and a hydrostatic pressure profile at the outlet. I will try to keep you informed of my findings.

Good luck!

Arnau.
Attached Images
File Type: jpg hydraulicjump.jpg (7.0 KB, 61 views)
arnau1985 is offline   Reply With Quote

Reply

Tags
interfoam outlet p_rgh

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
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Outlet boundary condition for wave flume with interFoam solver Arnoldinho OpenFOAM 8 May 23, 2012 06:25
Pressure Outlet Guage pressure Mohsin FLUENT 34 January 12, 2012 06:45
Fluent natural ventilation pressure boundary condition pierresandre FLUENT 24 November 8, 2011 15:32
Turbulent intensity for pressure Outlet Boundary condition Mohsin FLUENT 1 April 30, 2010 10:36


All times are GMT -4. The time now is 20:26.