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

Time dependant pressure boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 30, 2013, 02:38
Default Time dependant pressure boundary condition
  #1
New Member
 
yosuke
Join Date: Aug 2011
Posts: 5
Rep Power: 0
yosuke1984 is on a distinguished road
Dear all

Does anyone know validation result for unsteady icoFoam and smagorinsky model LES using pisoFoam ?
UNSTEADY here means both using 'unsteady solver' and 'time dependent boundary condition'

I have been using OpenFOAM about three month for aortic flow, but solver could not offer sufficient stabilities nor the results looks strange.
I need to solve identical geometry by unsteady pressure and unsteady velocity boundary conditions.
The result was identical in v2.1.1 and v1.6-ext.

Using inlet velocity curve was relatively stable, but chaos comes if time dependent pressure boundary condition is introduced.
I tested myself identical mesh in fluent 6.3.6 which gave 10 times smaller pressure ( pressure converted kinematic to real ) and fluent result matches measurement order.

The points I would like to ask is following.

1.
I found many comparisons with commercial softwares and experiments result unsteady calculation using time independent boundary condition, yet still can not find test result under unsteady boundary condition.
Is any such comparison available ? I am not fully confident with time dependent pressure boundary condition in OpenFOAM.

2.
What is the appropriate boundary condition settings for both time dependent velocity boundary condition and time dependent pressure boundary condition ?
Is anything wrong with my setting ?

-------------------------------------------------------------------
my setting for solving by time dependent pressure boundary (icoFoam)
-------------------------------------------------------------------
0/p

Quote:
inlet
{
type uniformFixedValue;
uniformValue tableFile;
tableFileCoeffs
{
fileName "$HOME/data/a0.5E-3.data";
outOfBounds clamp;
}
}

outlet
{
type fixedValue;
value uniform 0;
}

wall
{
type zeroGradient;
}

0/U
inlet
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

wall
{
type fixedValue;
value uniform (0 0 0);
}
note: I also test pressureInletOutletVelocity for inlet and outlet but result couldn't see notable difference.

---------------------------------------------------------------------
my setting for solving by time dependent velocity boundary (icoFoam)
---------------------------------------------------------------------
0/U

Quote:
inlet
{
type zeroGradient;
value uniform (0 0 0);
}

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

wall
{
type fixedValue;
value uniform (0 0 0);
}

0/p
inlet
{
type uniformFixedValue;
uniformValue tableFile;
tableFileCoeffs
{
fileName "$HOME/FOAM/kim2010/p_diff1.0E-5.data";
outOfBounds clamp;
}
}

wall
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 0;
}
yosuke

Last edited by yosuke1984; March 30, 2013 at 08:59. Reason: formatting and spell corrections
yosuke1984 is offline   Reply With Quote

Old   April 2, 2013, 06:14
Default
  #2
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 240
Rep Power: 9
olivierG is on a distinguished road
hello yosuke,

First, i would not use icoFoam for transient case: use pisoFoam or pimpleFoam instead.

Then i would say your BC settings are not optimal.
1) I do not see any difference between your time dependent velocity and pressure case, just the file you use: this is typo ?

2) You are setting P at inlet and outlet, and zeroGradient for velocity for inlet / outlet. This is clearly unstable/not physical if p is not constant at inlet or outlet, which is your case at inlet.
I have not the correct answer here, but you could try:
0/p
inlet: uniformFixedValue;// with your changing P field.
outlet: fixedValue 0
0/U
inlet: advective
outlet: advective (or zeroGradient).

But setting velocity at outlet (then zeroGradient for p), will clearly work here.

Your trouble come from the zeroGradient for velocity at inlet, since pressure is not constant. And you just discovert that your Fluent inlet/outlet is not a zeroGradient condition exactly.

Hope this help.

regards,
olivier
olivierG is offline   Reply With Quote

Old   April 7, 2013, 10:36
Default
  #3
New Member
 
yosuke
Join Date: Aug 2011
Posts: 5
Rep Power: 0
yosuke1984 is on a distinguished road
Dear Olivier

Thank you very much for your reply. It worked.
yosuke1984 is offline   Reply With Quote

Old   May 6, 2015, 06:16
Default Doubt with implementation of transient velocity b.c
  #4
Member
 
Saideep
Join Date: Apr 2015
Location: INDIA
Posts: 61
Rep Power: 2
Saideep is on a distinguished road
Hi guys;

I am relatively new to the forum.
I am trying to inject an air bubble into a fluid of ethanol and see the flow of the air bubble through a rectangular 2D channel as an initial step based on a paper.

I have a rectangular bubble which I would like to relax it from rectangular to (curved at edges due to the influence of surface tension). So, it can take around 0.003s. (Notice time scale is small and I deal with interFoam solver). After, relaxing i inject with a uniform velocity of 0.0167m/s for a brief period of time say 0.01s.

Could you please let me know what sort of a boundary condition is to be used for the inlet and also at the outlet.

Thanks a lot for your patience and help.
Saideep is offline   Reply With Quote

Reply

Tags
pressure boundary, transient bcs

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
pressure wall boundary condition in CFX murx CFX 4 October 9, 2012 06:50
Fluent natural ventilation pressure boundary condition pierresandre FLUENT 24 November 8, 2011 15:32
pressure boundary condition in fractional step Jean-Fran├žois Corbett Main CFD Forum 3 January 10, 2006 09:49
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18


All times are GMT -4. The time now is 05:08.