|
[Sponsors] |
June 6, 2006, 11:31 |
Hi,
In simpleFoam, is there
|
#1 |
New Member
Greg Zink
Join Date: Mar 2009
Location: Ames, Iowa, USA
Posts: 16
Rep Power: 17 |
Hi,
In simpleFoam, is there a way to set an inlet-BC knowing only pressure, rather than needing pressure and velocity? All the ones I've tried need a velocity at the inlet, too. Greg Z. |
|
June 6, 2006, 11:51 |
Yes, you need
pressureInlet
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
Yes, you need
pressureInletVelocity, which lives in src/finiteVolume/fields/fvPatchFields/derivedFvPatchFields/pressureInletVelocity /pressureInletVelocityFvPatchVectorField.H You will, of course, also fix the pressure at the outlet, right? Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
June 6, 2006, 13:07 |
Thanks Hrv,
Right now I am
|
#3 |
New Member
Greg Zink
Join Date: Mar 2009
Location: Ames, Iowa, USA
Posts: 16
Rep Power: 17 |
Thanks Hrv,
Right now I am running OpenFoam 1.2 and the closest I can find to what you mention is src/cfdtools/general/derivedFvPatchFields but there is no pressureInletVelocity directory there. Is it somewhere else in the older versions, or perhaps not there at all? Greg Z. |
|
June 6, 2006, 13:23 |
You should really wwitch to 1.
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
You should really wwitch to 1.3 as soon as you possibly can - there's no point of anyone asking questions or supporting the old version because this does not help us move forward.
As for the file, it lives in: /home/hjasak/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/fields/fvPatchFields/derivedFvPa tchFields/pressureInletVelocity If you want to see what data it needs, specify the b.c. type as pressureInletVelocity and look at the stuff it asks you to provide. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
June 7, 2006, 09:54 |
Thanks again.
Forgive the n
|
#5 |
New Member
Greg Zink
Join Date: Mar 2009
Location: Ames, Iowa, USA
Posts: 16
Rep Power: 17 |
Thanks again.
Forgive the novice question, but where do I need to put that file for the BC? I've looked through the code, but I'm not very experienced in C++, so I'm having some trouble figuring it out on my own. And I do plan to switch to 1.3, just as soon as the IT department has time to install it! Greg Z. |
|
June 7, 2006, 15:24 |
Nevermind, I found a previous
|
#6 |
New Member
Greg Zink
Join Date: Mar 2009
Location: Ames, Iowa, USA
Posts: 16
Rep Power: 17 |
Nevermind, I found a previous post about how to add the new library...
Greg Z. |
|
December 28, 2006, 14:24 |
Hello all,
In order to use
|
#7 |
Member
David Hebert
Join Date: Mar 2009
Posts: 31
Rep Power: 17 |
Hello all,
In order to use pressureInletVelocity, a value must be specified. Since velocity is supposed to be computed from flux, I'm not sure what the specified value for. Flow reversal? Could someone please explain? Thanks, David |
|
December 29, 2006, 06:38 |
The initial value entry is a p
|
#8 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
The initial value entry is a placeholder and will be filled with the value calculated from continuity once the simulation starts.
Typically you can simply specify: value uniform (0 0 0); Examine the updateCoeffs() function in src/finiteVolume/lnInclude/pressureInletVelocityFvPatchVectorField.C for details on how the boundary works. (This is true of most boundary conditions) |
|
December 29, 2006, 07:10 |
The initial value entry is a p
|
#9 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
The initial value entry is a placeholder and will be filled with the value calculated from continuity once the simulation starts.
Typically you can simply specify: value uniform (0 0 0); Examine the updateCoeffs() function in src/finiteVolume/lnInclude/pressureInletVelocityFvPatchVectorField.C for details on how the boundary works. (This is true of most boundary conditions) |
|
December 29, 2006, 07:54 |
Eugene,
Thanks for your exp
|
#10 |
Member
David Hebert
Join Date: Mar 2009
Posts: 31
Rep Power: 17 |
Eugene,
Thanks for your explanation, and thanks for pointing out where the boundary conditions are in the code. That will help for future endeavors. David |
|
December 28, 2011, 20:36 |
A conclusion
|
#11 |
Member
Amin Shariat KHah
Join Date: Apr 2011
Location: Shiraz
Posts: 86
Rep Power: 15 |
I need some one only tell me is it right my conclusion about pressure boundary condition or not:
if we have a pressure driven flow and we don't know about velocity but we know pressure condition we use velocity (U/0) in this form: inlet : type pressureInletVelocity value uniform(0 0 0 ) ; outlet: type zerogradient and pressure as below: inlet: type fixedValue; value uniform 1; (we assume 1 is value of pressure at inlet) outlet type fixedValue; value uniform 0; And another queation, is this pressure value real or divided by density? |
|
January 14, 2012, 09:25 |
|
#12 |
New Member
Bryan Lewis
Join Date: Jul 2010
Posts: 5
Rep Power: 15 |
The meaning of the pressure value is dependent on how the governing equations were written for the solver.
For the basic incompressible solvers (icoFoam, pisoFoam, simpleFoam, ...) the density is never specified, only nu=viscosity/density. Therefore, p is actually pressure/density. For solvers that can handle density changes (boussinesqSimpleFoam, ...), or fully incompressible solvers, this will not be the case. You have to look at the code to make sure you understand what things mean. You can get to all the code for the solvers by cd $FOAM_SOLVERS -Bryan |
|
July 28, 2016, 06:10 |
|
#13 |
Member
annn
Join Date: Jun 2016
Posts: 40
Rep Power: 9 |
did this work?
|
|
October 6, 2016, 10:42 |
Pressure BC Problems with my hot mixing case
|
#14 |
New Member
Martin Denison
Join Date: Oct 2016
Posts: 1
Rep Power: 0 |
I am trying to run a case involving the mixing of two streams, one hot with two inlet BCs. One is cold with a pressure specified. I am using reactingFoam with the reactions file
species ( O2 H2O CH4 CO2 N2 ); reactions { } notice that there are no reactions. For my inlet BC's I am using for the cold BC with the pressure specified U: type pressureInletVelocity; value uniform (0 0 0); p: type fixedValue; value uniform 94016.6; on the PIMPLE: iteration 1 I eventually get Foam::error:rintStack(Foam::Ostream&) at ??:? along with a call stack to Foam::EulerImplicit<Foam::chemistryModel<Foam:si ChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Fo am::janafThermo::Foam:erfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::solve(Foam::UniformField<double> ... When I run with a specified massflow at this BC, it runs ok. Do I have to manually iterate of the BC flowrate to get my desired pressure? How can I make the pressure BC more stable? |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
velocity inlet vs pressure inlet | cheong | FLUENT | 6 | April 9, 2011 03:07 |
subsonic inlet or supersonic inlet? | mali | CFX | 0 | November 28, 2008 20:57 |
reversed flow at velocity inlet / mass flow inlet | ib | FLUENT | 1 | March 26, 2007 13:11 |
How to set smoke inlet speed on inlet | Adam | FLUENT | 0 | October 4, 2005 08:18 |
Inlet | Christian Cordeiro | CFX | 3 | May 26, 2003 07:47 |