|
[Sponsors] |
November 29, 2022, 01:26 |
Why is fixedFluxPressure more stable ?
|
#1 |
New Member
HR
Join Date: Nov 2022
Posts: 17
Rep Power: 3 |
I recently an few multiphase scenarios using interFoam and found that fixedFluxPressure is more stable for the simulation than zeroGradient. What might be the issue for this ?
|
|
December 2, 2022, 18:17 |
|
#2 |
Senior Member
Paulo Vatavuk
Join Date: Mar 2009
Location: Campinas, Brasil
Posts: 197
Rep Power: 17 |
Hi HR,
At the 11th OpenFOAM Workshop there was a Training Course with the title "Learning how to use free surface flows in OpenFOAM 3.0" by Victoria Korchagova. This course is the only material that I found that explains this boundary condition. Is it for OF version 3, but I think that it also applies to newer versions. You can download the course material in this page: https://openfoam-extend.sourceforge....s/courses.html |
|
December 5, 2022, 03:48 |
|
#3 | |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,104
Rep Power: 26 |
The OpenFOAM user guide also mention it, despite not giving much details:
Quote:
There are also on old thread here discussing it: I need explanations about fixedFluxPressure My personal experience with buoyantSimpleFoam is that I get a flowrate through the walls when using zeroGradient and it does not happen with fixedFluxPressure. Yann |
||
December 10, 2022, 09:09 |
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
Hi,
This is because when you’re solving for p, zero gradient isn’t the correct boundary condition. Consider additional forces, such as gravity: if you zero gradient the pressure, such terms will give you flux through a wall. Fixed flux pressure compensates for it to achieve zero flux: you get a pressure gradient on the wall to balance all other flux contributions. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Decomposing error simple method | DanGode | OpenFOAM Pre-Processing | 1 | July 27, 2021 06:58 |
fixedFluxPressure BC: updateCoeffs(const scalarField& snGradp) MUST be called ... | MCrossover97 | OpenFOAM Running, Solving & CFD | 1 | June 25, 2021 06:03 |
bugs of buoyantBoussinesqPisoFoam or fixedFluxPressure in foam-extend 3.1 and 3.2 | Aaron_L | OpenFOAM Bugs | 5 | July 30, 2016 07:11 |
fixedFluxPressure with PisoFoam | me.ouda | OpenFOAM Running, Solving & CFD | 1 | October 27, 2015 05:30 |
rhoPimpleFoam with fixedFluxPressure + flowRateInletVelocity --> p diverges | tatu | OpenFOAM Running, Solving & CFD | 1 | March 21, 2013 15:10 |