|
[Sponsors] |
How to manually add Boussinesq Approximation to the momentum equation of a solver? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 17, 2020, 17:58 |
How to manually add Boussinesq Approximation to the momentum equation of a solver?
|
#1 |
New Member
Rosivaldo
Join Date: Nov 2019
Location: Brazil
Posts: 6
Rep Power: 7 |
Hello everyone,
Since there are no predefined solvers with those charcteristics, I'm trying to construct one wich uses VOF (it's a 2 liquid phases problem), solves for temperature and also considers buoyancy through the Boussinesq approximation (wich causes less processing effort than considering a compressible flow). For that I decided to modify the interFoam solver, having already added (to a copy of it) the energy equation by following some tutorials and threads in this forum. My problem now is with the Boussinesq aproximation. For those who don't know it, the approximation basically uses one constant property of the liquid (Beta), gravity (g) the temperature (T) and one reference temperature (T0), as follows: [...other terms of momentum equation] + (1 - Beta*(T - T0))*g So if I'm correct I'll have to add that to the momentum equation, at UEqn.H. The problem is I don't know how to do that, mainly how to to define Beta to use it in that file and the notation to write that in the momentum equation. Does anyone know where I could find information that would help me comprehend that? Until now, I have not found anything that suited... Thanks in advance for any help. Rosivaldo. Last edited by chymalaia; November 17, 2020 at 21:02. |
|
January 23, 2021, 06:37 |
|
#2 |
New Member
Join Date: Jan 2021
Posts: 10
Rep Power: 5 |
Hello Rosivaldo,
if you need beta as a constant, you can simply define it in your UEqn.H file. It might be not the best way to do that, since you will have to change the value in your source code and recompile, if you want to use a new fluid, but it works. It is also possible to interpolate beta from a table, dependent on the temperature. Fabian |
|
February 5, 2021, 10:07 |
|
#3 |
Member
Andrea Di Ronco
Join Date: Nov 2016
Location: Milano, Italy
Posts: 57
Rep Power: 10 |
Hi,
assuming you are talking about the Foundation OpenFOAM versions, Boussinesq-based solvers where removed starting from version 7. However you can still use version 6, or at least browse the source code. Look for the buoyantBoussinesqPimpleFoam solver. From UEqn.H Code:
if (pimple.momentumPredictor()) { solve ( UEqn == fvc::reconstruct ( ( - ghf*fvc::snGrad(rhok) - fvc::snGrad(p_rgh) )*mesh.magSf() ) ); fvOptions.correct(U); } Code:
rhok = 1.0 - beta*(T - TRef); I'm not familiar with VOF solvers, but this should be a good starting point. To understand the implementation, I suggest this nice blog entry: https://caefn.com/openfoam/solvers-b...nesqpimplefoam Hope it helps! Andrea |
|
Tags |
boussinesq approximation, boussinesq assumption, buoyancy, buoyancy driven flow, momentum equation |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
add a pressure drop term in the momentum equation | a.lone | FLUENT | 0 | July 3, 2019 07:48 |
How to add a wall momentum source to a solver | boeleman | OpenFOAM Programming & Development | 1 | February 6, 2013 20:32 |
error message | cuteapathy | CFX | 14 | March 20, 2012 07:45 |
Derivation of Momentum Equation in Integral Form | Demonwolf | Main CFD Forum | 2 | October 29, 2009 20:53 |
What is the Boussinesq Term in Momentum Equation | CFDtoy | Main CFD Forum | 0 | August 11, 2008 10:56 |