|
[Sponsors] |
September 9, 2010, 01:02 |
InterMixingFoam - Gravity Currents (bug?)
|
#1 |
New Member
Martin Sabarots Gerbec
Join Date: Feb 2010
Location: Argentina
Posts: 3
Rep Power: 16 |
Hi
I've already posted in the "OpenFOAM Running / Solving / CFD" section about this issue, but I'm starting to think that may be there is a bug in the interMixingFoam. I tried to test the interMixingFoam solver when studing gravity currents. So I took the tutorial example but changing the initial alpha fields. The initial condition is a horizontal free surface, and two separated phases, with different densities (I attach the whole example). I expected to see the gravity currents due the difference in density, but both liquid phases behave as they have the same properties. What could it be wrong? Thanks! Martin
__________________
|
|
September 9, 2010, 04:12 |
|
#2 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
We've finally got a proper bug reporting system :-)
Please report any OpenFOAM bugs on http://www.openfoam.com/bugs. |
|
September 28, 2010, 12:02 |
InterMixingFoam - Gravity Currents Bug-fix
|
#3 |
New Member
Nicolás Badano
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Dear Martin,
There's indeed a bug in interMixingFoam. The solvers incorrectly assigns the properties of phase 2 to phase 3, so both are identical, preventing the development of any density current. I found the bug in threePhaseMixture.C, located under /opt/openfoam171/applications/solvers/multiphase/inaMixingFoam/incompressibleThreePhaseMixture/ In lines 79 to 88 you should replace this piece of the constructor code: Code:
nuModel3_ ( viscosityModel::New ( "nu3", subDict(phase2Name_), U, phi ) ), Code:
nuModel3_ ( viscosityModel::New ( "nu3", subDict(phase3Name_), U, phi ) ), I was able to run your test case without any problem after this modification. It works beautyfully. I've uploaded a couple of pics of the resulting alpha3. Hope this helps. Best regards! Nicolas |
|
November 11, 2010, 12:21 |
Bug fixed!
|
#4 |
New Member
Nicolás Badano
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Although we never actually reported the bug officially, it seems to be corrected in the last 1.7.x version of OpenFOAM!
Nicolas |
|
April 1, 2011, 10:01 |
|
#5 |
New Member
Sarah Köhler
Join Date: Jun 2010
Location: Leoben
Posts: 11
Rep Power: 15 |
Hey guys,
i know my probelm doesnt fit that well in this Thread, but as you used interMixingFoam already i thought you might be able to help me i have a huge vessel with a tap (an electrical arc furnace). So, inside i have steel, slag and air. And i wanna simulate at wich level the slag flows into the tap. and I dont want steel and slag to mix (D=0, am i right??). my bc´s: phase 2 and 3 are slag and steel. the field has a really small velocity in -y g (0 -9,81 0) at beginning. what happens is, that Foam stops after the first time step (0,005) and i have a velocity from 600 m/s at the Outlet. Any Ideas? Thanks in advance Sarah |
|
April 1, 2011, 10:51 |
|
#6 |
New Member
Nicolás Badano
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Hey Sarah,
I don't really know much about metallurgy but; do slag and steel behave as separate phases (with sharp interface maintained by surface tension)?? If that's the case I think you should use multiphaseInterFoam instead of interMixingFoam. multiphaseInterFoam solves for n inmiscible phases. Maybe D=0 is not very interMixingFoam friendly! On the other hand, 600 m/s in 0.005 secs sounds like an inconsistency in BCs or a mesh problem (any bad elements according to checkMesh?). Can't really pinpoint anything more concrete without having a look at the actual case directory. Hope this helps! Best regards Nico |
|
April 4, 2011, 02:59 |
|
#7 |
New Member
Sarah Köhler
Join Date: Jun 2010
Location: Leoben
Posts: 11
Rep Power: 15 |
HEy Nico,
thanks i´ll give multiphaseInterFoam a try the Mesh is ok (i did the calculation in fluent before), but i think it really has a problem with the D=0, and how you use the phases. I changed steel against air (just to try it) and it worked much better (solution was senseless, anyway ) do you if there is still a bug in gravity? When i checked my Solutions i had air blowing through the tap in the steel, without patching any velocity ... Greetings, Sarah |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
InterMixingFoam - Gravity Currents (not working) | msabger | OpenFOAM Running, Solving & CFD | 1 | September 29, 2010 12:05 |
OpenFoam gravity bug? | Whyman | OpenFOAM | 7 | June 21, 2010 04:10 |
how to consider gravity in CFX | shrimp | CFX | 4 | September 8, 2008 20:41 |
Help: gravity in CFX | Dejun Jing | CFX | 2 | July 22, 2002 08:58 |
On gravity modelling... | Drona | CFX | 7 | November 22, 2001 10:28 |