|
[Sponsors] |
November 21, 2012, 05:37 |
Outlet/opening boundary condition
|
#1 |
New Member
Ed Musgrove
Join Date: Nov 2012
Posts: 2
Rep Power: 0 |
Hi
I am currently trying to model 2D free surface flow through a sump. I am having issues with my outlet boundary as I want to set it so there is no defined pressure or velocity. If I do set a pressure condition then fluid wants to flow back into the system due to the head loss through the sump. If I resolve this using an open boundary it is not realistic. I have looked at the 2d flow over bump tutorial but that sets a down stream water level which I don't want to do. Is there any outlet boundary condition or expression I can use which does not need to have a pressure or velocity set? Thank you |
|
November 21, 2012, 09:04 |
|
#2 |
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 277
Rep Power: 21 |
You can set the pressure level as an explicit result of the water level calculated by the solver. For a 2D case with a rectangular outlet boundary condition and gravity in +Y, this might do it:
Code:
LIBRARY: CEL: EXPRESSIONS: DenRef = 1.185 [kg m^-3] DenWater = 997 [kg m^-3] DenH = (DenWater - DenRef) areaWater = areaInt(Water.Volume Fraction)@outflow bottomYposition = 0 [m] domainWidth = 0.01 [m] aveWaterHeight = bottomYposition + areaWater / domainWidth HidPressure = DenH * g * (aveWaterHeight - y) * step( (aveWaterHeight - y)/1[m] ) END END END Cheers |
|
November 22, 2012, 09:51 |
|
#3 |
New Member
Ed Musgrove
Join Date: Nov 2012
Posts: 2
Rep Power: 0 |
Thanks that has worked for me. I have also run the test with a long channel downstream of the sump. Both methods give roughly the same results.
Thanks again Ed |
|
Tags |
boundary condition, outlet boundary, outlet boundary condition |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Domain Imbalance | HMR | CFX | 5 | October 10, 2016 05:57 |
Radiation interface | hinca | CFX | 15 | January 26, 2014 17:11 |
An error has occurred in cfx5solve: | volo87 | CFX | 5 | June 14, 2013 17:44 |
Setting outlet Pressure boundary condition using CAFFA code | Mukund Pondkule | Main CFD Forum | 0 | March 16, 2011 03:23 |
How to set boundary condition in Fluent for the fo | Peiyong | FLUENT | 1 | November 10, 2006 11:44 |