|
[Sponsors] |
October 16, 2010, 11:53 |
Change of B.C after solving !!!
|
#1 |
Senior Member
|
Dear Foamers,
i used buoyantBousiesqPimpleFoam to simulate a room ventilation. i defined B.C of inlet as temperature fixedValue 290K as seen below. Code:
boundaryField { wall { type zeroGradient; } inlet { type fixedValue; value uniform 290; } windows { type fixedValue; value uniform 305; } door { type fixedValue; value uniform 300; } } why is boundary fixed value changed? |
|
October 16, 2010, 13:08 |
|
#2 |
Senior Member
David Gaden
Join Date: Apr 2009
Location: Winnipeg, Canada
Posts: 437
Rep Power: 21 |
It shouldn't do that. Did you change the right files? OpenFOAM only reads the [case]/0 files when starting from time = 0. If you are resuming a run with existing data, it will read from whatever time value it needs. You'd have to change those ones.
|
|
October 16, 2010, 14:10 |
|
#3 |
Member
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 17 |
Hello maysam,
Your settings for a ventilation case look strange for me. Why don't you have an outlet boundary condition? I presumed that you expect the flow coming from the window and outgoing by the door (or the opposite). At the outlet I will preferably use an InletOutlet boundary condition. Frederic |
|
October 16, 2010, 22:05 |
|
#4 |
Senior Member
|
Thanks David and Fredric for your replies,
that was 0/T of my case. U is: Code:
dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { wall { type fixedValue; value uniform (0 0 0); } inlet { type fixedValue; value uniform (0 0 -0.1); } windows { type fixedValue; value uniform (0 0 0); } door { type inletOutlet; inletValue uniform (0 0 0); value uniform (0 0 0); } } and P is: Code:
dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { wall { type zeroGradient; } inlet { type zeroGradient; } windows { value uniform 0; type zeroGradient; } door { type fixedValue; value uniform 0; } } |
|
October 19, 2010, 10:59 |
Setting boundary condition
|
#5 |
Member
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 17 |
Hello Maysam,
Could you tell me which version of OpenFOAM you are using? For the boundary conditions, I would switch the door velocity and temperature condition to zeroGradient. I presumed you are not expecting the flow coming in from there. One important thing: For the pressure, you will have to use the "buoyantPressure" condition and not zeroGradient (have a look to the tutorial cases). Hope that those small hints will help you. Regards, Frederic |
|
October 19, 2010, 15:30 |
|
#6 | |
Senior Member
|
Quote:
The problem is setting ceiling fan inlet temperature cooler than walls and internal temperature, velocity arises to ceiling which remove the velocity of fan and contour of velocity shows a worse flow to top instead of down and it is not true in real. I think HeatTransfer solvers of OpenFOAM are not suitable for simulation of a room with having flow input and output because all of tutorials have no inlet or outlet patches. Any suggestion for ventilation simulation of a room? |
||
October 22, 2010, 09:12 |
|
#7 | |
Member
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 17 |
Quote:
I don't see why it shouldn't work. If I understand you right, you don't really know in advance, what the structure of the flow will be. So I presumed you have to change your boundary condition. I would try : for the "pressure" (p_rgh) along the walls "buoyantPressure" and fixedValue at the opening (need to take into account the gravity) and for the velocity put at the opening pressureInletOutletVelocity. I will also try first buoyantBoussinecqSimpleFoam to have a steady state solution to have a better idea of the mean flow. Good try, Frederic |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Moving mesh | Niklas Wikstrom (Wikstrom) | OpenFOAM Running, Solving & CFD | 122 | June 15, 2014 06:20 |
Differences between serial and parallel runs | carsten | OpenFOAM Bugs | 11 | September 12, 2008 11:16 |
Unknown error | sivakumar | OpenFOAM Pre-Processing | 9 | September 9, 2008 12:53 |
IcoFoam parallel woes | msrinath80 | OpenFOAM Running, Solving & CFD | 9 | July 22, 2007 02:58 |
Could anybody help me see this error and give help | liugx212 | OpenFOAM Running, Solving & CFD | 3 | January 4, 2006 18:07 |