CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Change of B.C after solving !!!

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2010, 11:53
Exclamation Change of B.C after solving !!!
  #1
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
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;
    }
}
After solving all grids have temperature of more than 300K
why is boundary fixed value changed?
maysmech is offline   Reply With Quote

Old   October 16, 2010, 13:08
Default
  #2
Senior Member
 
David Gaden
Join Date: Apr 2009
Location: Winnipeg, Canada
Posts: 397
Rep Power: 12
marupio is on a distinguished road
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.
marupio is offline   Reply With Quote

Old   October 16, 2010, 14:10
Default
  #3
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
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
fcollonv is offline   Reply With Quote

Old   October 16, 2010, 22:05
Default
  #4
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
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);
    }

}
i,ve revised door from aeroGradient ti inletOutlet.
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;
    }

}
the problem is i don't know how OF can use all of these 3 B.C with each other. you know we should define only one of P or U in other codes. Can this be the cause of problem?
maysmech is offline   Reply With Quote

Old   October 19, 2010, 10:59
Default Setting boundary condition
  #5
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
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
fcollonv is offline   Reply With Quote

Old   October 19, 2010, 15:30
Default
  #6
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Quote:
Originally Posted by fcollonv View Post
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
I use OpenFOAM 1.7.0

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?
maysmech is offline   Reply With Quote

Old   October 22, 2010, 09:12
Default
  #7
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Quote:
Originally Posted by maysmech View Post
I use OpenFOAM 1.7.0

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?
Hello Maysam,

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
fcollonv is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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 19:07


All times are GMT -4. The time now is 09:08.