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

Fluid flow through wall U %3d 0 ignored when set pressure gradient for buoyancy

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 29, 2008, 17:40
Default Hi there, I added buoyant f
  #1
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
Hi there,

I added buoyant force (1 + alpha*T)*g to an extended icoFoam solver, g = (0 -9.81 0), then set BCs for p as pressure gradient such that eq grad(p) = g is satisfied. And what happens is - fluid goes through a boundary where BC U=(0 0 0) is set! Maybe you have an idea why?

K.
kar is offline   Reply With Quote

Old   March 1, 2008, 01:27
Default Karlis, I'm guessing you'r
  #2
Senior Member
 
Michael Jaworski
Join Date: Mar 2009
Location: Champaign, IL, USA
Posts: 126
Rep Power: 8
mike_jaworski is on a distinguished road
Karlis,
I'm guessing you're setting this BC at the bottom of the domain. Have you tried setting it to a fixedValue boundary with a value of rho*g*h where h is your fluid depth? That strikes me as a more direct approach.

Regards,
Mike J.
mike_jaworski is offline   Reply With Quote

Old   March 1, 2008, 07:33
Default the flow you are seeing is bec
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
the flow you are seeing is because of your PRESSURE boundary condition. A non-zero pressure gradient means there must be flow through the boundary because of the pressure Laplacian. You did not account for this in the pressure equation and hence you are getting non-zero flux.

Remember, boundary conditions on p and U are not independent - as I am sure you already know.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 1, 2008, 12:34
Default Harvoje, I wouldn't ask and
  #4
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
Harvoje,

I wouldn't ask and make such useless experiments if I knew about BC non-independence etc.
Decided to implement gravitational force and temperature dependent density in icoFoam.

Looking at the buoyantFoam solver I see some dynamic pressure introduced and only that is used for laplace( p ). Don't understand that stuff yet...
-> Where to read more about how to build buoyant solver for incompressible fluid? I read your thesis, Harvoje, but I would appreciate if someone point me in the right direction for buoyancy stuff..
-> When I finish that solver, I would be happy to share it. Also I haven't found a BC patch type for convective + radiation heat transfer; BC is this:

grad(T) = - surfaceNormalVector/k * ( h*(T - Treference) + sigma*epsilon(T^4 - Treference^4) )

For sake of good usage constants h, Treference, epsilon must be read from 0/T file. I already begin a thread about this, but there is no reply so far. I wasn't able to access T field defined in solver from separate *.C file which defined class temperatureOpeningFvPatchScalarField : public fixedGradientFvPatchScalarField.

Best regards,
Kārlis
kar is offline   Reply With Quote

Old   March 1, 2008, 13:25
Default Harvoje, I found in an old
  #5
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
Harvoje,

I found in an old thread ( http://www.cfd-online.com/OpenFOAM_D...ges/1/815.html ), there was boussinesqBuoyantFoam by you, but link doesn't work... Maybe you could post it in again if you consider it useful?

K.
kar is offline   Reply With Quote

Old   March 1, 2008, 23:53
Default Karlis, I do not believe t
  #6
Senior Member
 
Michael Jaworski
Join Date: Mar 2009
Location: Champaign, IL, USA
Posts: 126
Rep Power: 8
mike_jaworski is on a distinguished road
Karlis,
I do not believe the pressure gradient term is correct as a boundary condition in the way you have used it. Namely, the gradient of the pressure is necessary *within* the fluid because of momentum balance. At a physical wall, however, pressure has a specific value. If you write out the equations for a momentum balance of the wall itself, the wall-fluid force is the (pressure)*(area), and has nothing to do with the gradient.

There already is a buoyant solver in OpenFOAM if I recall correctly. What does it specify for pressures?

Regards,
Mike J.
mike_jaworski is offline   Reply With Quote

Old   March 2, 2008, 06:42
Default Michael, first about BC: ph
  #7
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
Michael,

first about BC: physically there is gradient. Is there any reason to say it cannot be implemented in OpenFOAM?
Harvoje said: "You did not account for this in the pressure equation and hence you are getting non-zero flux."
So, my problem (one of..) appears to be writing correct pressure eq!

Second - I don't like specifying pressure because it is an integral quantity. There is static pressure and dynamic, but in case when density changes and flow is present, I'm not sure if it's still that simple. So I decided to use gradient as BC!

About buoyantFoam - it is for compressible flow and tries to separate p = pd + rho*gh + pRef; But I currently cannot accept that. How to show that it solves the same N-S equation with same conditions as for full pressure p?

K.
kar 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
How can I get the pressure gradient along the direction normal to the local wall surface qtian OpenFOAM Running, Solving & CFD 3 April 4, 2014 05:05
Pressure gradient for channel flow?? cfdIsMad CFX 1 July 3, 2008 22:22
Pressure boundary & buoyancy Bouke Main CFD Forum 2 October 22, 2002 11:37
pressure gradient term in low speed flow Atit Koonsrisuk Main CFD Forum 2 January 10, 2002 11:52
Pressure boundary on buoyancy-driven flow raymond CD-adapco 1 September 20, 2001 05:25


All times are GMT -4. The time now is 08:39.