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

buoyantBoussinesqPimpleFoam zero velocity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 27, 2012, 10:50
Default buoyantBoussinesqPimpleFoam zero velocity
  #1
Member
 
Join Date: May 2012
Location: Dresden, Germany
Posts: 32
Rep Power: 5
dl6tud is on a distinguished road
For making a new solver it is important to see, that without any force or pressure, the velocity is 0.
I tried that with the hotRoom example of buoyantBoussinesqPimpleFoam. I just changed the temperatur-field to be constant in the whole area and got the result shown in the picture.

It seems, that there is some velocity around the pressure reference cell. Has someone an explanation? I tried pRefCell and pRefPoint and got the same strange U-field.

fvsolution:
Quote:
pRefCell 0;
pRefValue 0;
T:
Quote:
internalField uniform 300;

boundaryField
{
floor
{
type zeroGradient;
}
ceiling
{
type zeroGradient;
}
fixedWalls
{
type zeroGradient;
}
}
p_rgh:
Quote:
internalField uniform 0;

boundaryField
{
floor
{
type buoyantPressure;
rho rhok;
value uniform 0;
}

ceiling
{
type buoyantPressure;
rho rhok;
value uniform 0;
}

fixedWalls
{
type buoyantPressure;
rho rhok;
value uniform 0;
}
}
Attached Images
File Type: jpg U.jpg (17.6 KB, 27 views)
dl6tud is offline   Reply With Quote

Old   September 4, 2012, 04:37
Default
  #2
Member
 
Join Date: May 2012
Location: Dresden, Germany
Posts: 32
Rep Power: 5
dl6tud is on a distinguished road
I found the reason, but do not know the solution yet. Can anyone help?

The pressure reference may be definded as
Quote:
pRefCell 0;
or
pRefPoint (0 0 0);
IMPORTANT: It seems that OF does not take the 'true' coordinate (0,0,0) but looks to which cell it belongs. (So if cell height = 1, it takes (0,0,0.5) as coordinate.)
In buoyantBoussinesqPimpleFoam, it seems, that p_rgh is interpolated to the cell face. If my first cell is 1m high and I use it as reference cell, than OF calculates p_rgh = pRefValue + (1/2) * g. The 0.5 is the distance between cell center and cell surface.
If I use a cell in the second layer as reference cell p_rgh= pRefValue + (1+(1/2))*h_cell *g.

What I want to say: as implemented now, p_rgh is not the pure dynamic pressure, but depends on where the pressure reference is. In my eyes it should be better to set p_rgh = 0 and use it as dynamic pressure. But how to do that?

This issue is a problem, because many people will not know about that. As it is now, p_rgh must allways be initialized with the correct values. Otherwise, the correct pressure will be calculated in the first time step. And that induces a movement of the liquid which is not correct at all. The hotRoom example of buoyantBoussinesqPimpleFoam is therefore slightly wrong!

Last edited by dl6tud; September 18, 2012 at 07:14.
dl6tud is offline   Reply With Quote

Old   September 13, 2012, 04:10
Default
  #3
Member
 
Join Date: May 2012
Location: Dresden, Germany
Posts: 32
Rep Power: 5
dl6tud is on a distinguished road
Update:

There are two problems:

(1) p_rgh contains a part of the hydrostatic pressure, depending on the pRefCell

(2) the laplace(T=const.) is not zero, described here: Laplace, Grad, snGrad of T

Problem 1 can be solved by initializing p_rgh with the correct values, or by correcting the code as follows:

Quote:
Originally Posted by pEqn.H
if (p_rgh.needReference())
{
/* p += dimensionedScalar
(
"p",
p.dimensions(),
pRefValue - getRefCellValue(p, pRefCell)
); */

p_rgh = p - rhok*gh;
}
Quote:
Originally Posted by createFields.H
if (p_rgh.needReference())
{
/* p += dimensionedScalar
(
"p",
p.dimensions(),
pRefValue - getRefCellValue(p, pRefCell)
);
*/

(
"p",
p.dimensions(),
pRefValue - getRefCellValue(p, pRefCell)
);

}

Last edited by dl6tud; September 18, 2012 at 07:21.
dl6tud 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
Plotting Radial Velocity and Tangential Velocity in CFD Post ashtonJ CFX 2 April 24, 2012 04:30
Velocity in Porous medium : HELP! HELP! HELP! Kali Sanjay Phoenics 0 November 6, 2006 07:10
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13


All times are GMT -4. The time now is 02:38.