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

irregular pressure field simpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 5, 2011, 04:42
Default irregular pressure field simpleFoam
  #1
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 6
k_xyz is on a distinguished road
Dear all,

I'm having some trouble with a simpleFoam computation around a solid body, with wall function boundary conditions at the wall: the pressure field is disturbed near the surface (jagged pressure distribution on the surface, and deformed iso-pressure lines, as shown in the attachment.)

The setup (fvSchemes, fvSolution, boundary conditions) follows pretty much the airFoil2D case (linearUpwind div-schemes), Re is around 500.000.

The case converges, but the pressure distribution is not correct. From the iso-pressure lines one might think it's a mesh problem - however, yPlus is between 30 and 130, and the mesh is as regular as possible... Doesn't seem to be the wall function either - the problem persists with different models.

Any suggestions where the problem could come from?
Attached Images
File Type: jpg pressure.jpg (12.1 KB, 45 views)
File Type: jpg iso_pressure.jpg (55.8 KB, 41 views)
k_xyz is offline   Reply With Quote

Old   September 6, 2011, 04:28
Default
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
What does your velocity field look like?

Also try leastSquares or extendedLeastSquares for the pressure gradient and snGrad.
eugene is offline   Reply With Quote

Old   September 6, 2011, 09:52
Default
  #3
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 6
k_xyz is on a distinguished road
Hi and thanks for your answer,

I've tried leastSquares as gradScheme and corrected as snGradScheme, however, the problem persists.
It's also visible in the velocity field as you'll see in the attachment (velocity is zero at the wall itself, the picture shows the internal mesh, cell values). Again, the overall distribution looks ok, but there's this jagged distribution in the first cell layer.

Could the problem be related to the mesh, e.g. caused by the intersection between the prism layers and the outer mesh?
Attached Images
File Type: jpg Screenshot.jpg (37.5 KB, 25 views)
k_xyz is offline   Reply With Quote

Old   September 6, 2011, 10:08
Default
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
snGradCorr gradient, not snGrad, like this:

gradSchemes
{
grad(p) leastSquares;
snGradCorr(p) leastSquares;
}

I doubt it will help, but you should also try extendLeastSquares.

The problem is almost certainly due to the irregular mesh, but that's hardly an excuse for the poor results. You should also try limiting the LUD gradient and the nonOrthogonal correction:

divSchemes
{
div(phi,U) Gauss cellMDLimited linearUpwindV Gauss linear 0.5;
}

laplacianSchemes
{
default Gauss linear limited 0.333;
}
snGradSchemes
{
default limited 0.333;
}
eugene is offline   Reply With Quote

Old   September 6, 2011, 12:33
Default
  #5
New Member
 
Join Date: Jun 2011
Posts: 3
Rep Power: 6
k_xyz is on a distinguished road
Hi,

still not looking better... I've tried out a couple of different snappy-meshes, but I don't see a way of getting something more regular there...

I've attached my fvSchemes and fvSolutions files - maybe there's an error I have overlooked.

Boundary conditions are: for velocity fixedValue inlet, InletOutlet at outlet, fixedValue 0 at the wall, for pressure zeroGrad everywhere except at the outlet, there it's fixedValue 0.

I've had a look at some of the tutorials and noticed a similar effect in the 'wingMotion' test case (also with a snappy mesh), whereas the airFoil2D case (Icem-mesh?) looks smoother...
Attached Files
File Type: txt fvSchemes.txt (1.7 KB, 37 views)
File Type: txt fvSolution.txt (2.0 KB, 12 views)
k_xyz is offline   Reply With Quote

Old   September 7, 2011, 08:16
Default
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Change your relTol on p solver from 0.1 to 0.001.

SIMPLE - set nOrthogonalCorrectors to 0

interpolation scheme should not be limited, just linear is fine.

snGradSchemes should be identical to Laplacian, i.e. limted 0.333

If none of the above works, try increasing the macthing height in snappy and adding more layers.
eugene 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
Pulsatile pressure inlet with pressure outlet a.lynchy FLUENT 3 March 23, 2012 14:45
pressure in incompressible solvers e.g. simpleFoam chrizzl OpenFOAM Running, Solving & CFD 7 August 24, 2010 11:19
custom pressure field at the faces Souviktor FLUENT 0 April 3, 2009 08:09
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51
How to get Pressure field from velocity field qunwuhe@hotmail.com Main CFD Forum 4 October 14, 2007 07:38


All times are GMT -4. The time now is 15:49.