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

OpenFoam validation of 3D Poiseuille Solution

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2012, 04:59
Default OpenFoam validation of 3D Poiseuille Solution
  #1
New Member
 
Join Date: Dec 2011
Posts: 3
Rep Power: 5
alinve is on a distinguished road
Dear foamers,
I'm new user of openfoam and I'm trying to run my first case.
I need to validate OpenFoam against Poiseuille analytical solution.
I need to modelling the 3D Poiseuille flow in a pipe due to a pressure drop.
I've build a case test to be used with icoFoam and a case test to be runned with simpleFoam, disabling the turbolence model. Both solver give me the same solution, that differs from the analytical ones.
The shape of velocity along radius has a parabolic profile but velocity is not zero at the wall, as I expected from the analitycal solution. I've got no idea on how to solve the problem.
I've attached the icoFoam case test, have you got an idea about where I get wrong??
Thanks for any suggestion,
Best Regards
Alice
alinve is offline   Reply With Quote

Old   January 25, 2012, 11:36
Default
  #2
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
Your case did not upload succesfully, so we can't review your setup files. Just to be absolutely certain, is your wall velocity truly set to zero in the /0/U file? It should look something like this:

Code:
     
wall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
danishdude is offline   Reply With Quote

Old   January 27, 2012, 07:20
Default
  #3
New Member
 
Join Date: Dec 2011
Posts: 3
Rep Power: 5
alinve is on a distinguished road
Sorry it is the first timethat I use this forum.
I imposed zero velocity at the wall , as you can see in U file:



Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet      
    {
        type            fixedValue;
        value           uniform (0 0.05 0);
    }

    outlet      
    {
        type           zeroGradient;
    }

    walls    
    {
        type            fixedValue;
    value         uniform (0 0 0);
    }
}
I try to upload the .zip file another time.
Thanks
Alice
Attached Files
File Type: zip Poiseuille3D.zip (4.9 KB, 53 views)
alinve is offline   Reply With Quote

Old   August 14, 2012, 11:38
Default
  #4
New Member
 
Jakub Pola
Join Date: Feb 2011
Posts: 17
Rep Power: 6
stainboy is on a distinguished road
Hello,

I was simulating 3D Poiseuille flow and I have problem with validation.
I have a cylinder 3.5mm in diameter and 21mm long. I was forcing flow by setting pressure difference between inlet and outlet (6.5Pa).
From the calculations(mu=3.5e-3Pa/s, nu=3.3e-6m^2./s, rho = 1050kg/m^3 - like human blood) I should obtain V_max=6.7cm/s but from simulation I've got 6.3cm/s. I'm little bit frustrated now.

I'm simulating laminar incompressible flow using simpleFoam.

p
Code:
dimensions    [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
    wall
	{
		type zeroGradient;
	}
	inlet
	{
		type fixedValue;
		value uniform 6.5;
	}
    outlet
	{
		type fixedValue;
		value uniform 0;
	}
}
U
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 pressureInletVelocity;
        value uniform (0 0 0);
		
	}
	outlet
	{
		type zeroGradient;
	}
}
I have mesh prepared in enGrid from STL file (attachement)

Does anybody have some suggestions what might be wrong with my simulation?

I was thinking if maybe the lenght of the pipe is too short. How can I put the fan BC on my inlet and outlet to make this geometry infinite?

Thank you very much in advance for any suggestions
Attached Images
File Type: jpg cyl_mesh.jpg (52.5 KB, 43 views)
File Type: png u_profile.png (22.5 KB, 40 views)
stainboy is offline   Reply With Quote

Old   August 14, 2012, 15:46
Default
  #5
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
Keep in mind pressure is dynamic pressure in m^2/s^2 (which is actually P/rho). It looks like you are running the wrong Reynolds number because you have not divided your pressure by the density. Check your transportProperties file as well to make sure you have the right viscosity in there.
danishdude is offline   Reply With Quote

Old   August 15, 2012, 03:28
Default
  #6
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
Hi,

the length of the pipe is a good candidate.

The mesh could do with a few more iterations to get the boundary layer straightened out -- the outer surface of the prismatic mesh should be smooth. You might also want to try out a polyhedral mesh, because it runs faster and delivers accuracy not far from hex grids.

Cheers,
Oliver
ogloth is offline   Reply With Quote

Old   August 16, 2012, 00:09
Smile
  #7
New Member
 
Jakub Pola
Join Date: Feb 2011
Posts: 17
Rep Power: 6
stainboy is on a distinguished road
Thank you very much for suggestions. I've found my mistake. Problem was laying in the pressure. I forgot to multiply it by rho. I wanted to have pressure drop equal to 6.5 Pa, so I should put the pressure in 0/p file equal to 6.5*1050. Now the results are as they should.
stainboy 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
OpenFOAM (Linux) in a MS-HPC-Cloud fossy OpenFOAM 6 September 23, 2010 11:48
OpenFOAM crashes when input is a steady solution kar OpenFOAM Bugs 0 May 4, 2008 11:42
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25
OpenFOAM Training and Workshop Zagreb 2628Jan2006 hjasak OpenFOAM 1 February 2, 2006 22:07
Wall functions Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16


All times are GMT -4. The time now is 14:05.