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

Poiseuille flow with pressure inlet problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 8, 2011, 16:40
Default Poiseuille flow with pressure inlet problems
  #1
New Member
 
Jun Yang
Join Date: Mar 2011
Posts: 1
Rep Power: 0
yangjun8285 is on a distinguished road
Dear all,

Has anyone ever simulated Poiseuille flow with pressure inlet and pressure outlet, as well as body force. I am trying to simulate the body force driven poiseuille flow with 0Pa at inlet and outlet. But the result is much smaller than analytical solution. Also, I tried to set up pressure at inlet equivanlent to the body force case, which means P=rho*bodyforce*length. The result is still smaller than analytical solution.
Have anybody met this problem before? Could you share your experience with me? I have been persecuted in this problem for a long time. Really appreciate!

Jun
yangjun8285 is offline   Reply With Quote

Old   August 14, 2012, 11:13
Default
  #2
New Member
 
Jakub Pola
Join Date: Feb 2011
Posts: 17
Rep Power: 6
stainboy is on a distinguished road
Hello,

I was simulating this problem and I have similar problems like you.
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 following mesh prepared in enGrid from STL


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
stainboy is offline   Reply With Quote

Old   August 15, 2012, 02:57
Default
  #3
Member
 
Daniel Tanner
Join Date: Apr 2009
Posts: 54
Rep Power: 8
Daniel Tanner is on a distinguished road
Your answer is pretty close so likely to be solver/mesh related.
What was the order of the schemes you have used, third order MUSCL etc?

Also your mesh is not ideal. Firstly to get the best result (which still will not be exact) you should be using hex elements. In any case I would suggest that the pentahedral boundary layer to tet core element transition is not ideal. The tet elements adjacent to the pentahedral elements are slightly skew.

How far are you pushing the residuals. Your convergence monitors should have as low a threshold as possible to get the most accuracy.

You are applying a pressure boundary condition but is this as a periodic condition or only as a pressure condition. If it is the latter then there will be a significant length of pipe needed to ensure the flow was sufficient length to become fully developed.

At the end of the day how close do you need it to be? The velocity along the centerline is within 6% which is pretty reasonable for most modelling applications.

Just some thoughts.
Daniel Tanner 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
reversed flow at pressure inlet and turbulent viscosity is limited.... cfdiscool FLUENT 10 June 10, 2015 06:15
Non-steady flow simplified for use in Vissim steamerandy Main CFD Forum 0 October 31, 2011 22:08
Domain Reference Pressure and mass flow inlet boundary AdidaKK CFX 12 February 11, 2010 21:28
flow simulation across a small fan jane luo Main CFD Forum 15 April 12, 2004 17:49
mass flow + pressure inlet??? whai FLUENT 2 June 24, 2003 13:42


All times are GMT -4. The time now is 23:07.