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

Outlet BC for disturbed Poiseuille flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 17, 2012, 11:52
Default Outlet BC for disturbed Poiseuille flow
  #1
Member
 
Max
Join Date: May 2011
Location: old europe
Posts: 81
Rep Power: 6
murx is on a distinguished road
Hi there,

i am simulating a 2D incompressible laminar pipe flow around an obstacle. There is a relative speed between obstacle and wall, so i applied a wall velocity. See the attached sketch for more details.

I have a problem finding a suitable outlet boundary condition. I expect the outlet velocity profile to be slightly disturbed by the obstacle, so i can't apply a parabolic velocity profile like at the inlet. An "Outlet" with pressure BC prevents flow into the solution domain, which is not suitable either because there is inflow due to the wall shear. So I choose a pressure "Opening" BC. But the resulting outlet velocity profile does not look like it makes physically sense, see attached picture. If I turn off the wall velocity and thereby switch of the backflow into the solution domain, I get the exact velocity profile that I expect.

Is there a suitable outlet BC that for this problem? Switching to openFOAM would be an acceptable option for me.
Or is the only way to solve the problem placing the outlet further downstream and applying a parabolic velocity profile? And if so... is there a rule of thumb how big the distance between obstacle and outlet has to be to assume undisturbed flow?

Thanks!

murx is offline   Reply With Quote

Old   February 17, 2012, 14:03
Default
  #2
New Member
 
m9819348's Avatar
 
Ries Bouwman
Join Date: Mar 2009
Location: Graz, Austria
Posts: 28
Rep Power: 8
m9819348 is on a distinguished road
Send a message via Skype™ to m9819348
Hi,

I would move the outlet backwards by ten times the diameter of the pipe and apply a uniform pressure outlet.


At the location where you want to know the pressure (according to your sketch), the parabolic velocity profile should occur.


This works in any code, open source or proprietary.


Ries Bouwman
m9819348 is offline   Reply With Quote

Old   February 18, 2012, 07:07
Default
  #3
Member
 
Max
Join Date: May 2011
Location: old europe
Posts: 81
Rep Power: 6
murx is on a distinguished road
Thanks for the quick reply, Ries!

A uniform pressure "outlet" is not possible as this prevents backflow into the domain, which is present due to the wall velocity. A pressure "opening" with inlet Flow velocity set as "normal to boundary" is what I applied. The green/blue arrows show the awkward calculated velocity profile at the outlet. Do you think moving the opnenig further downstream will fix this?
murx is offline   Reply With Quote

Old   February 18, 2012, 07:24
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,582
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Boundary conditions which have both forward and backward flow on the one boundary are always going to be difficult to get right. So I agree with Ries, you have to move this further away from your region of interest so the error in the boundary can be fixed up by the time it propogates to your region of interest.
ghorrocks is offline   Reply With Quote

Old   February 19, 2012, 14:21
Default
  #5
New Member
 
m9819348's Avatar
 
Ries Bouwman
Join Date: Mar 2009
Location: Graz, Austria
Posts: 28
Rep Power: 8
m9819348 is on a distinguished road
Send a message via Skype™ to m9819348
If you think it is not physical to elongate the outlet, there might be other options.

I am not sure what code you are using? (I did not see it in your email and also missed in what forum we are here...).

OpenFOAM: there is an outlet boundary condition called inletOutlet which allows the behaviour you are describing.

To my knowledge, FLUENT allows for something similar.
Hence I assume other widely used codes (STAR, ...) have similar options.

Summary:
- the easy way is elongating the geometry to prevent any numerical difficulties at the outlet to occur.
- the hard way is to use more sophisticated outlet boundary conditions, with the risk they might diverge more easily...

Don't forget: if what you are trying to simulate (or expect from the simulation) is not physical, your code (no matter which) will blow up most likely! :-)

Good luck!
__________________
Dr. Ries Bouwman
Business Development
ESI Group

004369917171525
@riesbouwman
m9819348 is offline   Reply With Quote

Old   February 19, 2012, 17:31
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,582
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Just to clarify Ries's reply - CFX does have a combined inflow/outflow boundary, it is called an opening. However, they are numerically less stable than the simpler single flow direction boundary (no matter what CFD code you are using) so that is why the simplest thing to try first is moving the outlet boundary down stream.
ghorrocks is offline   Reply With Quote

Old   February 20, 2012, 10:57
Default
  #7
Member
 
Max
Join Date: May 2011
Location: old europe
Posts: 81
Rep Power: 6
murx is on a distinguished road
I extended the domain so the distance between obstacle and outlet is now 6 times the channel diameter, which is more than the hydrodynamic entrance length according to the formula L = 0.03 * Re (=180) * D = 5.4 D.

Unfortunately, the velocity profile at the opening on the right still looks the same.
murx is offline   Reply With Quote

Old   February 20, 2012, 17:52
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,582
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You have missed our point. Moving the boundary downstream will not make the flow correct at the boundary. What it will do is allow enough room for the correct flow to establish between the boundary and your region of interest so the region of interest is correct.
ghorrocks is offline   Reply With Quote

Old   February 21, 2012, 03:39
Default
  #9
Member
 
Max
Join Date: May 2011
Location: old europe
Posts: 81
Rep Power: 6
murx is on a distinguished road
Ok, now i've got it
I thought that the lower extend of velocity perpendicular to the pipe axis further downstream would make the "normal to boundary" option in the opening settings more adequate and thereby help CFX to find a reasonable solution.

Since you said that this is a general numerical problem and not specifically a CFX-problem, I guess the next step for me will be to totally dismiss the pressure boundary condition and instead apply the same velocity profile as I did at the inlet. Though I know that in there is no ideal parabolic profile, it is still closer to reality than what I get with the pressure BC.

Thanks Ries and Glenn
murx is offline   Reply With Quote

Old   February 21, 2012, 17:12
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,582
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
No, you cannot apply a velocity boundary at the inlet and outlet for a steady state simulation. This is not well-posed. Read the documentation about setting up boundary conditions. You will probably need a velocity and a pressure boundary, but which is inlet and outlet does not matter.
ghorrocks is offline   Reply With Quote

Old   February 22, 2012, 14:55
Default
  #11
New Member
 
m9819348's Avatar
 
Ries Bouwman
Join Date: Mar 2009
Location: Graz, Austria
Posts: 28
Rep Power: 8
m9819348 is on a distinguished road
Send a message via Skype™ to m9819348
Hi,

I agree with Glenn.

The easiest solution in my opinion would be:
- original geometry
- inlet velocity profile as needed
- outlet elongated by roughly 10x the diameter
- give new outlet (at 10xdiameter original location) pressure outlet condition
- get your post-rpocessing data at original outlet condition and you will see the backflow (or whatever phenomena you want to see).

I am not available this week, but feel free to call me anytime next week.

Ries
__________________
Dr. Ries Bouwman
Business Development
ESI Group

004369917171525
@riesbouwman
m9819348 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
Pressure outlet in two-phase flow in horizontal 2D channel AlmostSurelyRob Main CFD Forum 0 November 17, 2010 08:32
pressure outlet (open channel flow) Willem Brantegem Main CFD Forum 0 April 3, 2007 09:39
Outlet BC for subsonic flow in pipe andrea panizza FLUENT 6 May 10, 2003 07:44
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
Mass Flow Outlet Glenn Price FLUENT 4 May 30, 2000 14:02


All times are GMT -4. The time now is 16:19.