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

A wall has been placed at portion(s) of an OUTLET

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

Like Tree4Likes
  • 3 Post By CycLone
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2008, 03:51
Default A wall has been placed at portion(s) of an OUTLET
  #1
Melvin
Guest
 
Posts: n/a
Hi

When I increase the timestep, I get the above notice after about 50 iterations and this continues until the case converges (1E-4). Will this affect the solution?

If I use the auto timescale, I dont get this notice but the simulation doesn't converged.

My model is described in http://www.cfd-online.com/Forum/cfx.cgi?read=24122
  Reply With Quote

Old   January 18, 2008, 04:25
Default Re: A wall has been placed at portion(s) of an OUT
  #2
Subha
Guest
 
Posts: n/a
Hai Melvin,

I think along with your error message you would have got this message also.

"There are some reverse flows in areas near your outlet. Try chaning your Outlet to Opening"

Changing to Opening should solve the problem.

Regards, Subha.
  Reply With Quote

Old   January 18, 2008, 08:09
Default Re: A wall has been placed at portion(s) of an OUT
  #3
Usman
Guest
 
Posts: n/a
Why is that we receive such a message in the first place. Is it because our outlet boundary is not far enough from inlet? I have been receiving this message for my steady state problem, but when i ran LES case i didnt get this message. I am not sure what is going on!

Usman
  Reply With Quote

Old   January 18, 2008, 12:25
Default Re: A wall has been placed at portion(s) of an OUT
  #4
CycLone
Guest
 
Posts: n/a
Hi Melvin,

Look at your flow field and pay attention to the % of the outlet area that is walled off (reported in the warning). The solver does this to prevent reverse flow, which you clearly don't want if you specified an outlet (otherwise you would have defined an opening, right?).

If the % area is small, it may not have a significant effect on your solution. If it is large, you should investigate the flow in the vicinity of the outlet. Try seeding streamlines from the outlet to see the reverse flow region, for instance.

In the end, you may have to extend your model to include more geometry downstream or change the boundary condition to more accurately represent what is occurring at this location. For instance, if you set an average static pressure but the flow dumps into a plenum beyond the outlet, a constant static pressure may be more appropriate. Similarly, if it is a mass flow specified outlet, set the pressure profile at the outlet to a constant value (which enforces a constant static pressure across your outlet which achieving the desired mass flow).

The key is to understand the physics and act accordingly.

-CycLone

  Reply With Quote

Old   January 19, 2008, 01:23
Default Re: A wall has been placed at portion(s) of an OUT
  #5
Melvin
Guest
 
Posts: n/a
Thank you for the suggestions SUbha and CycLone. I will try to lengthen my outlet and hope it resolves this problem.
  Reply With Quote

Old   July 18, 2014, 03:33
Default wall placed at Inlet (not Outlet)
  #6
New Member
 
shubham jain
Join Date: Dec 2013
Posts: 24
Rep Power: 4
shubham jain is on a distinguished road
hi, i am simulating a Brush seal using Porous medium approach in CFX.

My inlet (INLET) and outlet (OPENING) channels are very long. Cfx says that wall is placed at a portion of Inlet, then it stops the simulation.

However, when i see the streamlines, circulation was only at the outlet , not inlet.
Though the problem was solved by shortening the inlet as well as outlet channels, so that no circulation is coming at outlet. But i could not understand, why the shortening of channel length makes it (wall places at INLET) better??

Picture attached: Green region in right is inlet.... Dark yellow in the middle is the porous medium ..... light yellow in the left is outlet
FLOW DIRECTION IS FROM RIGHT TO LEFT

Thanks in advance
Attached Images
File Type: jpg geom_1.jpg (6.8 KB, 56 views)
File Type: jpg geom_1_3D.jpg (13.7 KB, 58 views)
shubham jain is offline   Reply With Quote

Old   July 24, 2014, 08:32
Default
  #7
New Member
 
Marco
Join Date: Dec 2011
Posts: 3
Rep Power: 6
marco.ian is on a distinguished road
http://www.arc.vt.edu/ansys_help/cfx_mod/i5500692.html

Here is the explanation!
marco.ian is offline   Reply With Quote

Old   July 24, 2014, 08:36
Default
  #8
New Member
 
shubham jain
Join Date: Dec 2013
Posts: 24
Rep Power: 4
shubham jain is on a distinguished road
thanks for the link... But that does not answer why the shortening of the channel length makes the wall placed at the inlet dissappear.

Also in recent simulations, i have noticed that for some high pressure drops, 100% wall is placed at the inlet. But when I decrease the temperature form the actual working conditions, it works.
This is also a little confusing for me.
shubham jain is offline   Reply With Quote

Old   June 5, 2016, 05:29
Post
  #9
New Member
 
Ahmed
Join Date: Jul 2011
Location: Birmingham, UK
Posts: 2
Rep Power: 0
ahmedrezk82 is on a distinguished road
Hi

It is great information. I have the same problem in the first few iterations, then disappeared and the simulation continue with good conversion rate. I am simulating turbine flow, and I am confident that the outlet section is long enough, would extending the inlet section solve the problem.

Quote:
Originally Posted by CycLone
;85459
Hi Melvin,

Look at your flow field and pay attention to the % of the outlet area that is walled off (reported in the warning). The solver does this to prevent reverse flow, which you clearly don't want if you specified an outlet (otherwise you would have defined an opening, right?).

If the % area is small, it may not have a significant effect on your solution. If it is large, you should investigate the flow in the vicinity of the outlet. Try seeding streamlines from the outlet to see the reverse flow region, for instance.

In the end, you may have to extend your model to include more geometry downstream or change the boundary condition to more accurately represent what is occurring at this location. For instance, if you set an average static pressure but the flow dumps into a plenum beyond the outlet, a constant static pressure may be more appropriate. Similarly, if it is a mass flow specified outlet, set the pressure profile at the outlet to a constant value (which enforces a constant static pressure across your outlet which achieving the desired mass flow).

The key is to understand the physics and act accordingly.

-CycLone
ahmedrezk82 is offline   Reply With Quote

Old   June 5, 2016, 06:22
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If the warning disappears after a while and convergence is good then you have nothing to worry about. The simulation just needed to sort itself out a bit and proceeded to converge well from there.
ahmedrezk82 likes this.
ghorrocks is offline   Reply With Quote

Old   June 5, 2016, 12:43
Default Thanks a lot ghorrocks
  #11
New Member
 
Ahmed
Join Date: Jul 2011
Location: Birmingham, UK
Posts: 2
Rep Power: 0
ahmedrezk82 is on a distinguished road
Thanks a lot ghorrocks.
ahmedrezk82 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
Compressible flow, no data at the outlet mireis FLUENT 6 September 3, 2015 02:10
Very technical question about solving wall boundary layer ... jlb001 FLUENT 6 December 27, 2014 06:56
modelling a porous wall as outlet Swen FLUENT 3 July 10, 2011 07:42
Combining BCs: wall - outlet. Boundary layer disappears MartinaF OpenFOAM Running, Solving & CFD 1 July 20, 2009 18:14
Question about bcdefw.f for wall temperature bc. Jimmy CD-adapco 10 March 18, 2008 16:28


All times are GMT -4. The time now is 08:36.