# "Wall" boudary condition setting

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 April 28, 2011, 23:14 "Wall" boudary condition setting #1 New Member   Joe Join Date: Mar 2009 Posts: 26 Rep Power: 10 Hello, everyone! I got puzzled by the solution result. Here is my case: Air flows through a duct, and turns down to the reactor. In order to optimize the distribution of velocity and try to make the flow angle as vertical as possiple, a rectifier is settled at the turning(as Geometry shows:the rectifer is constitute of non-thickness plate,with the space of 80mm between each other and height of 300mm). The inlet air has a uniform velocity of 15m/s, and the rectifer was defined as wall in fluent. As the rectifer has such a short space between each plate, I imagine the flow should be almost vertical after going through the rectifer, while the solution turns out a different result(see Velocity_Magnitude and Pathline). There is a huge vortex at the turning. It's really curious, I wonder if I've wrongly set some parameters about the rectifer as Wall, or is ther any other reason? Thank you for your attention! Picture link: Geometry: http://imageupload.org/?d=4DBA293D1 Velocity_Magnitude: http://imageupload.org/?d=4DBA29E51 Pathline: http://imageupload.org/?d=4DBA29E61

 April 28, 2011, 23:18 #2 New Member   Joe Join Date: Mar 2009 Posts: 26 Rep Power: 10 As seen from the pathline,the rectifer seems has no effect to guide the flow going downstream vertically. In another word, it seems that as if there is no rectifer at all.

 May 2, 2011, 07:12 #3 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,201 Rep Power: 34 check the velocity distribution close to the rectifier. Big zoom on it. Check also vectors. You can post the picture. If you want you can also upload your dbs file on a share server, I can check your geometry (the first picture sounds like to be from gambit) __________________ In memory of my friend Hervé: CFD engineer & freerider

May 2, 2011, 22:20
Thank you for your help
#4
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- check the velocity distribution close to the rectifier. Big zoom on it. Check also vectors. You can post the picture. If you want you can also upload your dbs file on a share server, I can check your geometry (the first picture sounds like to be from gambit)
Hi, mAx, thank you for your time and kindness, I've uploaded the velocity distribution and vectors at the following links:
velocity distribution: http://imageupload.org/?d=4DBF5F541
vectors: http://imageupload.org/?d=4DBF5F551
I also want to upload the .dbs file on a share server, if you have any good suggestion about which server is OK, plz tell me. I can send the dbs file to you instead, if you would like to leave me your Email, thank you!

 May 3, 2011, 01:45 #5 New Member   qingkai Join Date: Apr 2011 Posts: 11 Rep Power: 8 So courious, did you set the roughness of Wall bc?

May 3, 2011, 01:55
wall roughness
#6
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by sailor So courious, did you set the roughness of Wall bc?
Hi, sailor, thank you for your attention. I didn't set the roughness of Wall bc. Do you think that will impact the result? I didn't get a clue how to set that parameter. However, I think the roughness of the wall can cause viscous stress, which leads to the pressure drop on the rectifier layer, but I don't think that may heavily impact the direction of vectors after going through the layer.
Thank you again!

 May 3, 2011, 07:44 #7 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,201 Rep Power: 34 can you post picture of veocity contour, but really on the rectifer. here: Sans titre.png I checked your geometry and it is ok. I already defined such interior face (split) as wall, and fluent defined it as a baffle (consistent results). So it is supposed to work... __________________ In memory of my friend Hervé: CFD engineer & freerider

May 3, 2011, 23:58
#8
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- can you post picture of veocity contour, but really on the rectifer. here: Attachment 7530 I checked your geometry and it is ok. I already defined such interior face (split) as wall, and fluent defined it as a baffle (consistent results). So it is supposed to work...
Hi mAx, you know, I've already defined these split faces which consititute the rectifier layer as wall in Gambit. And I also checked them in fluent B.C. settings, they're still represented as wall. That's exactly what I want, I want them to be defined as wall, so when air flows down through them, the flow direction could be restricted as vetical as possible. However, the result ran out of my expection.
I'm afraid I didn't catch what you said. Any way, thank you for your lasting care about my problem.
Below is the velocity contour around the rectifier layer(the grids of rectifier is turned off).
http://dl.dropbox.com/u/28013317/Velocity-contour.png

 May 4, 2011, 01:09 #9 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,201 Rep Power: 34 your plane seems to go through a baffle row... (the blue contours show the zero velocity at walls which is correct) offset this plane in z direction (for being between 2 baffle rows) and repost picture. Then generate the same picture but on a yz-section __________________ In memory of my friend Hervé: CFD engineer & freerider

May 4, 2011, 02:02
#10
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- your plane seems to go through a baffle row... (the blue contours show the zero velocity at walls which is correct) offset this plane in z direction (for being between 2 baffle rows) and repost picture. Then generate the same picture but on a yz-section
Ok, mAx, I've generated a picture both on xy-section and yz-section, and I make sure that the two sections are not at the place where the wall is. While from the picture, it seems that they are still on the wall. That's really strange, and I guess that if it is caused by the grids. Since the distance between two split faces in x-direction is 80mm, and when I generated the grids on the rectifier layer volume, I set the mesh size as 80mm, so between the two split faces in x-direction, actually there is no grid nodes at all. In other words, the grid nodes are only on the wall.

links,
velocity-contour:
http://dl.dropbox.com/u/28013317/Vel...our-update.png

grids:
http://dl.dropbox.com/u/28013317/grids.png

 May 4, 2011, 02:19 #11 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,201 Rep Power: 34 ok then try to refine your grid. Typically you need at least 8 cells in a gap. But I would expect a flow rate even if you have just one cell in a gap. On your first picture (if the planes are placed between 2 walls) it seems you don't have fluid passing through the rectifer. Check if you don't defined top and bottom surfaces as wall (display/grid select only rectifer with option faces (light on) and check that the body isn't "closed") __________________ In memory of my friend Hervé: CFD engineer & freerider

May 4, 2011, 03:39
#12
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- ok then try to refine your grid. Typically you need at least 8 cells in a gap. But I would expect a flow rate even if you have just one cell in a gap. On your first picture (if the planes are placed between 2 walls) it seems you don't have fluid passing through the rectifer. Check if you don't defined top and bottom surfaces as wall (display/grid select only rectifer with option faces (light on) and check that the body isn't "closed")
Ok, I would have a try to refine the grids, but I think that would be a challenge for my computer resources to generate the grids with a very small mesh size(espetially as you mentioned, generally 8 cells are needed between a gap).
I've checked the grids by the method you suggested. From the picture, it seems the grid is OK, and it is not a closed volume. I think if the rectifier was a closed volume(which means if I set the top face of the rectifier layer as wall by mistake) , there wouldn't be flow going downstream after the rectifier layer, however, from the calculation result, we can see flow running through the rest of the reactor.
link,
grids-rectifier:http://dl.dropbox.com/u/28013317/grids-rectifier.png

 May 4, 2011, 03:43 #13 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,201 Rep Power: 34 then check where the fluid is passing through. Check velocity contour at section xz through the rectifier __________________ In memory of my friend Hervé: CFD engineer & freerider

May 4, 2011, 03:49
#14
New Member

qingkai
Join Date: Apr 2011
Posts: 11
Rep Power: 8
Quote:
 Originally Posted by wateraction Hi, sailor, thank you for your attention. I didn't set the roughness of Wall bc. Do you think that will impact the result? I didn't get a clue how to set that parameter. However, I think the roughness of the wall can cause viscous stress, which leads to the pressure drop on the rectifier layer, but I don't think that may heavily impact the direction of vectors after going through the layer. Thank you again!
Yeah, I think you are right. It cannot be the problem of roughness. The flow is not affected by the baffles, wish you solve the problem asap.~~

May 4, 2011, 04:08
#15
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- then check where the fluid is passing through. Check velocity contour at section xz through the rectifier
I've checked the velocity contour on xz-section about half height of the rectifier layer, and you're right that the result shows the velocity is zero on the section, which means there is no fluid passing through.
I think it might be caused by the fact that all cell nodes are on the wall(split faces), where the velocity is zero, then fluent may use the method of interpolation to calculate the velocity between the two walls, therefore, anywhere between the walls has a zero velocity.
link,
velocity-contour-xz-section:
http://dl.dropbox.com/u/28013317/Vel...xz-section.png

May 4, 2011, 04:09
#16
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by sailor Yeah, I think you are right. It cannot be the problem of roughness. The flow is not affected by the baffles, wish you solve the problem asap.~~
Thank you, sailor.

May 4, 2011, 05:14
#17
Super Moderator

Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,201
Rep Power: 34
Quote:
 Originally Posted by wateraction I've checked the velocity contour on xz-section about half height of the rectifier layer, and you're right that the result shows the velocity is zero on the section, which means there is no fluid passing through. I think it might be caused by the fact that all cell nodes are on the wall(split faces), where the velocity is zero, then fluent may use the method of interpolation to calculate the velocity between the two walls, therefore, anywhere between the walls has a zero velocity. link, velocity-contour-xz-section: http://dl.dropbox.com/u/28013317/Vel...xz-section.png
Then refine
And since your geometry is symmetric, compute just on half of your domain (I assume your BC's enable you to use one symmetry plane)
__________________
In memory of my friend Hervé: CFD engineer & freerider

May 5, 2011, 06:10
#18
New Member

Joe
Join Date: Mar 2009
Posts: 26
Rep Power: 10
Quote:
 Originally Posted by -mAx- Then refine And since your geometry is symmetric, compute just on half of your domain (I assume your BC's enable you to use one symmetry plane)
Thank you for your advice, mAx, I will have a try at a later time, cos another task is in emergency.

 Tags rectifer

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post NLao FLUENT 1 April 17, 2011 05:23 CFD XUE FLUENT 0 July 8, 2010 06:49 Purushothama CD-adapco 2 May 31, 2010 21:58 Antonis CFX 1 September 11, 2006 16:53 Saad Main CFD Forum 5 November 19, 2004 14:22

All times are GMT -4. The time now is 11:08.

 Contact Us - CFD Online - Top