# problems in meshing sudden expansion and contraction with hex

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

 LinkBack Thread Tools Display Modes
 June 13, 2010, 21:06 problems in meshing sudden expansion and contraction with hex #1 New Member   Join Date: Nov 2009 Posts: 14 Rep Power: 8 Hii all.. I am trying to mesh a slightly complicated structure using hexa using ICEM CFD. I have been able to successfully mesh the structure, however unfortunately the structure appears to have some peculariaties due to which I cannot figure how to reduce the skewness of the meshes. I have put up an illustration of the problem here. The picture below is a 2-dimensional view of the mesh along with the geometry of the part of the structure involved in the problem I am facing. To capture the tertiary channel, I used a simple blocking technique, as shown above, however it turned out that due to the sudden contraction of the channel, highly skewed meshes are formed. I was able to get the simulations running in Fluent, however I think due to this high skewness (Tgrid skewness > .95) in region surrounding the contraction, the error in the continuity equations never go below .3, as a result of which I never get a converged solution. Further the velocities come out to be around 10^4 times higher than in the outer regions, which doesn’t seem physically correct. This is why I think there is some problem with the mesh. Since the surface of channel has a elliptical shape, I thought an Ogrid might be suitable, so I tried an ogrid, while keeping the top and bottom surface fixed as shown below. I split the central box in the O-grid to obtain a better uniformity in the mesh size. This is the mesh distribution on the bottom surface: While the Tgrid skewness in the region surrounding the expansion reduced significantly, the skewness in a separate region increased dramatically to> .95. The second problem I am facing is in the skewness in the longer section of the tertiary channel connecting the primary and the secondary. Due to the high rate of expansion, this too gives rise to a highly skewed mesh. So I was wondering if there is some technique to reduce the skewness of the mesh which I can apply here. It would be great if somebody could give some advice. Thanks Last edited by thinktank; June 14, 2010 at 02:01.

 June 13, 2010, 21:20 #2 New Member   Join Date: Nov 2009 Posts: 14 Rep Power: 8 I have uploaded the project file without the mesh here http://www.megaupload.com/?d=ISKL29TT

 June 15, 2010, 21:44 #3 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Sure, no problem... The first area is really a half ellipse, so a CGRID would be better than an Ogrid. You would need to let it pass thru the adjacent block though... Select the faces like this... ThinkTank_01.jpg Then you get an Ogrid like this (with no down side . ThinkTank_02.jpg For the long diverging channel, your issue is that the one side is longer than the other. You should start by matching edges on the ends so that you have a smooth volume transition in and out of the channel. Then pick one of the edges and copy it to parallel to make them all the same. Since your model was tricky, I used copy to selected edges. you have this same feature over and over again in your model, so you could copy between features also. ThinkTank_03.jpg This will still leave you with some skewness simply because the starting ends line up, but the trailing ends do not. As the mesh is kept proportional, you distribute the end angle thru the length. ThinkTank_04.jpg This would probably run fine, but you could fix it a number of ways. For instance, you could set a larger size one and size 2 for the longer edge. Once you got the sizing right (trial and error probably), you could copy that to the other similar edges. A more controlled way would be to split across the duct so that the one section is nice and parallel and all the transition happens in the other section... ThinkTank_05.jpg You can also improve quality by surface projecting the edges where the duct meets the spiral. When these were edge projected, the corner was constrained to the poor quality angles. I also used edge splits => Control point here on the one side, perhaps it should be on both sides.

June 16, 2010, 15:32
#4
New Member

Join Date: Nov 2009
Posts: 14
Rep Power: 8
Quote:
 Originally Posted by PSYMN Sure, no problem... Then you get an Ogrid like this (with no down side . Attachment 3782
How did you acheive the curved edges. I assume that the black lines are edges of the block.

I always straight edges, as a result I have make multiple splits to make a uniform block mesh

 June 16, 2010, 16:05 Projected Mesh Shape #5 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,660 Blog Entries: 1 Rep Power: 38 Right click on "edges" in the display tree and turn on the option "Projected Mesh Shape". The downside is that it will try to recompute every time you make a change, which is annoying. So I usually just turn on this option for pictures. In the case of the above image, the ogrid might curve more if you had more than one element thru its thickness...

 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 carldaru ANSYS Meshing & Geometry 4 April 13, 2010 13:02

All times are GMT -4. The time now is 20:22.

 Contact Us - CFD Online - Top