# [ICEM] Meshing of a parabolic trough

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

June 5, 2012, 10:31
Meshing of a parabolic trough
#1
Member

Join Date: Jun 2012
Posts: 40
Rep Power: 5
Hello everybody,

I am working on this case now for quite a long time and haven't found the solution for my problem so i thought maybe you can help me out. I am a beginner at ICEM so maybe i just lack of knowledge and my problem isn't that difficult to solve.

We want to create a Hexa mesh around a parabolic trough. I have to make a numerical simulation for three different angles of the trough. You can see two of them in the pictures.

First I tried to create a block structured mesh with an O-Grid around the trough. But since the trough is very close to the bottom i wasn't able to create a high quality mesh (picture 1 shows the trough and the bottom).

After that I tried some tetra meshing using the octree method with prism layer around the mesh and at the bottom of the wind tunnel. This mesh was the best to this point but since my task is to create a hexa mesh I can't use it. It's still not perfect because i quit at some point when i understood how to create a tetra mesh in general.

At the moment i try to create a unstructured hexa mesh using the BFCart mesher. It took me quite some time while testing on how to create an unstructured hexa mesh to realize that the mesh has to be very dense around the trough. The mesh always went through the trough before. But since the trough has a very small thickness even very small hexas around the trough are still to big (see picture 2).

So once again, I am new to ICEM and this Forum so I hope you do understand my problem.

Attached Images
 picture1.PNG (12.9 KB, 182 views) picture 2.jpg (59.7 KB, 173 views)

 June 5, 2012, 12:38 #2 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,916 Blog Entries: 6 Rep Power: 39 create an ogrid around geometry

June 6, 2012, 04:40
#3
Member

Join Date: Jun 2012
Posts: 40
Rep Power: 5
Hello Far,

I already tried an O-Grid and it didn't work out that great.
I uploaded a picture of my O-Grid so you can see where i have trouble.
I'd be very happy for any advice to improve this grid

edit: Of course this grid needs some refinement etc. but my main problem the transition between the O-Grid and the surrounding mesh especially in the bottom area remains the same I think.
Attached Images
 ogrid.PNG (24.6 KB, 220 views)

 June 6, 2012, 04:48 #4 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,916 Blog Entries: 6 Rep Power: 39 you are almost there. just more splits and move vertices. Also reduce the size of o-block (go to edit block> rescale oblock). You may need some advance topology strategy. See the video tutorial series (famous 3 part YouTube video on air-foil meshing by Simon) where he has explained how to handle high staggered air-foil with advance blocking.

June 6, 2012, 04:55
#5
Member

Join Date: Jun 2012
Posts: 40
Rep Power: 5
Quote:
 Originally Posted by Far you are almost there. just more splits and move vertices. Also reduce the size of o-block (go to edit block> rescale oblock). You may need some advance topology strategy. See the video tutorial series (famous 3 part YouTube video on air-foil meshing by Simon) where he has explained how to handle high staggered air-foil with advance blocking.
I'll work on this mesh again after watching your suggested series.

edit: The series I found is for a 2D modell. Mine is 3D. Is it the one you were talking about? http://www.youtube.com/watch?v=tYrbScUH9RE

 June 6, 2012, 05:04 #6 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,916 Blog Entries: 6 Rep Power: 39 I cannot open link from my office (Youtube is banned). Here is the Google search revealed same videos I was referring http://www.google.com.pk/search?suge...+meshing+3part http://www.veengle.com/s/ICEM-CFD/2.html

June 6, 2012, 11:35
#7
Member

Join Date: Jun 2012
Posts: 40
Rep Power: 5
I worked on this basically the whole day and wasn't able to get it done.
I tried the rescaling of the O-Grid and got the error "No rescale direction specified." I don't know where I can specify this and I am not sure how this rescaling option works generally.

I watched the Tutorial. It was very interesting but I couldn't get too much out of it concerning my Problem.

While the mesh was mostly OK my main problem is still the bottom part of the O-Grid where the mesh becomes very dense (as shown in the attached picture). I wasn't able to fix this problem with my little ICEM knowledge.
Attached Images
 ogrid2.png (25.0 KB, 129 views)

 June 6, 2012, 11:46 #8 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,916 Blog Entries: 6 Rep Power: 39 send files

June 6, 2012, 12:43
#9
Member

Join Date: Jun 2012
Posts: 40
Rep Power: 5
Quote:
 Originally Posted by Far send files
There you go.

I hope my work is not too bad.

The farfield is huge in both x-directions because we wanna use this mesh to for two calculations to simulate different angles of the trough. Your welcome to comment on this also
Attached Files
 parabolic_trough_bazinga.zip (51.6 KB, 44 views)

 June 6, 2012, 15:50 Better Topology #10 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 36 Your topology is not great... Instead of thinking of this as some box at an incline, think of it as 1/4 of a circle (imagine the ogrid creating a box around the theoretical center) or as a fillet (imagine the surfaces extending up stream and up towards the top of the box... Here I will show how to capture the latter... Start with two splits, one below and one behind the curve... Banzinga_01.jpg Then put in a quarter Ogrid (one block with 4 faces) to capture the curvature. Banzinga_02.jpg I rescaled my Ogrid (0.3) to be closer to fitting the model... Banzinga_03.jpg Then I split out to fit the blade... Split upstream, downstream, upper surface, lower surface to box it out. Banzinga_04.jpg Other verts could be adjusted also to improve the angles, etc. Then use "Align verts" to get it nice and crisp. I don't have time to complete it for you, but this should get you started. Also, here is a 30 second start on the other option, the circle option... Here is the basic blocking after 4 splits and an Ogrid thru the model (one block, 2 faces). From here, you would split out the airfoil, etc. Banzinga_05.jpg Far, M201170944, venkat_aero2007 and 3 others like this. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 June 6, 2012, 18:55 #11 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 Here is what i got... i don't know why winrar couldn't compress it in zip format, so i made it in my dropbox, here is the link: https://dl.dropbox.com/u/35161486/parabolic.rar __________________ Regards, New to ICEM CFD, try this document --> http://goo.gl/G2gkE Ali

 June 6, 2012, 19:02 #12 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 picture is huge sorry about that __________________ Regards, New to ICEM CFD, try this document --> http://goo.gl/G2gkE Ali

 June 6, 2012, 21:50 #13 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 36 Yes, now the question is if that resolution is sufficient... (clearly it is not yet, but I assume you plan to keep working on it). I hadn't really taken a close look at the shape of your airfoil before... Quality on the curved "corners" won't be ideal. You could probably also place a small Ogrid around the airfoil blocks for an extra refined boundary layer... __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 June 6, 2012, 22:34 #14 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 true... because refining on a laptop requires a bit more of memory... but i added and o-grid around. hope it's correct here is new link : https://dl.dropbox.com/u/35161486/barabolic2.rar I don't know why this pictures are so big !!! Bazinga likes this. __________________ Regards, New to ICEM CFD, try this document --> http://goo.gl/G2gkE Ali

 June 6, 2012, 22:41 #15 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Canada Posts: 1,291 Blog Entries: 23 Rep Power: 20 of course quality can be improved more when playing with vertices...i'll play with it more in lab. PCs are faster there. thanks Simon for this blocking strategy and the advices . __________________ Regards, New to ICEM CFD, try this document --> http://goo.gl/G2gkE Ali

 June 6, 2012, 23:33 On the right track... #16 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,662 Blog Entries: 1 Rep Power: 36 Yea, I think you are on the right track now... The topology is done, and you just need to spend some time fine-tuning the vertex placement and working out the edge distributions... Make sure you learn how to use "Align Vertex" and "Set Location", both of these are under "Move Vertex" and can really help you align everything for maximum quality... You control the extent of their influence with the index control, so hopefully you have figured out how to use that also. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 June 7, 2012, 02:54 #17 Member   Join Date: Jun 2012 Posts: 40 Rep Power: 5 Wow, these are great ideas. Thank you very much everybody. I'll try to do it in a similar way on my own and post again when I am done.

June 7, 2012, 04:14
#18
Super Moderator

Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Posts: 3,916
Blog Entries: 6
Rep Power: 39
I have managed to make blocking as Simon suggested. Still internal o-block is remaining and also some splits on wing or whatever
Attached Files
 parabolic_trough_bazinga_Far.zip (51.7 KB, 35 views)

Last edited by Far; June 7, 2012 at 04:39.

June 7, 2012, 08:04
#19
Super Moderator

Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Quote:
 Originally Posted by PSYMN Start with two splits, one below and one behind the curve...
Horizontal split is necessary?

Quote:
 Then put in a quarter Ogrid (one block with 4 faces) to capture the curvature.
Should we crate the y-blcok at the corner where two splits meet?

Quote:
 the circle option... Here is the basic blocking after 4 splits and an Ogrid thru the model (one block, 2 faces). From here, you would split out the airfoil, etc.
Which option is better, this one or quarter Ogrid?

June 7, 2012, 13:31
#20
Senior Member

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
@ Far

Quote:
 Horizontal split is necessary?
The horizontal split assumes that there is a floor in this model... I assumed there is or the model would have centered the scoop. If there is a floor and we are considering viscous effects... It is nice to keep that boundary layer clean. Without that lower horizontal split, the boundary layer would peel away from the wall and shoot straight up, wasting mesh in the volume, creating volume jump problems and leaving no boundary layer for downstream...

Quote:
 Should we crate the y-blcok at the corner where two splits meet?
No idea what you mean about the Y block... But I don't think anything else is necessary. Simpler is usually better, even if the quality is just a little worse. This blocking suggestion should give more than adequate quality.

Quote:
 Which option is better, this one (circle) or quarter Ogrid?
That depends on what the flow looks like (or what is expected). If the flow is fast and this scoop sends a large portion upward for a long distance, the Quarter Ogrid will be good because you can get higher resolution in that area above (downstream) of the scoop. You could even come back and adjust the blocking slightly to align the vertical portion of the Ogrid with the flow and get better resolution.

But if the flow is lower speed and not much happens between the scoop and the top of the airfoil, then that mesh refinement is wasted in the quarter Ogrid and the circle method may be better... The circle method also has the advantage of being somewhat self contained... In other words, it doesn't propagate and cause difficulty elsewhere in the model. That is not a concern for this particular case, but imagine if we had many such scoops and all the quarter ogrids started intersecting, etc. It could become a mess.
__________________
-----------------------------------------

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

 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 [ANSYS Meshing] Migrating from GAMBIT to ANSYS Meshing David-CFD ANSYS Meshing & Geometry 1 April 1, 2011 05:22 benru OpenFOAM Bugs 42 November 13, 2009 08:59 Nutrex Main CFD Forum 4 July 29, 2008 11:03 Ken Main CFD Forum 0 September 4, 2003 11:09 ken FLUENT 0 September 4, 2003 11:08

All times are GMT -4. The time now is 05:48.