CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Volume Orientation Issue

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

Like Tree1Likes
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2013, 14:51
Default Volume Orientation Issue
  #1
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Hi,

I am currently investigating an enclosed rotating disc at high Reynolds numbers.

The Fluid volume has a quite simple geometry. It is bordered by two surfaces of revolution, one for the shroud and another for the shaft. There are also three surfaces adjacent to the disc, one for the rim and the others for the disc sides. Finally there are two periodic surfaces which close the volume. You can see the geometrie in the attached pictures below.

I need a node spacing of 0.01 mm on each wall and at this point I got stuck. ICEM found some volume errors and I don't know how to get rid of them. As you can see from the pictures the blocking topologie is also very simple. Just entered 0.01 for spacing 1 and 2 on each edge (except the edges on the periodics) and a ratio of 1.1 . It should be that easy, shouldn't it?

I also checked the associations with the geometrie. I can not find anything. So where am I wrong?

Thank in advance!
Attached Images
File Type: jpg Volumen Orientation.jpg (95.6 KB, 32 views)
File Type: jpg Spacing.JPG (95.7 KB, 18 views)
File Type: jpg Blocking.JPG (37.4 KB, 21 views)
File Type: jpg Association.JPG (55.6 KB, 19 views)
Daniel C is offline   Reply With Quote

Old   January 25, 2013, 15:15
Default Skewed Element
  #2
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
I saw some skewed elements. I can't fix them.
Attached Images
File Type: jpg Skewed.JPG (21.7 KB, 12 views)
Daniel C is offline   Reply With Quote

Old   January 25, 2013, 16:54
Default
  #3
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
I found a way to resolve this problem. I quit blocking and changed over to a 2D blocking and extrudet it by rotation and loaded the mesh finally with it. So in my opinion it is better to use an unstructured grid for this case.

But I am pretty curious and appriciate every hint, how to mesh this geometry in 3D. Essentially that should be no problem.
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 02:03
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
It is very simple geometry. The possible problems/solutions are:

1. Association

2. Edit edge commands

3. Splitting and snap vertices
Far is offline   Reply With Quote

Old   January 26, 2013, 10:11
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
When applying a bunching law, you have to make sure it is applied to the parallel edges as well. but not all the parallel edges has the same direction. may be one of youre edge has the same bunching law but in the reverse direction
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 26, 2013, 12:03
Default
  #6
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Thank you Far and diamondx for your hints.

I applied the bunching law to all parallel edges. Yes, sure one has to consider that some edges have reverse spacing direction, but in my case I just apply the same spacing for each direction, so I don't care about the direction.

I loaded a step file from CATIA V5, a very simple geometry. I assigned the outer most vertices to the corner points and split the block twice. Then I deleted the center block which represents the disc material, but not permanently. Finally I assigned all the new vertices to the geometry points and the faces to the respective surfaces. I controlled everything by EDGE\Show Association. All vertices are aligned and associated with the geometry.

I did it over and over again, but could not get any utilizable result. But if I use an unstructured 2D mesh, and let ICEM extrude it by rotation, everything is fine.

If it is not caused by my step file, I would say ICEM is very buggy.
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 12:10
Default
  #7
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Here is my tin file, just if somebody is interested in resolving my problem.
Attached Files
File Type: zip FLUID.zip (2.1 KB, 4 views)
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 12:44
Default
  #8
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I didn't find any problem.

Can you attach the problematic blocking?
Attached Files
File Type: zip FLUID_Far.zip (10.8 KB, 3 views)
Far is offline   Reply With Quote

Old   January 26, 2013, 13:12
Default
  #9
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Here is my blocking.

Thank you in advance!
Attached Files
File Type: zip Blocking.zip (3.2 KB, 3 views)
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 13:26
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Is it necessary to use .01? Why not .03?
Far is offline   Reply With Quote

Old   January 26, 2013, 13:33
Default
  #11
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Far, I used your blocking and got the same problems again. There are very few cells, what are erroneous. They should be identical to the other good cells, because of the constant curvature.

I am obviously doing something wrong.
Attached Images
File Type: jpg Orientation Error.jpg (97.8 KB, 18 views)
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 13:36
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Those cells are not perfect rectangles as other cells are. Dont know why !!!
Far is offline   Reply With Quote

Old   January 26, 2013, 13:39
Default
  #13
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
It is not necessary to use exactly 0,01 but I need to refine the wall spacing to get a certain y+ for the wall function. In the worst case I have to go below 0.01, namely 0,001.

It should be possible with 0,01, shouldn't it? Or is ICEM not capable to build such a grid with the blocking approach?

As I said, my problem is resolved. I use a 2D mesh and convert it to an unstructured mesh. The circumferential elongation is achieved by extruding the 2D mesh by rotation. I am usung -1 angle per layer and using 1 layer to get a 15 segment.
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 13:53
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Hey I found the solution. It was a geometry problem. Deleted all surfaces and recreated all from curves.

I even used 0.001 without any problem.

Although I made the blocking for one portion of the geometry this time but it is enough to prove my proposition.


Quote:
As I said, my problem is resolved. I use a 2D mesh and convert it to an unstructured mesh. The circumferential elongation is achieved by extruding the 2D mesh by rotation. I am using -1 angle per layer and using 1 layer to get a 15 segment.
Because here your mesh is not being influenced by the geometry inaccuracies.
Attached Files
File Type: zip Solved_Far.zip (29.8 KB, 1 views)
Daniel C likes this.
Far is offline   Reply With Quote

Old   January 26, 2013, 14:16
Default
  #15
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Far you are great!

That is a very subtle geometry failure. I will carefully reviev any geomery that is derived from a step file in the future.

I always appreciate your efforts!
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 14:38
Default
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Check this and give some comments that what is happening in ICEM
Attached Files
File Type: zip Full_Far.zip (41.5 KB, 5 views)
Far is offline   Reply With Quote

Old   January 26, 2013, 15:08
Default
  #17
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Haha, you have an accurate eye

After you discovered the issue with the erroneous surfaces, it was clear to me that this must be the source of error. So I tried to resolve it according to your advice and got rid of the problem. But I checked your solution and it is fine. So thank you very much Far, and once again I appreciate your efforts.
Daniel C is offline   Reply With Quote

Old   January 26, 2013, 15:16
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Actually it is not only the problem due to the erroneous geometry only. Say it is 30%.

You can observe I have made the intermediate surfaces between the thin and large blocks on both sides. First to get the overall idea I only made that surface in one portion. And to my surprise I got problem in the other side (where surface is not present) although with lower intensity.

So what I conclude that closed volume is necessary to get the prefect rectangles.

Also to avoid the walls due to those internal surfaces I placed the materials points with same names in all those closed surfaces.

Got it!!! Life is full of trial and error
Far 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
[ICEM] Volume orientation MGF ANSYS Meshing & Geometry 2 September 19, 2012 11:55
Volume 1 has invalid topology for mapped brick meshing georgewar ANSYS 0 July 24, 2011 16:02
Issue with volume fraction pranab_jha FLUENT 2 June 25, 2010 17:26
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
help needed about phase change Yanhu Guo Main CFD Forum 4 January 24, 2001 00:16


All times are GMT -4. The time now is 12:03.