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

[ICEM] Meshing problem with ICEM

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 14, 2013, 14:22
Default Meshing problem with ICEM
  #1
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hi to everybody,

I am a newbie with meshing and/but try to mesh a cylindrical furnace with a concentric cylindrical heating element. The air inside the furnace is connected to the surrounding area via two cylindrical drill holes (air inlet, air outlet).
First of all I only try to mesh the air (neiter insulation around the air, nor heating element) with a volume mesh.

Is it possible to add surface meshes for contact areas air/insulation and air/heating element???

I've tried to work with blocking and o-grids but awfully failed at the positions where the drill holes are connected to the air volume,
although I spent really much time.
How can I adjust the meshes of the air inlet and outlet and the air volume mesh???
Please help me!

Since the heating element does not belong to that mesh I need to delete the central block.

Aylalisa
Attached Images
File Type: jpg Air_Inlet.jpg (58.6 KB, 57 views)
File Type: jpg Air_Inlet_Outlet.jpg (26.9 KB, 47 views)
File Type: jpg distorted_cells.jpg (79.8 KB, 50 views)
aylalisa is offline   Reply With Quote

Old   January 15, 2013, 07:59
Default
  #2
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 9
energy382 is on a distinguished road
Associate face to surface (in the area of destroyed elements). If it doesn't work, use interpolate.

You've to provide your .tin and .blk files if you don't get rid of the bad elements




Quote:
Originally Posted by aylalisa View Post
Hi to everybody,

I am a newbie with meshing and/but try to mesh a cylindrical furnace with a concentric cylindrical heating element. The air inside the furnace is connected to the surrounding area via two cylindrical drill holes (air inlet, air outlet).
First of all I only try to mesh the air (neiter insulation around the air, nor heating element) with a volume mesh.

Is it possible to add surface meshes for contact areas air/insulation and air/heating element???

I've tried to work with blocking and o-grids but awfully failed at the positions where the drill holes are connected to the air volume,
although I spent really much time.
How can I adjust the meshes of the air inlet and outlet and the air volume mesh???
Please help me!

Since the heating element does not belong to that mesh I need to delete the central block.

Aylalisa
energy382 is offline   Reply With Quote

Old   January 15, 2013, 12:59
Default
  #3
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hi energy,

thanks too much for your support . 'Face to Surface > Part' and 'Face to Surface > Interpolate' helped me to get the attached models.

I've tried different proceedings:

Strömungsraum_6:
bottom-up
I've generated three blocks and then directly used O-Grid. With help of 'Face to Surface' I've reached that result but still receive quite a couple of bad cells.

Strömungsraum_8:
top-down
I've decomposed one big block in several small blocks, deleted some and finally merged the small ones together again. 'Face to Surface' has provided me that result.

Could you tell me how I can get rid off the ugly cells in Strömungsraum_6?
What strategy is in that case the best?

My final goal is to simulate the heating element (solid) and the air (fluid) that is heated up by convection and radiation. So I will end up with two meshes. Do you know if I have to build two individual meshes or is it necessary to built both in the same model, if that is possible at all.


Aylalisa
Attached Files
File Type: zip Stroemungsraum_6.zip (39.6 KB, 13 views)
File Type: zip Stroemungsraum_8.zip (41.9 KB, 8 views)
aylalisa is offline   Reply With Quote

Old   January 16, 2013, 04:55
Default
  #4
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 9
energy382 is on a distinguished road
I'll check it tomorrow. I'm out of office today.

Regards,
Christoph
energy382 is offline   Reply With Quote

Old   January 17, 2013, 11:51
Default
  #5
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
With your project number 6, the main problem is the edge of the O-grid of the cylindrical drill holes. They are associated to a surface (colored in black) but there are inside the fluid (they should be colored in blue).
I think you didn't associate the face to surface in the good way.
So use the tool "Blocking -> Blocking Associations -> Disassociate from Geometry -> Edges" and select those edges. They will turn in blue which will fix your issue
BrolY is offline   Reply With Quote

Old   January 21, 2013, 05:22
Default
  #6
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hi Alexandre,

thank u for your help!!! That worked , but still there are (only) a few skewed cells at the intersection where the drill hole meets the main pipe.

Why did that deassociate thing exactly work?

Do you know repair for the remaining skewed cells?
Refining the mesh does not really remove that skewed cells but unnecessarily increase the number of cells I think ...

Plenty of regards
Lisa
Attached Images
File Type: jpg Str6_last_skewed_cells.jpg (47.6 KB, 26 views)
Attached Files
File Type: zip Stroemungsraum_6b.zip (39.7 KB, 4 views)
aylalisa is offline   Reply With Quote

Old   January 21, 2013, 07:31
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
There is problem in blocking. Did you merge the vertices at some stage? Check through scan plane in the two pipes
Far is online now   Reply With Quote

Old   January 21, 2013, 07:47
Default
  #8
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hello Far,

thanks a lot for your reply!!!
I've not merged vertices but I've cut one big block in many small ones, deleted some and merged them again before I've used o-grid.
Is there maybe a possiblity to get rid of the bad elements without starting the whole procedure from the beginning?

What kind of proceeding is in that case the best one:
Start with one big block, cut in small ones, delete and merge to adjust the geometry, or
create three blocks: one for the main air volume and two additional small ones for inlet and outlet air pipes???
In each case I end up with a couple of bad cells, even if I don't merge vertices on the way?!
Do I make a principal mistake or could I improve the mesh quality by local adjustments?

Viele Grüße
Lisa
aylalisa is offline   Reply With Quote

Old   January 21, 2013, 09:44
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Angle > 34 deg
Quality > 0.5

Steps

1. One bigger block and o-grid. Delete inner block and associate edges to curves. Snap vertices.

2. Split at appropriate places (four along bigger pipe and two on two sides of smaller pipes).

3. Draw two curves through centre points in smaller pipes (see in attach files) and use extrude along curve option to extend blocking in smaller pipes and associate curves at the end of pipes and at intersection with larger pipe.

4. Make ogrid for smaller pipes. Select two blocks (one for smaller pipe and one in the larger pipe touching heating pipe and select two end faces)

5. Assign sizes on surfaces through part mesh setup (maximum size 3) and click on update all (blocking>edge mesh parameters> update all). And if necessary set the edge mesh parameters for the o-gird edges in the smaller pipes

genießen



Attached Files
File Type: zip Pipe_Far.zip (48.3 KB, 7 views)
aylalisa likes this.

Last edited by Far; January 21, 2013 at 12:16.
Far is online now   Reply With Quote

Old   January 21, 2013, 12:11
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by aylalisa View Post
Hi energy,

thanks too much for your support . 'Face to Surface > Part' and 'Face to Surface > Interpolate' helped me to get the attached models.

I've tried different proceedings:

Strömungsraum_6:
bottom-up
I've generated three blocks and then directly used O-Grid. With help of 'Face to Surface' I've reached that result but still receive quite a couple of bad cells.

Strömungsraum_8:
top-down
I've decomposed one big block in several small blocks, deleted some and finally merged the small ones together again. 'Face to Surface' has provided me that result.

Could you tell me how I can get rid off the ugly cells in Strömungsraum_6?
What strategy is in that case the best?

My final goal is to simulate the heating element (solid) and the air (fluid) that is heated up by convection and radiation. So I will end up with two meshes. Do you know if I have to build two individual meshes or is it necessary to built both in the same model, if that is possible at all.


Aylalisa
I didn't follow this thread, so I would like to ask two questions:
1. Your both approaches are producing the problem elements?
2. Do you need solid blocks?
Far is online now   Reply With Quote

Old   January 22, 2013, 09:51
Default
  #11
New Member
 
Alexander
Join Date: Nov 2009
Location: Blansko, Czech Republic
Posts: 28
Rep Power: 7
Pospelov is on a distinguished road
Hello everybody.
aylalisa. If it's geometry for CFD calculation I will do enouther blocks for this geometry. 1. You need boundary blocks. In attach file you can fine my solution.
The first errors was in black edges. The second in blocks.
Attached Files
File Type: zip Stroemungsraum_6.zip (38.8 KB, 9 views)

Last edited by Pospelov; January 22, 2013 at 10:28.
Pospelov is offline   Reply With Quote

Old   January 22, 2013, 10:29
Thumbs up
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by Pospelov View Post
Hello everybody.
aylalisa. If it's geometry for CFD calculation I will do enouther blocks for this geometry. 1. You need boundary blocks. In attach file you can fine my solution.
The first errors was in black edges. The second in blocks.
Better blocking. Well done.

Also check this blocking ...
Attached Files
File Type: zip pipe_Far2.zip (49.4 KB, 10 views)
Far is online now   Reply With Quote

Old   January 22, 2013, 11:15
Default Wow!!!
  #13
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
A very big thank you for all your approaches!!!!
I will figure out now to see if I can follow!

I am happy !

Lisa
aylalisa is offline   Reply With Quote

Old   January 22, 2013, 13:05
Default error message: extrusion of faces failed
  #14
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Quote:
Originally Posted by Far View Post
Angle > 34 deg
Quality > 0.5

Steps

1. One bigger block and o-grid. Delete inner block and associate edges to curves. Snap vertices.

2. Split at appropriate places (four along bigger pipe and two on two sides of smaller pipes).

3. Draw two curves through centre points in smaller pipes (see in attach files) and use extrude along curve option to extend blocking in smaller pipes and associate curves at the end of pipes and at intersection with larger pipe.

4. Make ogrid for smaller pipes. Select two blocks (one for smaller pipe and one in the larger pipe touching heating pipe and select two end faces)

5. Assign sizes on surfaces through part mesh setup (maximum size 3) and click on update all (blocking>edge mesh parameters> update all). And if necessary set the edge mesh parameters for the o-gird edges in the smaller pipes

genießen



There is still potential for mistakes that I always manage to make out.
May I ask you for detailed hints, especially according to the first three steps?

1. O-Grid
( ) without selection of top and bottom faces
( ) with selection of top and bottom faces
I've decided for the latter option.

Association:
outer edges of remaining blocks will be associated to outer circle
inner edges of remaining blocks will be associated to inner circle (center drill hole)

2. split at appropriate places
why 'four along bigger pipe'?
After 'snap vertices' it seems that there is only need for two splits along
bigger pipe?
--> screenshot
I understand 'two on two sides of smaller pipes'.

3. extrusions for smaller pipes
no problem with creation of two points,
no problem with creation of two curves,
BUT: I always receive an error message if I try the 'extrusion of faces'
--> screenshot
This also happend all the time during earlier attempts.

Why?

Finally I gave up to try using the extrusion command.
I use ICEM v14 on Windows 7

I thought I make some mistake but according to your description the usage of this command seems to be all right in this context.

Can anybody help???

Lisa
Attached Images
File Type: jpg after_two_along_bigger_pipe_and_two_for each_smaller_pipe.jpg (36.4 KB, 6 views)
File Type: jpg extrusion_error.jpg (48.4 KB, 6 views)
aylalisa is offline   Reply With Quote

Old   January 22, 2013, 13:18
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
1. Are you using extrude along curve option?

2. Are you selecting the correct face?

Quote:
t seems that there is only need for two splits along
bigger pipe?
correct

Quote:
I use ICEM v14 on Windows 7
So do I.
Far is online now   Reply With Quote

Old   January 22, 2013, 13:38
Default Now it works!
  #16
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
I've always tried the steps in the wrong order!

WRONG:
I've split the o-grid --> fine
I've tried to extrude faces before I've associated the edges to curve of small pipes

WORKING VERSION:
I've split the o-grid --> fine
I've associated the edges to curves (edges of new faces, generated by splits - curves of pipe)
then 'extrude faces' works

I really don't miss any chance to create problems .

Super!!!!

Viele Grüße
Lisa
Attached Images
File Type: jpg extrusion_of_faces_works.jpg (40.8 KB, 8 views)
aylalisa is offline   Reply With Quote

Old   January 22, 2013, 15:04
Default Perfect Result - but last question
  #17
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa
aylalisa is offline   Reply With Quote

Old   January 22, 2013, 15:24
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by aylalisa View Post
Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa
Correct options are :

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
Ansys fluent
Far is online now   Reply With Quote

Old   January 22, 2013, 17:43
Default
  #19
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by aylalisa View Post
Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa
Hi Lisa

I saw one thread in Openfoam forum, where it is discussed in detail how to export mesh for OF from ICEM. Check it.Converting mesh from Icem CFD to OpenFoam
Far is online now   Reply With Quote

Old   January 22, 2013, 18:02
Default
  #20
New Member
 
Alexander
Join Date: Nov 2009
Location: Blansko, Czech Republic
Posts: 28
Rep Power: 7
Pospelov is on a distinguished road
Quote:
Originally Posted by Far View Post
Better blocking. Well done.

Also check this blocking ...
Yes. This blocking is good too. And it's more easy to create it. ;-)
Pospelov 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] complex 2D meshing on ICEM kassab ANSYS Meshing & Geometry 26 April 14, 2014 21:02
[ANSYS Meshing] Hybrid meshing ICEM djoul ANSYS Meshing & Geometry 2 January 17, 2012 19:18
[ICEM] ICEM meshing problem xyq102296 ANSYS Meshing & Geometry 6 October 28, 2010 10:09
[ICEM] Meshing problem from ICEM CFD to Fluent cfdonlinederafa ANSYS Meshing & Geometry 2 September 21, 2010 16:16
ICEM meshing problem Forrest CFX 4 May 25, 2005 18:37


All times are GMT -4. The time now is 06:28.