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

[ICEM] 2D meshing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 15, 2012, 05:56
Default 2D meshing
  #1
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
Hi All.
I want to make a simulation of non newtonian fluid running in a tube. I have created a 2D mesh in ICEM, but when I'm trying to export the mesh I get the following error:
https://dl.dropbox.com/u/19953951/Capture1.PNG

Is this because ICEM don't understand that its only an area-mesh.
How do I construct a 2 dimensional mesh for my task?

Thansk
Thomashoffmann is offline   Reply With Quote

Old   November 15, 2012, 10:47
Default
  #2
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
I really don't understand why ICEM wants me to define a volume mesh on a 2 dimensional grid. Can anyone explain?

Thanks
Thomashoffmann is offline   Reply With Quote

Old   November 15, 2012, 12:05
Default
  #3
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
can you show us some picture of your geometry. did you make sure to sketch on the XY plane ? it has to be XY plan.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 15, 2012, 13:50
Default
  #4
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
Hi Ali.
I made 4 points by explicit coordinates; (0 0 0),(2 0 0)(2 0.1 0)(0 0.1 0) ie. a square in the XY-plan..
I created curves between the points and then I created a surface from the 4 curves.
Then I went to the mesh tap and then 'surface mesh setup' and computed the 'surface mesh only', see picture below
https://dl.dropbox.com/u/19953951/Capture2.PNG
But when I try to write the input I still get the same error (as shown in the picture)...
Am I missing something as I'm setting up the mesh?
Thomashoffmann is offline   Reply With Quote

Old   November 15, 2012, 13:58
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
have you created a body ?? once i had a problem similar and i created a body, named it fluid , then generated the mesh again. you trying to export for cfx ?
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 15, 2012, 14:20
Default
  #6
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
Yes, I just started over again. And I made a Body named fluid and generated a mesh as before.. I still get the exact same error

And yes I'm exporting for CFX
Thomashoffmann is offline   Reply With Quote

Old   November 15, 2012, 15:41
Default
  #7
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
weird, it should be a very small forgotten detail. i have never tried to export a mesh for cfx, may be the problem comes from the boundary condition you declared. if you don't mind sharing your project i can take a look at it...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 15, 2012, 16:15
Default
  #8
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
I tried to double check my boundary conditions, but couldn't see any problems.. I think it should be kind of simple, but I can't find it - but if you can help me with it I will be gratefull

https://dl.dropbox.com/u/19953951/cap.zip
Thomashoffmann is offline   Reply With Quote

Old   November 15, 2012, 18:01
Default
  #9
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
i couldn't locate the problem, i never had the chance to mesh a simple 2d geometry like this without using the block... that being said i blocked it and generated the mesh, when i exported it to fluent it work. you just need to change it to CFX. Also i noticed that you mentioned ANSYS-CFX, maybe you should try CFX-4 instead ?
here is the link : https://dl.dropbox.com/u/35161486/cap.zip
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   November 16, 2012, 01:43
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
In hexa meshing, ICEM automatically extrude the mesh by one element, when you output the mesh for CFX solver. But for direct meshing algorithms (denauly, octree or auto-block) you need to extrude the mesh by one element. For details see the attached pic



Attached Images
File Type: jpg a.jpg (64.1 KB, 4 views)
File Type: jpg b.jpg (45.1 KB, 3 views)
Far is offline   Reply With Quote

Old   November 16, 2012, 03:30
Default
  #11
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
Thanks Ali. It seems that I have to do blocking. I'm new in ICEM and I haven't heard about blocking before. Can you explain what it is? or do you know where I can read about it?
Thomashoffmann is offline   Reply With Quote

Old   November 16, 2012, 03:37
Default
  #12
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
@Far, If I extrude my mesh by one element in the Z direction wouldn't my geometry turn out as a 3 dimensional problem?
Thomashoffmann is offline   Reply With Quote

Old   November 16, 2012, 03:47
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
No. If you define the symmetry condition on two side walls (two x-y planes at two z locations) in CFX (or any code), you will get the 2d results. This is done (mandatory) because CFX is 3d solver and wont accept 2d meshes and therefore ICEM is not exporting 2d mesh for CFX and asking for volumes.

Try to export your original mesh and set the solver as Fluent and see the difference. You can also read this mesh in Fluent without any error.

Moreover you can export the mesh in Fluent format (.msh) and when you read this mesh in CFX, it will automatically extrude it by one element.

As Ali suggested blocking method is good thing to learn, although may be it is tough in starting and will give you full control.
Far is offline   Reply With Quote

Old   November 16, 2012, 05:09
Default
  #14
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
----------------

Last edited by Thomashoffmann; November 16, 2012 at 08:13. Reason: question answered
Thomashoffmann is offline   Reply With Quote

Old   November 16, 2012, 08:12
Default
  #15
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
ok thanks. But when I open my mesh in cfx and apply an inlet velocity it gives me a strange result, see below

https://dl.dropbox.com/u/19953951/Capture3.PNG

is this because my boundary conditions are made wrong?
I'm not sure whether I have to attach symmetry on my top curve or top plan. And the same for my wall condition - do I have to attach it on the bottom curve or the bottom plan?
Do I need to worry about the third dimension face - shouldn't it be defined as a fluid domain? and the same for the back face, or can I just ignore that face?
Thomashoffmann is offline   Reply With Quote

Old   November 16, 2012, 11:18
Default
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What boundary you would use for top and bottom if that was the 2d case?

Few thoughts:
If that is not the pressure outlet or inlet or wall or you are simulating wind tunnel then I will define them symmetry condition for top and bottom.


It is for sure that symmetry condition will be defined for two side walls.
Far is offline   Reply With Quote

Old   November 16, 2012, 12:00
Default
  #17
Member
 
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 4
Thomashoffmann is on a distinguished road
Never mind, I figured it out - Thanks for your help
Thomashoffmann 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
[ANSYS Meshing] Can I use ANSYS Meshing for manual meshing? Kirjain ANSYS Meshing & Geometry 3 June 12, 2012 08:35
Best Meshing scheme for Cylinder Nutrex Main CFD Forum 4 July 29, 2008 11:03
Meshing locks workbench window. andy2o CFX 0 February 1, 2008 06:01
Singularity of grid?Volume meshing vs face meshing Ken Main CFD Forum 0 September 4, 2003 11:09
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 11:08


All times are GMT -4. The time now is 19:30.