|
[Sponsors] |
November 15, 2012, 04:56 |
2D meshing
|
#1 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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 |
|
November 15, 2012, 09:47 |
|
#2 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
I really don't understand why ICEM wants me to define a volume mesh on a 2 dimensional grid. Can anyone explain?
Thanks |
|
November 15, 2012, 12:50 |
|
#4 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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? |
|
November 15, 2012, 12:58 |
|
#5 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
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 ?
|
|
November 15, 2012, 13:20 |
|
#6 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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 |
|
November 15, 2012, 14:41 |
|
#7 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
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...
|
|
November 15, 2012, 15:15 |
|
#8 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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 |
|
November 15, 2012, 17:01 |
|
#9 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
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 |
|
November 16, 2012, 00:43 |
|
#10 |
Super Moderator
|
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
|
|
November 16, 2012, 02:30 |
|
#11 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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?
|
|
November 16, 2012, 02:37 |
|
#12 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
@Far, If I extrude my mesh by one element in the Z direction wouldn't my geometry turn out as a 3 dimensional problem?
|
|
November 16, 2012, 02:47 |
|
#13 |
Super Moderator
|
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. |
|
November 16, 2012, 04:09 |
|
#14 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
----------------
Last edited by Thomashoffmann; November 16, 2012 at 07:13. Reason: question answered |
|
November 16, 2012, 07:12 |
|
#15 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
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? |
|
November 16, 2012, 10:18 |
|
#16 |
Super Moderator
|
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. |
|
November 16, 2012, 11:00 |
|
#17 |
Member
Thomas Hoffmann
Join Date: Oct 2012
Posts: 67
Rep Power: 13 |
Never mind, I figured it out - Thanks for your help
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
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 05:01 |
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 |