CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

GENERATE MESH IN ICEM and OPEN IN FLUENT 12

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

Like Tree1Likes
  • 1 Post By Galileo

Reply
 
LinkBack Thread Tools Display Modes
Old   January 28, 2011, 14:17
Post GENERATE MESH IN ICEM and OPEN IN FLUENT 12
  #1
Member
 
Engr Adeniyi
Join Date: Jan 2011
Posts: 32
Rep Power: 7
Galileo is on a distinguished road
Hi guys,
Can someone please explain, line by line as much as possible, with a very simple geometry like Rectangle, how to
(1) Create a Mesh in ICEM 12 and Generate .msh file
(2) Open the Mesh in Fluent 12

I have read a number of voluminous tutorials that are not organised in one location. After creating my mesh it saves as .uns and Fluent will not read it.
When I tried using Fluent_V6 as the solver and I generated a .msh file, Fluent will crash while reading it with errors like :

Error: Build_Grid: no cells in case file and at times no zone or cannot read file.

This is really frustrating...
Galileo is offline   Reply With Quote

Old   January 31, 2011, 11:28
Unhappy RE: GENERATE MESH IN ICEM and OPEN IN FLUENT 12
  #2
Member
 
Engr Adeniyi
Join Date: Jan 2011
Posts: 32
Rep Power: 7
Galileo is on a distinguished road
TUTORIAL FILE:

http://cobweb.ecn.purdue.edu/~aerody...romScratch.pdf

The tutorial above leads to the "how" but I don't still get why my system is giving this error:

When Run as 3D
> Reading "C:\My Documents\CFD\FLUENT\TUTORIALS\fluent.msh"...
1200 nodes.
1131 quadrilateral wall faces, zone 9.

Building...
mesh
Error: Build_Grid: no cells in case file.
Clearing partially read grid.

Error: Build Grid: Aborted due to critical error.

Error: Build Grid: Aborted due to critical error.
Error Object: #f


When Run in 2D

Error: Error reading "C:\My Documents\CFD\FLUENT\TUTORIALS\fluent.msh".
Error Object: #f
Reading "C:\My Documents\CFD\FLUENT\TUTORIALS\fluent.msh"...
1200 nodes.
1131 quadrilateral cells, zone 9.
2194 2D interior faces, zone 10.

Building...
mesh
Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.

Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: #f
seyedashraf likes this.

Last edited by Galileo; January 31, 2011 at 11:31. Reason: Wrong path, using the second one instead
Galileo is offline   Reply With Quote

Old   February 3, 2011, 10:38
Smile Resolved Reading ICEM 12.1 Mesh in Fluent 12.1
  #3
Member
 
Engr Adeniyi
Join Date: Jan 2011
Posts: 32
Rep Power: 7
Galileo is on a distinguished road
Thanks guys for trying to help me.

I was able to figure that I was not associating the "edges to the respective curves" properly, when that was done I was able to read in Fluent. The error displayed in Fluent was not good for a beginner and was misleading ACCESS_VIOLATION error.
Galileo is offline   Reply With Quote

Old   February 3, 2011, 16:46
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Exactly right. In ICEM CFD Hexa, only edges associated to curves generate line elements. These line elements form the boundaries for 2D meshes. These boundaries are critical and the Fluent solver can not run without them.

You must associate all the perimeter edges with the perimeter curves, even if they are straight and the edges already seem aligned.

Sorry about the error message. Usually it gives a "null pointer" error.
PSYMN is offline   Reply With Quote

Old   April 11, 2011, 04:05
Default Same problem
  #5
New Member
 
Phani
Join Date: Mar 2011
Posts: 5
Rep Power: 6
phanivasudev is on a distinguished road
Hey galileo,
I'm new to ICEM CFD. I'm facing the same problem, I read the tutorial that u have posted but i haven not come up with any solution.
I have tried in many ways to load the msh file that is created by icem. Can u please let me know how to do it? I have to submit my report in 10 days.
phanivasudev is offline   Reply With Quote

Old   April 11, 2011, 04:08
Default Same Issue
  #6
New Member
 
Phani
Join Date: Mar 2011
Posts: 5
Rep Power: 6
phanivasudev is on a distinguished road
Hey Galileo,
can u let me know how to associate curves to edges ?
phanivasudev is offline   Reply With Quote

Old   April 11, 2011, 12:39
Default Simple Tutorial -To Get Some Results
  #7
Member
 
Engr Adeniyi
Join Date: Jan 2011
Posts: 32
Rep Power: 7
Galileo is on a distinguished road
Quote:
Originally Posted by phanivasudev View Post
Hey Galileo,
can u let me know how to associate curves to edges ?
Hi,

If you can follow this simple tutorial, I hope it will help.
Assume you are drawing a dam
_____Top____
|***** *****|
|***** *****|
|***** *****|
|Wall1***** *|Wall2
|***** *****|
|****# *****|
|***** *****|
|____bottom__|

(@GEOMETRY TAB)
Specify the points and join the lines and create the parts as appropriate.
On the position # (anywhere inside the fluid domain) create a body named Fluid (eg)
(@BLOCKING TAB)
-Click Create Block (First item)
-In the DEZ part name=Fluid
-Type (This is a 2D Blocking, select 2D Blocking)
-Apply (All visible)
-Now Click Split Block and Split by click the Edge and split into the blocks that suits your case...Apply (this case does not need it)
- No Click Associate (item number 5) on Blocking Tab
-In the DEZ click second item ie Associate Edge
-Select Edge then Click Middle Button of your Mouse then Select the Curve and the Middle button of the mouse (Repeat this for all the edges)
_______________Edge
_____Top____
|***** *****| |
|***** *****| |Edge Wall
|***** *****| |
|Wall1** ****|Wall2
|***** *****| |
|***** *****| |
|***** *****| |
|____bottom__| |
_______________Edge bottom
e.g Click Edge Wall then Middle mouse and Click Curve Top, Then Click Edge wall then Curve Wall2 etc (Edge will be red curve will turn black)

You can redo each curve to edge if you are not sure (without need to undo)

Now proceed to 9th item (Pre-Mesh Param)
Go to item 3 on the DEZ
select the edge and put the number of nodes and apply (repeat for other edges -default is 2) ...in this case you need to select only Wall1/2 and Top/Bottom not the 4 ...you will notice that.

You now have your mesh set up.


Expand the Blocking Tree and click Pre-Mesh
Right-Click on the Pre-Mesh and Click -CONVERT TO UNSTRUCTURED MESH


Now Click OUTPUT TAB
Red Box:
DEZ: Select Solver: Ansys and Fluent 6
BC:
Select your BC
SAVE:
Remember to Click 2D (for this 2D case)
The default file name is fluent (you can change it to myfirstdam)

The file saves to myfirstdam.msh
You can open it in Fluent 6 or 12 or 13.
Enjoy and hope it helps
Galileo is offline   Reply With Quote

Old   April 20, 2011, 01:02
Default 3D meshing
  #8
New Member
 
Phani
Join Date: Mar 2011
Posts: 5
Rep Power: 6
phanivasudev is on a distinguished road
hey Galileo,

thanks for the advice. i was able to load cylinder into fluent. but i wish to load a mesh with little irregular geometry. i have attached the geometry.. i have not been able to create a perfect mesh for it.. maybe its because i'm not doing the blocking well.. please advice!!
Attached Images
File Type: png my work.png (39.2 KB, 39 views)
phanivasudev is offline   Reply With Quote

Old   April 20, 2011, 18:43
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
This is a basic Y pipe configuration... There are many ways to do it.

If the flow splits, then the best way is very similar to the pipe blade tutorial (just half of it). That tutorial will show you how to collapse blocks to make this configuration.

You could also do it with a T configuration (as is done for the 2D mixing pipe tutorial).

Optionally, you could create an actual Triangular YBlock (all hexa) in the middle, with radiating blocks... It is pretty straight forward but I don't think we have a tutorial for that.

Best regards,

Simon
__________________
-----------------------------------------
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
PSYMN is offline   Reply With Quote

Old   April 22, 2011, 07:31
Default tried but not working!
  #10
New Member
 
Phani
Join Date: Mar 2011
Posts: 5
Rep Power: 6
phanivasudev is on a distinguished road
hey simon,

thanks for the advise. but unfortunately i haven't been able to do as u suggested. the mesh that is getting created is not cylindrical as in figure and instead is polygonal and i cannot define the inlet and the outlet. can u suggest any other way to create geometry and then do the blocking as i'm guessing that the problem is geometry.

phani
phanivasudev is offline   Reply With Quote

Old   September 6, 2013, 13:26
Default
  #11
New Member
 
Join Date: Sep 2012
Posts: 2
Rep Power: 0
koya is on a distinguished road
hi Galileo,

I am stuck with this single element problem in ICEM. My geometry is a 3D IGES file. I imported and mesh it using the Delaunay scheme. The single elements error pops up when I check the mesh. Is there a way to get around this. I have attached the picture. Thank you very much.
Attached Images
File Type: jpg mesh.jpg (16.4 KB, 25 views)
koya 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
How to open Icem mesh in Ansys Fluent? emmkell FLUENT 26 June 9, 2015 15:38
Export 2D mesh from ICEM to Fluent enghamed ANSYS Meshing & Geometry 17 June 7, 2013 14:36
Export 2D mesh from ICEM to Fluent BuilttoSpill ANSYS Meshing & Geometry 4 August 28, 2010 08:16
ICEM Edit Mesh blackbody ANSYS Meshing & Geometry 3 March 8, 2010 03:49
ICEM CFD 5.1 Hex-Tet mesh merging failure bogesz CFX 1 January 29, 2005 07:46


All times are GMT -4. The time now is 01:15.