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

[ICEM] ICEM 2D -> Fluent

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2012, 05:18
Default ICEM 2D -> Fluent
  #1
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
The geometry is very simple for example. I tried to do two different ways:
1. Create a sketch in SW, fill it and import in ICEM, they create a grid.
2. Created in ICEM geometry of points and they create a grid.
Choose the solver Fluent V6 and save the output cyl2d.msh by selecting 2D.
In ICEM create 2D Planar, and then do as in the case of 3D. Am I correct to create a 2D mesh in ICEM?

Choose 2D & parallel Fluent. In both cases, displays a message:
Error: Failed in Fill_Domain.
Note: It is possible that this case or mesh file needs to be first
processed by the serial solver. To do this, please read
file into the serial solver and then save it. Next,
read saved file into the parallel solver.
MPI Application rank 0 exited before MPI_Finalize() with status -1073741819
Error: Build Grid: Aborted due to critical error.
Error Object: #f
The Parallel FLUENT process could not be started.

According to the recommendation choose serial. In both cases, displays a message:
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.
Attached Files
File Type: zip cyl2d.zip (41.2 KB, 14 views)
Ralen is offline   Reply With Quote

Old   May 6, 2012, 18:02
Default Associate Edge to Curve
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You did not associate your edges to your curves.

In ICEM CFD, associating edges to curves causes line elements to be created in the part name of the curves. When you send the mesh to Fluent, these are used as the boundaries.

Usually, I would expect to see a "null pointer error" or something like that... But I just associated the edges to the perimeter curves and it worked...

Simon

MeshInFluent.jpg
Ralen likes this.
__________________
-----------------------------------------
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   May 7, 2012, 00:39
Default
  #3
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
I just do not always associated the straight edge. Usually, they are automatically associated.
Ralen is offline   Reply With Quote

Old   May 7, 2012, 09:49
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
No, they are aligned because the edges are straight and the boundaries are straight, but that is not the same as associated... For 3D, it only matters if you smooth (because aligned nodes stay on the feature curves), but for 2D it is critical for creating boundaries.

Fluent 14.5 has had a slight improvement in that it now has a much better error message when you have this problem that should get you going in the right direction much more quickly.
__________________
-----------------------------------------
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   May 8, 2012, 01:15
Default
  #5
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
In the first project I only associated the edges and renamed SOLID in FLUID. Solver for Export - Fluent V6.
Fluent: k-epsilon, in - velocity inlet, out - pressure outlet. Initialize with X Velocity 10 or 100.
1. Air 100 m/s
2. Water Liquid 10 m/s
If I increase the number of nodes from 80 to 1000 (the minimum mesh size is ~ 1e-5 m) and set Settings->Model to 1e-14, then I get that on the third picture (Water Liquid 10 m/s).
Attached Images
File Type: jpg cyl2d.jpg (42.7 KB, 26 views)
File Type: jpg cyl2dw.jpg (42.9 KB, 24 views)
File Type: jpg fluent.jpg (37.4 KB, 19 views)

Last edited by Ralen; May 8, 2012 at 01:33.
Ralen is offline   Reply With Quote

Old   May 8, 2012, 10:02
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
This is a highly unstable flow. If you try to solve with a steady state solver, you will never get the same thing twice, even with the same mesh...

Try solving as transient.
__________________
-----------------------------------------
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   May 8, 2012, 10:56
Default
  #7
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
With a large grid more likely to get the result on the unsteady flow? And then, if the first two cases, the results appear as intermediate steps of unsteady solution, in the third there is no solution.

Last edited by Ralen; May 11, 2012 at 02:11.
Ralen is offline   Reply With Quote

Old   May 10, 2012, 13:43
Default
  #8
New Member
 
ali
Join Date: May 2012
Posts: 5
Rep Power: 4
dearali911 is on a distinguished road
Send a message via Skype™ to dearali911
i m the former gambit user .
i found icem totally different ,, can any body give ma kind of toturials about quadratic meshing
dearali911 is offline   Reply With Quote

Old   May 10, 2012, 15:41
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
ICEM CFD is very different to Gambit, but like gambit, it generates linear mesh.

There is a mesh editing option (add midside nodes) if you want to turn the mesh into quadratic mesh. You can do this with straight sides or you can have the mid side nodes project to the surfaces and curves...

As for tutorials... Check the customer portal. Actually, there are even some built into the help system (already in ICEM CFD), depending on your version.
__________________
-----------------------------------------
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   May 11, 2012, 02:14
Default
  #10
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
Air 10 m/s
Transient at 0.2 s
80 nodes (linear mesh law ~0.001 - 0.00013) Turbo viscosity Under-Relaxation Factor 1 by default
1000 nodes (linear mesh law ~0.0001 - 0.00002) Turbo viscosity Under-Relaxation Factor 0.1 for the convergence of solution.
Attached Images
File Type: jpg cyl2d_80_1000_0020.jpg (45.8 KB, 23 views)

Last edited by Ralen; May 14, 2012 at 07:12.
Ralen is offline   Reply With Quote

Old   May 11, 2012, 03:50
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What type of problem you are experiencing?
Far is offline   Reply With Quote

Old   May 11, 2012, 05:32
Default
  #12
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
Wrap the tube bundle. In the meantime, a very simple task to learn.
Ralen is offline   Reply With Quote

Old   May 11, 2012, 09:00
Default
  #13
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Ralen, that second solution gradient looks a lot like the mesh... Probably not a good sign.
__________________
-----------------------------------------
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   May 11, 2012, 09:32
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Ralen, that second solution gradient looks a lot like the mesh... Probably not a good sign.
Sign of line elements? in other words flow is not going inside
Far is offline   Reply With Quote

Old   May 11, 2012, 09:41
Default
  #15
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
No, I mean that you can clearly see the Ogrid shape around the cylinder in the second picture. If the result gradient flows the mesh that closely, it is usually a sign that your mesh is significantly influencing your results.

You could test this out by adjusting your mesh a little (pull the edges in or out, or adjust the distribution) and you will see a large difference in the result, even with the same solver settings.

Usually, when I see this sort of result gradient jump along a blocked edge, it is due to a jump in mesh size. Using match edges or smoothing the mesh should help.
__________________
-----------------------------------------
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   May 14, 2012, 07:12
Default
  #16
Member
 
Andrey
Join Date: Sep 2011
Location: Russia
Posts: 78
Rep Power: 7
Ralen is on a distinguished road
In previous example with 1000 nodes minimum size is 0.00002. On 1000 nodes (linear mesh law ~0.0001 - 0.00001) I get the same picture.

Then I increased the number of cells in the other direction from 41 to 410. The cell size is 4e-5*1e-5 instead of 4e-4*1e-5.
No errors where there are no small cells.

So in the flow cell is less than 1e-4 m highly undesirable.
Attached Images
File Type: jpg cyl2d_1000_410 0020.jpg (37.1 KB, 12 views)

Last edited by Ralen; May 14, 2012 at 08:20.
Ralen 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
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 06:28
[ICEM] Export ICEM mesh to Gambit / Fluent romekr ANSYS Meshing & Geometry 1 November 26, 2011 13:11
Dimension conflict between icem cfd and fluent highhopes ANSYS Meshing & Geometry 1 September 9, 2011 11:07
prob while exporting icem cfd hexa mesh to fluent mani CFX 4 March 7, 2007 04:41
ICEM Blocking 2D and Fluent error Dr. Flow Squad FLUENT 3 March 5, 2007 03:27


All times are GMT -4. The time now is 14:52.