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

[ICEM] Boundary conditions problem in ICEM and Fluent

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

Like Tree4Likes
  • 4 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   December 6, 2011, 03:43
Default Boundary conditions problem in ICEM and Fluent
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Dear all

I am trying to solve the problem of heat transfer from turbine rotor to cooling flow coming from compressor. So inlet is the cooling air and outlet is the air to turbine section. please refer to second Fig.

I have defined the boundary conditions as shown in Fig. 2 and defined them in ICEM BC panel as shown in Fig. 3.

My problem is that we I open this mesh file into fluent I only get the axis, rotor (wall), stator (wall) and stator shroud (wall) boundary conditions in Fluent. I tried many times but I am unable to get the inlet, outlet and rotor shroud boundary conditions in Fluent.

Any suggestion ?
Attached Images
File Type: jpg MESH.JPG (7.7 KB, 120 views)
File Type: jpg BCs.JPG (42.1 KB, 205 views)
File Type: jpg BCs_ICEM.JPG (66.2 KB, 177 views)
File Type: jpg BCs_Fluent.JPG (53.8 KB, 154 views)
Far is offline   Reply With Quote

Old   December 9, 2011, 12:34
Default No line elements in those parts...
  #2
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
Here is my guess...

The Bocos that you setup in ICEM CFD are based on the part names... They don't necessarily require you to have mesh in those parts, but only an entity such as a curve or point. This is so that you can set up the Boundary Conditions even before your mesh is generated. However, the boundary conditions do need to be applied to the mesh during output. If there is no mesh in a particular part, there is nothing to carry the boco out to Fluent.

I am guessing that if you turn off your geometry in ICEM CFD and just try to display your mesh in those parts (inlet and outlet) you won't have any. Optionally, you could try mesh info and see if any elements show in those parts...

If you want mesh in those parts, you will need to ensure that the related edges (I am assuming this is a 2D Hexa blocking) are associated to those curves. Also, if you have an edge that is spanning across parts, you will need to split that edge (or split the block) so that you can associate each edge segment to the correct curve.

Once you have line elements generated in the INLET and OUTLET parts, the output interface will be able to assign the boundary conditions and you will find them in FLUENT.

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   December 9, 2011, 12:48
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Dear Simon thank-you for your help. I have also attached the ICEM files for your reference, meanwhile I am trying your suggestions
Attached Files
File Type: zip rotor_stator.zip (6.2 KB, 41 views)
Far is offline   Reply With Quote

Old   December 12, 2011, 16:23
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
Right, so these files confirmed my theory...


Better than edge splits, i suggest you could just split the whole block, end to end, twice and then associate the middle segment with the inlet/outlet.... The advantage of this method (over edge splits) is that it gives you actual verticies that you can more easily (and precisely) associate to the specific points at the ends of the "openings"...



I should also note, that as your model currently stands, you only have very few elements across the inlet/outlet... make sure to put in at least 9, but probably more. Also the jump between the mesh size on the outlet edge and the mesh size of the adjacent element projected to the wall should be closer if you want to avoid convergence problems, use match edges...
__________________
-----------------------------------------
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   December 16, 2011, 12:30
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Yeah Simon you are 100% correct. Thank-you for your help

I tried all your suggestions and they did the magic. I have got very good convergence and results with V2F, SST , Reynolds stress model and low Reynolds number K-Epsilon models for my heat transfer calculations.

Again I thank-you for your time and help
Far is offline   Reply With Quote

Old   March 11, 2014, 01:32
Default
  #6
Senior Member
 
Crank-Shaft's Avatar
 
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 141
Rep Power: 4
Crank-Shaft is on a distinguished road
Hey Simon and Sijal,

It was interesting reading your comments above since I have a few issues myself with missing BCs in an exported mesh from ICEM.

It is simply a cube which is 200x100x100 (LxHxW) which is simply there to trial various methods of mesh export out to fluent solver. If the 'inlet' and 'outlet' BCs are actually assigned to the respective surfaces and there is clearly mesh on those surfaces (when turning them on and off), doesn't that mean that the BC, surface and the part is properly associated with the mesh?
__________________
--
Mechanical Engineering
Sydney, Australia


Crank-Shaft is offline   Reply With Quote

Old   September 10, 2014, 19:48
Default
  #7
Senior Member
 
Crank-Shaft's Avatar
 
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 141
Rep Power: 4
Crank-Shaft is on a distinguished road
Hello everyone,

I know this is reviving a very old thread, but I believe my concerns and questions are similar to save us starting yet another thread.

I've tried to block and mesh a very simple geometry - A uniform backward facing step - for validation of a turbulence modelling approach that I've been developing.

The first block (130 m long, adjacent to inlet) needs to have an BCSubsonicInlet at the front, then BCSymmetricPlanar at the sides. Both of these seem to be operating fine and is correctly identified in the CGNS output and my solver (
ICEMCurrent.jpg).

However, the top and bottom surfaces needs to have a BCSymmetricPlanar applied prior to the start of the BCViscousWall. In order to replicate the original configuration (backstep_bcs.jpg and backstep_mesh.jpg) I decided not to split the block further at this point and this also helps preserve node distribution. Unfortunately, this also means that the actual surface is only being associated with the mesh and BCViscousWall. The image attached (NotTakingSymmetry.png) is my wall proximity function and this reveals that the entire surface is detected as a BCWallViscous.

The BCSymmetricPlanar and the extended surface isn't being associated with any output mesh (ICEMCurrent.jpg and ICEMCurrent2.jpg). Is there a way to apply this BC without having an additional split in the block?

Thanks in advance for any suggestions you may have.
Attached Images
File Type: jpg ICEMCurrent.jpg (44.2 KB, 14 views)
File Type: jpg ICEMCurrent2.jpg (101.9 KB, 11 views)
File Type: jpg NotTakingSymmetry.jpg (17.2 KB, 11 views)
File Type: jpg backstep_mesh2.jpg (81.2 KB, 17 views)
Attached Files
File Type: zip BackStep.zip (5.7 KB, 0 views)
__________________
--
Mechanical Engineering
Sydney, Australia


Crank-Shaft 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] ICEM CFD boundary conditions conversion to Fluent problem kalyangoparaju ANSYS Meshing & Geometry 0 October 31, 2011 00:40
icem fluent mesh with cyclic boundary condition jiejie OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 April 5, 2011 03:36
[ICEM] ICEM CFD Boundary Conditions not found in Ansys Fluent sammyraj ANSYS Meshing & Geometry 2 April 12, 2010 15:23
Problem in IMPORT of ICEM input file in FLUENT csvirume FLUENT 2 September 9, 2009 01:08
ICEM --> FLUENT, boundary conditions Tobias CFX 1 July 9, 2007 10:35


All times are GMT -4. The time now is 16:10.