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

Need help icem cfd

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 30, 2010, 13:29
Default Need help icem cfd multiphase 2d mesh
  #1
New Member
 
Join Date: Dec 2009
Posts: 6
Rep Power: 7
kakhtar is on a distinguished road
Hi every body
I need help in ICEM CFD.
I am trying to simulate a 2D multiphase flow in Fluent and CFX.
I am using icem cfd .CFX had some problem with 2d mesh. So I switched to fluent. Fluent was working well for single phase but not for multiphase. I have some problem for multiphase flow. First let me describe the geometry. I have a 2d rectagnle one end is inlet of one phase of fluid i.e. air. other end of rectangle opens in a another rectangle having another fluid (phase 2 ) i.e. water. The second end of this rectangle having water openes in a third rectangle having again first phase ( air). The second end of this recgale is outlet for phase 1 ie air.
I meshed the geometry in ICEM CFD. when I import in fluent. It does not recognise as separate regions.Infact I am unable to initialze only air in first region water in second and air in third. In gambit we were doing this problem be defining three face one for each region. Here I donít know how to define a face like gambit which fluent will recognise as a separete region.

I will realy appreciate your help

Last edited by kakhtar; January 30, 2010 at 16:24.
kakhtar is offline   Reply With Quote

Old   January 31, 2010, 06:08
Default
  #2
Senior Member
 
feizaghaee's Avatar
 
moein
Join Date: Dec 2009
Posts: 132
Rep Power: 7
feizaghaee is on a distinguished road
Send a message via Yahoo to feizaghaee
what kind of problem do you have with CFX?
feizaghaee is offline   Reply With Quote

Old   January 31, 2010, 13:20
Default
  #3
New Member
 
Join Date: Dec 2009
Posts: 6
Rep Power: 7
kakhtar is on a distinguished road
@feizaghaee: When I import mesh into CFX. The message appears that cfx is unable to import mesh. No region has been found. I used to import mesh in CFX from gambit. It was 2D mesh. CFX automatically gave width in 3rd direction. The only step I am missing in ICEM from that of gambit is that in gambit I used to define faces by selecting edges. Then I meshed the face. Here I don't know how I can define a face. In Icem I creat geometry from curves. Associate a block with it. Mesh edges of block. Updates the mesh and then from out put convert into unstructured grid. I dont how to define face. But I can open the mesh in fluent. Now I need three different regions. Fluent take it as a one region. So if I define one fluid type in one zone it automatically assinge the to other zone. In gambit it would be simpliy defined as three faces. So I am stuck
kakhtar is offline   Reply With Quote

Old   February 3, 2010, 10:44
Default
  #4
mic
New Member
 
Join Date: Mar 2009
Location: Milan, Italy
Posts: 12
Rep Power: 8
mic is on a distinguished road
In CFX you can't import 2D mesh from ICEM. You have to generate the 3D volume mesh in Icem and than export to CFX.
Regarding the export from Icem to Fluent (I don't have experience with Fluent, only with Icem!), if I understand the problem, you have to define each boundary (inlet, outlet, etc), as a different part in ICEM (Part, RMB, Create new part) BEFORE meshing your geometry.
Hope this helps
fedefrance likes this.
mic is offline   Reply With Quote

Old   February 3, 2010, 12:40
Default
  #5
New Member
 
Join Date: Dec 2009
Posts: 6
Rep Power: 7
kakhtar is on a distinguished road
@mic: thanks mic. I got how to export 2D icem mesh into cfx. If u save the mesh in .mesh not .cfx. than. then in cfx pre select fluent for importing the mesh file. Lets see is it recoginse the surfaces as different parts.
kakhtar is offline   Reply With Quote

Old   February 3, 2010, 14:19
Default
  #6
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
Mic has the right idea...

CFX doesn't support 2D solve. But it does support 2.5D solve. Just take your 2D mesh and extrude it by 1 element in the Z direction... Then CFX can handle it.

As for the bocos for Fluent or any other solver... While most ICEM CFD users do create the parts (Inlet, Outlet, etc.) before meshing (easiest), if you already have your mesh, you can still do it after. In the end, it is the part name of the shell elements that matter. you can assign the elements to a new part name at the mesh level or you can change the geometry under the elements and use the option to change the mesh part based on the underlying geometry. This is similar to running flood fill for changing the volume part mesh.
PSYMN is offline   Reply With Quote

Old   February 4, 2010, 17:39
Default
  #7
Senior Member
 
feizaghaee's Avatar
 
moein
Join Date: Dec 2009
Posts: 132
Rep Power: 7
feizaghaee is on a distinguished road
Send a message via Yahoo to feizaghaee
cfx 12.0 support 2D problems
feizaghaee is offline   Reply With Quote

Old   February 5, 2010, 01:02
Default 12.0...
  #8
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
Oh, I hadn't heard that yet (about CFX 12.0 supporting 2D). Thanks for the update.

Simon
PSYMN is offline   Reply With Quote

Old   February 5, 2010, 09:31
Default
  #9
New Member
 
Join Date: Apr 2009
Posts: 14
Rep Power: 8
longbow is on a distinguished road
No. CFX 12 does not support 2D problem. It still treats 2D problem in the way described by PSYMN early.
longbow is offline   Reply With Quote

Old   February 8, 2010, 13:31
Default I asked...
  #10
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
I asked CFX support and was told that this was not a 2D solver in CFX, but rather " What is new (in v121 ) is that one could import a Fluent 2D mesh and CFX-Pre would automagically extrude the shells into volume elements."

So from a meshing point of view, I guess that is similar to 2D support and will surely be appreciated by users who can save a step on the meshing prep side...
PSYMN is offline   Reply With Quote

Old   February 8, 2010, 17:50
Default
  #11
New Member
 
Join Date: Dec 2009
Posts: 6
Rep Power: 7
kakhtar is on a distinguished road
Dear PSYMN,

Thank you very much. I also read that post. I am doing the same and its true also. CFX support 2D, mean 2D mesh from .mesh extension can be imported in CFX.
Now I am stuck in my original problem. I don't how to create multiple parts. I am trying different ways.
1) when I complete mesh ( geometry explained above) I right click on parts ( windows tree) select create new then selection I create the different mesh.
In CFX I have different regions but interface i.e. the boundary conditions is giving me a problem. Also when I import in fluent the mesh check fails with warning that the interface one zone is dettached from zon other ( some think like ). whis worries me.
kakhtar is offline   Reply With Quote

Old   February 8, 2010, 17:59
Default setup...
  #12
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
If generating in ICEM CFD, the mesh takes on the names of its underlying geometry. When in 2D, it is important for most solvers (including CFX) that the surfaces represent the materials (fluids) and the the curves and points represent the bocos (inlet, walls, outlet, etc.) and that these names are not shared. For instance, if your surface is in the "fluid" part, you don't want any curves or points in that part. Rather they should be in parts named "inlet", "outlet", etc. for easy setting of bocos. If you have multiple material regions, you would name the surface parts differently, "FLUID1", "POROUSMEDIA", "SOLID", etc.

Connectivity is also important. If you have two surfaces separated by a curve, it is important that the curve is shared by both surfaces. The Geometry => Repair Geometry => Build diagnostic topology option will take care of this for you. You enter a tolerance and it does the rest. You can even filter out curves between surfaces bases on angle.
PSYMN is offline   Reply With Quote

Old   February 8, 2010, 18:52
Default With Pics..
  #13
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
And here are some pics...

I started by putting each surface in a part (FLUID1, FLUID2, FLUID3). Then I put the INLET, OUTLET, INTERIOR and WALL curves into their respective Parts. FInally, I put all the POINTS into the WALL Part (I could have put them into their own part).

Next I ran the Diagnostic topology to make sure that everything was connected. Here, with color by count on, you can see that "double" curves (curves between two surfaces) are red. All the interior curves are red. Single edge curves are yellow. (Yes, I know this color convention seems odd to many.)

Next I generated a coarse uniform mesh (no fancy inflation or anything).

Then I setup BOCOS for Fluent. The Surfaces "Mixed/Unknown" are surface elements that are not against or between volume elements. The line elements are all in their own parts except for WALL which is mixed/unknown because it contains points.
Attached Images
File Type: jpg Kakhtar_01.jpg (26.5 KB, 157 views)
File Type: jpg Kakhtar_02.jpg (26.2 KB, 117 views)
File Type: jpg Kakhtar_03.jpg (39.9 KB, 107 views)
File Type: jpg Kakhtar_04.jpg (52.7 KB, 118 views)
PSYMN is offline   Reply With Quote

Old   February 8, 2010, 18:57
Default And some more pics...
  #14
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
And then I output it to Fluent as a 2D mesh (apparently this is also how to get a 2D mesh to CFX).

In Fluent, I see all my Bocos (plus it breaks out some extra bocos like "walls:001", which are the walls next to the middle fluid.)

I setup the Fluid2 region as water, set the inlet velocity to 100 m/s and ran the case to show it all worked.

Simon
Attached Images
File Type: gif Kakhtar_05.gif (9.1 KB, 78 views)
File Type: jpg Kakhtar_06.jpg (47.4 KB, 81 views)
File Type: jpg Kakhtar_07.jpg (49.8 KB, 68 views)
File Type: jpg Kakhtar_08.jpg (69.3 KB, 87 views)
PSYMN is offline   Reply With Quote

Old   February 9, 2010, 18:40
Default
  #15
Member
 
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8
triple_r is on a distinguished road
Thanks a lot Simon for these two great posts. I am new in ICEM CFD and I really appreciated your posts.
triple_r is offline   Reply With Quote

Old   February 15, 2010, 09:10
Default question
  #16
New Member
 
zeid
Join Date: Feb 2010
Posts: 2
Rep Power: 0
zeid82 is on a distinguished road
I have prblem about how can i mesh domain consist of rectangle in side him object(rectangle)snaller than first one by use unstructured mesh,so please help me how can make it step
zeid82 is offline   Reply With Quote

Old   February 15, 2010, 10:13
Default Material Points.
  #17
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
Do you mean two nested rectangles? Like the yoke in an egg?

ICEM CFD uses the concept of material points or "bodies". These are the 4th icon in the geometry tab.

Just create a material point in each region of interest (such as between the rectangles) and you will get mesh in that region.

Simon
PSYMN is offline   Reply With Quote

Old   February 15, 2010, 12:34
Default
  #18
New Member
 
zeid
Join Date: Feb 2010
Posts: 2
Rep Power: 0
zeid82 is on a distinguished road
I have prblem about how can i mesh domain consist of rectangle represent a tube in side him object(rectangle)smaller than first one by use unstructured mesh,so please help me how can make it step
zeid82 is offline   Reply With Quote

Old   February 15, 2010, 15:04
Default Sure...
  #19
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
I thought I did help But I guess I don't really understand your problem at this point. Probably just a language barrier.

If you want to attach a tetin file, I am happy to look at it and send you instructions.

Simon
PSYMN is offline   Reply With Quote

Old   February 16, 2010, 18:24
Default
  #20
New Member
 
Join Date: Dec 2009
Posts: 6
Rep Power: 7
kakhtar is on a distinguished road
Thak you very much PSYMN: Sorry I was off for few days. I followed your steps creat a mesh in icem. It worked.

Thankyou so much
kakhtar 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 CFD Scripts Vinod Dhiman Main CFD Forum 2 February 17, 2010 11:56
Help for ICEM CFD - urgent Tuks CFX 3 February 8, 2010 04:32
ICEM CFD to CFX geometry and mesh Luca CFX 6 February 4, 2010 17:31
How about ICEM CFD M.Gao Main CFD Forum 1 November 15, 1999 05:15
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 16:21.