CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   Need help icem cfd (

kakhtar January 30, 2010 13:29

Need help icem cfd multiphase 2d mesh
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

feizaghaee January 31, 2010 06:08

what kind of problem do you have with CFX?

kakhtar January 31, 2010 13:20

@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

mic February 3, 2010 10:44

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

kakhtar February 3, 2010 12:40

@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.

PSYMN February 3, 2010 14:19

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.

feizaghaee February 4, 2010 17:39

cfx 12.0 support 2D problems

PSYMN February 5, 2010 01:02

Oh, I hadn't heard that yet (about CFX 12.0 supporting 2D). Thanks for the update.


longbow February 5, 2010 09:31

No. CFX 12 does not support 2D problem. It still treats 2D problem in the way described by PSYMN early.

PSYMN February 8, 2010 13:31

I asked...
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...

kakhtar February 8, 2010 17:50


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.

PSYMN February 8, 2010 17:59

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 February 8, 2010 18:52

With Pics..
4 Attachment(s)
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.

PSYMN February 8, 2010 18:57

And some more pics...
4 Attachment(s)
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.


triple_r February 9, 2010 18:40

Thanks a lot Simon for these two great posts. I am new in ICEM CFD and I really appreciated your posts. :)

zeid82 February 15, 2010 09:10

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

PSYMN February 15, 2010 10:13

Material Points.
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.


zeid82 February 15, 2010 12:34

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

PSYMN February 15, 2010 15:04

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.


kakhtar February 16, 2010 18:24

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

All times are GMT -4. The time now is 16:45.