CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   Export 2D mesh from ICEM to Fluent (

enghamed July 28, 2010 23:47

Export 2D mesh from ICEM to Fluent
How can I export a 2d mesh from ICEM to Fluent?

I created a simple rectangle(1*1) from nodes and lines then made a surface of it. I created a part for each edge. then made a blocking and defined the nodes on the blocking edge. gone to pre-mesh and then file->mesh->load mesh from blocking.
then saved the goemetry, blocking and mesh.
went to output tab selected fluent and then created a B.C for each edge.
Then I clicked on write input. opened the mesh file and saved the file.
In fluent when i try to open it gives an error "file has wrong dimension"

Am I doing something wrong?

thanks for your help

Oxmox July 29, 2010 05:45

Same happened to me... have to declare the geometry 2-dimensional in workbench.
Just right-click on 'geometry', select properties and set the analysis type to 2D, at least that worked for me...
hope it helps...

enghamed July 29, 2010 06:41

I want to use fluent seperatly and not from workbench.
But yes in the start I click on 2D.

PSYMN July 29, 2010 09:30

It should work without a problem...
Did you use 2D blocking?

Is your model in the XY plane (Z = 0)?

Do you have quad 4 elements? (not hexas)

JOKER August 3, 2010 15:55

I think this is the best thread to start with..!

I m a beginner in CFD and also new ANSYS 11 ICEM user and i follow 2D car tutorial, find it really difficult what is ICEM's "top to bottom appoach" as i have used GRIDGEN little bit. Anybody suggest me how to "Think Like ICEM".

About CAR example; it is a hexa (2D quad.) meshing ..? I want to run it on Fluent 6.1.22 but in OUTPUT tab only option is FLUENT V6 (only support unstructured meshing). Is it possible to run this 2D CAR mesh on Fluent 6.1.22

PSYMN August 3, 2010 22:35

In ICEM CFD you think like a sculptor rather than a brick layer. You split blocks and delete the bits you don't need.

Imagine if you needed to have 8 blocks in the end... In ICEM CFD, you would start with the large block and split it three times (once across each direction) to get 8 blocks. That is three quick operations to get 8 blocks. It would take many more operations to build those from the bottom up. This argument only gets better as the blocking gets more complicated.

Imagine a pipe that you want an Ogrid in. In ICEM CFD, you start with the single block and you split it (one quick operation ) into 5 with the Ogrid tool. It would take a lot more time to build that bottom up. Again, as your model gets more and more complicated, Ogrid still only takes a single operation, but could create hundreds or thousands of blocks. The advantage of top down grows.

Also, ICEM CFD hexa can grow bottom up where ever that is helpful. You can create blocks, extrude faces into new blocks, etc.

For ICEM CFD hexa, there are really only 5 steps, I have covered these in other posts. (search for "only 5 steps"). They will help you "think ICEM"

Our Fluent6 output supports all the Fluent 6 versions including Fluent 6.1.22. Yes, that is an unstructured format, but that is fine for Fluent. Just to be clear, unstructured is just about how the nodes are stored (xyz not ijk), Hexa or Quad can be structured or unstructured.

If you want a structured format, you could output your multiblock mesh domains in Plot3D or CGNS format.

JOKER August 4, 2010 03:07


But I am not clear about "Storing nodes in unstructured format". What is advantage of this feature and who it works.

About Fluent V6. Did u mean setting output solver for 2D CAR example to V6 makes it 6.1.22 compatible? How I follows the steps !

JOKER August 7, 2010 12:14

Hy Guys!
I need your suggestion please.
I tried to follow ICEM tutorial: wing body. But after blocking and setting meshing parameters (suggusted) when i compute mesh message alert came: memory requirement fails for WIN32 system (don't remember exact words)

I have core i7 with 4G RAM i hope that is enough for tutorial at least!

PSYMN August 7, 2010 14:34

Sizes or bunching are too fine...
Hey Joker, why so serious?

I am sure you have enough memory for the tutorial, but you may have gone and put way too many elements on your blocking...

Check the bunching (right click option on edges in the model tree). If you set your sizes a few orders of magnitude too small, you would quickly go from a basic tutorial with a hundred thousand elements to a basic tutorial with a hundred billion elements and that would cause a memory problem.

You could also right click on surfaces and turn on hexa sizes to get an idea of the sizes set on your geometry.

JOKER August 12, 2010 09:24

Hy Again!

Thanks SIMON i got it. Previously i m not setting bunching parameters, it was not mentioned in tutorials then i got 2D airfoil tutorial on YouTube it has explained every thing...!

JOKER August 14, 2010 15:02

5 Attachment(s)
Hy Everyone..!

I m currently understanding 2D topology generation. So, i draw an aircraft curves and O-split a CH type domain and then further split to fit geometry. but there are some issue on which i seek help.
First I think O-Split i made it too early because during block splitting i hardly understand what is going on.

JOKER August 14, 2010 15:16

I have also used bunching option with bi-geometric Law but spacing is not in my control. If it is all about nodal spacing how to choose a perfect mesh law

PSYMN August 15, 2010 17:29

I am not sure what you mean by "spacing is not in your control". What happens if you try to adjust the edge distribution? Is it because you did something like linked the end spacing to something else, or perhaps because you are using a multigrid level and it is just adjusting the count to stay consistent?

The biggest problem I see from your pics is that the first few rows of elements above the fuselage seem to collapse into the tail... I am not sure why that should happen for you since there don't appear to be any splits...

I would look at that one edge very carefully.

From what you have shown, I don't know what the matter is. What other info can you give me?

piece_wood June 7, 2013 05:57

I really have a problem to generate a 2D mesh in ICEM. My Problem is 2D axis-symmetric.
It doesn't matter if I import the geometry from DM or if I create the points and curves in ICEM. When I import it to FLUENT (in workbench) it always wants to open the 3D solver. If I load the mesh directly, FLUENT says that it has wrong dimension.

Did you use 2D blocking?
I used 2D blocking planar, like in the 2D pipe junction tutorial

Is your model in the XY plane (Z = 0)?
my model is in the XY plane and at Info>Mesh Area/Volume I get: total volume is 0.0

Do you have quad 4 elements? (not hexas)
My generated mesh consists only of quads. At least this is written in tree.

But if I do a blocking info, it appears that I have a third dimension:
-- Blocking Info ---
Number of blocks:
All blocks: 28
Mapped blocks: 28
Current project directory: U:/Ansys/vordere_Brennkammer_files/dp0/ICM/ICEMCFD
Visible images:
min: -0.0359556 -0.0359556 -0.090121
max: 132.536 18.536 0.090121
Data objects:
min: -0.0359556 -0.0359556 -0.090121
max: 132.536 18.536 0.090121
Note: maximum number of processors is 6

On the other hand, In the family boundary condition window, there are no volumes.

Does anybody have an idea what I'm doing wrong? I'm really desperate :-(

RodriguezFatz June 7, 2013 06:44

When you export the mesh in ICEM do you choose "2d" in the window where you promt the name of the .msh file?

piece_wood June 7, 2013 07:16


Originally Posted by RodriguezFatz (Post 432622)
When you export the mesh in ICEM do you choose "2d" in the window where you promt the name of the .msh file?

I already used this button...but anyway, I exported it another time and it is working now, with the geometry that was generated in ICEM. Thank you for helping!

It is still not working within workbench. Am I the only one who has problem with ICEM to FLUENT in workbench (2d problem)?

RodriguezFatz June 7, 2013 07:23

Don't use workbench... ;)
Maybe in DM, you unintentionally created a 3d file? Go to workbench -> your DM - file and click on it. All settings will be shown in workbench. Also whether it is a 2d or a 3d geometry.

PSYMN June 7, 2013 14:36

Yea, Rodriguez is probably on to something... WB keeps track of things like 3D vs 2D... There is probably a way to sort it out, but I don't have time right now.

orangesky August 10, 2015 20:49

I also had this problem recently trying to convert my 2D Geometry from Design Modeler to ICEM and FLUENT.

Whenever I tried converting it directly from ICEM to FLUENT in Workbench by linking, FLUENT would only recognize it as 3D (and disable the 2D option). Even though it would correctly recognize it as 2D if put through the ANSYS mesher.

I got around it by going to the 'Output' tab and exporting the mesh with the 2D option selected and manually importing that file on FLUENT (in case this should help anyone who encounters the same problem). Not sure why FLUENT can't recognize a 2D mesh from ICEM automatically.

All times are GMT -4. The time now is 22:03.