CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   2D planar cylinder meshing problem (

saisanthoshm88 November 23, 2010 00:56

2D planar cylinder meshing problem
2 Attachment(s)
Hello every one, I'm a newbie user to ICEM CFD and I have a problem in meshing a 2D planar cylinder. I was making a 2D planar quad mesh in ICEM by a blocking approach to simulate the flow past a 2D cylinder. The attached image shows the block structure.

I wanted to have a denser mesh over the cylinder so as to capture well, the Boundary layer effects. Iíve used the curve mesh set up for the purpose. The first layer height on the circular curve was set to 0.003 mm and the height ratio was 1.1 I didnít apply these settings to any other curves except the circle but when the premesh was computed, I had refinement in many unwanted regions of the mesh as shown in the attached image.

The domain size is: 1000◊500 mm and the circle is of 100 mm diameter.

So please suggest some guidelines to achieve my objective of having a denser (refined) mesh over the cylinder and at the same time avoiding unwanted refinement. I some how suppose that the Bunching laws (or) the curve mesh set up can help but Iím not exactly clear about them. Please provide some clarification.

saisanthoshm88 November 23, 2010 05:16

O-grid solution
2 Attachment(s)
Yep the problem was solved by making an O-grid around the circle. The block topology was indeed made different ( Attached images can throw a better illustration.).

PSYMN November 24, 2010 11:22

Great... If you have need of more wake refinement, you can always wrap that in a CGRID.

And Don't forget you can also move verticies, etc. to get that Ogrid just the size and shape you want.

anno_x December 26, 2010 10:15

Hi, I have the same 2D geometry. I created the same pre mesh with edge params and curve mesh setup. now for the analysis in ANSYS WB I should generate mesh from this pre mesh. my first question is about Pre-mesh smooth. when I click pre mesh smooth, this message appears:
max value can not be less or equal than min value; resetting the histogram min/max values to defaults.
I don't know what is this message concerning about!:confused:
and my second question is about surface mesh generation for 2D analysis in ANSYS WB. I reviewd ANSYS ICEM 2D tutorials but they are not continue after pre mesh. So I couldn't understand how to generate mesh from these pre mesh to export to ansys. I used compute surface mesh but I think the created mesh doesn't follow the pre mesh!!!

I am really sorry for my silly questions, but I am new to ICEM and I am running out of time for this project as a part of my thesis:o

saisanthoshm88 December 26, 2010 10:28

I've never done any meshing in ANSYS WB. But then regarding your second question to export your mesh to ANSYS you need to convert it into an Unstruct mesh.

In ICEM CFD you can do this as:

Model tree-->Blocking--> Pre mesh Right click and select convert to unstruct

I'm sorry that I can't help you to the fullest extent.

anno_x December 26, 2010 11:19

thank you for your quick help santhosh. after I generated unstructured mesh as you mentioned in your post, then I clicked Write Input (in output tab) to save the mesh as cfx5 format,but the following error appeared:
Error: No Volume elements found. child process exited abnormally

So, It would be great if you know what this problem is concerning about?

saisanthoshm88 December 26, 2010 12:35

I suppose that you are working with a 2D mesh and indeed CFX doesn't allow you to export a 2D mesh.CFX always requires a volume (or) 3D mesh.

Fluent supports even the 2D meshes.

However there is a way by which you can probably fix this problem with CFX.
While writing the input file to the solver, set the solver as Fluent.
i.e.., output your mesh file in the Fluent format.

you'll now have a solver input file with the extension .msh Now open this .msh file CFX- Pre

When you do this CFX automatically extrudes the mesh and there should be no problem.

But again while writing the input file to the solver in Fluent format from ICEM CFD dont forget to choose the 2D option in the window that opens up.

Hope this helps you.

anno_x December 26, 2010 16:19

thank you Santhosh.;) the problem is concerning cfx doesn't accept 2D mesh! I saved the file as fluent mesh.
and one other question about importing the mesh to Ansys WB;
in ansys WB, I opened Fluid Flow (cfx) and imported the mesh. although I determined BCs in ICEM before saving the file, when I want to determine boundaries in cfx setup, the parts don't appear to select as wall. inlet and outlet.:confused:

also I need to ask if I want to model FSI, should I change the meshing type?

thanks for you kind help.

anno_x December 27, 2010 02:52

I also extruded my mesh with 1 layer thickness and exported as cfx5 file. but still when I want to select a location for boundaries, non of my ICEM parts appears!

saisanthoshm88 December 27, 2010 08:58

Are you working with the .msh file as suggested

anno_x December 27, 2010 10:31

yes Santosh! As you mentioned, I used msh file format, but when I open it in cfx, no boundary appears to select!

I wonder if you have any time to check the ICEM file as attached. I am really confused!!!


PSYMN December 27, 2010 11:01

check elements are in the boco parts.
The boundary condition names are based on the parts the elements are in in ICEM CFD. If your geometry curves have those part names (such as INLET), but you did not associate the blocking to the curves, the line elements will not form around the shells and your boundary conditions will not be associated with any elements...

To check this, please go back to your unstructured mesh in ICEM CFD... Go to Info => Mesh info, and see if it lists elements in those parts (such as INLET). You could also turn off all the parts except Inlet and see if any line elements are displayed on the screen (make sure to turn on display for mesh=>Lines).

If you don't have the elements in the parts, that totally explains your problem.

Go back to Hexa, associate edges with curves (even straight ones that already seem aligned. Generate a new premesh, convert to a new unstructured 2D mesh, output in fluent format and then read that into CFX-Pre (which should automatically extrude it to 2.5D).

Best regards,


PSYMN December 27, 2010 11:08

About the Premesh smooth error...

Try to get a newer version and maybe convert to premesh and use the Edit Mesh => Orthogonality Smoother instead.

anno_x December 27, 2010 11:18

Thanks for the reply Simon, I checked the parts as you instructed. But I guess only closed shape parts eg. circles export to .msh format. Inlet is a line part, but
it can't be exported to fluent as BC

saisanthoshm88 December 27, 2010 11:41

There is nothing like only closed shapes get exported as Boundaries. Just try the steps suggested by Simon i.e.., make proper associations and then try outputting in fluent format. I suppose you should be able to fix the problem.

anno_x December 27, 2010 12:14

I did every step Simon mentioned above! but the problem was concerned about splitting the block. when I created the first 2D block, I associated it to box BCs. but I didn't know after splitting the block, again edges of newly constructed blocks should be associated to the box!
Now everything seems to be alright! now it's the time for cfx Analysis!!!:D

Thanks again Simon and Santhosh for really useful helps

All times are GMT -4. The time now is 18:05.