CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] [Student] Problem: Nodes Merging (

FALCON_SR71 March 11, 2010 12:57

[Student] Problem: Nodes Merging
2 Attachment(s)

Iím an engineer student and I have to study the heat transfer on a fin. But I encounter a problem in the mesh assembly between the mesh of the flow part and the mesh of the solid part.

The case:

Schematic draw of the case
Picture (geo2)

The mesh of the fluid is made by the blocking method and it is converted in an unstructured format. Itís the first body part.

The mesh of the fin is obtained by the same way but for the solid part.


The mesh of this picture is not the real one but the main idea.

During this step, I have tried to have the same node distribution on the commons face for improving the nodes merging.

I tried a lot of solution unsuccessfully, the different ways are:

First one: Applying the merging nodes methods with tolerance on the common surface. The merging seems too be good, but when I check the mesh quality, multiple edge subsets need to be created. This problem cause invalid cell for Fluent.

I see in the help topic that the problem comes from:

Multiple edges
Refers to elements with at least one edge shared among three or more elements. Legitimate multiple edges would be found at a "T" junction, where more than two geometry surfaces meet

The second one: the merge mesh method creating tetra cell for the connection. But the same problem occurs and I will prefer having only a hexa mesh.

What are the different solutions to resolve the problem?

Thanks for your reply and your help.

rikio March 11, 2010 21:58

You could ignore this Multiple Edges error messages, set the proper BC would be OK to import into Fluent.
Make sure that you set BCs in the Output tab.
Wish it helpful.

FALCON_SR71 March 12, 2010 04:25

Thanks for your reply,

But I already tried to launch Fluent.

I define different parts for the different surfaces, and I use them to define the boundary conditions to export the mesh to Fluent.

May be I miss a step?

The problem is that when I display the results like the temperature. The core of the solid part and the center of the surface are good. But I encounter problem in some nodes (like the two nodes in front in the upper face of thefin) and some part of the edges.

When I import the mesh in fluent, the mesh is auto partitioned in different parts:

Wall -> Wall (28) and wall: 002(2)
Note: Separating wall zone 28 into zones 28 and 2.

Than for a surface like Wall, I have different surfaces appearing like:


Thanks for your help.

PSYMN March 12, 2010 15:02

Do it all at once...
Rikio is right that multiple edges are not generally a problem, but you shouldn't have any multiple edges in this model, so if you are seeing them, they may be a problem...

Going up a little higher in your description... Are you blocking this as one blockng with two materials (preferred method) or are you blocking this as two separate blockings and then trying to merge the unstructured meshes together? (much more work for you and may lead to problems if you miss something).

Block it again, but instead of deleting the blocks in the fin, right click on parts and "Create a new Part". In the Create Part DEZ, the last icon is for creating blocking material... type in a new name (like FIN_SOLID) and put the fin blocks in there instead. Then setup you mesh params. Everything will naturally remain consistent and matched but you will need to match edges to get a smooth volume transition.

I recommend you also create an ogrid around and possibly even inside your fin for the most efficient way to capture the boundary layer and thermal gradients normal to the surface...

Have fun.

PSYMN March 12, 2010 15:09

Multiple edges around where the fin meets the floor.
Sorry, I guess you would have multiple edges where the fin meets the floor... Those should be expected and will not be the problem...


FALCON_SR71 March 13, 2010 05:12

I going to try the solution on the case and will come back to inform you in a few days.

Tanks for your help

FALCON_SR71 March 18, 2010 06:47

3 Attachment(s)

I tried your solution on a test case: Making one main block and associating the fin and the fluid parts to a part subset.

(Figure: geo)

But now, I have another problem. Indeed, the mesh seems to be good. But when I start the simulation on Fluent, there are no interaction between the fin and the flow (when I draw the temperature field, they is no wake).

Remark: The velocity field around the fin seems to be good.

The case is:
  • I define the fin like a wall (with the default condition temperature: Coupled)
  • I define the base of the material support of the fin like a wall with a temperature of 500K (I already tried heat flow).
The inlet and outlet surfaces are defined by a temperature of 300K
The Perfect gas law, the energy and k-epsilon model is active

You can see the problem on the picture Tt and Ts.

Tanks for your help

PSYMN March 18, 2010 20:33

I wouldn't say there was no wake... I can see some flow disturbance... I can even see that the leading edge is being cooled slightly... It just doesn't look like much heat is transferring to the flow...

Assuming your bocos and material properties are all good and that this is a meshing problem (just an assumption) what sort of boundary layer resolution do you have? Is your wake region refined enough to capture what it should?

Maybe post an image of the cutplane across the mesh.

Generally for capturing viscous effects or heat transfer, you will want a larger number of nodes perpendicular to the wall with a very small intial height... An ogrid usually does the trick (and will here also).

If your mesh looks fine and we were going to look at bocos next, First thing I would ask is if you have a "no slip" condition at the wall...


FALCON_SR71 March 21, 2010 06:47


I compared the simulation results with the experimental ones and it seems to be good. Indeed the temperature of the fluid increased about 30 K and its velocity is 70m/s. At first the figures seemed me very low but after analyzing them deeper the scale order is right.

The real case is working now.

Thanks for your help.

All times are GMT -4. The time now is 13:03.