CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Black and unconnected edges problem (

Santos-Dumont February 14, 2012 06:39

Black and unconnected edges problem
Hi there,

I'm a beginner in ICEM. I'm trying to mesh my first complex geometry using quad elements in 2D.
I made the blocking and the mesh result is fine, though I could make some improvements out of it.

It was long and painful to get to that result but I think I learned a lot.
Still, It's very frustrating because I can't test it with Fluent. I had an error "Warning : Mesh has uncovered faces" when exporting to Fluent. I fixex it with the mesh check and repair option but I was not sure that it was a clear job. I once succeed to put it into Fluent but I had a boundary with two edges in the middle of my FLUID Part. These two edges are the edges that are black on my blocks.

During my block creation history, I had to remove two blocks and make some manoeuvers to get to that result. I'm unsure that it was the best strategy, but still what's done is done. Is there now a way to make these edges blue. I have the feeling that ICEM doesn't count them as part of the blocking and that seems to be the source of my problem.

Do I have a solution or do I have to start over ?

Also, the best solution for me would be to merge the three blocks between the two black edges into one single block. That would help meshing but I didn't succeed in doing that, is that possible to merge the three edges on the geometry and make one single block ?

Thanks for your time

energy382 February 14, 2012 08:15

blocking -> merge verticies by number -> 2 verticies

First vertix you choose is the vertix who remains. In your case, you have to choose the verticies of the two black edges first and then the verticies between the black edges (one after the other)

Santos-Dumont February 14, 2012 10:22

Thanks energy for your advice.
I successfully merged these two blocks, redone association of the edge with the 3 curves below, and I now have a nice mesh !

But still, the exportation still doesn't work... When exporting I get a lot of message like this one : " Error : face (near node 51537) is attached to more than 2 cells."
I read that it is due of overlapping elements. So I tried to check the quality mesh and I have some overlapping problems. None of the repair trials have worked so far.

With a very close loop, I found these very ugly things on the previously black edge

That's my problem for sure !
I think it's a common problem, what did I do wrong ?


energy382 February 14, 2012 12:52

looks like there are some association failure. try rmb blocking -> faces -> face projection and check it.

by default, faces were projected to clostest surface. you can also project them manually: blocking -> associate -> face to surface -> and then part or selected surface

Santos-Dumont February 14, 2012 13:54

I tried to associate the faces to the fluid surface, it worked. Still I have the same number of overlapping elements.

I noticed something strange when I print the blocks faces. There is two extra edges. Still, I have only 5 faces so these two edges dont belong to any faces. That is surely my problem.

That's annoying not to be able to merge of remove things as easily as it was with Gambit...

energy382 February 15, 2012 11:35

Hey Charles,

please provide .tin .blk and .uns file

PSYMN February 15, 2012 15:07

I am not sure what rabbit hole you headed down. The black edges are "surface projected" edges that naturally happen at the boundary of a blocking. If you want to start over, this could be done properly in very few clicks if you started with a half OGrid...

Here are the steps to recreate this model properly (you can decide if it is easier to go back or press on).

1) Initialize blocking with no selections. This will give you a big block for the whole domain.

2) Associate the top and sides with the appropriate curves. (easier to do this now while you have no splits).

3) Use the Ogrid tool. Select the block and the bottom edge. This will give you a half OGrid.

4) Slide the vertices of the central block of the Cgrid over to your object. (can't slide like that in gambit). Position the corners appropriately.

5) Delete the central block... (don't check the delete permanently button)

6) Associate the remaining edges correctly.

7) Set sizes and generate the premesh...

8) you had a 4 extra splits on the top of your model. You didn't need them for your topology, but you can decide if you want them (after looking at your premesh). If so, create them with block splits. You probably just created them so it would look like the mesh was following these edges, don't worry, it will. You can adjust the display by right clicking on edges if you don't like the straight edge display.

9) Done in less than 10 minutes. You can try the smoother if you want.

Santos-Dumont February 15, 2012 18:51

Thank you all for your help, I made good progress, started over and my mesh is now under calculation in Fluent. I used the merge vertices method that energy gave me but I also did a quick test with the PSYMN, OGrid method and that was quite good too, I begin to understand the point of Ogril.

Even with more that 250 000 nodes of Quad Elements I'm still unsatisfied with the results I get with Fluent. Even with a Reynolds of more that 2 million the flow is not unsteady enough to me. It may be due of the fact that it is transonic, but that problem is now about Fluent more than ICEM.

Thanks again for your help

All times are GMT -4. The time now is 10:07.