help with mesh of an i-beam with web holes

[engn555]

Hi, I was wondering if someone could help me to find an easier way to mesh an i-beam with some bolt holes in the web.

Please see the attached document for screen shots for clarification. These are simpler versions of my actual design.

I am trying to mesh a solid model of an i-beam. The solid model is created in workbench, and i am trying to mesh it in Ansys classic (both v10) after importing it as an *.anf file.

I want to use solid185 hex elements because I am trying to verify my model results against some previously published research, and that is the element that the researchers used to create and verify their model against some experimental testing, with fairly good results.
(Rahman et al 2007 AISC Engn Journal 2nd Quarter pg 117).

As I understand the Ansys meshing manual, to mesh a volume with hex elements I must do the volume sweep procedure. What I can't understand is why this will work fine when the web has no holes (fig A), but fails when there is a hole (fig B).

The error message says:
"Volume 2 could not be swept because a source and target area could not
be determined automatically. Try the VSWEEP command again for this
volume and specify a source and target area."

At first I thought that the hole in the web was the problem, but as illustrated in the second set of screen shots, I can sweep mesh the web alone with a hole in it no problem.

The real problem, as far as I can determine, is the the cross section of the i-beam cannot be area meshed (to serve as a source or target for the volumetric sweep operation) when there is a hole present. I have no idea why???? It seems to have no problem meshing the section when there isn't a hole, and it seems to have no problem meshing the web alone with a hole. The problem only seems to appear when I add the flanges to the cross section.

I have got it to work by cutting the model into 3 separate volumes and sweeping each separately. But with this approach the nodes/elements at the web-flange interface do not line up. Will this cause a problem??? Can anyone suggest a method to force these elements to line up at the flange-web interface???

Anyhelp would be greatly appreciated.
Thanks

 

[slumdogengineer]

Sweep meshing requires that your shape is a prism of some sort - so it must be a volume that has identical (or very similar) shaped faces on opposite sides, with no "interruptions" in the middle of the solid (like the hole). This is because it works by area-meshing one of the faces, then sweeping that area pattern through the solid, placing nodes at regular intervals to create hex elements. If you have a hole half-way through, there will places where nodes will occur outside of the solid, so you will get an error message. So in short, you can't sweep-mesh your i-beam with a hole.

Check "7.5.5. Generating a Volume Mesh By Sweeping" for more details.

To mesh this, you will have to divide the volume, either as you have done, then use LESIZE commands to size the meshes so the nodes overlap, then merge with NUMMRG,NODE to get a continuous mesh; or divide into 7 volumes so that at the joining points between volumes they share common areas. This way, ansys will automatically join the meshes.

 

[engn555]

slumdogengineer, thanks for the response.

You are right. I figured out why it meshed the web with the hole (second set of screen shots). It was autodetecting the source and target areas as the flat faces of the web. That way the mesh is swept in line with the axis of the hole "cylinder".

 

[qwicker]

You could also just use Tets.

 

[engn555]

I am trying to avoid using tets because I am trying to compare to a paper that used bricks. I figured enough things could go wrong to cause my results to diverge so I am trying to minimize difference between my and their approach.

I was always told to avoid using tets unless I really had to.

Not really sure if it would really make that much of a difference?