Learning Forum

[emirdegirmenli]

I am trying to get modal analysis results of a plate which has different thickness region. for example, the thickness is 2 mm at center and 1,4 mm at edges. Thus I sketched different surface and I gave different thickness value on mechanical. All contacts are bounded but they move separately. Actually, later I will need to do this for complicated plate such as violin top plate. 

Best,

Emir

 

[peteroznewman]

Hello Emir,

You want to go into DesignModeler where it will show 4 Parts, 4 Bodies.
Select all four parts, right click and select Form New Part, then it will say 1 Part, 4 Bodies.
The 4 bodies can still have 4 different thickness values.
In Mechanical, Update Geometry from Source, then delete all your contacts, since the mesh will connect these 4 bodies with common nodes at the common edges. This is called Share Topology in DM and this is much better than using contact.

The reason the parts were not connected in your original model is the pinball radius was not large enough to detect the adjacent nodes. Increasing the pinball radius will solve that problem, assuming you have mesh controls to actually create coincident nodes. But you really want the solution in the first paragraph.

Cheers, Peter

 

[emirdegirmenli]

Dear Peter, I use SpaceClaim and I found 'Share Topology' from properties and only click 'share'. Thank you very much again, best

Emir 

[peteroznewman]

There is another method to replace Contact elements and that is the Mesh Connection Group.

Here is what you have, where the red edges mean that is the edge of a body.

After Insert Mesh Connection Group, Detect Connections and Generate, you get a connected mesh.