Problems with Shell command - Please Help !
The problem's probably down to the 0.1 fillets, you should try and shell before adding small fillets.
It does shell with a 0.05 offset but guess you want more than that. PS this would be simple to fix if you'd used history.
Mark
Mark Hughes
Owner, Hughes Tooling
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After removing all the 0.1mm external radii I can shell at 0.5mm, the next smallest radii in the design.
Mark
Mark Hughes
Owner, Hughes Tooling
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Sorry can't help with a form, never use them. What was wrong with the first part you attached? all you need to do is select each chain of radii and delete, shell then reapply the external radii.
You only need to delete the convex radii. See attached file with timeline, just step along the timeline to see what I did.
Mark Hughes
Owner, Hughes Tooling
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@Monodon - I really don't think that the Form environment is the right one for this design. This design seems to have lots of planar and cylindrical faces on it and Form is not good for that kind of analytic geometry. Personally, I would take @HughesTooling 's advice, and remove the small fillets, do the shell, then re-apply the small fillets after the shell.
As to the problems in the form, the tool shows you where the intersecting faces are if you click on the error:
One thing to be aware of: The offset capability in Form is much different than the solid shell. It works by creating an offset control frame network, then re-fitting a TSpline surface over that network. Uniform thickness is not guaranteed, and for small offsets, it will often result in these exact kinds of intersecting faces.
Also, as Mark says: Use history, it is much easier to fix up problems when they happen if you can go back and edit features.
Jeff Strater
Engineering Director
@Monodon wrote:
... So I took different approach.
Yes, but that did not work because you don't actually appear to understand what the problem is.
Sketch an arc ay 90 degrees with a radius of 2mm.
Try to offset the arc 3mm toward the inside or center of the arc. What is the geometry going to look like?
That is what you are asking Fusion 360 to do. In some circumstances, the resulting "bowtie" geometry is removed automatically and that results in a sharp edge, but the fillets on this model don't lend themselves to this.
So you either follow @HughesTooling's advise, or you need to re-think yot approach to geometry.
In a design without design history, this is very labor-intensive and somewhat error-prone. Thus my recommendation to work with the timeline enabled.
