Tangent entities from Intersection...aren't...

matt_zerega

I may have stumbled on a bug. The scenario: a Plane ("Lens Bevel Plane") intersects a Part ("Lens"). I want the inner series of tangent lines and arcs, that define the interface between the shelled surface and intersecting Plane, to define one side of an extruded lip on my Lens. While in a Sketch on the Plane, I use the Intersection tool to select the narrow face shown below; two adjacent sets of lines and arcs appear defining where the shelled Part intersects the Plane. Great, so far...  Then, I select the inner set of contiguous lines and arcs that represents the inner surface of my "Lens" Part, and I use the Offset tool to create a second set of contiguous lines and arcs in an attempt to define a new, narrow surface that I want to extrude in order to create a "lip" on my Lens Part -- at least that's what I try to achieve. Here's the problem I'm observing: OnShape apparently does not treat the area between the two sets of lines and arcs as a surface. Why? Upon close inspection, one of the lines and arcs shown to be Coincident by virtue of the Coincident icon, do not appear Coincident when I zoom in as far as possible i.e., the area between the sets of contiguous lines and arcs is not fully enclosed, which would explain why I can't select the "Surface"..because it's not a surface. But why?

In this image, I'm using my cursor in an attempt to select the narrow area/'surface' between the inner set of lines and arcs..and the new, offset set of lines and arcs. The problem: I can't select the narrow surface...I can only select the individual line or arc segments.

In this image, we can see the inner and offset sets of lines and arcs more clearly. Note what appear to be 'coincident' segments circled in red.


Here, we're zoomed way in on the same segments circled in red, above. Note the Coincident icon.  Let's zoom in farther....

Here we see the unexpected condition. The icon suggests that these entities are coincident, but the GUI suggests that they are not. Why is this happening?

NeilCooke

You can report that as a bug if you want. The intersection produces splines and conics, which are then offset again and look to be too approximate to close properly. In the meantime, I would extrude the lip edge as a surface then thicken.

Evan_Reese

you can confirm that this is the problem area by adding more sketch geometry that would close the region. For example, make a sketch circle exactly how you annotated your image with the red circle. If it fixes it, the face turns gray.

matt_zerega

Thanks Neil and Evan.  A bit of follow-up: In an attempt to extrude the edge as a Surface, the operation fails if both of the segments are included that have the end points shown to be Tangent via the Tangent Constraint icon...that are not displayed as tangent when zoomed all the way in.

Neil..if anyone on your development could benefit from accessing this model for the purposes of debug, they're more than welcome.
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Here's what happens when attempting to Extrude the edge (line and arc segments) as a Surface:

Neil's suggested work-around works great on all segments..except one....


For this particular segment, before Extrude is chosen on the toolbar, this segment can be selected...

And then....once the Extrude tool is chosen...

S1mon

There's probably some small issue with the tangency/continuity of the inside surface edges. There may also be some weird microscopic edge in there that you aren't selecting.

You might be able to get where you need to go by building everything off of the outside edge. Either sweeping along it or extruding it as a surface and offsetting it. 

Keep in mind that when you offset curves or surfaces, there is no good closed-form general mathematical solution to offsetting a spline other than a degree 2. Every CAD system is approximating the offset. Edges which have been created by offsets (shells), extensions, or draft start to be a bit like a photocopy of a photocopy - a lot of noise gets added. Ends are especially suspect. Check the curvature combs of the inside and outside edges of your shelled part. You will likely see some weirdness on the inside.

It's always more robust to go back to the original sketch or surface edge if you can.