rounding extruded edges on sides, not faces

adamohern

I'm extruding rectangles, and by trial and error I found that the following code does exactly what I want:

var filletCandidates = qCreatedBy(id + ("extrude" ~ i), EntityType.EDGE);
                var filletEdges = qUnion([
                        qNthElement(filletCandidates, 0),
                        qNthElement(filletCandidates, 1),
                        qNthElement(filletCandidates, 2),
                        qNthElement(filletCandidates, 3)
                    ]);
                opFillet(context, id + ("fillet1"), {
                            "entities" : filletEdges,
                            "radius" : definition.edgeRadius
                        });

This works for rectangular extrudes, because it just-so-happens that Onshape puts the extruded edges (the ones running normal to the sketch plane) first in the qNthElement() list. All I have to do is gather up the first four, and I know I've got all of the vertical edges.

Two questions:

1) Is there a cleaner way to do this in my situation?

2) Is there a generalized way to access all of the non-end-cap edges of an extrude regardless of profile shape?

jacob_kingery

Have you seen qCapEntity()?  It takes in an id (e.g. id + ("extrude" ~ i)) and a boolean for whether to return the start or end cap entities (I don't see a way to get both at once).  Using a qSubtraction() between your filletCandidates and the results of the qCapEntity()s should give you just the non-cap edges.

adamohern

Sounds promising! Will give this a shot. Many thanks!

adamohern

Beautiful, Jacob. This worked for me. Thanks again.

var filletCandidates = qCreatedBy(id + ("extrude" ~ i), EntityType.EDGE);
var capEntities = qUnion([
    qCapEntity(id + ("extrude" ~ i), true),
    qCapEntity(id + ("extrude" ~ i), false)
    ]);

var filletEdges = qSubtraction(filletCandidates, capEntities);

opFillet(context, id + ("fillet1"), {
    "entities" : filletEdges,
    "radius" : definition.edgeRadius
    });