Lofting Woes

thomas_o_connell

So I've made two parts I need to join a loft.   In looking at some of the other questions, it looks like me trying make the hollow aspects myself (customized) sort of breaks the way the tool works.   Is there any way to get these glued together as is, or if not, where should I rethink things.

What I thought I might could pull off: take the two sets of edges, loft as Surface, and then thicken the result.

Project is public:

Dual Extruder Fan - Rigidbot MK8 V6 v2

Photo:


Not sure if links work:
https://cad.onshape.com/documents/1a6dac8f1d2842ffb92ffbf9/w/0b7f42c818e7489798f803fd/e/adac0e04d32248159ecbe311

andrew_troup

Your proposed plan is a good one. What is needed to make it work controllably in Onshape is to make a dedicated sketch duplicating the destination circle, but splitting it into as many arcs as there are entities in the round-ended slot which is the profile of departure. (Use the "Split" tool - refer Help)

You should create that sketch with the arcs are disposed symmetrically about both a horizontal and a vertical centreline (using the symmetrical constraint between corresponding endpoints) and use an angular dimension to drive the relative lengths of short vs long arcs.

This way, when you come to fine-tune the shape of the resulting surface loft, you can do so easily.
When you pick the two profiles, pick the segments around the departure profile in careful sequence, and then pick each corresponding arc in the destination profile in the corresponding sequence.

If you find this too tedious, you could resort to 'vertex matching' (See Help)

andrew_troup

Further clarification: the arcs should be produced by either "Use/Project" from the circular edge they are intended to match, or be constrained "Coincident" with that edge (which works like "Coradial" in SW)
You will know if you have nailed it down properly because the sketch arcs will all go black instead of blue.