Best Of

You have to give us the link here…
Sharing with support shares with Onshape tech support (needed when creating a support ticket), not the forums.

Hey @simon_blum I looked at your design. It doesn't seem like the design is right for the frame tools. What you are making are a large collection of flat parts. A frame is a collection of segments with a constant cross section. Think tubing, or 2-by-4s. For frames, a cutlist would be a list of the different segments, their lengths, and their start and end angle conditions.

From looking over your design, it looks you have a collection of flat parts like what would be done on a CNC router table or laser. I think you probably mean "cut list" in the sense of "these 4 parts are geometrically identical, so somewhere there should be a list that says "Top Vert, Quantity 8" or whatever. If I look at the assembly BOM (flyout from right-side menu), I see that every part is unique:

because every part is unique in the part studio. So you probably want a BOM where it tells you: go make 4 of the verticals, 8 of the bottoms, 2 of the horizontals, 1 of the short horizontals, etc.

What you've done (and many, many people including myself do/did/still do but regret it) is design the assembly in a part studio. What you really want to do is: design the parts in the part studio, but assemble them in an assembly (should be called an assembly studio for parallel grammatical structure but Im not in charge, so). When you have two parts that are the same, for example, your "Top Vert L1" and "Top Vert L2" - dont do this. Or rather: do it all you want in the part studio, but when you assemble in your assembly, just use the "Top Vert" part. Insert one "instance" of it, mate it to the right location, etc. Then when you go to insert the next vertical part, insert another instance of the "Top Vert" part and place that one. Then your BOM will start to look like this:

See - Im reusing the Top Vert L1 and the BOM knows that it's the same thing so you get the correct count of parts you need to manufacture.

I think you'd benefit by hitting the learning pathway re: assemblies. Onshape assemblies are extremely powerful but also a point of departure from other CAD applications so understanding how Onshape does them will help.

Your design looks good! In my evening hours I have a Cricut and a lasercutter and vinyl for miles. I love the material. Would love to know what you are making!

Last, in case I have profoundly misunderstood your design intent around frames, here's what that message means:

RE "Paths cannot contain a branch" The frames tool takes your various input selections and constructs paths out of them. A path is a sequence of edges and connects them end to end and then creates the segments as a series of sweep operations along those edges. If it can't find this single path (connecting all the selected edges end to end) because there's a branch somewhere, it just fails with a message. This is what @rick_randall probably meant by selection order.

Here's an example to explain: We construct a cube (4 edges for the bottom square, 4 for the top square, then 4 verticals). We do the top and bottom squares because those edges create two disjoint paths. But add a single vertical edge to the mix and it falls over because its trying to find a single path through all edges and it fails:

Hope that helps!