Sketches: everything in one sketch or separate sketches for separate features?

james_aguilar160

Friends, a simple and open ended question today from an OnShape newb:

Often you have a choice to incorporate multiple features into a single sketch, or to make separate sketches for different features. To pick a naive example, if I want to extrude something, and then make a hole on the same face that I extruded, I could make one sketch for the extrude, and then sketch on the new face to make the hole. Or I could put the vertexes for the hole into the first sketch.

As a general rule, do you find it better to have separate sketches for separate features, even when they are on the same plane (or a parallel plane) to another sketch? Or should you generally try to put all the features for a given plane into the same sketch? Does either approach have any implication for performance?

S1mon

It really depends on the purpose of the sketch, and how you anticipate wanting to modify it later. In the end, the point of a parametric modeler like Onshape is the ability to - hopefully - make changes which would be hard with direct modeling tools, very easily by modifying a dimension or two.

Performance-wise things really only get painful with tons of sketch entities, or complex series of constraints.

I would avoid adding too many details like fillets, chamfers, or patterns to a sketch, unless there's really no good way to solve for your design intent otherwise. Offsets, use edge, intersection curves and tangent relations are also more "brittle".

Keep in mind that a sketch is one of the few places where Onshape acts like a solver of simultaneous equations. It doesn't care what order you created the sketch entities within the sketch. If your design intent changes significantly, it's easy to go back and edit the sketch and change the dimensioning scheme to change what is driving what. This is not so easy with sequential features. 

A sketch is a unit of design intent. In complex models, I often organize things in a more schematic way in some basic views (plan and section, or top/right/front etc..), and then add more detail in later sketches and features.

While I really appreciate things like TooTallToby's speed modeling competitions, the approach that gets to a finished model the fastest is often the least maintainable and useful longterm. 

When I was using Solidworks, I would sketch as much as possible on the default planes and then extrude from/to vertexes (partially to help with how I would use draft during extrudes for injection molded parts). This would keep the number of extra planes down, simplifying the modeling tree. In Onshape, using mate connectors as sketch planes is super powerful, and helps reduce the clutter of lots of planes. If you're only going to create one sketch on a plane, consider using a mate connector instead. It really depends on the down stream features that you're using the sketches for, and what sorts of parts you're creating. Surfacing features (e.g. loft) need the curves to be in their real locations.

CFried

Is the hole important for the basic shape of the extruded? Then but it in the sketch of the extrude (maybe as an construction line only) .

If not put it in another sketch. Especially for holes this is the way you should handle it, so you can add chamfers/pattern as well and put everything in a folder.

Design intend is key in parametric modeling. To many features in one sketch makes it impossible to find problems. Keep it simple