Discussion of Spoon Challenge

spoonsweepThanks again to everyone who submitted a model for this challenge. I’m getting some good feedback from people about this series, particularly from those who haven’t had the opportunity to do much surfacing work in the past. There’s no pressure, and we’re all just here to learn.

I want to start this by discussing the reason I built my model the way I did. I started with a sweep from an arbitrary position along the spoon. It’s not really arbitrary, I started it at the point where I wanted the decorative pattern to fade into the smooth face of the handle.

Because both ends of the spoon are going to be round, or come to a point, I just needed a place to start the sweep. A sweep can only come to a point on one end. Mark B at SWW this year showed that sweep paths no longer need to end in the plane of the profile, so that was one thing I wanted to show. Another reason I chose the sweep was to show something about splines. If I had chosen an arc for the sweep profile, the sweep would fail where the handle transitions into the bowl. That is because arcs cannot flip convexity (from being cupped up to being cupped down). So I had to use a spline as the profile.

Also if you notice, the sweep itself is symmetrical, but I only have a guide curve on one side. You cannot mirror things like projected curves. The way I handled this was to establish a Symmetric sketch relation with the ends of the spline. Because a sweep rebuilds the sketch at every intermediate section (intermediate sections can be seen by clicking the eyeglasses icon at the bottom of the Sweep PropertyManager), which means that they convexity flipping and symmetry are important to build into the sketch. Boundary and Loft don’t do this kind of thing, so the sketches can be “dumb”, but a sweep profile sketch has to be “smart” enough to rebuild at every point along the sweep.

spoonhandle

Next I built the tail of the handle. Notice that I ignored the fact that the spoon is supposed to be round at this end. The reason for that is that it isn’t easy to draw the stepped sketch on a curved surface, so I just decided to build it this way and trim it off. Anyway, what I’m trying to do is to create a scallopped pattern that fades into the smooth face. I drew several 2 pt splines, using handles to make them J shaped, then mirrored them. Then I made a Boundary surface between the sketch and the edge of the original sweep, reusing the rest of the mid plane sketch. Reusing sketch entities is an important aspect of both modeling efficiency and associativity.

fillspoonNext I tried to thicken the spoon, but it wouldn’t work. The problem was this bit at the end where the sweep created a degenerate point. Get used to that word if you’re gonna work in surfacing. It’s not a new concept, it’s just that SolidWorks has been shy about using industry standard terminology. See the Surfacing Bible or Entry #9 of the original Spoon Challenge post for a description of “degeneracy”.

Because the degeneracy wouldn’t thicken, I cut it off with a Trim feature. Before I did that, though, I made a Ruled surface that goes around the part to maintain the edge of the tip that was being trimmed away. When I trimmed the spoon, I also trimmed away the part of the Ruled surface that I didn’t need. The best way to describe this is to just look at the part and see what happens in Surface-Trim3.

Then from the trimmed edge of the spoon and the remaining section of the Ruled surface, I built a Fill. Notice that the Fill does not create a degeneracy. This is one of the best reasons for using a Fill.

spoontailNext I trimmed off the handle end of the spoon, knit it all together and tried to thicken it. Again, thicken wouldn’t work. This time the reason was the sharp edges between the scallops on that Boundary surface. I tried different thicknesses and different directions. In the end, I wound up making little fillets to take away the sharp corners.

Notice two other things going on in this image. First, the edges between faces are all shown as phantom. This uses the setting View, Display, Tangent Edges As Phantom. Past versions of SW had a different interpretation of “how tangent is tangent enough”. SW09 seems to be pretty liberal, comparatively speaking. I think what we have now can be called a “fix” rather than just “sloppy”. We used to have the problem where tangent edges didn’t always display as phantom. I had hoped that the problem would be solved by making the modeler more accurate, but I think what has happened is that they relaxed the tolerance on the display. Is this right or wrong? I haven’t had any problems with it, and I do like to see edges shown as tangent.

The second thing happening in the image above is the blue edge. You can set surfaces to show open edges (edges that bound only one surface) in a different color. This helps with other types of models where it is important if a model is open or closed.

So that’s how and why I built this model that way.

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