Surfaces & Splines | 09- Build Better Chamfers

In this installment of Surfaces & Splines, techniques for manually creating aesthetic chamfers are discussed.
Production modeling of consumer products can be intimidating without the right combination of skills and modeling strategies. This video series discusses techniques to accurately create production models of the most challenging shapes present in today’s cutting-edge product designs using SOLIDWORKS.

[@DiMonteGroupInc]

Thanks for the question, Markus. Sharp eye! What Markus is questioning happens at roughly 2:27, when Andrew is creating Boundary Surface 25. If the Boundary Surface 25 had just been created between Curve6 and Curve8, it would have taken a straight-line path between the two. By adding Sketch63 as a Direction 2 curve to the definition of Boundary Surface 25, it makes the boundary surface follow the general curve of the part. Truth told, the more disciplined approach would be to have Sketch63 projected onto the outer face of the solid body for finer control of the shape. But this is a simple enough shape that it doesn't matter. Bonus information#1: Andrew not only made the boundary surface curve by adding Sketch63 to the definition of the Boundary, but it also elongated the boundary surface past the ends of the solid by a little bit. Boundary is kinda cool that way - it has the option to extend to the extents of all of the defining curves. If you did this with a loft, you'd still get about the same surface but without the elongation to the ends of Sketch 63. When modeling curvy stuff in SOLIDWORKS, it's important to go past coincidence because of round-off discrepancies in the background math Bonus information#2: Using "Split part" instead of "Split Line" to create the edge needed here keeps all of the adjacent edge IDs intact. Want more stable models? Avoid "Split Line" unless there is no alternative. -Ed

[@dcsev]

A basic question that I hope you can help shed some light on... If we would like to use "helper" surfaces or "helper" construction lines to ensure that a part will mirror smoothly (with tangency), how can we have the curves that instead are tangent to the construction line that is at a drafted angle? Would this not mirror smoothly? Thanks! Looking forward to your clarification because it is confusing me quite a bit.

[@DiMonteGroupInc]

Daniel, Your question would indeed be about a legitimate contradiction if we were creating a surface that was intended to blend seamlessly with its mirror. The thing is, that is not what we are trying to do here. As Industrial Designers, we can’t forget the “Industrial” part of the job title. This part needs to be molded. Which means that the surfaces of the part needs to be drafted, even all the way to the mirror plane, so the manufactured article can be ejected properly from the mold. That reference surface, or “helper” as Andrew liked to call them, is drafted to ensure that that resulting adjacent surface which uses it as a directional reference is also drafted. I really love this question because it forces a spotlight on manufacturing issues that are often forgotten with a lot of Industrial Design models we see out there. You might already know this, but maybe other readers won’t, so I’m going to bring up a simple example of the importance of draft that I think that everyone can relate to. Everyone has noticed that the sides of a cupcake or muffin are angled. The angled sides are there so the pastry will fall out of the cupcake pan easily after baking. If the sides of the pan were parallel, the pastry would get stuck in the pan. Injection molding has this same issue. Plastic parts without draft would stick in the mold, or would have drag marks on their surface if forced out of a mold with no draft. As Designers we might want to make parts that are perfectly smooth at the parting line, but as INDUSTRIAL designers we have to build in that draft angle, and hopefully use visual tricks in our design to imply that the sides are smoothly connected when in fact there is a slight ridge. The only exception where you *might* be able to exclude that draft is if, after talking with a molding resource, you can count on a part shrinking away from the cavity of a mold as the part cools (thermoplastics) or cures (thermoset plastics). But in practice this is almost never an option. I just checked a couple of blow molded bottles I have here at home and even those show a little draft at the parting line, and those definitely shrink away from their cavities. The best plan is always to include draft up front. OK, that said… There is a mistake in this model due to 2D thinking when making “Sketch 72”. The short edges of “Draft Reference - Surface-Extrude3”, if it is extruded with draft like it should be, ought to already have the correct draft. That draft is foreshortened in the plane normal to “Sketch 72”, but the actual necessary draft is there. Adding 2° to the centerline of “Sketch 72” is not necessary, and is actually contradictory. In 3D, the upper short edge of “Draft Reference - Surface-Extrude3” is actually the mathematically correct one as projected onto the plane normal to “Sketch 72”, and is what the curve should be tangent to. We all get tunnel vision when designing and it is easy to lose track of foreshortening in 3D, especially when we are cranking through a design. So yeah, that was a mistake, and thanks for calling us out on it (if that was what was originally confusing you). Thanks again Daniel for the excellent question! - Ed Eaton , DiMonte Group

[@muhammadzeeshantariq4683]

@@DiMonteGroupInc Crazy! All I can say is I'm amazed at how you guys are explaining things in detail. I had exact same thought that why in Sketch 72 we added a draft of 2 degree . Thanks for the explanation.