# Technical drawing for a part with complex (non-line, non-arc) geometry

I've been making technical drawings for various parts I've designed. Since these parts were meant to be 3D printed, this is mainly just to have them in my portfolio so I have something to show/talk about at the upcoming career fair (I'm an undergraduate ME student).

I've encountered difficulty with one particular part, which is designed to hold the motor for a perpetually spinning top. Because the motor ran a little hot when turning the rather heavy disc it was attached to, I used the SolidWorks wrap tool to remove portions of the cylindrical casing in order to encourage heat dissipation.

As you can see in the image, SolidWorks is unable to annotate the resulting dimensions, at least not using the basic tools I'm familiar with. So my question is: how would the dimensions of this part be represented on a technical drawing? Relatedly, since it probably determines the answer: by what process could a part like this be machined, if 3D printing was not an option and the arguably unnecessary complexity could not be removed?

• Critiques of the drawing unrelated to the question are also welcome. – Jessica Alan Jan 11 '17 at 19:38
• A general comment on the drawing: don't leave so much blank paper - make the views bigger! Orienting the axis of the cylinder horizontally instead of vertically might match the shape of the drawings better to the shape of the paper. The overall assembly drawing will show the orientation of the parts in the complete device. – alephzero Jan 12 '17 at 4:48

You don't need to dimension it at all, because as you probably know, that part would never be manufactured by looking at the 2D.

At my company, one of the standard notes we put on every drawing is "Referring to solid model for geometry not dimensioned is permissible. All unspecified surfaces must match solid model within .020 in. (and we put the .020 in a GD&T profile symbol)

• "Referring to solid model for geometry not dimensioned is permissible" - if that is OK in your industry then great, but it doesn't work for everybody. Try working on a collaborative project with half a dozen large companies all using different CAD software, and the probability that "the solid model" will look the same when they all import it into their own system is just about zero. And when mistakes can kill people, that also makes a difference. – alephzero Jan 14 '17 at 0:36
• Sure, but since the actual part is being 3d printed, I think it's acceptable in this case too. And if you define the STL file as the canonical solid model, it should look the for everyone because it's just triangles--there are no rounds or splines (to pick two examples) that will get implemented differently on different systems. – regdoug Jan 14 '17 at 4:08
• That;s probably true, but I wouldn't consider an STL file as "a technical drawing". At best, it's an approximation (of unknown quality!) to the geometry that the designer had in mind. It can't even begin to represent important design information like geometric tolerances. – alephzero Jan 18 '17 at 18:32
• @alphazero that used to be true. But importers have become remarkably good at this lately so i wouldnt count on it to screw up. For example the automotive industry is moving towards digital only drawings. And to my understanding toyota is allready there for most parts, offcourse they can demand change of application. Simply this is the step we must take, this is why 3D tolerancing and dimensioning standards have evolved. Anyhow using this kind of object as ones portfolio item shows bad understanding so its not – joojaa Jan 19 '17 at 4:47

You probably need some auxiliary sections as well as the three basic views.

For example if you draw a section at mid-height looking down the axis, you can easily dimension the "straight" ribs. If you draw a section normal to one of the curved ribs, you can dimension the cross section of that rib, and presumably they are all the same.

Since the dimensions of the ribs don't look very critical (presumably only the top part is actually load-carrying) just conveying the message that "this rib follows the contours of the cylinder and its cross section is approximately $x$ inches square" is probably as much information as anyone needs in real life.

Unless you really want it to look like that for aesthetic reasons, a way to machine something with the same functionality would be make to a hollow cylinder, and then drill a pattern of holes through it radially. Since the cylinder is thin, it might be easier to drill a pattern of radial blind holes into the solid cylinder before you bore out the interior.

If you wanted to machine something that looks more like your 3D printed version, you could mill triangular holes with fillet radii in the corners, instead of drilling circular holes. (The fillets radii would be the same size of the milling tool, of course.)

With either of those options, it's more obvious what you need to include on the drawing - the purpose of the auxiliary views and dimensions is to tell the operator how to set up the machine tool, and the tool itself will "automatically dimension" everything else.

"Try working on a collaborative project with half a dozen large companies all using different CAD software, and the probability that "the solid model" will look the same when they all import it into their own system is just about zero."

I disagree, step file translation and exchange is industry standard works great.. Undimensioned drawings are common practice... Partial dimensioned drawings are also called "Critical Feature Drawings" or "Limited Dimension Drawings".