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I personally think, for the challenge to have any validity, the sketches should all be driven from a single ruling dimension, no external calcs or magic angle inputs. All geometry should be derived from a regular pentagon.
My sketches so far have not complied, because I was focussed on arriving at the simplest possible modelling approach, but I am confident of being able to remedy that, when I get a bit more time.
Thanks for that
(I have a further confession: I admit to sweating a bit, in spare moments, about condensing the construction to only two sketches for my revised, asymmetric orientation!)
A question remains on the other point: can you lay out how you think the steps should be counted?
Thanks
Dave
https://cad.onshape.com/documents/60d93351f66d4936a7de2399/w/23b9cc0586fa48b7915732d7/e/c091518dadb747b8a1cd37e6
I'm not thrilled with the constructions being so inelegant, but I console myself that it's mainly because there is currently no way of making dimensions equal between two sketches, unless the sketch planes happen to be parallel.
ON EDIT: I should have written: "unless the line on the first sketch lies parallel to the sketch plane of the second" .... which is what I was able to exploit.
I had to, because with only two sketches, they had to be mutually perpendicular
The full explanation (and many people may not realise this):
the "Equal" constraint does NOT make two lines equal: it makes their projection in the current sketch equal.
(Which, I hasten to add, is as it should be, and as it is in other parametric modellers I'm familiar with)
Essentially the large base pentagon is lofted to a point and rotated as shown. The Boolean intersection is the finished dodecahedron.
If, in future, the ability to specify "Intersection" becomes an option in "Transform/Rotate", that would eliminate a further entry in the feature list.
My revised two sketch, three feature solution rates as 9 features, by that yardstick: perhaps it's the number of features raised to the exponential power of the number of sketches
Very cleaver, I didn't understand the fundamental geometric relationships of the dodecahedron.Thanks for laying it out nicely.
Sorry to have kept asking questions you had already answered, and refraining from answering questions you had asked:
The reason is that I somehow missed out on seeing the last few posts on page 1 before it rolled over to p2. Mea culpa.
I do seem to have accidentally responded to your challenge to put up a nine-feature solution (by Onshape's reckoning) without any sleight of hand involved in the sketches.
I personally think it's a bit unfair Onshape charging me for the use of the third construction plane, when I only used two .... but I did use the origin, so I'll concede it's an eight-feature procedure.
Someone else can run with this ball now; I think I've got it out of my system!
Equal rights, self-determination .... and a cut on any resulting profits...
(and before anyone casts aspersions on the nature and extent of their self-regard: they assure me it is purely Platonic)
https://cad.onshape.com/documents/7cb790ec4f9a4854bab35a2a/w/b9f42bd50a274e85bc1ad861/e/6cfac795c8274b139bdc45c3
Instead of making a second sketch and lofting the pentagon to a point, I extruded the pentagon and set the draft angle to atan(2)/2.
philip_thomas said:
@andrew_troup : Agreed (to both the rules and your confession
Nice model, but given that you're not using construction sketches for the draft angle, but relying on an externally derived calculation formula, you might have to consult your colleague as to whether it really qualifies, under the rules we agreed.
(PS: Forum software is screwing up quotes even worse than usual. My quote from Philip's post previewed properly, but does not post correctly)
CAD is a tool for Engineers that enables us to capture our ideas. Parametric CAD enables us to evaluate our ideas over a range of values. We encode within our models known conditions (constraints, constants and formulas) that enable the models to regenerate over reasonable ranges of parameters. These constants may include things like PI that we use without having to derive the relationship between the circumference of a circle and it's radius each time we use it. In Jon's model, he has derived a relationship (angle) that he uses to define the geometry. If this constant worked for only one inscribed diameter (the only variable), I would tend to disqualify the solution. Not only does it work for all (reasonable) diameters, but the numeric value of the draft angle is calculated by an expression that could/does indicate the logic. I therefore rule Jon's submission valid (and kudos to Onshape for allowing a drafted extrude to tend to a singularity without failing and for allowing expressions in numeric fields)
Hey, I didn't think it possible, but you've persuaded me, in spite of myself.
The rules which I proposed (and you agreed) included "no external calcs or magic angle inputs", the latter being expressly designed to make the construction sketches definitive.
One scenario I envisaged, and was trying to forestall as not kosher, was exactly what transpired (extrude with draft at a "magic angle", whether as two steps or one)
But you're unarguably right, damn you!
Note that my smiley does not have gritted teeth - I can afford to be magnanimous, given that your ruling does not (at least, not yet) knock my submission off the top step of the podium, and I don't mind sharing that step with jon, whose model (I have to admit) is both more geometrically and trigonometrically interesting (and elegant) than mine.
Anyone who wants to see all the different approaches in one place can make themselves a copy of this model:
https://cad.onshape.com/documents/f9c6f62ce60a4cbea05f3e63/w/267933797acc43f693478d4f/e/44189f8d9d9242a790a27887
y2k (you're too kind)
Incidentally, the point you make about "allowing a drafted extrude to tend to a singularity without failing" is one worth taking seriously, I reckon.
I still recall smoking out that Solidworks had implemented it in that way.
(Gee, I realise this is unlikely, bordering on nutty, but let's just try it all the same ...... Yes !!! )
I always hated using "revolve" for trivial operations like chamfering a nut, or providing a conical bottom to a cylindrical hole (say to represent a drill tip).To me, it offends the First Law, the one about economy of effort.
In the former instance, we can now pick the inscribed circle of the hex. and "Extrude/Intersect/with draft 60deg"
But your point about singularities being tolerated comes into play in the second case: for drill tips (#), it's now just a matter of clicking on the bottom face of the hole and "Extrude/Remove/with draft 60deg", or whatever angle we want, specifying any depth we fancy, provided it's greater than the expected depth of the cone.
No need to laboriously create a local sketch plane through the hole axis, then sketch, constrain and dimension a triangle, and a revolve axis, then choose "Revolve" and another click to select the axis.
In SW, having done it the easy way once, we can even 'drag and drop' that feature to other holes of differing sizes.
Now THAT'S what I call lazy (sorry, "economical"
---
(#) yup, I know, we now have "Hole Feature" - but only for standard situations.
Like this ^
Indaer -- Aircraft Lifecycle Solutions
We, too, have a local saying, which is non verbal, consisting of shuffling the feet and looking sheepish...
Probably the nearest verbal equivalent from the dominant culture on this forum would be "shucks", followed by a quiet but heartfelt "gee thanks".
1) I'd love to see a proof that this forms a regular dodecahedron. My 14 year old son had some trivial proof that it wasn't, but I wasn't listening. It doesn't look like it couldn't be right and yet it does look like it IS right. Can all the platonic solids be generated by some generalization of this technique? Actually...don't answer any of these questions. I want to try.
2) This is an amazing technique even if it isn't geometrically perfect. I found this while looking for a way to make a faceted, turtle shell-like shape. It seems to be working perfectly. I've been doing CSG for a while so I understand the technique, but for some reason in OS I've been only building things up piece-wise like I'm actually fabricating them.
3) Once you've generated a part like this, you can click around to all the edges and vertices and the OnShape "heads up display" will tell you the distances and angles. Is there a way to generate a drawing of each face individually? I'd like to cut them out of plate and weld an irrelgular polyhedron together.
A dodecahedron is convex -- therefore it is the intersection of half-spaces on its faces.
Take a dodecahedron and place it on a table -- the faces form 4 "layers": the bottom face, the lower 5 faces, the upper 5 faces, and the top face.
Let's split the faces into two sets:
1. The bottom face and the upper 5 faces
2. The lower 5 faces and the top face
When you intersect the half-spaces on the faces in set 1, because of the symmetries of the dodecahedron, you get a pentagonal pyramid (the bottom one in the picture). When you intersect the half-spaces on the faces of set 2, you get a congruent pentagonal pyramid (the top one in the picture).
When you intersect the pyramids, you're effectively intersecting the half-spaces of all 12 faces, so you get back the dodecahedron.
If you started with 12 regular pentagons and walked through your half-spaces, you'd end up two "pentagonal cones" that, intersected, would re-create the original dodecahedron. But that's kind of useless.
I guess I was assuming that any pair of cones like this would create a regular dodecahedron, but it's trivially obvious to show that can't be. So the real question is what properties the cones have to have to make the final polyhedron regular. I can probably figure this out if I ever need it. Fortunately my project just needed a "faceted structure", not anything regular.
https://cad.onshape.com/documents/2c40f522f1b5a02f6ce9ce01/v/88890a276bbd7271707e659d/e/a73b7ceefb331b792b81aa84
It can also make some other polyhedrons