Does anyone have a dodecahedron tutorial or can comment on techniques to make one?

daniel_hoffacker

Anyone have any good methods for creating a 12 sided dodecahedron in on shape?  Has anyone made one successfully?  I saw two tutorials for other cad programs but no examples in on shape for making this geometric shape.  I found this one: http://www.inventortales.com/2012/11/all-for-fun-again-modeling-12-sided-die.html  and also this one from solid works http://learnsolidworks.com/solidworks_tutorials/how-to-model-a-dodecahedron-in-solidworks.

Any help would be grateful!!  Thank you so much!

Dan

nav

Hi @daniel_hoffacker here a link with my approach, to be honest I used the following Solid Edge video as reference and did the same but with the tools available in OS.

https://www.youtube.com/watch?v=a1CpThxqhgo

Here is the public URL:

https://cad.onshape.com/documents/b86179670fa44e5f8b21b133/w/c1850f8e165a449a8120ed4a/e/88488bdabd954d66bf9b57f1

lougallo

@nav Awesome!!  I copied your start of sketches (the hardest part) and simplified a bit.

Doc link:  https://cad.onshape.com/documents/a6f9725433784b5ba56affb1/w/574d0540967243e0b7a2febd/e/d1bf3b4566e34f69966f0d08



You can thicken sketches... so no need to do lofts and once you have half, you can mirror and transform 36 degrees.  Fun exercise...

3dcad

I haven't ever created one (and haven't seen any videos), but at first sight I would begin with creating planes in certain angles and create sketch of one pentagonal face. Extrude with symmetric option. Copy sketch to other planes -> symmetric extrude. In the end boolean all together and add fillets.

If I have time in weekend, I will give it a try.

andrew_troup

You will get some help from the thread linked below. Although it's a different Platonic solid, some of the same principles will apply

https://forum.onshape.com/discussion/comment/7053#Comment_7053

nav

Hi @daniel_hoffacker here a link with my approach, to be honest I used the following Solid Edge video as reference and did the same but with the tools available in OS.

https://www.youtube.com/watch?v=a1CpThxqhgo

Here is the public URL:

https://cad.onshape.com/documents/b86179670fa44e5f8b21b133/w/c1850f8e165a449a8120ed4a/e/88488bdabd954d66bf9b57f1

daniel_hoffacker

Thank you so much for the help.  I'm going to try making my own this weekend!

lougallo

@nav Awesome!!  I copied your start of sketches (the hardest part) and simplified a bit.

Doc link:  https://cad.onshape.com/documents/a6f9725433784b5ba56affb1/w/574d0540967243e0b7a2febd/e/d1bf3b4566e34f69966f0d08



You can thicken sketches... so no need to do lofts and once you have half, you can mirror and transform 36 degrees.  Fun exercise...

andrew_troup

Thanks @lougallo and @nav

(somewhere along the way, the endpoint of Sketch 4 in Lou's model has lost what I infer was its pierce relation to sketch 3, BTW)

nav

Hi @lougallo first time I make one of those, knew the workflow could be improved, did not know you could thicken sketches, Thanks Lou.

andrew_troup

Would Extrude work, for thicken?

nav

andrew_troup said:

Thanks @lougallo and @nav

(somewhere along the way, the endpoint of Sketch 4 in Lou's model has lost what I infer was its pierce relation to sketch 3, BTW)

Hi Andrew actually when I was doing the sketch couldn't pinpoint well that intersection, tried all constraints / + Use to see if the intersection got detected and just when I got two Coincident symbols on the intersection of both curves  I drew the perpendicular line to it and then drew a point, In Solid Edge, there is a constraint that detects the intersection between a curve and plane as shown in the video. Didn't know it was going to work in OS, apparently it did but I also doubted about that intersection between Sketch 4 and 3 as you mentioned.

andrew_troup said:

Would Extrude work, for thicken?

Just did a version in the public Doc I shared above using Extrude and it works as well

andrew_troup

@nav
Thanks for your typically thorough and thoughful message. I was able to add a pierce constraint no problem between the endpoint of the line and the circle from sketch 3, BTW, and that fully constrained that endpoint.
Pierce relation does indeed capture the point where a curve passes through the sketch plane. Give it a go!

lougallo

Extrude would work just fine.  I like these challenges... @nav this was my first go as well.  It is much easier to take a more efficient stab at it when someone blazes the trail!! Nice work!

andrew_troup

To anyone after a more conceptual challenge: here's one which is quite fun to solve using Onshape:

The view below represents the top view, side view and front view (all orthogonal, no tricks) showing all visible edges and contours of a single body.

What does the isometric view look like?

(To anyone who has already encountered this one: it would be nice to hold off any spoiler posts until someone has solved it from scratch) 

jordan_cannon

andrew_troup said:

To anyone after a more conceptual challenge: here's one which is quite fun to solve using Onshape:

The view below represents the top view, side view and front view (all orthogonal, no tricks) showing all visible edges and contours of a single body.

What does the isometric view look like?

(To anyone who has already encountered this one: it would be nice to hold off any spoiler posts until someone has solved it from scratch) 

That was a fun exercise. I'll admit to overthinking it quite a bit on my first stab. The isometric view should look like this:

https://cad.onshape.com/documents/be38bd57d9c94b8ebe63c5a3/w/bb52af5f6b6d429f91dccdcb/e/1f4e140d4fb749b3b5eb52b4

andrew_troup

Yay! and thanks for not posting the view here, leaving the option open for those who still want to crack it for themselves. 

nav

Hi @jordan_cannon nice thanks for sharing, @andrew_troup ´s challenge kept me awake a few times yesterday, I couldn't figure it out.

philip_thomas

Hmm - I posted a dodecahedron as a public document back in March including my email address and using just 15 features.
No one has emailed me saying they were able to do it in less, so i would go with my solution   
(and I win the whole internet)

http://bit.ly/dodecahedron_public

philip_thomas

jon_sorrells) - Well done!!! Of course 'loft' wasn't available when I did mine - lesson: study the what's new carefully to see if a new capability can improve the efficiency of an existing workflow.
Again - congratulations Jon.
(link redacted because it pointed to an internal server - i will post it when @jon_sorrells recreates it on production!!!! )

jon_sorrells

Here's a link to my model

https://cad.onshape.com/documents/e24d1462c393404888cee882/w/173143f610874497b0482b22/e/4c785c6c51d948a487b97c32

andrew_troup

@philip_thomas
Does that mean you have to give the internet back? 

andrew_troup

I seem to have done it with one step less than @jon_sorrells took
https://cad.onshape.com/documents/9d0cf267925b4d55860e528d/w/27869f5acf6d49ce967b429d/e/0ee54e01680346dfbce11720

I imported a finished dodecahedron as a cheat to avoid have to construct my sketch geometry from scratch: hence the two "Fixed" points in Sketch 1, which started life as vertices of the finished solid.

It would be a trivial exercise for a Platonic geometer to do sketch 1 the proper way... and (unrelated point) I have an inkling there's the potential to save at least one more step.

andrew_troup

Potential confirmed, similar process is doable using one less step ... but Sketch 1 would get trickier to construct (using pure geometry: not much harder if you cheat like me)

andrew_troup

Actually: looking at the png sketch @philip_thomas posted:
the first two sketches are easy for the revised method: it was staring me in the face

The first key is to draw sketch 2 before sketch 1, and draw both the inner and outer pentagons on the base plane as in Philip's posted sketch. The second key is to align one of the pentagon edges, on that base plane (from either pentagon, it's immaterial which) parallel with a construction plane (the Right plane in this example). This will ensure that horizontal line in sketch 2, which serves as the axis for the first"Transform-Rotate" operation, is parallel to one of those edges, in which case that single "Transform-Rotate" is sufficient and the second can be eliminated.

The angle line in what has become sketch 2 is now drawn from the base circle of the larger pentagon, not from a vertex or midpoint of an edge.
A horizontal line whose midpoint lies above the origin, at the height of the dodecahedron, serves as a proxy for the upper base circle, which the angled line needs to pass tangent to. The sole purpose of the angled line is to position the tip of the loft.
The attached graphic might clarify this a bit. The upper circle is an extra sketch for explanatory purposes only:
In the model, it is represented (as mentioned above) by a horizontal line in the existing sketch on the "Right" plane.

OK, so the bar is now set at two (relatively simple) sketches and three (very simple) features.

I look forward eagerly to seeing the bar set higher still.

philip_thomas

@andrew_troup : Cannot open your link. Also - please build an example of your most recent 'theory' - it sounds promising

andrew_troup

@philip_thomas   Hmm...
The document should open now from the original link (I set sharing on the wrong one)
But I'm puzzled why the graphic I attached to my llatest post has become detached. Here it is again:

philip_thomas

Nicely done @andrew_troup, slick solution. Hmm, using my crystal ball i predict that very soon that I might be able to knock one if not two features off that count

andrew_troup

@philip_thomas
Yay! At this rate, we'll be into negative feature count territory early next week....

philip_thomas

Jon Sorrells has already done it in 9 - but you will have to wait a little longer to see how (and what cool new doo-dad) he used

andrew_troup

@philip_thomas
My enhanced method would have two sketches and three features (the one I posted had 2/4)

It's not clear to me exactly how you're counting, because @jon_sorrells' previous effort was 2/5 by my count, yet you imply that nine would be an improvement?  

_Ðave_

Are we counting every item in the feature list, sketch, plane, extrude etc. and does the sketches have to define and prove all the calculations or can calculations be done outside the document.

philip_thomas

Andrew - I am using the count at the top of the feature manager - this includes the origin and 3 default planes.
Using your accounting method, that would put Jon's new solution at 5
If you also have a '5' solution please post it.
I apologize for casting aspersions, but a more cynical person than I, might look at your previous solution and suggest that you could not have developed that sketch without first having built the model, referenced the geometry and then deleted it!
Under the glare of a bright light, would you care to comment?