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

daniel_hoffackerdaniel_hoffacker Member Posts: 2
edited August 2015 in Using Onshape
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

Best Answers

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Answers

  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,376 PRO
    edited August 2015
    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.
    //rami
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    edited August 2015
    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
  • daniel_hoffackerdaniel_hoffacker Member Posts: 2
    Thank you so much for the help.  I'm going to try making my own this weekend!
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    edited August 2015
    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)
  • navnav Member Posts: 258 ✭✭✭✭
    Hi @lougallo first time I make one of those, knew the workflow could be improved, did not know you could thicken sketches, Thanks Lou.
    Nicolas Ariza V.
    Indaer -- Aircraft Lifecycle Solutions
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    Would Extrude work, for thicken?
  • navnav Member Posts: 258 ✭✭✭✭
    edited August 2015
    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.

    Would Extrude work, for thicken?
    Just did a version in the public Doc I shared above using Extrude and it works as well

    Nicolas Ariza V.
    Indaer -- Aircraft Lifecycle Solutions
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    @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!
  • lougallolougallo Member, Administrator, Moderator, Onshape Employees, Developers Posts: 1,617
    edited August 2015
    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!
    Lou Gallo / PD/UX - Support - Community / Onshape, Inc.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    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_cannonjordan_cannon Member Posts: 6
    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_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    Yay! and thanks for not posting the view here, leaving the option open for those who still want to crack it for themselves. 
  • navnav Member Posts: 258 ✭✭✭✭
    Hi @jordan_cannon nice thanks for sharing, @andrew_troup ´s challenge kept me awake a few times yesterday, I couldn't figure it out.
    Nicolas Ariza V.
    Indaer -- Aircraft Lifecycle Solutions
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    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)

    Philip Thomas - Onshape
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    edited August 2015
    Update: Another Onshape employee has done it in 11 features (@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!!!! :))

    Philip Thomas - Onshape
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    @philip_thomas ;
    Does that mean you have to give the internet back?  :)
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    edited August 2015
    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_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    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_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    edited August 2015
    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_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    @andrew_troup : Cannot open your link. Also - please build an example of your most recent 'theory' - it sounds promising :)

    Philip Thomas - Onshape
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    edited August 2015
    @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_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    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 ;)
    Philip Thomas - Onshape
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    @philip_thomas ;
    Yay! At this rate, we'll be into negative feature count territory early next week....
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    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 :)
    Philip Thomas - Onshape
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    @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__Ðave_ Member, Developers Posts: 712 ✭✭✭✭
    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_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,225
    edited August 2015
    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? :)

    Philip Thomas - Onshape
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