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 Post subject: Need help with solidworks.
PostPosted: Wed Mar 13, 2013 7:50 am 
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I have several questions i need clarification on for designing puzzles.

1) For shell mechanisms, how thick should each 'zig zag interlocking grooves' part be?

2) How does one convert a solid sphere into a sphere-spider hybrid random holey core?

3) What is shapeway's minimum wall thickness now? The page says 1mm, but in Eitan's video, he mentions 'shell to 0.7-0.8mm'

Thanks in advance!

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 3:54 am 
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bump. I still need help D:

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 11:28 am 
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The wall thickness can still be in between 0.7-0.8mm, but only for WSF material. For WSF polished you should have a wall thickness of 1-2mm, since the polishing process can remove quite a bit of material from the outside of a part.

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 3:15 pm 
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Hey! There are a lot of factors, but if you post an image of your sketch, I know a lot of people would be willing to chime in.

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 9:50 pm 
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Here is the sketch of a puzzle I am working on.

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Right now, all the segments are 2mm wide.

One more question, must the area where corner stalk meets corner base be filleted?

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 10:00 pm 
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rubikcollector123 wrote:
One more question, must the area where corner stalk meets corner base be filleted?

I would recommend doing it because the angle there is usually very sharp, but you don't need much. About 0.5mm-0.7mm will work.
Also, the shell levels themselves need to be 2-3mm thick at a minimum, while the groove layers (the ones that hold each shell together) need to be between 1.5-2mm thick at a minimum (this keeps them stable).
Also, are you designing a puzzle with more than 2 shell layers? If so I recommend using 2 layers of grooves for the last shell: the first one (if you count from the origin) should be deeper cut than the desired cut depth, while the second should be shallower cut than the desired cut depth (this results in a style similar to V-cube mech). This stabilizes the pieces a bit better. You don't need them on the internal shell layers since the pieces from the next shell up tend to hug them and stop them from wiggling too much.
One more thing: it looks like the mechanism is too close to the surface of the dodecahedron. You need to make it just a little deeper to make the outside more solid (not too deep, otherwise it may not be big enough to be stable).

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 Post subject: Re: Need help with solidworks.
PostPosted: Sat Mar 23, 2013 11:04 pm 
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Thanks!
Dont worry about the sketch being close to the surface. I intend to turn it into a cube so that part is extended

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 Post subject: Re: Need help with solidworks.
PostPosted: Sun Mar 24, 2013 5:40 am 
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Oh yes, how does one do a body delete to remove duplicate parts without clicking a lot of parts? Seems eitan was able to do that in his video.

Is 0.5mm fillet radius ok?

How is a spider in a holey sphere core made?

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 Post subject: Re: Need help with solidworks.
PostPosted: Sun Mar 24, 2013 12:27 pm 
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rubikcollector123 wrote:
Oh yes, how does one do a body delete to remove duplicate parts without clicking a lot of parts? Seems eitan was able to do that in his video.

Simply select the pieces you want to keep, and then hide them (right click). Once you've hidden all of the unique parts, simply insert a body delete (using the filter bodies tool) and select every body on screen (click on a corner, then drag over every body) and then hit ok. Every body except the ones you've hidden are now gone.
Quote:
Is 0.5mm fillet radius ok?

Usually I actually use 1mm radius on the internals and 2mm radius on the edges which are part of the solid's external edges. However I recommend using 0.75 or 0.5mm fillets where 1mm is too big.
Quote:
How is a spider in a holey sphere core made?

My way of doing it is quite long, but you will probably need to edit your sketch a bit. Draw it so the bottoms of the center pieces become flat, not curved (make it so the pieces also extend toward the origin). Like this:
Attachment:
File comment: This is a 3x3 example.
spider core sketch.jpg
spider core sketch.jpg [ 161.63 KiB | Viewed 2312 times ]

Once you have that, add 2 split features: one with the external cutting surfaces, and one with the inernal surfaces (applied just to the centers). After that, draw a circle on the plane perpendicular to a center piece (make the circle the same size as the inscribed circle of the bottom face of the center). Then you can extrude boss/base, and extend the resulting cylinder up to the bottom face of that center piece (be sure to uncheck merge result!) Then you have one arm of the spider. After a circular pattern of that arm, combine all of the arms into one body and Bam! there it is:
Attachment:
6-arm spider.jpg
6-arm spider.jpg [ 290.48 KiB | Viewed 2312 times ]

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Mar 27, 2013 6:09 am 
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Thanks for everything so far.

Couple more questions, and hopefully I can print an awesome puzzle!

Alright, when I shelled a piece, a weird thing where the inside of the piece is transparent and the outside isn't. Weird huh?
Also, on some pieces, it can't shell. No errors pop up, it just refuses to shell no matter how much I click.
Next, tolerances just act to reduce the need for breaking in right? Could a puzzle be made smooth turning with zero tolerances and lots of break in?
Finally, for the typical M3 screw/bolt, what options should be selected in hole wizard?

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Mar 27, 2013 10:33 am 
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Good questions...
rubikcollector123 wrote:
Alright, when I shelled a piece, a weird thing where the inside of the piece is transparent and the outside isn't. Weird huh?

This actually happened to me once. What you can try is using the delete face feature to remove any excess faces or edges (these usually cause the bodies to shell incorrectly.) Insert->face->delete, then select "delete and fill" and then select all of the unwanted faces and hit ok. It will go from this...
Attachment:
face-1.jpg
face-1.jpg [ 190.87 KiB | Viewed 2200 times ]

...to this.
Attachment:
face-2.jpg
face-2.jpg [ 183.46 KiB | Viewed 2200 times ]

Also, be sure your fillets do not overlap, that also causes problems.
rubikcollector123 wrote:
Also, on some pieces, it can't shell. No errors pop up, it just refuses to shell no matter how much I click.

Same tips I mentioned above.
rubikcollector123 wrote:
Next, tolerances just act to reduce the need for breaking in right? Could a puzzle be made smooth turning with zero tolerances and lots of break in?

No, tolerances are important, because without them, the puzzle will jam constantly, and will be very hard to break in. Did you add any tolerances?
rubikcollector123 wrote:
Finally, for the typical M3 screw/bolt, what options should be selected in hole wizard?

For center pieces, select counterbore->ansi metric->hex head machine screw. For the core, select straight tap->ansi metric->tapped hole, then M3x0.5.
Good luck!

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Mar 27, 2013 12:09 pm 
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Hey rubikcollector123,

I'm sorry I didn't see this post until today. It looks as though many of the questions have been answered, but here's my method of making the core.

Eitan's Core Tutorial

1) When I make the sketches for my cutting surfaces, I always put a flat line about 4mm wide right before the axis of rotation (see blue highlighted line in image). This creates small flat dimples exactly where the screw holes will be.
Attachment:
Core Cleanup - 1 Flats.JPG
Core Cleanup - 1 Flats.JPG [ 121.59 KiB | Viewed 2186 times ]

2) Next, I make a 2.5mm through-hole for each screw.
Attachment:
Core Cleanup - 2 Holes.JPG
Core Cleanup - 2 Holes.JPG [ 77.52 KiB | Viewed 2186 times ]

3) Before I can shell the core, I have found that I have to get rid of those weird extra lines that show up on the core after the split. Since I also want to shrink the core a bit in the process of adding tolerances, I do a revolved cut like this to kill 2 birds with 1 stone.
Attachment:
Core Cleanup - 3 Revolved Cut.JPG
Core Cleanup - 3 Revolved Cut.JPG [ 103.71 KiB | Viewed 2186 times ]

4) Then I shell the BODY (not a face) of the core.
Attachment:
Core Cleanup - 4a Shell Feature.JPG
Core Cleanup - 4a Shell Feature.JPG [ 74.49 KiB | Viewed 2186 times ]
Attachment:
Core Cleanup - 4b Shell.JPG
Core Cleanup - 4b Shell.JPG [ 127.16 KiB | Viewed 2186 times ]

5) Now I can put holes in the surface of the sphere. This differs from puzzle to puzzle, depending heavily on the size of the core, the pieces that get close to the core, and how much effort I really want to put into it. I recall that Drew Cormier really liked to do cool patterns on his cores. Here, I'm just using some points and planes (reference geometry) to make an extruded cut out of the puzzle. I recommend giving the holes a diameter of at least 6mm.
Attachment:
Core Cleanup - 5 Outer Holes.JPG
Core Cleanup - 5 Outer Holes.JPG [ 122.03 KiB | Viewed 2186 times ]

6) Finally, I pattern the outer hole around, and fillet the edges to taste. (Not sure how necessary this is, but it makes it look awesome.)
Attachment:
Core Cleanup - 6 Hole Pattern and Fillets.JPG
Core Cleanup - 6 Hole Pattern and Fillets.JPG [ 105.56 KiB | Viewed 2186 times ]


Hope this helps!

-Eitan

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 Post subject: Re: Need help with solidworks.
PostPosted: Sun Mar 31, 2013 10:46 am 
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also You can see my: Solidworks Training model cube 3*3*3
viewtopic.php?f=9&t=19498

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 Post subject: Re: Need help with solidworks.
PostPosted: Tue Apr 02, 2013 6:15 am 
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Thanks pirsquared and grigr.
I have noticed that the holes you made do not seem to contain any threads. Do you actually have threads hidden somewhere inside or do you use the fact that screw threads are sharp to make the screw 'drill' its way through?

This seemed to be the case on my curvy copter skewb. Or the screws I used were wrongly labeled m3, or the core was a bad print..

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 Post subject: Re: Need help with solidworks.
PostPosted: Tue Apr 02, 2013 6:57 am 
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If you print the model using Shapeways nylon material, for "standard" M3 screw threads, if the holes are around 2.7mm diameter, the screw makes its own threads in the hole. As long as you have a deep enough hole and long enough screw, to allow for several turns of the screw, the resultant assembly is very good. The modelling of M3 threads in the hole is not necessary (and probably not possible, with the given accuracy of the Shapeways process).

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Apr 10, 2013 4:31 am 
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More problems D:

Image




All the areas denoted by red lines have 0.4 mm gaps for tolerances.. Is this ok? My concern is that the rightmost piece cannot be held in and may move upward. Is that normal? (This is the second shell layer by the way))

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Apr 10, 2013 6:49 am 
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Ah, tolerencing, this is indeed a thorny subject. I would read this thread and this one for a start.

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 Post subject: Re: Need help with solidworks.
PostPosted: Wed Apr 10, 2013 8:23 am 
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Like I mentioned before, I often use between 0.2mm-0.3mm total between surfaces (0.1mm-1.5mm per face) and while some will claim that this is too little, my philosophy is that you can always add extra tolerance to a puzzle (by breaking in, adding springs etc.) but remember that you can NEVER remove tolerance once the puzzle is printed. If the designed tolerance is between 0.3-0.4mm, the printer could accidentally add too much tolerance, up to 0.1mm inaccuracy (it isn't a perfect process, you know) and could make a puzzle potentially looser than it should be, even though in theory it would work perfectly. I add smaller tolerances like I previously mentioned to be on the safe side.

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 Post subject: Re: Need help with solidworks.
PostPosted: Fri Apr 12, 2013 6:44 am 
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One last question:

How do I compact the parts together so the bounding box discount whatever thingy applies? So excited!!!

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 Post subject: Re: Need help with solidworks.
PostPosted: Fri Apr 12, 2013 7:55 am 
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Well, this depends on the puzzle design. What I do is put all of the volumes of the parts into a spreadsheet, which gives me an idea of the maximum size of the required bounding box - see the attachment.
Attachment:
File comment: Shapeways Calculator
Shapeways Calculator.xls [23 KiB]
Downloaded 28 times
Now, I find that the simplest way is to pull all of the parts apart by 2-3mm (although I think that about 1mm distance is the minimum) to "explode" the puzzle. If you are lucky, the result will be less than the size of the maximum bounding box to give you the discount.

If this does not work, you may have to manually arrange all the parts to maximise the packing density.

If this is not enough, you can include "dummy" parts which fit in otherwise unused spaces which will increase the density over 10%. You have to pay extra for the dummy parts of course, but if if this gets you the discount this is usually more.

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 Post subject: Re: Need help with solidworks.
PostPosted: Fri Apr 12, 2013 7:59 am 
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rubikcollector123 wrote:
One last question:

How do I compact the parts together so the bounding box discount whatever thingy applies? So excited!!!

This is my favorite part! I usually pack all of my pieces tightly together in one .stl file, to save a buttload of money. Remember though that the triangle limit for Shapeways is 1 million, so be sure your model is under that amount. To pack pieces tightly, I often use a scaling technique. I insert a scale feature, then scale every part down by the centroid, usually by an amount between 0.8-0.6 of their original size (you want the parts separated by about 2-1mm apart). Then after that scale is applied, I then scale every part back up from the origin. Take 1 and divide it by your original scale-down factor to get your scale-up factor (try to avoid irrational scale factors if you can). Then scale every part back up by the origin, and instantly all of your pieces are separated out for printing! After you upload to Shapeways, you're ready to print! Good luck!

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Last edited by benpuzzles on Sun Apr 14, 2013 2:58 pm, edited 1 time in total.

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 Post subject: Re: Need help with solidworks.
PostPosted: Fri Apr 12, 2013 8:56 pm 
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Yes I am making one.

Not quite though. If it was exactly that, piece proportions would be weird.

I hope you aren't making one. :lol:

Though that hint picture doesnt look like it.

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