puzzle joint

[don62]

i have an older prt96 with the 4g upgrade. works just fine except when making puzzle joints - that is when runout shows itself. specifically there are severe gaps between curves of the two pieces. have tried slowing cut speed and doing final cut of say .01 - neither works effectively - should add that i work primarily with corian - wondering if anyone has tricks of the trade on how to make these joints

[steve_g]

Don…
Are you sure it’s the machine showing its age or is it possibly a router bit diameter issue? Have you tried making the part toolpaths using the “inlay” feature of VCP?
SG

[Mike Windsor]

I have a unistrut machine and make puzzle joints for kayak panels . I offset one side about .010 in the cad program . The joints are not perfect , but the epoxy fills any voids .

[don62]

i am feared it is the machine. probably need to tighten up the z axis. the way i design them is to draw the curve then offset to either side for the male and female peices. i then do another offset for the rough cut and then another for the final cut. my goal is to have the two pieces as separate pieces yet have a nice to look at joint. attached is a sample of what i do - there are 4 pieces to this puzzle - the joints are pretty good, but it is trial and error - you basically get one try - if it does not work, start with a new piece.

[bleeth]

Although I haven't done puzzle joints in Corian I have cut a lot of it where pieces need to align perfectly. I use a straight single flute o-flute, ramp in, take 2 passes leaving a skin on all parts, and then a final pass cutting all through. I don't use an offset allowance at all. I learned that this gives me the smoothest edges and the parts fit great. When the part (and for drop edges these are pretty skinny parts and for radius corners they are pretty small) gets the final cut they don't move or jump at all. I've used it for making large curved counters and curved drop edges where the curves were so large that several pieces were needed either due to the overall size or just getting efficient use of the material.

[don62]

Dave, i like where you are going - i have used my general cutting bits and have not focused on the quality of the cut. looking at onsrud i found a 65 series bit (65-033 specifically) that talks of a polished flute that 'allows razor sharp cutting edge' - this series usage includes solid surface - this is a spirala bit, not straight. they have a straight bit (56-450 double edge solid carbide) that cuts solid surface. is it your finding that the straight bits makes a smoother cut than the spiral?

[bleeth]

I have used both and find that at that last moment when the part is being cut away from the nest I get less movement of the part. They both leave a pretty nice surface with the right strategy, definitely good enough for joining with a minimal of sanding.

[don62]

okay, just had an informative conversation with Gary at Onsrud and have ordered the 65-023 single edge - solid carbide upcut spiral o flute. new to me was his direction that the length of the cut (CEL) should be close to the thickness of the material you are cutting. that if the CEL is considerably longer that the thickness of the material the upper edge cut will not be as smooth. that means a 1/4 CED bit with a 5/8 CEL will cut a better edge on 1/2 material than a 3/8 CED bit with a 1-1/8 CEL. very interesting. he also stated key is for a constant feed rate, cut conventionally and if desired do a 0.02 offset for a final cut. since i will be cutting at a slow feed rate, reduce rpm to 6k. got a bit coming this friday and will try it out over the weekend

[bleeth]

That is a good bit but it is also very tender. Be gentle with it! I wouldn't go all the way through in one pass for anyone. You should get an acceptable finish in 2 passes without doing an offset, although, based on being gentle and not wanting to buy too many of those expensive bits I do usually run two passes leaving a skin and then a final skin. Always ramp in. I run around 1.5ips and 8k.

[don62]

Dave, i hear you and i am prepared to go slow and easy. but i found this little video on youtube http://www.youtube.com/watch?v=wqbV8Em62wA
it show the bit cutting half inch corian at 180 ipm with router speed of 18k. and with no dust collection. interesting. btw appreciate your valued input. Don

[bleeth]

I wouldn't cut that way on a Shopbot. That had to be a servo/ball screw/linear rail machine.
I wonder what their holdown method was? I can't imagine those parts not jumping at the end of the cuts unless they were glued down with 2 faced tape all over or something.

[don62]

Dave, got the bit and tried out - here is pix of second test cut - cutting on either side of the line - no offset. two cuts -.25 and -.4. the run out is totally acceptable.the joint is actually a little loose - might do another test cut with a negative offset. looks like the router bit did the trick. again thanks for the help. don

[bleeth]

Glad it's working out.
BTW I guess you have followed up on checking all for tightness and square by now. If it's been a while I would inspect the pinions for wear. Also If you're running a spindle it could be time for a new collet and if it's a router you might look into the aftermarket collet that reduces runout on them.

[don62]

have done a visual and have found no obvious play - am using pc with relatively new collets. looking closely at the joint i see no obvious runout like i did before - the bit seems to cut easier. the joint is loose, but it is so close to a perfect fit that i am hesitant to make much change. i have several puzzles i need to make, so i plan to do another test and compare to the fist test, then decide if i tighten the joint

[jerry_stanek]

Check out precision bits have good collets with little runout