[tkubic]

Gotta cut a bunch of holes in a bunch of boards for holders. I raise the boards off the table to allow the round scrap piece fall without interfering with the rotating bit.



The problem I have is sometimes the bit catches the falling part and binds causing steppers to stall and sometimes parts flying across the room. I would like a more robust machining process that won't result in stepper stalling and part destruction.

I thought about doing a drilling process first and dropping dowel pins to keep the slug from getting caught.

What does everybody else do when machining out slugs?

[ger21]

I can't see how a bit can get stuck in the hole from the cutoff piece? What material are you cutting? What kind of bit, and what size hole?

[txcncman]

In the metalworking world, we would take a little extra time and machine away the inside material, turning it into chips, thus nothing to drop out or bind a cutting tool. Even if you just machined away and extra 1/4" per side, it would likely stop your problem.

[tkubic]

in the final pass sometimes the cutting force breaks the slug out before finishing the pass. The bit then hits the free slug and bounces it causing it to lift sideways and thus binding in the hole between the bit and the side wall. i recall reading about people cutting out the puzzles and having parts fly across the room

[ger21]

I've had that happen lots of times, but the bit has never gotten caught at all, as it usually just takes a big bite out of the slug while throwing it out of the way.

[louieatienza]

In the metalworking world, we would take a little extra time and machine away the inside material, turning it into chips, thus nothing to drop out or bind a cutting tool. Even if you just machined away and extra 1/4" per side, it would likely stop your problem.

I agree. I now pocket out all my holes in aluminum over 1/4", even large holes. Sometines this is actually faster than doing a profile cut.

If you must profile cut for some reaon, I'd do a profile cut a percentage away from the cut line, and leave a skin so the slug doesn't fall. Then cut the profile; this will give the bit some clearance. If the hole is less than 3 times the bit diameter, you could just drill a hole in the center before profiling. If the hole was less than 2 times the bit diameter you obvously don't need to drill a hole; the profile cut will cleat out the hole. You could also try a down-spiral bit; it may help push the slug down instead of up.

[Walky]

I agree that pocketing is the way to go, I started doing that after getting the bit caught with the inside piece a couple of times.

BTW, for big irregular shapes with small, semi closed features, I sometimes add a small auxiliary vector to previously pocket critical parts that would otherwise leave small dangerous pieces floating, to avoid having to pocket the entire big vector.

[RomanLini]

I cut with two circles, first the inner circle (maybe 1mm to 2mm smaller) and last the outer circle, and leave a thin skin at the bottom maybe 0.5mm to 1mm thick (depends on material).

Then the final cut that removes the slug is only through a thin skin at the bottom, and is the outer circle size. Then because the slug is smaller than the outer circle there is very little grabbing and the slug just sits loose in the bottom of the hole.

The two curcles gives a better finish in the wall of the hole too.

[tkubic]

sorry i should of provided more info, these are 1.75" diameter holes in 1/2" HPDE. 21 holes per sheet. 29 sheets to do lol.

Pocketing the whole feature would make an extremely large mess and also be very time consuming.

Cutting a smaller hole and leaving a skin then doing the edge sounds like i may be the way to go.

With 609 holes to cut i wanted something that wouldn't take too much machine time. I didn't know if there was some sort of industry standard for this type of thing or if people just have their own kinda thing for doing it.


Thanks to everybody that has replied so far.

[louieatienza]

sorry i should of provided more info, these are 1.75" diameter holes in 1/2" HPDE. 21 holes per sheet. 29 sheets to do lol.

Pocketing the whole feature would make an extremely large mess and also be very time consuming.

Cutting a smaller hole and leaving a skin then doing the edge sounds like i may be the way to go.

With 609 holes to cut i wanted something that wouldn't take too much machine time. I didn't know if there was some sort of industry standard for this type of thing or if people just have their own kinda thing for doing it.


Thanks to everybody that has replied so far.

What size is your collet? Amana makes a 1.75" straight bit with a 1/2" shank, center cutting, and you could do the hole with one plunge.

[tkubic]

using an m12vc router. with a 1.75" bit i think it would take a bit more horsepower than I have and also likely lower rpm then what it is capable of.

I am hoping I can fixture this correctly to make it a robust process that doesn't need to worry much about those silly slugs.

I don't necessarily need to optimize the time taken per hole I suppose, but if I can reduce it from pocketing greatly that would be favorable lol.

This is also an issue for me when doing other processes that aren't just these 1.75" holes, the whole bit catching and flinging problem has bothered me for some time, ever since I started destroying 3d puzzle pieces from odd flinging parts

[louieatienza]

using an m12vc router. with a 1.75" bit i think it would take a bit more horsepower than I have and also likely lower rpm then what it is capable of.

I am hoping I can fixture this correctly to make it a robust process that doesn't need to worry much about those silly slugs.

I don't necessarily need to optimize the time taken per hole I suppose, but if I can reduce it from pocketing greatly that would be favorable lol.

This is also an issue for me when doing other processes that aren't just these 1.75" holes, the whole bit catching and flinging problem has bothered me for some time, ever since I started destroying 3d puzzle pieces from odd flinging parts

If you have your work raised off the table, and use a downspiral bit, it should push those slugs down toward the table instead of up and away!

The slick way if you had to make a ton if these would be to make a vacuum fixture; you could use o-rings as seals for the slugs.

When I worked for an interior sign company we used an old NewHermes engraver (now GravoGraph). It had a vacuum table which was basically a grid, with a rubber gasket with holes in it. It probably wouldn't be hard to make such a thing, and you could just change the gasket for different jobs.

[JerryBurks]

I usually route a 5mm hole in the middle first and use a screw to hold the future slug down on the wasteboard. When the bit breaks through the slug sometimes spins around the screw but does not bounce around.

But I see that may be a chore with 609 holes.

Depending on the accuracy of you part cutout you might profile the hole down to an thin layer and then flip that plate to finish the cut from the other side with a mirror image tool path and maybe even a smaller bit.

[jjacstcy]

Add a few bridges to hold them in place. Pop them out when your done cutting.

[louieatienza]

There's another idea: Profile as normal, leaving two tabs about .02" or so, 180 degrees apart. Then take the same bit and plunge down to cut the tabs off.