broken 1/16th endmil in 1/8' acrylic

[iSign]

I used 2 passes, 150 IPM feed, 60 IPM plunge, and 18000 rpm spindle..

I also used a 3D "line in" in enroute (meaning the bit plunges & begins to advance simultaneously, instead of drilling a hole and trying to advance against the full depth from a dead stop...

as you can see in the pics, I made it through several pieces, but 80% of the way to completion I broke another tool...

any suggestions?

 

[Jet Fast Printing]

Have you tried calling Onsrud directly? I had issues just like yours before and they had me slow it down and wa-laa stopped breaking bits.

800-234-1560 <----- Onsrud

 

[signmeup]

I have no router so take this for what it's worth.. could spinning something that small, that fast, snap it if it was even the tiniest bit out of balance? If it went harmonic it would dissappear, I would think. Again, I have no idea how much would be sticking out of the collet.

 

[Typestries]

For a 1/16th bit I think your feed rate is waaaay too high even for 2 pass cutting. Like 100 too high, as is the plunge.

It could also be a vibration issue. Any chance the piece is vibrating as it's cutting, small bits are very susceptible to vibration breaks.

Reducing the speed to something like 30 ipm might also reduce potential vibration.

Do they break in the same spot on the shape?

 

[J Hill Designs]

also, I would never use a 1/16th bit in 1/8' (1.5") acrylic

haha j/k

 

[GB2]

I agree, way too high feed and plunge rate, everything else seems OK though. Those bits get expensive fast don't they?!

 

[m giese]

Cast or extruded ACR?

General rule of thumb with acrylic cutting is the cut depth/pass should be half the d of the tool.

I have found that a plunge rate of 15-20, and a feed ipm of 120-140. At slower speeds I start to have reweld issues.

The other factor that can come in to play is acceleration rates. Too high, too much stress on the tool

The key to the small d tools seems to be in minimizing the stress on the carbide by cutting down on the pass depth.

Of course, a larger d tool couldn't hurt, but I assume you choose the 1/16 tool for a reason.

 

[m giese]

Just looked at your images, couple of thoughts...

if you are cutting w vac hold down, you may be getting to much vibration and movement, as another poster suggested. based on the close proximity of the newly created holes, ie part to part distance. Hold down looks better near the beginning, and becomes an issue farther down the nest.

For the delicate work, switch to paper masked material instead of the film, doesn't wrap up around the tool, and stays in place until you choose to remove it. Use the 1/16 bit for the inner, smaller geometry, and switch to a .125 end mill for the outer geometry, obviously changing your tool paths, and last but not least when using the 1/16 to cut the inner geometry, keep the kerf cleaned out with some air, particularly on the subsequent depth passes.

 

[signs2trade]

Good suggestions here.

You may also try maxing out the RPM of your spindle. The faster you spin the smaller bits the stronger they effectively become.

 

[iSign]

Thanks for the tips guys...

I assumed the 1/8" tool would spoil the detail, but it actually didn't compromise the design nearly as much as I thought... But more passes, with slower feed and faster rpm is my lesson here...

The words "acceleration rate" was used, below mention of feed rate by the same person, what does that mean, if not the same as " feed"

 

[m giese]

Acceleration rate is the rate that the tool accelerates in movement from the initial plunge, if you are not using ramping. IE, tool plunges at entry point, and then accelerates to feed speed, decelerates at direction changes in geometry. May or may not be a setting you have control over, but high acceleration rates contribute to tool breakage, especially with smaller diameter carbide bits.

If you need any spare packaging for those 63-700's I have a few you could add to your pile...

- Mark

 

[iSign]

Acceleration rate is the rate that the tool accelerates in movement from the initial plunge, if you are not using ramping. IE, tool plunges at entry point, and then accelerates to feed speed, decelerates at direction changes in geometry. May or may not be a setting you have control over, but high acceleration rates contribute to tool breakage, especially with smaller diameter carbide bits.

If you need any spare packaging for those 63-700's I have a few you could add to your pile...

- Mark

Thanks Mark!

I use Enroute 4, and I don't remember noticing acceleration adjustments, but that makes sense that it doesn't hit top speed from the get go, and also makes sense that having control is a good thing... so I'll expect to find it now that i plan to look...

regarding the packaging... glad to hear I'm not alone building up a little stack... just think, soon we'll have enough to recycle into justifying one more bottled soda consumption!

 

[Design4cnc]

I know this is very late to the post date but your accel speeds would be in actual router settings or in router post. What kind of CNC do you have?

 

[iSign]

Hi D4CNC,
I have the Multicam 3000 series

 

[k.a.s.]

I have had zero success with 1/16 inch bits, if it cant be done with an 1/8 it needs to be done on a laser. JMO


Kevin

 

[astro8]

Your speeds were far too high, about x5 too high! Those little bits even though spinning at 18000 rpm don't have much surface speed at the cutter. If you have a mister it helps to blow just the air over the tool on acrylic but with water will give you a better edge.

We do a fair bit of cutting with 1/16" bits on our router, aluminium, brass, acrylic, mdf, acp. Even taking all precautions, ramp ins, acceleration adjustments, they don't last all that long...buy them in boxes of 50 at a time.

 

[daveb]

I used to use 3/32'' bits for cutting small stuff, tried 1/16'' and ran through a ton of them and then Hartlouer suggested using the 3/32'', worked like a charm. I was routing 080 alum. faces which is probably a lot different than what you're doing. You do however sacrifice a "little" detail. Always talk to your supplier, they know their product and should be able to point you in the right direction. Hartlauer was always very helpful, of course it has been several years since I was in the router room full time but I don't think much has changed.

 

[88flstf]

try this

I had a lot of 1/16" bits break... just look at them at they break. Then Hartlauer suggested that the problem was the 1/4" shank and so I switched to the 1/8" shank with a 1/8" collet and presto... no more broken bits. They just get dull now. But you still have to run and plunge quite slowly even with running at 24,000.

 

[iSign]

boggles my brain how much I have to learn...

but it's a pretty mind boggling reality how much information is available to learn here... so, one day at a time...

by the way, what those cuts were for is a little side project I started fitting in after other router jobs were getting done over a few weeks time... I decided to invest 3 or 4 square feet of each of several materials, including even some Koa exotic hardwood material I ran through a planer... and I came up with a few dozen material sample fandecks to use as a sales tool with the highest end clients like resort properties, as well as for possibly branching out into offering wholesale services to my competitors.

Anyway, here are the finished products:

 

[Mainframe]

Cool sample, I like it, nice work!