[CLP CORP.]

I'm having an issue with snapping bits on my cnc router. Working with 3/4" boards, typically MDF, melamine or plywood, 1/4" solid carbide bits, 1/4" depth per pass. I believe it's an issue with the speed and feed rates. Currently set at 20,000 rpm. I'm finding conflicting info on recommended feed rates and as the problem is still occurring I am obviously doing something wrong. Any input would be appreciated. Thanks.

[CNC_BOB]

how many flutes? what feedrate are you snapping off at? I have milled a good amount of wood and it can get hot if spindle speed is too fast. is 10000 RPM an option? if so, 60-80 IPM seems a good starting point. most of my experience is pine mounting bases for a taxidermist. hope this helps

[CLP CORP.]

Two flutes. Feed rate was originally at 300ipm & 20,000rpm. Slowed it down to 80ipm at 18000rpm and snapped another bit. Sounds like I should have decreased the rpms along with the feed rate?

I've also heard that going too slow will cause heat build-up because the bit is remaining in the same spot for too long?? (like I said - I'm finding conflicting info)

Appreciate any ideas you've got. Thanks Bob.

[ger21]

What kind of bits are they? Spiral? Straight? What brand?

[the_paco]

You are cutting in a single pass?

Is that a carbide tipped tool or solid carbide and as Gerry asked, is it spiral?

18 000 and up is way too fast a RPM if you ask me...

[CLP CORP.]

All bits are Amana, solid carbide, most often spiral but I've also used straight cut.

Cutting in three passes. 3/4" material, 1/4" depth per pass.

[bradyfb]

Hey hows it going? Just a few questions; #1 When your bit breaks is it about 1/8" to 1/4" inch from the collet (the break)? #2 If you were to put your dail indicator on the bit and zero it then push on it how much play is there?

[ger21]

What kind of spindle is this?

Do the bits break when new, or after you run them awhile? If a while, about how long? Are they getting dull before they break? And where exactly do they break? In the middle, at the collet?

I'd recommend trying a 3 flute, like the Vortex 1830 If you buy four or more, you get 30% off the price shown. I've been using them for almost 10 years, and have never broken one.

[the_paco]

I'd say it's being fed too slow and it turn too fast... it's most probably getting burning hot.

Those three different material mention above doesn't cut the same. MDF and particulate board could be cut at 120"/min. at 14 000 RPM with a stepdown (pass depth) of 0.25". Plywood on the other hand can be much more harder. Slow it down to 90"/min.

A strong hold down is important as chattering could easily break a such small tool.

Have you considered a larger CED (diameter) tool such as, say, 3/8"?

Keep us post.

[CLP CORP.]

Unfortunately I don't have a dial indicator & I'm not sure what kind of spindle - it's a Gerber Sabre CNC.

The bits are breaking when new, no chance to get dull, breaking in the middle (about 1/4"+ from the collet). Could the bit be too long?

Maybe this is part of the problem?... The Amana bits I'm using are longer. for example - 3" long with a 1-1/2" cutting depth. I'm only going through 3/4" board, at 1/4" depth per pass. Should I be getting a bit with only a 3/4" cutting depth, or less because I am making several passes? Do I need to make that many passes?

I was initially using Gerber bits which are shorter.. 2" to 2-1/2" with only a 1/2" cutting depth and I'm thinking now that I don't remember ever breaking any of those.

Ger21 - Three flute sounds like a good idea and I appreciate the link. How long do they take to deliver? You've been in this for a while, what kind of material are you cutting and at what speeds/feeds?

I'm going to give a 3/8" bit a shot too.

Thanks to all for your help!!

[ger21]

Vortex is very quick, and they'll overnight them if you need them to. We cut MDF, Particle board and plywood. With a 1/4" bit, usually around 200ipm at 18K rpm. If you can use a bigger diameter tool, I'd do that. But you shouldn't be breaking bits at only 1/4" depth of cut. Guys cut through 3/4" Particle board at 900+ipm with 1/4" compression bits

[CLP CORP.]

While I'm troubleshooting, perhaps someone has advise on a solution to one other problem I've come up against?

In routing white melamine board I can't seem to avoid the material chipping along the cut edges. I've tried one and two flute bits, straight and spiral. Neither is better than the other. Would a down cut bit make any difference? Would adjusting the speeds help?

[the_paco]

Yup, 1-1/2" CEL (cutting length) is too long for your application. You need to be very gentle with such long tool in hard material (pretty much anything else than foams).

I'd use no more than 1" CEL or better yet 0.875".

If you go with the 3/8" CED, you still want to keep the CEL as short as possible.

[the_paco]

I cut melamine with standard router bit. 2 straight edges carbide tipped. Again, as short as possible. So far, I mainly use 1/4" CED X 3/4" CEL to do both the cut, dados and the holes. 14 000 RPM at 240"/sec. with a 0.375" stepdown.

Clean cut up to 30 sheets. The only small chipping I have is when "drilling" through for the middle section shelf holes.

Hold down for me a one or two clamps at end and vacuum mainly. The clamps are for the few last parts.

[ger21]

While I'm troubleshooting, perhaps someone has advise on a solution to one other problem I've come up against?

In routing white melamine board I can't seem to avoid the material chipping along the cut edges. I've tried one and two flute bits, straight and spiral. Neither is better than the other. Would a down cut bit make any difference? Would adjusting the speeds help?

A downcut bit would work, but they dull quickly. I use an insert 1/2" straight bit for that, or a 1/4" downcut spiral if the 1/2" is too big. I also use 1/2" compression spirals if I'm cutting all the way through.

[CLP CORP.]

Ger - Thanks again for all the info! I'm going to assume those speeds are for three flute bits, yes? Do you make any adjustments based on the material your cutting?

Another question, if I were to use a 3/8" bit would I then have to slow down the settings?

I also cut corian on occasion, with this would I slow it down as well?

[ger21]

I'd go faster with a larger tool, and lower the rpm. I cut corian with 1/2" tools, and with a good sharp tool, you can cut corian very fast, 400ipm at 15,000 rpm with a 3 flute 1/2" tool.