broken carbide end mill.

[ihavenofish]

so, my latest adventure was getting some help making a cam program to cut out some vise clamps in 1018 steel.

i ran a program in steel - hand coded - as a test. it worked well, the slotting seemed to wear the bit tips down, and after some research, should have been done at 1/3 the rpm than the side cutting, 1/2 the feed, and 2 or 3 times the depth i was doing. all made sense to me. did some manual test cuts in the same scrap of steel, all was looking good. was taking side cuts at 15ipm, .01" width and .625" depth, and they worked great. im using a 1/4" carbide 2 flute bit.

so today i ran the cam program. the first level was .08" depth, .035" step over, and 12 ipm and 5000rpm. it made a bit of noise doing the helical plunge at 5ipm, and then cut as expected. i should note that the cutting path was trocoidal so there was no slotting, and the stepover was no to excede .035". analyzing the tool path showed this was the case.

level 2 was .3" below the first. stepover the same, speeds the same. helixed in and began to cut. worked fine for a few seconds and the bit snapped clean.

so, now i want to know why?
the bit had one chipped point, and one good one after the break.

i was not using coolant, as in the tests it seemed to work best with none.

what normally causes bit breaks in an otherwise "correct" cut?

[Geof]

I think your rpm was too low, your stepover too large, possibly your depth of cut a bit large and you should be using four or five flute TiAlN coated with an airblast.

We have discussed trochoidal elsewhere, yes(?) and I have mentioned my pseudo-trochoidal with a 1/2" cutter running at 6000 rpm (I think) with a stepover of 0.025". To equal the peripheral speed I used your cutter needs to turn at 12,000 rpm which is probably impossible. When the cutting speed is not high enough you don't get the same heating in the chip which reduces the tensile strength of the steel in the cut.

Couple this with only two cutting edges so your chip load per cutting edge is higher than would be the case with four or five flute and the fact that a two flute cutter does not have as much meat in its cross section as a four flute.

There are plenty of reasons why you had the potential or predisposition for the tool to break.

[Superman]

Originally Posted by ihavenofish the first level was .08" depth, .035" step over, and 12 ipm and 5000rpm. it made a bit of noise doing the helical plunge at 5ipm, and then cut as expected. i should note that the cutting path was trocoidal so there was no slotting, and the stepover was no to excede .035". analyzing the tool path showed this was the case. level 2 was .3" below the first. stepover the same, speeds the same. helixed in and began to cut. worked fine for a few seconds and the bit snapped clean. what normally causes bit breaks in an otherwise "correct" cut?

The cuts were not the same
level 1 was at 0.08" DOC, & no walls to keep chips near the tool
level 2 @ 0.3"

2nd pass was 4x the depth, and the feed should be dropped down to take into account the extra cutting forces, plus a wall the chips now have to clear

you said "no coolant" , are you using air to get the chips out ? , don't allow to "re-cut" the chips, this is the main cause of premature tool wear and chipping on the cutting edges, once that point goes, the pressure on the tool goes off the scale- result = snappo

The air will also allow cooling of the tool

[ihavenofish]

Originally Posted by Geof I think your rpm was too low, your stepover too large, possibly your depth of cut a bit large and you should be using four or five flute TiAlN coated with an airblast. We have discussed trochoidal elsewhere, yes(?) and I have mentioned my pseudo-trochoidal with a 1/2" cutter running at 6000 rpm (I think) with a stepover of 0.025". To equal the peripheral speed I used your cutter needs to turn at 12,000 rpm which is probably impossible. When the cutting speed is not high enough you don't get the same heating in the chip which reduces the tensile strength of the steel in the cut. Couple this with only two cutting edges so your chip load per cutting edge is higher than would be the case with four or five flute and the fact that a two flute cutter does not have as much meat in its cross section as a four flute. There are plenty of reasons why you had the potential or predisposition for the tool to break.

eep. information overload!

1/4" at 5k rpm is 327sfm. thats the lower end of the tool makers recomendations. high end is 600. i dont have an air blast, but indeed the tool and workpiece were very hot after the break.

it does seem logical to think that in my earlier tests, which were short and interupted, the tool didnt heat up the same as after 9 minutes of continous load.

on a future run then, a 4 flute at 15-20ipm, with a .02 stepover. at the lower speed range, would a mister be more useful than an air blast? i cant run flood coolant or the like due to the location of the machine.

i really have a genetic gift for breaking tools




on the bright side, i seem to be learning alot on the whole textbook vs real life thing. real life is more complicated - and expensive.

i suppose my airbrush compressor (to be used with a mister soon) wont cut it for air blast? its 25psi continuous at whatver cfm and iwata airbruch is (less than 2 i think).

[ihavenofish]

Originally Posted by Superman The cuts were not the same level 1 was at 0.08" DOC, & no walls to keep chips near the tool level 2 @ 0.3" 2nd pass was 4x the depth, and the feed should be dropped down to take into account the extra cutting forces, plus a wall the chips now have to clear you said "no coolant" , are you using air to get the chips out ? , don't allow to "re-cut" the chips, this is the main cause of premature tool wear and chipping on the cutting edges, once that point goes, the pressure on the tool goes off the scale- result = snappo The air will also allow cooling of the tool

sorry, guess my scambled post wasnt clear enough. yes, the first pass was .08, second .3. but i had already tested the .3 cut previously with much success. the top cut was tested fine with a .08 stepover, but the code made it all uniform.

heres the test (with slotting).

YouTube - kx1 cnc milling vise clamp in 1018 steel

YouTube - kx1 cnc milling vise clamp in 1018 steel

.
might want to turn the volume down, video turned out very loud for some reason. not that loud in real life. the "chirping" half way through is workpiece vibration - that got fixed in the "real" run.

as for recutting, there shouldnt have been any, this is an open contour, not a pocket. all the chips were flying away. the helical plunge is pointless in the code really - i dont know why its there it would have been better to come in from the side. perhaps that can be edited for a future version.

i agree though that i should rig up and air blast.

thanks for the suggestions.

[Geof]

25 psi should be okay provided it has enough volume to maintain that pressure through a 0.1" dia orifice.

I can reduce the information overload:

Use a four flute cutter, coated as I said with TiAln and run the speed up as close to 600 SFM as your machine can get.

Question: how much cutter was sticking out of the holder? Quarter inch dia cutters are not strong and if you have an inch or so of shank sticking out you can snap off the cutter under conditions that would be fine with only 1/2" out.



EDIT:

I looked at your video. how wide is the slot? It looks a lot wider than 1/4", why are you not using a larger cutter.

Incidentally did I ever give you the link to my videos?

[dertsap]

looks to me your burning up the tool , the heat is apparent when you give a spray of coolant and there is a puff of steam

[ihavenofish]

Originally Posted by Geof 25 psi should be okay provided it has enough volume to maintain that pressure through a 0.1" dia orifice. I can reduce the information overload: Use a four flute cutter, coated as I said with TiAln and run the speed up as close to 600 SFM as your machine can get. Question: how much cutter was sticking out of the holder? Quarter inch dia cutters are not strong and if you have an inch or so of shank sticking out you can snap off the cutter under conditions that would be fine with only 1/2" out. EDIT: I looked at your video. how wide is the slot? It looks a lot wider than 1/4", why are you not using a larger cutter. Incidentally did I ever give you the link to my videos?

ive seen youre videos. they gave me some of the ideas for what i was trying.

so lets see....

- top speed on the machine is 5000rpm, so with 1/4" its 327sfm tops. true speed under load is probably more like 300sfm as well.

- the slot in the video is .27" wide at the bottom (.61" deep), but .5" wide at .375" deep. the cam program has allowed more space in the slot at the bottom, about .35" for the trocoidal pattern.

- the end mill was sticking out a hair under 1", the cutting flute length was .76" on this end mill.

- i actually had a niagra 5 flute tialn cutter. i broke that crashing into 304 stainless at rapid speed! grr. it cut amazingly well while it lasted.

at the moment im mostly just playing and learning, so im buying one end mill at a time. i think once ive got a handle on all this, ill buy a bunch and get some real work done. its really only steel thats giving me a hard time. i use m42 3 flute cutters in aluminium with a dab of coolant and it runs like butter.

[ihavenofish]

Originally Posted by dertsap looks to me your burning up the tool , the heat is apparent when you give a spray of coolant and there is a puff of steam

in the slot, yes, thats exactly what it did. if you watch the chips, you can see they are silver on the side cutting, but black/blue in the slot. too hot. very bad.

that was th etest though, the cam run didnt have this issue, however the workpiece and tool still got very hot.

[ihavenofish]

so i tore the machine down for cleaning and adjustments and to measure something for a modification.

while i was at it i measured spindle runout. .002" about 1/2" from the nose. that cant be right... id measured before and there was none measurable on my indicator. so i took the tool out and went about cleaning, and this morning measured the taper... dead on.

tool back in... .002"

damned POS collet!

so do you think .002" runout on a 1/4" carbide 2 flute bit in 1018 cold rolled steel is enough to case the tool to break? thats basically pulsing the tool to cut .003" on entry at one tooth instead of .001" per tooth. i think that could easily explain breaking on a trochoidal cut but not others.

yes, no, maybe?

[ihavenofish]

success!

well, maybe. i went through the machine (tore it apart actually) and cleaned and tightened everything. i found a flaw on my z axis that was making it rock on a short section of it - basically ways werent 100% parallel. gave it a bit of a scrape and overtightened the gibs. z axis rapids got knocked down due to lack of torque but everythings tight. i reseated the collet and its got slightly less runout now. still needs to be replaced though.

overally, the machine now had only a few thousands of flex under normal cutting loads in any direction and springs back when no force is applied.

loaded a new 1/4" TiAlN coated 2 flute ball end mill and my steel bar. the end mill is all i happened to have, im ordering some 4 flute ones today. i also poured a little coolant on the workpiece.

spindle at 5000 rpm, feed at 8ipm, depth at .25" (including ball) and about .08" width. this wast the heaviest cut... i worked my way up from lighter width ones.

result, a flawless cut, very little noise, no chatter, silver chips, and a flawless finish. on top of that, a second "spring pass" showed the cut was actually accurate - nearly no tool deflection. it was not like this before at all even on lighter cuts.

so i think theres a few factors here:

1 - more rigid machine, less chatter, better cut, less deflection, no broken bit.
2 - TiAlN bit plus coolant - less heat, better cut.
3 - ball nose bit - no sharp points = less cutting stress maybe and less prone to breaking and chatter?

if thats correct thinking, would it make sense to do the rough pass with a radiused corner TiAlN 4 flute, and only run a sharp corner bit for finishing where its needed?

im pretty happy with this test though. proves to me that the machine is quite fine for steel... its only my skills that suck.