[1875]

Hi Folks,

Trying to figure out why my cutter broke. I was cutting a steel plate, basically like an o-ring groove on my Bridgeport mill. The steel came from a piece of 12"x12" angle bracket used to mount file cabinets (so I do not know exactly what metal it is).

I made an Excel spreadsheet to help me figure out my feeds and speeds, and this is what I had set-up for the cut. It starts cutting the first arc at the surface of the steel. Right at the end of the first arc, just as it was going to start the second pass, the end mill shattered.

I was hand blowing air to clear chips and brushing on cutting oil.

Cutter Diameter= 0.25" carbide
Flutes= 4
SFM= 98.25
RPM= 1500
Chip Load= 0.00117"
IPR= 0.00467
IPM= 7

...
G00 X0.000 Y0.625 Z0.020
G1 F7
Z0
(CCW circle)
G03 X0.000 Y0.623 Z-0.070 I0.0 J-0.623
(end mill snaps about here)
G03 X0.000 Y0.623 Z-0.140 I0.0 J-0.623
...

I did have my feed at 17% over the ideal setting of 6.1 IPM. Is it likely this sensitive or more likely a chip lodged or other fluke, or something else I should have known?

I installed a new (used) end mill and picked up the program at 50% feed, then bumped it to 80% to finish the cut to full depth of 0.470" without any issue.

According to my spreadsheet, I could run this cut at 4500 RPM and 18 IPM, depending on what I pick for SFM (which I was using 100).

Thanks.

[CitizenOfDreams]

I'm not a g-code expert, so forgive me for my naive question... During the transition between the first circle and the second circle, at what speed does the tool plunge from Z=-0.070 to Z=-0.140? Feed speed or rapid speed?

[1875]

I'm not sure how the controller interprets the feed in 3 dimensions, but the cut is a continuous downward spiral. I am also not sure if there is a very slight pause at each line though. This would have the end mill cutting 0.070 deep, then stop, then pop back into motion against a 0.070 cut. That does not seem logical though.

[CitizenOfDreams]

I see. I guess it depends on the controller, but theoretically it should be one smooth continuous motion with no pauses or plunges. At least on my Mach3 machine it is.

[Eldon_Joh]

with my dull end mills, 1/4th inch dia, 4 flute, .75 inch length of cut, if i tried to take .001" per flute.. I could probably see the end mill bend.


did it shatter or did it break off? if it shattered that might be an indication the machine tried to drill a hole at 7ipm, with half of the end mill unsupported radially, having already cut the slot.

of course, you are using mystery metal. hot rolled steel is bottom of the barrel mystery metal, but if its from the usa its still better than what comes out of africa or china.

[sajurcaju]

Did you check to see if the steel is hardened? An angle bracket sounds likely to be.

Steve

[chuckorlando]

So this is a helical ramp?

Does your control execute all 3 at one time or z first?

I am not sure what exactly you are doing or the machine rigidity, but .001 seems pretty low for carbide. .003 is more run of the mill. Carbide has to keep a chip or it rubs and dies

[Superman]

Cutter Diameter= 0.25" carbide
Flutes= 4
SFM= 98.25
RPM= 1500
Chip Load= 0.00117"
IPR= 0.00467
IPM= 7

...
G00 X0.000 Y0.625 Z0.020  ...... should it be 0.623 ?
G1 F7
Z0
(CCW circle)
G03 X0.000 Y0.623 Z-0.070 I0.0 J-0.623
(end mill snaps about here)
G03 X0.000 Y0.623 Z-0.140 I0.0 J-0.623
...

.

does the toolpath do as you think it does ?.....some machines would assume it is at the same point as the start point, & just plunges down,
the following breaks the circle into 2 pieces

...
G00 X0.000 Y0.623 Z0.020  S6000 M3
G1 F20.
Z0
(CCW circle)
G03 X0.000 Y-0.623 Z-0.035 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.070 I0.0 J0.623
G03 X0.000 Y-0.623 Z-0.105 I0.0 J-0.623
G03 X0.000 Y0.623 Z-0.140 I0.0 J0.623
G03 X0.000 Y-0.623 I0.0 J-0.623
G03 X0.000 Y0.623 I0.0 J0.623
...

Your cutting speed seems slow for a carbide , should be up round the 400 SFM (~ 6000 RPM)
your data would be more suited to a HSS cutter

as a general rule of thumb...... carbide run 4 times faster than HSS

The other thing to check is the under side of the cutter .... not just the side edges.... can the cutter "end cut" ?

[1875]

I have been cutting and drilling this metal, so it is not hardened. It does have a somewhat rough finish, but is painted. Perhaps some of the scale remains in various places. The machine is a Bridegport Boss 3 CNC, the more flexible one...lol.

The end mill shattered, just the tip... it did not drill straight down, and where it broke there was still full metal under it because when it initially started the cut, it slowly ramped down. If it would plunge on these cuts, I would expect it on the first circle when it started.

Superman, you found a slight error in my code. Yes, it should have been 0.623. I decided to make a final finish pass out to 0.625 and missed that line. The end mill is center cutting, or it has one cutting lip going across the entire diameter.

The cutter was not new, so perhaps that and running too slow dulled it out, and there could have been some scale, maybe some chip build-up. I'll try bumping the speeds when using carbide, but I am limited to around 4k RPM.

Thanks.

[chuckorlando]

Chip load more important then feed. Max the spindle and feed to that for chipload. Same reason guys can run 1000ipm.

[1875]

I'll have to expand my chip load charts, but that is an interesting way of looking at it. I was calculating RPM based on SFM, and working the rest based off that and a chip load of around 0.001 - 0.004, depending on material. My axis stalls are around 120 IPM no loads. I think cutting steel is safer up to 80 IPM straight or maybe 60 if doing multiple axis. I think I need to be careful because it's open loop.

[chuckorlando]

Yea I am not suggesting to kill the machine. When using hsmadvisor I wil often plug in my spindle and chip load then let it give the feed. If I plug in if I have a haas vf3 with 10k spindle and I plug in 10k and chip load of .003 it give me a feed of 120ipm now if I change that spindle to 3000rpm it give me 36ipm but my chip load is the same.

The beauty of a prog like hsmadvisor is it take torque curves and machine rigidity into account.

On carbide you want to stay around .003 up to .005 or so. Carbide hates to rub