Feed Rates/ SS for a 1/16 Flat Endmill into 6061

[clemens1292]

Hello,



I'm trying to run slots in a Aluminum 6061 heat sink (stock size 4" X 4.5" X 0.25" held in a vice with parrallels) and I keep breaking the end mill unless I lower the feedrate to around '15', which then requires the job to take almost an hour for OP-10.

The slots are 0.1139 deep and 0.06496 wide. As I mentioned in the title, I'm running a 1/16" end mill.

I have the stepover percentage at 50% (0.03125) and a maxmimum depths of cut of 0.03125.

I'd figure with that much, I should be able to have the feedrate pretty high, or at least everything I've read has told me that.

If any of this is completely ridiculous, feel free to let me know, I'm new to programming and this is all being done in Master Cam and on a HAAS VF-3YT:



Feed Rate: 60

FPT: 0.001

Plunge Rate: 10.00

Spindle Speed: 15,000

SFM: 245



My entry motion is a ramp at 0.03125



Here's a small initial portion of the .NC file where the endmill is first called up:

(TOOL - 12 | 1/16 FLAT ENDMILL)
T12 M6
G0 G90 G54 X4.1257 Y-.6535 S15000 M3
G43 H12 Z.25 M8
Z.2
G1 Z-.0285 F10.
Y-3.3465 F60.
G3 X4.1282 I.0013 J0.
G1 Y-.6535
G3 X4.1257 I-.0012 J0.
G1 Z-.057 F10.
Y-3.3465 F60.
G3 X4.1282 I.0013 J0.
G1 Y-.6535
G3 X4.1257 I-.0012 J0.
G1 Z-.0855 F10.
Y-3.3465 F60.
G3 X4.1282 I.0013 J0.
G1 Y-.6535
G3 X4.1257 I-.0012 J0.
G1 Z-.114 F10.
Y-3.3465 F60.
G3 X4.1282 I.0013 J0.
G1 Y-.6535
G3 X4.1257 I-.0012 J0.
G1 Z.086 F10.
G0 Z.136
Z.25
X4.0319 Y-.6142
Z.2
G1 Z-.0285
Y-3.3858 F60.
X4.0321 Y-3.3861
X4.0354
X4.0356 Y-3.386
X4.0357 Y-3.3858
Y-.6142
X4.0356 Y-.614
X4.0354 Y-.6139
X4.0321
X4.0319 Y-.614
Y-.6142
Z-.057 F10.
Y-3.3858 F60.
X4.0321 Y-3.3861
X4.0354
X4.0356 Y-3.386
X4.0357 Y-3.3858
Y-.6142
X4.0356 Y-.614
X4.0354 Y-.6139
X4.0321
X4.0319 Y-.614
Y-.6142
Z-.0855 F10.
Y-3.3858 F60.
X4.0321 Y-3.3861
X4.0354
X4.0356 Y-3.386
X4.0357 Y-3.3858
Y-.6142
X4.0356 Y-.614
X4.0354 Y-.6139
X4.0321
X4.0319 Y-.614
Y-.6142
Z-.114 F10.
Y-3.3858 F60.
X4.0321 Y-3.3861
X4.0354
X4.0356 Y-3.386
X4.0357 Y-3.3858
Y-.6142
X4.0356 Y-.614
X4.0354 Y-.6139
X4.0321
X4.0319 Y-.614
Y-.6142
Z.086 F10.
G0 Z.136
Z.25
X3.938
Z.2
G1 Z-.0285
Y-3.3858 F60.
X3.9382 Y-3.3861
X3.9416
X3.9418 Y-3.386
Y-3.3858
Y-.6142
X3.9416 Y-.6139
X3.9382
X3.938 Y-.614
Y-.6142
Z-.057 F10.
Y-3.3858 F60.
X3.9382 Y-3.3861
X3.9416
X3.9418 Y-3.386
Y-3.3858
Y-.6142
X3.9416 Y-.6139
X3.9382
X3.938 Y-.614
Y-.6142
Z-.0855 F10.
Y-3.3858 F60.
X3.9382 Y-3.3861
X3.9416
X3.9418 Y-3.386
Y-3.3858
Y-.6142
X3.9416 Y-.6139
X3.9382
X3.938 Y-.614
Y-.6142
Z-.114 F10.
Y-3.3858 F60.
X3.9382 Y-3.3861
X3.9416
X3.9418 Y-3.386
Y-3.3858
Y-.6142
X3.9416 Y-.6139
X3.9382
X3.938 Y-.614
Y-.6142

And here's an image of where it just broke. This is the very beginning of the first slot (there's around 30).



Again, I'm relatively new to this, so I apologize for anything that looks completely foolish.

[cadcam]

go .01 deep on the cut you are using full width of the tool.

[clemens1292]

go .01 deep on the cut you are using full width of the tool.

So I'm running it right now with the same feeds and speeds, but with a 0.01 depths of cut like you recommended and it appears to be doing great. It's half way through, more efficient and the tool seems to be having no troubles.

However, I just got off the phone with a rep from the tool manufacturer and he said that my feed rate would create way too much chip load and that the depth of cut of 50% should be fine. His recommendation was to run it at a feed rate of 21, with the same RPM and at 50% depth of cut.

Considering what I'm doing now is working, and I feel like I've tried the way he's recommending and still broken a tool, I'll stick with this for now. But I thought I'd throw that out there incase anyone agrees with that route.

Thanks again.

[txcncman]

Tool reps are generally not machinists. They tell customers what they have been told to say. I bet your tool could do exactly what the rep said, under ideal machining conditions. Rarely will you ever have ideal machining conditions.