It's hardly rocket science but there doesn't seem to be a clear consensus on speeds and feeds for milling acetal. Much of the problem is that quoted feeds and speeds for plastics seem to default to acrylic, not acetal.
From APT-Tools:
According to APT, for acrylic you can feed a 10mm single flute cutter at 2400 mm/min at 8000rpm. That's 0.3 mm/rev for a single flute cutter. Wow. That surface speed comes out at about 250 m/min....
From Cutwel (YG):
This seems to agree with APT - and again relates to acrylic, not acetal.
From plasticshop:
They actually give data for acetal. In terms of feeds, they speak of <0.05 mm per tooth. At 6000rpm, that's 300 mm/min, which is some way short of 2400 mm/min, like a factor of 20:1. Certainly, I can imagine cutting at 0.05 mm per tooth, whereas 0.3 mm per tooth is hard to imagine. Although APT are talking about acrylic, not acetal, I hadn't realised there's quite that difference!
Boedeker Plastics Inc:
The figures from them seem to agree with plasticshop, albeit in Imperial units. However, their recommendations are 270 - 450 sfm (80 - 140 m/min) and 2 thou per tooth (0.05 mm per tooth). That is reassuring.
Finally, for drilling, Boedeker suggest about 0.02" / rev for a 16mm drill. That's about 0.5mm / rev and the recommended surface speed of 150 m / min corresponds to about 3000 rpm! That would take some balls.
However, the notes at the top of the page say:
The insulating characteristics of plastics require consideration during drilling operations, especially when hole depths are greater than twice the diameter.
Small diameter holes (232" or 1mm to 1.0 or 25mm) - High speed steel twist drills are generally sufficient for small holes. To improve swarf removal, frequent pull-out (peck drilling) is suggested. A slow spiral (low helix drill will allow for better swarf removal.
Large diameter holes (1.0” or 25mm and larger) - A slow spiral (low helix) drill or general purpose drill bit ground to a 118° point angle with 9° to 15° lip clearance is recommended. The lip rake should be ground (dubbed off) and the web thinned.
It is generally best to drill a pilot hole (maximum 1/2” diameter) using 600 to 1,000 rpm and a positive feed of 0.005” to 0.015” per revolution....Secondary drilling at 400 to 500 rpm at 0.008 to 0.020” per revolution is required to expand the hole to larger diameters.
Conclusions:
For milling, I'll go with 0.05 mm per tooth for the 10mm cutter and although I can't manage more than 6000rpm, that would result in around 190 m/min which doesn't sound silly - so I could actually afford to reduce that. 4000 rpm for the 10mm cutter would give me about 125 m/min surface speed. Doesn't sound silly slow and certainly I want to avoid any danger of melting, as that would surely result in broken cutters.
Note that the feed per tooth seems to be proportional to the cutter diameter, so an 8mm cutter would be good for about 0.04 mm per tooth and a 4mm cutter would be good for about 0.02mm per tooth. Obviously for both of those tools, the machine needs to be running at full speed (6000 rpm).
For drilling, My 6.5mm pilot drill (also used for the M6 clearance holes) needs to be running at about 1000 rpm and 0.25 mm/rev. The 16mm drill should be down at ~500 rpm and 0.25 mm/rev.
Tool table setup for acetal machining:
So finally, the tools, feeds and speeds I plan to use are:
- 10mm carbide single flute end mill. 4000 rpm, 0.05mm/tooth.
- 8mm carbide 2-flute chamfer mill. 6000 rpm, 0.04mm/tooth.
- 4mm carbide single flute end mill. 6000 rpm, 0.02mm/tooth.
- 6.5mm HSSCo drill (pilot). 1000 rpm, 0.25 mm/rev.
- 16mm HSSCo drill. 500 rpm, 0.25 mm/rev.
- 10mm carbide ball end mill. 4000 rpm, 0.05mm/tooth.
Let's set them up, then!
No comments:
Post a Comment