CNC routing HDPE

[mkepke]

This isn't wood, but it is for a woodworking jig, so I thought I'd share my experiences machining HDPE. This is for Hitch's segmented bowl jig in another thread.

I had trouble finding consensus on feeds and speeds for this but for full thickness profile (slot) cutting and pocketing thru holes in 0.5" thick material, what I found worked well is:

0.125" dia conventional upcut endmill, two flute (a 1 flute O-flute is often recommended but I didn't have one of those)
100 IPM @ 0.08" DOC (probably could go a both faster AND deeper - provided one can clear chips)
spindle speed ~11K rpm (even slower normally better with HDPE, but it seemed like I had a harmonic around 10K)
plunge cuts at 30 IPM with full retract (to clear chips - probably could plunge faster)
conventional cut (NOT climb cut)
no finish/skim cut required for a good surface finish

..and the big secret: blow compressed air at the bit to aggressively clear chips. A dust shroud was simply inadequate for clearing chips in the slots, leading to chatter and chip-welding back onto the base material.

 

[blackhawk]

A 1/4" bit will help clear chips out better. I generally run at least 120 ipm and 16,000 rpm with a 1/4" bit.

 

[mkepke]

Yeah, with this particular job I could do all three operations (engrave text, drill hole, cut out piece) with the same bit so it made sense to run the 1/8”.

I’ll run some test cuts using a 1/4” up cut and see how it does with the normal dust shroud/no air assist.

-Mark

 

[Rick Mainhart]

Hi Mike,

My past experience with machining UHMW led to a discussion with the technical folks at Onsrud. They recommended a two-flute "O Flute" bit, and to adjust speed and feed to produce chips about 0.007" thick. This thickness provided the best heat removal, cutting speed, and cutter life. If you are melting material, your feed rate is too slow.

An important point they brought up was NEVER exceed 1/2 cutter diameter as cutting depth (1/4" cutter, 1/8" max cut depth).

Using a ShopBot PRT with the Porter Cable 3.25 HP* router allowed us to cut at 3"/second. Longest continuous cut was a six-hour job in 2-1/2" thick cast UHMW for a rather complex, large part.

Oh, the router has had one set of brushes changed in 21 years, and is still running well. As others have pointed out, using a proper spindle motor producing an actual 3-4 HP would allow me to increase my feed speed ... but I'm no longer machining anything but wood these days and don't need the production improvement.

Hope this helps.

Regards,

Rick


*Yea, maybe

 

[HITCH-]

Thanks again for your help Mark!

 

[mkepke]

Thanks again for your help Mark!

Glad I could help. Please let me know if they do/don’t work as expected!

-Mark