Delrin & Nylon S & F please

Hey guys.

So i want to start machining some Nylon parts and some Delrin parts.

I am using a CNC router, 1.5kw spindle, I have flood coolant available.


What's the best speed, feed & cut depth, my thickness total would be approximately 16mm

Craig

iv not done a lot of nylon.
i cut acetal/delrin with single flute carbide... i find there is a broad range of speeds that work as long as your tool is sharp
you will have to do some experiments with your 1.5kw spindle (im not sure how slow one of those will run)
i cut all my acetal at sub 3000rpm eg, 3.175mm single flute carbide at 2mm step down at aprox 2000rpm 200mm feed and can make my way through 22mm depth with a tool width slot.
if you aim for your chips to be a nice curl a tiny bit of air will easily clear them (no liquid coolant needed)
acetal is an absolute pleasure to machine :)

Quote:

---

Originally Posted by craigrobbo

What's the best speed, feed & cut depth, my thickness total would be approximately 16mm

---

Really depends on the size and type of cutter you plan on using.?
Also whether you want to cut full slot IE: cutter enclosed both sides like when profiling out of sheet, or if your mainy cutting with a step over.? The step over amount will greatly affect feed rates.
The strength of your a machine will also play a part.!

I don't cut much plastics but here's some figures that G-wizzard spat out for hard plastics.! I would use these a guide only and adjust to suit your machine.

Here's a few based on 50% cut diameter for DOC.

HSS 3m 1 flute= DOC 1.5mm FR 1200mm/min RPM 16200
HSS 6mm 1 flute= DOC 3mm FR 1050mm/min RPM 8100
HSS 3m 2 flute= DOC 1.5mm FR 2350mm/min RPM 16900
HSS 6mm 2 flute= DOC 3mm FR 2100mm/min RPM 8100


Carbide 3m 1 flute= DOC 1.5mm FR 1400mm/min RPM 23400
Carbide 6mm 1 flute= DOC 3mm FR 1250mm/min RPM 12000
Carbide 3m 2 flute= DOC 1.5mm FR 2800mm/min RPM 23400
Carbide 6mm 2 flute= DOC 3mm FR 2500mm/min RPM 12000

Hope this helps.