CNC Routing Nylon 6 Material

Hi guys,

I am currently machining some Nylon 6 material, 25mm thick, using a 6mm diameter twin flute, up spiral carbide cutter, with a 30mm cut length.

My question is - what would be the ideal pass depth for Nylon 6, im currently taking off 2mm. Also what feedrate and rpm would you recommend for this material??

I am snapping tools and there seems to be a lot of vibration when i cutting the material, ive tried slowing the feedrates/rpm and this has improved a little.

Any answers would be highly appreciated.

Many thanks :)

what spindle speed are you running and what spondle power have you got? with plastics you need a high feedrate to actually cut not rub then melt the material, and obviously the higher the spindle speed the higher the feedrate needs to be... thats why single flute cutters are sometimes better in plastics. You say you're taking of 2mm, I guess thats depth but what width of cut? 3mm?

I've cut a significant amount of nylon using a 6mm single flute cutter at 3mm depth per pass and 1700mm/min, 12500rpm without air cooling. With a 2 flute cutter your feedrate would need to be about twice that, but that would probably be too much force on the cutter so reduce the depth of cut.

It sounds like you're putting too much force on the cutter, so since the cutting speed for nylon is about 170m/min I would reduce the depth of cut to 1mm and use 9000rpm. If the cutter still breaks then reduce then you can either reduce the depth per pass further, or the feedrate and spindle speed proportionately. Similarly if the cutter survives you can try increasing the depth of pass until you find the limit. You would be much better off using 6mm single flute cutters as for such a large thickness it helps if there is more space for the swarf to eject.

I would be wary of using coolant since nylon absorbs water.

I am very interested in this thread. I too broke 2 x 3mm cutters at only 1mm DOC - More than likley my feed & speed was wrong as the cutters was BRAND NEW.

My Speed and feed(off the top of my head) was approximately 640 and 800mm/m and speed was around 200hz and also tried 250-280hz on 1.5kw spindle(not sure what that relates to in RPM but i guess about 12k - 15k)

Craig

I tried using an airline with the feed/speed I quoted and it did improve the finish a little, but the finish was good enough without and I couldn't have gone any faster without the tool deflecting too much, hence I didn't bother with it. My machine isn't especially rigid, otherwise it may have been more worthwhile.

Quote:

---

Originally Posted by CLaNZeR

You will need to start with shallow depth cuts and slow feedrates and see what you can push both to, to suit your machine and avoid chatter.

---

The risk here is if you start will too low a feedrate (without also using a very low spindle speed, but there's a limit to how slow you can go with the VFD driven spindles) you can risk the material melting on to the cutter which can break the cutter just as fast as going too fast. This is probably what's happening to Craig as with a 4mm cutter at 200hz (12000rpm) the feedrate should be around 950mm/min for single flute or 1900mm/min for two flute.
When trying a new material or tool I always start with 'normal' or recommended feedrates and a shallow cut, then gradually increase the depth of cut.

Either way it will help a lot to see a picture of the machine this is being cut on to give an idea of how rigid it is.

Quote:

---

Originally Posted by craigrobbo

also tried 250-280hz on 1.5kw spindle(not sure what that relates to in RPM but i guess about 12k - 15k)

---

You can press the >> key on the VFD to scroll through the readings until you find RPM if you're not sure. An easy way to remember it is that you know the spindle must do 24000rpm at 400Hz, since that's the maximum, so just work it out proportionately from that. Hence 250Hz is 250/400*24000=14400rpm and 280Hz is 16800rpm.

Quote:

---

Originally Posted by Jonathan

You can press the >> key on the VFD to scroll through the readings until you find RPM if you're not sure. An easy way to remember it is that you know the spindle must do 24000rpm at 400Hz, since that's the maximum, so just work it out proportionately from that. Hence 250Hz is 250/400*24000=14400rpm and 280Hz is 16800rpm.

---

Thanks for that, I wasn't a million miles off with 15k as a guesstimate :D