What's new
What's new

chip control when turning nylon advice or tips please

alonzo83

Stainless
Joined
Mar 20, 2013
Location
Missouri
I am in the middle of turning down a 26" diameter pulley from what used to be a square block of nylon right now I am not having any problems as I still am in the interrupted cutting on the od where I roughed it out on the bandsaw.

I have turned nylon in the past and it seemed to wrap around everything spindle lead screws and make a mess of things.

Is there a civilized means or way to turn this stuff?

Thanks for your input.

Regards,

Alonzo
 
IME the only way to have any control over nylon chips is to create a break in the ribbon, either by an interrupted cut or pausing the feed.

As far as a job that size goes I would keep my spindle speed below 50 rpm (<> 300ft /min) - 25RPM would be nice:) use a very sharp HSS tool with a LOT of clearance, take monster DOC's and feed it hard 0.020 - 0.030 /rev, and use an air gun to blow the ribbon away from the machine.
 
Thank you limey, right now I am running about 850 sfm and taking .200 doc.

Damn newb I am, doing everything backwards.
 
I used to turn a lot of UHMW and rigged a shop vac hose behind the tool holder. Once the string gets started down the hose, it sucks it all in pretty well.
 
I used to turn a lot of UHMW and rigged a shop vac hose behind the tool holder. Once the string gets started down the hose, it sucks it all in pretty well.

That's okay ...........until it goes wrong, a full drum or blockage in the tube can cause the swarf to back up, get caught in the work or chuck jaws, grab the hose ..............and before you know it, the shop vacs coming at you like an enraged Dalek :eek:
 
I have had pretty good luck with turning Nylatron running 800-1000 SFM, high feeds .015-.020 ipr, and fairly big depth of cut, using a high positive aluminum insert. It would actually produce a chip, but on occasion would chip out on entry and exit. I know Nylon and Nylatron are a bit different but that's where I would start with your job.
 
A pulley?

Do a sketch and then drill a couple of chip breaker holes. A radial hole will go right into the bottom of the groove. String the holes or step them out if Deep V.

A saw kerf or two (or three) in the blank to the point of maximum finished diameter will take care of the lions share.

Just fleshing out Limy's good advice. ;-)
 
A pulley?

Do a sketch and then drill a couple of chip breaker holes. A radial hole will go right into the bottom of the groove. String the holes or step them out if Deep V.

A saw kerf or two (or three) in the blank to the point of maximum finished diameter will take care of the lions share.

Just fleshing out Limy's good advice. ;-)

step drilling a chip breaker is a great idea. thank you.
 
I think I would try mounting a die grinder or router to the lathe and use router bits to rough out the part. A router will throw discrete chips. Turning will produce one continuous chip.
 
That's okay ...........until it goes wrong, a full drum or blockage in the tube can cause the swarf to back up, get caught in the work or chuck jaws, grab the hose ..............and before you know it, the shop vacs coming at you like an enraged Dalek :eek:

Nice imagery Limi! I almost blew my drink across my keyboard when I read your metaphor :D

daleks.png



Alonzo,

I've had good luck using a slitting saw on a die grinder to cut a slit in the part that caused the chip to break each revolution. On edit, I see Cal beat me to it ;)!
 
I like deep cuts, fast feeds and slow RPM, but my buddy Rod at Precision Machine likes to show off with a negative rake and some RPM. The chips fly high over his head and into a bucket on the floor.
 
When I machine nylon I use a very sharp bit with a lot of rake. What I do is advance the bit about .100 or .200 and drag it across the nylon using the longitudinal feed. This cuts a groove in the nylon and when you go back and turn it the nylon comes of in short piece one diameter long that don't wrap up in everything. Only takes a second to do it and it sure saves time in the long run.
 
I use an aluminum specific sharp insert with the heaviest depth and feed I think I can get away with and peck. But my favorite solution is convince the customer that Acetal is the superior choice for their application☺
 
alonzo83 - Practical Machinist(375945) on Vimeo

Thanks for the assistance fellas on the Od I had a cut off wheel handy so I made 4 slices and kicked my feed up a bit. Chips broke nicely

On the grooving operation I had a lot of chatter on the first groove until I realized it was the chips building up so I inverted the cutter and ran in reverse.

ImageUploadedByTapatalk1458343595.476872.jpg
 
Nice - and a Kelly bar as well :)

I wasn't sure what to call it I knew I need to reach around the material So I made it with what I tripped over first. . Now I know.

I want to make a better one out of 4140 if I get more of these in the door. it just couldn't take the heavy feeds I should have been running.
 
Cut so heavy it is astounding, drill holes - everywhere except where features need to be, millions of holes. And on the other side of the coin, turn it painfully slow, like 200 sfm. I have also used G73 while turning, face grooving, boring so you break the chip up. Drilling a million holes is the best IMO.

Robert
 
never turn what you can saw

toss it on the rotab, and use a long end mill to "saw" off the bulk of it

If it were my call I would have tossed it in the marvel with a 45 deg support. 10 second cut. But someone else was holding the tail on this goat. Hands tied. . .
 








 
Back
Top