Machining nylon - please help

Hello,

I wonder if you guys could be kind enough to share your experience machining nylon. I have 20,000 bushings to cut. The bushing is 9mm long +/- 0.1, 10mm OD, and 6.6 +/- 0.1mm ID. I have never cut nylon before. I would appreciate a heads up so I have some time to prepare. What inserts would you guys reccomend? What brand? What feed, and what speed?

Customer supplies solid rods, so I have to drill. What drill would be suitable to do the job quickly and leave a nice finish?

I think they mentioned the nylon type to be LC94, PAS. This is not for sure, though.



Thanks ahead.

The nylon I worked with before was the natural 6/6 I think its called, not sure how similar it is to what you're using. I do know that it likes to squeeze drills and make them heat up fast, then it sticks to the drill. So you might have to dial in the speed depending on how they come out. I'm not sure if you can run flood coolant on it, I ran them dry. Although coolant would help the heat, I really don't know how much it'll make it swell or if some types of coolant may be bad for it so look into that.

Turning= high rake polished inserts, like thos used on AL, or HSS.

When I have to turn nylon, I use high speed steel. I grind a large radius on it and sharpen it so that it will shave. I run it at low RPM's to avoid the melting thing discussed earlier. You can drill it with a normal twist drill, and probably ream it without a problem. Again, keep your rpm's low.

High positive rake inserts, uncoated. Dead sharp is best.

Nylon is best machined after annealing. This eliminates the long strings
and wrap-up. We did it dry, at most a spray or two of WD40 as a cutting
fluid.

Jim

Nylon machining

have done quite a lot of work with nylon-
There are some types of material with which you would swear and &^£"£(!!(&....
If you are machining POM, Acetal you are in the clear. there is a waxy type of nylon which is not pleasant to work with.
I would suggest HSS tools throughout.
Speeds of 600 RPM- play around,
Feeds of 0.1 meters per minuite would be ideal but you have to play around with these to get the finish you desire.
and pleny of Luck as sometimes the easiest job can turn nightmare easily....

We do quite a lot of high quantity jobs from nylon and everytime we get the order I cry a little!
I find that you can 'scream' through the stuff when your removing the majoriy of material. Low spindle speed with high feed should keep your swarf thick and easier to remove. Don't worry about special tooling for this, you could use a spoon to cut it.
On finishing passes, however, a higher speed and a slower feed will be best but keep the depth of cut to a minimum and this will stop the swarf from ganging around the tip. The tip should be sharp as possible too. Edges should last a lifetime!
Good luck sir.
T13.

All these guys are right. The tools must be dead sharp. I grind my own highspeed tools and then sharpen them on a hone until I can shave with it. Nylon is a walk in the park compared to some of the stuff I have machined over the years, polypropylene, uhmw, and teflon.

I wouldn't suggest drilling 'to size'. As soon as the swarf builds up on he drill it will melt together and a: be difficult to remove and b:leave the bore finish the same as the melted swarf.
I would reccomend drilling rough and then boring to size exactly as I mentioned above.
We use a 4 flute end mill to drill because it helps with a flat bottom and you can force into the material but there is no reason why a HSS drill won't do the job just as good.

I would use flood coolant. Sharp HSS or polished carbide inserts for turning. I would bore it out to finish size.

Jim, you mention "Nylon is best machined after annealing. This eliminates the long strings
and wrap-up"

What do you mean by annealing nylon ?

Sounds intresting, as a current job involves maching a black nylon which is non-lubricating and after a test machining i got a lot of long strings and wrap-up. A real pain.

Mark

Gakor

What type of nylon is it. Natural, oil fill, graphite, high impact? I like sharp tool small radius. Beware of thermal expansion as the coefficient of expansion is very high with plastic as compare to steel.

Robert

A sharp tool; but most important! A 15 degree end relief. The stuff is springy and will rub the outside of the tool.

I had a new woodruff cutter making "fur" on the nylon. I ground a single lip tool and made a 1 flute flycutter. Mirror finish. It didn't make too much difference what rpm I used. I mean nothing special.

15 Degree end relief!

Regards,

Stan-

Pretty much what everyone said here.... If you can get the customer to change the roder to Delrin, that's the best thing you could do, but usually they are pretty stubborn...
I've ground a 20 degree positive rake on a carbide insert for nylon and had it work pretty good with flood coolant, i had a bunch of lines and used it just to knock the chips away from the part, otherwise the chips would just wrap up and ruin the part >_<
1/2 round drills work GREAT for nylon, though you dont have to go deep, so it's not such a big deal. they leave a mirror finish on the inside though =)
good luck!

The one standard reply is sharp pos tool. Thing is, there's nylon and then there's NYLON. Not up on yours, but if it's glass filled or oil impregnated cast, it won't cut like the others. Can you be more specific whether it is cast, injection, virgin, filled, etc? Some is easier than poly, uhmw and the like, and some is a nightmare.

Well, one important thing! Use a shop Vacuum, it will make sure you get no interference form chips/strings!

Thanks

I always got best results with a 15 - 20 relief all the way around a brazed carbide tool. Top of carbide flat.

Hole made with half round carbide. Cold coolant should flash cool the melted swarf, lay a pieces of razor blade on flat of drill with slight spring presure, When the drill falls back the razor cleans the drill, then blast with a shot of air to clean off.

Tried many many different tool geometery. Feeds and speeds.

Best results where always tool geometry, cool cut flood lubricant with a cold air gun blowing cold air into coolant to reduce temp even more.

Of course this was natural nylon and a Tornos T-4.

Woudl much rather run nylon thatn PTFE teflon.

One843 said:

Hole made with half round carbide. Cold coolant should flash cool the melted swarf, lay a pieces of razor blade on flat of drill with slight spring presure, When the drill falls back the razor cleans the drill, then blast with a shot of air to clean off..

Click to expand...

Whaaat?

One843 has it right. Positive rake tooling is nonsense.

Nylon and other thermoplastics have a very high thermal coefficient of expansion and very low thermal conductivity. When you turn it the heat doesn't leave with the chip. It builds up on the cutting edge and begins to sink into the work. Heat in the work causes the work to expand by a large amount rapidly. So you need a large amount of side and end relief. Positive top and back rake just make for a thin and weaker edge.

So unless you turn with a PCD (diamond) insert, a home made carbide tool is best. 0 degree top rake, 0 degree back rake 20-30 degree end and side relief. PCD inserts are impervious to the heat and will last longer. Particularly if the nylon is glass filled.

Half round drills work like magic in nylon. Never peck, no matter how deep the hole.

For unfilled Nylon rough turn at 700 SFM finish turn at 800 SFM. Feed rates should be LOWER than when you cut steel. Say a maximum of 0.01" IPR for roughing, ).005" IPR for finishing.

For glass filled rough around 400 SFM and finish turn at 500 SFM.

If you use a HSS half round run at 250 SFM in unfilled, 125 SFM in filled. Double the SFM for carbide. HSS won't last worth a damn in filled nylon.

Feed at 0.006" IPR for your 6.6mm drill.

OK, I used to work nights for a company called Timco in peekskill. They're owned
by Licharz, and my job was to manufacture lots of parts out of nylon 6,6.

Licharz produced cast nylon bar stock, which was slugged using an auto cutoff saw
into near net size blanks.

The blanks were the loaded into wire baskets, and heated above 100C in gas fired
furnaces for about 40 hours. This was the annealing step.

If you try to machine un-annealed nylon it will be a disaster. We would NEVER try
doing this as the rate of production would be horrible.

Once annealed the slugs were machined on Okuma lathes using high positive rake
carbide inserts, at just about the maximum SFPM speeds available on the lathe being
used. Roughing on a 12 inch diameter blank of nylon would routinely happen at
3000 rpm on the OD of the part.

At those speeds, annealed nylon swarf comes off as fine powder. Tiny chips that
can be simply shovelled out of the machine. Many's the night my work output
consisted of a wire basket stacked full of nylon crane sheaves, and about 10 full
size garbage cans packed with nylon powder.

The annealing step for this material is *critical* and makes all the difference in terms
of surface finish and machinability. I suggest that the manfufacturer of the material
be contacted, and queried closely about the annealing schedule. The parts have to
be slugged, you can't just anneal the whole bar because the surface area has to be
present.

Timco:

http://www.timco-eng.com/sheaves.php

Licharz:

http://www.licharz.de/index.php?id=10

Timco is a local distributor for them, and carries a full line of all kinds of
polymer materials, nylon, oilamid, polyacetyl, PEEK, etc.

Jim

Food for thought, thankyou.

Mark