Machining Torlon 4301 in a swiss. Never used it before, how does it cut?

[MCImes]

Hello,
Im going to be making a square part from Torlon 4301. I will have 3/8 round stock and have to face it, mill it to a .250 square, add a .100 deep step at the front and back and mill a 30* angle on 3 of the sides.

First, Ive never machined plastic in a swiss machine before. anything I should know? since its a square part the only turning I will be doing is facing and cutoff so most of my questions regard milling. what have you used for good feed and speed?

also, the part is only .700 long but when I mill the last 2 sides the stock will be unsupported on the backside. Think i should decrease feeds for those 2 sides?

for my endmill I was either going to use:
a 2 or 3 flute .375 dia EM that would be .465 from the bushing face (2 flute AlTiN coated or uncoated, 3 flute ZrN coated, Aluminum geom EM)
or
a 2 or 4 flute .250 dia EM that would be .075 from the bushing face. (both uncoated or AlTiN)

Id rather use a .375 because I would be able to cut the .250 flat in 1 pass versus 2 but Im worried that the extra .400 stick out on my large tool station might allow a fair amount of flex/chatter. Do i have unfounded fears or a possible problem?

Any help is appreciated

[SirDenisNayland]

I've not machined that particular plastic, so I cannot speak for its properties when machining.

However Ive machined a good bit of delrin and other plastics, and I would generally use an uncoated endmill because you want it to be as sharp as possible. Also, you are likely going to have to support the part fully, any chatter will come from the plastic itself bending, not the tool, especially not a 3/8 end mill.

Ive had a job where I had to mill out an octagon shape in aluminum over a 3" length, and it had to be done in portions because of sides being unsupported in the guide. We machined the first hundred thou or so into the octagon and then came in and supported the part with the sub because chatter and flex off the aluminum was bad enough.. 3/8 plastic is basically a noodle and is going to bend out of the way with ease and cause you all kinds of nightmares if you arent planning to support it with your pickoff.

I would personally do your flats in portions, moving the tool in x or y (depending on your machine) rather than to feed in Z.

Feeds and speeds, well, I generally haul ass in these types of material, you shouldnt have to worry about melting with a steady oil flow, but I would say the amount your part is going to flex will dictate just how fast you can cut it more than anything.

Cheers

edit::
what exactly do you mean by from the bushing face, I initially assumed you meant how far the tool sticks out but from reading your post over you mean to say that each tool would have different center positions? Im confused with this part to be honest heh.. I can guess youre er11 tools are closer to the guide than your er16s, which seems odd as ive never come across a machine like this, what machine is it?

[MCImes]

Your re-read is correct. My er11's have a 5mm bushing to tool center line,
the er16 has 15mm to center line.

The machine is a Tsugami BS19 or BX12. Both have the same live tool config. Also the Nexturn SE32 machines i used to run had a .590" G50 on 3 tools and .750 on one. (for a saw is what they show in the manual)

I think I will have to use the er11 tool station with a .250 endmill since I dont think I will get a .250 square pick off collet ordered for this job I will only use the sub to catch parts in a basket. If I use the er11 station I only have .070 bushing to close side of EM so theres not much room to flex.

I also like the idea of moving the EM in x/y rather than z.

Thanks for the thoughts

Originally Posted by SirDenisNayland I've not machined that particular plastic, so I cannot speak for its properties when machining. edit:: what exactly do you mean by from the bushing face, I initially assumed you meant how far the tool sticks out but from reading your post over you mean to say that each tool would have different center positions? Im confused with this part to be honest heh.. I can guess youre er11 tools are closer to the guide than your er16s, which seems odd as ive never come across a machine like this, what machine is it?

[SirDenisNayland]

As far as using the sub to catch with a basket you may run into issues there. Like I said I don't know this particular plastic, but any plastic I've worked with creates 'stringies' from the cutoff and turn which love to wrap around the part, and if youve got a basket sitting below you may find your basket jamming full of plastic strings and all your parts sitting in tray instead of your part receptical.

Just something to keep in mind.

[MCImes]

Well, I finished the 2 jobs and figured I would report my experience for anyone else doing this sort of thing..

Tooling:
I was using a .250 endmill, 4 flute, carbide, OSG, uncoated, 4000 rpm at 20 IPM on the non critical sides and roughing, 12 ipm for finish/critical sides. I side cut the whole thing except for the steps. Also I climb milled the entire time.

Tool wear: Overall it ran great. Once I got everything dialed in I would only have to make offsets about 2 times in a ten hour shift. The carbide tools held up for more than 800 parts. The HSS centerdrill on my cross tools wore out about half way through the jobs.

That said, the only turning I was doing was facing off .060 and cutoff. On the cutoff the stringy chip was not a problem as I did a .05 second dwell at x.050" then finished the cutoff and dropped the part into a basket.

After a while the end mill started to leave a fairly large burr on the sides but I threw one in the tumbler and it came off, so if you tumble your parts its worth trying it and seeing if it comes off before you go to the trouble of changing anything. Also for reference I could scrape off the burr with the back of my thumb nail and a little pressure.

Process/other thoughts: quick recap: I was making 2 similar parts about .7" long and .250 square. they had a couple angles and steps cut into the front and back. also a cross hole. I started with .375 ground torlon. Also I fed all my milling in Z as opposed to doing it .250 at a time and indexing 4 times, then advance Z again.

I had to program in about .010 taper over the .700 length on 3 sides. I started by doing my angle profile, then re-cut with the same path to try to get my most critical side fairly square.

2nd side didnt really matter so it was a 1 pass hog out material operation.

the 3rd side was a little tricky because I had to get it parallel to the first side within .002 or so. My overall tolerance was +-.005 but it was an "unwritten tolerance" that they wanted the top and bottom fairly parallel. I had to do a roughing cut leaving about .030 for my 2 finish cuts as the leading corner would chip out even with a brand new endmill. I also added about .010 of taper on the finish cuts. I had to lie to get size too, so I started at .235 and ended at .245 to get my .250 in real life.

the 4th side was another easy one as the sides didnt matter too much and I only tried to hold them parallel within .004.

A couple things I learned that Ill do next time:
I notated my program a lot. almost every line had some note on it and I am very glad I did that. I had to edit the crap out of my program to get it to work and man did my initial program notes help remind me of what my thought was when I made the process.

Next time I will make my taper numbers and angle points macros at the top of my program instead of hard numbers in the program body. something like:

#100 =.235 (C0. taper start)
#101 =.245 (C0. taper end)

#102 =.0193 (1st angle start in x)
#103 =.120 (1st angle end in z)

#104 =.620 (2nd angle start in z)
#105 =.030 (2nd angle end in x)

#105 =.239 (c180 taper start)
#106 =.249 (c180 taper end)

Then I dont have to dig through the program to find my numbers and I only have to change the number once instead of 2 or 3 times. Also eliminates more chances for mistypes or misreads.

The last 2 sides I cut totally unsupported by the bushing thus the large amounts of taper but there was minimal to no chatter and once you got it right it held size very well. I would feel comfortable holding +-.003 all day with this setup. If i had to get tighter than that it wouldnt be hard, it would just require checking parts twice as often and replacing the tools once or twice on a 800 piece job. generally more babysitting.

Overall not too bad though. Thanks for the input Denis