Machining/working polypropylene

[Tom Szelag]

Has anyone had good experience working with PP? Some part I have to make is a modified syringe, bout half inch diameter with ~.063 walls.

 

The hard part is milling a thru slot about a quarter inch long by .063 wide, perpendicular to the axis of the syringe. And it has to be machined dry.

 

Tried using a .063 endmill, low speed with the feed up. Fast speeds made the thing melt and gum up. In any event, it always comes out with a nasty burr and about .010 undersize, probably to the material being so soft. Requires considerable time with an exacto knife and gauge pins to clean it out and bring it to spec.

 

First they wanted a prototype, then a batch of 85, and now they want 600-1000!!! So I need a better way to run these things. Either machined so it comes out cleanly on one pass or something else. I'm thinking of maybe making a punch tool.

 

Anyone have some experience working with this stuff?

[The Iron Chef]

SHARP tools, air blast.

 

Why no coolant?

 

-Keith, from home

[crazy^millman]

Left hand sprial right hand cut is the only way to go with this stuff. Seen a .015 thinkness done and hold .0004 tolerence on it using these types of endmils. I would also look to an arbor to do these parts on maybe suck a vacuum on the parts. I have done a arbor then stick the whole thing in a rough cut vice to keep parts like this from collasping.

 

HTH

[The Iron Chef]

Or use a slitting saw, SHARP, with air blast

 

 

-Keith, from home

[Tom Szelag]

Hmm, I'll have to try some of this.

 

Can't use coolant because the end use is as a sample container for a cell culture for space flight. They want to keep these as clean as possible and not have to spend loads of time swabbing them out.

 

Still kinda leaning towards the punch idea. Running these with the .063 EM I was using about 260rpm and 1.5ipm. Faster spindle speed and the damn thing would melt more and make a nastier burr. Faster feeds and it cracks/shatters. For 1000 of these think it would be easier to make a press that punches out the slot (slot by the way has radius ends) on say 10 at a time in one swift movement. Rather than having to take the thing, put it in a collet, mill one side, flip it 180 degrees, mill the other side, and take it out.

[crazy^millman]

Well the idea of a punch would worry me wit hthis material. You would need a knife type cutting actino almost like a shearing verse a punch action like that of a standard punch. If it engaged it wit ha 5 to 7 degree shearing action it might work but would worrry about the stress being introduced into the part with the cut. Milling on an anvil would be my first coice for that small of a quainity. I would wonder how much the tooling would cost to design make and then perfect a tools for only 1000 parts if doing 2000 and above might be worth the investment but just my opinion.

 

I am thinking like 10 to 15 sec a slot if done on an anvil and a 4th axis. Use to make a nylon tube .250 od wit ha .188 id 6" long on a screw machine it took longer to get the tools indicated in perfect to make them than to make the whole 200 piece order. My point is milling it once you have it down is done where as a punch might require a lot more trial and error before you get the desired results. I would also be worried about pushing material into the bore with a punch not so with a good sharp endmill.

 

HTH

[Chris Rizzo]

Any chance of convincing them to use a machinable plastic..like Delrin? Although I believe Delrin absorbs moisture. ?

Occasionally you'll get a designer who will spec something for the hell of it, and have no real clue as to it's manufacturability or even if it's the best material for the application.

[Tom Szelag]

Heh, "only" a thousand parts. We do almost exclusively small batches. Large piece of hardware that gets put in a locker and blasted into space. Ran some contraption a while ago, 75 of em (each with 6 parts) and that was a lot!

 

4-axis, not a bad idea I guess. That ties up our only CNC though, for quite some time (maybe 30 sec of milling but then gotta take it out and put a new one in and start the program again each time). Don't think that's an option, got some parts that need surfacing and many tool operations.

 

I had been running it on a Bridgeport tracker (2 axis).

[Bruce Caulley]

I used to do a lot of this. Unfortunately your coolant situation is a bit of a problem. You could try a single flute straight edged carbide router bit. At the low speeds you would be using I reckon that might do the trick. Cheap too!

 

HTH

Bruce

[Tom Szelag]

"Any chance of convincing them to use a machinable plastic..like Delrin?"

 

Oh I wish. But what they're doing is taking off-the-shelf syringes and modifying them into this thing. Our customer has the part listed as a "one-time use throwaway" type deal. So we need lots of them and on the cheap.

[Fig sign]

Try to use HSS ball mill ,low speed reasonably big feed

Raise your tool after every cut high enough for

airblast to clean it .

Airblast must blast the part and the mill too.

Do not make slow feed ,otherwise the chip will

spin over mill .

PP is not the end of the world .

Why ball mill ? _less vibration ,smoother cutting conditions ,better strength of mill.

You can fast enough mill the slots with end mill after that ,if you`ll need it ,if you decide to use ball mill as a rough mill .

BTW , I used once an air-blast with a cooler .

May be useful in this case

As a last resort drill slots with ball mill before slotting .

Same thing low speed reasonably big feed ,and jumps short enough to not spin chip over mill

.

BTW ,can you use as a coolant alcohol ?

If it not dissolves PP it is sterile too and can cool your parts .

You`ll need to wear mask ,or you`ll be dizzy LOL !

 

Best regards

[Fig sign]

May be some stuff like vodka :

60% distilled water ,40 of ethanol and no recycling

[Tom Dorgan from American Precision]

I would vote for the slitting saw. Nice clean cuts and you can get them with the radius as well. Set up several on arbors in a vise and slot several at a time.

[MACHINEMASTERG]

id vote for the slitting saw also with a cold air gun blast but i also like the idea of alchol as a coolnt and it cleans as well also try frezing the parts in the frezer before machining and see what that does for the melting ???just a thought ive done this before when working with rubber and it solved some of my melting problums