Milling Polypropylene

[MetalMarvels]

Does anyone have any experience in milling black polypropylene. I am looking for suggestions on speeds, feeds, and tooling choices. Machinerys' Handbook wasn't much help..... The various plastics options in job setup don't appear to be working very well.

 

Thanks.

[Guest CNC Apps Guy 1]

I don't remember Speeds and Feeds but I do remember that HSS was the better choice due to the fact that the tools are MUCH sharper and cut better than Carbide.

 

HTH

[Keith Graydon]

hIYA,

James has the key here. SHARP TOOLS. You may need to stone up a small radius on the corners of you mills to. plenty of water soluable( s) coolant. dont let the tools dwell. also be mindfull of chips wrapping around drill bits during drill operations. they can pack and gall the workpiece around the hole as they are forced against it during pecking cycles

 

HTH

-KLG

[chris m]

I agree with James; I'd think 2 flute HSS would be the way to go because of sharp cutting edges and plenty of clearance for gummy chips. I don't know about speed but I'd think that I'd start with conservative speed and a healthy feed to avoid melting the stock.

 

Sorry I'm not more help

 

C

[Jim Whipple]

It's been my experience with plastic to use HSS and spin the Holy Hoopie out of it with lots on coolant to flush the chips. about .005 chip load ought to put you in the ball park

Sometimes you have to slow the feed around delicate sections or reduce the amount of material being taken to avoid breaking the piece

I step down .05 to .125 a pass on lots of parts

I only have a 6K spindle and it lives there when cutting plastic.

Hope this helps

Jim

[Lucky 7]

Is this an expanded polypropylene bead?

[Jim Ruhl]

I agree also the sharper the tool the better and with HSS. Certain cuts may require a conventional cut instead of climb cutting...due to cracking.

Something else to think about.

Even though I don't know exact speeds and feeds.

[Carl Vallance]

Again High speed steel tools

From Machining Data Handbook

End milling Peripheral

300 to 400 fpm

.005 to .010 Inch / tooth

 

Drilling

200 fpm

.003 to .010 ipr

 

Jim Whipple has a good point about delicate sections and step down passes.

[Matthew]

I have no experience with polypropylene, but have machined Acetron. I found that high speed is OK for milling, but for drilling a slower speed (comparable to cutting mild steel) but increase the feed rate. The chips break up much better and do not melt to the part while they are spinning.

[Roger Peterson]

What everybody else said.

 

When drilling crank your fpr way up and have a very high retract plane to help get the strings off. Very gummy when heated up, if your going to plunge into the part crank your plunge rates way up to about double your feedrate. It will stick to your cutter when plunging in if you don't have a very high chip load.

 

Again I don't have any real good #'s for you it's been a while. Set your rpm to whatever you want but I would start at .005 to .007 fpt, you will be able to go up from there.

 

Let us know what works out for you,

[MetalMarvels]

Thanks everyone, looks like some good places to start - particularly with the HSS tooling. I didn't think about it, but most carbide has a blunter cutting angle than the HSS. It makes sense that it would shear the plactic better. I am using a semi-synthetic coolant and tend to stay around 6800 rpm as a max (7500 max spindle - but it heats up fast above 7000 rpm).

 

Lucky7: The material is a solid, high-density polypropylene rather than the expanded bead stuff. I am unsure of the additives to make it black. It about the density of Delrin.

 

It also sounds like a short peck with a fast feed might be one ticket.

 

Thanks again. When I get the stock in (next week - I only had a small piece to muck about with right now) I will let you know what the ticket turned out to be.

 

[datengo]

Chip evacuation is important. Dragiging chips over

the stock will compromise finish. Use a high helix hss. 2 flute cutter. Check the chips to see if they show signs of melting together. If they dont your on the right track

[MACHINEMASTERG]

when we cut plastics hss cutters very sharp as you have all said and climb to ruff conventional to finish leaves clean finish

[MetalMarvels]

Thought I would bring this back up to the top with a status report. The dead-sharp HSS tools make a big difference - great finish with few to no burrs. Short pecks (0.03 inches) and big retracts work very nicely in keeping the stringy drill chips from wrapping onto the drill bit (0.125 inch drill bit). I found that I could pull off .015 inch chips with no issues with full-flood coolant. Thicker chips than that started leaving a poor surface. Step-downs of 0.25 inches worked well also. Choosing my operations order helped significantly in reducing the feathery little burrs.

 

Thanks for the help guys. the parts are coming off very nicely.