Machining PEEK with 30% Carbon Fiber

[65Mustang]

Hi everyone,

I have a job coming up that I need to machine out of PEEK with 30% carbon fiber.

It's a support bracket with .15 & .1 thick walls, profile tolerances of .002, .160 Dia Hole's and slots w/tolerances of .0005 & true positions of .002 . The part is approximately 2" x 2" x 3". Any good feeds and speeds for drilling / milling with carbide, tool selection would be greatly appreciated. This is a non medical part so can I run it in coolant? Should we stress relieve or just rough & finish. I will be running this on a small 5 axis so I can 90% rough before finishing. I have 20 of these to make so I can buy some specific tools if required

 

 

Thanks

Frank

[Mic6]

I like to use single flute tools like Onsrud for material like these

[65Mustang]

I like to use single flute tools like Onsrud for material like these

 

 

 

Thanks, did you run it wet or dry?

[kh012]

I have had to cut this stuff before. The main problem with the carbon is tool wear, it's outragious. your only running 20 parts so it may not be to bad.

we ended up using diamond coated tools! even the carbide tools will show wear after 1 or 2 parts. professinal plastics has a base guide for speeds and feeds.

we used coolant to clear the swarf.

[65Mustang]

Thanks for the reply.

Do you think that this material can support a dovetail without cracking?

I need to either hold with a dovetail or drill and tap

into the material to hold the part for 5axis machining.

[Matthew Hajicek - Singularity]

I'd expect it to resist cracking, that's what the carbon fill is for. Should be pretty strong stuff. If you tap it you'll wear out your taps pretty quickly. Second on the diamond coated tools.

[Philcott]

PEEK also had a tendency to chip as your drill breaks through so keep your tools sharp. Change them often.

[T_MALENA]

I never touched 30 carbon fiber. But I've run PEEK & glass filled PEEK without coolant contacting the part to "wash the swarf" also. I think it causes the part to swell. Also used diamond coated cutters from Round Tool(D2) & OSG(list 7040). And drilling blind holes was ok. Any through holes were helix milled. Never had to tap. Sharp positive/shearing action & diamond coatings. Please report back with what worked for you.

[65Mustang]

Thanks T_Malena,

I have ordered some diamond surfaced cutters from Harvey tool that I hope will be in next week.

Today to prep the material I used a 3 flt carbide TIALN coated mill @ 400 SFM and dulled the tool

in about 9 mins. This SFM is apparently to fast. What SFM did you use?

[T_MALENA]

I had small cutters & 10k max rpm so SFM wasn't always correct. And the larger cutters running at 600sfm didnt take long to cut & didnt wear out. The target was 550-700SFM & 2%-4% of the tool dia in chip load per rev.(.25 mill=.005-.01/rev). Heaver for roughing. Lighter only to get the tol & surface finish needed. ALSO I WAS WRONG ABOUT COOLANT. I did use coolant ON THE PART. Not sure if that will cause you problems but it didn't for me. And you will need to rgh machine to stress relieve before finishing if you'll be removing lots of material. Also the material will delam/fray at the breakout of a through drill & when a mill comes out the edge of a deep radial cut.

 

Non diamond coated - try 250-300 sfm with a heaver chip(4% above ex.) Avoid slotting.

 

Good luck.

[T_MALENA]

Higher SFM is for milling only! Diamond coated drills were 150sfm max. & heavy chip load. I should also clarify I took up to 150% of the mill dia in doc(sometimes more) but only 10-15% in radial stepover. So the programs were long. Tricoidal type cuts etc. So 100% doc=15% radial. 150%doc=10% radial.

[65Mustang]

I'm glad to here that you used coolant! I have lots of material

to remove. These parts are about a 75% Material removal 25% part.