Carbon Fiber cutting Feed/Speed values ?

[CyberPlainsDrifter]

Hi Guys,
Ive got a client requesting me to cut some CF. Seems like he has multiple peices...


Anyone have some good feed / speed values to start out?

Material I think is 3/16th thick (bullet proof?!?!?) and If possible Just to cover the bases,
Im looking for values related to:
1/4" tungsten bit
1/8" tungsten bit
1/16" tungsten bit

I suspect that in order to reduce material fraying , a straight fluted bit should be used...But single double triple or quadflute is also a question..

I wont even mention diamonds... I think this -even though its the right tool for the job, it has been priced far out of reach at this juncture...

Ive got the machine and a good mask.. I just need some math..

Thanks in advance...

If I can get to the bottom of this, I will be considering making parts for our hoby too. Not just carbon but various palstic parts too.. "made in North America"

Regards, Rich.

[TMoore]

What HP spindle do you have available, how tightly can you hold the workpiece and when you say Tungsten, do you mean Carbide?

TM

[CyberPlainsDrifter]

Yep, Tunsten Carbide bit. (High Rockwell bit) and I can clamp the work down as much or as little as needed.

Diamond bits are supposed to be the cats a$$ but pricy.

The spindle I use is an HSD (made in America!!!) 5HP 3 phase. 3000-24000 rpm. Amazingly quiet at 24K! Has ceramic bearings...

Got any speed/feed values?

Im starting to get the impression that I am going to have to simply do some of my own testing.. Not a lot of info out there and the people who do have info seem to be apprehensive about giving it up.. Like its a big secret or something... Anyway that could just be my own brain feeding me disinformation....

Cheers, Rich.

[TMoore]

For one thing the stuff cuts like butter but CF is abrasive so that will determine the F/S that you can run the cutter at because it will wear out not from cutting pressure but from the abrasiveness of the material.

Start with a .125" cutter at full depth, 7500 rpm at 15-20 ipm. This isn't very fast and I would start with the Feedrate override down at 50% and ramp it up with a little air or vacuum in the zone. After you get a feel for the cutting action, I would say you could triple the speed and feed without splaying the material if the machine is rigid enough.

TM

[CyberPlainsDrifter]

Thank You Mr. Moore.

I will attempt a cut at your suggestion. See where it ends up. I had a figure in my head of about 21000 @ 60 ipm... Your figures and my figures jive.. So maybe I was in the ballpark all along...

Thanks again for your inputs! Much appreciated.

Regards. Rich

[CaptainIncompetent]

I think TMoore has suggested a good place to start, but keep in mind that a CF (or any FRP) layup is anisotropic to a degree that few other materials are, so expect to spend some time and material on experimentation.

Probably not helpful if you only have a mill, but if it's just flat sheet, waterjet really is a better choice for this.

Good luck!

[TMoore]

A water jet is completely unusable in CF. The jet splays the CF at the cutting zone and it delaminates. I sell WJ's and I've tried it on the stuff that I've sold in the past and it is not workable.

TM

[CaptainIncompetent]

I've had good results having CF cut via waterjet, but I emphasize the disclaimer that there is huge variation in layups, so ymmv.

[X-Gear]

I just cut a 1/4" thick kevlar and carbon layup for some college kids with our waterjet and it turned out very well. There was no delamination, there was a touch of fur along the edges, but there was no delamination of any of the layers.

[TMoore]

.25 is easy to cut compared to 2mm. Try it and see the result. I've never used .25" CF for Frames.

TM

[rcflyerheli]

Go to Harveytools.com. They manufacture bits of all kinds and sizes. Their website has the basic formulas for feed rates based on material/bit parameters.

[CyberPlainsDrifter]

That is a great link! Everything there to get a guy goin'
Thanks alot...

My latest project was for a Trex500 I cut some rudder control rod guides for a bud at teh field.. check out the photo..

Thanks for the great info guys!

@Tmoore The .25 was for a custom tool/projector mount.. nothing to do at all with Heli's. I got a really sweet piece of 1/16 CF today.. Im going to cut some parts for my Mcpx and 250..

So with the formulae that are available at Harvey tool , this should be a cake walk!

[kustom20]

Hi All,

I noticed this old thread and wanted to add some input maybe of some help for anyone milling carbon sheet.

Material Sheet Thickness 2.0mm
Rotary Burr Cutters - normal single 2 flute 3 flute etc end mills can cause delamination and pull fibre strands

1.4mm 1.5mm 1.6mm 3.175mm cutter diameter we run at 100mm per minute 3.0mm depth cut - 20,000rpm (1.0mm below material thickness)

Material spaced 3.0mm above milling table with 3.0mm plates in each corner - this allows 2.0mm material to drop below the lowest part of material and cutter depth - t-bolt clamped in each corner

Material submersed underwater for cutting - not cutting fluid.

The final finish is excellent, the resin stays in tact and no excessive heat due to water, no delamination, no strands of fibre uncut, no whiskers so to speak, and no dust in the air keeping it all contained in liquid.

We could ramp the speed of 3.175mm up to 200mm per minute but we get a slightly lower cut quality on the edge.

We have cut 2.0mm sheet at 400mm per minute with 3.0mm cutters but we prefer a better finish quality on the edge produced by slower feed.