Hey you carbon fiber guys

[Jeremy Herron@DBS Solutions™]

I have a trim project that is carbon fiber about .2 thick. My custom does tons of Kevlar, but not much of this stuff. The parts we have just work so I haven't messed with them. What tools, speeds, and feeds would you start with? I did a search but I didn't come with much.

[mkd]

Onsrud has a line of CF specific tooling.

cant say enough about diamond coatings or Diamond like coatings/ worse case.

 

i've rung .38 cutters in the 5-10k range, but have not done extensive testing of one setting vs the other to chart tool life.

[Jeremy Herron@DBS Solutions™]

I stared with a 3/8 uncoated at 7500 rpm and 15 ipm. I have to slow it down so much due to having the tool hungout 10 x d on this Temporary MDF fixture. I have some 1/4 diamond coated I can run.I will just have to get creative with my clearance.

[CJep]

The smaller dia tool is not going to grab as much. I've used reversed flute tools with thin materials, they tend to keep the material from climbing the cutter.

[Oscar R.]

http://www.onsrud.co...oc/Carbide-Burr

 

This is what we use.

 

You can run the Burr or Carbone Graphite ones pretty fast for roughing(leave .02"-.015"). Then just finish with carbide.

 

I usually start with 4000rpm at 30-40ipm depending on the hangout and depth of cut, for roughing.

 

With dynamic milling I've cut G10 with a 3/4 or 1/2dia. Diamond Burr at 3500rpm @ 75-100ipm, full radial d.o.c., 15% stepover. Like butta.

Haven't gotten the chance to try dynamic milling on Carbon Fiber yet though.

 

Carbon fiber tends to delaminate a little easier though. Just food for thought.

 

 

3.750" stick out maybe a bit of an issue though.

Edited June 11, 2014 by Oscar R.

[Jeremy Herron@DBS Solutions™]

I cut some extra clearance on the fixture. I can run the 1/4 diamond burr stuck out 1.5" now. On the other carbon fiber part they run it at 8000 and 30 ipm. I will start at 4000 and 30. I was having to slow the 3/8 down so much it was burning.

[Oscar R.]

Burning, yup, sound like the rpm is kicked up way too high.

 

1/4"dia., 1.500" stickout should be no problem.

 

Let us know how it turns out for you.

[Jeremy Herron@DBS Solutions™]

Will do.

[jfich]

I cut variety of different carbon fiber materials every day. This is the best all-around cutter I have found. Without going to the expensive PCD cutters.

Regular end mills will cause the material to delaminate and will wear down extremely fast.

 

http://www.onsrud.com/product/Item/m/itemDetail.html?q=66-911altin&itemId=66-911ALTIN

 

My default RPM is 9200, IPM is 50. This can change a lot depending on the fiber in the material. When I first started cutting carbon I was surprised how much feeds and speeds vary depending on the type carbon and fibers that are used. Kevlar, Aramid and ceramic fiber will burn the cutter up fast and there is not a lot you can do about it. I have found that using the smallest cutter diameter possible seems to work the best. You shouldn’t have any problem using a .250” cutter on .200” material but might have to slow the feed down.

 

This cutter will leave little ridges down the trim since it is a diamond shaped flute. If you need a smooth edge just come back and have a finish pass with a regular end mill, finishing the least amount possible. I try to leave less than .010". If you use a diamond like coated end mill for this it will last a long time, they can be found fairly cheap.

[Jeremy Herron@DBS Solutions™]

The first cut is a full slot to remove the excess. It seemed to be cutting good 4000rpm and 10ipm. I started increasing the feed rate and I think it snapped at around 20.

[Oscar R.]

The first cut is a full slot to remove the excess. It seemed to be cutting good 4000rpm and 10ipm. I started increasing the feed rate and I think it snapped at around 20.

 

Are you running air or anything else on this for chip evac?

What's the D.O.C?

Seem like a pretty slow feed to snap a tool unless chips clogged up in there. Which is pretty common by the way, especially on a full slot pass.

[Jeremy Herron@DBS Solutions™]

.3 (.2 of carbon fiber + .1 of MDF). and doh! I forgot to put the air lines back.

[Oscar R.]

.3 (.2 of carbon fiber + .1 of MDF). and doh! I forgot to put the air lines back.

 

Doh!

Yep, ya gotta let the tool breath a little. Man, I'm surprised the MDF didn't catch fire on you, LOL.

[guitar]

Mind if I suggest a compression cutter for the finish pass? This type of cutter prevents burring along the top and bottom edges of the part that composites and plastics are notorious for.

[Jeremy Herron@DBS Solutions™]

Okay, with air it cut fine at 30 ipm. Compression cutter?

[Jeremy Herron@DBS Solutions™]

Doh!

Yep, ya gotta let the tool breath a little. Man, I'm surprised the MDF didn't catch fire on you, LOL.

 

LOL. Who said it didn't a little.

[Oscar R.]

Compression cutter?

 

They're definitely worth a look into, but are a bit more $ than standard carbide tools.

 

Here's the sales pitch.

 

[Jim at Gentex]

Not much to add, just confirming what others have said here based on my own experience.

 

+1 on the Onsrud tools!

 

Also the down-spiral flute for thin section materials works great, and the smaller diameter tool the better is a good rule of thumb.

 

Speed / feed is also key as jfitch points out, and is dependent on the type of material.

Again, the general rule of thumb is lower spindle speeds to prevent burning / glazing / chipping of edges, and also helps tool life.

 

Unfortunately it often comes down to trial and error to get the speed & feed dialed in for any given material.

However if you have a good starting point it's usually not too painful a process to tweak the s&f to get the best results.

[Jeremy Herron@DBS Solutions™]

Well all the 2d panels ran well at 4000 rpm and 30 ipm. Now for the 5-axis ones. Thanks for the help guys. This was a tear down project and I had an AOG.

[Oscar R.]

Glad it turned out good, and as always, glad to help.