AMCNitro

Anybody have experience cutting Carbon Fiber?

Recommended Posts

At first I drilled it with cobalt drills, knowing that it wasn't ideal, but it was a prototype made in quickly.  Then I bought carbide drills, but still having the same problem.  The problem Im having is the hole delaminating slightly when the drill comes out of the other side of the sheet.

Share this post


Link to post
Share on other sites

HSS drills will work in a pinch, carbide is preferred, diamond coated dreamers are best for drilling. I would try to helical bore holes in carbon fiber making sure to support the material around the holes for best results. there will more than likely be some delamination  however you produce the hole, keeping it to a minimum is the goal. Use a solid carbide multi flute c-sink tool on the backside of hole to clean any delamination. good luck, 

P.S. use plenty of air on the tool

  • Like 1

Share this post


Link to post
Share on other sites

I heard talk of "down cutting" reverse helical endmills for lamination issues.

35 minutes ago, MetalSlinger5 said:

diamond coated dreamers

almost married one of those!

  • Like 1
  • Haha 2

Share this post


Link to post
Share on other sites

1/8 th diamond cut carbide endmill or microcut will do a nice enough job for high quality edges with no delam. 

Having suction from a vacuum head is ideal..

  • Like 1

Share this post


Link to post
Share on other sites

Best solution is to use a Compression Cutter, which is undersized to the hole. For a .500 hole, use a .375 or .250 cutter. Plunge or tight-helix through the material, slowing down just before the hole exit. (0.03-0.06 before the material bottom [0.75-1.5mm]), then Circle Mill to the finish diameter, with entry/exit. Sometimes we had better luck with Conventional Milling! Don't be afraid to try weird stuff in Carbon Fiber or Fiberglass.

Try Plastic Drills, and crazy endmills including 1-flute tools, can work. Sharp, sharp, sharp tools, with lots of rake and relief angle. 

For small diameter drills, I've used Brad Point (I think that is what they are called).

The tip is shaped like:

|    |

|    |

V V V

Where there is a tip in the center with a sharp point, and two sharp chisel points, on the outer edge. They work great for composite panels. Feed through the top skin at F20., for about 0.12", then feed down through the core at F200., and feed the last 0.12" through the bottom skin only, at F20. This same technique can be used with regular Plastic Drills as well, but don't over-feed through the core. If your drill isn't sharp, it won't shear the paper core. It will push the core down and compact it, which will cause a big patch of skin to delaminate, and may break the drill, or shove the packed core to the side (stays trapped in the panel).

 

Share this post


Link to post
Share on other sites

The holes I'm having problems with are 1/8 diameter and 3/32 diameter.  Ill try the Bad Point drills and feed it faster.  The sheet is only 4mm, so it should ok.  As far as cutting it with endmills I haven't got there yet, but I was planning for diamond cut endmills like THeByte said.

This is for a project of my own that I'm working on on weekends and after hours, so its slow going.  I appreciate all the help.

Share this post


Link to post
Share on other sites

The small endmills by MICroCut are .03125 or they will surely not delaminate, however the feedrate is small and a ramp entry is a must, tools are also prone to breaking on the probe at that size if thats a thing, .0625 diamond cut sounds the best in that case, likely 1 shot cut w/lead in no depth cuts.

If the carbon fibre is thick enough for compression cutter it could be good i suppose, usually the upcut portion is thicker than the material unless you are planning to cut deep in your table/fixture. I dont waste my time with compression tools mostly they are only good for mdf.

Share this post


Link to post
Share on other sites

I wouldnt suggest drilling either..

I wouldnt suggest drilling either..

Share this post


Link to post
Share on other sites

Compression Endmills are really not designed for full carbon fiber sheet. They are designed to machine a 'composite sandwich', where you have 'pressed skins' on some type of lightweight core material.

I'm with Peter on this; I'd recommend not drilling the sheet, and using a small endmill/router bit, to machine the holes, rather than drilling the holes. Use a helical ramp, then spiral outwards to the finished diameter.

  • Like 2

Share this post


Link to post
Share on other sites

Cutting 2 and 3mm CF plates I use these and they seem to last and have seen no delamination.  

carbide tools.jpg

  • Like 2

Share this post


Link to post
Share on other sites

Depending on how many of these parts you are going to cut.  For a few, diamond cut routers and brad spur drills are the ticket. They are inexpensive, but a bit slow and wear out quick.  For long term production, I generally prefer diamond coated routers like OSG BNC and PCD drills, Robbjack has a good selection, many others out there.  This combo has given me an average 60% cycle time reduction and 700+% tool life increase.  A bit pricey, but they last a long time.  Carbon fiber is all I have cut in the last 8 years.

  • Like 2

Share this post


Link to post
Share on other sites

I recently purchased a 3D cnc table top router to cut 2mm and 3mm carbon fiber sheets for RC cars making out of date parts for people and making new parts. The machine I got came with free software for programming and design and software to run the machine, Does anyone know of a good easy to use software program for 2D design, I've been using MC but can't do it all the time when needed. the files I create to cut are all wireframe DXF files I haven't figured out there design software yet but programming and cutting is pretty simple. Does anyone know of a good easy to use design software similar to MC that's either free or will not break the bank? 

Share this post


Link to post
Share on other sites
7 hours ago, TERRYH said:

I recently purchased a 3D cnc table top router to cut 2mm and 3mm carbon fiber sheets for RC cars making out of date parts for people and making new parts. The machine I got came with free software for programming and design and software to run the machine, Does anyone know of a good easy to use software program for 2D design, I've been using MC but can't do it all the time when needed. the files I create to cut are all wireframe DXF files I haven't figured out there design software yet but programming and cutting is pretty simple. Does anyone know of a good easy to use design software similar to MC that's either free or will not break the bank? 

Thats exactly what Im making.

Havent had a chance to work on the project since the post.  Ill update you guys when I go back to it.

Thanks for all the help so far.

Share this post


Link to post
Share on other sites

Rhino is pretty awesome. Fusion is decent, and free for hobbyists. Rhino is more for surface modeling, and you can get some cool plug-ins to do things like parametrically pattern a surface. (Grasshopper) www.rhino3d.com

 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us