Looking for some insight on machining carbon fiber sheets


Results 1 to 12 of 12

Thread: Looking for some insight on machining carbon fiber sheets

  1. #1
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default Looking for some insight on machining carbon fiber sheets

    Wasn't sure where to put this. Can be moved if there's a more relevant section.

    Lately I've been doing some jobs for a drone company. Mostly just prototypes and small preproduction runs. I'm cutting small parts out of 2mm, 3mm, 4mm, and 5mm carbon fiber sheet. Most parts only a few inches in size, many in a sheet. This has been a huge challenge and very hard to be efficient.

    I'm curious if anyone on here has experience cutting higher volume of cf parts and how they do it. The 2 challenges are tooling and fixturing. Currently I'm doing submerged milling since it gives the best tool life, best looking edge, and completely eliminates all dust. Very bad stuff to breath. I'm doing this by first holding the sheet down at the corners and drilling all the holes in the parts. Pretty much everything is 3mm holes for m3 screws. Then I drill the same holes with a 2.5mm bit in an aluminum plate. I pick at least 3 or 4 holes per part. These 2.5mm holes in the aluminum plate are then tapped for m3 and I screw in 10mm tall standoffs. The drilled carbon fiber sheet is then placed on top of the standoffs, and secured with m3 screws so every part is supported as it's cut out of the sheet. I then proceed to fill the milling bath with water and a small amount of coolant to slightly above the sheet and cut all the parts. For tooling I'm using a diamond pattern or "burr rotary tool", which seems to be the most recommended tool for cf plate. Running at 24k rpm. Ive experimented with quite a few and tool life is terrible. A regular uncoated 2mm cutter lasts about an hour before it dulls to the point of no longer giving a perfect edge, or snapping. Fastest I can feed without snapping tools is about 100mm/m (4 inches) in the thinner stuff, and 60mm/m in the thicker 4 and 5mm sheets. At that feed, an hour doesn't get you that many parts. A 400mm x 500mm sheet full of parts can be many hours of machining time. Ive tried diamond coated tools and that only increased life maybe 50%, but 4 times the cost of uncoated, so not efficient at all. When using the cheaper uncoated tools, the cost isn't terrible, but the problem is having to babysit the machine to watch for snapping tools and changing it out often. These jobs wouldn't be bad if it could just run reliably unattended for at least a few hours. Aside from the tool life issue, my fixturing method with the tapped holes in aluminum and standoffs is obviously tedious and somewhat expensive. There has to be a better way but I don't know what it is. The company I'm doing the small runs for has their production runs done in China for less than half what I charge and as it is, im only getting 20/hr or so. They only use me for the quick turnaround time when needed in a hurry.

    How are these parts being cut in volume efficiently and cheap? I guarantee they aren't fiddling around with tapped holes in plates and standoffs. Is there a better way? Tabbing the parts instead of holding every part down is not an option, since sanding every tab off to get perfect edges would be even more manual work than using standoffs. Also when I don't suspend the sheet above the surface, tools snap much quicker since it cant evacuate chips above and below.

    Anyone have some insight on this?

    Similar Threads:


  2. #2
    Community Moderator wendtmk's Avatar
    Join Date
    Dec 2005
    Location
    USA
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    Waterjet.

    Mark



  3. #3
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by wendtmk View Post
    Waterjet.

    Mark
    Yeah, that's what another guy told me. Bad news for me since I don't have that capability, but at least good to know how it's done efficiently



  4. #4
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    So it sounds like waterjet is the best way to do this, but since I can't do it that way, is there any way for me to improve my process? I'm considering investing in dust collection and trying it dry. Biggest issue i need to solve is holding parts as they finish cutting. Is there any option other than screwing them down through the parts after they've been drilled? I considered an mdf vacuum table, but i would be really surprised if it held on to the small parts



  5. #5
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    33794
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    and as it is, im only getting 20/hr or so
    At $20/hour, you're not really making any money. Especially with all the aggravation.

    If you can use a 1/8" tool, maybe these? They claim cutting speeds in the 30-35ipm range.

    https://www.amanatool.com/46008-k-so...outer-bit.html

    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  6. #6
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    At $20/hour, you're not really making any money. Especially with all the aggravation.

    If you can use a 1/8" tool, maybe these? They claim cutting speeds in the 30-35ipm range.

    https://www.amanatool.com/46008-k-so...outer-bit.html
    That tool looks very promising, just ordered a couple. If it does what the feed/speed chart shows, I'll be 5 times as productive. Looks like it takes a different approach than the more common diamond pattern cutters which you basically spin as fast as you can and feed slow to grind the carbon away. This tool makes an actual chip, .003. Not only blows away my current feedrate, but at 3 thou chip, I don't think dust is gonna be a problem. Really hoping it does what it claims. Price isn't bad either. Thanks for the tip!

    As for the 20/hr I'm using to bid, it's really not terrible considering it's a home built machine that i run at home after work and on weekends. Basically no overhead. Also 20/hr is on top of what I figure for tooling and material. But yes, it's still not great considering I have to baby sit the machine. Although if these new tools work out the way they're supposed to and I keep bidding the same, not only will a 10 hr job turn into 2 hours, but I'll be able to leave the machine alone or at least work on programming other stuff

    Last edited by QuinnSjoblom; 06-11-2019 at 02:36 PM.


  7. #7
    Member
    Join Date
    Apr 2004
    Location
    Oakland CA USA
    Posts
    4736
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    You're right; dust is going to be a problem if you do this dry. I doubt you'll be able to effectively remove it in your home shop. I'd say keep doing it under water, the way you've been doing it heretofore; the new tool should work under water at least as well as the old one.

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  8. #8
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by awerby View Post
    You're right; dust is going to be a problem if you do this dry. I doubt you'll be able to effectively remove it in your home shop. I'd say keep doing it under water, the way you've been doing it heretofore; the new tool should work under water at least as well as the old one.
    But with a 3 thou chip using the new tool, will it really even be dust anymore? I would think it should at least be coarse enough to not go airborne

    Hmm, apparently they dont know how to do math. First of all, it shows 2 thou, not 3. I was wrong there, but it's still way off. For the 1/8" 10 flute tool, slotting at 1xD, it says 18 inches/minute at 12,200rpm and .002 chip load per tooth. Not even close, I'm getting 0.00014, (about one and a half tenths). Still a much bigger chip than running the burr cutters at 24k and 3 inch per minute, but nowhere near 2 thou



  9. #9
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    33794
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    Yes, there will always be dust.

    running the burr cutters at 24k and 3 inch per minute
    This may have a lot to do with your short tool life and broken cutters. Have you tried higher speeds and/or lower rpm?

    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Member
    Join Date
    Nov 2017
    Location
    United States
    Posts
    406
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    Yes, there will always be dust.



    This may have a lot to do with your short tool life and broken cutters. Have you tried higher speeds and/or lower rpm?
    Increasing the chip load by either lowering rpm or raising feed snaps the cutters even quicker. I think that's just the way those burr cutters are though. The amana tool has actual flutes on it



  11. #11
    Activation process peteeng's Avatar
    Join Date
    Jul 2018
    Posts
    471
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    Hi Quinn - Onsrud have composite tooling as well. Peter

    https://www.onsrud.com/Series/Composites.asp



  12. #12
    Member
    Join Date
    Mar 2017
    Location
    United States
    Posts
    771
    Downloads
    0
    Uploads
    0

    Default Re: Looking for some insight on machining carbon fiber sheets

    Quote Originally Posted by QuinnSjoblom View Post
    But with a 3 thou chip using the new tool, will it really even be dust anymore? I would think it should at least be coarse enough to not go airborne

    Hmm, apparently they dont know how to do math. First of all, it shows 2 thou, not 3. I was wrong there, but it's still way off. For the 1/8" 10 flute tool, slotting at 1xD, it says 18 inches/minute at 12,200rpm and .002 chip load per tooth. Not even close, I'm getting 0.00014, (about one and a half tenths). Still a much bigger chip than running the burr cutters at 24k and 3 inch per minute, but nowhere near 2 thou
    Cutting carbon fiber always produces dangerous dust. Speaking from experience, you should invest in a quality forced air mask. Any regular dust mask won't work. I have met people who weren't careful when cutting CF. They can hardly breath...

    You also need to be hyper vigilant about vacuuming with a shop vac that has the appropriate filter to stop the micro dust getting back into the air. Even if you cut under water, that black goo will dry and go airborne the following day...

    If you can't invest in the appropriate safety kit, $20 /hour is not nearly enough to risk your lungs imo.

    On the spindle speed / working time, It would be better to invest in a higher speed spindle. NSK make some 50,000 rpm spindles for composites and there is usually a few used ones going cheap on ebay. 24000 rpm is not enough to do a great job on composites with small diameter tooling.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Looking for some insight on machining carbon fiber sheets

Looking for some insight on machining carbon fiber sheets