Waterjet.
Mark
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:
Waterjet.
Mark
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
At $20/hour, you're not really making any money. Especially with all the aggravation.and as it is, im only getting 20/hr or so
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
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
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.
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]
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
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?running the burr cutters at 24k and 3 inch per minute
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Quinn - Onsrud have composite tooling as well. Peter
https://www.onsrud.com/Series/Composites.asp
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.
I work on luxury yachts and deal with FRP's non stop. I would strongly suggest a FLAT foot dust shoe for dust collection with carbon dust. I see your using a RASP bit in your photos. !GOOD make sure your running 25k RPM minimum. I run 60krpm using an AIR pen grinder on a cnc with diamond grit bits. Air tools are immune to carbon dust electrical conductive issues. If you are ever running into tear out with the rotary rasps, ether ensure your not pushing to high of a feed rate OR low rpms. Using a festool vacuum is a good idea also having your exhaust air piped outside is very important as well. The festool contains the carbon dust and has extra filters in the system. It also makes it easy to clean. Full bag toss it in the dumpster, blow out the filter and the body of the festool vacuum OUTSIDE and reset. If you have an FRP questions I can likely answer anything. I use to build Hinckley yachts. The average yacht I work is worth $50k-$50million and we the company I work for do everything.
Using a water table will work but You will likely find that its more of a pain then a blessing. Blessing if you use a pump system to keep the water moving and use a filter system. FYI carbon will absorbs water and turn into a sludge that clogs filters fast. You will need gloves to remove the parts from the water. As the water gets dirty it will be hard to remove parts FROM the water and same with screws. all in all dry with good dust removing and outside collection system is the ideal choice.
Holding down Carbon, I always suggest using Starboard hold downs. there are a million different designs but I would suggest using 3/4" Starboard and cut hold down tabs. They will flex a bit when under high torque but they wont snap likely. And they are very unlikely to leave marks on the carbon. Peronally if you have a set design for parts that your going to make a lot of. I would suggest an elevated holding system. That way you can cut all the way though the carbon with out wearing the waste table.
Below an example of my starboard hold downs and a Starboard vacuum plate for doing milling on my home cnc machine.
Last edited by berin; 11-10-2019 at 10:32 PM.