What's new
What's new

Melting cutters in g10 fr4

MiniMachinist13

Plastic
Joined
Jul 13, 2022
Having an issue with our cutters in g10. Using 2 flute carbide 1/4in at 8k rpm with a feed of 150ipm. DoC is .135in. After one set of parts cutter has already lost .0045in on diameter and by the second set of parts the corners are rounded and the tool is at ~.241in. Is there anything we can do to keep the rpm’s and feeds without sacrificing cutters every 10 minutes?
 
+1 firstly your running way too fast, secondly it's G10, cutters aren't going last long anyway.

Is the G10 de-laminating at those speeds?
 
Seems pretty fast. G10 does eat through tooling. You could try some CVD coated tooling. I think that might be your best bet. A tool that might work is linked below:
 
You want around 150-200 sfpm max unless you're using diamond coated tooling. But you can feed it fast. Just beware of edges, they will split and delaminate on you. Approach each edge by cutting into the part when roughing, try not to cut toward an edge when roughing or else it will most likely split/crack on you.
I cut this shit all the time and the best non-diamond coating that I've found is TiCN coating. It will still break down,but it will last longer than other coatings.
If you're using UNcoated then you're just going to replace the end mill constantly.
 
Cutter must make a chip, not dust. Chip may easily crumble to dust. High rpms produce high heat and a chip carries more of that away then dust. Cutter gets attacked by both the abrasive qualities of the material, and a chemical reaction from released stuff from the material. Cannot really stop the wear, but speeds and feeds can reduce released chemicals that break down the tool. Coating ^ helps too.
 
G10 is fibreglass-reinforced resin, Scruffy887, as used in printed circuit boards (among other things). It's not going to make much of a chip, no matter what the tool is. Abrasive as hell, and chemical attack on ferrous group elements (including cobalt binder in carbide tools) wouldn't surprise me.
 
When I was at an OEM shop that cut a lot of carbon fiber, G10, and fiberglass, we used tools of this variety for roughing:
The burr tools seem to grab and delaminate less than regular flutes in roughing. We finished with PCD endmills, nothing else would survive long enough to trust, but we would leave them running for hours. In any case, 150 IPM seems really fast, what thickness of G10 are you cutting?
 
Last edited:
This material is OLD.

I remember we had moved off "XXP" Phenolic to FR4 for PCB's before 1960 arrived .

Drilling it was only done for the onesies in the R&D lab. For production, 22 holes in a tiny hand-wired, pre-integrated-circuit, all "discrete-components" hearing-aid PCB, we PUNCHED.

Not that punches didn't wear. But the holes all went in at one go, and we shop-fabbed and heat-treated replaceable pins for the progressive die by the batch every day, and rather cheaply.

Surely 50 or 60 years on, there must be an easier to machine material as can get the job done?
I didn't make it clear, I was only referring to the general shape of the tool, the "burr" type, not those tools specifically. I'll ask one of my old coworkers who is still there to see what specific tools they are using.
 
PCD is the ultimate cutter for this job, and will last longest by far, but they are very expensive.
Harvey has some too, and yes those aren't cheap.
What we do is buy uncoated end mills and drills, then send it to our resharp guy and they have it diamond coated. It's not perfect but they last way longer, and this is a much much cheaper route than buying OTS diamond tooling.
 
G10 is fibreglass-reinforced resin, Scruffy887, as used in printed circuit boards (among other things). It's not going to make much of a chip, no matter what the tool is. Abrasive as hell, and chemical attack on ferrous group elements (including cobalt binder in carbide tools) wouldn't surprise me.
Understood. But any cutter will loose is new sharp edge in seconds or minutes in phenolic. If chipload is very low you will end up rubbing the material away. Hot nasty dust. I have a production part that I make from .375 linen phenolic. The part is about 5" x 1.25 sort of shaped like an S. Cut out with a down spiral 5mm Onsrud bit, single flute. These are nested parts and a bit will generally last through 4 sheets of 48" x 96". Once in a while a piece will get loose and the bit will snap if plunged into a loose piece. That is a lot of parts and the bit gets tossed every 4 sheets.
 
I looked up an old job 1/8 2 fl carbide 9000 rpm 40-55 ipm
3/8 or 5/16 3 fl carbide 9000 rpm 75 ipm
100s of parts 1/8 thick, larger end mill had about 19 inches of contouring per part
feeds are probably more related to keeping the part in the machine than cutting efficiency
yeah tools wear. Its why they make tool comp
Used to do a job cutting circles ~1" out of 1/4 plate with a 5/32 ball endmill and 4 holes, if I could remember the part number I could look it up
 
yeah tools wear. Its why they make tool comp

That's fine and dandy as long as you're making a 1 off. But if you have a whole pallet of dozens of parts, then find out that you need to re-run the finish cycles because you're too proud to run the tool correctly you've just wasted a ton of time with something that could have been avoided.
 








 
Back
Top