[ranchak]

I've looked around on the interent and can't seem to find an answer. I'm machining 3/8" thick phenolic, G10FR4. What I found is guys cutting with 1/2" - 1" diameter cutters, cutting at 800ipm. My problem is I am using a 13/64" cutter and I can't cut at 800ipm. I have a FlexiCam router with a 3HP spindle. I was cutting at 30ipm, a depth of cut at .125". Spindle speed around 10,000-12,000rpm. This was working until the cutter got dull, which was pretty quick. Well I scrapped the material I was working on and ordered another piece, but I really need to get this figured out before I waste another piece. Can anyone please help? Thanks in advance.

[ger21]

I'd reduce the depth of cut and increase the feedrate to 80-100, keeping the same rpm.
Edit: If that has glass fibers in it, ideally you'll want to use special cutters made for that stuff, as regular ones won't last long as all.

[txcncman]

G10 is a fiberglass composite.

[ranchak]

Thanks for the reply. What I could see most guys are using carbide cutters usually two flute. I was thinking of going to .063" depth of cut and increasing the speed some. I just checked with GFWizard and it says using a .25 end mill at 7000rpm the feed should be 75.8ipm. I guess maybe tomorrow I'll try cutting some plywood at these settings and see what happens. I'm worried that the speeds are going to be a bit fast for cutting a hole that is 2" in diameter. I'll never know until I try!

[txcncman]

Nothing wrong with slowing things way down. 3500 RPM and 20 IPM maybe. And increasing axle DOC to 0.200.

[ranchak]

I got better results running with the settings that I got with GWizard. The edges are not real smooth in some areas, I'll wait to see what the customer thinks.

[FlexiCAM]

FlexiCAM uses custom made three flute cutters for machining phenolic.

We are doing LOTS of them (most machine vacuum tables are made from phenolic, so you can imagine).

Tools are available in 3/8" and 1/2".

For your application I would recommend the 3/8x1/2x3/8x1-1/2 3FL Upcut (FlexiCAM P/N TP096).

Drop me a PM if you are interested.

[rockcliff]

phenolic board is for sure one of the top 5, on my nasty material list,

I normally will use a rasp type carbide cutter, it will leave a rougher edge, but seems to be better for cutter life.

I always try to order Cotton based phenolic, which is a bit easier to cut then the fiberglass based

[uli12us]

For this material yo should use diamond coated tools. They are rather expensive, but lasts much longer than any other tools. If you can get it, you should buy a tool with filleted edge, that increases the tool life dramatically.

[cncshootist]

I know I'm digging up an old thread, but my searches keep returning with links here...

I've read similar posts, all questions, no answers. Even the length specific-bit thread did not cover phenolic. I tried to PM the original poster, but he has them turned off.

I'm running into the same problem (for g/10 and micarta) but haven't seen a posted solution for speeds and feeds with high rpm, and small dia bits. I'm running a shopsabre 4x4 sidekick and have even bought Gwizard to help out. Gwizard's site talks about diamond cuts, but they aren't a tooling option in Gwizard itself. I've bought a few as they're supposed to be designed for phenolics. And I'm wondering exactly what they're capable of and what they can be run out with my (or similar) machine.

If anyone has specific information or info on what they are using as a substitute for Gwizard, it would be helpful.

Thanks,
Matt

Thanks,
Matt

[Hezz]

I've looked around on the interent and can't seem to find an answer. I'm machining 3/8" thick phenolic, G10FR4. What I found is guys cutting with 1/2" - 1" diameter cutters, cutting at 800ipm. My problem is I am using a 13/64" cutter and I can't cut at 800ipm. I have a FlexiCam router with a 3HP spindle. I was cutting at 30ipm, a depth of cut at .125". Spindle speed around 10,000-12,000rpm. This was working until the cutter got dull, which was pretty quick. Well I scrapped the material I was working on and ordered another piece, but I really need to get this figured out before I waste another piece. Can anyone please help? Thanks in advance.

The kind of phenolic you are cutting will effect things a great deal. Usually phenolic panels are composite panels with phenolic and paper, linen, glass fibers or carbon fiber. If you are cutting the glass fiber kind it's just going to be really hard on your tools and you probably won't get much tool life. It looks to me that you may need to bring your RPM's down and your feed rate down as well. Some kind of water based emulsion coolant may help with this if you can do it. Since most router don't use coolant you can try putting some in a spray bottle and doing it by hand.

First a reality check. This stuff you are trying to cut is more difficult than cutting mild steel. So if you are approaching it from a kind of wood material mindset it's just in the wrong ballpark.

This is really tough stuff you are cutting and usually it would be cut on a mill rather than a router. It can have a higher strength to weight ratio than steel and most routers are designed to cut wood and plastic and foam. If you are using a HSS end mill you should try out a cemented carbide end mill. But they are expensive compared to HSS. It could be that high speed and feed and shallow cuts would work the best. Try a little large endmill if you can. A .500 inch if you can get one. If it will fit in your machine. Make sure the end mill is short. No longer than two inches out. The shorter it is out the better. For a 13/64 endmill it should extent no longer than about 1 inch or less for hard materials.

You need to try some more cuts on that scrap piece you have until you find what will work the best on your machine. Try using a high feed rate and shallow cut (.063) but make sure that your RPM is set correctly for the feed rate so that each chip is the correct uniform size. You will need to consult a machinist textbook if you don't have the formula. If that does't work try slowing things way down. The problem like I said is that most routers are not build rigid enough for this tough material. So you are most likely going to have more than desirable vibration. The vibration will kill the end mill really fast in this kind of hard to cut material. So you need to do everything that you can to minimize it.

If you are using a small DIY router with a wood router motor as the spindle the bearings are just not adequate for the side loading that is required for this tough and hard material. Like I alluded to above. You need to have a machine that can cut steel to do this kind of material.

[Hezz]

I know I'm digging up an old thread, but my searches keep returning with links here...

I've read similar posts, all questions, no answers. Even the length specific-bit thread did not cover phenolic. I tried to PM the original poster, but he has them turned off.

I'm running into the same problem (for g/10 and micarta) but haven't seen a posted solution for speeds and feeds with high rpm, and small dia bits. I'm running a shopsabre 4x4 sidekick and have even bought Gwizard to help out. Gwizard's site talks about diamond cuts, but they aren't a tooling option in Gwizard itself. I've bought a few as they're supposed to be designed for phenolics. And I'm wondering exactly what they're capable of and what they can be run out with my (or similar) machine.

If anyone has specific information or info on what they are using as a substitute for Gwizard, it would be helpful.

Thanks,
Matt

Thanks,
Matt

There is no solution for a high speed spindle except to have a high feed rate. If the machine can't do both it's not adequate for the job. There is a ratio of rpm to feed that has to be respected so that the cutter is not over loaded. But to do this requires high rigidity and high horsepower combined with high feeds and RPM. If the rpm is too high for the feed the cutter is rubbing instead of cutting. Especially with hard materials. So the mill just vibrates and rubs and dulls itself quickly. The smaller the mill is the more exact these calculations need to be. Because the mill flexes more easily.

The only solution is to slow the spindle way down so that is going the right speed for the feed rate that the machine can do and handle.

[BrendaEM]

You might want to wear a mask when the machine is running--especially if running at speeds that might get it hot.