3D router tooling

[paulend]

Hi,

I am currently setting up a 3-axis CNC router to be used to cut 3D parts in plywood and resin.

The machine has a 12mm max collet size and would be required to cut at around 120mm in depth.

At present I am using metal working tooling so I would just like to ask for any advice regarding what type of tooling I should be using?

Cheers

[sdantonio]

Personally I'm a big fan of solid carbide end mills. Cobalt is good too. and is TiAIN-TiCN. But I feel carbide is the best for both wood and plastics.

Resin will require a slower spindle speed so you don't melt it into a ball of goo. 10-15K rpm at a 70imp feed rate with an upspiral bit will probably work well for the resins. Keep the depth of cut to about .100 - .200 inches.

See the attachment too.. strictly according to the atachment resins should be run at a spindle speed of about 3K rpm. But you router would have little is any torque at that speed. In rapid feed rate and upspiral bit will help compensate for this.

Steven

[ger21]

I'd guess you might have to get some custom made tooling to get the length you need with a 12mm collet. I don't know about any UK suppliers, but I've had special tooling made at www.vortextool.com

Are you cutting parts in 120mm thick resin? Acrylic or something similar? Depending on the tooling, I'd go faster than Steve mentioned, maybe 150-250ipm. Again, depends on tooling, and what you are making, and the actual material you're cutting. If your'e cutting a deep slot through plastic, it's gonna melt. Very hard to avoid, unless you can use a coolant, or possibly blow compressed air into the slot directly at the tool.

Virtually ALL tooling designed to cut plywood (any woods, really) will be solid carbide, with no coatings.

Another good source of info is www.onsrud.com

[paulend]

Thanks for the replys.

Im currently running solid carbide tools (12mm diameter) at 15000rpm with a feed of 6000mm/min (158 ipm) depth of cut being 3-4mm (I am using a torus/bull-end cutter with 4mm rad) on plywood, which seems to be working OK for roughing.

For finishing I have been running 4000mm/min with a depth of cut of 0.5mm. Is this too conservative?

I have not yet cut resin but you are correct sdantonio, the router has very little torque.

I really need to know more about tool geometry i.e. Wedge, Rake and Helix angles. And what is best for wood/resin. I have been getting most of my advice so far from a metal working CNC machinist.

Paul

[sdantonio]

You should be aboe to get extra long emd mills. I have seen then in MSC

[paulend]

You should be aboe to get extra long emd mills. I have seen then in MSC

Yes I have one 160mm and one 200mm. The 200mm has its shank turned down to 12mm from 16mm.

Should I be looking for "wood specific" tools instead of using the metal working ones I am currently using?

Paul

[sdantonio]

I don't see much advantage in wood specific end mills. I haven't noticed to much of a difference when using them. The gullet shape and chip clearing ability is slightly different. But I think these differences tend to be more important in dealing with the difference between ferrous and nonferrous metals (the impression I get is that cutting metals in a lot touchier than cutting wood) and less important with wood. Gerry can actially comment more on this.

[ger21]

I've never used metal cutting endmills, so can't comment on those. But not only is the chip clearing and gullet shape different, but tooling for both wood and plastics have different cutting edge geometry as well. The downside is that tooling made for wood and plastics is a lot more expensive, from what I've seen.

I'd recommend roughing with straight chip breaker bits, and removing whatever is left with the ballnose. I'd at least try some good quality ballnose bits for wood, and see if they make a difference. I'd think you should be able to go a bit faster.

[carlnpa]

What kind of resin? I cut alot of plastic materials. Ger 21 mentioned Vortex (I tried and liked on Ger recommendation) tools and Onsrud. I use solid carbide 2 flute spiral upcuts intended for aluminum with good results in the 1/2" (13mm) sizes at 8000rpm down to 30ipm. For surfacing operations the tools leading edges should be radiused instead of pointy to provide a smoother less or no fuzzy finish, try 50% stepover. Smaller mills I use HSS 2 flute spiral upcuts for aluminum. The trick with plastics is keep the tool extremely sharp and never allow any stationary dwell of the cutting tool, they will burn instantly, always keep the tool moving. I touch up carbide tools with a fine diamond hone after every run (30-60 minutes run time). The small HSS tools will begin to smear the material when they go (4-8 hours), the cost is low, so I finish the run and replace the tool. These smaller tools can be run down to 10ipm at 15000rpm or so without problem. I have been using the small tools in HSS over carbide due to lower production cost (unable to to touch the edges up between runs).
HTH
Carl

[NIL8r]

Have you tried PCD tooling? (That stands for Polycrystalline diamond) These are very common in the woodworking industry and have a growing market in soft metals as well.
Can be purchased as milling cutters, drills, and reamers. The size your talking would probably require a carbide body with PCD tips.

Costs are more than a carbide tool. But if you handle them with care, you'll make it up in tool life.

I've seen tools from Dihart (www.kometgroup.com) cut aluminum at spindle speeds of 8K RPM and produce as much as 150,000 cuts in 3 inch diameter bores before requiring sharpening. Also, they work great with acrylic. Not sure about resin though. Best part is, with proper speeds and feeds, the surface does not allow the acrylic chips to burn and adhere to he cutting edges.

Hope this helps.

[bradodarb]

I use to use vortex tooling until the carbide mills invariably crept out of the collet. The mirror finish on their mills is sexy, but when you polish a bit out of tolerance, it probably isn't worth it. This problem was the worst with my HSK63e with an ER40 collet. Tribos and Iso30 didn't slip.

Depending on the size/curvature of your part and the diameter of your cap nut, you might be able to get away with a shorter bit. With a bit that long and with such slow rpm you will most likely encounter severe deflection at your described feed-rates. At any rate you should save that bit for the last of the operations that cannot be accomplished without a 5" bit.