We recently purchased a Pratix nest machine. We use 2 sided melamine particl board and laminated particleboard. What is the best tooling for the CNC and at what feed rate should we expect to run it?
From contributor L:
You're about to get 1000 responses but it really comes down to a couple of factors:
feedrate= # of flutes x rpm x chipload
Chip load - size of chips produced by the feed and speed (rpm). The right size is needed to remove heat while also producing a quality cut. Higher rpms and multiple flutes need higher feed rates to remove the right size chips.
Achievable feed rate - how fast are you going to be able to cut when considering acceleration and deceleration; if you're cutting mostly long straight shapes you'll be able to physically achieve faster feed rates than cutting small or parts with curves. If you're doing a lot of long straight shapes, you can use over two flutes to achieve faster feeds. If not, the extra flutes won't help much.
Depth of cut - how deep you are trying to cut in one pass; usually depends on the thickness of material, but also the diameter of the tool. You can use high up shear compressions or mortise style tips depending on the thickness of material. I prefer mostly mortise tips unless I'm cutting thicker than 3/4 inch material. Larger diameter tools can cut deeper in one pass.
Carbide - there are different grades of quality when it comes to carbide, and in most cases you get what you pay for.
Brands I like include Vortex, Lueco, Onsrud and Amana. Maybe start out with the cheap stuff so you won't feel bad when breaking a bit. Collets, tool holders and the spindle need to be properly maintained to get the best performances out of tools. Onsrud and Vortex have some basic feed and speed charts available online to give you an idea; you'll have to fine tune to your application.
Start out with a double edge (two flute) 3/8 compression running 16000-18000 rpm at 500-600 ipm. Don't plunge with compression bits if you can help it; use a lead in and lead out. For 1/4 diameter bits use 400 ipm.
It takes some experience but eventually you'll get a feel for it. Just remember, loud noises are bad in most cases, and something needs to be adjusted (feed, speed or depth of cut).
On the other hand, HPL has a nasty problem of chipping carbide where the plastic and carbide meet. Look at your worn out tool and see if you notice a tiny nick in the tip. Sometimes when the laminate is on the bottom, a small piece will get stuck to the tip when you cut through. You'll notice scorch marks on your spoilboard when this happens. The only real way to prevent this is to adjust lead in and lead out and number of passes at different depths until you get better results. Try using a rough pass with another tool if possible, so you're trimming the laminate rather than trying to plunge through it.
Sometimes when dealing with HPL board, it's best to just go through a bunch of cheap straight flutes at a lower feed rate, or in your case, keep the feed rate the same. Disposable tooling basically. I can get through about 10-12 sheets of hpl with a diablo 3/8 diameter/ 1 inch cel from using 2-3 passes. Not an ideal solution - people will probably laugh at you, but it works and it's cheap.
Maybe look into insert tooling if that is the primary material you're cutting and you cut a lot of it. These tools have a larger diameter and increased kerf, but you can replace and/or flip the carbide when it wears down.
I can usually get away with using a high quality 2 flute compression, but I'm not cutting more than 15 sheets at a time for most jobs.
Some people swear they can run 60+ sheets with Vortex Xp 3 flutes or similar, so there must be some combination of feed, speed and cut depths that works for them.
I tried one of the budget brand 3 flute compressions and the noises it made scared me enough to put it away until I get desperate enough to try it again.