Feed rates, router speed, router bits

[Bill Watt@PM]

We are using Mastercam to create geometry and toolpaths which we are then manufacturing in hard and soft woods with our CNC router.We typically use feed rates of 20-40 f/min, router speeds of 19-21,000 RPM and are using two flute up spiral solid carbide end mills. The bits seem to dull very quickly. I'm wondering what other people are doing to compare methods and experience. Sincerely, Bill Watt

[Michael Reynolds]

If your cutters are dulling too quickly, I'd say you need to be feeding faster or slowing down your spindle. I'm not a router guy, but it makes sense to me.

 

Mike R.

[Glenn Bouman]

quote:

---

typically use feed rates of 20-40 f/min

---

If that is feet per minute you are ok. If it is inches per minute you are 12X too slow.

 

Make sure your endmills are meant for wood and not steel. Steel-cutting endmills will not have enough clearance.

[sir Camalot]

A good source for helpful information can be found in the first couple of pages of C. R. Onsrud’s brochure; Production Routing Tools for Wood. This is a great place to start . This shows federates, formulas and wood types. You will have to modify for your machine and tools though.

Secondly, we will use a rougher and follow up with a profile cutter. This saves tool life of the more costly profile tools and allows faster feed rates, which reduces heat, (which kills the edge). Some tools that work well are 3 flutes with chip breakers (C. R. Onsrud) and Novitec (Guhdo). These tools can run exceptionally faster and work well in all woods. The 3 flute also reduces vibration as compared to the 2 flute. (This could cause premature dulling.) With the Novitec cutter I can run 325 IPM in 1” –1.5” thick red oak all end grain at 18,000 rpm all day without a cutter change. “It’s like cutting butter, baby!” I have noticed that a 2 flute with a finish similar to Onsrud # 52-200, I would change tools about 3-4 times in a day. HTH.

[Guest CNC Apps Guy 1]

Sir Camalot - Cool Name!!!

[Charles Davis]

Michael and Glenn are right.

 

In hardwood, using a .500 carbide, 4 flute end mill, I had the best results taking relatively light cuts (say .25 deep), a feedrate of 350-400 IPM, and an RPM between 18000-20000.

 

We tried all sorts of things (like 18K, .500 deep and 15->300 IPM), but found the light cuts and kicking up the feedrate yielded the best results and least tool wear.

[Mark Lovelace]

Okay, I'm not sure how I ended up on the Instructor Forum, but I would like to add to Charles' comments. I worked with hard woods on a CNC router for 6 years, making musical instruments, and would typically run carbide cutters with a minimal rake. Our machine typically ran at 12,000 rpm, and with a theoretical 500" bit, I would take passes up to .750" deep, .300" stepover, and feed at 80-100 inches per minute for pocketing. When cutting 3D surfaces with a small stepover, I would go as fast as the machine could handle without banging the ballscrews. Slowing down will really burn up cutters, especially in, say, maple or rosewood.