3 months by cncdivi

The article is sourced from our cookbook on Speeds and Feeds.

Many beginners are taught to use a 2 flute in aluminum for chip clearance, but must we always use 2 (or perhaps 3 flutes) for Aluminum and never 4? Now that we know why fewer flutes must be used (chip clearance), we can think effectively about when we might not be restricted to fewer flutes. In general, when you have plenty of room for the chips to escape, you can use a 4 flute cutter, and you’ll get a better surface finish.

How much is “plenty” of chip clearance?

Forget slots and plunging. Those are the worst cases. Try to avoid tight inside corners or interpolated holes whose diameter is at all close to the tool’s diameter, those are nearly as tough. But what if we are profiling around the outside of a part and there’s no concave curves, only convex? Tons of chip clearance there, so have at it. If you have a sufficiently roomy pocket, you may also get away with a 4 flute, especially if you can open up a big hole in the middle of the pocket to get started in.

The best case for more flutes is when you have a finishing pass, particularly if you’re already committed to changing tools to get the best possible surface finish from a newer sharper tool that hasn’t been roughing. The finishing pass will be very shallow and the rougher will have opened up plenty of room for chip clearance. Consider using 2 or 3 flutes for roughing followed by 4 flutes for finishing in materials like aluminum. In harder materials that don’t need so much chip clearance, tools with as many as 10 flutes may be used.

This doesn’t just apply to aluminum either. More exotic tools are available with 5, 6, 10 or more flutes. Experienced hands will tell you that if you’re profiling (where there’s lots of chip clearance) steel and aren’t using 5 or 6 flutes, you’re leaving money on the table. Let’s run the numbers in G-Wizard. Suppose we’re profiling some mild steel–1020 or some such. We’re going to profile the outside of a part, so there’s plenty of clearance. Cut depth will be 1/2″, cut width 0.100″, and we’ll use a 1/2″ TiAlN Endmill. Here are the numbers:

– 4 Flute: 3158 rpm, 29.8 IPM. MRR is 1.492 cubic inches/minute. A little over 1 HP.

– 5 Flute: Same rpms, now 37.3 IPM. MRR = 1.865. 1.3 HP. That’s 30% faster cutting.

– 6 Flute: Now 44.8 IPM. MRR = 2.238. 1.6 HP. 60% faster than the 4 flute case.

How much more profitable are your jobs if you could run them 60% faster? The cost to do so is a more expensive endmill and a tool change for profiling. Harder materials can benefit particularly well because they’re already up against surface speed limits. More flutes is the only way to get faster feeds.

Sometimes we have to go the other way too. If you’ve got some really sticky stainless steel that’s giving you fits in tight chip clearances, try a 3 flute instead of a 4.


Like what you read on CNCCookbook?

Join 100,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!

Just enter your name and email address below:

Full Name
Email *
100% Privacy: We will never Spam you!

Rate this post

Recently updated on March 1st, 2024 at 12:12 pm