Improving Relief Cut Quality

Advice on bits, RPMs, and more for getting clean, sharp cuts in complex relief surfaces. March 1, 2006

Id like some feedback on how to improve my cut quality when I run high relief complex 3D parts. I have a home built servo machine that has decent rigidity for the size of my z axis 18" and what I'm cutting - maple art pieces. I'm using a Makita router and 1/8" carbide ball end mills, running a finish pass around 40 to 50 IPM with a .015 to .018 step over. Generally I'm taking off 1/8" of wood on a finish pass. Should I be up cutting or down cutting? Should I be using 2, 3, or 4 flute tools? What RPM should I be running? I have noticed that I get excessive fuzzing on certain aspects of the part and a good finish on others. Why is this? My parts are big so more than one finish pass is not an option.

Forum Responses
(CNC Forum)
From contributor A:
This is a broad subject so I will attempt to help with generalizations. First, there are several things that can influence the inconsistent finish you are experiencing. Even though you are using a ball cutter, since your part is 3D, remember that the cutter is not tangent to the cut at all times. This would require a 4 or 5 axis machine, depending on the application. In essence you are cutting on different aspects of the profile of the cutter depending on where you are cutting at any given moment. Not a huge issue, but something to keep in mind. Generally speaking your feed should be minimized to get a better surface finish. Another consideration for you is the cusp or step over. You can achieve a better finish simply by reducing the step over. Trade offs are typically longer cycle times and accelerated cutting edge wear. Speeds - I am ballparking here, but I would say for that cutter somewhere in the 30K RPM would be on the low end in wood. Feed rate would be a direct product of chip load for the particular cutter you are using. Since your machine is homemade and the length of Z axis travel lead me to believe rigidity could come into play, I would start with a two flute cutter to reduce the tendency to chatter. You can always step up flutes at a later date.

From contributor B:
Use the 2 flute upshear ball end. A downshear type, which we have produced, loads the cutter and will break. Make sure you use a ball end tool designed for the wood industry, not some generic type used for metal. Clearance angles are completely different. This is a possible cause for fuzzing. Your feed speeds are OK, RPM around 18000 is also OK. COURMATT has just provided Shop Bot with similar tools and no fuzzing.

From contributor C:
You have gotten some really good answers here. One thing no one mentioned is the size of your bit. If you can use a large ball nose bit, you get better results. I usually start with a 1" ball and do everything possible with it. Anything I can do with a straight bit (not ball end), I do with a straight bit, and then I go smaller. Programming work is a bit more but the end product is better. Your speeds and RPM seem OK to me too. One other thing, if you have contours that are consistent, like a piece of molding, you can speed up your cut time considerably doing contour - rather than surface - tool paths.