If you have spent any considerable time in a machine shop I am sure you have heard the term “dynamic milling.” There are many other names out there depending on the CAM software you use – Edgecam calls it “Waveform” while Surfcam calls it “TrueMill.” Solidcam calls it “iMachining” while Mastercam calls it “Dynamic Milling.” You get the point. Every CAM package will claim theirs is the best, and while they may approach certain cuts differently, they are all based on a simple principle that in practice will give you amazing results. I have been a machinist and CNC programmer for ten years, and my first experience with dynamic toolpaths had me speechless. Today I hope to open that same door for you.
Dynamic toolpaths are not a new concept by any means. There is a very good reason many machinists have long used light depth (axial) cuts with heavy side (radial) cuts to achieve their machining goals. Any machinist who has been in the industry more than 25 years remembers a day when CNC was the minority. Current CAM software allows for significantly more complex and lengthy programs and precision. When you are turning handles on a Bridgeport maintaining a 10% step or a specific chip load would be impossible with dynamic motion involved. Can you imagine hand writing and punching tape for a 600,000-line G-code program? It’s been done, but it certainly can’t be called efficient. So it’s not for a lack of knowledge, simply a lack of technology that dynamic toolpaths are not standard practice … yet.
Maximize Tool and Spindle Life with Dynamic Toolpaths
Dynamic strategies have a very simple principle – maintain a constant chip load throughout the entire cut utilizing a full depth (axial) cut and very light side (radial) cut. The benefits you will see from this type of cut include longer tool life, longer spindle life, improved surface finish, greater efficiency and awesome rooster tails. No really though, I’m not joking. You are going to have people standing there watching the machine run just because of how the chips are flying.
First and foremost is tool life. I will also throw spindle life in with tool life because they really go hand in hand. You get multiple benefits for both your tool and spindle if you properly apply dynamic strategies. If you are cutting a pocket or any internal feature that doesn’t allow an approach from outside the material, then entry into the cut is not only the first consideration, but one of the more important. I always use a helical entry motion with a 1%-3% helix angle, or entry angle. You want to use an entry diameter that is somewhere between 120% and 150% of your tool diameter – be careful, sometimes the CAM software asks for a radius rather than a diameter and that information makes a huge difference. Once you are at depth the real fun begins. Due to the light radial cut you can really be aggressive with your feed rate. Depending on the limits of the spindle RPM, use the tooling manufacturers specifications on chip load and surface feet per minute (check my blog on shop math). In my first experience with a dynamic toolpath I was running a 3-flute .500” end mill with a 1.5” flute length. The cut was 1.375” deep, with a 10% (.05”) step over with a feed rate of 144 inches per minute. I used a high helix end mill to assist in chip evacuation which created a “rooster tail” of chips trailing the cut. It was a thing of beauty. Even though the cut was so fast and seemingly aggressively deep, the tool lasted through 32 parts and gave the same finish on part 32 that it had given on part 1. The full depth cut means that you are wearing the entire flute length evenly, therefore you are not going to get lines on your finish. The light radial cut reduces the cutting forces, thereby reducing overall wear on both the tool and the spindle.
Efficiency is also a significant benefit. Pretend for a moment that you are cutting a 1.375” deep pocket with features at 4 different depths. Using a standard toolpath and a light depth with a heavy step over you will cut from the top of your part down. Depending on how aggressive you are with your step down you will cut many passes on each depth, with the deepest being the most time consuming. Utilizing a dynamic strategy you will cut from the bottom up, meaning each depth will consist of one pass, with all previous passes having already cleared out other material at that depth. Therefore, at each depth you are only cutting the remaining material, essentially creating a “rest rough” toolpath that minimizes total machining time.
With dynamic toolpath strategies you will not only improve tool life, spindle life and surface finish but also overall cycle time and cost efficiency. Not to mention you will impress the boss and anybody else who happens to walk by. Do me a favor, and give it a shot. You won’t be sorry you did.