Better-Machined Mold Finishes in Less Time
This short video shows you the science and math behind achieving the desired milled surfaces with ball end mills. You can consistently attain better machined mold finishes in less time, while also decreasing polishing time.
Reduce Machine Cycle Time
You can reduce machine cycle time and polishing time by calculating the needed step over and chip load per tooth for milling.
When a finer finish is needed, the normal strategy is to decrease the step over, but this may not be the most efficient means of improving the finish.
Ideally, the step over and the chip load per tooth should be matched. This provides a symmetrical surface and optimal productivity.
Watching a ball mill cutting a surface, we just see the blur of the rotating cutter and the fast motion of today’s high speed CNC. Slow it down a lot and we can see individual cutting edges shearing metal away a single chip at a time, while the cutter advances over the material.
Here’s a sample of a flat surface milled in this way, with a matched step over and chip load per tooth. Look at the symmetry, with equal spacing between the surface’s individual lobes. This surface will glisten in the light, reflecting light from virtually all angles.
Here’s a sample of the same flat surface milled differently, with mismatched step over and chip loads. The surface doesn’t look as good, and polishing or finishing it is more complicated because of the grain-like effect, similar to the grain in wood finishes. Finishing with or against the grain will produce different results.
As we mentioned earlier, the benefit of symmetrical finishing is both appearance and productivity.
Companies work hard to achieve high levels of polish, yet maintaining mathematical surface accuracy through polishing can be a challenge. A fine and symmetrical surface finish can minimize polishing to maximize accuracy.
Surface finish is generally defined today as R A, the Roughness Average. This means that the average difference in a surface’s peaks and valleys from mean is within that number of millionths of an inch. A 32 R A finish means that the average of high to low features is 32 millionths of an inch. This can help us select the required cusp height. The cusp height should be equal to or less than the R Max, four times R A.
Your finish milling time can be minimized by matching the step over with your surface finish requirements, and matching the chip load per tooth with your step over. Let’s look at the math for this. To calculate the step over for a cusp height, we only need to know the cutter’s radius and that cusp height. The step over equals the square root of h, the cusp height, times 8, times r, the radius of the tool.
As an example, a 1 millimeter diameter ball end mill will produce a 10 millionths of an inch cusp height by using a 12 ten-thousandths of an inch step over.
The chip load per tooth should be equal to the step over already calculated. Milling with a two flute ball mill at 30,000 RPM and a 12 ten-thousandths of an inch chip load per tooth, our feed rate should be 72 inches per minute.
Stay Within the Limitations of the Cutter
It’s important to stay within your cutter's limitations for optimum cutter life. Recommended speeds and feeds for each specific cutter are usually listed in the manufacturer’s catalog or website.
The benefit of matching step over and chip load per tooth was vividly demonstrated while preparing a machining demonstration. We weren’t pleased with the sample part’s finish. The programmer suggested cutting the step over in half. That would double our cycle time.
Doing the math, we found we could actually increase our step over and decrease the chip load per tooth, reducing cycle time. Within the cutter's limits, we increased the rpm and kept nearly the same feed rate. The net result was a better looking part in less time.
It’s important to maximize productivity while machining the required surface finish. For your finishing passes, calculate the step over to achieve your required finish, and then match the chip load per tooth and calculate the feed rate. Your parts will look better, require less polishing, and take less time to manufacture.