What’s all the fuss about High Feed and High Speed Milling? Part 1 of 2
It's all about the "Chip"! Part 1
High Feed Milling
Those of you that have followed my blog for any amount of time understand I don’t give a hoot about the parts you make; all I care about are chips. At the end of a machining process you have two things, a finished part, and a pile of chips. Most people focus on the part, that’s why I focus on the chips. It’s not about being contrary. I believe if you produce a lot of really good chips, really fast, you can make a lot of money machining parts. That is why I picked what is all the fuss about High Speed and High Feed milling While they are very different in many respects they have some similarities. In this two-part blog series, I will attempt to explain both. As the title states; it’s all about chip. I digress, so let’s get started.
What two things does it take to make a chip? Metal cutting is a process of plastic deformation. This act of plastic deformation requires “heat and pressure.” The heat is created by the friction at the shear zone. The amount of heat is regulated by the rotational speed of the cutter in a milling. The pressure is generated by the feed. It is important to note the same “heat and pressure” that is required to plastically deform the material and shear it away is the same heat and pressure that causes tool wear and failure. Where do we want the heat to go; into the chip, but first you must have a thick enough chip to absorb the heat. That is where the high feed rates come from in High Feed milling.
So, what’s chip thickness got to do with “High Feed” milling? Everything. All High Feed milling cutters; solid and indexable alike have one very important thing in common; very large lead angles. The cutting edge on High Feed cutters can be straight or have a very large radius, either way the resulting average lead angle is very high. Usually somewhere between 78° and 82°. What impact does a high lead angle have on the chip? As the lead angle on a milling cutter increases from 0° or square shoulder to 45° or 75°, things start to happen to the chip. At 0° (square shoulder) your chip thickness is equal to your feed per tooth. As the lead angle increases your chip thickness decreases. You can calculate your actual chip thickness by multiplying your feed rate IPT by the cosine of the lead angle. So, a .010” IPT feed rate, using a 78° lead angle would result in a .002 actual chip thickness. That’s thin, and not nearly thick enough to absorb any heat. Remember, your feed rate must always be greater than your edge preparation hone or T-land or you turn you milling cutter into a piece of sandpaper. To achieve .010” chip thickness using a 78° lead angle tool you will need to program an IPT of .048”. That is a 385% increase in feed rate hence the name High Feed milling.
The extremely high feed rates achieved with high feed milling do come with one drawback. Due to the large lead angles their DOC (depth of cut) capabilities are limited. Most high feed mills maximum DOCs range between one and two millimeters. There are a few indexable exceptions to this rule that incorporate large IC inserts. In most cases the increased cost can be justified; at least, three to four times faster than normal, an extra pass here or there is cost justified and will provide productivity and profitability gains. In addition to the productivity gains there is one other huge benefit to high feed milling. It’s all about the force.
You may recall another one of my golden rules; cutting forces are always perpendicular to the cutting edge. High Feed cutters, with an average lead angle of between 80° and 82.5° generate some of the lowest radial forces in milling. That’s right, almost all the cutting forces are directed axially up into the spindle. The greater the ratio of axial to radial forces you have the more stable the operation. This can work to your advantage, especially when your tooling set-up or part configuration requires a large gauge length. Long reaches and deep cavities are not an issue when high feed milling. Gauge lengths on the magnitude of 10 to 1 length to diameter ratio are common; however, moderation of the feed rate may be required.
There are a few other application techniques to consider when High feed milling. Keep as much of the cutter diameter engaged in the cut as possible. This will balance the axial forces generated by the high lead angle. As your ae (radial width of cut) decreases and approaches 50-60% of the cutter diameter stability is diminished. Care should also be taken when programing your cutter path. At high feed rates, smooth transitions in cutter path direction are preferred. Avoid 90° turns at all cost as they create excessive radial engagement, resulting in high radial forces, and chatter. Program an arc or radius in corners at least 50% larger than the cutter diameter when changing directions. Remember, when transitioning from straight line move to an arc your feed rate must be reduced. In the example provided above you would reduce the feed rate by 33%. The formula used to determine the corner or circular interpolation feed rate compensation is;
((2 x arc radius) – cutter diameter)) / (2 x radius).
In summary, High Feed milling is all about chip thinning. You must increase your feed rate to compensate for the chip thinning effect created by the large lead angle typically 80° to 82.5°. In most cases your feed rate is four to five times faster than standard feed rates utilizing square shoulder or 45° lead milling cutters. The large lead angle while somewhat limiting the axial DOC (depth of cut) pushes most of the cutting forces axially up in to the spindle increasing stability and allows for long reach capabilities. Just like in car racing; care must be taken when entering corners and changing cutter path directions. Use feed the rate compensation calculation to reduce your feed rate and use smooth arcs or radius tool paths when changing directions to prevent excessive cutter engagement and chatter. When applied correctly High Feed milling is an extremely productive metal removal process and can be a life saver in deep cavity and long reach applications.
Visit us next week when we will tackle part two of this topic, High Speed milling.