Milling is one of the most flexible machining methods. It can create almost any shape possible, producing flat or angled surfaces, slots, edges, profiles, pockets, cavities and even threads. With the right machine, say a five-axis mill, the sky is the limit on what shapes can be made. The downside of this great flexibility is there are many more variables built into the process, making it a challenge to optimize a milling process.
Fortunately, Tooling U-SME offers help in understanding how to perfect milling in your operations. A subject matter expert for Tooling U-SME, John Pusatera, senior training specialist for Sandvik Coromant, recently recorded a webinar doing just that, titled “Virtual Metal Cutting Technology: Milling Best Practices.” Here are a few tips from that webinar—tune in to the recorded session for even more.
Among the many elements of machining, such as tool geometry and edge prep, getting the right toolpath is critical in maximizing both metal removal rate and tool life.
To develop an optimum toolpath, it is important to realize that milling is intermittent and cyclic. The individual teeth or inserts of a cutting tool go through three phases: 1) enter a cut, 2) engage the material of the workpiece over an arc, and then 3) exit from the cut. Each phase puts its own stress on the tool, machine, and workpiece. Done right, a good chip is formed that maximizes both metal removal rate and tool life.
What is a good chip? The golden rule in milling is “thick to thin.” The initial cut should be thick as the cutting edge enters the workpiece and then progressively thins out as the tooth exits the cut and ejects its chip. Why? The entry into the cut is the least sensitive of the three cutting zones. The tooth starts in the cut with a compressive load (forces coming down on top of the insert). Carbide copes well with the compressive stresses on the impact of entering the cut with a thicker chip. But when the tooth exits the cut, there is a natural spring into a tensile load depending on chip thickness. A thick chip on exit creates a sudden change in load from compressive to tensile. This can cause damage on a carbide insert and wear the tool edge.
Good toolpath programming can help determine the best chip formation. An example of a bad toolpath is when the cutter is programmed to enter straight into the workpiece; thick exit chips will be produced until the cutter is fully engaged. Tool life will be dramatically reduced, to a point that to achieve acceptable tool life the feed for the entire process tends to be reduced (reducing MRR.)
There are two solutions that help create a good toolpath that optimizes feed rate when the cutter is fully engaged:
Program straight into the cut but with the feed reduced to 50 percent until the cutter is fully engaged, then increase the feed rate to 100 percent.
Roll into the cut in a clockwise motion at 100 percent feed rate. (Note: counter-clockwise will not solve the thick chip problem.)
Sandvik Coromant has shown that a rolling entry into the cut in Inconel 718 with a 46 HRC extends tool life up to seven times longer, without reducing MRR. Sandvik Coromant has had comparable results with 316 and 300 stainless steels. That is important enough to use a roll-into-cut toolpath program. This notion of rolling can be extended into longer toolpaths as well. Sharp changes of direction in a cut will generate thick chips upon exit. Adding a roll to a corner is not a major program change and is worth the effort.
Conventional milling (or up milling), turning the cutting teeth into the workpiece, is not the ideal toolpath. It both violates the “thick-to-thin” rule and tends to burnish and work harden the workpiece. Climb milling (or down milling), with the feed direction opposite cutter rotation, avoids burnishing, work hardening, and produces less heat. Most importantly, it is easier to follow the “thick-to-thin” rule, so the first choice is to use down (climb) milling for the best cutting conditions. However, there are exceptions with weaker setups and different component shapes or thin walls.
Another key element is the position of the cutter; off-center to the left is the best way to achieve a thicker chip at entry and a thin chip at exit. A more constant and favorable direction of the cutting forces is achieved, minimizing vibration tendencies. If the cutter is positioned symmetrically on the center line, thick chips will be generated upon exit, and there is a higher risk for vibration tendencies. The cutter diameter, DC, should be 20–50 percent larger than the width of cut, ae. Available spindle power must also be considered, as it influences the choice of pitch.
It is important that machining professionals communicate both precisely and with ease. The accompanying diagram shows some of the most common terms involving cutting tools.
Spindle speed (n) is measured in rpms and is the number of revolutions the milling tool on the spindle makes per minute.
Cutting speed (Vc) in m/min (ft/min) indicates the surface speed at which the cutting edge machines the workpiece.
Cutter diameter (DC) is the specified diameter of the tool when speaking of a shoulder type mill. When the tool has something other then a 0º (90º) entering (lead) angle, the cutter then would have a maximum cutting diameter (DCX) as well and then, depending on the depth of cut (DCap), which is the basis for the cutting speed Vc, this would be called the effective cutting speed (Ve).
For more information on Tooling U-SME and access to this webinar in particular, visit www.toolingu.com or www.toolingu.com/resources/Watch-and-Listen
Connect With Us
