▪Favor a tool with shorter flutes (and therefore a larger and more rigid central core).
FINE GRAIN CARBIDE
Most applications call for carbide tooling and the grade should be chosen not just for its hardness (resistance to wear), but also for its toughness (resistance to shocks). High-speed machining is often high-shock machining; impact, vibration, and temperature changes are more dramatic at higher speeds. A tool with higher toughness is less likely to chip or crack as a result of these shocks.
A good compromise between hardness and toughness comes from carbides with small grain sizes. Many fine-grain carbides available today deliver improved toughness, with little change in hardness compared to coarser grades, Fig. 2-1-21.
TiAIN and TiCN Coatings
TiAIN is an effective coating for a wide variety of HSM applications. The coating delivers a variety of benefits to extend tool life, including:
▪High-temperature wear resistance – High-speed machining is often high-temperature machining. The cutting tool must be chosen not just for its wear resistance, but also for its ability to retain this wear resistance at higher temperatures. TiAIN protects the tool by acting as a thermal barrier. The coating is about 35% more heat resistant than titanium nitride (TiN).
Fig. 2-1-20 Use short cutting tools to reduce vibration at the tool tip. (Modern Machine Shop)
Fig. 2-1-21 Fine carbide grades provide a balance between hardness and toughness. (Guhring)
▪Lubricity layer for chip removal - High-temperature cutting with TiAIN encourages the formation of a useful outer layer of aluminum oxide. This layer is both hard and slick. While the hardness helps with wear resistance, the slickness lubricates the hot chip to help it slide away without adhesion or heat transfer.
▪Abrasion resistance - TiAIN’s abrasion resistance makes it effective for machining graphite.
Because the coating performs effectively at high temperatures, tools with TiAIN are generally run dry, Fig. 2-1-22A. TiCN (Titanium carbon nitride) is a less expensive coating suitable where hardness and speed are not at the highest levels, Fig. 2-1-22B. For a ball-nose tool, TiCN may be appropriate when workpiece hardness is less than 42 Rc and cutting speed is less than 800 sf/min. At these conditions, use of coolant is acceptable.
USE OF COOLANT
High-speed machining often means dry machining. The mechanics of the high-speed cut can convey some heat away. As for the rest, a consistent high temperature may be better for the tool than the widely varying temperature that coolant can bring about.
Coolant does have a role. Use it where lubrication is necessary to protect either the surface finish or the tool, Fig. 2-1-23.
MATERIALS
As newer materials are developed, manufacturers look for methods of machining them faster. It is always wise to follow the material and cutting manufacturer’s recommendation when cutting new materials or using new cutting tools. The following are general guidelines for a few materials:
▪Aluminum – Machine speed should be at least 10,000 sf/min. with a chip thickness of not less than .001 in. to prevent built up edge from forming on the tool that results in premature tool failure.
Fig. 2-1-22 Coatings provide abrasion resistance and lubricity to carbide tools. (Balzers Tool Coating, Inc.) (A) TiAIN coating (B) TiCN coating
▪Compacted graphite iron – Harder than previous cast irons, is more difficult to machine and requires a sturdy machine to support the greater cutting forces.
▪Cast irons – Machine aggressively at speeds up to 3,500 sf/min. with silicon nitride, CBN, or diamond tools.
▪Composites – Use negative cutting tools so that most of the forces applied go into the tool and not the material.
▪High-temperature alloys – Use a coated carbide or CBN tool that cuts well at 500 r/min. as well as 15,000 r/min. to avoid using two machines. Cutting these alloys requires higher horsepower and better tooling.
DRY MACHINING
A steady high temperature at the cutting edge can be better than temperature that fluctuates because of coolant. Coated carbide tools can stand up to the heat, but intermittent cooling can cause carbide to crack. Also, TiAIN coating may perform better when hot, that’s why HSM processes are often run dry.
HSM may even create its own heat-management effect. Fast cutting at a light depth encourages heat to leave the work zone with the chip instead of building up in the part, Fig. 2-1-24. One result is that chips may be harder than the parent material. Therefore, protect the tool during dry machining by using forced air to blow these hard chips away.
USE COOLANT FOR LUBRICATION
The cooling effect of coolant may not be well suited to HSM, but the lubrication effect may be valuable. Use coolant for gummy materials such as aluminum or soft stainless steel to help the chip slide along the flute without adhering. In these materials in particular, consider coolant when taking cuts near the tip of a ball-nose tool where sf/min. approaches zero. When the cut is very light, hot material can be welded to this region of the tool, affecting finish quality. Coolant helps minimize this effect.
Fig. 2-1-23 Coolant can be used to lubricate the tool and protect the surface finish. (Modern Machine Shop)
Fig. 2-1-24 A model showing that most of the heat is carried away with the chip. (Third Wave Systems)
SPEED, FEED RATE, AND DEPTH OF CUT
Tool life and tool performance in HSM are determined largely by how much load there is on the tool. Because speed increases the effect of small differences resulting from factors such as toolholding, tool path and control, this will vary from process to process. How fast each process can be machined may require that the starting point should be at the lower range and increased until ideal machining conditions are reached.
The following are general guidelines when using HSM with a ball-nose tool for finishing operations:
▪Speed - At or near maximum spindle r/min.
▪Feed rate – Use light cuts at chip load equivalent to that of lower speeds.
▪Depth of cut - No more than 10% of cutter diameter, even less for harder materials.
Note: It is important not to exceed a tool’s maximum safe speed. Always follow safety precautions appropriate to higher speeds.
SAFETY AT HIGH SPINDLE SPEEDS
Centrifugal force at high spindle speeds can turn any loose insert, screw, or tool fragment into a dangerous projectile, Fig. 2-1-25. Use the following precautions when machining at high spindle speeds:
▪Do not exceed a tool’s maximum spindle speed rating.
▪Check tools and toolholder