Technical Articles:

The Ins and Outs of High-Speed Machining
An Interview with Ron Field, Millstar

Competitive Mold Maker caught up with Ron Field (now with Millstar) recently to discuss high-speed machining. Field was Makino's head milling applications engineer and spends most of his time helping die and mold manufacturers implement high-speed machining applications. From this hands-on experience, Field provides us with answers to commonly asked questions about high-speed machining.

Speeds and Feeds: How do high-speed machining speeds and feed differ from conventional CNC machining?
"There is a big difference," says Field. "Conventional machining using carbide cutters normally will not exceed 600 surface feet per minute (sfm). Feedrates reach up to 40 inches per minute (ipm) and require high levels of coolant to keep the cutter and workpiece cool, so the tool wear is kept to a minimum. High-speed machining, however, starts at 1,000 sfm and can go up to more than 3,000 sfm with feedrates of 80 to 100 ipm. Using coolant, or compressed air, feedrates can go as high as 1,000 ipm or more."

High Speeds: Does machining at such high speeds warp the workpiece and impact the machining center?
According to Field, head dissipation is not a problem in high-speed machining if performed correctly. If the machining speed is causing inferior surface finish or impacting the machining center, the application is not within high-speed tolerances. "From my own experience and collaboration with several applications engineers at Makino," says Field. "I have a working theory that there are ranges of speeds and feeds--a sweet spot--in which you can operate a machining center for best results. Makino is researching how to optimize cutting conditions to push the speeds and feeds even further, while achieving optimal surface finishes and shorter than ever cycle times. With the proper configurations, we hope to take our latest machines into even higher ranges."

Depth of Cut: What depth of cuts are used in high-speed machining?
Field recommends using a shallow depth of cut with a high width of cut during high-speed roughing applications (Figure 1). Shallower cuts promote longer tool life and higher accuracy with near net shape results. "In many cases you eliminate semi-finish, which also impacts cycle time," says Field.

Hardness: When performing high-speed machining for cavity and core pieces, what is the allowable hardness of the workpiece?
Depending on the machine's rigidity and the spindle technology being used, Field quotes hardness of up to 70 HRc being machined with the proper machining techniques. The most common hardness being used in high-speed applications seems to be around 50 HRc. In fact, most of the high-speed machining techniques were developed for this hardness.

A common industry misconception is that machining hardened metal is difficult to do at high speeds. High-speed machining, with the proper programming actually facilitates the machining of hardened metals. "In some test cut applications, I've cut H13 50 HRc just as easily, and as accurately as softer metals," says Field. "The harder the metal the more brittle it becomes and it can be more easily chipped off than softer, gummier metals. And since material is chipped off more quickly in high-speed applications, more heat is released into the chip."

Cutters: What kind of cutters are necessary to machine hardened metals and non-heat treated metals?
For tools ranging from 1.5" to .5" diameter, carbide insert tools are usually the tool of choice. Several tooling manufacturers offer a variety of coatings and geometries. TiCN coatings are sufficient for material less than 42 HRc, while ALTiN coatings are used for material 42 HRc and over. For tools with a diameter .5" and under, tooling with an 8 to 12 percent cobalt content submicrograin is best suited. And while cutters for high-speed machining will normally not exceed 1.5" in diameter, face milling in high-speed applications uses tooling with diameters up to 3".

"When purchasing solid carbide tools," says Field, "the higher quality tools will definitely pay for themselves with longer tool life and better application results." Field also recommends testing tooling within each specific application to determine the best speeds and feeds for each tool. "Use your tooling to your machine's specifications, not the tooling supplier's specifications." says Field. "Tooling manufacturers cannot test their products on every machining center on the market--it is just not feasible. Machine tool manufacturers purchase a wide variety of tooling and know to what levels they can be taken. Your machine tool manufacturer can help you in this regard while working on the application. Regardless, never exceed the maximum rpm rating for insert cutters or toolholders."

Toolholders: What kind of toolholders suit high-speed machining best, and do balanced toolholders really make a difference?
When machining at high rpm, toolholder balance is critical. Balanced toolholders and the runout of the tool/toolholder combination must be examined carefully for high-speed machining. "The balance of the toolholder should be less than the G2.5 specification and, depending on the rpm being used, this might need to be checked by asking the manufacturer," says Field. "It is possible to buy a 15,000 rpm toolholder that is not balanced or within the G2.5 specification. The rpm ratings do not necessarily provide enough information about the spindle--ask your tooling supplier. Surface finish and spindle damage can occur if it's not within the above specifications. Runout should be no more than .0002". Less runout translates into longer tool life. Probably the best holder for high-speed machining is shrink-fit, as it has more than acceptable gripping force and perfect runout characteristics. Plus, by having no moving parts, it is very easy to balance. The second-best toolholders, in my opinion, are probably hydraulic chucks."

Coolant: Is high-pressure, through-spindle coolant necessary for high-speed machining?
While this has been the predominant approach, other methods of heat dissipation have evolved. Makino's patented Flush Fine machining process can now be implemented using nozzle air, or through-spindle air. The Flush Fine process is a high-speed, high-definition and low-heat machining process that combines high spindle speeds with precisely controlled, high-pressure coolant or forced air to blast away chips and prevent heat buildup, either in the workpiece or the tool. This permits high speed machining with greater thermal stability and chip control, resulting in a superior accuracy and finish, as well as high metal removal rate and longer tool life. This also results in minimal workpiece movement during and after machining, which is traditionally caused by machining stresses and heat.

CAD/CAM: How does high-speed machining impact CAD/CAM?
This CAM system must have toolpaths set within specific tolerances for optimum results, including the step over and pick feed. The CAM tolerance is the amount of deviation that is allowable from the actual surface of the model. The tolerance for finishing should be set at no more than .0001" for the optimum finish. The step over or pick feed is the value used to establish the cusp height. The cusp should be set to .00005" or less for optimum finish. Editor's note: more information on the relationship between CAD/CAM and high-speed machining can be found in Competitive Mold Maker's 3.2's CAD/CAM FAQ, or you can visit www.moldmakermag.com and read it online.

Look Ahead: How much block look ahead is necessary to conduct high-speed machining?
Field notes that a common misconception about look ahead is that a thousand block look ahead is necessary to conduct high-speed machining. "This is an incorrect assumption," says Field. "If the machining center is designed well, it will not need to rely on this large of a look ahead capability. The machining center relies more on the data transfer time, which ensures there is no data starvation."

Look ahead tracks surface geometry, allowing the machining center to accelerate and decelerate most efficiently through tooling compensation. "Makino's Super Geometric Intelligence (GI) software greatly simplifies programming," says Field. "Especially for corners, curves and other part geometry changes, Super GI helps prevent overshoot. Basically, you program for chip load, then enter the highest speeds and feeds that will give you the desired chip load. In machining operations, Super GI takes over and adjusts feeds on the fly to maintain that chip load, enabling the machining center to hold high speeds longer before a toolpath change, minimize slowing while maintaining programmed toolpath/axis changes and resume high speeds faster."

Machining Center Design: Can any machining center perform high-speed machining?
The machining center is the most important factor in successful high-speed machining. "Older CNC machines simply cannot support the speeds and feeds we are describing," says Field. "A machining center must have been designed with high-speed applications in mind to provide quality results. For example, the machining center requires high levels of rigidity. The spindle must also be rigid with very low vibration characteristics. The machining center's servos and control must be advanced enough to support look ahead and quick response times and a high data transfer rate is necessary to handle larger sized programs. I've seen shops attempt to use conventional CNCs for high-speed applications and the results are not what they expect. These machines cannot support the physics of high-speed machining."

Source: Competitive Mold Maker, Volume 4, Number 1

Back to Top