thumbnail group

Connect With Us:

Manufacturing Engineering Media eNewsletters

ME Channels / Machines & Automation
Share this

High-Speed Milling of Hard Metals

 

It can be done, but there's more involved than buying a new spindle

 

By Craig McQueen
Application Team Leader
Makino Inc.
Mason, OH
Craig.McQueen@makino.com

  

Until recently, metals above RC45 were considered too hard to machine at high speed, so the soft-steel part would be roughed and semifinished, and when it came back from hardening the details would be finished off by a capable machine tool or by hand. These operations ran at slow speeds to keep the machine from crashing, and to avoid breaking the tool.

To machine hardened steels at high speed, you must have a machine tool, control, and tooling that are up to the task. Also, you must be able to write a program that gives appropriate consideration to the stresses a tool undergoes at high speeds when milling hardened material. And finally, you must rethink how your people are trained, because a different mindset is required to successfully machine hardened steels at high speed.

Given the requirements inherent to high-speed machining (HSM) of hard materials, and the challenges summarized above, why is this process worth pursuing?

Quite simply, once mastered, it's a great way to improve productivity. On average, we've been able to reduce cycle times from traditional hard-milling processes by half to two-thirds, and improve surface finishes to the point that no hand polishing or bench time is required. In fact, we're consistently seeing surface finishes of 7 µm Ra in highspeed, hard-milling applications of steels hardened to RC60. We are successfully removing hardened metal at 1000 fpm (305 m/min) for steels hardened to RC45, as much as 600 fpm (183 m/min) for steels to RC45–58, and as high as 400 fpm (122 m/min) for RC 60+ material.

Testing continues, and we're finding that we can push our spindles faster everyday, removing even more hardened metal at higher speeds.

So what's involved in successful high-speed hard milling? As a first requirement, it's pretty obvious that the spindles had to speed up for HSM—from 20,000 rpm on average to around 40,000 rpm—to permit faster feeds without increasing cutting force. The speed isn't the most important thing to note, however, because higher speeds don't necessarily mean shorter cycle times. If you can't hold the same accuracies in HSM as in conventional machining, and have a reliable system, you'll just spend more time fixing problems. When you bump up the spindle speed, you must be confident of your machine's stability and be certain that other aspects of system performance, such as processing, control, communication, servomotors, bearings, chip management, and tool rigidity can handle the process.

To handle a spindle operating at high speed, CNC processing speed has had to improve. Today's high-speed processors are significantly faster than those used years ago, and the control software is more advanced. Our company's latest control software package, for example, which is designated SGI.4, has been optimized specifically for HSM. In addition, modern bus architecture and connection speeds have enabled controllers to communicate with the spindle much more efficiently and reliably.

Functional parts, such as the servomotors and bearings, must be able to handle HSM. The servomotors must be designed to get maximum torque without overloading the motors, to increase acceleration of the axes, while maintaining smooth motion that preserves mechanical components. Many of the new digital servosystems provide 16 million pulses/ballscrew revolution to assist in this task. Right now, the best bearings for HSM are hybrid steel race ceramic balls, which permit less torque at higher speed with finer finishes, and are electrically inert.

Don't forget to consider the chip management system. It's important when doing HSM that chips are evacuated from the workspace quickly and efficiently, given the increased metal removal rate.

When you're cutting into materials that are over RC45, the process generates vibration and heat. Both can lead to inaccuracies, chatter, tooling failures, growth and other problems.

The first step to take in dealing with vibration and heat is to employ a stable machine tool and toolholder. Stable machine tools have rigid, heavy castings. Cast-iron construction is especially important to limit deflection and provide thermal stability. More massive machine tools will fight the forces you're applying to hardened material. Not that you should buy a machine tool based solely on its weight, but mass is something to be kept in mind if you'll be hard milling.

Another important feature is thermal control. As a part is machined over long periods of time, the machine experiences thermally driven changes caused by ambient temperatures. A stable machine will not permit those temperatures to negatively influence part-cutting.

Many molds are machined for days, especially large molds, and thermal control becomes important to maintain polish-free surface finishes and tool-to-tool blending. A well-cooled spindle that provides repeatable, predictable thermal growth helps maintain these characteristics.

Spindle core cooling is a process patented by our company that can reduce spindle growth in high-speed spindles. Core cooling limits the amount of thermally driven growth, and enables the spindle to stabilize very quickly. Cooling oil temperature is accurately controlled, and the same oil is pumped into the center of the spindle. So the oil that lubricates the spindle also cools it.

As for the toolholder, you need to decide what kind of holder fits your application best. A mill chuck, for instance, is great for roughing in hardened steels. It provides excellent vibration damping, good runout, and rigidity. Mill chucks aren't very accurate, though, so a collet chuck might be a better option.

The biggest thing to consider when picking a toolholder is how much damping you need. The toolholder system should not allow energy to transfer into the spindle interface, the critical contact point between the tool and the spindle. Minimizing the damage that roughing will do by absorbing energy with a toolholder damping system will extend tool life, and improve bearing life and runout. Runout for roughing tools will typically range from 0.005 to 0.0001" (0.127–0.003 mm) while finishing tools held in shrink-fit holders can achieve runout of about 0.002 to 0.00004" (0.05–0.001 mm).

A well-made collet chuck will absorb vibration, has good runout, accepts many tool sizes, and can be used for the finish work needed in most applications. If you need to get really accurate, a shrink-fit holder becomes your best option. In most roughing applications, however, it won't absorb the vibration created during high-speed roughing of hard materials. Basically, shrink-fit holders should be used for semi-finish and finish routines.

No matter what toolholder you use, when you're running high speeds in hardened steels it becomes especially important to balance them. We balance all holders to g2.5 at maximum system cutting rpm.

You need to use a tool that is specifically designed for cutting hardened steels. Don't assume normal tooling will work. Several manufacturers offer tools that are rated to cut 50 RC, even RC 60, materials. Be sure to do some tests with your tool, machine tool and toolholder to make sure all the ingredients add up.

Make sure your programming software allows the use of many techniques that can be valuable when tackling hardened steels at high speeds. Trochidal roughing, effective lead-in and lead-out control, arc-fitting corners, high-tolerance toolpaths, and gouge-checking can influence your ability to hard mill. If the program on the CNC won't allow control of these factors or permit employment of these techniques, look for new software. Usually, software capable of handling these techniques is designed specifically for hard milling.

Another important programming factor involves understanding how to handle stepovers and stepdowns relative to material hardness. This often-overlooked point can make a big difference in how well you can hard mill. Table 1 shows our company's basic guidelines. We suggest that chip load be kept at about 1% of cutting-tool diam. And when cutting hardened materials at high speeds, we recommend leaving 5% of the semifinish cutting tool diameter as plus stock (the amount of material left after the roughing routine).

During the roughing operation, you'll need to determine the effective diameter of the cutting tool to engage to maximize feed rate and decrease cycle times according to the appropriate formula.

Basically, be sure that your program and programming ability can handle high speeds in hardened steels. Without the proper techniques, you'll burn up tools and scrap parts left and right. If you've never programmed for high speed machining before and/or for hardened steels, odds are you won't be able to do both without some training.

Hard milling at high speed is very different from hard milling at slow speeds, and is very different than high-speed soft milling. The same principles don't necessarily apply, and the margin of error is much slimmer. Given these facts, we believe it's essential that shops who take on high-speed hard milling have a staff prepared to handle this change.

A good example of the difference between soft milling and hard milling at high speeds is the tendency to think that it's OK to leave mistakes to be machined, benched, or polished later. If your goal is to reduce cycle time by skipping the soft-roughing step, there's no room for benching after the piece is machined. Instead, each step of the manufacturing process must be scrutinized, and the part must be examined and approved for the next step. This "error-free" process must be instituted at every step, from receiving the blank to the final examination of the part. If a bad part is left unchecked or passed onto the next step, the whole process collapses, lead times increase, and you might as well go back to the old way of doing things.

Machinists and machine operators must be trained on how hard to push the machines and tooling. It's easy, once you see progress in high-speed hard milling, to push the process until something breaks. But crashing a machine tool, ruining a spindle, or destroying specialty tooling can become expensive and time-consuming. Make sure your people are trained on the capabilities of the equipment and tooling used for high-speed hard milling, not just in general.

 

 Training is not only important to protect your capital equipment and keep your scrap rate low, but also so the rest of the organization can prepare for how the part flow might change. Many companies who implement HSM realize that bottlenecks quickly form. When an operation is used to running at a certain pace, it can be overwhelmed when a particular component is sped up. This becomes especially important when you begin high-speed hard milling, because times decrease a great deal, often more than 50%.

We recommend sending your machinists to a class that teaches the art of high-speed hard milling, and even bringing in a high-speed hardmilling applications engineer to talk about how things might change.

 

This article was first published in the January 2007 edition of Manufacturing Engineering magazine. 


Published Date : 1/1/2007

Manufacturing Engineering Media - SME
U.S. Office  |  One SME Drive, Dearborn, MI 48128  |  Customer Care: 800.733.4763  |  313.425.3000
Canadian Office  |  7100 Woodbine Avenue, Suite 312, Markham, ON, L3R 5J2  888.322.7333
Tooling U  |   3615 Superior Avenue East, Building 44, 6th Floor, Cleveland, OH 44114  |  866.706.8665