Get more from your milling cutter

Get more from your milling cutter

Fowler, David

The right cutter, insert, and cutting conditions can boost tool life 30% in this highly aggressive cutting process

Are you having surface finish problems in a finish milling application? Examine the tool’s depth of cut (DOC). Many engineers still believe finish passes should remove 0.005-0.010″ (0.13-0.25 mm). A better choice in most work materials is a DOC of 0.015-0.025″ (0.38-0.64 mm). When the carbide inserts do not have enough materials to bite into, the tool will rub against the work surface instead of cutting, reducing tool life and surface finish quality.

You may also be milling a hard material without realizing it. In turning, you can classify any work material above R^sub c^45 as hard. In milling, you should consider any work material of R^sub c^32 and above as hard. Improving tool life and surface finish may require a change in cutter geometry, insert grade, insert entry angle, and operating conditions.

Unlike the single-point turning tool, a milling cutter enters and exits the cut many times. The dual motion of the rotating cutter and the feeding worktable generates varying chip thicknesses and cutting forces. Pressure exerted on each insert can be as high as 100,000 psi (699,500 kPa) when it first enters the work material. Extreme thermal cycling during cutting also has an effect: An insert’s edge temperature can reach as high as 2000degF (1093degC) in materials like titanium, dropping off as it disengages from the cut.

Extreme though milling may be, cutters fail most often because the operator didn’t calculate the magnitude of shock or force acting on the cutter in that application and specify cutter position, operating conditions, and geometry accordingly.

Geometry Lessons

Milling cutters come in three basic geometries, positive radial rake and positive axial rake, negative radial rake and negative axial rake, and positive axial rake and negative radial rake. The insert’s orientation in the direction parallel to the cutter axis is the axial rake angle. The insert’s orientation in the direction of the cutter radius is the radial rake angle.

Negative-negative cutters compress or push the work material, producing tremendous forces in the part and the machine, which may preclude their use on older machines with worn bearings or in applications cutting thin-section parts. Their benefit is that they have twice as many cutting edges as positive-positive or positive-negative cutters. They also are extremely strong, providing long insert life on tough applications, such as cast iron with scale. In applications producing problematic chips, though, the cutter will require gullets to help with chip ejection.

On the down side, they consume a lot of power and, in many applications, do not produce as good a surface finish as positive-rake cutters. In general, you should not use negativenegative cutters on workhardening materials, including most stainless steels, alloy steels, high-temperature alloys, or soft gummy materials like aluminum. Negative-negative cutter chips can curl back toward the machined surface, marring the surface finish or breaking the insert. Because chips are not ejected cleanly, they do not work well in slotting operations.

Inserts in positive-positive cutters shear the work material in both the axial and radial directions. Tools are extremely freecutting, with good chip ejection. They consume less power than negativenegative cutters and can provide improved surface finish. Unlike negative-negative cutters, they usually will direct chips up and out the flutes. These tools work well in tough materials, including high-temperature alloys and stainless steels, as well as soft, gummy materials like aluminum. Their low cutting forces also reduce vibration when milling long, thin parts or fragile workpieces.

Disadvantages of positive-positive cutters are that inserts provide only half the cutting edges of negative-negative tools; the most vulnerable edge of the insert enters the workpiece; and the direction of forces tends to lift the workpiece away from the table.

Positive-negative cutters eject chips in spirals up and out of the flutes, providing the best chip flow of the three cutter geometries. They work in a wide range of work materials, including soft ductile metals, effectively balancing cutting forces on the part and machine spindle. Power consumption is low, and surface finish is good. Still, inserts only provide half the cutting edges of negative-negative tools.

Downsizing Is Not Always Rightsizing

Standardizing on a few cutter diameters may cut your initial tool costs, but this practice isn’t always wise for milling applications, where cutter diameter should be closely matched to the part geometry to be milled. Proper cutter diameter selection is important because of the effect of diameter on cutter positioning. Cutter positioning, in turn, influences factors like tool life and resistance to insert breakage. For example, you should avoid cutting with the entire tool diameter because the balanced side forces will slow the cutter and cause machines with loose spindle bearings to vibrate. You also should avoid cutting with the cutter centerline aligned on the centerline of the part.

Also examine the insert entry angle. When the tool first enters the cut, the insert entry angle should be 45-85deg. This will allow initial impact between insert and workpiece to be on the insert face, a stronger section than the cutting edge.

To achieve a negative entry angle and adequate chip thickness at tool entry and exit, position the cutter so engagement is at least three-quarters of diameter. Cutter overhang on the exit side should be 5% of cutter diameter for most materials, 10% for stainless steels. The tool will engage the work along a shorter arc, there will be less rubbing because the chip is thicker at insert entry, and there will be less power consumption because fewer inserts are in the cut. You may need to make more passes to mill the part, but if you increase the table feed, you can make those passes in roughly the same time as before and increase tool life 30% or more.

Avoid Shaky Cuts

Because milling is an aggressive cutting process, with inserts entering and leaving the cut, it encourages vibration. There is a tendency for operators trained on low-power machine tools to use conventional milling, where the cutter rotation opposes the table feed, and the resultant forces are directed upward, even when using new higher-power machine tools. The method has disadvantages: The chip thickness at insert entry is zero, which promotes rubbing instead of cutting; cutter forces may lift the part out of the fixture; and there may be vibration; and there can be problems with surface finish.

Whenever possible, you should use climb milling, which requires a more powerful, rigid machine, rather than conventional milling. Table feed should be in the same direction of cutter rotation, and the resulting downward forces help keep the part in the fixture even if the fixture is weak. The most significant advantage over conventional milling, though, is the maximum chip thickness at insert entry. There is no rubbing, so tool life will improve.

On no. 40 taper machine tools, you should use a very-short-gagelength rotary adapter for end milling applications. This is in keeping with short overhang, and normal laws of physics will apply.

Although normal milling encourages vibration, it is even more of a problem in two cases:

True interrupted-cut milling of surfaces with holes, slots, or depressions. To reduce vibration and improve surface finish, at least two or three inserts should be cutting metal at all times.

Machining thin or unsupported part sections. Use a machine tool with enough horsepower, a backlash eliminator, and fixturing with end stops and side stops. Select a positive cutter with large lead angles, coarse pitch, and differential pitch. Spacing inserts unequally around the cutter breaks up the harmonics equally spaced inserts create. Varying axial and radial rakes slightly from pocket to pocket may help.

Use Proper Care and Feeding

Even skilled machinists have problems selecting the right feed per tooth, also called chipload. Feed per tooth, equal to the width of the thickest part of the chip, must be large enough for each tooth to engage in the workpiece deeply enough to start cutting. If feed per tooth is too small, the teeth may rub the workpiece, generating heat and workhardening the surface. This, in turn, generates more heat and reduces life of the tool.

During milling, the chip thickness will vary as the insert rotates through the part. As a rule, feed per tooth should be at least 0.004″ (0.10 mm) to avoid rubbing and burnishing the workpiece. On inserts with edge reinforcement like a T-land, feed per tooth must exceed the T-land width.

When the radial depth of cut is less than half the cutter diameter, maintain an average chip thickness of no less than 0.001″ (0.03 mm), with average chip thickness determined by the ratio between cutter diameter and radial depth of cut. To compensate for the difference in chip thickness in this case, use the following formula:

H = F^sub 1^ (A/D)^sup 1/2^ where H is average chip thickness (in inches), F^sub 1^ is feed per tooth (in ipm), A is radial depth of cut (in inches), and D is cutter diameter (in inches). If the machine cannot maintain the feed rate, change to a smaller diameter cutter or increase the radial depth of cut.

Insert shape and lead angle also affect feed per tooth. For a 45deg leadangle cutter, for example, average chip thickness is 25-29% less than for a 0deg lead-angle cutter. As the lead angle increases, the average chip thickness decreases. Thus to calculate the true average chip thickness, you must multiply feed per tooth by the sine of the cutter lead angle.

For round inserts, the chip thickness changes with the depth of cut. The larger the depth of cut, the larger the lead angle. Taking the maximum depth of cut with a button cutter, for instance, results in about a 45deg lead angle and a relatively thick chip if the radial DOC is over onethird the cutter diameter. A very small depth of cut produces about an 80deg lead angle and an extremely thin chip incapable of removing heat that could also produce severe rubbing. When you must take a very small depth of cut with a button insert, you can reduce these effects somewhat by using extremely high feed rates.

You also must take radial runout into account. No multi-insert cutter has zero runout. Common radial runout is about 0.003″ (0.08 mm). Consider a case where feed per tooth is 0.005″ (0.13 mm), the high insert protrudes 0.003″ and has a chip load of 0.008″ (0.20 mm), and the low insert has a maximum chipload of only 0.002″ (0.05 mm). A common mistake is to conclude that the larger chipload will contribute to poor insert life. In reality, the opposite is true. Too small a chipload can be more of a problem.

The cutter also will have some axial runout (the difference between the height of the topmost insert and the lowest insert in a two-insert cutter, as measured by an indicator). While axial runout affects both surface finish and tool life, it affects surface finish most. If all inserts have a corner facet, then the insert that sticks out the most will wipe the surface of the part and produce a very good surface finish, provided that feed per revolution is less than facet width.

At the Cutter Edge

Eventually, all inserts will fail. A combination of flank and crater wear is desirable because tools last longer than with other failure mechanisms, such as chipping, thermal cracks, builtup edge, notching, or fracturing, and tool life is very predictable.

Be aware that the true wear mechanism acting on a tool may not be obvious. Examine worn inserts carefully to determine the true failure mechanism and the right corrective action to take. Don’t assume that inserts are failing because of abrasive wear. More than half the time, chipping, which begins with microcracking or builtup edge, will cause the failure.

Builtup edge, for example, occurs when particles of work material adhere to the cutting edge and fragments break loose, pulling minute carbide particles and leaving a rough, uneven edge. Aluminum and soft stainless steels are particularly susceptible to builtup edge.

Until recently, many tool users believed that increasing cutting speed reduced or eliminated builtup edge formation. Research has shown, though, that builtup edge forms at a certain temperature relative to the cutting speed. Identify this temperature zone, and you can minimize builtup edge by either increasing or decreasing cutting speed, which can be advantageous on machines limited in power and speed

Copyright Society of Manufacturing Engineers Jul 1996

Provided by ProQuest Information and Learning Company. All rights Reserved