Cutting Tool Engineering
January 2011 / Volume 63 / Issue 1

Milling Mastery

By Edmund Isakov, Ph.D.

Boosting milling productivity requires understanding the process.

Milling is a complex process in which a rotating solid or multiple indexable-inserts cutter removes metal or other material. Each insert removes a small amount of metal with each revolution of the spindle. Because the workpiece and cutter can be moved in more than one direction at the same time, surfaces with almost any orientation can be machined.

Milling includes three major elements: workpiece, cutting tools (diameter, number of inserts, cutting geometry and milling parameters) and machine tool. The main differences between milling and other machining processes are:

• Interruptions in cutting occur as the cutter’s inserts alternately engage and leave the workpiece,

• Small chips are produced, and

• Chip thickness varies.

Workpiece Hardness

It’s imperative to know a workpiece’s hardness prior to milling. Normally, a supplier provides the hardness, usually in a Brinell or Rockwell number. When a hardness number is provided in the Rockwell B or Rockwell C scale, it must be converted into a Brinell hardness number. (The author developed not only the formulas to make such conversions, but also the formulas to calculate the ultimate tensile strength of a workpiece based on its Brinell hardness. The ultimate tensile strength of a workpiece is used for calculating cutting force.)

Types of milling tools include face-mills, endmills and specials. Because of space limitations, only facemills’ features are described in this article because facemilling removes most of the stock and represents general milling.

Facemills can be made to almost any size, but usually range from 3.0 " to 20.0 " in diameter. A facemill should have enough teeth, or inserts, to provide uninterrupted contact with the workpiece. One tooth (insert) in contact with the workpiece (Figure 1b) will cause vibration and chatter, resulting in a poor surface finish, dimensional inaccuracy and excessive tool wear. Too many teeth in the cut (Figure 1a) may block chip evacuation because of too little space between the inserts. Chip interference increases power consumption and may damage the mill, workpiece or both.

Figure1.psd
Courtesy of Metals Handbook, Ninth Edition, Volume 16

Figure 1. Effect of number of teeth, or inserts, on milling.

(a) Too many teeth in the cut may block chip evacuation because of too little space between the inserts.

(b) One tooth in contact with the workpiece will cause vibration and chatter, resulting in a poor surface finish, dimensional inaccuracy and excessive tool wear.

(c) Complete dynamic stability of the cutter is achieved when at least two inserts are engaged with the workpiece.

Dynamic stability when facemilling extends tool life and improves surface finish by preventing the cutting edge from chipping. Complete dynamic stability of the cutter is achieved when at least two indexable inserts are engaged with the workpiece (Figure 1c). The author developed a formula showing how the two inserts (Z2) would be in contact with the workpiece:

Z2 = Zmin × α ÷ 360° (1)

Zmin = Z2 × 360° ÷ α = 720° ÷ α (2)

Where Z2 is 2, Zmin is the minimum required number of inserts in a facemill and α is the engagement angle.

Table 1. Engagement angle and required minimum number of inserts in the cutter.

ae/D

1

0.85

0.75

0.70

0.65

0.60

0.55

0.50

0.45

Engagement angle

180

134

120

114

107

102

96

90

84

Zmin

4

5

6

6

7

7

8

8

9

The formula for calculating the engagement angle (α) was described and explained in the July 2010 CTE article “New Mill.” The engagement angle depends on the radial WOC (ae) and the mill’s diameter (D). Table 1 shows the engagement angles and respective required minimum number of inserts (Zmin) in the facemill to ensure two inserts are engaged with the workpiece. The required minimum number of inserts is a guideline for selecting the appropriate facemill based on nomenclature in a toolmaker’s catalog.

Cutting Geometry

A facemill’s cutting geometry is usually one of the following:

• Double positive (positive axial rake and positive radial rake)

• Positive negative (positive axial and negative radial rake)

• Double negative (negative axial and negative radial rake)

The angular relations of the cutting edge greatly impact cutting efficiency. Axial rake controls chip flow, tangential force and cutting edge strength. Contemporary facemills have positive rake angles, typically from 5° to 20°. An increase in axial rake reduces tangential force and edge strength.

Radial rake has a major influence on chip evacuation and tool life. Positive radial rake angles typically range from 1° to 14°. Positive rake angles direct chips up and away from the workpiece. Negative radial rake angles, which strengthen cutting edges, typically range from -2° to -11°.

Facemills with positive-negative and double-positive geometries are applied for cutting carbon, alloy and stainless steels; ductile and malleable cast irons; titanium alloys; and high-temperature alloys. Facemills with double-positive geometries are mainly used for cutting aluminum alloys and some other nonferrous materials.

Lead angle (λ) is the angle between the side-cutting edge of the insert and the line parallel to the axis of rotation (Figure 2). This definition agrees with customary U.S. units of measure.

The angle between the side-cutting edge of the insert and line perpendicular to the axis of rotation agrees with the metric units of measure (Figure 3). This angle (γ) is called “cutting edge angle” or “approach angle.” Based on their definitions, lead and approach angles relate to each other as:

λ = 90° - γ (3)

γ = 90° - λ (4)

Facemills with a 0° lead angle and 90° approach angle produce chips that have a thickness equal to the feed per tooth. Facemills with a lead angle greater than 0° or an approach angle less than 90° produce chips thinner than the feed per tooth.

Lead angles can vary from 0° to 45°. Other lead angle values can be 15°, 20° and 30°, which are equivalent to approach angles of 75°, 70° and 60°, respectively. The most common lead or approach angle is 45°.

Fig1 copy.tif

Figure 2. Lead angle is the angle between the side-cutting edge of the insert and the line parallel to the axis of rotation.

Angle copy.tif

Figure 3. Approach angle is the angle between the side-cutting edge of the insert and line perpendicular to the axis of rotation.

These angles affect chip thickness (hm): at 0° lead angle (90° approach angle), the chip thickness equals feed per tooth (fz). At any other angle, chip thickness is defined by the formulas:

hm = fz cosλ (5)

hm = fz sinγ (6)

Adjustment to chip thickness is needed to increase the feed per tooth (fza) and keep the same productivity as when using a 0° (90°) lead (approach) angle:

fza = fz ÷ cosλ (7)

fza = fz ÷ sinγ (8)

Milling Parameters

Programmed milling parameters include axial DOC (ap), feed per tooth (fz), cutting speed (VC) and radial WOC (ae). Axial DOC depends on the indexable-insert geometries, carbide grades and workpiece hardness. When roughing, the axial DOC is about one-half of the height of the insert.

Feeds per tooth are established values based on the following values:

• 0.003 " to 0.006 " for light milling

• 0.006 " to 0.010 " for medium milling

• 0.010 " to 0.020 " for heavy-duty milling

Cutting speeds vary greatly based on recommendations from cutting tool manufacturers (Table 2 on page 66). Cutting speed data is based on the type of work material, its hardness, cemented carbide grades, chip thickness and the ratio (ae ÷ Dc) of the radial WOC (ae) to the facemill diameter (D).

Enlarged view

Figure4.tif

Negative angle of entry

Courtesy of Kennametal

Figure 4. A negative angle of entry is recommended whenever possible because the insert contacts the workpiece at its strongest part, which is away from the cutting edge.

Selecting cutting speed is a challenge. There are no set criteria for choosing cutting speed because too many independent variables are involved in milling. If machine shops are not sure about the cutting speed, they should contact their cutting tool supplier for recommendations.

Selecting the radial WOC (ae) is also a challenge because it plays several important roles.

1. Along with axial DOC and feed rate, it affects metal-removal rate. An increase in the radial WOC increases the mrr.

2. The ratio of the radial WOC to the cutter’s diameter is a measure of the radial engagement of a cutter with a workpiece. Radial WOC defines the position of the cutter centerline: If ae is greater than D ÷ 2, the cutter centerline is located on the workpiece; when ae is less than D ÷ 2, the cutter centerline is not located on the workpiece.

3. The ratio of ae ÷ D determines the uniformity of chip thickness. When radial WOC is equal to the cutter’s diameter (ae ÷ D = 1, i.e. full engagement), the chip being formed starts at zero thickness at the point of entry. It increases to a maximum thickness at the centerline of the cutter, and thins to zero at the point of exit. This type of cut produces nonuniform chips, generates maximum friction at the cutting edges, and, as a result, cutting resistance increases. Full engagement should not be used unless absolutely necessary. Uniform and sufficiently thick chips are produced when the radial WOC is about 70 to 75 percent of the cutter’s diameter. This type of cut generates less friction at the cutting edges and decreases cutting resistance.

4. Radial WOC defines the cutter’s angle of entry into a workpiece, which can be negative or positive. If the cutter’s centerline is on the workpiece (ae is greater than D ÷ 2), the angle of entry is negative (Figure 4). A negative angle of entry is recommended whenever possible because the insert contacts the workpiece at its strongest part, which is away from the cutting edge. If the cutter’s centerline is not on the workpiece (ae is less than D ÷ 2), the angle of entry is positive (Figure 5). A positive angle of entry is not recommended because the insert contacts the workpiece with the cutting edge, which is the weakest part. That can result in insert chipping. If a positive angle of entry is necessary, then a more shock-resistant carbide grade and a cutting edge with a T-land or hone are recommended.

Table 2. Starting cutting speed values for selected grades of steel and titanium alloys.

Nomenclature

Kennametal Inc.1

Sandvik Coromant2

Walter USA Inc.3

Type of cutter

KSSM 45,

45º lead angle

30° to 45° lead angle, large engagement

Face/shoulder

milling cutters

Carbide grade

KC935M,

CVD coating

GC4220

CVD coating

WKP 25

CVD coating

Material group

Alloy steel

Brinell hardness

1.7225

AISI 4140

Not provided

02.1

AISI 4140

175 HB

6

AISI 4140

180 HB

Chip thickness, in.

Not provided

0.012

Not provided

Engagement, %

Not provided

80

100 to 50

Cutting speed, sfm

780 750 850

Carbide grade

KC935M,

CVD coating

GC1030

PVD coating

WSM 35

PVD coating

Material group

Stainless steel

Brinell hardness

1.4401

AISI 316

Not provided

05.21

AISI 316

200 HB

14

AISI 316

180 HB

Chip thickness, in.

Not provided

0.008

Not provided

Engagement, %

Not provided

80

100 to 50

Cutting speed, sfm

830 590 430

Carbide grade

KC725M,

PVD coating

GC1030,

PVD coating

WSM 35,

PVD coating

Material group

Titanium alloy

Tensile strength, MPa

3.7165

Ti6Al4V

Not provided

23.22

Ti6Al4V

1,050

37

Ti6Al4V

1,050

Chip thickness, in.

Not provided

0.008

Not provided

Engagement, %

Not provided

80

100 to 50

Cutting speed, sfm

180 155 160
1 Catalog 6050 inch, pp. 83, 232, 517, 518 and 520. 2 Main catalog (2008), pp. D223, D225, D241, I 7, I 8 and I 10. 3 General catalog (9/2007), pp. 447 and 600.

5. When the radial WOC is less than half the facemill’s diameter (ae is less than D ÷ 2), a feed rate adjustment (Fa) is necessary to maintain the same productivity (the same mrr) as when the radial WOC is higher than half the facemill diameter, i.e. (ae is greater than D ÷ 2). The following formula can be used for the adjustment:

Figure5.tif

Where fz is feed per tooth (in.), Z is the number of inserts in a cutter, n is the rotational speed of a cutter (rpm), D is cutter diameter (in.), ae is radial WOC (in.), and R is cutter radius (in.).

Milling Machines

Milling is performed in almost every type of machine that can rigidly hold and rotate a cutter while moving a workpiece toward the cutter or vise versa. Machines used for production milling should incorporate:

• Variable-speed motors

• Ballscrew or hydrostatic worm precision gears and bearings

• Hydrostatic liners

• NC or CNC

• Automatic drives

• Automatic toolchangers

Machines that drive cutters with horizontal and vertical spindles are widely used. Some special-purpose machines have horizontal, vertical and angular spindles that operate consecutively, simultaneously or both.

Enlarged view

Figure5.tif

Positive angle of entry

Courtesy of Kennametal

Figure 5. A positive angle of entry is not recommended because the insert contacts the workpiece with the cutting edge, which is the weakest part. That can result in the insert chipping. If a positive angle of entry is necessary, then a more shock-resistant carbide grade and a cutting edge with a T-land or hone are recommended.

[Note: Information in this section is adapted from Metals Handbook, Ninth Edition, Volume 16, Machining, ASM International, fourth printing, 1999.]

Regardless of the type of milling machine, the following specifications should be available to allow setup of the machine for maximum productivity.

• Spindle maximum rating, hp (kW)

• Spindle maximum torque, ft.-lbs. (N∙m)

• Spindle speed at maximum torque, rpm

• Spindle maximum speed, rpm

• Spindle (or main drive) efficiency factor, percent.

The following example shows how the three elements of an integrated face-milling system (workpiece hardness, facemill nomenclature with selected cutting parameters and milling machine specification) interact to produce the required power and torque values in comparison with those available from a given milling machine.

(The following technical information was adapted from Metals Handbook, Ninth Edition, Volume 16, Machining.)

1. Workpiece:

1030 steel plate, hardness 165 to 185 HB

Width, 12 "; length, 147 "

2. Facemill nomenclature:

Diameter, 16.0 "

Number of teeth, 32 (cemented carbide inserts)

Machining conditions:

Spindle speed, 72 rpm

WOC, 12.0 "

DOC, 0.125 "

Feed per tooth, 0.027 "

3. Machine tool specification:

Fixed-rail, bed-type milling machine

Vertical spindle maximum rating, 100 hp

Calculated data:

Cutting speed, 302 sfm

Feed rate, 62 ipm

mrr, 122 in.3/min.*

Power required at the cutter, 95 hp

* The mrr of 122 in.3/min. is incorrect. Based on the WOC, DOC and feed rate, the mrr = 12 × 0.125 × 62 = 93 in.3/min.

[Note: It is obvious that the calculation of the required power was performed by the conventional method based on the mrr and the average unit power. The conventional method was described by the author in “New Mill” (CTE, July 2010, p.46).]

Based on the previous information, the author performed the calculations using his new method described in the “New Mill” article. Contemporary metalcutting terminology is used.

1. Workpiece:

Medium-carbon steel, AISI 1030

Brinell hardness, 165 to 185 HB

The higher number of hardness (185 HB) is taken for calculating the ultimate tensile strength (σ) using the linear regression formula developed by the author.

σ = 471 × HB + 4,376 = 471 × 185 + 4,376 = 91,500 psi

2. Facemill:

Nomenclature is the same as shown previously.

Machining conditions:

Cutting speed, 302 sfm

Radial WOC, 12.0 "

Axial DOC, 0.125 "

Feed per tooth, 0.027 "

3. Machine tool:

Specification is the same as shown previously.

Calculated data:

Milling calculator developed by the author was used to perform conventional and advanced calculations (the calculated data is shown below).

Conventional calculations:

Spindle speed, 72 rpm

Feed rate, 62.3 ipm

mrr, 93.4 in.3/min.

Cutting time per pass, 2.36 min.

Advanced calculations

Number of teeth (inserts) in the cut, 11

Tangential cutting force with sharp cutting edges, 4,940 lbs.

Tangential cutting force with dull cutting edges, 6,420 lbs. [4,940 × 1.3 (1.3 is a tool wear factor, Cw)]

Torque at the cutter with sharp cutting edges, 3,290 ft.-lbs.

Torque at the cutter with dull cutting edges, 4,280 ft.-lbs. (3,290 × 1.3)

Power required at the cutter with sharp cutting edges, 45.2 hp

Power required at the cutter with dull cutting edges, 58.8 hp (45.2 × 1.3)

Power required at the main drive with sharp cutting edges, 56.5 hp (45.2 ÷ 0.8); estimated main drive efficiency factor, E = 0.8

Power required at the main drive with dull cutting edges, 73.5 hp (58.8 ÷ 0.8)

The new calculation method allows users to obtain data not available from the conventional calculation method. That data includes ultimate tensile strength vs. workpiece hardness, number of teeth (inserts) in the cut, tangential cutting force when the cutting edges are sharp or dull, and torque at the cutter when the cutting edges are sharp or dull. The power required for a milling operation shown in this example is less than 50 percent of that estimated by the conventional method. CTE

EdIsakov.tif About the Author: Edmund Isakov, Ph.D., is a consultant, writer and frequent contributor to CTE. He is the author of the books “Mechanical Properties of Work Materials” (Modern Machine Shop Publications, 2000), “Engineering Formulas for Metalcutting” (Industrial Press, 2004), “Cutting Data for Turning of Steel” (Industrial Press, 2009) and the software “Advanced Metalcutting Calculators” (Industrial Press, 2005). He can be e-mailed at edmundisakov@bellsouth.net or reached at (561) 369-4063.



CUTTING TOOL ENGINEERING Magazine is protected under U.S. and international copyright laws.Before reproducing anything from this Web site, call the Copyright Clearance Center Inc.
at (978) 750-8400.