Volume 16 - Machining Part 7 pdf

The trepanning tool used had two carbide cutters mounted on an 1141 steel body; tool design is shown in Fig.. Figure 5 shows a basic engine lathe setup, in which a cylindrical workpiece

When a center hole is unobjectionable, the trepanning tool consists of an adjustable fly cutter mounted on a twist drill (Fig 1); the drill serves as both driver and pilot, and the single-point tool can be positioned as desired to change the size

of the circle cut If a center hole cannot be permitted, a tool of the type shown in Fig 1 can be used without a drill pilot

By this technique, however, rigidity is more difficult to maintain, and there is greater likelihood of tool chatter and loss of dimensional control

Fig 1 Drill-mounted adjustable fly cutter used for trepanning various sizes of disks from flat stock, or grooves

around centers

There is no established maximum thickness or diameter of disks that can be cut by this method of trepanning Because of the load imposed on the tool, however, the process is seldom used for cutting material more than about 6.4 mm ( in.) thick In addition, because rigidity decreases as diameter increases, disks cut by this method are usually less than 150 mm (6 in.) in diameter Larger cuts by trepanning are not made if other methods can be used Smaller trepanning cuts may compete with press-working (if the means are available), and larger cuts may compete with other methods, such as flame cutting

In this type of trepanning, slow speeds (ranging downward from about 10 m/min, or 35 sfm) are ordinarily used and feed

is controlled manually Cutting fluids are seldom employed

Large Shallow Through Holes

Round through holes having diameters that exceed depth by a factor of about five or more can often be efficiently and accurately produced by trepanning Workpiece configuration often dictates the trepanning technique used because special fixturing may be necessary to ensure adequate rigidity The tools and techniques employed in one application are described in the following example, in which trepanning was preferred to drilling

Example 1: Nine Shallow Holes in Web of a Steel Gear

Trepanning proved more practical than drilling for producing nine weight-reducing holes in the web section of an aircraft accessory drive gear made of 9310 steel (Fig 2) Depending on the size of these gears, the holes ranged from 19 to 32

mm ( to 1 in.) in diameter, and web-section thickness ranged from 3.56 to 6.35 mm (0.140 to 0.250 in.)

Fig 2 Shallow holes produced by trepanning in aircraft gear shown at top left Top-brazed carbide inserts cut

only 40% as many holes per grind as side-brazed inserts

Trepanning was done with carbide-insert single-point tools at a speed of 91 m/min (300 sfm) and a feed of 0.05 mm/rev (0.002 in./rev) Originally, a top-brazed insert (bottom left, Fig 2) was used, but tool life was only 30 holes per grind By changing to side-brazed inserts (bottom right, Fig 2), tool life was increased to 75 holes per grind With either tool, maximum tool life was obtained when the tool was not allowed to cut completely through the web A thin section was left

to hold the plug, and this section was easily knocked out during indexing of the gear

Circular Grooves

The tools and techniques used for producing round disks or large shallow through holes can also be used to provide metal parts with circular grooves for accommodating O-rings or for other purposes The only difference is that the cutter must

be shaped to form the desired cross-sectional shape of the groove

When a groove to be cut is only slightly larger in diameter than a concentric pilot hole, optimum results are obtained by the use of a combination drilling-and-trepanning tool that resembles a hollow mill (Fig 3) With this tool, a twist drill is inserted into a hollow cutter and held by a setscrew This type of trepanning cutter usually has two or more cutting edges

to provide balance, which assists in maintaining dimensional control Cutting edges have a back rake angle of about 20° for most applications

Fig 3 Combination tool for producing a groove close to a concentric pilot hole

Any machines normally used for drilling are suitable for driving combination tools of the type shown in Fig 3 Speeds up

to 30 m/ min (100 sfm) are ordinarily used, in conjunction with feeds of about 0.1 mm/rev (0.004 in./rev) Soluble oils are usually satisfactory as cutting fluids, although sulfurized oils are preferred when tolerance and finish requirements are critical The following example describes an application in which trepanning was more efficient and economical than the use of single-point tools for producing a circular face groove

Example 2: Trepanning Versus Single-Point Plunge Cutting

Originally, the 73 mm (2 in.) groove in the 4140 steel part shown in Fig 4 was produced in roughing and finishing operations on a lathe, using single-point carbide-insert tools Chip build-up and tool breakage were continual problems Tool life per sharpening was only 25 pieces, and production time per piece was 3.9 min

Fig 4 Tool used in trepanning operation (shown at top left and bottom) The part is shown at top right

Dimensions given in inches

Tool breakage and chip buildup were eliminated (and grooving was reduced to a one-operation job) by substituting trepanning for the original method The trepanning tool used had two carbide cutters mounted on an 1141 steel body; tool design is shown in Fig 4 Trepanning also reduced time per piece to 1.8 min (less than half, compared with the original method) and doubled tool life to 50 pieces per sharpening

Deep Holes

Trepanning is often the most practical method of machining deep holes or tubes from the solid Deep-hole Trepanning is similar to gun drilling (see the article "Drilling" in this Volume) in that both processes require a pressurized cutting fluid system and employ self-piloting cutting action The two main differences are:

• Trepanning is practical only for larger holes (more than about 50 mm, or 2 in., in diameter)

• Trepanning produces a solid core, while gun drilling forms only chips

As a means of producing holes 50 mm (2 in.) in diameter or larger (especially holes whose depth is eight or more diameters), Trepanning offers the following advantages over spade or twist drilling, with their allied operations:

• Closer tolerances can be met on diameter and straightness

• Drilling of deeper holes is feasible

• Rate of metal removal is higher

• In machining costly work materials, cores are more valuable than chips

Trepanning can also be used to produce a tube from a cylindrical billet when machining space-age metals such as beryllium The trepanning of a cylindrical core from the center of a solid cylinder of metal is not ordinarily done in regular mass production Beryllium, however, is a problem metal that needs special methods

Misalignment is probably the most frequent single source of difficulty in deep-hole trepanning The misalignment may be caused by insufficient rigidity in the tooling and the setup Accurate alignment and rigidity are essential for control of dimensions and finish and for satisfactory tool life at high depth-to-diameter ratios

Machines for Deep-Hole Trepanning

For trepanning holes less than about five diameters deep, simple vertical drill presses are usually satisfactory However,

as the depth of the hole exceeds five times diameter, any type of vertical equipment becomes progressively more impractical In addition, as the depth-to-diameter ratio increases, accuracy is lost more rapidly in equipment in which the tool is rotated and the work is held stationary Therefore, engine lathes, turret lathes, or horizontal drilling machines are preferred for Trepanning deep holes In all of these machines, the workpiece is rotated while the tool remains stationary This technique results in greater accuracy, other conditions being constant

Regardless of the type of machine used, it must be rigid and capable of speeds up to 185 m/min (600 sfm) to accommodate carbide tooling It should also have variable feed control

Engine Lathes. Figure 5 shows a basic engine lathe setup, in which a cylindrical workpiece is rotated, the tool is fed into it, and an inside-diameter-exhaust trepanning head is used (see the section "Tools for Deep-Hole Trepanning" in this article) Such a setup is used for holes about 50 to 115 mm (2 to 4 in.) in diameter One end of the workpiece is held in

a three-jaw chuck, and the other end in a roller steady rest (rollers are about 150 mm, or 6 in., in diameter) A relatively long workpiece requires an additional steady rest midway between the chucking headstock and the roller steady rest

Fig 5 Engine lathe setup for trepanning deep holes

The end of the workpiece next to the steady rest must be faced at right angles to the spindle centerline The facing cut, made by a tool on a cross slide, provides a flat surface for the fluid seal on the guide bushing and prevents the runout that could make the fluid seal leak The guide bushing should be mounted on ball bearings which are the most economical means of support at the speeds involved

Cutting fluid under pressure enters the leakproof rotary joint behind the bushing and flows into the annular space around the hollow boring bar The fluid then flows to the cut between the bushing and the periphery of the tool head, picks up the chips, and flushes them through the head between the cutter and the core and then out along the space between the core and the inner wall of the boring bar An additional fluid seal is necessary at the rear of the guide-bushing/fluid-transfer unit The tailstock end of the boring bar is mounted in a headstock on the lathe carriage and is rigidly clamped in position

by means of a bearing cap and clamping nuts

To serve as a vibration damper, a steady rest is located directly behind the guide-bushing/fluid-transfer unit This damper

is of the same construction as the boring-bar headstock, except that a two-piece bronze bushing is used to damp vibration and to allow the boring bar to slide

Alignment is critical The spindle, chuck, steady rests, guide bushing, and boring-bar headstock must be as nearly in line

as possible In addition, the machine ways must be aligned, and the boring bar must be ground to uniform diameter and straightness

The bores in the guide-bushing/fluid-transfer unit, the vibration-damper unit, and the boring-bar headstock should be large enough to accommodate the boring bar for the largest-diameter hole to be trepanned on the machine For smaller holes, smaller boring bars can be used with appropriate bushings

For holes more than about 115 mm (4 in.) in diameter, other setups are sometimes more economical and can be used with an outside-diameter-exhaust head for trepanning relatively deep holes (see the section "Tools for Deep-Hole Trepanning" in this article) One of these adaptations is the use of a three-roll support on the bed of an engine lathe A three-roll support used in conjunction with an outside-diameter-exhaust head effects a savings by eliminating the need for

a starting or guide bushing

Turret lathes are also suitable for trepanning relatively deep holes, as indicated in the following example

Example 3: Use of a Turret Lathe for Trepanning

Holes 127 mm (5 in.) in diameter and 915 mm (36 in.) deep were trepanned in vacuum-melted 4340 steel using an outside-diameter-exhaust trepanning head with a 19 mm ( in.) wide carbide cutting tip A turret lathe of 11 kW (15 hp) capacity was used to rotate the workpieces at 190 rev/min (76 m/min, or 250 sfm).Water-soluble oil, under pressure of

275 kPa (40 psi) was pumped through the cutting area at 190 L/min (50 gal./min) At a feed rate of 0.18 mm/rev (0.007 in./rev), two pieces per hour were produced

Tools for Deep-Hole Trepanning

Boring bars for trepanning are hollow tubes that allow the workpiece core to enter with enough clearance for cutting fluid

to flow to the cutter or for fluid and chips to be forcibly exhausted from the cutter The bar is usually made from 52100 bearing steel or a similar steel Wall thickness ranges upward from about 7.9 MM ( in.) depending on the length of the bar and the required resistance to torsional forces

Trepanning heads are cylindrical and usually employ a single solid-carbide or carbide tip cutter Multiple-cutter heads, despite their desirable chip-breaking action, are used to a lesser extent because they pose problems in attaining balanced cutting action without which hole accuracy may be sacrificed

Single-cutter heads (Fig 6) are self-piloting; they are supported and guided by wear pads located about 90 and 180 ° behind the cutter The head fits onto the boring bar by means of a pilot diameter and can be driven by three lugs With this mating design, the head is locked to the bar screws Some heads are secured to the bar by Acme threads around the inner circumference of the head, but high torsional forces can cause thread seizure Ahead of the cutting edge on the outside diameter of the head is a relief for intake of cutting fluid or for exhaust of cutting fluid and chips

Fig 6 Two types of single-cutter trepanning heads

One type of head (Fig 6a), usually for holes up to 115 mm (4 in.) in diameter and with depths of 12 to 15 diameters, accommodates cutting fluid flow from the inside diameter of the bar and exhausts the fluid on the outside diameter Recommended maximum depths for holes trepanned with outside-diameter-exhaust heads are as follows:

For holes 116 mm (4 in.) in diameter and larger, maximum depth is limited only by machine design

With this type of head, chips and fluid are exhausted along a longitudinal groove milled on the outside diameter of the head The clearance between the core and the inside wall of the head must be controlled so that the volume of cutting fluid is restricted As a result, there is a high-velocity centrifugal action that forces the chips away from the cutting edge

In production trepanning, one plant found that a fluid-inlet area of 645 mm2 (1 in.2) produces a pressure of about 345 kPa (50 psi) on a 178 mm (7 in.) diam head This size of inlet area allows full pump flow through the head and provides sufficient velocity for chip disposal As the hole size decreases and the inlet area remains constant, the pressure increases Increased pressure is desirable as hole diameter decreases or as depth increases For holes less than 100 mm (4 in.) in diameter, however, an inlet area of 645 mm2 (1 in.2) is not possible; for these holes, the inlet area should be made as large

as possible to provide adequate volume without weakening the head

The outside diameter of an outside-diameter-exhaust head is only 0.50 to 0.64 mm (0.020 to 0.025 in.) smaller than the diameter of the hole being cut; this prevents chips from escaping between the head and the wall of the hole As a result, the possibility of a marred finish is lessened, and channeling of the fluid and chips through the exhaust groove is facilitated

To minimize the problem of chip disposal in holes more than about 15 diameters deep, an inside-diameter-exhaust head (Fig 6b) is used With this type of head, fluid under pressure flows to the cutting edge over the outside diameter of the bar and head The fluid and the chips are exhausted through the inside diameter of the boring bar

Wear pads (Fig 6) are essential components of single-cutter heads Wear pads balance cutting force, control hole size, and provide a burnishing action that may improve finish

Ordinarily, wear pads have steel bodies and brazed-on carbide wearing surfaces The wear pad body may have two angular sides that result in a dovetail fit in the head.The pads are circle ground so that when they are positioned in the head they will clear the bore wall by about 0.05 mm (0.002 in.) and will project about 0.25 mm (0.010 in.) from the head One pad is located approximately 90° behind the cutting edge; this pad steadies the head against the bore and balances the cutting force The other pad is about 180° behind the cutter and automatically controls the size of the hole If the cut is oversize, the bore is large, and the pressure on this pad is immediately decreased As a result, the head moves away from the surface being cut, reducing the bore size until equilibrium is again established Similarly, if the cut is undersize, pressure on the pad is increased, and the head moves toward the surface being cut

Initial cutting action is controlled by a guide bushing (Fig 5), by a counterbore, or by a starting tool that cuts a groove (Fig 7).If a bushing is used, starting feeds are relatively light and characteristically produce stringy chips, which must be removed at intervals The counterbored hole or starting groove should be deep enough to ensure self-piloting by the trepanning head

Fig 7 Starting tool for trepanning

Conventional cutters (Fig 8) have a carbide tip brazed on a tool steel body (Because index positions are limited and chip flow is obstructed, disposable-insert tooling has not been widely used in trepanning.) The brazed cutter is designed

so that the single edge has three steps to break the chip into three equal widths Each step includes a parallel chip breaker The cutter is commonly 19 mm ( in.) wide, but wider cutters have been successfully used for holes more than about 100

mm (4 in.) in diameter

Fig 8 Typical design of a trepanning cutter for producing deep holes Dimensions given in inches

The radial position of the cutter when used in a stationary head is important.Viewed from the cutting end of the head, the cutter should be approximately at the 2 o'clock position; thus the cutting fluid will wash the chips away from the cutter through the relief on the outside diameter of the head, and the core, when cut, will fall away from the cutter

Multiple-cutter heads are sometimes more appropriate than those with single cutters This is especially true when hole starting is difficult or for minimizing shock on the bar or other components in the driving mechanism

Example 4: Use of a Three-Cutter Head for Trepanning Transversely Through a Steel Cylinder

A 64 mm (2 in.) diam hole was trepanned through the 100 mm (4 in.) diameter of a solid cylinder of 8615 steel A specially designed three-cutter head (Fig 9) of 4140 steel was used in order to minimize spindle shock This head, of the outside-diameter-exhaust type, included three 150 mm (6 in.) long bronze conventional wear strips, spaced 120° apart and 30° behind each cutter To provide maximum stability and accuracy, an additional set of three cylindrical carbide wear strips (7.9 mm, or in in diameter and 32 mm, or 1 in., long) was incorporated A guide bushing was used in conjunction with a modified drill press that provided 22 kW (30 hp) at the spindle Cutting fluid (active mineral oil) was pumped through the bar at 345 kPa (50 psi) and 380 L/min (100 gal./min)

Fig 9 Three-cutter trepanning head used for cutting a 64 mm (2 in.) diam hole through a solid cylinder of

8615 steel Dimensions given in inches

use of a four-cutter head The first pair of cutters produces a narrow groove; this is then widened to final dimensions by the second pair of cutters Initial and maintenance costs, however, are greater for this type of tool than for a single-cutter head Figure 10 illustrates the recommended coolant pressure and flow rates for multiple-cutter internal chip removal trepanning tools

Fig 10 Recommended coolant pressures (a) and volumes (b) for multiple-cutter internal chip removal

trepanning tools

Speed and Feed in Deep-Hole Trepanning

Table 1 lists speeds and feeds for trepanning deep holes in a variety of carbon, alloy, and stainless steels These values are useful as a starting point for selecting efficient and economical rates

Table 1 Speeds and feeds for the deep-hole trepanning of various steels with high-speed tool steels and carbide tools

Speed Feed(a) Tool material

175-225 Hot rolled,

normalized, annealed, or cold drawn

150 500 0.18 0.007 P30 C-6

15 50 0.15 0.006 S9,

S11(b)

T15, M42(b)

100-150 Hot rolled,

normalized, annealed, or cold drawn

185 600 0.20 0.008 P30 C-6

32 105 0.18 0.007 S4,

S5

M2, M3

Low-carbon leaded: 12L13, 12L14, 12L15

200-250 Hot rolled,

normalized, annealed, or cold drawn

85-125 Hot rolled,

normalized, annealed, or cold drawn

150 500 0.20 0.008 P30 C-6

23 75 0.18 0.007 S4,

S5

M2, M3

125-175 Hot rolled,

normalized, annealed, or cold drawn

135 450 0.20 0.008 P30 C-6

9 30 0.10 0.004 S9,

S11(b)

T15, M42(b)

125-175 Hot rolled,

annealed, or cold drawn 145 475 0.18 0.007 P30 C-6

14 45 0.10 0.004 S9,

S11(b)

T15, M42(b)

18 60 0.15 0.006 S4,

S5

M2, M3

175-225 Hot rolled,

annealed, or cold drawn 115 375 0.15 0.006 P30 C-6

9 30 0.10 0.004 S9,

S11(b)

T15, M42(b)

17 55 0.13 0.005 S4,

S5

M2, M3

High carbon: 50100, 51100, 52100, M-50 175-225 Hot rolled,

annealed, or cold drawn 105 350 0.15 0.006 P30 C-6

Wrought stainless steels

27 90 0.075 0.003 S4,

S5

M2, M3

76 250 0.15 0.006 P30 C-6

15 50 0.075 0.003 S9,

S11(b)

T15, M42(b)

Martensitic: 403, 410, 420, 422, 501, 502

275-325 Quenched and

tempered

60 200 0.10 0.004 P30 C-6 Source: Metcut Research Associates

(a)

Based on standard 19 mm ( in.) cutting edge, single blade

(b) Any premium high-speed tool steel (T15, M33, M41-M47) or (S9, S10, S11, S12)

Processing conditions for a given application are best determined by production trials The nature and amount of machining to be done, the size and shape of the part, the work material, and the equipment and tooling may necessitate substantial deviations from the nominal speed and feed

In deep-hole trepanning, the ability to use optimum speed and feed largely depends on the rigidity of the boring bar and

on the effectiveness with which the cutting fluid cools, flushes away chips, and prevents chips from forcibly contacting the newly machined surface The speed and feed values given in Table 1 assume effective use of a suitable cutting fluid

Cutting Fluids for Deep-Hole Trepanning

Cutting fluids often represent the difference between success and failure in a trepanning operation In general, the cutting fluids recommended for trepanning are similar to those recommended for gun drilling, that is, straight oils Extreme pressure (EP) additives significantly improve tool life, particularly the life of the wear pads

In applications in which high-nickel or high-cobalt alloys are trepanned, sulfurized or other EP-enhanced cutting oils are critical to the life of the wear pads If the lubricating film between the wear pad and the workpiece breaks down, the cobalt binder in the carbide is quickly attacked, and the wear pads disintegrate In critical applications for nuclear materials in which chlorine and sulfur are not allowed because of stress corrosion problems, synthetic coolants used at ratios as low as 5:1 with heavy EP additives can result in a successful application of trepanning

The volume of the cutting fluid is also critical to the success of a trepanning operation Trepanning produces a large number of chips at a very high rate of speed in an extremely confined area Assuming the trepanning bit produces consistent, small chips, there is an immediate need to evacuate these chips as quickly as possible High volumes of coolant with increased viscosity will normally accomplish this task The power consumption of the coolant pump often equals the power consumption of the machine spindle driving the tool

In an application involving the vertical trepanning of platens for plastic injection molding presses, a 45 kW (60 hp) vertical mill was used The platens were 610 mm (24 in.) thick, and a 318 mm (12 in.) hole had to be trepanned through

1020 steel The cutting fluid was an EP-sulfurized mineral oil Vertical application necessitated the use of large volumes

of cutting fluid at high pressure to remove the chips from the hole A 45 kW (60 HP) coolant pump was successfully used

in the operation The starting bushing was combined with a chip evacuation box surrounding the workpiece to reduce the flow of coolant to the bed of the machine and to direct the waste chips and coolant to a settling tank Outside-diameter-exhaust trepanning was successfully used in this application

Planing

Introduction

PLANING is a machining process for removing metal from surfaces in horizontal, vertical, or angular planes In this process, the workpiece is reciprocated in a linear motion against one or more single-point tools Although planing is most widely used for producing flat, straight surfaces on large workpieces, the process can also be used to produce contours and a variety of irregular configurations, such as deep slots in large rotors, helical grooves in large rolls, and internal guide surfaces in large valves It is often possible to produce one or two parts on a planer in less time than is required merely to set up for machining by an alternative method; therefore, planing is often used for machining parts to meet production emergencies

Process Capabilities

As the hardness of the workpiece increases above about 25 HRC, metal removal rate and tool life decrease However, metals hardened to 46 HRC or higher can be planed For example, planing is often used to produce flat surfaces on large, heat-treated die blocks

The size of the workpiece that can be planed is limited only by the capacity of the available equipment Standard equipment is available that can make cuts as long as 15 m (50 ft), and still larger machines have been built to special order

Although planing is most widely used for machining large areas, it is also used for machining smaller parts or areas For example, jig-frame weldments can be squared and tooling-pad surfaces leveled on areas of less than 0.09 m2 (1 ft2) However, 305 mm (12 in.) is about the minimum planing stroke Another common practice is tandem, or gang, planing, in which a number of relatively small but identical workpieces are lined up on the table and planed at the same time

Tolerance and Finish. Even though the equipment used for planing is relatively large and rugged, close tolerances in

both flatness and parallelism can be achieved with planers For this reason, planing is sometimes selected over competitive processes

Flatness variations can be held within 0.013 mm (0.0005 in.) total indicator reading on workpieces up to 0.4 m2 (4 ft2) in area or up to about 1.2 m (4 ft) long Cast iron workpieces can be planed to a finish of about 1.60 m (63 in.) and steel workpieces to about 0.80 m (32 in.)

Planers

The planer develops its cutting action from the straight-line reciprocating motion between the tool and the workpiece On

a planer, the work is reciprocated longitudinally while the tools are fed sideways into the work The feed in planing is intermittent and represents width of cut Planer tables are reciprocated by either mechanical or hydraulic drives Most planers, however, are mechanically driven by such means as variable-voltage, constant-torque drives

The speed at which a mechanical-drive planer operates depends on the speed of the driving motor and on the gear ratio In hydraulic planers, table speed depends on the effective area of the piston and on the volume of oil pumped against the piston area per unit of time Regardless of whether the drive is mechanical or hydraulic, the efficiency of planers can be greatly increased by incorporating a means of increasing table speed on the return stroke, during which time no cutting is done

Double-housing planers (Fig 1) incorporate two vertical uprights that support the crossrail Double-housing planers are more rigid than open-side planers, but they are limited as to the width of workpiece they can accommodate

Fig 1 Significant components of a double-housing planer with a tool head on one of the two vertical support

uprights in addition to the two tool heads on the crossrail Another tool head can be supported on the other upright in some models The two uprights are immovable and limit the width of workpiece that can be planed in this machine

Open-side planers differ from double-housing planers mainly in that they have only one upright column, from which the crossrail is cantilevered over the table Open-side planers can accommodate wider workpieces than the double-housing machines because the workpieces can overhang from the side of the table without interfering with the planer mechanism When the workpiece is considerably wider than the table, an outboard rolling table can be used to support the overhanging section of the workpiece

The main disadvantage of open-side planers is that they are less rigid than double-housing planers Open-side planers are also limited to three tool heads: two on the crossrail and one on the single upright column However, an open-side planer can be converted into a double-housing planer by using an outboard detachable housing Outboard housings are available

as optional equipment and can be mounted or dismounted in about 1 h This added support increases the rigidity of the machine and permits the use of an additional tool head

Planer mills (adjustable rail mills) have been developed from the use of accessory milling and boring heads on planers These machines have various combinations of planing, milling, and boring heads, and they can perform multiple operations on a single workpiece setup

Workpiece Capacity. Both double-housing and open-side planers are available in a wide range of sizes housing planers are rated by width, height, and length, in that order Width refers to the maximum width of workpiece that can pass between the upright housings Height refers to the maximum height of workpiece that can pass under the crossrail when supported on the table Length refers to the maximum stroke Open-side planers are similarly rated with regard to size, except that the width is table width, not maximum workpiece width

Double-Tool Capacity. Although only three tool heads can be used on an open-side planer, and four on a double-housing planer, tool capacity can be increased through the use of special holders that accommodate more than one single-point tool It is common practice to use a roughing tool and a finishing tool in the same head, thus completing a planing operation in one pass instead of two (usually with some sacrifice in surface finish)

For straight planing, the efficiency of the planer can be greatly increased by using double-cutting tools, in special holders

on special heads, which permit planing on both the forward and return strokes of the planer When these tools are used, the speed of the normally noncutting return stroke which on most modern planers is several times greater than that of the forward stroke is of course reduced

Special Accessories. Automatic controls and tracer attachments can be used to improve planing capabilities Many planers are equipped for full control of speed and feed ranges from one suspended station and for automatic rail positioning and leveling Tracer attachments permit the contour planing of such parts as large propeller blades, steam chests, and rocker arms for bridge supports

Grinding and milling accessories can also be mounted in place of one of the rail or side heads At slow feed rates, milling heads provide an increased stock removal rate The use of grinding heads during slow feed rates can improve surface finish

Planing is a rugged cutting operation, and setting up the work is probably the most important aspect This is particularly true for the tandem planing of small or medium-size pieces Serious damage and operator injury can also occur if the workpiece moves during planing

Clamping Hardware. Setup hardware includes planer vises, jackscrews, clamps, and T-slot devices An ample supply

of setup hardware in a wide variety of types and sizes can greatly decrease the time required for setting up large and irregularly shaped workpieces, thus decreasing down-time Inexpensive and seemingly inconsequential items of hardware can often reduce floor-to-floor time For example, special T-slot nuts can be dropped into a 100 mm (4 in.) long cleared section of the slot at the desired location and given a quarter turn, thus eliminating the need to clear chips from the entire slot for loading another workpiece

Cleaning chips from T-slots and stop-pin holes consumes operator time and machine time For example, an operator might spend 40 min planing a workpiece and 30 min picking chips from slots and pin holes before the next workpiece can

be set up This loss of time can be prevented by placing specially cut lengths of hardwood strips in the T-slots, and metal covers on the stop-pin holes These protective devices can be quickly removed to permit loading of the next workpiece

Magnetic Chucks. Cast iron or steel workpieces are often held to planer tables with magnetic chucks Magnetic chucking, however, is reliable only for holding workpieces that have a large table-contact area in relation to height For this reason, holding by means of magnetic chucks is generally restricted to the planing of platelike workpieces To ensure against movement of a workpiece held by magnetic chucking, an end stop should be placed against it counter to the cutting stroke (if double cutting is used, an end stop should be at each end of the work)

Setup Plates. Planing productivity can often be increased through the use of setup plates A setup plate resembles a planer table in length and width, and it has T-slots for mounting the work In production planing, the work is secured to the plate away from the planer, and the assembly is then carried to the planer table and located on it by keys at each end

of the setup plate that fit into the center T-slot in the table When two setup plates are used, one load can be planed while another is being set up a procedure comparable to the use of a duplex table (see below)

Tandem (Gang) Planing. Specially designed fixtures that allow quick loading and unloading can greatly increase productivity in tandem planing However, the cost of such fixtures can rarely be justified, except for continued production

of identical or closed similar workpieces

Duplex Tables. Planers with duplex, or divided, tables allow planing on one half of the table while the other half is being unloaded or reloaded Duplex tables are split crosswise into two sections The two sections can be fastened together and used as one long table, or they can be split for planing shorter workpieces When split, one section of the table can be loaded and set up while work is being planed on the other section This practice greatly increases the productivity of a planer, because in many applications setup time exceeds machining time

Workpiece Setup

Once the workpiece is placed on the table, the first step is to ensure that it rests solidly If there is any wobbling, shim jacking must be used For large workpieces with relatively slender sections, such as some weldments, jacks or blocks should be used to damp vibrations A strap or pin clamp should be used over each jack or block to ensure that the workpiece rests solidly

Platelike Workpieces. When magnetic chucks are not available or when a platelike workpiece does not lend itself to this method of mounting, various clamping devices are used Figure 2 illustrates a common method of securing a long, flat plate to a planer table by using chisel points, T-slot stop blocks, stop pins, guide stops for initial alignment, and an end stop Two precautions must be observed with this method First, the adjusting screws contacting the chisel points must not extend beyond the stop blocks or stop pins by more than the distances suggested in Fig 2 (one or two diameters), or the screws may bend and allow the workpiece to loosen Second, the chisel points must be set at an angle of

8 to 12° (Fig 2)

Fig 2 A common method for securing a long, flat plate to a planer table

Irregularly Shaped Workpieces. A typical method of securing a large, irregular casting to a planer table is illustrated in Fig 3 This setup uses an angle bracket and an outboard support If double-cutting practice were employed,

an angle bracket and two end stop pins would be used at each end of the workpiece For workpieces of this type that are more than 1 or 1.5 m (4 or 5 ft) long, the use of two outboard supports and screw jacks is recommended

Fig 3 Typical arrangement of securing and supporting devices for mounting a large, irregular workpiece on a

planer table

Workpieces for tandem planing must either be tightly butted together (so that the tool cuts continuously for the entire stroke) or separated by 150 to 200 mm (6 to 8 in.) (for a fully interrupted cut) If the workpieces are separated by only 25 to 50 mm (1 to 2 in.), the tool is likely to break, because of deflection by chips lodged between the workpieces or because the sudden release of pressure on the tool shank as the tool emerges from the cut will cause a vibration and allow the tool to enter the next workpiece before becoming fully seated

Other Workpieces. Bases for large presses or diesel engines are usually large rough castings, forgings, or weldments produced one at a time, and planing is often the first operation in machining them Setup of these pieces on a planer is extremely critical because the planed surfaces will be used as a means of locating for subsequent operations

Tool Materials

High-speed steels, cast cobalt-chromium-tungsten alloys, and carbides are used as materials for planer tools High-speed steels and cast alloys are often interchanged In some heavy-duty planing applications, cast alloy tools have proved superior to high-speed steel tools However, high-speed steel tools are used more often for planing

Most planer tools have relatively large cross sections because they are made for maximum rigidity (note the typical planer tool and mounting shown in Fig 4) Because of the size of these tools, it is common practice to make the shank from an alloy steel (such as 4140 or 4340) heat treated for high strength, then use inserts of high-speed steel (brazed or mechanically secured)

Fig 4 Planer tool and method of holding for maximum rigidity

High-Speed Steels. General-purpose high-speed steels such as T1 and M2 have proved satisfactory for many planer tools or cutting edges However, in applications involving hard work metals or heavy cuts, the cobalt types of high-speed steel, such as T6, T15, M6, or M44, will give better tool life These more highly alloyed high-speed steels are generally used as inserts

Carbides. Under conditions of maximum rigidity of machine, tools, and workpiece, carbide tools are more efficient than high-speed steel or cast alloy tools Planing time is often reduced by 50% or more through the use of carbide instead of high-speed steel cutting tools, because cutting stroke speed can be increased up to 90 m/min (300 sfm)

In selecting tool material for planing, however, overall time is a more important consideration than machining time alone

In many applications, setup time is far greater than planing time, and under these conditions, large reductions in planing time have a relatively small effect on total processing time

Before considering the use of carbide tools for planing, it must be ensured that the planer is rigid and in good condition and that it is capable of the high speeds required (90 m/min, or 300 sfm) The rail should be securely clamped to the housing or column, and the head should fit snugly onto the rail The tool box and apron should be free of spring and excessive wear to permit the apron to seat in its clapper box The planer should also be equipped with tool lifters to prevent the carbide tools from dragging or bouncing on the return stroke Sufficient power must be available; in the rough planing of steel with one carbide tool, as much as 70 kW (90 hp) is sometimes required

A shock-resistant type of carbide must be used, regardless of whether it is a straight-tungsten grade for planing gray iron

or a steel-cutting grade Carbides suitable for planing usually contain up to about 16% Co

Carbide planer tools should not be considered for the following:

• Workpieces that limit tool runout to about 75 mm (3 in.); the higher speeds used in carbide planing require a greater runout margin

• Workpieces that require the use of a longitudinal extension on the tool holder for reaching into blind areas (a practice known as poke planing)

• Workpieces that require excessive tool overhang in a vertical plane; as the tool is lowered in the holder, rigidity decreases

• Weldments in which metal hardness at junctions may vary considerably; for this condition, high-speed steel tools operated at slow speed will generally give better results

• Planing of metals that are harder than about 40 HRC; these must be planed at slow speeds, with which

the inherent advantages of carbide tools cannot be realized

Tool Design

Recommended design details for the cutting portions of high-speed steel planer tools are shown in Fig 5 Tools are available in a variety of configurations suited to the undercutting, slotting, and straight planing of either horizontal or vertical surfaces Tools having the small nose radii shown in Fig 5 are preferred for roughing cuts; broad (often as wide

as 38 mm, or 1 in.), flat-nose tools are better for the finishing of most metals

Fig 5 Recommended designs of high-speed steel planer tools

Carbide Roughing Tools. The back rake angle for carbide planer tools ranges from 0 to -15° In general, the more difficult the work metal is to machine, the more negative is the back rake angle A 0° back rake is used for soft metals; -3

to -5° for cast iron, low-carbon steel, and medium-carbon steels; and -5 to -15° for difficult-to-machine steels (such as

4340 alloy steel at 40 HRC) Negative back rake is also sometimes used when planing gummy metals because it aids chip flow and reduces face wear

Side rake angles range from 3 to -15°, also depending on the machinability of the work metal A side rake angle of 3 to 0°

is usually suitable for free-cutting metals, 0° for medium-carbon steels, -3° for gummy metals, and up to -15° for difficult-to-machine steels Excessive negative rake angles should be avoided because they are likely to cause chatter

Side rake, or the land of the tool, is the largest single factor in controlling chip flow The use of optimum side rake eliminates the need for chip breakers This is an advantage because mechanical chip breakers are readily knocked off by the heavy chip produced in planing, and ground-in chip breakers weaken the cutting edge of the tool Chip control is aided by grinding the land into a triangular shape This causes the edge of the chip at the surface line of the cut to curl before the edge of the chip at the tool point, thus flowing the chip toward the side of the tool and back onto the workpiece

The lead, or side cutting edge, angle directly controls chip thickness in relation to feed A 45° lead angle will produce a thin chip, a 10° lead will produce a thicker chip, and a 0° lead will produce a chip equivalent in thickness to the feed used The lead angle should be such that the chip produced is thick enough to take the initial shock away from the cutting edge and yet thin enough to curl property In planing low-carbon steel, a lead angle less than 15° will cause excessive shock, and a lead angle greater than 35° will produce a long, straight chip A lead angle of 23 to 25° is near optimum for many metals, allowing the chip to flow onto the workpiece or against the tool holder and break into small segments However, a lead angle of about 30° is most commonly used to obtain an acceptable chip thickness in roughing

Carbide tools require a comparatively small nose radius to prevent machining stress from focusing at the radial point of the radius and rupturing the carbide A small radius permits heat and stress to flow straight through the tip, causing less chatter A nose radius of 1.6 to 3.2 mm ( to in.) is suitable for cast iron, and a 0.8 mm ( in.) radius for steel

Relief (clearance) angles should vary with the type of material being planed Side and end relief angles of 5° are usually suitable for cast iron For the planing of most steels, it is advisable to strengthen the cutting tool as much as possible by reducing the side clearance angle, thus providing a larger area of carbide for dissipating heat and absorbing shock

Figure 6 shows a type of carbide-insert tool widely used for the rough planing of cast iron and steel When ground to the configuration shown in Fig 6, the tool is best suited for planing cast iron, although tools of this design have been successfully used on brass and aluminum For planing carbon and alloy steels, the design of the tool should be modified

in accordance with the recommendations discussed above

Fig 6 Carbide-insert tool for the rough planing of cast iron

Round or square button-type carbide inserts are also used for rough planing Between regrinds for sharpening, the inserts can be rotated to present new cutting edges, thus allowing greater total tool life Square button inserts can be ground in position Round button inserts 25 mm (1 in.) in diameter and 13 mm ( in.) thick are suitable for depths of cut to 9.5 mm ( in.); for greater depths of cut, inserts 32 mm (1 in.) in diameter and 19 mm ( in.) thick should be used For planing cast iron, 0° back and side rakes and a 6° side relief are satisfactory For planing steel, a -5°, 0.8 mm ( in.) wide land

on the cutting face has proved successful

Finishing Tools. Figure 7 shows a typical broad-nose finishing tool that can also be used for slotting Either a carbide

or a high-speed steel insert can be used in this type of tool As Fig 7 shows, the bottom of the insert is serrated

lengthwise, and the top of the insert is serrated across the width This design permits offsetting the insert to the left or right as needed and provides a rigid lock The cross serration at the top prevents vertical movement of the insert

Fig 7 Typical insert tool for semifinish and finish planing or for slotting

The insert is held in place mechanically by a serrated clamp, which is secured by a socket screw When the cutting edge becomes dull, a new insert can be installed without removing the shank from the tool holder

Gooseneck-holder finishing tools (Fig 8) are primarily intended for use on cast iron, but have been successfully used for the finish planing of other metals Gooseneck tools carry the cutting edge behind center so that the cutter is dragged in cutting It does not dig in or chatter as readily as a cutter that is ahead of center

Fig 8 Gooseneck-holder tool used for light cuts in finish planing Dimensions given in inches

Inserts for gooseneck holders can be made of high-speed steel or carbide, but greater accuracy is obtained with high-speed steel High-speed steel inserts, which are available in widths up to 44 mm (1 in.), should be ground with a slight positive back rake; cutting edges should be honed with an oilstone to obtain maximum sharpness For surfaces that require extreme accuracy (as for fitting to template gages), it is possible with high-speed steel inserts to take cuts of less than 0.025 mm (0.001 in.) on cast iron

Carbide inserts, up to 32 mm (1 in.) wide, are also used in gooseneck holders for producing flat cuts Edges of carbide inserts are not as keen as those of high-speed steel inserts; therefore, carbide inserts should not be used for depths of cut less than 0.05 mm (0.002 in.)

Double-Cutting Tools. Double-cut planing uses both strokes of the planer table for cutting and requires special tool holders mounted to a spindle in the planer head (Fig 9) This spindle oscillates 13° clockwise and places a tool in cutting position for the normal cutting stroke At the completion of the normal cutting stroke, the spindle oscillates 13°

counterclockwise and positions a second tool for cutting on the return stroke of the planer table In addition, a conventional finishing tool can be mounted in the clapper box of the head to semifinish a workpiece simultaneously with the roughing cut This technique is known as triple planing

Fig 9 Tool for double-cut planing

Speed, Feed, and Depth of Cut

Table 1 lists recommended speeds and feeds for various depths of cut in the rough and finish planing of several different metals with high-speed steel or carbide tools The values given in Table 1 are not maximum, but are typical values that have proved consistent with optimum tool life and efficiency of metal removal

Table 1 Recommended speeds and feeds for planing with high-speed steel or carbide tools

Depth of cut: 3.2 mm ( in.)

Depth of cut: 6.4 mm ( in.)

Depth of cut: 13 mm ( in.)

Feed,

mm (in.) per stroke

Speed, m/min (sfm)

Feed,

mm (in.) per stroke

Speed, m/min (sfm)

Feed,

mm (in.) per stroke

Speed, m/min (sfm)

Feed,

mm (in.) per stroke

Finishing speed(a), m/min

(0.060-max

0.075)

(0.06-max

0.090)

(0.060-max

0.090)

(0.090-max

0.125)

(0.090-max

0.100)

(0.090-max

0.090)

(0.060-max

Bronze Soft max

0.150)

(0.090-max

0.125)

(0.090-max

0.125)

(0.090-max

0.100)

(0.090-max

(a) For a depth of cut ranging from 0.08-0.38 mm (0.003-0.015 in.) Finishing feeds at these speeds

depend on the type of tool used Flat-nose tools are used for cast iron and bronze at feeds of 13-25 mm ( in.) per stroke; variations of flat-nose tools are used for steel at feeds of 3.2-13 mm ( - in.) per stroke Round-nose tools are sometimes used at feeds of 1.1-1.5 mm (0.045-0.060 in.), depending on the nose radius and on the finish desired

Minor variables in work metal, tool design, or machine conditions often indicate the need for adjustments in speed, feed,

or both On new jobs, it is often necessary to inspect the tool after a few passes for the following conditions:

• Edge wear, which indicates too much speed or not enough feed

• Face wear, which indicates too much feed or not enough speed

• Redness at the tool point, which may occur in extreme cases of interrupted cutting and which should be kept to a minimum by adjusting speed, feed, or both

In general, it is advisable to plane steel with as heavy a feed and as high a speed as possible, because this promotes good chip flow without the aid of mechanical or ground-in chip breakers A heavy chip will curl and break into small segments better than a thin chip Increased cutting speed maximizes heating of the chip and is the best means to prevent overheating

of the workpiece and the tool Using carbide tools, thin plates have been more successfully planed by increasing the cutting speed from 70 to 90 m/min (225 to 300 sfm), thus transmitting more heat to the chips

Uniform cutting speed and feed should be maintained throughout the entire stroke of the planer It is not necessary to start the cut with a slow speed and a low feed, nor is it advantageous to preheat the tool before beginning a cut

When carbide tools are used for planing medium grades of gray iron ( 200 HB), common practice is to operate at 46 to

53 m/min (150 to 175 sfm) and 2.0 to 2.4 mm ( to in.) feed per stroke with a 13 to 19 mm ( to in.) depth of cut

By decreasing the depth of cut to 9.5 mm ( in.), speed can safely be increased to 55 to 60 m/min (180 to 200 sfm), and feed can be increased to 2.4 to 3.2 mm ( to in.) per stroke

Low-carbon steel can be planed at higher speed than gray iron with carbide tools; 90 m/min (300 sfm) and a feed of 2.4 to 3.2 mm ( to in.) per stroke with 9.5 mm ( in.) depth of cut is common practice Medium-carbon low-alloy steel such as annealed 4130 can be planed at 53 to 60 m/min (175 to 200 sfm), 2.0 mm ( in.) feed, and 9.5 mm ( in.) depth of cut For higher-carbon higher-alloy steels such as 4350, common practice is 30 to 45 m/min (100 to 150 sfm) at 1.2 to 1.6 mm ( to in.) feed and 9.5 mm ( in.) depth of cut Die blocks at about 36 HRC have been planed with carbide tools at 30 m/min (100 sfm), 1.2 mm ( in.) feed per stroke, and 13 mm ( in.) depth of cut Heat-treated die blocks at 46 HRC have been planed with carbide at 4.5 to 6.0 m/min (15 to 20 sfm), 0.8 mm ( in.) feed per stroke, and 6.4 mm ( in.) depth of cut

A carbide tool may break because of side pressure as it makes the last one or two passes on a workpiece To minimize this possibility, on cuts of more than 6.4 mm ( in.) depth it is advisable to reduce the feed to about 1 mm ( or in.) and

to decrease the speed by 50% for four or five strokes before the tool emerges from a cut This will often prevent the breakage caused by pressure on the side clearance portion of the tool from the elastic behavior of the work metal That is, too much feed will deflect the thin flange or remaining portion of the work at the cutting edge of the tool, thus preventing the tool from removing the full amount of metal for which the feed is set As the tool continues through the stroke, the metal flange, with the deflected amount of stock still intact, will spring back to its normal position and rub against the side clearance edge of the tool on the return stroke, thus generating heat by friction Even if this does not cause immediate tool failure, breakout of the steel may be caused when the tool, under automatic feed, overtakes the deflected metal and plows through an oversize flange equivalent to a double or triple feed This will set up intense chatter and cause the tool to chip

Fig 10 Contour planing with a template

Planing Versus Alternative Processes

Broaching or even sawing can be used as an alternative to planing, but milling and grinding are most often the competitive processes The selection of planing in preference to an alternative process is usually based on the following considerations:

• The initial cost of a planer is about half that of a planer-type milling machine for performing the same job

• Because of the lower initial cost of the planer, the burden rate is lower, regardless of whether the machine is used part time or full time

• Certain shapes, such as dovetails and V-sections, are particularly suited to planing

• For some parts, such as large machine tool components, the dimensional accuracy required is obtainable only by planing

• Planing is preferred for bearing surfaces that must be finished by scraping because the surface condition that results is more suitable than that produced by milling

• Because of its versatility, low tooling cost, and short tooling-up time, planing is more economical for low production

Planing Versus Sawing. In some applications, planing and band sawing are competitive operations The following describes an application in which either planing or band sawing could have been used to obtain acceptable results, but planing was used because it was less expensive

Example 1: Planing Versus Gas Cutting Versus Band Sawing for Slitting Steel Plate

Figure 11 shows the setup of a planer for slitting 9.5 mm ( in.) alloy steel plates that were 925 mm (36 in.) wide by 1.8 m (6 ft) long into three 300 mm (12 in.) wide strips Strips were originally produced by band sawing, but this method was slow and costly Gas cutting had been tried, but was rejected because an additional finishing operation was needed to smooth the cut edges As indicated in the table with Fig 11, planing produced the strips in less time than band sawing

Fig 11 Slitting steel plate by planing and comparing with band sawing Dimensions given in inches

Planing Versus Milling. Compared with milling on the basis of volume of metal removed per unit of time, planing is relatively inefficient; metal can be removed about twice as fast by milling as by the most efficient planing method (double-cut) However, the longer setup time required for milling and the more expensive equipment and tooling (for one job, tooling for milling costs fifty times as much as tooling for planing) can be justified only when large quantities of similar parts are to be produced For extremely large workpieces, production is usually low; therefore, planing is the less costly method

Planing is often the most practical approach for machining several surfaces to a given absolute level, as in constructing jig-frame components or machining large, irregular workpieces For such applications, milling would seldom be practical, mainly because only unit production is involved

Cutting Fluids

A flood of cutting fluid is seldom used for planing operations because two of the three functions of cutting fluid (chip disposal and cooling) are less important in planing than in operations such as turning In most planing operations, chips are relatively thick and are thrown clear Therefore, they seldom interfere with successive cutting strokes As chips begin

to pile up on the table or fixtures they should be brushed away The use of compressed air is not recommended, because chips are likely to lodge in the mechanism

In planing, the tool is seldom engaged more than 75% of the time Therefore, cooling of tools and workpieces usually presents no problem In some planing operations, however, cutting fluids will improve dimensional accuracy, finish, and tool life by minimizing the adherence of work metal to the tool When cutting fluids are used, a common practice is to apply the fluid directly to the cutting area with a swab A spray mist of cutting oil diluted with a lower-viscosity oil such

as mineral seal oil is sometimes effective A film of oil mist aids the cutting action and has a mild cooling effect on the tools in planing operations

Shaping and Slotting

Introduction

SHAPING AND SLOTTING are machining processes that remove metal from surfaces through the use of a single-point tool supported by a ram that reciprocates the tool in a linear motion against the workpiece Shaping can be done on machines with either vertical or horizontal rams, while slotting is commonly done on machines with vertical rams

Process Capabilities

Shaping and slotting, although versatile processes with short setup times and relatively inexpensive tools, are comparatively inefficient means of metal removal The cost per cubic inch of metal removed by shaping or slotting may

be as much as five times that for removal by milling or broaching in a given job For this reason, shaping and slotting are generally confined to unit or small-quantity production, as in toolrooms or model shops

As the hardness of the workpiece increases above about 25 HRC, metal removal rate and tool life decrease On the other hand, when the occasion demands, pieces much harder than this can be cut on a shaper Steel hardened to 46 HRC, or even higher (heat-treated die blocks, for example), has been successfully machined by shaping and slotting

Size of the workpiece that can be shaped or slotted is limited by the maximum length of stroke, which for standard shapers or slotters is about 915 mm (36 in.) When surfaces longer than 915 mm (36 in.) must be machined, planing or some other suitable processes used

The usual range of cutting stroke is even less from 150 to 610 mm (6 to 24 in.) Although machines with longer strokes could be built, they would be impractical for most purposes because dimensional accuracy decreases as stroke length increases On even the best-maintained shapers, deviation from dimensional accuracy is about 0.04 mm/m (0.0005 in./ft)

of ram travel

Configuration of Workpiece. Although shaping is most commonly used for machining flat surfaces, the process can also be used to produce contours and a variety of irregular configurations Shaping is sometimes used to machine contours because production quantities are too low to justify the expense of the tooling required for producing the same configurations by milling or broaching In addition, some complex configurations are machined on a shaper because they would be difficult or impossible to produce by milling or broaching for example, deep internal slots and tortuous contours and configurations in blind holes

Because of its versatility and short setup time, shaping is often used for the emergency production of gears, splined shafts, racks, or similar parts It is often possible to produce one or two such parts in a shaper in less time than is required merely

to set up for production on other, alternative equipment with a higher output rate

Machines

Shaping and slotting machines develop cutting action from a straight-line reciprocating motion between the tool and the work The tool is driven forward and recovered by a sliding ram The work is fed at right angles to the direction of the ram stroke in small increments Most shapers have rams that drive the cutting tool in a horizontal direction, but a few shapers have rams that drive the cutting tool in a vertical direction Slotters also operate in a vertical direction In either type of shaper, the workpiece rests on a flat bed, which advances it toward the cutting tool

Horizontal shapers can either be crank driven or operated hydraulically A hydraulic shaper uses a piston and cylinder

to operate the ram However, because of the higher cost of a hydraulic unit, the comparatively low efficiency of the hydraulic drive, and the difficulty in obtaining stroke length accuracy with hydraulic shapers, most horizontal shapers are crank driven

Figure 1 shows a sectional view of a crank-driven horizontal shaper and identifies its important working components The rocker arm is reciprocated by a crankpin mounted on the crank gear The crank mechanism is an application of a Whitworth quick-return mechanism

Fig 1 Sectional view of a crank-driven horizontal shaper

For increased efficiency, shapers are built so that the ram speed in the return stroke is greater than that in the forward, or cutting, stroke This is accomplished as indicated in the rocker-arm cycle illustrated in Fig 2 As shown in Fig 2, 220° of the circle is used for the cutting stroke and only 140° for the return stroke a ratio of approximately 1.6 to 1 This ratio between forward and return strokes is not a fixed ratio; it varies among different designs of machines and with the length

of the stroke

Fig 2 Velocity diagram and rocker-arm cycle for a crank-driven horizontal shaper See text for discussion

Horizontal shapers are furnished with either plain or universal tables The universal table, in conjunction with a swivel vise, provides rotation on all three axes Graduations on all three movements allow angular setups to be made quickly

Horizontal shapers range in size from small bench models with a maximum stroke length of less than 150 mm (6 in.) to large, rugged machines with a maximum stroke of as much as 915 mm (36 in.) On a machine of any size, however, the length of stroke can be varied from its maximum to slightly less than 25 mm (1 in.) for the largest machine and to about 3.2 mm ( in.) for the smallest

Horizontal shapers are commonly provided with powered table feeds ranging from about 0.25 mm (0.010 in.) per stroke (for a machine with a 150 mm, or 6 in., maximum stroke) to 5.00 mm (0.200 in.) per stroke (for a machine with a 915

mm, or 36 in., maximum stroke) Over the same range of machine sizes, vertical power feeds on the tool head will range from about 0.125 to 2.50 mm (0.005 to 0.100 in.) per stroke

Slotters and vertical shapers are very similar and are also much like the horizontal shaper except that the ram operates vertically, rather than horizontally, cutting on the downstroke The slotter, as the name implies, was first developed for cutting slots or keyways The vertical shaper, usually a much smaller version of the slotter, was developed for toolroom work Slotters can have ram strokes up to 1800 mm (72 in.) long Most vertical shapers have strokes of 150

to 300 mm (6 to 12 in.) In these vertical machines, because the ram must be pulled against the force of gravity on its upward stroke, a counterweight is added to equalize the power requirements on the up and down strokes and to enable a smoother action of the machine

Most vertical shapers have a means of adjusting the ram and its guides so that it can be set at an angle as great as 15 ° to the vertical This permits the cutting of proper clearances in dies and similar work Many slotters also have this ram adjustability

Tables on vertical machines can be rotated and can be moved longitudinally or transversely With this degree of flexibility

in direction of feed, a vertical machine can cut almost any type of groove, slot, or keyway

Vertical shaping machines have longitudinal and transverse power feeds ranging from about 0.05 to 2.50 mm (0.002 to 0.100 in.) per stroke for short-stroke machines and up to 3.80 mm (0.150 in.) per stroke for a 915 mm (36 in.) stroke machine Rotary feeds usually range from 0.10 to 4.45 mm (0.004 to 0.175 in.) on a 500 mm (20 in.) circle

The ram speeds of most shapers can be adjusted to provide incremental increases in surface speeds from about 1.5 to

90 m/min (5 to 300 sfm) Speeds are changed by positioning the range and speed levers Typical shapers have four speeds available in each of four ranges; this permits adjustment in order to obtain 16 different speeds within the total speed range

of a given machine Cutting speed in meters per minute is a function of both length of stroke and the number of strokes per minute This relationship is shown quantitatively in Table 1