Cutting Tool Applications Chapter 12: Milling Cutters and Operations

Milling is a process of generating machined surfaces by progressively removing a predetermined amount of material from the workpiece, which is advanced at a relatively slow feedrate to a milling cutter rotating at a comparatively high speed.

A typical milling operation; the on-edge insert design is being used. (Photo by courtesy of Ingersoll Cutting Tool Co.)

High-speed steel (HSS) shell end milling cutter. (Photo by courtesy of Morse Cutting Tools)

A variety of indexable milling cutters. (Photo by courtesy of Ingersoll Cutting Tool Co.)

A face-milling cutter with wedge-clamped indexable inserts. (Photo by courtesy of Iscar Metals Inc.)

Face-milling cutters with indexable inserts and wedge-clamped milling carriages. (Photo by courtesy of Greenleaf Corp.)

Indexable-insert ball-nosed milling cutters using the screw clamping method. (Photo by courtesy of Ingersoll Cutting Tool Co.)

Slotting and face-milling cutters with screw-on indexable inserts. (Photo by courtesy of Duramet Corp.)


The two basic cutting tool types used in metalworking are the single-point and multi-point designs. Fundamentally, they are similar. By grouping a number of single point tools in a circular holder, the milling cutter is created.

Milling is a process of generating machined surfaces by progressively removing a predetermined amount of material from the workpiece, which is advanced at a relatively slow feedrate to a milling cutter rotating at a comparatively high speed. The characteristic feature of the milling process is that each milling cutter tooth removes its share of the stock in the form of small individual chips.

Types of milling cutters
The variety of milling cutters available helps make milling a versatile machining process. Cutters are made in a large range of sizes. Milling cutters are made from High Speed Steel (HSS), others are carbide tipped and many are replaceable or indexable inserts.

Periphery milling cutters — Periphery milling cutters are usually arbor-mounted to perform various operations. Common high-speed steel milling cutters include the staggered tooth cutter, side-milling cutter, plain-milling cutter, single-angle milling cutter, double-angle milling cutter, convex milling cutter, concave milling cutter, and corner-rounded milling cutter.

Light-duty plain mill — A general-purpose cutter for peripheral milling operations. Narrow cutters have straight teeth, while wide ones have helical teeth.

Heavy-duty plain mill — Similar to the light duty mill except that it is used for higher rates of metal removal. To aid it in this function, the teeth are more widely spaced and the helix angle is increased to about 45 degrees.

Side milling cutter — Has a cutting edge on the sides as well as on the periphery. This allows the cutter to mill slots.

Half-side milling cutter — Same as the one previously described except that cutting edges are provided on a single side. It is used for milling shoulders. Two cutters of this type are often mounted on a single arbor for straddle milling.

Stagger-tooth side mill — Same as the side-milling cutter except that the teeth are staggered so that every other tooth cuts on a given side of the slot. This allows deep, heavy-duty cuts to be taken.

Angle cutters — The peripheral cutting edges lie on a cone rather than on a cylinder. A single or double angle may be provided.

Shell endmill — Has peripheral cutting edges plus face cutting edges on one end. It has a hole through it for a bolt to secure it to the spindle.

Form mill — A peripheral cutter whose edge is shaped to produce a special configuration on the surface. One example is the gear tooth cutter. The exact contour of the cutting edge of a form mill is reproduced on the surface of the workpiece.

End-milling cutters — End mills can be used on vertical and horizontal milling machines for a variety of facing, slotting and profiling operations. Solid end mills are made from high-speed steel or sintered carbide. Other types, such as shell end mills and fly cutters, consist of cutting tools that are bolted or otherwise fastened to adapters.

Solid end mills — Solid end mills have two, three, four, or more flutes and cutting edges on the end and the periphery. Two flute end mills can be fed directly along their longitudinal axis into solid material because the cutting faces on the end meet. Three and four fluted cutters with one end cutting edge that extends past the center of the cutter can also be fed directly into solid material.

Solid end mills are double or single ended, with straight or tapered shanks. The end mill can be of the stub type, with short cutting flutes, or of the extra long type for reaching into deep cavities. On end mills designed for effective cutting of aluminum, the helix angle is increased for improved shearing action and chip removal, and the flutes may be polished.

Special end mills — Ball end mills are available in diameters ranging from 1/32 to 2-1/2 in., in single and double-ended types. Single purpose end mills such as Woodruff key-seat cutters, corner rounding cutters, and dovetail cutters are used on both vertical and horizontal milling machines. They are usually made of high-speed steel and may have straight or tapered shanks.

Milling cutter nomenclature — As far as metal cutting action is concerned, the pertinent angles on the tooth are those that define the configuration of the cutting edge, the orientation of the tooth face, and the relief to prevent rubbing on the land.

Outside diameter — The diameter of a circle passing through the peripheral cutting edges. It is the dimension used in conjunction with the spindle speed to find the cutting speed (SFPM).

Root diameter — This diameter is measured on a circle passing through the bottom of the fillets of the teeth.

Tooth — The tooth is the part of the cutter starting at the body and ending with the peripheral cutting edge. Replaceable teeth are called inserts.

Tooth face — The tooth face is the surface between the fillet and the cutting edge, where the chip slides during its formation.

Land — The area behind the cutting edge on the tooth that is relieved to avoid interference is called the land.

Flute — The flute is the space provided for chip flow between the teeth.

Gash angle — The gash angle is measured between the tooth face and the back of the tooth immediately ahead.

Fillet — The fillet is the radius at the bottom of the flute, provided to allow chip flow and chip curling.

The terms defined above apply primarily to milling cutters, particularly to plain milling cutters. In defining the configuration of the teeth on the cutter, the following terms are important.

Peripheral cutting edge — The cutting edge aligned principally in the direction of the cutter axis is called the peripheral cutting edge. In peripheral milling, it is this edge that removes the metal.

Face cutting edge — The face cutting edge is the metal removing edge aligned primarily in a radial direction. In side milling and face milling, this edge actually forms the new surface, although the peripheral cutting edge may still be removing most of the metal. It corresponds to the end cutting edge on single point tools.

Relief angle — This angle is measured between the land and a tangent to the cutting edge at the periphery.

Clearance angle — Is provided to make room for chips, thus forming the flute.

Radial rake angle — The angle between the tooth face and a cutter radius, measured in a plane normal to the cutter axis.

Axial rake angle — Measured between the peripheral cutting edge and the axis of the cutter, when looking radially at the point of intersection.

Blade setting angle — When a slot is provided in the cutter body for a blade, the angle between the base of the slot and the cutter axis is called the blade setting angle.

Indexable milling cutters
There are a variety of clamping systems for indexable inserts in milling cutter bodies.

Wedge clamping— Milling inserts have been clamped using wedges for many years in the cutting tool industry. This principle is generally applied in one of the following ways: either the wedge is designed and oriented to support the insert as it is clamped, or the wedge clamps on the cutting face of the insert, forcing the insert against the milling body. When the wedge is used to support the insert, the wedge must absorb all of the force generated during the cut. This is why wedge clamping on the cutting face of the insert is preferred, since this method transfers the loads generated by the cut through the insert and into the cutter body.

The wedge clamp system however, has two distinct disadvantages. First, the wedge covers almost half of the insert cutting face, thus obstructing normal chip flow while producing premature cutter body wear, and secondly, high clamping forces causing clamping element and cutter body deformation can and often will result. The excessive clamping forces can cause enough cutter body distortion that in some cases when loading inserts into a milling body, the last insert slot will have narrowed to a point where the last insert will not fit into the body. When this occurs, several of the inserts already loaded are removed and reset. Wedge clamping can be used to clamp individual inserts or indexable and replaceable milling cutter cartridges.

Screw clamping— This method of clamping is used in conjunction with an insert that has a pressed countersink or counterbore. A torque screw is often used to eccentrically mount and force the insert against the insert pocket walls.

Screw clamping is excellent for small diameter end mills where space is at a premium. It also provides an open unhampered path for chips to flow free of wedges or any other obstructive hardware. Screw clamping produces lower clamping forces than those attained with the wedge clamping system. However, when the cutting edge temperature rises significantly, the insert frequently expands and causes an undesirable retightening effect, increasing the torque required to unlock the insert screw. The screw clamping method can be used on indexable ball milling cutters or on indexable insert slotting and face milling cutters.

Milling cutter geometry
There are three industry standard milling cutter geometries: double negative, double positive, and positive/ negative. Each has certain advantages and disadvantages that must be considered when selecting the right milling cutter for the job.

Double negative geometry — A double negative milling cutter uses only negative inserts held in a negative pocket. This provides cutting edge strength for roughing and severe interrupted cuts. When determining cutter geometry it is important to remember that a negative insert tends to push the cutter away, exerting considerable force against the workpiece. This could be a problem when machining lightly held workpieces, or when using light machines. However, this tendency to push the work down, or push the cutter away from the workpiece may be beneficial in some cases because the force ends to "load" the system, which often reduces chatter.

Double positive geometry — Double positive cutters use positive inserts held in positive pockets. This is to provide the proper clearance for cutting. Double positive cutter geometry provides for low force cutting, but the inserts contact the workpiece at their weakest point, the cutting edge. In positive rake milling, the cutting forces tend to lift the workpiece or pull the cutter into the work. The greatest advantage of double positive milling is free cutting. Less force is exerted against the workpiece, so less power is required.

Positive/negative geometry — Positive/negative cutter geometry combines positive inserts held in negative pockets. This provides a positive axial Take and a negative radial rake and as with double positive inserts, this provides the proper clearance for cutting. In the case of positive/negative cutters, the workpiece is contacted away from the cutting edge in the radial direction and on the cutting edge in the axial direction. The positive/negative cutter can be considered a low force cutter. In positive/negative milling, some of the advantages of both positive and negative milling are available.

Lead angle — The lead angle is the angle between the insert and the axis of the cutter. Several factors must be considered to determine which lead angle is best for a specific operation. First, the lead angle must be small enough to cover the depth of cut. The greater the lead angle, the less the depth of cut that can be taken for a given size insert. In addition, the part being machined may require a small lead angle in order to clear a portion or form a certain shape on the part.

The lead angle also determines the thickness of the chip. The greater the lead angle for the same feed rate or chip load per tooth, the thinner the chip becomes. As in single point tooling, the depth of cut is distributed over a longer surface of contact. Therefore, lead angle cutters are recommended when maximum material removal is the objective. Thinning the chip allows the feed rate to be increased.

Lead angles can rage from zero to 85 degrees. The most common lead angles available on standard cutters are 0, 15, 30 and 45 degrees. Lead angles larger than 45 degrees are usually considered special.

Milling cutters with large lead angles also have greater heat dissipating capacity. However, if more of the tool can be employed in the cut, as in the case of larger lead angles, the tool's heat dissipating capacity will be improved. Additionally, axial force is increased and radial force is reduced, an important factor in controlling chatter.

Milling insert corner geometry
Indexable insert shape and size were discussed in Chapter 2. Selecting the proper corner geometry is probably the most complex element of insert selection. A wide variety of corner styles are available. The corner style chosen will have a major effect on surface finish and insert cost.

Nose radius — An insert with a nose radius is generally less expensive than a similar insert with any other corner geometry. A nose radius is also the strongest possible corner geometry because it has no sharp corners where two flats come together. For these two reasons alone, a nose radius insert should be the first choice for any application where it can be used.

Inserts with nose radii can offer tool life improvement when they are used in 0 to 15 degree lead angle cutters.

Chamfer — There are two basic ways in which inserts with a corner chamfer can be applied. Depending both on the chamfer angle and the lead angle of the cutter body in which the insert is used, the land of the chamfer will be either parallel or angular (tilted) to the direction of feed.

Inserts that are applied with the chamfer angular to the direction of feed normally have only a single chamfer. These inserts are generally not as strong and the cost is usually higher than inserts that have a large nose radius. Angular-land chamfer inserts are frequently used for general purpose machining with double negative cutters.

Inserts designed to be used with the chamfer parallel to the direction of feed may have a single chamfer, a single chamfer and corner break, a double chamfer, or a double chamfer and corner break. The larger lands are referred to as primary facets and the smaller lands as secondary facets. The cost of chamfers, in relation to other types of corner geometries, depends upon the number of facets. A single facet insert is the least expensive, while multiple facet inserts cost more because of the additional grinding expense.

The greatest advantage or using inserts with the land parallel to the direction of feed is that, when used correctly, they generate an excellent surface finish. When the land width is greater than the advance per revolution, one insert forms the surface. This means that an excellent surface finish normally will be produced regardless of the insert face run-out.

Sweep wipers — Sweep wipers are unique in both appearance and application. These inserts have only one or two very long wiping lands. A single sweep wiper is used in a cutter body filled with other inserts (usually roughing inserts) and is set approximately 0.003 to 0.005 in. higher than the other inserts, so that the sweep wiper alone forms the finished surface.

The finish obtained with a sweep wiper is even better than the excellent finish attained with a parallel land chamfer insert.

Basic milling operations
Before any milling boon is attempted, several decisions must be made. In addition to selecting the best means of holding the work and the most appropriate cutters to be used, the cutting speed and feed rate must be established to provide good balance between rapid metal removal and long tool life.

Proper determination of a cutting speed and feed rate can be made only when the following six factors are known:
• Type of material to tie machined
• Rigidity of the set-up
• Physical strength of the cutter
• Cutting tool material
• Power available at the spindle
• Type of finish desired

Direction of milling feed
The application of the milling tool in terms of its machining direction is critical to the performance and tool life of the entire operation. The two options in milling direction are described as either conventional or climb milling. Conventional and climb milling also affect chip formation and tool life.

Conventional milling — The term often associated with this milling technique is 'up-cut' milling. The cutter rotates against the direction of feed as the workpiece advances toward it from the side where the teeth are moving upward. The separating forces produced between cutter and workpiece oppose the motion of the work. The thickness of the chip at the beginning of the cut is at a minimum, gradually increasing in thickness to a maximum at the end of the cut.

Climb milling — The term often associated with this milling technique is 'down-cut' milling. The cutter rotates in the direction of the feed and the workpiece, therefore advances towards the cutter from the side where the teeth are moving downward. As the cutter teeth begin to cut, forces of considerable intensity are produced which favor the motion of the workpiece and tend to pull the work under the cutter. The chip is at a maximum thickness at the beginning of the cut, reducing to a minimum at the exit. Generally climb milling is recommended wherever possible. With climb milling a better finish is produced and longer cutter life is obtained.

Advantages and disadvantages — If the workpiece has a highly abrasive surface, conventional milling will usually produce better cutter life since the cutting edge engages the work below the abrasive surface. Conventional milling also protects the edge by chipping off the surface ahead of the cutting edge.

Limitations on the use of climb milling are mainly affected by the condition of the machine and the rigidity with which the work is clamped and supported. Since there is a tendency for the cutter to climb up on the work, the milling machine arbor and arbor support must be rigid enough to overcome this tendency. The feed must be uniform and if the machine does not have a backlash eliminator drive, the table gibs should be tightened to prevent the workpiece from being pulled into the cutter. Most present-day machines are built rigidly enough. Older machines can usually be tightened to permit use of climb milling.

The downward pressure caused by climb milling has an inherent advantage in that it tends to hold the work and fixture against the table, and the table against the ways. In conventional milling, the reverse is true and the workpiece tends to be lifted from the table.

George Schneider, Jr., is the author of Cutting Tool Applications, a handbook to machine tool materials, principles, and designs. He is the Professor Emeritus of Engineering Technology at Lawrence Technological University, and former Chairman of the Detroit Chapter of the Society of Manufacturing Engineers.

TAGS: Features
Hide comments

Comments

  • Allowed HTML tags: <em> <strong> <blockquote> <br> <p>

Plain text

  • No HTML tags allowed.
  • Web page addresses and e-mail addresses turn into links automatically.
  • Lines and paragraphs break automatically.
Publish