7-4 GENERAL LATHE OPERATIONS

LATHE SPEEDS, FEEDS, AND DEPTH OF CUTS

General operations on the lathe include straight and shoulder turning, facing, grooving, parting, turning tapers, and cutting various screw threads. Before these operations can be done, a thorough knowledge of the variable factors of lathe speeds, feeds, and depth of cut must be understood. These factors differ for each lathe operation, and failure to use these factors properly will result in machine failure or work damage. The kind of material being worked, the type of tool bit, the diameter and length of the workpiece, the type of cut desired (roughing or finishing), and the working condition of the lathe will determine which speed, feed, or depth of cut is best for any particular operation. The guidelines which follow for selecting speed, feed, and depth of cut are general in nature and may need to be changed as conditions dictate.

Cutting Speeds.

The cutting speed of a tool bit is defined as the number of feet of workpiece surface, measured at the circumference, that passes the tool bit in one minute. The cutting speed, expressed in FPM, must not be confused with the spindle speed of the lathe which is expressed in RPM. To obtain uniform cutting speed, the lathe spindle must be revolved

faster for workplaces of small diameter and slower for workplaces of large diameter. The proper cutting speed for a given job depends upon the hardness of the material being machined, the material of the tool bit, and how much feed and depth of cut is required. Cutting speeds for metal are usually expressed in surface feet per minute, measured on the circumference of the work. Spindle revolutions per minute (RPM) are determined by using the formula:

12 X SFM = RPM
3.1416 X D

Which can be closely approximated as:

4 X SFM = RPM
D

Where:

SFM is the rated surface feet per minute, also expressed as cutting speed.
RPM is the spindle speed in revolutions per minute.
D is the diameter of the work in inches.

To use the formula, simply insert the cutting speed of the metal and the diameter of the workpiece into the formula and you will have the RPM.

Turning a one-half inch piece of aluminum. cutting speed of 200 SFM. would result in the following:

4 X 200 = 1600 RPM
1/2

Table 7-2 ists specific ranges of cutting speeds for turning and threading various materials under normal lathe conditions, using normal feeds and depth of cuts. Note that in Table 7-2 the measurement calculations are in inch and metric measures. The diameter measurements used in these calculations are the actual working diameters that are being machined. and not necessarily the largest diameter of the material. The cutting speeds have a wide range so that the lower end of the cutting speed range can be used for rough cutting and the higher end for finish cutting. If no cutting speed tables are available, remember that, generally. hard materials require a slower cutting speed than soft or ductile materials. Materials that are machined dry. without coolant. require a slower cutting speed than operations using coolant. Lathes that are worn and in poor condition will require slower speeds than machines that are in good shape. If carbide-tipped tool bits are being used, speeds can be increased two to three times the speed used for high­speed tool bits.

Table 7-2. Cutting speeds for straight turning and threading with HSS too bits.

Feed

Feed is the term applied to the distance the tool bit advances along the work for each revolution of the lathe spindle. Feed is measured in inches or millimeters per revolution, depending on the lathe used and the operator’s system of measurement. Table 7-3 in Appendix A is a guide that can be used to select feed for general roughing and finishing operations. A light feed must be used on slender and small workplaces to avoid damage. If an irregular finish or chatter marks develop while turning. reduce the feed and check the tool bit for alignment and sharpness. Regardless of how the work is held in the lathe, the tool should feed toward the headstock. This results in most of the pressure of the cut being put on the work holding device. If the cut must be fed toward the tailstock. use light feeds and light cuts to avoid pulling the workpiece loose.

Depth of Cut

Depth of cut is the distance that the tool bit moves into the work. usually measured in thousandths of an inch or in millimeters. General machine practice is to use a depth of cut up to five times the rate of feed, such as rough cutting stainless steel using a feed of 0.020 inch per revolution and a depth of cut of 0.100 inch. which would reduce the diameter by 0.200 inch. If chatter marks or machine noise develops, reduce the depth of cut.

MICROMETER COLLAR

Graduated micrometer collars can be used to accurately measure this tool bit movement to and away from the lathe center axis (Figure 7-45). Thus. the depth of cut can be accurately measured when moving the tool bit on the cross slide by using the cross slide micrometer collar. The compound rest is also equipped with a micrometer collar. These collars can measure in inches or in millimeters, or they can be equipped with a dual readout collar that has both. Some collars measure the exact tool bit movement. while others are designed to measure the amount of material removed from the workpiece (twice the tool bit movement). Consult the operator’s instruction manual for specific information on graduated collar use.

Figure 7-45. Graduated micrometer collar.

FACING

Facing is machining the ends and shoulders of a piece of stock smooth. flat, and perpendicular to the lathe axis. Facing is used to cut work to the desired length and to produce a surface from which accurate measurements may be taken.

Facing Work in a Chuck

Facing is usually performed with the work held in a chuck or collet. Allow the workpicce to extend a distance no more than 1 1/2 times the work diameter from the chuck jaws. and use finishing speeds and feeds calculated using the largest diameter of the workpiece. The tool bit may be fed from the outer edge to the center or from the center to the outer edge. Normal facing is done from the outer edge to the center since this method permits the operator to observe the tool bit and layout line while starting the cut. This method also eliminates the problem of feeding the tool bit into the solid center portion of the workpiece to get a cut started.. Use a left-hand finishing tool bit and a right-hand tool holder when facing from the outer edge toward the center. Work that has a drilled or bored hole in the center may be faced from the center out to the outer edge if a right-hand finishing tool bit is used. Avoid excessive tool holder and tool bit overhang when setting up the facing operation. Set the tool bit exactly on center to avoid leaving a center nub on the workpiece (Figure 7-46 ). Use the tailstock center point as a reference point when setting the tool bit exactly on center. If no tailstock center is available, take a trial cut and readjust as needed. If using the cross slide power feed to move the tool bit (into the center), disengage power when the tool bit is within l/16 inch of the center and finish the facing cut using hand feed.

Figure 7-46. Positioning tool bit for facing.

Facing Work Between Centers

Sometimes the workpiece will not fit into a chuck or collet, so facing must be done between centers. To properly accomplish facing between centers, the workpiece must be center-drilled before mounting into the lathe. A half male center (with the tip well lubricated with a white lead and oil mixture) must be used in the lathe tailstock to provide adequate clearance for the tool bit. The tool bit must be ground with a sharp angle to permit facing to the very edge of the center drilled hole (Figure 7-47). Start the facing cut at the edge of the center-drilled hole after checking for tool bit clearance, and feed the cutting tool out to the edge. Use light cuts and finishing feeds, which will reduce the tension put on the half male center. Replace the half male center with a standard center after the facing operation, since the half male center will not provide adequate support for general turning operations. Only a small amount of material can be removed while facing between centers. If too much material is removed, the center-drilled hole will become too small to support the workpiece.

Figure 7-47. Facing using a side finishing tool and a half-male center.

Precision Facing

Special methods must be used to face materials to a precise length. One method is to mount the work in a chuck and lightly face one end with a cleanup cut. Then, reverse the stock and face it to the scribed layout line. This method may not be as accurate as other methods, but it will work for most jobs. A more precise method to face a piece of stock to a specified length is to turn the compound rest to an angle of 30 degrees to the cross slide and then use the graduated micrometer collar to measure tool bit movement, Figure 7-48. At this angle of the compound rest, the movement of the cutting tool will always be half of the reading of the graduated collar. Thus, if the compound rest feed is turned 0.010 inch, the tool bit will face off 0.005 inch of material. With the compound rest angled at 30°, a light cut may be made on the first end, then the piece reversed and faced to accurate length. Always lock the carriage down to the bed. This provides the most secure and accurate base for the cutting tool and helps eliminate unwanted vibration during facing operations. Another way to face to a precise length is to use the lathe carriage micrometer stop to measure the carriage and tool bit movement. Using the micrometer stop can sometimes be faster and easier than using the compound rest graduated collar for measuring tool bit movement.

Figure 7-48. Facing using a graduated micrometer
collar to measure bit movement.

STRAIGHT TURNING

Straight turning, sometimes called cylindrical turning, is the process of reducing the work diameter to a specific dimension as the carriage moves the tool along the work. The work is machined on a plane parallel to its axis so that there is no variation in the work diameter throughout the length of the cut. Straight turning usually consists of a roughing cut followed by a finishing cut. When a large amount of material is to be removed, several roughing cuts may need to be taken. The roughing cut should be as heavy as the machine and tool bit can withstand. The finishing cut should be light and made to cut to the specified dimension in just one pass of the tool bit. When using power feed to machine to a specific length, always disengage the feed approximately 1/16-inch away from the desired length dimension, and then finish the cut using hand feed.

Setting Depth of Cut

In straight turning, the cross feed or compound rest graduated collars are used to determine the depth of cut, which will remove a desired amount from the workpiece diameter. When using the graduated collars for measurement, make all readings when rotating the handles in the forward direction. The lost motion in the gears, called backlash, prevents taking accurate readings when the feed is reversed. If the feed screw must be reversed, such as to restart a cut, then the backlash must be taken up by turning the feed screw handle in the opposite direction until the movement of the screw actuates the movement of the cross slide or compound rest. Then turn the feed screw handle in the original or desired direction back to the required setting. -

Setting Tool Bit for Straight Turning

See Figure 7-49. For most straight turning operations, the compound rest should be aligned at an angle perpendicular to the cross slide, and then swung 30° to the right and clamped in position. The tool post should be set on the left-hand side of the compound rest T-slot, with a minimum of tool bit and tool holder overhang.

Figure 7-49. Setup for straight turning.

When the compound rest and tool post are in these positions, the danger of running the cutting tool into the chuck or damaging the cross slide are minimized. Position the roughing tool bit about 5° above center height for the best cutting action. This is approximately 3/64-inch above center for each inch of the workpiece diameter. The finishing tool bit should be positioned at center height since there is less torque during finishing. The position of the tool bit to the work should be set so that if anything occurs during the cutting process to change the tool bit alignment, the tool bit will not dig into the work, but instead will move away from the work. Also, by setting the tool bit in this position, chatter will be reduced. Use a right-hand turning tool bit with a slight round radius on the nose for straight turning. Always feed the tool bit toward the headstock unless turning up to an inside shoulder. Different workplaces can be mounted in a chuck, in a collet, or between centers. Which work holding device to use will depend on the size of the work and the particular operation that needs to be performed.

Turning Work Between Centers

Turning work that is held between centers is one accurate method that is available. The chief advantage of using this method is that the work can be removed from the lathe and later replaced for subsequent machining operations without disturbing the trueness of the turned surface in relation to the center holes of the workpiece. The lathe centers must be in good condition and carefully aligned if the turning operation is to be accurate. If necessary, true the centers and realign as needed. After the workpiece is center-drilled, place a lathe dog (that is slightly larger in diameter than the workpiece) on the end of the work that will be toward the headstock, and tighten the lathe dog bolt securely to the workpiece). If using a dead center in the tailstock, lubricate the center with a mixture of white lead and motor oil. A ball bearing live center is best for the tailstock center since this center would not need lubrication and can properly support the work. Extend the tailstock spindle out about 3 inches and loosen the tailstock clamp-down nut. Place the work with the lathe dog end on the headstock live center and slide the tailstock forward until the tailstock center will support the work; then, secure the tailstock with the clamp-down nut. Adjust the tail of the lathe dog in the drive plate slot, making sure that the tail does not bind into the slot and force the work out of the center. A good fit for the lathe dog is when there is clearance at the top and bottom of the drive plate slot on both sides of the lathe dog tail. Tension should be applied to hold the work in place, but not so much tension that the tail of the lathe dog will not move freely in the drive -plate slot.

Check tool bit clearance by moving the tool bit to the furthest position that can be cut without running into the lathe dog or the drive plate. Set the lathe carriage stop or micrometer carriage stop at this point to reference for the end of the cut and to protect the lathe components from damage. Set the speed, feed, and depth of cut for a roughing cut and then rough cut to within 0.020 inch of the final dimension. Perform a finish cut, flip the piece over, and change the lathe dog to the opposite end. Then rough and finish cut the second side to final dimensions.

Turning Work in Chucks

Some work can be machined more efficiently by using chucks, collets, mandrels, or faceplates to hold the work. Rough and finish turning using these devices is basically the same as for turning between centers. The workpiece should not extend too far from the work holding device without adequate support. If the work extends more than three times the diameter of the workpiece from the chuck or collet, additional support must be used such as a steady rest or a tailstock center support. When turning using a mandrel or faceplate to hold an odd-shaped workpiece, use light cuts and always feed the cutting tool toward the headstock. Every job may require a different setup and a different level of skill. Through experience, each machine operator will learn the best methods for holding work to be turned.

MACHINING SHOULDERS, CORNERS, UNDERCUTS, GROOVES, AND PARTING

Shoulders

Frequently, it will be necessary to machine work that has two or more diameters in its length. The abrupt step, or meeting place, of the two diameters is called a shoulder. The workpiece may be mounted in a chuck, collet, or mandrel, or between centers as in straight turning. Shoulders are turned, or formed, to various shapes to suit the requirements of a particular part. Shoulders are machined to add strength for parts that are to be fitted together, make a corner, or improve the appearance of a part. The three common shoulders are the square, the filleted, and the angular shoulder (Figure 7-50).

Figure 7-50.   Common shoulders

Square shoulders are used on work that is not subject to excessive strain at the corners. This shape provides a flat clamping surface and permits parts to be fitted squarely together. There are many different ways to accurately machine a square shoulder. One method is to use a parting tool bit to locate and cut to depth the position of the shoulder. Straight­tuming the diameter down to the desired size is then the same as normal straight turning. Another method to machine a square shoulder is to rough out the shoulder slightly oversize with a round-nosed tool bit, and then finish square the shoulders to size with a side-finishing tool bit. Both of these methods are fine for most work, but may be too time-consuming for precise jobs. Shoulders can be machined quickly and accurately by using one type of tool bit that is ground and angled to straight turn and face in one operation (Figure 7-51).

Figure 7-51.  Straight and shoulder turning in one pass.

Set up the micrometer carriage stop to align the shoulder dimension; then, in one pass of the tool bit, feed the tool bit left to turn the smaller diameter until contact is made with the carriage stop. Change the direction to feed out from center and face the shoulder out to the edge of the workpiece. The lathe micrometer stop measures the length of the shoulder and provides for a stop or reference for the tool bit. Shoulder turning in this manner can be accomplished with a few roughing cuts and a finishing cut.

Filleted Shoulders

Filleted shoulders or comers, are rounded to be used on parts which require additional strength at the shoulder. These shoulders are machined with a round-nose tool bit or a specially formed tool bit (Figure 7-52). This type of shoulder can be turned and formed in the same manner as square shoulders. Filleted corners are commonly cut to double-sided shoulders (see Undercuts).

Figure 7-52.  Cutting a filleted corner.

Angular Shoulders

Angular shoulders although not as common as filleted shoulders, are sometimes used to give additional strength to corners, to eliminate sharp corners, and to add to the appearance of the work. Angular shoulders do not have all the strength of filleted corners but are more economical to

produce due to the simpler cutting tools. These shoulders are turned in the same manner as square shoulders by using a side turning tool set at the desired angle of the shoulder, or with a square-nosed tool set straight into the work (Figure 7-53).

Figure 7-53.  Two different tools for cutting angular shoulders.

Corners

Corners are turned on the edges of work to break down sharp edges and to add to the general appearance of the work. Common types of corners are chamfered, rounded, and square (Figure 7-54). Chamfered (or angular) corners may be turned with the side of a turning tool or the end of a square tool bit, as in angular shoulder turning. Round corners are produced by turning a small radius on the ends of the work. The radius may be formed by hand manipulation of the cross slide and carriage using a turning tool. An easier method is to use a tool bit specifically ground for the shape of the desired corner. Still another method is to file the radius with a standard file. A square corner is simply what is left when making a shoulder, and no machining is needed.

Figure 7-54.  Corners.

Undercuts

Undercuts are the reductions in diameter machined onto the center portion of workplaces (Figure 7-55) to lighten the piece or to reduce an area of the part for special reasons, such as holding an oil seal ring. Some tools, such as drills and reamers, require a reduction in diameter at the ends of the flutes to provide clearance or runout for a milling cutter or grinding wheel. Reducing the diameter of a shaft or workpiece at the center with filleted shoulders at each end may be accomplished by the use of a round-nosed turning tool bit. This tool bit may or may not have a side rake angle, depending on how much machining needs to be done. A tool bit without any side rake is best when machining in either direction. Undercutting is done by feeding the tool bit into the workpiece while moving the carriage back and forth slightly. This prevents gouging and chatter occurring on the work surface.

Figure 7-55.  Machining an undercut.

Grooves

Grooving (or necking) is the process of turning a groove or furrow on a cylinder, shaft, or workpiece. The shape of the tool and the depth to which it is fed into the work govern the shape and size of the groove. The types of grooves most commonly used are square, round, and V-shaped (Figure 7- 56). Square and round grooves are frequently cut on work to provide a space for tool runout during subsequent machining operations, such as threading or knurling. These grooves also provide a clearance for assembly of different parts. The V-shaped groove is used extensively on step pulleys made to fit a V-type belt. The grooving tool is a type of forming tool. It is ground without side or back rake angles and set to the work at center height with a minimum of overhang. The side and end relief angles are generally somewhat less than for turning tools.

Figure 7-56.  Common grooves.

In order to cut a round groove of a definite radius on a cylindrical surface, the tool bit must be ground to fit the proper radius gage (Figure 7-57). Small V-grooves may be machined by using a form tool ground to size or just slightly undersize. Large V-grooves may be machined with the compound rest by finishing each side separately at the desired angle. This method reduces tool bit and work contact area, thus reducing chatter, gouging, and tearing. Since the cutting surface of the tool bit is generally broad, the cutting speedmust be slower than that used for general turning. A good guide is to use half of the speed recommended for normal turning. The depth of the groove, or the diameter of the undercut, may be checked by using outside calipers or by using two wires and an outside micrometer (Figure 7-58).

Figure 7-57.  Checking tool bit with a radius gage.

 

Figure 7-58. Checking the depth of a groove.

When a micrometer and two wires are used. the micrometer reading is equal to the measured diameter of the groove plus two wire diameters. To calculate measurement over the wires, use the following formula:

Measurement = Outside Diameter+ (2 x wires) – 2 x radius).

Parting

Parting is the process of cutting off a piece of stock while it is being held in the lathe. This process uses a specially shaped tool bit with a cutting edge similar to that of a square-nosed tool bit. When parting. be sure to use plenty of coolant, such as a sulfurized cutting oil (machine cast iron dry). Parting tools normally have a 5° side rake and no back rake angles. The blades are sharpened by grinding the ends only. Parting is used to cut off stock. such as tubing. that is impractical to saw off with a power hacksaw.

Parting is also used to cut off work after other machining operations have been completed (Figure 7-59). Parting tools can be of the forged type. inserted blade type. or ground from a standard tool blank. In order for the tool to have maximum strength, the length of the cutting portion of the blade should extend only enough to be slightly longer than half of the workpiece diameter (able to reach the center of the work).

Figure 7-59.  Parting.

Work that is to be parted should be held rigidly in or collet, with the area to be parted as close to the device as possible. Always make the parting cut at angle to the centerline of the work. Feed the tool bit into the revolving work with the cross slide until the tool completely severs the work. Speeds for parting should be about half that used for straight turning. Feeds should be light but continuous. If chatter occurs. decrease the feed and speed. and check for loose lathe parts or a loose setup. The parting tool should be positioned at center height unless cutting a piece that is over 1-inch thick. Thick pieces should have the cutting tool just slightly above center to account for the stronger torque involved in parting. The length of the portion to be cut off can be measured by using the micrometer carriage stop or by using layout lines scribed on the workpiece. Always have the carriage locked down to the bed to reduce vibration and chatter. Never try to catch the cutoff part in the hand; it will be hot and could burn.

RADII AND FORM TURNING

Occasionally, a radius or irregular shape must be machined on the lathe. Form turningjs the process of machining radii and these irregular shapes. The method used to form-turn will depend on the size and shape of the object. the accuracy desired. the time allowed. and the number of pieces that need to be formed. Of the several ways to form-turn. using a form turning tool that is ground to the shape of the desired radius is the most common. Other common methods are using hand manipulation and filing, using a template and following rod, or using the compound rest and tool to pivot and cut. Two radii are cut in form turning, concave and convex. A concave radius curves inward and a convex radius curves outward.

Forming a Radius Using a Form Turning Tool

Using a form turning tool to cut a radius is a way to form small radii and contours that will fit the shape of the tool. Forming tools can be ground to any desired shape or contour (Figure 7-60), with the only requirements being that the proper relief and rake angles must be ground into the tool’s shape. The most practical use of the ground forming tool is in machining several duplicate pieces, since the machining of one or two pieces will not warrant the time spent on grinding the form tool. Use the proper radius gage to check for correct fit. A forming tool has a lot of contact with the work surface, which can result in vibration and chatter. Slow the speed, increase the feed, and tighten the work setup if these problems occur.

Figure 7-60.  Forming tools.

Forming a Radius Using Hand Manipulation

Hand manipulation, or free hand, is the most difficult method of form turning to master. The cutting tool moves on an irregular path as the carriage and cross slide are simultaneously manipulated by hand. The desired form is achieved by watching the tool as it cuts and making small adjustments in the movement of the carriage and cross slide. Normally, the right hand works the cross feed movement while the left hand works the carriage movement. The accuracy of the radius depends on the skill of the operator. After the approximate radius is formed, the workpiece is filed and polished to a finished dimension.

Forming a Radius Using a Template

To use a template with a follower rod to form a radius, a full scale form of the work is laid out and cut from thin sheet metal. This form is then attached to the cross slide in such a way that the cutting tool will follow the template. The accuracy of the template will determine the accuracy of the workpiece. Each lathe model has a cross slide and carriage that are slightly different from one another, but they all operate in basically the same way. A mounting bracket must be fabricated to hold the template to allow the cutting tool to follow its shape. This mounting bracket can be utilized for several different operations, but should be sturdy enough for holding clamps and templates. The mounting bracket must be positioned on the carriage to allow for a follower (that is attached to the cross slide) to contact the template and guide the cutting tool. For this operation, the cross slide must be disconnected from the cross feed screw and hand pressure applied to hold the cross slide against the follower and template. Rough-cut the form to the approximate shape before disconnecting the cross feed screw. This way, a finish cut is all that is required while applying hand pressure to the cross slide. Some filing may be needed to completely finish the work to dimension.

Forming a Radius Using the Compound Rest

To use the compound rest and tool to pivot and cut (Figure 7-61), the compound rest bolts must be loosened to allow the compound rest to swivel. When using this method, the compound rest and tool are swung from side to side in an arc. The desired radius is formed by feeding the tool in or out with the compound slide. The pivot point is the center swivel point of the compound rest. A concave radius can be turned by positioning the tool in front of the pivot point, while a convex radius can be turned by placing the tool behind the pivot point. Use the micrometer carriage stop to measure precision depths of different radii.

Figure 7-61.  Pivots of the compound radius.

TAPER TURNING

When the diameter of a piece changes uniformly from one end to the other, the piece is said to be tapered. Taper turning as a machining operation is the gradual reduction in diameter from one part of a cylindrical workpiece to another part, Tapers can be either external or internal. If a workpiece is tapered on the outside, it has an external taper; if it is tapered on the inside, it has an internal taper. There are three basic methods of turning tapers with a lathe. Depending on the degree, length, location of the taper (internal or external), and the number of pieces to be done, the operator will either use the compound rest, offset the tailstock, or use the taper attachment. With any of these methods the cutting edge of the tool bit must be set exactly on center with the axis of the workpiece or the work will not be truly conical and the rate of taper will vary with each cut.

Compound Rests

The compound rest is favorable for turning or boring short, steep tapers, but it can also be used for longer, gradual tapers providing the length of taper does not exceed the distance the compound rest will move upon its slide. This method can be used with a high degree of accuracy, but is somewhat limited due to lack of automatic feed and the length of taper being restricted to the movement of the slide.

The compound rest base is graduated in degrees and can be set at the required angle for taper turning or boring. With this method, it is necessary to know the included angle of the taper to be machined. The angle of the taper with the centerline is one-half the included angle and will be the angle the compound rest is set for. For example, to true up a lathe center which has an included angle of 60°, the compound rest would be set at 30° from parallel to the ways (Figure 7-41).

If there is no degree of angle given for a particular job, then calculate the compound rest setting by finding the taper per inch, and then calculating the tangent of the angle (which is the: compound rest setting) .

Figure 7-62. Taper problem.

For example, the compound rest setting for the workpiece shown in Figure 7-62 would be calculated with these two formulas:

TPI = D – d
L

Where:

TPI = taper per inch
D = large diameter
d = small diameter
L = length of taper
 

angle = tan(TPI/2)

Where:

angle = compound rest setting in degrees
tan = the tangent function
TPI = taper per inch

The problem is actually worked out by substituting numerical values for the letter variables:

TPI = D – d = 1.000 - 0.375 = 0.625 = 0.833
L 0.750 0.750

angle = tan(TPI/2) = tan(0.833/2) = tan (0.41650)

Using a handheld calculator, you will see that  tan(0.41650) = 22º 37'.
So the angle is 22 degrees and 37 minutes.

To machine the taper shown in Figure 7-62, the compound rest will be set at 22° 37’. Since the base of the compound rest is not calibrated in minutes, the operator will set the base to an approximate degree reading, make trial cuts, take measurements, and readjust as necessary to obtain the desired angle of taper. The included angle of the workpiece is double that of the tangent of angle (compound rest setting). In this case, the double of 22° 37’ would equal the included angle of 45°14’.

To machine a taper by this method, the tool bit is set on center with the workpiece axis. Turn the compound rest feed handle in a counterclockwise direction to move the compound rest near its rear limit of travel to assure sufficient traverse to complete the taper. Bring the tool bit into position with the workpiece by traversing and cross-feeding the carriage. Lock the carriage to the lathe bed when the tool bit is in position. Cut from right to left, adjusting the depth of cut by moving the cross feed handle and reading the calibrated collar located on the cross feed handle. feed the tool bit by hand-turning the compound rest feed handle in a clockwise direction.

Offsetting the Tailstock

The oldest and probably most used method of taper turning is the offset tailstock method. The tailstock is made in two pieces: the lower piece is fitted to the bed, while the upper part can be adjusted laterally to a given offset by use of adjusting screws and lineup marks (Figure 7-63).

Figure 7-63.  Tailstock offset for taper turning.

Since the workpiece is mounted between centers, this method of taper turning can only be used for external tapers. The length of the taper is from headstock center to tailstock center, which allows for longer tapers than can be machined using the compound rest or taper attachment methods.

The tool bit travels along a line which is parallel with the ways of the lathe. When the lathe centers are aligned and the workpiece is machined between these centers, the diameter will remain constant from one end of the piece to the other. If the tailstock is offset, as shown in Figure 7-64, the centerline of the workpiece is no longer parallel with the ways; however, the tool bit continues its parallel movement with the ways, resulting in a tapered workpiece. The tail stock may be offset either toward or away from the operator. When the offset is toward the operator, the small end of the workpiece will be at the tailstock with the diameter increasing toward the headstock end.

Figure 7-64. Taper turning with tailstock set over.

The offset tailstock method is applicable only to comparatively gradual tapers because the lathe centers, being out of alignment, do not have full bearing on the workpiece. Center holes are likely to wear out of their true positions if the lathe centers are offset too far, causing poor results and possible damage to centers.

The most difficult operation in taper turning by the offset tailstock method is determining the proper distance the tailstock should be moved over to obtain a given taper. Two factors affect the amount the tailstock is offset: the taper desired and the length of the workpiece. If the offset remains constant, workplaces of different lengths, or with different depth center holes, will be machined with different tapers (Figure 7-65).

Figure 7-65. Effect of fixed amount of setover with
different lengths of workpieces.

The formula for calculating the tailstock offset when the taper is given in taper inches per foot (tpf) is as follows:

Offset = TPF x L
24

Where:

Offset = tailstock offset (in inches)
TPF = taper (in inches per foot)
L = length of taper (in feet) measured along the axis of the workpiece

For example, the amount of offset required to machine a bar 42 inches (3.5 feet) long with a taper of 1/2 inch per foot is calculated as follows:

Offset = 1/2 X 42 =  21 = 0.875 inch
24 24
 

Therefore, the tailstock should be offset 0.875 inch to machine the required taper. The formula for calculating the tailstock offset when the taper is given in TPF is as follows:

OFFSET = TPI X L

2

Where OFFSET = tailstock offset TPI = taper per inch

L = length of taper in inches

For example, the amount of offset required to machine a bar 42 inches long with a taper of 0.0416 TPI is calculated as follows:

OFFSET = TPI X L

2

OFFSET = 0.0416 x 42

2

OFFSET = 1.7472 or rounded up 1.75 2 2

OFFSET = .875 inch

Therefore, the tailstock should be offset 0.875 inch to machine the required taper.

If the workpiece has a short taper in any par of it’s length and the TPI or TPF is not given. use the following formula:

OFFSET = L X (D-d)

2 X L1

Where :

D = Diameter of large end d = Diameter of small end

L = Total length of workpiece in inches diameter (in inches)

L1 = Length of taper

For example, the amount of tailstock offset required to machine a bar 36 inches (3 feet) in length for a distance of 18 inches (1.5 feet) when the large diameter is 1 3/4 (1 .750)

inches and the small diameter is 1 1/ 2 (1.5) inches is calculated as follows

OFFSET = L X (D-d)-

2XL1

OFFSET =36 X (1.750 - 1.5)

36

OFFSET =36 X 0.25

36

OFFSET = 9/36 OFFSET = 0.25 inch

Therefore, the tailstock would be offset (toward the operator) 0.25 inch to machine the required taper.

 

Figure 7-66.

Metric tapers can also be calculated for taper turning by using the offset tailstock method. Metric tapers are expressed as a ratio of 1 mm per unit of length. Figure 7-66 shows how the work would taper 1 mm in a distance of 20 mm. This taper would then be given as a ratio of 1:20 and would be annotated on small diameter (d) will be 1 mm greater (d + ). Refer to the following formula for calculating the dimensions of a metric taper. If the small diameter (d), the unit length of taper (k), and the total length of taper (1) are known, then the large diameter (D) may be calculated. The large diameter (D) will be equal to the small diameter plus the amount of taper. The amount of taper for the unit length (k) is (d + 1) - (d). Therefore, the amount of taper per millimeter of unit length = (l/ k). The total amount of taper will be the taper per millimeter (l/ k) multiplied by the total length of taper (l).

For example, to calculate for the large diameter D for a 1:30

taper having a small diameter of 10 mm and a length of 60 mm, do the following:

Since the taper is the ratio 1:30, then (k)= 30, since 30 is the unit of length.

Thus, to determine the tailstock offset in millimeters for the taper in Figure 7-67, substitute the numbers and solve for the offset. Calculate the tailstock offset required to turn a 1:50 taper 200 mm long on a workpiece 800 mm long. The small diameter of the tapered section is 49 mm.

 

Figure 7-67.

The tailstock would be moved toward the operator 8 mm.

Tailstock offset is calculated as follows:

D = large diameter d = small diameter

I = length of taper

L = length of the workpiece

Another important consideration in calculating offset is the distance the lathe centers enter the workpiece. The length of the workpiece (L) should be considered as the distance between the points of the centers for all offset computations.

Therefore, if the centers enter the workpiece 1/8 inch on each end and the length of the workpiece is 18 inches, subtract 1/4 inch from 18 inches and compute the tailstock offset using 17 3/4 inches as the workpiece length (L).

The amount of taper to be cut will govern the distance the top of the tailstock is offset from the centerline of the lathe. The tailstock is adjusted by loosening the clamp nuts, shifting the upper half of the tailstock with the adjusting screws, and then tightening them in place.

There are several methods the operator may use to measure the distance the tailstock has been offset depending upon the accuracy desired (Figure 7-68 ).

 

Figure 7-68.

One method is to gage the distance the lineup marks on the rear of the tailstock have moved out of alignment. This can be done by using a 6-inch rule placed near the lineup marks or by transferring the distance between the marks to the rule’s surface using a pair of dividers.

Another common method uses a rule to check the amount of offset when the tailstock is brought close to the headstock.

Where accuracy is required, the amount of offset may be measured by means of the graduated collar on the cross feed screw. First compute the amount of offset; next, set the tool holder in the tool post so the butt end of the holder faces the tailstock spindle. Using the cross feed, run the tool holder in by hand until the butt end touches the tailstock spindle. The

pressure should be just enough to hold a slip of paper placed between the tool holder and the spindle. Next, move the cross slide to bring the tool holder toward you to remove the backlash. The reading on the cross feed micrometer collar may be recorded, or the graduated collar on the cross feed screw may be set at zero. Using either the recorded reading or the zero setting for a starting point, bring the cross slide toward you the distance computed by the offset. Loosen and offset the tailstock until the slip of paper drags when pulled between the tool holder and the spindle. Clamp the tailstock to the lathe bed.

Another and possibly the most precise method of measuring the offset is to use a dial indicator. The indicator is set on the center of the tailstock spindle while the centers are still aligned. A slight loading of the indicator is advised since the first 0.010 or 0.020 inches of movement of the indicator may be inaccurate due to mechanism wear causing fluctuating readings. Load the dial indicators follows: Set the bezel to zero and move tailstock towards the operator the calculated Famount. Then clamp the tailstock to the way.

Whichever method is used to offset the tailstock, the offset must still be checked before starting to cut. Set the dial indicator in the tool post with its spindle just barely touching far right side of the workpiece. Then, rotate the carriage toward the headstock exactly I inch and take the reading from the dial indicator. One inch is easily accomplished using the thread chasing dial. It is 1 inch from one number to another.

Alternatively, 1 inch can be drawn out on the workpiece. The dial indicator will indicate the taper for that 1 inch and, if needed, the tailstock can be adjusted as needed to the precise taper desired. If this method of checking the taper is not used, then an extensive trial and error method is necessary.

To cut the taper, start the rough turning at the end which will be the small diameter and feed longitudinally toward the large end (Figure 7-64). The tailstock is offset toward the operator and the feed will be from right to left. The tool bit, a right-hand turning tool bit or a round-nose turning tool bit, will have its cutting edge set exactly on the horizontal centerline of the workpiece, not above center as with straight turning

Taper Attachment

Figure 7-69.  Taper attachment.

The taper attachment (Figure 7-69 ) has many features of special value, among which are the following:

  • The lathe centers remain in alignment and the center holes in the work are not distorted.
  • The alignment of the lathe need not be disturbed, thus saving considerable time and effort.
  • Taper boring can be accomplished as easily as taper turning.
  • A much wider range is possible than by the offset method. For example, to machine a 3/4-inch-per-foot taper on the end of a bar 4 feet long would require an offset of 1 1/2 inches, which is beyond the capabilities of a regular lathe but can be accomplished by use of the taper attachment.

Some engine lathes are equipped with a taper attachment as standard equipment and most lathe manufacturers have a taper attachment available. Taper turning with a taper attachment, although generally limited to a taper of 3 inches per foot and to a set length of 12 to 24 inches, affords the most accurate means for turning or boring tapers. The taper can be set directly on the taper attachment in inches per foot; on some attachments, the taper can be set in degrees as well.

Ordinarily, when the lathe centers are in line, the work is turned straight, because as the carriage feeds along, the tool is always the same distance from the centerline. The purpose of the taper attachment is to make it possible to keep the lathe centers in line, but by freeing the cross slide and then guiding it (and the tool bit) gradually away from the centerline, a taper can be cut or, by guiding it gradually nearer the centerline (Figure 7-70), a taper hole can be bored.

Figure 7-70.  Taper turning and boring.

A plain taper attachment for the lathe is illustrated in Figure 7-69. A bed bracket attaches to the lathe bed and keeps the angle plate from moving to the left or the right. The carriage bracket moves along the underside of the angle plate in a dovetail and keeps the angle plate from moving in or out on the bed bracket. The taper to be cut is set by placing the guide bar, which clamps to the angle plate, at an angle to the ways of the lathe bed. Graduations on one or both ends of the guide bar are used to make this adjustment. A sliding block which rides on a dovetail on the upper surface of the guide bar is secured during the machining operation to the cross slide bar of the carriage, with the cross feed screw of the carriage being disconnected. Therefore, as the carriage is traversed during the feeding operation, the cross slide bar follows the guide bar, moving at the predetermined angle from the ways of the bed to cut the taper. It is not necessary to remove the taper attachment when straight turning is desired. The guide bar can be set parallel to the ways, or the clamp handle can be released permitting the sliding block to move without affecting the cross slide bar, and the cross feed screw can be reengaged to permit power cross feed and control of the cross slide from the apron of the carriage.

Modern lathes use a telescopic taper attachment. This attachment allows for using the cross feed, and set up is a bit faster than using a standard taper attachment. To use the telescopic attachment, first set the tool bit for the required diameter of the work and engage the attachment by tightening the binding screws, the location and number of which depend upon the design of the attachment. The purpose of the binding screws is to bind the cross slide so it may be moved only by turning the cross feed handle, or, when loosened, to free the cross slide for use with the taper attachment. To change back to straight turning with the telescopic attachment, it is necessary only to loosen the binding screws.

When cutting a taper using the taper attachment, the direction of feed should be from the intended small diameter toward the intended large diameter. Cutting in this manner, the depth of cut will decrease as the tool bit passes along the workpiece surface and will assist the operator in preventing possible damage to the tool bit, workpiece, and lathe by forcing too deep a cut.

The length of the taper the guide bar will allow is usually not over 12 to 24 inches, depending on the size of the lathe. It is possible to machine a taper longer than the guide bar allows by moving the attachment after a portion of the desired taper length has been machined; then the remainder of the taper can be cut. However, this operation requires experience.

If a plain standard taper attachment is being used, remove the binding screw in the cross slide and set the compound rest perpendicular to the ways. Use the compound rest graduated collar for depth adjustments.

When using the taper attachment, there may be a certain amount of “lost motion” (backlash) which must be eliminated or serious problems will result. In every slide and every freely revolving screw there is a certain amount of lost motion which is very noticeable if the parts are worn. Care must be taken to remove lost motion before proceeding to cut or the workpiece will be turned or bored straight for a short distance before the taper attachment begins to work. To take up lost motion when turning tapers, run the carriage back toward the dead center as far as possible, then feed forward by hand to the end of the workpiece where the power feed is engaged to finish the cut. This procedure must be repeated for every cut.

The best way to bore a taper with a lathe is to use the taper attachment. Backlash must be removed when tapers are being bored with the taper attachment, otherwise the hole will be bored straight for a distance before the taper starts. Two important factors to consider: the boring tool must be set exactly on center with the workpiece axis, and it must be small enough in size to pass through the hole without rubbing at the small diameter. A violation of either of these factors will result in a poorly formed, inaccurate taper or damage to the tool and workpiece. The clearance of the cutter bit shank and boring tool bar must be determined for the smaller diameter of the taper. Taper boring is accomplished in the same manner as taper turning.

To set up the lathe attachment for turning a taper, the proper TPF must be calculated and the taper attachment set-over must be checked with a dial indicator prior to cutting. Calculate the taper per foot by using the formula:

TPF = D - d x 12

L

TPF = taper per foot,

D = large diameter (in inches), d = small diameter (in inches), L = length of taper

After the TPF is determined, the approximate angle can be set on the graduated TPF scale of the taper attachment. Use a dial indicator and a test bar to set up for the exact taper. Check the taper in the same manner as cutting the taper by allowing for backlash and moving the dial indicator along the test bar from the tailstock end of the head stock end. Check the TPI by using the thread-chasing dial, or using layout lines of 1-inch size, and multiply by 12 to check the TPF. Make any adjustments needed, set up the work to be tapered, and take a trial cut. After checking the trial cut and making final adjustments, continue to cut the taper to required dimensions as in straight turning. Some lathes are set up in metric measurement instead of inch measurement. The taper attachment has a scale graduated in degrees, and the guide bar can be set over for the angle of the desired taper. If the angle of the taper is not given, use the following formula to determine the amount of the guide bar set over:

Guide Bar Set Over (in millimeters) =

 

D = large diameter of taper (mm) d = small diameter of taper (mm) I = length of taper (mm)

L = length of guide bar (mm)

Reference lines must be marked on the guide bar an equal distance from the center for best results.

A metric dial indicator can be used to measure the guide bar set over, or the values can be changed to inch values and an inch dial indicator used.

Checking Tapers for Accuracy

Tapers must be checked for uniformity after cutting a trial cut. Lay a good straight edge along the length of the taper and look for any deviation of the angle or surface. Deviation is caused by backlash or a lathe with loose or worn parts. A bored taper may be checked with a plug gage (Figure 7-71) by marking the gage with chalk or Prussian blue pigment. Insert the gage into the taper and turn it one revolution. If the marking on the gage has been rubbed evenly, the angle of taper is correct. The angle of taper must be increased when there is not enough contact at the small end of the plug gage, and it must be decreased when there is not enough contact at the large end of the gage. After the correct taper has been obtained but the gage does not enter the workpiece far enough, additional cuts must be taken to increase the diameter of the bore.

An external taper may be checked with a ring gage (Figure 7-71). This is achieved by the same method as for checking internal tapers, except that the workpiece will be marked with the chalk or Prussian blue pigment rather than the gage. Also, the angle of taper must be decreased when there is not enough contact at the small end of the ring gage and it must be increased when there is not enough contact at the large end of the gage. If no gage is available, the workpiece should be tested in the hole it is to fit. When even contact has been obtained, but the tapered portion does not enter the gage or hole far enough, the diameter of the piece is too large and must be decreased by additional depth of cut

 

Figure 7-71. 

Another good method of checking external tapers is to scribe lines on the workpiece 1 inch apart (Figure 7-72); then, take measurements with an outside micrometer. Subtracting the small reading from the large reading will give the taper per inch.

 

Figure 7-72. 

Duplicating a Tapered Piece

When the taper on a piece of work is to be duplicated and the original piece is available, it may be placed between centers on the lathe and checked with a dial indicator mounted in the tool post.. When the setting is correct, the dial indicator reading will remain constant when moved along the length of taper.

This same method can be used on workplaces without centers provided one end of the workpiece can be mounted and held securely on center in the headstock of the lathe. For example, a lathe center could be mounted in the lathe spindle by use of the spindle sleeve, or a partially tapered workpiece could be held by the nontapered portion mounted in a collet or a chuck. Using either of these two methods of holding the work, the operator could use only the compound rest or the taper attachment for determining and machining the tapers.

Standard Tapers

There are various standard tapers in commercial use, the most common ones being the Morse tapers, the Brown and Sharpe tapers, the American Standard Machine tapers, the Jarno tapers, and the Standard taper pins.

Morse tapers are used on a variety of tool shanks, and exclusively on the shanks of twist drills. The taper for different numbers of Morse tapers is slightly different, but is approximately 5/8 inch per foot in most cases. Dimensions for Morse tapers are given in Table 7-4.

Brown and Sharpe tapers are used for taper shanks on tools such as end mills and reamers. The taper is approximately 1/2 inch per foot for all sizes except for taper No 10, where the taper is 0.5161 inch per foot.

The American Standard machine tapers are composed of a self-holding series and a steep taper series. The self-holding taper series consists of 22 sizes which are given in Table 7-5. The name “self-holding” has been applied where the angle of the taper is only 2° or 3° and the shank of the tool is so firmly seated in its socket that there is considerable frictional resistance to any force tending to. turn or rotate the tool in the holder. The self-holding tapers are composed of selected tapers from the Morse, the Brown and Sharpe, and the 3/4-inch-per foot machine taper series. The smaller sizes of self-holding tapered shanks are provided with a tang to drive the cutting tool. Larger sizes employ a tang drive with the shank held by a key, or a key drive with the shank held with a draw bolt. The steep machine tapers consist of a preferred series and

an intermediate series as given in Table 7-6. A steep taper is defined as a taper having an angle large enough to ensure the easy or self-releasing feature. Steep tapers have a 3 1/2-inch taper per foot and are used mainly for aligning milling machine arbors and spindles, and on some lathe spindles and their accessories.

The Jarno taper is based on such simple formulas that practically no calculations are required when the number of taper is known. The taper per foot of all Jarno tapers is 0.600 inch per foot. The diameter at the large end is as many eighths, the diameter at the small end is as many tenths, and the length as many half-inches as indicated by the number of the taper. For example: A No 7 Jarno taper is 7/8 inch in diameter at the large end; 7/10 or 0.7 inch in diameter at the small end; and 7/ 2, or 3 1/2 inches long. Therefore, formulas for these dimensions would read:

Diameter at small end= No. of timer

8

Diameter at small end= No. of taper

10

Length of taper= No. of taper

2

The Jarno taper is used on various machine tools, especially profiling machines and die-sinking machines. It has also been used for the headstock and tailstock spindles on some lathes.

The Standard taper pins are used for positioning and holding parts together and have a 1/4-inch taper per foot. Standard sizes in these pins range from No 7/0 to No 10 and are given in Table 7-7 in Appendix A. The tapered holes used in conjunction with the tapered pins utilize the processes of step-drilling and taper reaming.

To preserve the accuracy and efficiency of tapers (shanks and holes), they must be kept free from dirt, chips, nicks, or burrs. The most important thing in regard to tapers is to keep them clean. The next most important thing is to remove all oil by wiping the tapered surfaces with a soft, dry cloth before use, because an oily taper will not hold.

SCREW THREAD CUTTING

Screw threads are cut with the lathe for accuracy and for versatility. Both inch and metric screw threads can be cut using the lathe. A thread is a uniform helical groove cut inside of a cylindrical workpiece, or on the outside of a tube or shaft. Cutting threads by using the lathe requires a

 

 

 

 

 

Screw Thread Terminology

thorough knowledge of the different principles of threads and procedures of cutting. Hand coordination, lathe mechanisms, and cutting tool angles are all interrelated during the thread cutting process. Before attempting to cut threads on the lathe a machine operator must have a thorough knowledge of the principles, terminology and uses of threads.

The common terms and definitions below are used in screw

thread work and will be used in discussing threads and thread cutting.

 

External or male thread is a thread on the outside of a cylinder or cone.

Internal or female thread is a thread on the inside of a hollow cylinder or bore.

Pitch is the distance from a given point on one thread to a similar point on a thread next to it, measured parallel to the axis of the cylinder. The pitch in inches is equal to one divided by the number of threads per inch.

Lead is the distance a screw thread advances axially in one complete revolution. On a single-thread screw, the lead is equal to the pitch. On a double-thread screw, the lead is equal to twice the pitch, and on a triple-thread screw, the lead is equal to three times the pitch (Figure 7- 74).

Crest (also called “flat”) is the top or outer surface of the thread joining the two sides.

Root is the bottom or inner surface joining the sides of two adjacent threads.

Side is the surface which connects the crest and the root (also called the flank).

Angle of the thread is the angle formed by the intersection of the two sides of the threaded groove.

Depth is the distance between the crest and root of a thread, measured perpendicular to the axis.

Major diameter is the largest diameter of a screw thread. Minor diameter is the smallest diameter of a screw thread.

Pitch diameter is the diameter of an imaginary cylinder formed where the width of the groove is equal to one-half of the pitch. This is the critical dimension of threading as the fit of the thread is determined by the pitch diameter (Not used for metric threads).

 

Threads per inch is the number of threads per inch may be counted by placing a rule against the threaded parts and counting the number of pitches in 1 inch. A second method is to use the screw pitch gage. This method is especially suitable for checking the finer pitches of screw threads.

A single thread is a thread made by cutting one single groove around a rod or inside a hole. Most hardware made, such as nuts and bolts, has single threads. Double threads have two grooves cut around the cylinder. There can be two, three, or four threads cut around the outside or inside of a cylinder. These types of special threads are sometimes called multiple threads.

A right-hand thread is a thread in which the bolt or nut must be turned to the right (clockwise) to tighten.

A left hand thread is a thread in which the bolt or nut must turn to the left (counterclockwise) to tighten.

Thread fit is the way a bolt and nut fit together as to being too loose or too tight.

Metric threads are threads that are measured in metric measurement instead of inch measurement.

Screw Thread Forms

The most commonly used screw thread forms are detailed in the following paragraphs. One of the major problems in industry is the lack of a standard form for fastening devices. The screw thread forms that follow attempt to solve this problem; however, there is still more than one standard form being used in each industrial nation. The International Organization for Standardization (IS0) met in 1975 and drew up a standard metric measurement for screw threads, the new IS0 Metric thread Standard (previously known as the Optimum Metric Fastener System). Other thread forms are still in general use today, including the American (National) screw thread form, the square thread, the Acme thread, the Brown and Sharpe 29° worm screw thread, the British Standard Whitworth thread, the Unified thread, and different pipe threads. All of these threads can be cut by using the lathe.

 

The IS0 Metric thread standard is a simple thread system that has threaded sizes ranging in diameter from 1.6 mm to 100 mm (see Table 7-8 in Appendix A). These metric threads are identified by the capital M, the nominal diameter, and the pitch. For example, a metric

thread with an outside diameter of 5 mm and a pitch of 0.8 mm would be given as M 5 x 0.8. The IS0 metric thread standard simplifies thread design, provides for good strong threads, and requires a smaller inventory of screw fasteners than used by other thread forms. This IS0 Metric thread has a 60° included angle and a crest that is 1.25 times the pitch (which is similar to the National thread form). The depth of thread is 0.6134 times the pitch, and the flat on the root of the thread is wider than the crest. The root of the ISO Metric thread is 0.250 times the pitch (Table 7-9).

The American (National) screw thread form is divided into four series, the National Coarse (NC), National Fine (NF), National Special (NS), and National Pipe threads (NPT), 11 series of this thread form have the same shape and proportions. This thread has a 60° included angle. The root and crest are 0.125 times the pitch. This thread form is widely used in industrial applications for fabrication and easy assembly and construction of machine parts. Table 7-9 in Appendix A gives the different values for this thread form.

The British Standard Whitworth thread form thread has a 55° thread form in the V-shape. It has rounded crests and roots.

The Unified thread form is now used instead of the American (National) thread form. It was designed for interchangeability between manufacturing units in the United States, Canada, and Great Britain. This thread is a combination of the American (National) screw thread form and the British Whitworth screw thread forms. The thread has a 60° angle with a rounded root, while the crest can be rounded or flat. (In the United States, a flat crest is preferred.) The internal thread of the unified form is like the American (National) thread form but is not cut as deep, leaving a crest of one-fourth the pitch instead of one-eighth the pitch. The coarse thread series of the unified system is designated UNC, while the fine thread series is designated UNF. (See Tble 7-9 in Appendix A for thread form and values.

The American National 29° Acme was designed to replace the standard square thread, which is difficult to machine using normal taps and machine dies. This thread is a power transmitting type of thread for use in jacks, vises, and feed screws. Table 7-9 lists the values for Acme threads.

The Brown and Sharpe 29° worm screw thread uses a 29° angle, similar to the Acme thread. The depth is greater and the widths of the crest and root are different (Table 7-9 in Appendix A). This is a special thread used to mesh with worm gears and to transmit motion between two shafts at right angles to each other that are on separate planes. This thread has a self-locking feature making it useful for winches and steering mechanisms.

 

The square screw thread is a power transmitting thread that is being replaced by the Acme thread. Some vises and lead screws may still be equipped with square threads. Contact areas between the threads are small, causing screws to resist wedging, and friction between the parts is minimal (Table 7-9 in Appendix A).

The spark plug thread (international metric thread type) is a special thread used extensively in Europe, but seen only on some spark plugs in the United States. It has an included angle of 60° with a crest and root that are 0.125 times the depth.

Different types of pipe thread forms are in use that have generally the same characteristics but different fits. Consult the Machinery’s Handbook or a similar reference for this type of thread.

THREAD FIT AND CLASSIFICATIONS

The Unified and American (National) thread forms designate classifications for fit to ensure that mated threaded parts fit to the tolerances specified. The unified screw thread form specifies several classes of threads which are Classes 1A, 2A, and 3A for screws or external threaded parts, and 1B, 2B, and 3B for nuts or internal threaded parts. Classes 1 A and 1 B are for a loose fit where quick assembly and rapid production are important and shake or play is not objectionable. Classes 2A and 2B provide a small amount of play to prevent galling and seizure in assembly and use. and sufficient clearance for some plating. Classes 2A and 2B are recommended for standard practice in making commercial screws. bolts. and nuts. Classes 3A and 3B have no allowance and 75 percent of the tolerance of Classes 2A and 2B A screw and nut in this class may vary from a fit having no play to one with a small amount of play. Only high grade products are held to Class 3 specifications.

Four distinct classes of screw thread fits between mating threads (as between bolt and nut) have been designated for the American (National) screw thread form. Fit is defined as “the relation between two mating parts with reference to ease of assembly. ” These four fits are produced by the application of tolerances which are listed in the standards.

The four fits are described as follows:

 

Class 1 fit is recommended only for screw thread work where clearance between mating parts is essential for rapid assembly and where shake or play is not objectionable.

Class 2 fit represents a high quality of thread product and is recommended for the great bulk of interchangeable screw thread work.

Class 3 fit represents an exceptionally high quality of commercially threaded product and is recommended only in cases where the high cost of precision tools and continual checking are warranted.

Class 4 fit is intended to meet very unusual requirements more exacting than those for which Class 3 is intended. It is a selective fit if initial assembly by hand is required. It is not. as yet. adaptable to quantity production.

Thread Designations

In general. screw thread designations give the screw number (or diameter) first. then the thread per inch. Next is the thread series containing the initial letter of the series. NC (National Coarse). UNF (Unified Fine). NS (National Special). and so forth. followed by the class of fit. If a thread is left-hand. the letters LH follow the fit. An example of designations is as follows:

Two samples and explanations of thread designations are as follows:

 

No 12 (0.216) -24 NC-3. This is a number 12 (0.216-inch diameter) thread. 24 National Coarse threads per inch. and Class 3 ways of designating the fit between parts. including tolerance grades. tolerance positions. and tolerance classes. A simpler fit.

1/4-28 UNF-2A LH. This is a l/4-inch diameter thread. 28 Unified Fine threads per inch, Class 2A fit, and left-hand thread.

 

 

 

 

 

Cutting V-threads with a 60 degrees thread angle is the most common thread cutting operation done on a lathe. V-threads. with the 60 degree angle. are used for metric thread cutting and for American (National) threads and Unified threads. To properly cut V-shaped threads. the single point

 

 

 

7-47

Metric Thread Fit and Tolerance

The older metric screw thread system has over one hundred different thread sizes and several ways of designating the fit between parts. including tolerance grades. tolerance positions. and tolerance classes. A simple system was devised with the latest ISO Metric thread standard that uses one internal fit and two external fit designations to designate the tolerance (class) of fit. The symbol 6H is used to designate the fit for an internal thread (only the one symbol is used). The two symbols 6g and 5g6g are used to designate the fit for an external thread. 6g being used for general purpose threads and Sg6g used to designate a close fit. A fit between a pair of threaded parts is indicated by the internal thread (nut) tolerance fit designation followed by the external thread (bolt) tolerance fit designation with the two separated by a stroke. An example is M 5 x 0.8-Sg6g/ 6H. where the nominal or major diameter is 5 mm. the pitch is 0.8 mm. and a close tit is intended for the bolt and nut. Additional information on ISO metric threads and specific fits can be found in any updated engineer’s handbook or machinist’s handbook.

THREAD CUTTING TOOL BITS

tool bit must be ground for the exact shape of the thread form. to include the root of the thread (Figure 7-75).

For metric and American (National) thread forms. a flat should be ground at the point of the tool bit (Figure 7-76). perpendicular to the center line of the 600 thread angle. See the thread form table for the appropriate thread to determine the width of the Sat. For unified thread forms. the tip of the tool bit should be ground with a radius formed to fit the size of the root of the thread. Internal unified threads have a flat

on the tip of the tool bit. In all threads listed above. the tool bit should be ground with enough side relief angle and enough front clearance angle (Figure 7-76). Figure 7-77 illustrates the correct steps involved in grinding a thread-cutting tool bit.

TC 9-524

 

 

For Acme and 29° worm screw threads, the cutter bit must be ground to form a point angle of 29°. Side clearances must be sufficient to prevent rubbing on threads of steep pitch. The end of the bit is then ground to a flat which agrees with the width of the root for the specific pitch being cut. Thread-cutting tool gages (Figure 7-78) are available to simplify the procedure and make computations unnecessary.

To cut square threads, a special thread-cutter bit is required. Before the square thread-cutter bit can be ground, it is necessary to compute the helix angle of the thread to be cut (Figure 7-79). Compute the helix angle by drawing a line equal in length to the thread circumference at its minor diameter (this is accomplished by multiplying the minor diameter by 3.1416 [pi]). Next, draw a line perpendicular to and at one end of the first line, equal in length to the lead of the thread. If the screw is to have a single thread, the lead will be equal to the pitch. Connect the ends of the angle so formed to obtain the helix angle.

The tool bit should be ground to the helix angle. The clearance angles for the sides should be within the helix angle. Note that the sides are also ground in toward the shank to provide additional clearance.

The end of the tool should be ground flat, the flat being equal to one-half the pitch of the thread to produce equal flats and spaces on the threaded part.

When positioning the thread-cutter bit for use, place it exactly on line horizontally with the axis of the workpiece. This is especially important for thread-cutter bits since a slight variation in the vertical position of the bit will change the thread angle being cut.

 

 

 

 

7-48

 

The thread-cutter bit must be positioned so that the centerline of the thread angle ground on the bit is exactly perpendicular to the axis of the workpiece. The easiest way to make this alignment is by use of a center gage. The center gage will permit checking the point angle at the same time as the alignment is being effected. The center gage is placed against the workpiece and the cutter bit is adjusted on the tool post so that its point fits snugly in the 60° angle notch of the center gage (Figure 7-80).

In cutting threads on a lathe, the pitch of the thread or number of threads per inch obtained is determined by the speed ratio of the headstock spindle and the lead screw which drives the carriage. Lathes equipped for thread cutting have gear arrangements for varying the speed of the lead screw. Modern lathes have a quick-change gearbox for varying the lead screw to spindle ratio so that the operator need only follow the instructions on the direction plates of the lathe to set the proper feed to produce the desired number of threads per inch. Once set to a specific number of threads per inch, the spindle speed can be varied depending upon the material being cut and the size of the workpiece without affecting the threads per inch.

The carriage is connected to the lead screw of the lathe for threading operations by engaging the half nut on the carriage apron with the lead screw. A control is available to reverse the direction of the lead screw for left or right-hand threading as desired. Be sure the lead screw turns in the proper direction. Feed the cutter bit from right to left to produce a right-hand thread. Feed the cutter bit from left to right to produce a left-hand thread.

Direction of feed. For cutting standard 60° right-hand threads of the sharp V-type, such as the metric form, the American (National) form, and the Unified form, the tool bit should be moved in at an angle of 29° to the right (Figure 7- 8 1), (Set the angle at 29° to the left for left-hand threads). Cutting threads with the compound rest at this angle allows for the left side of the tool bit to do most of the cutting, thus relieving some strain and producing a free curling chip. The direction is controlled by setting the compound rest at the 29° angle before adjusting the cutter bit perpendicular to the workpiece axis. The depth of cut is then controlled by the compound rest feed handle.

For Acme and 29° worm threads, the compound rest is set at one-half of the included angle (14 1/2°) and is fed in with the compound rest. For square threads, the cutter bit is fed into the workpiece at an angle perpendicular to the workpiece axis.

THREAD CUTTING OPERATIONS

Before cutting threads, turn down the workpiece to the major diameter of the thread to be cut and chamfer the end. Engineering and machinist’s handbooks have special tables listing the recommended major and minor diameters for all

thread forms. These tables list a minimum and a maximum major diameter for the external threads, and a minimum and maximum minor diameter for internal threads. Table 7-10 in Appendix A lists the most common screw thread sizes. The difference between the maximum and minimum major diameters varies with different sizes of threads. Coarse threads have a larger difference between the two than fine threads. It is common practice, when machining threads on the lathe, to turn the outside diameter down to the maximum major diameter instead of the minimum major diameter, thus allowing for any error.

The workpiece may be set up in a chuck, in a collet, or between centers. If a long thread is to be cut, a steady rest or other support must be used to help decrease the chance of bending the workpiece. Lathe speed is set for the recommended threading speed (Table 7-2 in Appendix A).

To cut threads, move the threading tool bit into contact with the work and zero the compound rest dial. The threading tool bit must be set at the right end of the work; then, move the tool bit in the first depth of cut by using the graduated collar of the compound rest. Position the carriage half nut lever to engage the half nut to the lead screw in order to start the threading operation. The first cut should be a scratch cut of no more than 0.003 inch so the pitch can be checked. Engaging the half nut with the lead screw causes the carriage to move as the lead screw revolves. Cut the thread by making a series of cuts in which the threading tool follows the original groove for each cut. Use the thread chasing dial, Figure 7-82, to determine when to engage the half nut so that the threading tool will track properly. The dial is attached to

the carriage and is driven by means of the lead screw. Follow the directions of the thread chasing dial, Figure 7-83, to determine when to engage the half nut lever.

After making the first pass check for proper pitch of threads by using one of the three methods in Figure 7-84. After each pass of the threading tool bit, the operator must move the threading tool bit out of the threaded groove by backing out the compound rest handle, taking note of the setting. Traverse the carriage back to the start of the thread and move the compound rest dial back to the original setting plus the new depth of cut. At the end of each cut, the half nut lever is usually disengaged and the carriage returned by hand. (The cross slide dial can also be used to move the tool bit in and out, depending on the preference of the operator.)

After cutting the first depth of thread, check for the proper pitch of threads by using one of the three methods in Figure 7- 84. If the thread pitch is correct as set in the quick-change gearbox, continue to cut the thread to the required depth. This is determined by measuring the pitch diameter and checking the reference table for-the proper pitch diameter limits for the desired tit.

Some lathes are equipped with a thread chasing stop bolted to the carriage which can be set to regulate the depth of cut for each traverse of the cutter bit or can be set to regulate the total depth of cut of the thread.

When the thread is cut the end must be finished in some way. The most common means of finishing the end is with a specially ground or 45 degree angle chanifer cutting bit. To produce a rounded end, a cutter bit with the desired shape should be specially ground for that purpose.

Metric Thread Cutting Operations

Metric threads, are cut one of two ways by using the lathe, designed and equipped for metric measurement or by using a standard inch lathe and converting its operation to cut metric threads. A metric measurement lathe has a quick-change gear box used to set the proper screw pitch in millimeters. An inch- designed lathe must be converted to cut metric threads by switching gears in the lathe headstock according to the directions supplied with each lathe.

Most lathes come equipped with a set of changeable gears for cutting different, or nonstandard screw threads. Follow the directions in the lathe operator manual for setting the proper metric pitch. (A metric data plate may be attached to the lathe headstock.) Most lathes have the capability of quickly attaching these change gears over the existing gears then realigning the gearing. One change gear in needed for the lead screw gear and one for the spindle, or drive gear.

The metric thread diameter and pitch can be easily measured

 

 

with a metric measuring tool. If there are no metric measuring After backing the tool bit out from the workpiece, traverse

tools available, the pitch and diameter must be converted from the tool bit back to the starting point by reversing the lathe

millimeters to inch measurement, and then a inch micrometer spindle direction while leaving the half-nut lever engaged. If

 

 

and measuring tools can be used to determine the proper pitch .the correct pitch is being cut, continue to machine the thread

t

 

 

to the desired diameter measurement. Convert the linearthe half-nut lever stays engaged.

and diameter. Millimeters may be converted to inch measurement either by dividing millimeters by 25.4 inches or multiplying by 0.03937 inches.

For example, a thread with a designation M20 x 2.5 6g/ 6h is read as follows: the M designates the thread is metric. The 20 designates the major diameter in millimeters. The 2.5 designates the linear pitch in millimeters. The 6g/ 6h designates that a general purpose fit between nut and bolt is intended. Therefore, to machine this metric thread on a inch designed lathe, convert the outside diameter in millimeters to a decimal fraction of an inch and machine the major diameterpitch in millimeters, to threads per inch by dividing the linear pitch of 2.5 by 25.4 to get the threads per inch ( 10.16 TPI).

Now. a 8-13 TPI thread micrometer can be used to measure the pitch diameter for this metric thread.

To sum up how to convert metric threads to inch measurement:

 

Convert major diameter from millimeters to inch measure.

Convert pitch and pitch diameter to inch measure, Set quick change gears according to instructions.

Set up the lathe for thread cutting as in the preceding paragraphs on screw thread cutting, Take a light trial cut and check that the threads are of the correct pitch using a metric screw pitch gage. At the end of this trial cut, and any cut when metric threading, turn off the lathe and back out the tool bit from the workpiece without disengaging the half-nut- lever. Never disengage the lever until the metric thread is cut to the proper pitch diameter, or the tool bit will have to be realigned and set for chasing into the thread.

o the desired depth.

NOTE: If the tool bit needs to be realigned and chased into the thread due to disengagement, of the half-nut lever or having to remove the piece and start again, then the lathe must be reset for threading. Start the lathe, with the tool bit clear of the workpiece engage the lever. Allow the carriage to travel until the tool bit is opposite any portion of the unfinished thread; and then turn off the lathe, leaving the engaged. Now the tool bit can be set back into a thread groove by advancing the cross slide and reference. Restart the lathe, and the tool bit should follow the groove that was previously cut, as long as

TAPERED SCREW THREADS

Tapered screw threads or pipe threads can be cut on the lathe by setting the tailstock over or by using a taper attachment. Refer to the references for taper per inch and nominal measurements of tapered thread forms. When cutting a tapered thread, the tool bit should be set at right angles to the axis of the work. Do not set the tool bit at a right angle to the taper of the thread. Check the thread tool bit carefully for clearances before cutting since the bit will not be entering the work at right angles to the tapered workpiece surface.

MEASURING EXTERNAL V-SHAPED SCREW THREADS

The fit of the thread is determined by its pitch diameter. The pitch diameter is the diameter of the thread at an imaginary point on the thread where the width of the space and the width of the thread are equal. The fact that the mating parts bear on this point or angle of the thread, and not on the top of it, makes the pitch diameter an important dimension to use in measuring screw threads.

The thread micrometer (Figure 7-85) is an instrument used to gage the thread on the pitch diameter. The anvil is V-Shaped to fit over the V-thread. The spindle, or movable point, is cone-shaped (pointed to a V) to fit between the threads. Since the anvil and spindle both contact the sides of the threads, the pitch diameter is gaged and the reading is given on the sleeve and spindle where it can be read by the operator.

 

Figure 7-85.

Thread micrometers are marked on the frame to specify the pitch diameters which the micrometer is used to measure. One will be marked, for instance, to measure from 8 to 13 threads per inch, while others are marked 14 to 20, 22 to 30, or 32 to 40; metric thread micrometers are also available in different sizes.

The procedure in checking the thread is first to select the proper micrometer, then calculate or select from a table of threads the correct pitch diameter of the screw. Lastly, fit the thread into the micrometer and take the reading.

The 3-wire method is another method of measuring the pitch diameter for American National (60 degree) and Unified threads. It is considered the “best” method for extremely accurate measurement. Table 7-11 shows three wires of correct diameter placed in threads with the micrometer measuring over them. The pitch diameter can be found by subtracting the wire constant from the measured distance over the wires. It can be readily seen that this method is dependent on the use of the “’best'” wire for the pitch of the thread. The “best” wire is the size of wire which touches the thread at the middle of the sloping sides. in other words, at the pitch diameter. A formula by which the proper size wire may be found is as follows: Divide the constant 0.57735 by the number of threads per inch to cut. If. for example, 8 threads per inch have been cut, we would calculate 0.577358 = 0.072. The diameter of wire to use for measuring an 8-pitch thread is 0.072.

Table 7-11. Three-wire measurement for metric threads.

The wires used in the three-wire method should be hardened and lapped steel wires. they, should be three times as accurate as the accuracy desired in measurement of the threads. The Bureau of Standards has specified an accuracy of 0.0002 inch. The suggested procedure for measuring threads is as follows:

After the three wires of equal diameter have been selected by using the above formula, they are positioned in the thread grooves as shown on page A-28 in Appendix A. The anvil and spindle of an ordinary micrometer are then placed against the three wires and the reading is taken. To determine what the reading of the micrometer should be if a thread is the correct finish size. use the following formula (for measuring Unified National Coarse threads): add three times the diameter of the wire to the diameter of the screw; from the sum, subtract the quotient obtained by dividing the constant 1.5155 by the number of threads per inch. Written concisely, the formula is:

m = (D + 3W) – 1.5155
n

Where:

m = micrometer measurement over wires.
D = diameter of the thread.
n = number of threads per inch.
W = diameter of wire used.

Example: Determine m (measurement over wires) for 1/2 inch, 12-pitch UNC thread.

Proceed to solve as follows, where:

W = 0.04811 inch
D = 0.500 inch
n= 12
m =  (0.500+ 0.14433) – 1.5155
12

m = (0.500 + 0.14433) 0.1263

m = 0.51803 inch (micrometer measurement)

When measuring a Unified National Fine thread, the same method and formula are used.

An optical comparator must be used to check the threads if the tolerance desired is less than 0.001 inch (0.02 mm). This type of thread measurement is normally used in industrial shops doing production work.

CUTTING INTERNAL THREADS

Internal threads are cut into nuts and castings in the same general manner as external threads. If a hand tap is not available to cut the internal threads, they must be machined on the lathe.

An internal threading operation will usually follow a boring and drilling operation, thus the machine operator must know drilling and boring procedures before attempting to cut internal threads. The same holder used for boring can be used to hold the tool bit for cutting internal threads. Lathe speed is

To prevent rubbing, the clearance of the cutter bit shank and boring tool bar must be greater for threading than for straight boring because of the necessity of moving the bit clear of the threads when returning the bit to the right after each cut.

The compound rest should be set at a 29° angle to the saddle so that the cutter bit will feed after each cut toward the operator and to his left.

Although the setup shown in Figure 7-86 would be impractical on extremely large lathes, it allows a degree of safety on common sized machines by having the compound ball crank positioned away from any work holding device that would be in use on the lathe, eliminating the possibility of the operator’s hands or the compound rest contacting the revolving spindle and work holding devices.

 

Figure 7-86.

Cutting 60° left-hand threads. A left-hand thread is used for certain applications where a right-hand thread would not be practicable, such as on the left side of a grinder where the nut may loosen due to the rotation of the spindle. Left-hand threads are cut in the same manner as right hand threads, with a few changes. Set the feed direction lever so that the carriage feeds to the right, which will mean that the lead screw revolves opposite the direction used for right-hand threading. Set the compound rest 29° to the left of perpendicular. Cut a groove at the left end of the threaded section, thus providing clearance for starting the cutting tool (see Figure 7-87). Cut from left to right until the proper pitch dimension is achieved.

 

Figure 7-87.

CUTTING EXTERNAL ACME THREADS

The first step is to grind a threading tool to conform to the 29° included angle of the thread. The tool is first ground to a point, with the sides of the tool forming the 290 included angle (Figure 7-88). This angle can be checked by placing the tool in the slot at the right end of the Acme thread gage.

 

Figure 7-88.

If a gage is not available, the width of the tool bit point may be calculated by the formula:

Width of point = 0.3707P – 0.0052 inch

Where P = Number of threads per inch

Be sure to grind this tool with sufficient side clearance so that it will cut. Depending upon the number of threads per inch to be cut, the point of the tool is ground flat to fit into the slot on the Acme thread gage that is marked with the number of threads per inch the tool is to cut. The size of the flat on the tool point will vary depending upon the thread per inch to be machined.

After grinding the tool, set the compound rest to one-half the included angle of the thread (14 1/2°) to the right of the vertical centerline of the machine (Figure 7-89). Mount the tool in the holder or tool post so that the top of the tool is on the axis or center line of the workpiece. The tool is set square to the work, using the Acme thread gage. This thread is cut using the compound feed. The depth to which you feed the compound rest to obtain total thread depth is determined by the formula given and illustrated in Table 7-9 in Appendix A. The remainder of the Acme thread-cutting operation is the same as the V-threading operation previously described. The compound rest should be fed into the work only 0.002 inch to 0.003 inch per cut until the desired depth of thread is obtained.

The formulas used to calculate Acme thread depth are in Table 7-9 in Appendix A. The single wire method can be used to measure the accuracy of the thread (Figure 7-90). A single wire or pin of the correct diameter is placed in the threaded groove and measured with a micrometer. The thread is the correct size when the micrometer reading over the wire is the same as the major diameter of the thread and the wire is placed tightly into the thread groove. The diameter of the wire to be used can be calculated by using this formula:

Wire diameter = 0.4872 x pitch

Thus, if 6 threads per inch are being cut, the wire size would be:

0.4872 x 1/6= 0.081 inch

Cutting the 29° worm screw thread (Brown and Sharpe). The tool bit used to cut 29° worm screw threads will be similar to the Acme threading tool, but slightly longer with a different tip. Use Table 7-9 in Appendix A to calculate the length of the tool bit and tip width. The cutting is done just like cutting an Acme thread.

CUTTING SQUARE THREADS

Because of their design and strength, square threads are used for vise screws, jackscrews, and other devices where maximum transmission of power is needed. All surfaces of the square thread form are square with each other, and the sides are perpendicular to the center axis of the threaded part. The depth, the width of the crest, and root are of equal dimensions. Because the contact areas are relatively small and do not wedge together, friction between matching threads is reduced to a minimum. This fact explains why square threads are used for power transmission.

Before the square thread cutting tool can be ground, it is necessary first to determine the helix angle of the thread. The sides of the tool for cutting the square thread should conform with the helix angle of the thread (Figure 7-79).

For cutting the thread, the cutting edge of the tool should be ground to a width exactly one-half that of the pitch. For cutting the nut, it should be from 0.001 to 0.003 of an inch larger to permit a free fit of the nut on the screw.

The cutting of the square thread form presents some difficulty. Although it is square, this thread, like any other, progresses in the form of a helix, and thus assumes a slight twist. Some operators prefer to produce this thread in two cuts, the first with a narrow tool to the full depth and the second with a tool ground to size. This procedure relieves cutting pressure on the tool nose and may prevent springing the work. The cutting operation for square threads differs from cutting threads previously explained in that the compound rest is set parallel to the axis of the workpiece and feeding is done only with the cross feed. The cross feed is fed only 0.002 inch or 0.003 inch per cut. The finish depth of the thread is determined by the formula.

Depth = ½P

The width of the tool point is determined by this formula also and will depend upon the number of threads per inch to be machined. It is measured with a micrometer, as square thread gages are not available.