1/4 diameter, change to a 3-flute tool
.002 CLT x 3 flutes = .006 chip load per tool @6,000 RPM = 36 Inches per minute

TECHNICAL TIP #20; THREADING: TAP HOOK AND RELIEF

There are four basic design features that are incorporated into the design of all cutting tools, including taps. They include cutting face (hook), relief, base material, and surface treatment or coating. We will begin this series of tips with hook and relief.

The cutting face is that portion of the tap flute, between the major and minor diameter of the thread, that cuts or shears the workpiece material. The entry angle of the cutting face into the workpiece material is measured in degrees, from positive to negative, from a perpendicular reference line through the axis of the tool. Positive hooks are used for soft materials that produce continuous (stringy) chips such are aluminum, mild steel, and stainless. Due to the positive angle, the cutting faces are fragile and may chip easily. Negative hooks are used for materials producing broken or powder chips, or those that have been hardened. This type of cutting face is much stronger and is also less prone to chipping.

Relief on a tap may be found on the chamfer's major diameter (required for tapping), or in the threads, in the form of radial clearance or back taper. Radial or thread relief is a thinning of the tooth from the cutting face to the heel to relieve cutting pressures and friction across the land of the tap. Thread relief is applied for materials that are tough, hard, or have high elastic memory (shrinks or squeezes the tap creating friction). Back taper is the reduction of the major, pitch, and minor diameters from the first thread at the front of the tap to the last thread near the shank. While thread relief is applied for specific applications, back taper is applied to all taps.
Thanks to Paul May for the suggestion for this topic!

TECHNICAL TIP #21; THREADING: TAP DESIGN/APPLICATIONS:

Today, It seems as though there are as many tool designs as there are part materials to be tapped. However, when taking a closer look at the geometry of the various specialty taps for these materials, a few basic design philosophies emerge. Let's take a closer look.

A. The most common and easiest to machine, are soft, ductile materials that produce long continuous (stringy) chips. They range from non-ferrous such as aluminum and copper to mild to medium alloy steels and also include some free machining stainless steels. These materials are easy to cut, produce minimal heat, and are not very abrasive. Taps for this material are designed with medium to high hook cutting geometry, minimal or no thread relief, general-purpose high speed steel such as M1 or M7, and either an oxide, nitride surface treatment, or Titanium Nitride (TiN). Most GP taps or those for stainless fall into this category.

B. Heat treated ferrous materials, generally above 275 Bhn. Considerably more difficult to produce a chip, heat generated during cutting becomes a consideration, and they are generally abrasive. Taps are designed with low or negative hook cutting geometry, relief to generate a chip, and require a heat resistant material such as cobalt or tungsten based HSS such as M42, Rex 45, or T15. Thin film coatings TiN, TiCN, and TiAlN are often preferred for lubricity, heat resistance, and abrasion resistance. Heavy duty and HP taps for hard alloys are designed with these features.

C. Tough alloys, such as nickel and titanium, are generally not hard, but their toughness makes it very difficult to produce a chip. There is more elastic memory (closing in), which causes friction and heat, and are quite abrasive, and easily work harden. The chips produced are generally long. Taps are designed similar to those for hard materials, but the hook and relief are often higher to reduce friction and heat. When tapping materials such as titanium, higher H limits are recommended to overcome shrinkage.

D. The last category is materials that produce very broken chips or powder, such as cast iron or brass. Because these materials are cast, they are also abrasive. Although they are very soft, the hook is normally low or neutral and no relief, other than the back taper, are required. General purpose HSS is often sufficient, and either a nitride surface treatment or one of the thin film coatings help with abrasion resistance.

TECHNICAL TIP #22; THREADING: THE RELATIONSHIP OF H-LIMITS AND CLASS OF FIT:

H limits are used to properly size a tap for the threaded hole to be produced. They are selected based upon the tolerance required for the part. These tolerances are defined by the symbols class 1B, 2B, or 3B. Class 1B has the broadest tolerance and is generally applied to DIY (Do It Yourself) type nuts and bolts. Class 2B is the most common and is used for general fasteners and threaded parts. Class 3B is the tightest tolerance and used for close fit and high strength fastening applications, primarily in the automotive and aerospace industry.

Once the class of thread and part tolerance has been defined, an H limit is selected to produce a thread that is within the minimum and maximum limits for that class if fit. These limits are the same as the Go and Not Go thread plug gage dimensions. The goal is to select a tap with an H-limit that is near the middle of the part tolerance. For instance, if the total tolerance was .005", the tap should be approximately .0025" larger than the minimum limit of the part and .0025" smaller than the maximum. However, to handle the widest variety of tapping conditions, the "40% rule" is commonly used. Using this rule, the tap is placed at 40% of the part tolerance. For example, if the part tolerance is .005", multiplying .005" by 0.40 equals .002". Thus, the tap would be .002" larger than the minimum limit of the part or Go thread gage.

With the position of the tap in relationship to the part tolerance established, the selection of an H limit number, such as H3, H4, H5, etc. is possible. H limits are a sequence of size "steps" in .0005" increments beginning at the minimum size limit of the part, starting with H1. In other words, an H1 limit is one .0005" increment larger than the minimum limit or Go gage, an H2 is two .0005" increments (or .001) larger than the minimum limit, an H3 is three .0005" increments (or .0015") and so on. In the example above, a tap that is .002" larger than minimum limit, is four .0005" increments larger, or an H4. This would be the tap H limit recommendation for this tolerance.

If after selecting the proper H limit, an oversize or undersize thread exists, or if shrinkage due to heat treating or plating will occur, larger or smaller H limits may be required to adjust to the condition.

TECHNICAL TIP #23; MILLING: CORNER RADIUS:

Corner radius end mills are typically used in the aerospace industry because of the need to reduce or eliminate stress points in work pieces. End mills can be made with a corner radius up to 25% of the diameter or even larger depending on the application.

Adding a corner radius to end mills when not required by the work piece can have a significant effect on tool life, performance, and overall productivity of the operation.

A corner radius can be made tangent to both the end of the end mills and the outside diameter. It can be tangent to one, both, or not tangent to either. (e.g. The pivot point of a .030 radius that is tangent on both the cutting diameter and end teeth would be.030 from the end and .030 from the side or diameter of the end mill.)

A corner radius has the effect of thinning out the chip and distributing the cutting forces equally around the radius. This strengthens the corner and reduces chipping or fracture problems normally associated with the corner of the end mill. This will also allow the end mill to run at higher chip loads and significantly improves the life as compared to mills with sharp corners.

A corner radius also has an impact on the finish of the work piece surface produced by the end of the mill. The larger the radius, the better finish produced. For example a .060 corner radius will produce a much better finish than a .005 corner radius. Adding a wiper flat, with or without a corner radius, will also improve the surface finish produced by the end cutting teeth.

TECHNICAL TIP #24; THREADING: TAPER PIPE REAMERS

One practice that is frequently recommended for taper pipe tapping may not always be that beneficial. Many believe that holes should be reamed with a tapered reamer prior to tapping. If reaming depth is not closely controlled, it may cause the tap to cut unacceptable threads or shorten tap life. (Suggested diameter size at large end of hole is available through our technical hotline) A hole correctly reamed to size is approximately .008 to .010 smaller than the minor diameter of the threads after the hole is tapped to try and insure that full thread height is achieved. Reaming an oversized hole will result in insufficient thread height. If the reamed hole is too small, it will subject the tap to an extreme cutting load. Even a correctly reamed hole is subject to these forces at the cutting points, or thread crests, because all the teeth begin cutting at the same time. Additional, materials that tend to work-harden could pose problems for the following tap. Unless there is a compelling reason for taper pipe reaming, it may be best to adjust the drilled holes so that they can be tapped without reaming. In some cases, such as high-pressure assembly where four or more "perfect" threads are required, reaming would be called for. But, in most cases, tapping a non-reamed hole will produce enough "perfect" threads to satisfy sealing requirements. In other words, taper pipe reaming should not be considered standard procedure.

TECHNICAL TIP #25; DRILLING: ENLARGING EXISTING HOLES:

Occasionally, there is a requirement to enlarge pre-existing holes, or to create large diameter holes utilizing successively larger drill diameters to achieve the final size. Often, standard two flute twist drills or reamers are used. While these tools may do the job successfully, they are not the ideal for these situations.

Conventional twist drills are designed to penetrate the workpiece at the center of the point, known as the chisel, and cut over the entire length of the cutting lips. Once the outside diameter penetrates the face of the part, the finish size is established. However, when using a conventional drill to enlarge a hole, the drill point will hit the pre-drilled hole in the middle of the cutting lips. Because of the positive rake created by the helix of the drill, this can cause the cutting lips to chip, creating a groove or worn spot across the land on the end of the point. In addition, the drill tends to chatter or seize in the hole, effecting hole size, hole shape, and finish in the part.

Reamers on the other hand, are intended to improve finish and control size. They follow the existing hole and are designed to remove up to a 1/16" of material on diameter depending upon size. Because of their multiple and shallow flutes, they do not have the chip carrying capability to remove large amounts of material necessary to enlarge holes. Chips will pack in the flutes, preventing cutting fluids from reaching the front of the reamer. This will cause excessive heat and wear in the chamfer area. In extreme cases the chamfer teeth will chip or break.

The ideal tools for enlarging holes are core drills. They have a 118 included angle point that does not cut to center and can open up a pre-drilled hole from as small as 60% of the tools diameter. They usually come in three or four flutes with straight or tapered shanks. Four flutes have less chip space and are recommended for shallower holes, but will produce the best finish and size. Three flutes provide more chip space allowing them to be used in deep holes where a larger volume of chips are created.

TECHNICAL TIP #26; DRILLING: PECK FEEDING

Drilling of holes 2 to 3 diameters deep can usually be accomplished with one step. When the need arises to drill 4, 5, or more diameters deep it becomes much more difficult to evacuate chips, especially with non-Coolant hole drills. The deeper the hole the greater the tendency of the chips to becomes jammed in the flutes preventing coolant from reaching the drill tip. This buildup of heat at the drill tip will eventually result in premature failure.

This problem can be overcome by introducing a peck cycle. A peck cycle is where the entire drill is periodically withdrawn from the hole to remove chips, and then re-entering the hole to drill a small distance and withdrawing the drill again until the full hole depth is reached. The first 2 diameters can usually be drilled before initiating a peck drilling cycle. Obviously, peck feeding would not be very efficient for any kind of production work.

The use of coolant hole drills and high-pressure coolant systems will in most cases eliminate the need for peck drilling. Special purpose drills with high spirals and/or parabolic flute forms can also be used to drill deeper holes without peck drilling.

TECHNICAL TIP #27; MILLING; OVERHANG AND DEFLECTION RATIOS:

• Use the largest end mill the work piece will allow.
• Minimize the amount of overhang from the spindle nose.
• Reduce feed per tooth.
• Reduce radial or axial depth of cut.
• Reduce number of flutes.
  

TECHNICAL TIP #28 DRILLING; WHY SUBLAND VS. STEP DRILLS?:

A Subland Drill is considered to be two conventional twist drills with different diameters combined into one tool. Subland construction has built in concentricity between diameters for the length of flutes, whereas a step drill may be eccentric due to grinding of the small diameter out of the large diameter.

The lands of a subland tool extend back the full flute length to the shank making it easier to evacuate the chips from the drill cavity. Sublands are easier to resharpen due to its independent flutes while a step drill tends to weaken at the intersection of the small and large diameter after so many regrinds. When this happens to a step drill, you must cut off the small diameter and recreate it again. Additionally, sublands have their own web for each diameter and do not have to be web thinned like a step drill.

Subland tools eliminate operations, reduces set up time, perform two or more operations at once, and produce both quality and accurate holes.

TECHNICAL TIP #29; DRILLS; DRILLING ON INCLINED SURFACES:

TECHNICAL TIP #30; FORMULAS FOR CUTTING TOOL SPEEDS & FEEDS:

Speeds and feeds are the most important factors to consider for best results from cutting tools. Improper speeds and feeds often cause low production, poor quality, and damage to the tool. Too high a speed or too light a feed leads to rapid wear and dulling of the cutter, reducing tool life.
Speed is measured in peripheral feet per minute. It is often referred to as cutting speed or surface speed. Feed is normally measured and stated in inches per minute (IPM). It takes into consideration the number of cutting teeth (or flutes), the feed per tooth (or cutting edges), and the revolutions per minute. Feed recommendation tables for drills generally are based upon two flute drills.
In establishing operating conditions, all feeds rates should be calculated from the chip load or feed per tooth. The highest possible feed per tooth will usually give longer tool life. However, excessive feeds may overload the tool causing chipping of the cutting edges or breakage.
Following are many of the commonly used formulas for calculating operating parameters for cutting tools:

SFM: Surface Feet per Minute/Cutting Speed: .262 X RPM X D (D=Diameter)
RPM: Revolutions Per Minute/Rotational Speed: (3.82 X SFM)/D or SFM/(.262 X D)
IPM: Inches Per Minute: Machine Feed Rate: RPM X IPR or T X IPT X RPM (T= # of teeth)
IPT: Inches Per Tooth/Feed Per Tooth: IPM/(RPM X T)
IPR: Inches Per Revolution-Feed Per Revolution: IPT X T or IPM/RPM
Inches to mm: Inches X 25.4 or Inches/ 0.03937
MM to inches: mm/25.4 or mm X 0.03937
If you would like a handy Excel.xls calculator for these formulas (and others) to download to your desktop, reply to this message and we will return it as an attachment!

TECHNICAL TIP #31; DRILLING; MORE DEEP HOLE TIPS:

Drilling of deep holes in some cases required drilling to depths of 20 times drill diameter. Drilling to these depths causes concern for chip evacuation and heat build up on the tool, generating excessive wear at point.

Here are some factors to consider when drilling to these deep depths.

Material to be cut and its hardness will determine whether to use high-speed steel M-7 or the cobalt grade M-42. Although M-7 is the most frequently used HSS, M- 42 is the choice when machining in the BrineIl range 296 and above.

Tool construction must be of a heavy-duty style, with typical web thickness of 45 to 60 percent of the drill diameter to maintain rigidity over the long flute length.

Helix angles of 36 to 45 degrees are common to evacuate the chips efficiently up the flutes.
Points are generally 135 degrees heavy duty split, Some times referred to as crankshaft drill points. Other flute styles to consider are parabolic with double margins.

Due to the OAL of the tools being extremely long, here are some points that will help to increase tool life.

When calculating OAL consider the reach length, amount of re-sharpening required, bushing or fixture length and part thickness. Minimize excessive overhang. Drill points should always be kept sharp. Proper lubrication is critical and coolant should be well filtered.

The most critical machining function is the evacuation of chips, drilling depth and the critical path of chip evacuation as well as knowing when to withdraw the tool before the chips get hot and anneal the tool.

For controlling the chip the right feeds and speeds must be chosen, in general 50 to 65 SFM is standard the feed will depend on the tool diameter.

If the chip is long and stringy, increase feeds until chip is broken into smaller pieces.

TECHNICAL TIP #32; MILLING; REDUCING VIBRATION & CHATTER:

When chatter arises it tends to be self-sustaining until the problem is corrected. This condition causes poor finish on the part and will damage and significantly reduce the life of end mills. Carbide end mills are peculiarly susceptible to damage.

When experiencing chatter problems, the basic reflex action is the reduction of cutting forces.
This can be done by:
(1) Reducing the number of flutes.
(2) Decreasing the chip load per tooth by reducing the feed or increasing the speed or RPM.
(3) Reducing the axial or radial depth of cut.
Even though these steps can and will reduce chatter, slowing down the cutting process is not always the best course of action and reducing the chip load can be detrimental to the cutter.

Better first steps are to improve rigidity and stability:
(1) Use a larger end mill with a larger core diameter.
(2) Use end mills with reduced clearance or a small circular margin.
(3) Use the shortest overhang from spindle nose to tip of tool.
(4) Use stub length end mills where possible.
(5) Use balanced tool holders.
(6) Rework fixture to hold the work piece more securely.
(7) Reprogram the cutter path shifting cutting forces into stiffer portions of the work piece.
(8) Look for sweet spots in spindle speeds then adjust feed accordingly.

A common source of chatter is the machining of corners. As the end mills enters the corner the percentage of engagement increases the number of teeth in the cut. This drastically increases the cutting forces, causing chatter. Using circular interpolation and producing a bigger corner radius then the part print calls for then going back and removing the remaining stock with a smaller end mill using circular interpolation will reduce the tendency to chatter.

TECHNICAL TIP #33; MILLING, WHEN AND HOW MUCH TO REGRIND:

TECHNICAL TIP #34; COATINGS; COATINGS FOR CUTTING TOOLS:

Our group receives many questions regarding coating recommendations for different tool types in an infinite variety of materials. Many of you have also suggested that we cover this topic in your suggestions of things for us to address. We are preparing some future specific tips to cover this exact topic. As a preface to those tips, we would like you to understand a couple of important fundamental things regarding high performance coatings.

You may be assured that any Kennametal-Greenfield IPG coated tool will set the standard for the highest possible performance available in the marketplace.

TECHNICAL TIP #35; COATINGS: TAPS

Below are shown our current recommendations for taps in various materials. They are listed in order of preference. Those in parenthesis should be viewed as alternatives, but not in order of preference. When Maxi #1 is shown, that is our designation for Nitride. Remember to increase SFM by 50% for TiN and TiCN and 100% for TiAlN.

While many factors contribute to tap failure, one that is often overlooked - the drilled hole size.

When a problem arises, generally the drill size being used is checked against a tap/drill chart, and if correct, we look for some other cause for the failure. But are the tap/drill charts giving us the right information?

First, it must be understood that these charts were developed in the '50's and '60's. Drill diameters for the various thread sizes were selected based upon the "probable" hole size a standard bright jobber drill with a conventional point would produce. For example, a #7 (.201") diameter drill, used for a -20 thread, would generally produce a hole that was approximately 0.004" larger than the drills diameter, or about .205". Comparing that to the .196-.207 hole size required for that tap, the #7 drill produces a hole near the maximum limit, which is ideal. This results in approximately a 70% thread height. Removing most of the excess material with the drill significantly reduces the load on the tap without reducing the strength of the thread.

Today, things have changed significantly. There are many advanced drill designs, materials, points, coolant holes, and coatings. Also, accuracy of all drills has improved dramatically as a result of improved drill manufacturing equipment and processes. Today's advanced drills, powered by more accurate, high-speed computer controlled machine tools, are producing holes much closer to, or even the same as, the actual size of the drill.

Utilizing modern drills, CNC's and holders with conventional drill charts could result in tap breakage where none existed before. The #7 drill may no longer be the correct drill size for a -20. It may be producing a hole much too small for successful tapping. It is recommended that the tap/drill chart be used as a reference, or starting point, and select a drill diameter for the best hole size. The finished hole size is what is relevant! In the case of the -20, any drill that produces a hole close to .207" could be used. Even a #5 (.2055") or a special diameter may be acceptable based upon the drill design and conditions.

TECHNICAL TIP #37; COATINGS; RESHARPENING OF COATED TOOLS:

Our group receives many questions regarding tool life after resharpening coated tools. Typically when drills or end mills are resharpened the coating is only removed from the clearance or flank area of the tool. When resharpened in this way there is still coating protection on the rake face of the tool. In these cases tool life typically decreases by 30% or more but will still be much better then an uncoated tool. If the regrind process removes the coating from the rake face, the tool will then perform no better than an uncoated tool. As a general rule tools should be re-coated after resharpening to restore the full protective effect of the coating.

It is our consensus that if metal removal is the goal for a reground not re-coated tool that speeds and feeds can be left very close to coated parameters. If tool life is the goal that you should reduce speeds and feeds by 20-30% to achieve close to coated tool life. Additionally, after multiple recoats, drills, reamers, and other close tolerance tools can become oversize due to the layering effect of coating on top of coating. In these cases the tools can be stripped, resharpened and recoated to restore the tool to original specifications.

As a follow-up to tip #36 regarding tap/drill charts, we have developed a nifty Excel Tap/Drill Calculator that computes drill sizes for inch size cutting and form taps and metric cutting and form taps. If you would like that calculator, send me an e-mail and I will send it back as an attachment-

TECHNICAL TIP #38; THREADING; PIPE TAPS, HOW DEEP TO THREAD?

A common question that we are often asked concerning pipe threads is: How do I know how deep to run a pipe tap into a drilled hole before it is stopped? In other words, how do I know when the pipe thread is either too small to accept the L-1 thread plug gage, or too large to be flush within 1 turn on the gage.

The answer is actually quite simple. Pipe threads are sized differently than standard straight thread. They are based on the basic size at the top of the threaded hole that has been produced by the pipe tap. The Basic size occurs approximately 12 threads for the front of the taper pipe tap. This is commonly called the 12-thread count. You can therefore run any standard projection pipe tap into the drilled hole approximately 12 threads from the front of the tap, and that should be approximately the Basic size for that pipe thread.

TECHNICAL TIP #39; THREADING; NPT vs. NPTF TAPER PIPE THREADS:

The two most common taper pipe threads used in the United States are NPT and NPTF. Applications range from electrical conduits and hand railings to high-pressure pipe lines that carry gas or caustic fluids. NPT threads are for mechanical or low-pressure air or fluid applications and require the use of sealing compounds like Teflon tape, to provide the seal. When the application is more critical, and the sealing compound may fail due to high heat or pressure, NPTF Dryseal threads are used. This mechanical seal is produced by the mating and slight crushing of the threads when a wrench is applied to tighten the fittings.

Visually, both threads appear to be identical. Both have a " taper over one foot of length. Both have the same pitch diameter at the top of the hole of internal threads or end of the pipe on external threads, and both have the same thread lengths or depths. However, there is a subtle difference in the thread form that differentiates the two. The major and minor diameters of both threads are differ slightly. With NPT threads, after a wrench is applied, slight spaces at the major and minor diameters may exist that would allow the assembly to leak and therefore a sealing compound is used to fill any gaps. On the other hand, NPTF threads are designed to ensure that sufficient crushing of the entire thread form will take place to produce a mechanical seal.

How does the difference in thread forms effect the tooling used to produce NPT and NPTF threads? Taps are available for both NPT and NPTF threads having the appropriate form to produce each type of thread. Since NPT threaded parts require sealing compounds, it is acceptable to use an NPTF tap for NPT applications. However, NPT taps cannot be used for NPTF applications, as it will likely produce a thread that will leak. The same is true of external threads. In most cases the tap drill is the same for both forms.

The most significant difference in the two threads is the inspection required. Since sealing compounds will be used for NPT threads, only a single plug with a step, known as an L1 plug (internal thread) or a single thin L1 ring (external) are required to check size. However, since the taper and the position of major and minor diameters are so critical to the sealing of NPTF threads, the additional threads in the assembly known as L2 and L3, and the major and minor diameters are inspected with either special plug or ring gages.

TECHNICAL TIP #40; REAMING; REDUCING CHATTER:

The most common problems associated with poor reamer life and hole finish can be attributed to "Chatter". Chatter is characterized as synchronized vibrations that are set up in the cutting tool, work piece, and machine, or a combination of vibrations in all of these elements. This vibration causes the tool to deflect against the work piece at a continuous, rapid and often irregular pace. The tools attempt to restore balance and resume its natural position against the vibration thus creating chatter. Consequently, chatter leaves poor or torn finishes and possibly tool failure.

Chatter can be caused in one of several ways and can have devastating effects on the quality of the application. Some of the more common reasons include:

1. Excessive speed
2. Lack of rigidity in the bushing or machine
3. Insecure holding of the work piece
4. Excessive overhang of the reamer or spindle
5. Too light a feed
6. Insufficient rake or clearance

Due to the relative small amount of stock being removed from the work piece, reamers perform much better at higher feed rates and lower speeds. A general rule of thumb is to run the tool at feed rates ranging from 200-300% higher than those for drilling. Feed rates will vary depending on the material being reamed. Speed rates should be 2/3's of typical drill requirements. This will allow the tool to cut rather than burnish or rub the material. Increasing the feed rate will promote tool stability within the work piece, reducing deflection between the tool and work piece.

If chatter persists, check the rigidity of the tool in the bushing or machine. Ensure that the holder is securely placed in the spindle. Often the chatter is caused not by the tool but by some facet of the machine setup. Be sure to troubleshoot the holding mechanism for worn or loose bushings or holders. Replace any worn parts that cannot be adjusted and take out all "play" where adjusting can be done. It is also helpful to check the spindle and other driving parts for adequate strength. Weakened driving parts may cause deflection under the cut to be taken.

Eliminating any unnecessary overhang of the reamer or holder. Remember that using the shortest possible tool significantly increases rigidity within any tool. Shorter shanks create less vibration and reduce the danger of deflection and chatter.

It is also important to select the correct style or design of the tool. Also consider the type of material being reamed. Choose a style that provides sufficient rake or clearance. A straight fluted design is common in applications of a "general purpose" nature. This style is best used in a horizontal position for through holes due to its inability to lift chips from the hole. However, right hand helical flutes provide a more positive cutting face, which is advantageous in lifting chips that are free cutting and non-ferrous materials such as aluminum alloys and copper. Left handed helical flutes push the material forward requiring more thrust. This action takes up the slack in the machines setup and aids in containing chatter. Using the proper tool type will reduce chatter and also produce better surface finish.

TECHNICAL TIP #41; THREADING; TAP CHAMFERS:

For a tap to create a thread, it must have a chamfer. These are the tapered or incomplete threads at the front of the tap. The major diameter of the threads are ground to a smaller diameter at the front. This diameter, known as the point diameter, is generally slightly smaller that the pre-drilled hole size or tap-drill size. When the tap enters the hole and begins to cut, each tooth in the chamfer gradually enlarges the thread in the part. Only the "first full thread" behind the chamfer produces the finished size of the thread. The teeth beyond the first full thread serve to guide and support the tap as it creates the desired complete threaded depth of the tapped hole.
There are different lengths of standard chamfers. The most common are "taper", "plug", and "bottoming". The taper has 7 to 10 threads tapered, plug 3 to 5 threads tapered, and bottoming 1 to 2. In general, a taper chamfer, often referred to as a "starter" tap, is used for roughing or sometimes heat-treated material. Plug is the preferred chamfer for most tapping applications and are most common. Bottoming chamfers are used when there is not enough depth of hole for the taper or plug.

Chamfer lengths are selected based upon the type of hole to be tapped. If the hole goes completely through the part or the drill depth is considerably deeper than the required thread depth, a taper or plug chamfer is used. A bottoming chamfer should only be used when the threads must come close to the bottom of the drilled hole and should be avoided whenever possible. A bottom tap will create the greatest amount of tapping torque, requires slower speed (RPM), produces a rougher finish, and substantially reduces tool life.

In addition to the three most common chamfers, semi and modified bottoming chamfers found on specialty taps such as high performance taps and some cast iron taps used in the automotive industry. Semi-bottoming are usually 2 to 2-1/2 threads long, and modified bottoming range between 2-1/2 and 4 threads long depending upon the style of tap. The additional length is used to reduced chip load, add tool life in difficult to machine materials and to allow higher tapping speeds.

TECHNICAL TIP #42; THREADING; THREAD MILLS:

Thread milling has become quite popular in recent years as an alternative to tapping or other forms of threading.

Thread mills look similar to taps, but function entirely different. Taps feed into the part at the rate of the lead of the thread utilizing the chamfer and first full thread beyond the chamfer to cut and enlarge the thread to finished size. On the other hand, a thread mill has no chamfer. The mill is inserted into the hole along the axis of the spindle, deep enough to produce the full thread depth required. The controller moves the thread mill out to the hole diameter until the threads cut into the sidewalls of the hole. The thread mill then moves in a 360 circular motion until it is back to it starting position. During this circular motion the mill must be lifted toward the top of the hole or moved along the "Z" axis of the machine one thread pitch or lead to produce a thread. This lifting movement in conjunction with the circular motion is called "helical interpolation". All machines must have a helical interpolation program capability to utilize a thread mill. After the 360 rotation, the tool returns to the center of the hole and extracted from the part.

Thread mills are most commonly found in solid carbide, with either straight or helical flutes. They are also available in indexable style with carbide inserts, or premium high-speed steel (powdered metal) with helical flutes. Ideally all thread mills are coated with TiN, TiCN, or TiAlN depending upon the application. Indexables are typically for sizes " or larger, and accommodate a variety of threads per inch by replacing the insert. Solid carbide is generally for production threading and for materials up to 62 Rc. Powdered metal HSS thread mills are recommended for materials softer than 30/32 Rc, less rigid setups, interrupted bores and machines that have a limited speed capability.

When should a thread mill be selected over taps? In general, for production threading up to 3/8", taps are more efficient. However, if producing a wide variety of parts, threads, and materials on the same machine, threads mill are far more versatile. They will produce right or left hand, internal or external threads, single or multiple lead from #2-56 with the same mill. Materials range from soft, non-ferrous alloys to heat-treated steels, or tough alloys such inconel and titanium, where tap breakage often occurs. Pipe threads are easily produced without leaving the normal "stop lines" and creating the troublesome stringy chips normally produced by taps. In addition, thread mills can produce full threads to within one pitch of the bottom of the drilled hole.

TECHNICAL TIP #43; MILLING: CLIMB VS. CONVENTIONAL MILLING:

Climb: Milling is when the cutter rotates in the same direction as the feed at the point of contact. When climb milling the chip goes from thick to thin and the pressure of the cutter will force the work down rather than lift it up.

Conventional: Milling in which the cutter rotates in the direction opposing the feed at the point of contact and the rotation of the end mill opposes the direction of the work piece feed. When conventional milling the chip goes from thin to thick. Cutting forces tend to lift the work piece.

In today's more rigid, backlash free machines, climb milling can be used for most milling applications and is the preferred method. In conventional milling the sliding action created as the chip goes from thin to thick dulls the cutter rapidly and creates increased heat in the cutting zone. Work hardening of the surface is much more pronounced under these conditions, especially with stainless steels and high temp alloys. When climb milling the cut starts at full chip thickness without the initial rubbing action, thus cutting temperatures are reduced. This reduces the work hardening effect, and substantially improves cutter life. Re-cutting of chips is less of a problem because chips pile up behind the cutter rather than in front of it. Dimensional and finish requirements of the work piece are usually much improved when climb milling.

Conventional milling will usually produce better cutter life in work pieces with hard and highly abrasive surfaces, since the cutting edge engages the work below the abrasive surface. This protects the edges by allowing them enter on a clean surface.

As a follow up to last weeks tip regarding HSS thread milling, some have asked for a SFM/Feed chart to cover those, e-mail me and I will send as an excel attachment.

TECHNICAL TIP #44; THREADING; UNJ-MJ THREADS:

UNJ and MJ threads, often referred to as "J" threads, are predominately used in the aerospace industry and other applications requiring high fatigue strength, including some automotive applications. The "UNJ" designation is used for inch screw threads and "MJ" for metric threads.

"J" threads are similar to standard Unified or metric threads except they have a large radius in the root or minor diameter of the external thread. This radius eliminates sharp corners in the minor diameter of the bolt to increase the stripping strength. This technique is based upon the principle of using filets or radii in sharp corners on parts to strengthen stress points were cracking or failure may occur due to changes in temperature, vibration, or heavy loads. All other dimensions, such as pitch diameter and major diameter, are the same as standard threads.

Since the radius on the external thread increases the minor diameter of the bolt, the internal thread or nut must be modified to allow it to assemble. The minor diameter of the internal thread must be enlarged to clear the radius. This is the only change to the internal thread. All other dimension are the same as standard Unified and metric threads.

What type of tools are used to produce "J" threads? For the internal threads, since the only change is the minor diameter size, only the tap drill size will need to be changed. The same tap used to produce standard threads is used to produce "J" threads. All tooling for external threads, such as dies, thread rolls, and chasers, must be made to produce a radius at the minor diameter. In addition, all run-out or incomplete threads must also have a radius. In other words, the chamfered teeth on dies and chasers must have rounded crests. Unfortunately, rounded chamfered teeth are difficult to produce, and therefore, not readily available on dies and chasers. In order to use these tools to produce "J" threads on a part, an undercut or clearance must be incorporated beyond the full thread requirement to accommodate the chamfer.

TECHNICAL TIP #45; THREADING; THREAD FORMING TAPS

Thread forming has become commonplace in the metalworking industry. The ability to generate threads without creating chips, using a tool that is generally much stronger than cutting taps, and the ability to produce parts much faster, has made forming an attractive option. While there are limitations to applying these tools, they have found their way into all types of manufacturing operations producing anything from simple components to advanced aerospace parts.

Unlike thread cutting where material is removed to create the thread, thread forming moves or displaces the material to generate the thread form. Since the metal's grain structure displaces along the thread profile rather than being severed by cutting, the threads produced are much stronger. Generally, the threads have a smooth, burnished surface finish.

The taps used to produce formed threads have a special shape. The forming takes place on the high spots or "lobes" in the thread form located around the circumference of the tap. Oil or lubrication "V" grooves are located between the lobes to provide lubrication to the forming threads at the front of the tap. The forming threads are taper threaded instead of chamfered as with conventional cutting taps. Plug and bottoming tapers are available as standard to accommodate through and blind hole tapping. The H limit is generally larger than for the equivalent cutting tap to compensate for the slight shrinkage or "closing in" that occurs in the hole after that tap is removed.

There are many applications that are suitable for thread forming. However, there are a few requirements for them to work successfully. First, the drilled hole size must be larger than for cutting taps. When forming, the minor diameter will be generated by the forming process. Therefore, the minor diameter will be smaller than the pre-drilled hole size. If the part has been punched or drilled for cutting, the hole will have to be opened up for forming. Second, displacement should take place very rapidly. Normally, the RPM should be double the speed used for cutting taps. Third, the material must be capable of being displaced. Generally, materials over 30 Rc, cast materials, and non-metallics should not be formed. Finally, since there is a lot of friction and heat created during this process, lubrication is essential. Straight oils are preferred over soluble oils. Thin film coatings such as TiN and TiCN are also beneficial.

TECHNICAL TIP #46; MACHINING; ELEMENTS OF TOOL TESTING:

Our sales organization routinely conducts tool testing against our competitors to validate cost savings. When evaluating our tools performance against another in the same application there are many variables to take into consideration. Our Productivity Analysis form makes sure we take every aspect of the operation into consideration. Obviously many factors are normally fixed and not changeable such as desired hole depth, thread size, finished diameter, machine cost per hour, material etc, but some performance factors can vary significantly and include:

Lot size may well impact how important these variables become. Goals of the comparison may also vary from tool life, tolerance, scrap reduction and amount of material removed in a given timeframe etc. Machine condition and type also may limit or increase options available.

One common mistake is to compare the exact same tool types, styles, coatings or operating parameters to define cost effectiveness. The goal of testing should be to examine each element of the operation and select the best possible combination to maximize performance.

TECHNICAL TIP #47; THREADING: H LIMITS vs. D LIMITS

In a previous Tech Tip,(#22) "H Limits and Classes of Thread", we discussed the H limit numbering system. To review, H limits are a sequence of numbers in .0005" increments larger than the minimum limit of the part, starting with H1. An H1 limit is one .0005" increment larger than the minimum limit or GO gage, an H2 is two .0005" increments (or .001) larger, an H3 is three .0005" increments (or .0015") and so on. The recommended H limit for a particular size should be approximately 40% of the thread tolerance larger than the minimum limit of the thread.

D limits are similar to H limits and follow the same numbering system. However, H limits are used primarily for inch threads, while D limits are used exclusively for metric threads. As is the case with H limits, D limits are a sequence of numbers in increments larger than the minimum limit or GO gage, but the increments are .013mm or .00051". Starting with D1, a D1 is one .013mm increment larger, a D2 is two .013mm (or .026mm) increments larger, and so forth. As with inch threads, the "40%" rule is applied based upon the tolerance or class of thread.

There are two primary differences between H limits and D limits. The first is very subtle. As we have discussed, H limit numbers are in .0005" increments, while D limits are in .013mm increments, which are slightly larger than .0005". The second difference is much more dramatic. An H or D limit number defines the maximum size of the tap. A tap manufacturing tolerance is then applied to establish the minimum limit. For H limit taps the tolerance is minus .0005" for all sizes through 1" diameter. Tap tolerances for D limits are larger for all thread sizes. The smallest tolerance is .015mm (.00059) and becomes larger with the diameter. For example, an M3 has a .015mm (or .0006") tolerance, an M6 has a .020mm (or .00079") tolerance, and an M20 tap has a .041mm (or .00161) tolerance. That is over 3 times the amount of tolerance of an equivalent " tap. As you can see from these examples, the tolerance allowable becomes quite large.

TECHNICAL TIP #48; MILLING/DRILLING: CARBIDE VS. HSS: HOW TO SELECT?

Several factors must be considered when selecting which cutting tool material to use.
(1) Age, type, strength, condition and horsepower of machine tool
(2) Rigidity of machine, tooling and fixtures
(3) Spindle speed available
(4) Manual or power feed
(5) Work piece material & condition
(6) Number of work pieces to be produced, small quantities or high volume
(7) Material removal rate required
HSS cutting tools are very tough, with a much higher resistance to shock and are very forgiving in applications where machine conditions are not ideal. Machine tools with low horsepower, low spindle speed, manually operated, or have overall poor rigidity should be tooled with HSS.

The development of Cobalt HSS and Powdered Metal along with PVD coatings has helped bridged the gap between HSS and Carbide. These materials have the toughness of HSS, but can in many cases operate near the same speeds and feeds as carbide.

Carbide cutting tools can withstand much higher cutting speeds (not feeds) and temperatures than HSS and typically operate at 2 1/2 to 4 times the speed of HSS. However they can only withstand these high speeds if the machine tool has the strength, rigidity, spindle speed, and power to make use of what carbide tools have to offer. Modern machining centers are generally capable of operating at these higher speeds and feeds, and carbide is a logical choice for drills and end mills up to one inch in diameter. Over 1" the high cost of solid carbide may make HSS, Cobalt HSS and PM cutting tools more economical.

TECHNICAL TIP #49; THREADING: THE CORRECT TAP LUBRICATION

To produce high quality threads, it is important that the tap be well lubricated. A good tapping fluid helps to minimize galling and "built up edge" (BUE), allowing the cutting edges to remain sharp to produce a smoother finish and better size control in the part. It also reduces friction that generates heat, which affects tool life. Additionally, fluids help with the evacuation of chips and allow the tool to run at higher speeds.

Generally, for best tap performance, straight oils should be used. For ferrous materials, sulfur or sulfur/chlorinated oils are preferred. For non-ferrous and non-metallic materials, light oils or soluble oils are recommended. Often, machining centers are equipped with soluble oils for a mixture of carbide and high-speed steel tooling. However, most soluble mixes are not suitable for tapping. Soluble mixes are blended to provide adequate cooling for a variety of tools. However, tap need to be lubricated, not cooled! The coolant may be applied in sufficient volume, but lacks the lubrication necessary to obtain acceptable tool life and part finish. One method of increasing the lubrication of soluble oils is to use special purpose additives. Consult your coolant specialist for recommendations. It is also imperative that high lubrication oils be used when tapping with a thread-forming tap.

In addition to selecting the proper cutting fluid, some thought should be given to the method of application. It should be applied to the cutting area under the highest pressure available. Ideally more than one nozzle surrounding the tap is preferred. The nozzles should be close to the surface of the part as possible, and at an angle close the axis of the tool. They should be close to the tool and pointing directly into the hole. This is important, because not only is the fluid providing lubrication, it is also being used to flush the chips from the flutes.
Lastly, brushing or squirting fluid onto the tap does not provide sufficient lubrication. In fact, combined with heavy viscosity oil, the chips may actually "stick" or "cling" to the tap causing increased chances of breakage.

TECHNICAL TIP #50; THREADING: WHY ARE ROLL FORM TAP RECOMMENDED "H" LIMITS HIGHER THAN CUT THREAD "H" LIMITS?

Roll form tapping is a great way to produce internal threads in production applications. There are many benefits to this process including the absence of chips.

Some factors need to be considered before proceeding with roll form taps such as the material to be tapped, the hole size before tapping, machine capabilities, and the class of fit requirement after tapping.

In the case of "class of fit", the requirement for the finished thread is the same regardless if it is a cut or rolled form thread. Use a 5/16-18 2B internal thread as an example. 2B is the designation for internal thread minimum and maximum values after tapping. It is normally checked with GO and NOT GO thread gages. When cutting this thread the recommended tap "H" limit value is H-5 but when roll forming the same thread the recommended value is H-7. There are published charts in our catalogs detailing other sizes and fit recommendations.

The reason for this larger value is due to the slight shrinkage that occurs in the hole after the tap is removed. All metals have a memory and will try to spring back to their original shape. When displacing metal using a roll form tap, this condition will occur. The higher "H" limit compensates for it by forming a slightly larger thread which shrinks slightly after the tap is removed.

Some other factors may interfere, but in general the recommended "H" limit values published for cut or roll form threads will give acceptable gaging results.

TECHNICAL TIP #51; DRILLING: DRILL REGRINDING

Good tool management is knowing how to recognize drill wear in preparation for resharpening.
Sign's of wear start as soon as the drill starts to cut. All tool regrinding should be done by machine.

Reconditioning of drills has tolerances and clearance angles, which can be found in the USCTI brochure titled Tolerances for Twist Drills and Reamers.

TECHNICAL TIP #52; MILLING: COOLANT FOR CARBIDE MILLS:

When to use misters or flood coolant depends on the application. When conditions permit, misters are preferred for solid carbide end mills, particularly in high-speed machining and finishing operations. As the cutting edges of an end mill go in and out of the cut, the heating and cooling of the edges can cause thermal shock. Misters using cutting oils or coolants are very effective at reducing this effect.

PVD coatings like TiAlN create a thermal barrier, allowing higher operating speeds which dissipates more of the heat with the chip. These coatings are very capable of running in dry or near dry conditions.

Misters also eliminate the cost associated with the disposal and maintenance of cutting fluids, and the contamination of chips. In heavy roughing operations with high radial depths of cut, the need for chip flushing, work piece temperature control, or when other tooling is involved, flood coolant should be used.

TECHNICAL TIP #53; THREADING: SHRINKING THREADED HOLES

At times, threaded holes will "close in" or shrink due to heat shrinkage or perhaps "build-up." In either case, the threaded hole becomes tighter in the process. The "fix" for this condition is to use a slightly larger tap to compensate for shrinkage. This practice is also common for parts to be plated.

If there is a buildup, the solution is fairly simple. We simply take the amount of the build up, multiply that by four, and increase the tap's H limit size accordingly. For example, if .00025" buildup, then .00025 x 4 = .0010. .001" is equivalent to two H limits, therefore, if you were using a H6 you should use a H8.

If there is shrinkage to heat, the solution is to use a larger tap, but the problem is trying to decide how much larger you should go. There is no formula that will give you an exact number. Generally, it is done by trial and error. Our recommendation is to use your GO gage as a guide. If the GO fits snugly but still enters all the way, one or two H limits should be plenty. If the gage locks up tight from the start, then three, four, or more is probably necessary. (Each H limit is .0005" larger than the previous one) If it is heat shrinkage, there could be another problem. When parts shrink, they shrink in ALL directions. So a threaded hole gets smaller in diameter, but it also shrinks along the axis of the thread, producing less than the desired pitch thread. This would be like compressing a coil spring, the distance between each coil is now smaller. The effect would be similar to attempting to screw a 1.5mm pitch thread gage into a 1.25mm threaded hole. This kind of error isn't very significant, but it does happen. We have a few customers that buy taps with a long lead, anticipating it will shrink to normal after heating. Generally, the configuration of the part determines the amount of shrinkage. We recommend starting with a tap that is a couple of H limits larger and see how it gages.

TECHNICAL TIP #54; MILLING: FEED RATE COMPENSATION

When we apply end mills it is important that the metal removal rate is not too light, and the proper chip loads are maintained. Due to the nature of finishing operations the radial depth of cut is generally not more than 25% of the diameter of the end mill. In these cases the chip generated becomes much thinner than what it would be if the depth of cut were 50% of the end mill diameter. The lighter the depth of cut, the more the feed rate must be increased to compensate.
In the case of ball nose end mills, when only the ball nose is engaged in the cut the same chip thinning effect occurs when the axial engagement of the ball is smaller the actual cutting diameter. These cases should be compensated for in the same way.

The effective speed of a ball nose end mill also changes when the axial engagement of the ball is smaller than the actual cutting diameter, and should be adjusted based on the diameter of the ball at the axial depth of cut.

Making these adjustments in feeds and speeds when appropriate can dramatically improve productivity.

The question is how to re-calculate the feed adjustments to get what you thought you were getting? If the answer to this is something you need, e-mail me and I will return an excel calculator that does that for you. As always, just free, no strings attached!

TECHNICAL TIP #55 SAWBLADES; BANDSAW BLADE BREAK-IN

Achieving superior blade life is very dependent upon proper break-in procedures.

First, define the recommended band-speed for the material to be cut. When cutting easily machined materials, cutting rate (square inches per minute) should be set at 1/3 to 1/2 the recommended rate for the first 50 to 75 square inches of material cut. Gradually increase the feed pressure/rate until you achieve the recommended cutting rate after 50 to 75 square inches. When possible, the first gradual adjustment should not be made until the total width of the blade is in the cut.

When cutting difficult to machine materials, such as tool steels or work hardening alloys, set cutting rate at 75% of the recommended rate for the first 25 square inches. Gradually increase the feed until you achieve the recommended cutting rate after 25 square inches. When possible, the first adjustment should not be made until the total width of the blade is in the cut.

TECHNICAL TIP #56; GAGING; CARE OF GAGES:

Clean the part before gaging. Get rid of dirt and chips so that the gage is checking product size unaffected by foreign material.

Keep the gage clean and lightly oiled, both in use and in storage. Light oil will greatly increase wear life. It also helps to prevent "loading" or "smearing" of product material onto gage threads. There can, of course, be some circumstances or materials where oil is objectionable.
Align and start threads carefully. Cross threading can damage end threads of both product and gage.

Don't force the gage. Use reasonable light pressure only. Use common sense to prevent damage or wear on the gage and to correctly evaluate acceptance or rejection of parts.

Protect gages from damage, rust, knicks or jams that could ruin a gage and allow inaccurate results to result. Furnish some kind of protective box at the workbench. Seal/peal plastic dip on gage threads in storage is desirable.

Use thread ring gages equally from both faces. Many times ring gages, submitted for reinspection or reconditioning, are found to be worn/tapered only on the stamped side. The ring is made to be used from either face. Using it alternatively from each end will prolong the wear life.

Gages must be checked/recalibrated periodically to insure they are still within proper tolerances and in suitable condition for continued usage.

TECHNICAL TIP #57; THREADING; OVERSIZE TAPPED HOLES:

One of the most common tapping problems is oversize tapped holes where the NOT GO gage threads into the hole 4 or 5 turns or more. The National, Federal, and Military gaging standards allow three turns max. on the NOT GO.

The first obvious cause for oversize threads is misalignment between the drilled hole and spindle, particularly when the hole is drilled in another station or machine. Under these circumstances, it is extremely important that the fixturing be maintained and is clean when loading the part to insure accuracy. Slight misalignment can be compensated for by using a "radial" float holder, which allows the tap to freely move from side to side to align itself with the drilled hole. In a properly maintained CNC machine, where the hole will be drilled, chamfered and then tapped, a radial float holder is generally not necessary.

A less obvious cause for oversize tapping, but one that accounts for the vast majority of oversize tapped holes, is "shaved" threads. Shaving is a condition where the tap chews or "shaves" away the sides or flanks of the threads in the part. The teeth become thinner or narrower which allows the NOT GO gage to enter the hole beyond the three turns. This "shaving" is caused by a slight mis-match between the lead of the thread on the tap with the feed of the machine. If overfed, the tap is pushed faster than the taps thread lead, which shaves away the front flanks of the threads in the part. These would be the flank surfaces you would see when looking into the top of the hole. This is the most common form of shaving. If the tap is underfed, it will shave away the bottom flanks.

Shaving can occur with all types of feeding mechanism, including the most sophisticated CNC's with synchronous or rigid tapping. Permissible tolerances in both the tool and machine may cause a slight mis-match of lead and feed, which may result, is shaving. When this occurs, the tap should be fed slightly less (approx. 98%) than the thread lead and use an "axial" float holder (pull out-tension/push in-compression) with tension to allow the tap to follow its own lead.

TECHNICAL TIP #58; DRILLING; USE OF SPOTTING DRILLS:

Spot drills are commonly found in 90 and 120 point angles, while most drills come with 118 and 135 points. When is each used and why? For jobber and longer length drills, better positioning and size control can be achieved by first spot drilling. Spotting drills typically have short flutes, short overall lengths and no body clearance or margins. Eliminating margins allows chucking close to the point so that they will produce a true start or center. Spot drills with 90 point angles are used when you want to pre-chamfer the hole, and should only be used with HSS or cobalt drills.
120 spot drills to precede either 118 or 135 HSS drill points generally work well. Carbide following drills will be prone to chipping if the spotting angle is less than the drill point angle. Spotting for carbide drills should always have a flatter angle than the drill point angle, so that the chisel edge area of the drill makes contact first. A 120 spot angle is ideal for a carbide drills with a 118 drill point. A 140 spot angle for carbide drills with 135 points is also ideal.

TECHNICAL TIP #59; DRILLING; DRILL BUSHINGS:

To help select the correct bushing for your application there are some points to consider.
Headless press fit bushings are the most popular and in general are used for single drilling operations. This bushing style is pressed into the prepared hole in the jig or fixture, flush with the jig plate. When inserting bushings, consider using a hand arbor to press the pre-lubricated bushing into the liner. If no arbor is available, insert the bushing with two steel plates drawn together for leverage. If you use a hammer, utilize a block to take the hammer blows, never hit the bushing directly.

During the operation of inserting the bushing, take care to maintain the perpendicular centerline, otherwise inaccuracies may result.

When drilling cast iron or any material that produces small chips, the bushing should be located less than a drill diameter from the work piece. If the material produces long, stringy or heavy chips allow one to one and a half the drill diameter. There are some exceptions. If your application calls for a precision hole, the bushing should be right up to the work piece for better accuracy. Bushing length ratio on a regular spiral drill is 1-1/2 to 2-1/2 times the diameter of the drill.
Always be sure that the drill flutes are long enough to carry the chips to the top of the bushing. If the flutes are still inside the bushing, they have no way to be ejected and will score the bushing.

If using a metric drill in an ANSI bushing the flute length could be shorter and also damage the bushing.

Most wear is caused by poor alignment between the drill and the bushing. Always use sharp tools and self-centering drill points when possible, to avoid walking. Use coolant to protect the bushing and drill from excess heat.

Various other bushings come with chip breakers or directed coolant holes to flush the chips away from the workpiece. Headliner bushings are used when excessive loads are applied which could dislodge a headless liner.

TECHNICAL TIP #60; MACHINING: WORK HARDENING

1. Make sure the cutting tools are always sharp!
2. Run at the recommended feeds and speeds for the material being machined. If incorrect, rubbing vs. cutting will increase heat.
3. Use coolant-feeding tools. Water based coolant should be used at about 8% to 10% mix.
4. Do not dwell tool in one position.
5. When drilling, run with constant feed if possible.
6. If peck drilling, reduce number of pecks and withdraw each one tool diameter.
7. When experiencing tap breakage, the cause may not be the tap, but a work hardened hole.
8. Materials likely to work harden are stainless steels and high temperature alloys.
9. Once again, proper tool maintenance will help to reduce work hardening problems.
   

TECHNICAL TIP #61; THREADING; MACHINE SCREW SIZES:

TECHNICAL TIP #62; END MILLS; CHIP BREAKER VS. ROUGHER?:

Some confusion surrounds the role of chip breaker and roughing mills. How are they different? Are their functions interchangeable? Chip breaker end mills were originally designed for deep pocketing, and slotting. The chip breakers made the chips generated shorter and more manageable. Because chip breakers reduced the cutting forces generated they could also be used in some applications as a rougher. Manufactures began to refer to these end mills as rougher finishers, and others as simply roughers.

With the development of the new generation rougher and rougher finisher end mills in both carbide and HSS with very complex profiles, these terms no longer apply. The new generation end mills substantially reduce the cutting forces and allow for much higher material removal rates in roughing operations then the original chip breaker type end mills.

TECHNICAL TIP #63; END MILLS; MAXIMIZING COATINGS BENEFITS:

PVD TiN coatings are still the primary GP coating for end mills, but TiCN and TiAlN are growing in use. In milling applications we have had questions as to when to use these advanced coatings, and what speeds to run them.

TiCN is a harder coating than TiN with good abrasion resistance. It is very good in milling applications for steels, stainless steels, and non-ferrous materials. End mills coated with TiCN should be operated at speeds up to 50% over un-coated end mills.

TiAlN is a HP for all material types. It is about the same hardness as TiCN but will maintain that hardness at a much higher cutting temperatures. This makes it very effective in high temperature alloys, high speed machining, and dry milling applications. End mills coated with TiAlN should be operated at speeds up to 100% over un-coated end mills.
Bottom line, coating can yield great savings, but that savings is in proportion to your machine capability to achieve the high speeds required.

TECHNICAL TIP #64; REAMING; BRIDGE AND CAR REAMERS:

These terms are somewhat of a "throwback" to times where misalignment of holes in structural steel components were more common than today. Misalignment of holes for bolts in bridges, early automobiles and railroad box cars required a method to create a usable hole from two or more holes that were not aligned properly. A rotating tapered reamer is inserted to a depth that creates a usable diameter for the fastener to fit into. Bridge and car reamers both are designed to cut on their sides as opposed to conventional reamers, which cut on the chamfer. Both styles are heavy webbed for strength and are right hand cut and left hand helix to push the cut chips ahead of the tool. A bridge reamer is typically 3 fluted with a long lead and a car reamer is typically 5 fluted and slightly shorter, thus being more rigid.

TECHNICAL TIP #65; THREADING; TAP CHAMFER LENGTH VS. TOOL LIFE:

For those regular readers of our Technical Tips, Tip No. 41 explained what a chamfer is and its purpose. It also explains what are considered as standard chamfer lengths used in industry today. In this tip we want to emphasize the importance of using the longest chamfer possible for the tapped hole condition and sometimes this includes purchasing a special. An increase in chamfer length will result in an increase in tap life!

To determine the longest chamfer for blind holes you would subtract the full thread length required plus one pitch, to allow clearance at the bottom of the hole for spindle over spin and chips. From the drill depth, divide this by the number of threads per inch (TPI). Now select a tap with a chamfer length no longer than that figure.
Example:
Size: -20 NC
Full thread length: .250
Drill depth: .473
Pitch: 1/ 20 = .050
.473 -.250-.050= .173
.173/ .050=3.5
Now select a standard tap with at with no longer than a 3.5 thread chamfer. Ideally, for a safety margin, a 3-thread chamfer may be preferable. A 4 flute semi-bottoming tap has a total of 12 working teeth vs.8 for the bottoming tap. This is a 50% increase in the number of tap teeth having to shear the work, resulting in dramatically improved tap life!

By selecting a tap with a longer chamfer length, you will reduce chip load per tooth and tapping torque, allowing for higher tapping speeds and increased tool life. When tapping harder steels and space age alloys such as nickel, titanium and stainless, a longer chamfer length may be the difference between success and failure.

If circumstances require you to purchase a special tap, perhaps going through this exercise and specifying the proper chamfer length will insure greater tool life and at no additional cost. For each chamfer tooth added, the tap life will increase exponentially. If you did not receive Technical Tip No. 41 mentioned above just request it by e-mail.

TECHNICAL TIP #66; MILLING; HELIX ANGLES, WHAT ROLE DO THEY PLAY?

Standard end mills are offered with helix angles as low as 15 to as high as 60 angles. General-purpose end mills are generally around 30 . Any increase in the helix angle increases the effective shearing action thus reducing cutting forces and the amount of heat generated during the milling process. Chip ejection is also improved. Lower helix angle end mills are used on more difficult to machine materials where maximum edge strength and rigidity are important.

With straight flutes the load builds up almost instantaneously, making the end mills prone to self excited chatter. With helix angles, chip load is applied to the entire flute length in a progressive siding action similar to that of a snowplow with its blade angled off to one side. This makes the cutting forces much more constant with less chance for chatter. End mills with a higher helix also tend to produce much better work piece finish. The 50 and higher helix angles significantly reduce side loading on the mill making it possible to periphery mill thin wall sections with much less deflection.

TECHNICAL TIP #67; REAMING; "QUALIFIED" REAMERS

Perhaps the word "Qualified," in and of itself, truly reflects what we need to know about the tool.
"Qualified for Rotation" means that the diameter of the shank and the O.D. of the reamer head run concentric to each other within .0002 (typically .0001) with less than .00005 taper. These characteristics lend themselves to the best angular and radial alignment of the reamer, no matter the application.

We can use qualified reamers to great advantage in both rotating and stationary applications. Any time you are utilizing the shank diameter to align the tool in a high tolerance diameter or finish application, the tools should be qualified. If one does not request a qualified reamer, there is potential for angular as well as radial misalignment that you cannot correct at the spindle. This situation is most evident in lathe applications utilizing the "Barber Coleman" up-sharp" style reamer with the pin float hole in a conventional ER style collet chuck. These tools are designed to be run with a pin float holder, the tolerance is put into the cross hole with respect to angular alignment, not in the diameter of the shank. The shanks are ground for clearance in the float. It is important to note that a qualified tool runs equally as well in a pin float holder. An un-qualified tool may or may not run well in an ER collet style holder.

When ordering, if you need "Qualified" tolerances, you will need to specify that in your request.
Chucking Reamers typically hang out of hydraulic chucks, collet chucks, end mill holders, and even three jaw chucks in some cases. If you are using a hydraulic chuck, they require metric h6 shank tolerance.

TECHNICAL TIP #68; GAGING: PLAIN CYLINDRICAL "PIN" GAGES

GO-NOT GO plain cylindrical gages are used to check plain holes to ensure the holes are within tolerance. If the GO member is long enough to check the entire depth of the hole, it is also checking for straightness from top to bottom. Special design "locating" gages can be used to check the position of holes. One of the most common uses for plain gages is to check the minor diameter of tapped holes produced by a drill prior to tapping.

Plain cylindrical gages are available in four classes, "XX", "X", "Y", and "Z". "XX" gages are made to the tightest tolerance and used for master or setting gages, or for part tolerances that are very precise. "X" tolerance are sometimes used for master gages or gaging close work. "Y" and "Z" gages are generally used for inspecting work pieces only.

How do you know which class to select? Selecting the right class of cylindrical gage is not only important to ensure that it rejects "bad" parts, it is equally important to minimize rejecting valuable "good" parts. If a lower class gage is used on a tight tolerance part, the gage tolerance will consume most of the part tolerance, rejecting good parts as being bad. Gage manufactures call this "thievery", stealing part tolerance for the gage tolerance. To ensure accepting the maximum number of good parts, select a class using the "5% rule". That is, the gage tolerance should be no more than 5% of the part tolerance. For example, if the part tolerance is 0.001", the gage tolerance should be no more than 0.00005". Select a class that has a 0.00005" tolerance or less. Our gage catalogs or gage standards publish charts showing the classes and tolerances.

TECHNICAL TIP #69; THREADING; FORM TAPPING STAINLESS STEELS:

Stainless steel is generally more difficult to machine than alloy steels, but may be thread formed if precautions are taken. It is dependent upon the type of stainless steel, and of course the hardness of the material at the time it is being formed. Those that are considered free machining, such as 303, 416 and 440F, form readily and are good applications for thread forming. Tough, non-work hardening stainless, such as 403, 410 and 440C, and work hardening chrome-nickel stainless steels, such as 302, 321 and 316, are more difficult and may not be good candidates. Roll form tapping Precipitation Hardening (PH) stainless, such as 13-8 Mo and 17-4, are generally not recommended.

Free machining stainless steels can generally be thread formed in most existing machine tool applications, provided the machine has a spindle speed that is capable of tapping at twice the RPM that is recommended for cutting taps. While straight oils are recommended for forming, soluble oils are acceptable if additives for lubrication and film strength are added.

Tougher stainless steels are more difficult to form and require additional care. Use the largest drilled hole sizes possible to minimize tapping torque. The feed of the drill should be high and positive to minimize work hardening. Peck drilling or dwelling should be avoided. High lubrication is critical for material displacement. Soluble oils generally do not have sufficient lubricating properties for the high pressure and friction during the forming process. Horsepower available at the spindle should be at least 50% greater for forming this group of materials. For work hardening stainless consider bottoming style form taps to more rapidly displace the material.

PH stainless steels very easily work-harden, which can induce cracking in the thread form during the displacement process, and therefore, are not recommended for thread forming. Stainless steels that are 28Rc or higher are also not recommended for thread forming.

TECHNICAL TIP #70; DRILLING; DEEP-HOLE DRILLING ADJUSTMENTS:

Drilled holes that are more than 3-4 times the drill diameter are considered "Deep Holes" and some adjustments for speed and feed may be required. In deep-hole drilling there is an increasing tendency for chips to pack in the flutes the deeper you drill.

Peck drilling is often used with conventional or standard fluted drills in deep holes.
Peck drilling is withdrawing the drill repeatedly to clear chips from the flutes and allowing coolant to get to the bottom of the hole. The deeper the hole, the more "pecks" you will need.
Today, parabolic fluted drills are the recommended flute style for deep-hole drilling.
Wide flute parabolic drills can drill up to 10-15 diameters without peck drilling in soft materials.
Wide land parabolic drills such as our Q-Cobalt series can drill up to 6-9 diameters in medium hard and tough material without peck drilling.
When deep-hole drilling, a reduction in the speed and feed is often needed to reduce heat generated at the cutting edge.
The following is a table for reduction of standard speeds and feeds for deep hole drilling.
This reduction is for conventional fluted and parabolic fluted drills like our Q-Cobalt series.

TECHNICAL TIP #71; DRILLING; LEFT-HAND DRILLS, WHY?:

Obviously because some people are left-handed! But actually, drills are also made with a left- hand flute spiral as opposed to the customary right hand spiral. Normally, these are seen in the jobbers and screw machine style and have the same flute and overall dimensions as their right- handed mirror image. They are normally in the general-purpose design to drill a wide range of materials and are available in other styles as specials.

Initially, left hand drills were primarily made for multi spindle (two or more) gear driven drilling heads, where the spindles rotated in opposite directions. They also are used in screw machines whose spindle may be rotated counterclockwise. Screw machines are used to manufacture smaller parts made from bar stock or tubing. Screw machines are multi-tasking and may turn, cut-off, drill and tap using multiple cutting tools with different holders.

Left hand drills are often used today to help extract a broken bolt or screw from a threaded hole. In some cases a left hand drill can be used counterclockwise to bring the right hand threaded fastener without damaging the part. This is sometimes done when a preferred screw extractor is not available.

TECHNICAL TIP #72; DRILLING; DOUBLE AND TRIPLE MARGIN DRILLS:

Double margins refer to an additional margin ground just behind the leading margin on each drill land. Double margin drills generally range to one inch in diameter while triple margin drills kick in above one inch in diameter. One function of these additional margins is to stabilize the drill when going thru drill bushings. You now have four location points on the drill instead of two inside of the bushing, providing increased bushing support of excess of 200%. Controlled back taper is also tighter aiding additional support that gives better hole location, a "rounder" hole and better hole finish.
Double margin drills can also perhaps eliminate a reaming operation if you have a slightly wide reamed hole tolerance. When using short drill bushings alignment can be improved considerably with the addition of extra margins. The trailing margin does not actually cut a chip but burnishes the part making a smoother finish and contributes to a uniform hole size.
Double margin drills are also effective on special multi-diameter tools when the large diameter will aid the small diameters centrality and helps give a more concentric drilled hole as well as any chamfered sections.
Double margin drills also reduce tool, bushing and spindle wear due to its bushing contact and rigidity. In Deep hole drilling double margins help, as the margins will support the drill when going deep!
Some of the operations that can be reduced using double margin drills include center drilling and spot drilling.

TECHNICAL TIP #73; THREADING; ACME THREADS:

The uses of Acme Threads usually involve special designs requiring individual consideration. Each tapping job becomes a minor engineering project of its own. The inherent exactness in application of Acme taps makes close coordination between manufacturer and user particularly important. An example of an Acme Thread application may be aircraft wing flap hydraulic actuators or a simple car bumper jack.
American Standard Acme Threads are used to produce traversing motion in valves and other power transmission mechanisms requiring high strength and free movement over long periods of operation.
American Standard General Purpose Acme Thread: Provides clearance of all points of contact between external and internal surfaces for free movement. Normally these applications are indicated with a Class of Fit symbols of "2G", "3G", or "4G". The numbers 2, 3 and 4 will control the amount of backlash allowed. Included flank angle is 29
American Standard Centralizing Acme Threads: Clearance at pitch and minor diameters, with limited clearance at major diameter so that alignment of screw and nut is controlled. The class of fit symbols here are indicated with "2C", "3C", and "4C". Included flank angle is 29
Stub Acme: Stub Acme are similar to General Purpose Acme but are used where coarse pitch thread of shallow height is required. Included flank angle is 29
60 Stub Threads: May be substituted where axial leads do not require the smaller flank angle. They are also for applications where shallow thread height is required as on fitting-up bolts and nuts. Included flank angle is 60.
Modified Square Threads: Used as an equivalent to Square Threads for all practical considerations. However, they should not be used where Acme Threads can serve the same purpose. Modified Square Threads have 10 included flank angles.

Acme thread profile characteristics pose a challenge for internal threading because their block like profile requires that large amounts of material must be cut and removed. Chip load becomes a major factor and the types mentioned are designed to control this.
Taps are furnished in normally two types for most of the above. Sets include either one or two roughers and a finisher. Single pass tandem taps can also be designed with the roughing section built ahead of the finishing section on the same body. -Wes Emerson-VTD Field Sales Manager
Thanks and a gift to Steve Wegner for suggesting we address this topic!

TECHNICAL TIP #74; DRILLING; HIGH PERFORMANCE DRILL POINT ANGLES:

Why do high performance drills all have points in the 130-150 range instead of 118 points?
As a general rule harder materials are drilled with 130 to 150 points and softer materials like wood, hard rubber, plastics, and fibers are drilled with 90 to 100 points. 118 points are somewhat in the middle and are considered to be more general-purpose type points.

High performance drills are generally used in more difficult to machine materials like alloys steels, stainless steels and high temperature alloys. These materials are more effectively cut with points that produce thicker chips. Drills with 130 to 150 points have shorter cutting lips, which do produce thicker chips for a given feel rate. These thicker chips also reduce the tendency of these materials to work harden. Torque requirements are also reduced with higher points angles. -David Ford, Senior Technical Specialist
Thanks and a gift to Mike Harvey in California for suggesting we discuss this topic!

TECHNICAL TIP #75; THREADING; MINIMUM TAP DRILL DEPTH:

The tap drill depth for tapped holes should be deep enough to allow for the minimum thread depth, the taps chamfer, any chips that may accumulate in the bottom of the hole and any over-travel of the spindle as it slows to a stop before reversing. So what minimum drill depth would be ideal?

To answer that, we start with this basic rule: At a minimum, the tap drill depth should be at least of one thread or pitch beyond the chamfer of the tap. In other words, for a -20 tapped hole requiring a 3/8" (.375) thread depth, if a two thread bottoming chamfer is used, having a length of .100", and adding a minimum of one additional thread or .050", the minimum drill depth would be .525" (.375 + .100 + .050 = .525").

However, many times using the "one-pitch rule" does not prevent the tap from hitting the bottom of the hole. In this case three things need to be taken into consideration. The first is the machines capability to stop the spindle rotation at the bottom. Many of the newer machines are able to stop and reverse in one-half turn or less. If this is the case, the "one pitch rule" may be sufficient. However, depending on the age of the machine, many spindles over-travel one, two, or even three pitches. In this case, the additional drill depth should be at least one pitch beyond the over-travel amount. The second consideration is the chips produced. Spiral taps extract chips, preventing them from accumulating in the bottom of the hole. However, chips from straight flute hand taps are likely to be flushed to the bottom by the coolant. The front of the tap may bottom on these chips, chipping or breaking the tap. In this case, one diameter of additional depth is recommended. The third consideration is part of the tap design. If a plug or taper chamfer is used, tap sizes through 3/8" diameter are manufactured with a 90 external centers that could hit the bottom. Therefore, when using a plug chamfer a rough rule is to add one-half the diameter to the length for sufficient clearance.-Dave Miskinis-Senior Technical Specialist

TECHNICAL TIP #76; BASIC MACHINING: COOLANT CONSIDERATIONS:

As you know, we manufacture cutting tools and not coolant, but coolant certainly can dramatically effect the performance of our tools and thus ultimately the cost of your operation. We do have some knowledge we can pass onto you.
Cutting fluids have two basic functions to perform when used in drilling, milling and threading.

Coolant, generally in a water based form helps to cool the chip when it is sheared away from the work piece.

Lubrication helps to reduce friction between the chip and the tool. This improves the surface finish and also is a vehicle for the cut chips to evacuate the flutes. Obviously, tool life is improved because excessive heat and friction cause a dulling action on the tool.

It is our experience that companies sometimes lower the coolant/water ratio significantly assuming this is an easy cost cutting measure. What is sacrificed however is tool life. An example may be taking a recommended soluble oil concentration of 8%-10% and reducing that to 5%. We know from experience that tool life will decrease very rapidly. A drill for example, which always gets thousands of holes, may now get only hundreds of holes. At this point, we get the concerned call about sudden poor tool life from the drill. Many times, our investigation may uncover the coolant issue and once resolved, tool life returns.

For high speed machining tools with carbide tools, the most important benefit is providing cooling characteristics of water-based fluids, however if you are high speed steel tapping you will benefit from using a heavier oil based coolant. We recommend that you follow the manufacturers mixing recommendations.-John Woodbridge, IPG Senior Technical Specialist

TECHNICAL TIP #77; THREADING; TAPPING AND TORQUE CONSIDERATIONS:

Torque requirements play a key role in threading, some guidelines are as follows:

1. Diameter: In small diameter taps, (especially machine screw sizes) the torque required to thread is very close to the torque required to break the tap. Larger taps will have heavier cores.
2. Thread depth; Torque to thread 9 full threads deep may be over double to thread 5 full threads.
3. Percentage of thread: Torque for 80% thread may be double that for 60% threads.
4. Threads per inch: Torque for -20 may be double that of -28 thread, for example.
5. Coatings: Torque reduces dramatically with thin film coating like Tin, TiCN or TiALN.
6. Tap Styles: Torque can effect style selection, spiral fluted taps have very weak cores and may break in tougher materials.
   

If threading with a -20 tap with a " length of engagement, (1-dia.) a tap drill chart may direct you to a #6 drill (.2040) Using the chart above, it falls into the 2/3 to 1-1/2 diameter range and allows the use of a .207 hole size.

The advantage to you may include longer tap life, fewer tap problems, less torque required etc.

A chart for each size is shown in the Greenfield Screw Thread Manuals, one manual for unified and the other for metric threads. Note: This being said, you cannot violate the given minor diameter specification for the thread size.

TECHNICAL TIP #81, DRILLING; CORE DRILL FEEDS AND SPEEDS:

The proper tool to use for enlarging a predrilled hole is not a larger two-flute drill, but a core drill, per tech Tip #25. What we need to make clear in this tip is that the required Speeds and Feeds for enlarging a predrilled hole with either a 3 or 4 flute core drill, are different than a standard 2-flute drill. The recommended Speed for an application is to run the core drill about 2/3's of the speed used to drill with a conventional drill. Example: A 2-flute drill with recommended SFM of 90 SFM in low carbon steel should be run at approximately 60 SFM using a three or four flute core drill. The feed rate of a core drill, however, must maintain the same chip load per flute as a standard 2-flute drill. In other words if the feed rate for a standard 2 flute drill was recommended to be .004 / revolution (or .002 per flute), we would run the core drill (depending on if it was three or four flute) at either .006 or .008 per revolution. -Michael Plankey-Senior Technical Specialist

TECHNICAL TIP #82, DRILLING; ASME-USCTI-DIN-JIS-ISO SPECIFICATIONS:

More and more Metric specifications are showing up in manufacturing prints in the USA. To help clarify abbreviations we offer explanations below.

ASME/USCTI: USA Tool Standards.
American Society of Mechanical Engineering / United States Cutting Tool Institute, all standards are specified in the Imperial measurement (Inches).
DIN: German Standard
Deutsches Institut Fur Normung / German Institute for Standard, all measurements are to the Metric system.
JIS: Japanese Standard
Japanese Industrial Standard, all measurements are to the metric system
ISO: Global
International Standardization Organization, all measurements are to the metric system.

Other countries do have there own standards that would relate to specific products like aircraft and automotive. In the USA other standards like NAS - National Aero Space SAE - Society of Automotive Engineers are related to that type of industries.
Here are some examples of differences in Metric Jobber Drills versus an Inch Jobber Drill.

-John Woodbridge-Senior Technical Specialist

TECHNICAL TIP #83, THREADING: TAPPING TITANIUM:

Titanium and titanium alloys are most often found in aerospace applications due to its lightweight and high strength. However, other industries are discovering the benefits of titanium as well. One of the more common alloys is Ti 6AL-4V. It is generally machined at a hardness ranging from approx. 28 to 37 Rc. One the characteristics that makes titanium difficult to tap is its tremendous elastic memory. When tapping, the material closes tightly around the cutting tool, generating friction and heat, resulting in increased wear of the cutting edges. This material also easily work hardens.

To successfully tap titanium, a tap specifically designed with additional clearance to overcome the extreme elastic memory of the material is recommended. Tap clearances would include extra back taper of the threads from the front to the back of the thread section, full radial clearance in the threads across the tap lands, and additional relief in the tap chamfer area. All of these features are used to reduce friction and heat. In some cases, larger H limits might be required to overcome the shrinkage. Premium grade materials are also used for heat and wear resistance. Obviously we offer these in our standard product lines.

Lubrication and proper pre-tapped hole size are vital to success. A compatible tapping fluid should be used that provides plenty of lubrication to reduce friction. The drill should be selected to produce the largest hole size that is allowed by the thread class callout (2B or 3B). Due to the additional clearances required on these tools, positive feeding of the tap is highly recommended. -Dave Miskinis, Senior Technical Specialist-Greenfield IPG

TECHNICAL TIP #84, MILLING: HOW ARE "KEYWAY" ENDMILLS DIFFERENT?:

Both standard and keyway end mills are generally manufactured to the same geometry features such as rake, clearance and base material. Even the blank dimensions and coatings applied are the same. The difference is the tolerance of the cutting diameter of the tool.

Most standard single-end mills are manufactured with a plus tolerance from its nominal size. This, coupled with a slight back taper over the length of cut helps to compensate for deflection and provides additional tool life. On the other hand, to produce the proper slot width for standard key stock, a keyway end mill, manufactured with a minus tolerance from its nominal size, should be used. The minus tolerance allows the tool to mill a finished slot as close to nominal as possible, insuring a slop-free or light press fit of the key. If there is excessive over-cutting of the slot when using a standard keyway end mill, particularly when milling on older equipment, undersize keyway mills are also available in 0.001" increments to compensate for that.
-David Miskinis, Senior Technical Specialist

TECHNICAL TIP #85, THREADING: TAPPING DEPTH FOR PIPE THREADS:

Standard taper pipe taps are designed to produce sufficient thread depth for standard pipefittings. This would include 4 to 5 turns or threads for assembling the parts "hand tight". These are known as L1 threads. Following these are three additional turns for "wrench" tightening to provide the sealing of the assembly. These are known as L3 threads.

Since all taps have a chamfer for producing the threads, the tap must be fed into the part deep enough to produce the full threads plus allow for the incomplete threads produced by the chamfer. Most standard pipe taps have a maximum chamfer length that ranges between 3 and 4 threads. Therefore, the tapping depth should be the approx. 5 threads for the "hand tight", 3 threads for "wrench tight", and 4 threads for the chamfer, or approx. 12 threads total. We call this the "12 thread count". In other words, count approximately 12 threads back from the front of the tap. This is the position (thread size) that should be flush with the face of the part or top of the tapped hole when the tap is fed to full depth.

When using Short Projection taps, (taps designed for holes shallower than those found on standard fittings) the tapping depth should be the projection marked on the tap plus the L1 length. The L1 length can be found in the Machinery Handbook, ASME thread and gaging standards, etc.

There is no standard thread or tapping depth for straight pipe taps. However, when producing straight pipe fittings that will be assembled with tapered external pipe nipples, the user should allow, at a minimum, for the full thread length on the external part. This length is called the L2 length, which is approximately 8 threads. As with tapered threads, you must also account for the taps chamfer length when setting the taps stroke depth.-David Miskinis, Senior Technical Specialist
Thanks and a gift to Bob Bateson in Oskaloosa, IA for suggesting we address this topic!

TECHNICAL TIP #86, DRILLING: "OFFHAND" HSS DRILLING VS. RIGID SETUPS

Many operations require the ability to take the drilling to the workpiece as opposed to bringing the workpiece to a stationary machine with a rigid set-up. At this point many control variables come into play, perhaps the lack of control over speeds and feeds is the most challenging. Obviously the workpiece material dictates a wide range of proper speeds and feeds based upon hardness, thickness and even curved surfaces may come into play. Additionally, the lack of lubrication or coolant will alter the effectiveness of offhand drilling.

Some guidelines include: Support your workpiece as best you can. The tendency with offhand drilling is to overspeed and under feed, creating heat and premature drill wear and failure. If your tool is variable speed, do your best to keep the speed constant. Drills must be fed relatively hard to take a chip every revolution. Proper alignment is also important. Allow the drill to cut evenly on both cutting lips without deflection. Split points will stop the tendency of the point to "walk" and not center properly. Shorter style drills such as screw machine or stub lengths will work better than longer jobbers length drills. Drills containing cobalt and 135 split points are valuable over 32 Rc hardness.
Thanks and a gift to Robert LeRoy, Manitoba Canada for suggesting we address this topic!

TECHNICAL TIP #87, THREADING: "GUN" TAPS

Gun taps were invented by Greenfield Tap and Die in the early 1900's. They are also known as spiral pointed taps. Gun taps have unique negative gash ground in the front of the tap. This is called a gun shear. The gun shear allows the chips that are cut to curl upon themselves and are "shot" forward, thus, the name gun tap. This is a tremendous advantage in "through" hole tapping to keep the cut chips away from the taps following teeth and flutes.

Gun taps normally have fewer flutes because they are not required for chip storage, allowing a larger core for additional strength. Additionally, gun taps can be run 40% faster than straight fluted or spiral fluted taps.

A gun tap should be run to at least one or two threads above the gun shear to insure that all chips are completely severed and propelled forward.

Gun taps are primarily offered with a plug chamfer only but Greenfield does also offer a bottom chamfer. Greenfield also makes a gun tap with no flutes that is very effective and strong for tapping very thin material less than a one diameter to depth ratio.-Mark Matlock, Technical Specialist

Thanks and a gift to Betty Jacques in Los Alamos, NM for suggesting we write about this topic!

TECHNICAL TIP #88, CUTTING TOOL SAFETY: ENLARGING EXISTING HOLES

Often, we become aware of avoidable injuries suffered from the improper use of cutting tools. One very common injury occurs from attempting to enlarge an existing hole with either one or successively larger drill bits to achieve the desired hole size. This injury is most common when using a portable electric, air or cordless drill. The problem occurs when a 2 fluted drill grabs and wedges itself in the existing hole and the torque of the drill will pulls it out of your closed hand. As the drill body continues to rotate at very high rpm's, it normally strikes the user on the hand and broken bones are the usual result. This happens very quickly and is very violent. Occasionally, if the power tool is large like a " or " chuck capacity, an arm bone can be easily broken.
Solution? Never attempt to enlarge an existing hole with a drill bit. To enlarge an existing hole, use only a 3 or 4 fluted core drill for enlarging to 60% of the hole diameter or a reamer for very slight and precise hole enlarging.

TECHNICAL TIP #89; THREADING; PULLEY TAPS AND EXTENSION TAPS:

We are frequently asked by end-users to provide a "pulley" tap to produce a longer thread length than what is on the tap, but in all cases the standard "pulley" tap has a shank diameter that is greater than the tap major diameter, and therefore cannot be used to produce longer thread lengths without altering the shank diameter. They are indeed great for producing threads where reach is required to get to where the tap begins to thread, but will not normally produce longer lengths of thread.

Hand taps; spiral point, spiral flute, and form taps are all commonly made to USCTI Table 302, or 302A in the United States. All of these taps have shanks that are larger than the major diameter of the thread itself up to and including 3/8". Anything over 3/8' will have a shank diameter that is smaller than the thread major diameter, and therefore can be used for producing threads that are longer than the standard tap thread length.

The truth of the matter is that all pulley taps intentionally have shanks that are bigger than the thread major diameter on the tap thread, because they were originally designed to thread screw holes in pulleys, and the larger shanks were used to guide the tap thru the pulley and into the center of the pulley to be threaded.

Extension taps (4 and 6 inch long) also are nothing but hand, or spiral pointed taps with a longer shank than normal. They also are made for reach. The shanks on all standard extension taps follow the same rules per USCTI table 302. They are supplied with the same size shanks as all other taps of the same sizes, taps 3/8" or smaller must be ordered special to have shanks smaller than the tap major diameter.-Michael Plankey-Senior Technical Specialist

Thanks and a gift to Pete DuBois in Houston for suggesting we write about this topic!

TECHNICAL TIP #90; THREADING; SELECTING THREAD MILL DIAMETERS:

When producing internal threads, selecting the right thread mill diameter insures it will operate efficiently. Thread mills are usually offered in several cutting diameters for a given threads per inch. Smaller diameters are used for small thread sizes, such as 3/8-16 NC. A larger tool diameter could be used for producing a 3/4-16 NF. However, the smaller thread mill could be used to produce the larger 3/4-16 as well.

Generally, for coarser pitches (coarser than 14 TPI), selecting a cutting diameter no larger than 70% of the nominal thread size to be produced is recommended. For finer pitches, the thread mill can be as large as 75% of the nominal diameter. Although the tool has radial clearances similar to end mills, if the tool diameter is too close to the thread diameter, the tool may rub, producing more heat that could result in excessive wear. This rubbing may also distort the thread form affecting the thread angle.

The question is, should the largest thread mill that will fit the hole be used? The answer is, not necessarily! For the greatest efficiency, smaller mills will remove more cubic inch of metal than a larger one, resulting in greater productivity. There will be more clearance for the tool and more space for coolant and chips. However, to optimize the tool, it will be rotating much faster, which may exceed the capability of the machine. Also, the thread length on the tool may be too short for the thread depth required. On the other hand, the larger diameter thread mill will minimize deflection, particularly on coarse thread series, but is more prone to rubbing and chip congestion.-Dave Miskinis; Senior Technical Specialist

TECHNICAL TIP #91; MILLING: SELECTING NUMBERS OF FLUTES:

Flute selection with end-mills offers the same challenges as with drills and taps. Flute selection is normally a matter of compromise between available chip space and strength of the remaining core of the tool. Obviously, deeper and wider flutes make a smaller diameter core cross-section, which becomes sometimes unacceptably weaker. Providing a stronger, thicker core reduces space available in the flutes for chips. Considerations include:

With increasing the number of flutes, you do have the opportunity to increase production. (IPM)
The calculation for this is: RPM X IPT (feed per tooth) x # Flutes (cutting teeth) = IPM
Example: Milling stainless steel 50 SFM at 381 RPM'S at .002 IPT
2 Fluted mill: 381 RPM'S x .002 IPT x 2 Flutes = 1.524 IPM
3 Fluted mill: 381 RPM'S x .002 IPT x 3 Flutes = 2.286 IPM
4 Fluted mill: 381 RPM'S x .002 IPT x 4 Flutes = 3.048 IPM
-Mark Matlock, Technical Specialist

TECHNICAL TIP #92; THREADING; SELECTING COARSE vs. FINE THREADS:

Coarse Threads:

Fine Threads:

Thanks and a gift to Jack Hayse for suggesting this topic!

TECHNICAL TIP #93; DRILLING; DOUBLE FEED DRILLS:

When choosing an indexable drill do you need a good surface finish or do you need high productivity? If you need high productivity start with the double feed drill followed by the square negative drill, positive rake drill and last the spade drill. If you need a good surface finish your first option would be the spade drill followed by positive rake drill, square negative drill and last the double feed drill.

The Double-Feed drill is a two effective-flute drill. This allows feed rates that are double the conventional indexable drills. The Double-Feed drill cuts equally on both inserts, and thus the chip load times two is the feed per revolution. The Metcut line of indexable drills comes in 3:1, 5:1 and 7:1 depth to diameter ratios. It can do stacked material or be used as a core drill.

TECHNICAL TIP #94; THREADING; MULTIPLE LEAD (STARTS) THREADS:

Chances are that when you think of threads you think of threads in which the pitch and the lead are the same. An example would be 1/4-20 with both a .050 pitch and lead. However on a daily basis you may use multiple start threads far more than single start threads. Multiple lead threads are advantageous because they allow far more travel in one turn than single lead threads. Examples are; household faucets and taps, milk bottle caps, toothpaste lids, salt shaker lids etc. Multiple lead threads are very efficient for certain tasks. Normally threads are used to hold things together, multiple start threads are used to easily transfer motion. Threads can be created that allow even 10 times more travel in one rotation than normal. Calculating multiple start threads is simple and expediential; simply add another pitch for each additional lead required.
There is an illustration of multiple leads attached!
Thanks and a gift to Mark Muir in Burbank, CA for suggesting we address this topic

TECHNICAL TIP #95; THREADING; SHORT PROJECTION PIPE TAPS:

Taper pipe taps are used ordinarily for tapping pipe fittings but they also have numerous other applications such as valves, faucets and other components.
Some applications call for a shorter thread lengths because design does not allow for normal lengths. These cases require short projection taps to achieve threads that have very short lengths of engagement. Projection is measured from the small end of an American National Standard L1 thin taper pipe thread ring gage to the small end of the tap.

Greenfield offers both standard and short projection taps from stock. For shallow applications, a standard offering of short projections pipe taps are available which include: Dryseal American National Standard Taper Pipe Thread series, PTF-SAE SHORT, PTF-SPL SHORT and PTF-SPL EXTRA SHORT. These short projection taps are manufactured to produce the NPTF form but can also be used for NPT applications. We also offer special projection taps from our quick delivery Lightning Service.
One Method of determining the projection needed is by having the minimum hole depth available and using the formula and table below.

The formula is:
Min Hole Depth: (L1Length + 2P or pitches + .031) = Projection required or
2 Min Hole Depth - C1 from table = Projection required
Example: -14 NPT with a .700 Min Hole depth: .700 - (.320 + .143 +.031) = .206 Projection

Thanks and a gift to Dwight Carter for suggesting we address this topic!
We need suggestions for topics for future tips, tell us what you want to know about and if we address your topic idea we will send you a gift! To submit a topic, request all past tips or be removed from the list, e-mail don.dejarnette@kennametal.com
Kennametal-Greenfield Technical Support phone at 1-888-GFI-TOOL (434-8665), by fax at 1-888-GFI-FAXX (434-3299)

TECHNICAL TIP #96; THREADING; TECHNICAL BULLETINS:

Did you know? Our technical support group creates very detailed technical bulletins on a variety of threading topics of interest. Each is available via an attachment we e-mail. Most have helpful illustrations, charts or graphs as well as detailed text about the individual topics.

Our current library of technical bulletins is around 50 and growing. For your convenience, I have included a list of bulletins available. Should you ever be in need of one, simply e-mail us and request the bulletin by number. We will reply with the bulletin as an e-mail attachment in Microsoft Word.

TECHNICAL TIP #97; DRILLING; HSS STACKED PLATE DRILLING:

Drilling of tube sheets for heat exchangers is typically done with radial drills, gang drills, vertical boring mills and CNC's. Materials that are drilled range from aluminum to stainless steels.

Stack drilling of 4 plates 1" thick is common and hole sizes vary from " to 1-" and larger.

If you spot drill prior to drilling, it is advisable to spot only 1/3 of the drill diameter or just larger than the chisel width, as you need to have the following drill cut on the outer lips as quickly as possible to maintain a more rounded hole.

The most effective drill used is a thru coolant oil feed drill. Drill construction should be heavy-duty parallel, notched or pre-thinned. The parallel web gives the tool maximum strength and rigidity and decreases spring vibration when drilling deep holes.

Suggested helix would be 35 to 38 to enhance chip evacuation. The pre-thinned point should have a machine ground notch with a positive axial and radial rake to allow unrestricted chip formation and flow. This web also allows accurate centering and reduces thrust necessary to drill the hole.

Most important is to control the chip, If your material is gummy or ductile and you are producing long stringy chips, we would suggest checking your feeds and speeds. If they are within recommended range and bird nesting is still present, increase speed by 10% and feed by 25%. If this action fails, look into a chip breaker drill or changing the rake angles of the point.

Coolant is an integral part of drilling. Adequate coolant pressure keeps the drill point cool and helps evacuate chips as fast as possible and create a smoother hole. Coolant backpressure floods the chip back up the spiral. When using soluble oil it is recommended to use an 8% to 10% mix for effective cooling and lubrication. Coolant pressure can range from 100 to 200 psi but make sure that the part is also flooded.

Helical or racon points will improve performance but most times cannot be reproduced in-house for regrinds. Coatings are another technical advance in today's drilling but make sure your machines are capable for higher feeds and speeds to take advantage of their properties. Special double margin drills may also eliminate the following ream step.
-John Woodbridge, Sr. Technical Specialist

TECHNICAL TIP #98; DRILLING; DOUBLE FEEDING DRILLS:

The "double-feed" drill is a two effective drill, having both opposing carbide inserts and flutes 180 apart. This allows feed rates that are double that of a conventional indexable single feed drill. This is possible because the drill inserts cut equally on both inserts and also cut to center, which is unique.

These Metcut indexable drills are available in 3:1, 5:1 and 7:1 depth to diameter ratios. It can drill stacked materials and also can be used as a core drill to enlarge existing holes.

Productivity or finish quality? If you need high productivity, choose the Double Feed Drill followed by the Square Negative Drill, Positive Rake Drill and last the Spade Drill.

If you need a good surface finish your first option would be the Spade Drill followed by Positive Rake Drill, Square Negative Drill and last the Double Feed Drill.
-Lonnie Stewart, Technical Specialist

TECHNICAL TIP #99; THREADING; THREAD MILL CHECKLIST:

Thread milling continues to be a hot topic for Greenfield. This tip reviews advantages and situations where thread mills are a viable consideration.
Features and benefits:

When to consider thread milling:

TECHNICAL TIP #100; CARBIDE BURS; SELECTION AND USE

Burs are sometimes referred to as rotary files and come in many shapes and sizes. Typical applications are weld preparation, weld smoothing, deburing, chamfering, deflashing, and scale removal. Burs are typically chucked in air driven die grinders and used in hand operations.
Bur Selection:

Use Of Burs:

Vendor Selection:
When selecting a vendor for burs, users should look for suppliers with modern up to date CNC equipment. In the past burs were hand ground and very inconsistent in quality, and performance. Today burs from top tier manufactures are made on CNC machines designed specifically for grinding burs. They are very high quality and consistent from lot to lot. –David Ford, Sr. Technical Specialist

TECHNICAL TIP #102; THREADING; TAP HOLDERS:
Selecting the right tap holder depends upon the equipment to be used for tapping.  Machines not capable of accurately feeding a tap through the entire feed/retract cycle, including hand feed, cam, gear, hydraulic or air tappers, or conventional drill/mill/turn CNC machine, should use axial float holders.  The most common have both tension and compression float that allow the tap to compress within the holder or pull out to allow the tap to follow its own lead to compensate for the feed errors in the machine.

If the hole in the part has been cast, punched or drilled in another machine or station, radial float holders are recommended.  Radial float holders allow the tap to move off-axis while maintaining parallelism to the spindle axis.  Holders are available that combine axial and radial float to provide both axial and radial movement of the tool.

If tapping is performed on lead screw tappers or machines that have synchronous or rigid tapping capability, the feed in these types of machines is far more accurate, allowing the use of solid holders.  This would include collet, shrink fit, or hydraulic holders.  Collets should be selected that are specifically designed for taps.

The newest holders are a floating type specifically designed for rigid or synchronous type machines.  They provide approximately .015” of minimal float to compensate for slight errors that exist within any synchronized system.  This slight movement compensates for any possible feed errors in the machine or lead error on the tap, to insure the tap operates to peak efficiency.

Self-Reversing holders do not require the spindle to reverse to retract the tap from the hole.  They are used when the spindle cannot reverse or to prevent wear and tear from the constant cycling for those that do.  They also allow higher tapping speeds for smaller diameter taps, where the recommended RPM may exceed the tapping speed of the spindle.  In this case, since the spindle is not reversing, the full speed available for drilling can be used for tapping. Dave Miskinis, Sr. Technical Specialist
Thanks and a gift to Ron Christiaens in British Columbia for suggesting we write about this topic!

TECHNICAL TIP #103; THREADING; USING LARGER OR SMALLER H-LIMITS:
In the Tech Tip #22, “H Limits and Classes of Thread” we discussed selecting the recommended “standard” H Limit for the various classes, 2B, 3B, etc.  However, there are situations when larger or smaller H limits would be more appropriate.
Larger H limits: The primary reason for using larger H limits is for plated or heat-treated parts.  In both cases the thread must be made larger (and sometimes oversize) to accommodate the reduction in size due to the plating thickness or heat shrinkage.
Selecting an H limit for plated parts is relatively easy.  Using the plating thickness, the oversize pre-plate thread dimensions can be calculated.  Then, using the “40% rule”, the H limit for the oversize thread can be calculated.
Selecting a larger H limit for heat-treated parts is more difficult and generally requires trial and error due to the fact that different materials and part configurations shrink by varying amounts.

Another reason for larger H limits is part configuration.  If the part is very thin walled, the tap may expand the part when cutting, but will close in once the tap is removed.  Again, trial and error is required to find the appropriate H limit size.

The final reason for using larger H limits is extremely important but seldom used.  A larger tap will allow for more tool wear, producing more parts!  When the tapping operation is very consistent, the largest H limit that will provide good gaging with the NOT GO thread plug can be used for greater productivity.

Smaller H Limits: Generally, the only time a smaller H limit is used is to overcome problems with the process that would result in an oversize thread, such as runout, misalignment, or improper feed of the tap.  However, this technique is usually used as a temporary “band-aid” fix, until a permanent solution can be employed.
Also, small or undersize H limit taps are occasionally used for parts that require a tight or smooth, slop free fit between the mating threads.-Dave Miskinis, Sr. Technical Specialist
Thanks and a gift to Os Taylor in Danville, VA for suggesting we write about this topic!

We always need suggestions for topics for future tips, tell us what you want to know about and if we address your topic idea we will send you a gift! To submit a topic, request all past tips or be removed from the list, e-mail don.dejarnette@kennametal.com

Technical Tips Courtesy of Kennametal-Greenfield Technical Support