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.

Peek 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 A peck cycle is where the entire drill is periodically withdrawn from the hole to remove chips, and then re-entering the hole to drill a small distance and withdrawing the drill again until the full hole depth is reached.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 parabolic flute forms can also be used to drill deeper holes without peck drilling.

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.

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.

Use of Spotting Drills

Spot drills are commonly found in 90º and 120º point angles, while most drills come with 118º and 135º 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 90º point angles are used when you want to pre-chamfer the hole, and should only be used with HSS or cobalt drills.

120º spot drills to precede either 118º or 135º 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 120º spot angle is ideal for a carbide drills with a 118º drill point.  A 140º spot angle for carbide drills with 135º points is also ideal.

Drilling Inclined Surfaces

Drilling on inclined or curved surfaces can generally be accomplished by a reduction in feed. After the drill tip has penetrated past the incline or curve then feed rate can return to normal. Jobber length drills will need a greater reduction in feed than stub length drills.

Incline          Stub            Jobber
    1°                0%                30%
    2°               20%              40%
    3°               35%              50%
    4°               50%
    6°               70%

Incline angles or curves more than 6° must be spot drilled or milled flat. Drills should always have self-centering point geometry when used on any irregular, inclined, or curved surface.

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.

1.     Removal of Worn Section: Wear on the outer corners will appear as a slight rounding. You will see a reaction of wear on the cutting lips and on the chisel-edge. This then forms a conical surface and if continually used will only rub in the cavity rather than cut. With this condition of wear on the point, the horsepower and thrust increases which in turn increases wear at a faster rate. The next step in wear will appear along the margins this could result in loss of size. To resharpen a tool in this condition you will have to remove all of this worn section.  Assuming that you are cutting off ¼” to ½” of worn material with an abrasive cut off wheel, care is needed not to burn the high-speed steel.  If this happens you will lower the hardness by about  5Rc points, softening the steel and resulting in a dramatic loss of performance.

2.     Web Thinning: Most standard drills have webs, which increase in diameter all the way to the shank end.  As the drill is resharpened the web will get thicker and web thinning is necessary.  Web thinning done on a tool and cutter grinder or CNC for accurate control. The same amount of stock should be removed from both sides to ensure web centrality. If web centrality is incorrect you can cause rapid wear failure and an out-of-round hole.  Free cutting wheels should be used so as not to burn the cutting edges.  The contour of the flute should be blended in with the original web shape so as to not hinder chip flow.

3.     Drill Pointing: This is the most critical operation in drill re-sharpening. The two cutting lips of a drill should be accurately ground to equal angles and equal length.  If your drill point has lips of equal length but at unequal angles or vise versa, one cutting edge will do most of the cutting and will cause an oversize condition, excessive wear and short tool life.

4.     Lip Relief Angles: The lip relief angle is the angle measured across the margin at the periphery of the drill.  This angle has a bearing on the amount of clearance to obtain the correct chisel edge angle.  When grinding the lip relief angle, both sides should be on the same plane.  In general, the diameter of the tool dictates what that angle should be.  Fragile small diameter tools require larger clearance angles to help them penetrate.  For instance, a #80-#61 would have an angle of 24°, a ¾” tool would be about 8° to 10°.  Material hardness also plays here, if drilling harder materials, reduce angles by 2° and increase for softer materials by 2°.

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

Tap Hook and Relief

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 these 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 a 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.

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.

Longer Lengths of Engagement

ASME B 1.1 allows the use of larger drill sizes dependent upon the depth of the hole to be threaded.  This can be a great advantage for minimizing tapping problems as well as extending tool life.  Allowances are for 1/3 to 2/3’s diameter, 2/3’s to 1-1/2 diameter and 1-1/2 – 3 times diameter.  These specific sizes can be found at the top of each page of the Greenfield Screw Thread Manual (EDP GI 039) for each tap size or by contacting Technical Support.

Drill Formula for Metric Taps

The formula is Basic Major Diameter Minus the Pitch = Hole Size.  For example, a M5 X 0.8 thread would be calculated as follows:  5.00mm minus 0.80mm = 4.20mm hole size.  Simply select the nearest available drill size.  The hole produced would yield approximately 70%-75% percentage of thread.