Starter kit

Author Cutting Tool Engineering
June 01, 2012 - 11:15am

Everyone has spot drilled at some point to start a hole. For a tight-tolerance hole, spotting is required to prevent the secondary drill from walking (the amount the tool deflects from a straight path). Spot drilling creates a location for the secondary drill to enter, acting as a guide.

A spot drill is short and rigid, with a very short flute. It has just enough point geometry to drill an indent in the workpiece. The web on most spot drills is thin, creating a chisel edge with an efficient cutting action.


The spot drill is taken deep enough to create the desired chamfer diameter while spotting the hole. Image courtesy 2L.

“The chisel edge is the very center of the drill where the two flutes leave a little bit of material between the two of them,” said Bob Hellinger, national sales manager, standard products for Guhring Inc., Brookfield, Wis. “That chisel edge doesn’t cut—it tends to push the material. Drills with large chisel edges wander more than drills with reduced chisel edges. A spot drill has a very thin chisel edge.” Guhring offers HSS and carbide spot drills.

Drills with split points reduce the need for spot drilling. “A split-point drill is self-centering in that the chisel edge is reduced to almost zero,” Hellinger said. “However, the split point is a little harder to apply in manufacturing. Drills with a 135° point angle often have a split point because they are recommended for harder materials.”

The higher the length-to-diameter ratio of a drill, the more apt it is to walk. A long drill can deflect when it initially contacts a flat surface, making spot drilling necessary. Some drill makers agree that for holes more than 5 diameters deep, spotting is needed. Others say that threshold is 7 or 8 diameters deep or more.

“Spot drilling also may be used if you are not drilling into a flat surface, say into a 10° to 15° angled surface or a large radius,” said Ben Davis, national product manager for drilling, Iscar Metals Inc., Arlington, Texas. “The spot drill can slightly flatten that area before you do the drilling.” He added that other tools, such as an endmill, can also flatten a surface.

Chamfering Holes

Spot drills are also applied for chamfering a hole prior to drilling. The spot drill is taken deep enough to create the desired chamfer diameter while spotting the hole. “You can create a spot to start the secondary drill and produce a chamfer at the top of the hole in one step,” said Brad Gray, application engineer for Allied Machine & Engineering Corp., Dover, Ohio. “Spot drilling a little deeper creates a larger diameter than that of your secondary drill. Then, when you come in with that smaller diameter secondary drill, the larger diameter chamfer is at the top of the hole.”


A spot drill, like this one from Guhring, is short and rigid, with a very short flute. Image courtesy Guhring.

Many machinists use a spot drill to create a chamfer when they will be tapping or reaming a hole. “The chamfer allows for a smooth lead into the hole,” said Susan Valenti, product manager–holemaking for Ingersoll Cutting Tools, Rockford, Ill. Ingersoll’s Y-Series quick-change, replaceable-tip, extended-length spot drills are offered in 90° and 140° styles.

Point Angle

Some users aren’t sure what the point angle of the spot drill should be compared to the secondary drill. “Everyone takes it for granted that it is understood, but people do ask us a lot what angle to use,” said Lance Nelson, president of 2L inc., Hudson, Mass., which sells solid-carbide spot drills with 90°, 120° and 145° point angles.


A spot drill has a very thin chisel edge compared to a standard drill. The chisel edge does not cut material; it pushes or displaces it. Image courtesy Guhring.

“Secondary drills typically have point angles of 118°, 120° or 135°, and some stronger ones are wider than that,” he continued. “Some people use the 145° spot drill for a 135° point-angle drill. When you get into tougher materials like stainless or Inconel, it takes more of a toll on the secondary drill, so it’s important to use the 145° spot drill. However, most people just use whatever they have in their shop—such as a 90° spot drill for any application.” 

Most toolmakers agree the point angle of the spot drill should be equal to or larger than the secondary drill’s angle. The drill should make contact with the starter hole at the drill’s tip, not its cutting edges. This eliminates undue stress on the drill’s edges, which would cause premature tool failure and reduce hole quality.

Nelson said: “You want the spot drill to have a larger point angle so when the secondary drill goes in, its tip touches the bottom of the hole and finds the center. Then, as the drill plunges into the hole, its edges contact the hole edges at the same time. It prolongs the life of the secondary drill.”

Another method is to use the same point angle for the spot and secondary drill. Then, the secondary drill’s tip and cutting edges engage the workpiece at the same time. “Personally, I don’t recommend it,” Nelson said. “There is a chance of chattering because you have an identical angle touching an identical angle. Chattering can cause the secondary drill to chip.”


In addition to spotting, Ingersoll’s Spot-In FAK indexable tools can be used for engraving. Image courtesy Ingersoll Cutting Tools.

Guhring’s Hellinger said the rule of thumb that the spot drill should be flatter than the secondary drill is true in terms of carbide drills. “However, for HSS and cobalt secondary drills, you want the cutting edges to engage the workpiece before the chisel edge (tip) of the drill,” he said. “On an HSS drill, the cutting lips aren’t as fragile as on a carbide drill, so you want to contact the cutting edges before you contact the chisel edge. The chisel edge, again, doesn’t cut so it will skate or wander if it engages the workpiece first.”

For carbide drills, the opposite is true. “Carbide drills tend to have reduced chisel edge designs, and you do not want to engage the cutting edges due to the brittleness of the carbide,” he added. “Therefore, a spot drill with a greater point angle is recommended so the chisel edge engages in the cut before the cutting edges.”

So, are the speeds and feeds for spot drills the same as the secondary drill? “Proper speeds and feeds depend on the workpiece material, insert substrate and coating, as well as the drilling application itself,” Allied’s Gray said. “Generally, spot drilling utilizes slight reductions in surface feet per minute and reduced feed rates. Your goal when spotting is to provide a good starting location for the secondary drill, so you really don’t need the high penetration rate. Just give the drill a chance to establish and run true.”


 Iscar’s SumoCham drill features interchangeable carbide bits that can be used for spot drilling and chamfering. Image courtesy Iscar Metals.

No Spot

Most solid-carbide drills typically do not need a starter hole because they are rigid and resist walking. Most are self-centering; they are designed to start their own hole. Spot drilling the workpiece before using this type of drill may even be counterproductive, causing the edges to chip or break.


Allied offers Super Cobalt 90° indexable spade drills in a variety of diameters for spotting and chamfering. Image courtesy Allied Manufacturing & Engineering.

“Most modern solid-carbide drills have thin chisel edge designs similar to split points,” Guhring’s Hellinger said. “They are reduced to eliminate the chisel edge or, for example, some have a helical point style where the chisel edge actually cuts. It has that to eliminate the need for spot drills.”

If required, Gray recommends creating a shallow spot for a solid-carbide secondary drill. “Measure the web of the carbide drill and use this thickness as the spot drill depth,” he said. “This provides a small spot to guide the secondary drill without placing it under excessive stress.”

Center Instead?

Shops sometimes use a center drill to make spot holes, but the drills are not designed for that. The purpose of a center drill is putting a hole in the end of a part to secure it in the tailstock of a lathe or to mount it between centers for grinding.

“Center drills are combination drill and countersink tools, which are not the best tool for spot drilling,” Hellinger said. “They are actually a step drill and create two different spot angles—a 60° pilot hole with a 90° countersink on the top. The secondary drill encounters the countersink angle at the top of the starter hole and then a different angle at the bottom of the hole created by the pilot portion of the center drill. This creates an opportunity for the secondary drill to wander.” 

More than a Spot

Spot drills have evolved and are no longer “just spotting tools,” according to Valenti. For instance, Ingersoll’s Spot-In FAK indexable spotting tools are offered in 82°, 90°, 118°, 135° and 140° styles for a variety of operations: spot drilling, countersinking, engraving, chamfering and edge deburring. 


A center drill (top), which is usually double-ended, is sometimes used for spot drilling but is not as accurate as a true spot drill (bottom). Image courtesy Guhring.

Iscar also offers tools with interchangeable carbide bits, such as the SumoCham drill or the Multimaster, which is intended more for milling but can perform chamfering and spot drilling. “However, we recommend you create more of a prehole than a starter hole,” Davis said. “Basically, you prehole with a short drill about 1 diameter deep. A prehole is within an H8 tolerance of the secondary drill with a drill point the same size or larger than the secondary drill. The prehole supports the drill margin as well as the point.

“We recommend taking the drilling tool and putting chamfering bits on it,” Davis added. “The drill will be a step drill with a drilling insert on the end and chamfer inserts toward the back of the drill, allowing for drilling and chamfering/counterboring with one tool.”

As cutting tool technology improves, spot drills are becoming less important because users can drill straight holes 
with longer drills. Allied’s Gray agreed and noted the high quality of today’s 
tools and machines often eliminates the need for spot drilling, reducing cycle times and tool inventories. “But, again, it depends on the application. You have to ask yourself if a spot drill is really needed.” CTE

About the Author: Susan Woods is a contributing editor for CTE. Contact her at (224) 225-6120 or


Allied Machine & Engineering Corp.
(800) 321-5537

Guhring Inc.
(800) 776-6170

Ingersoll Cutting Tools
(866) 690-1859

Iscar Metals Inc.
(877) BY-ISCAR

2L inc.
(978) 567-8867

Related Glossary Terms

  • center drill

    center drill

    Drill used to make mounting holes for workpiece to be held between centers. Also used to predrill holes for subsequent drilling operations. See centers.

  • centers


    Cone-shaped pins that support a workpiece by one or two ends during machining. The centers fit into holes drilled in the workpiece ends. Centers that turn with the workpiece are called “live” centers; those that do not are called “dead” centers.

  • chamfering


    Machining a bevel on a workpiece or tool; improves a tool’s entrance into the cut.

  • countersink


    Tool that cuts a sloped depression at the top of a hole to permit a screw head or other object to rest flush with the surface of the workpiece.

  • countersinking


    Cutting a beveled edge at the entrance of a hole so a screw head sits flush with the workpiece surface.

  • drilling tool ( drill or drill bit)

    drilling tool ( drill or drill bit)

    End-cutting tool for drilling. Tool has shank, body and angled face with cutting edges that drill the hole. Drills range in size from “microdrills” a few thousandths of an inch in diameter up to spade drills, which may cut holes several inches in diameter. Drills may have tapered shanks with a driving tang and fit directly into a spindle or adapter, or they may have straight shanks and be chuck-mounted. The rake angle varies with the material drilled. Styles include twist drills, straight-flute drills, half-round and flat drills, oil-hole drills, indexable drills and specials.

  • endmill


    Milling cutter held by its shank that cuts on its periphery and, if so configured, on its free end. Takes a variety of shapes (single- and double-end, roughing, ballnose and cup-end) and sizes (stub, medium, long and extra-long). Also comes with differing numbers of flutes.

  • feed


    Rate of change of position of the tool as a whole, relative to the workpiece while cutting.

  • flat ( screw flat)

    flat ( screw flat)

    Flat surface machined into the shank of a cutting tool for enhanced holding of the tool.

  • flutes


    Grooves and spaces in the body of a tool that permit chip removal from, and cutting-fluid application to, the point of cut.

  • gang cutting ( milling)

    gang cutting ( milling)

    Machining with several cutters mounted on a single arbor, generally for simultaneous cutting.

  • grinding


    Machining operation in which material is removed from the workpiece by a powered abrasive wheel, stone, belt, paste, sheet, compound, slurry, etc. Takes various forms: surface grinding (creates flat and/or squared surfaces); cylindrical grinding (for external cylindrical and tapered shapes, fillets, undercuts, etc.); centerless grinding; chamfering; thread and form grinding; tool and cutter grinding; offhand grinding; lapping and polishing (grinding with extremely fine grits to create ultrasmooth surfaces); honing; and disc grinding.

  • high-speed steels ( HSS)

    high-speed steels ( HSS)

    Available in two major types: tungsten high-speed steels (designated by letter T having tungsten as the principal alloying element) and molybdenum high-speed steels (designated by letter M having molybdenum as the principal alloying element). The type T high-speed steels containing cobalt have higher wear resistance and greater red (hot) hardness, withstanding cutting temperature up to 1,100º F (590º C). The type T steels are used to fabricate metalcutting tools (milling cutters, drills, reamers and taps), woodworking tools, various types of punches and dies, ball and roller bearings. The type M steels are used for cutting tools and various types of dies.

  • lathe


    Turning machine capable of sawing, milling, grinding, gear-cutting, drilling, reaming, boring, threading, facing, chamfering, grooving, knurling, spinning, parting, necking, taper-cutting, and cam- and eccentric-cutting, as well as step- and straight-turning. Comes in a variety of forms, ranging from manual to semiautomatic to fully automatic, with major types being engine lathes, turning and contouring lathes, turret lathes and numerical-control lathes. The engine lathe consists of a headstock and spindle, tailstock, bed, carriage (complete with apron) and cross slides. Features include gear- (speed) and feed-selector levers, toolpost, compound rest, lead screw and reversing lead screw, threading dial and rapid-traverse lever. Special lathe types include through-the-spindle, camshaft and crankshaft, brake drum and rotor, spinning and gun-barrel machines. Toolroom and bench lathes are used for precision work; the former for tool-and-die work and similar tasks, the latter for small workpieces (instruments, watches), normally without a power feed. Models are typically designated according to their “swing,” or the largest-diameter workpiece that can be rotated; bed length, or the distance between centers; and horsepower generated. See turning machine.

  • milling


    Machining operation in which metal or other material is removed by applying power to a rotating cutter. In vertical milling, the cutting tool is mounted vertically on the spindle. In horizontal milling, the cutting tool is mounted horizontally, either directly on the spindle or on an arbor. Horizontal milling is further broken down into conventional milling, where the cutter rotates opposite the direction of feed, or “up” into the workpiece; and climb milling, where the cutter rotates in the direction of feed, or “down” into the workpiece. Milling operations include plane or surface milling, endmilling, facemilling, angle milling, form milling and profiling.

  • point angle

    point angle

    Included angle at the point of a twist drill or similar tool; for general-purpose tools, the point angle is typically 118°.

  • tapping


    Machining operation in which a tap, with teeth on its periphery, cuts internal threads in a predrilled hole having a smaller diameter than the tap diameter. Threads are formed by a combined rotary and axial-relative motion between tap and workpiece. See tap.

  • tolerance


    Minimum and maximum amount a workpiece dimension is allowed to vary from a set standard and still be acceptable.

  • web


    On a rotating tool, the portion of the tool body that joins the lands. Web is thicker at the shank end, relative to the point end, providing maximum torsional strength.