The lips cut; the flutes give chips a way out

A twist drill makes a round hole with cutting edges at its point. The lips run from the center region toward the outside diameter. The helical grooves are flutes: they provide space for chips and a route for cutting fluid. The web is the central core between the flutes.

The chisel edge crosses the center of a conventional point. It pushes material aside with substantial thrust. Narrow strips called margins run along the outside of the drill body and help guide it in the hole. The relieved body behind them reduces rubbing. The shank is the portion held by the machine.

Point angle and split point describe different features

118° and 135° are included point angles, measured across the point in an axial view. A 135° point is flatter and shorter than a 118° point of the same diameter. A 118° point is common on general-purpose drills; 135° points are common on drills intended for tougher materials. Select the complete tool for the material and setup, not by angle alone.

A split point has extra grinding near the center to reduce the chisel edge and improve starting behavior. “135°” does not automatically mean “split point.” A split point is also not a guarantee that the hole will be located accurately without a suitable setup.

Supporting detail: Addendum 1 — Why a damaged or uneven point makes a poor hole.

Read the diameter system before selecting the drill

Read the marking and confirm the cutting diameter when identification is uncertain. A drill index is storage, not proof that someone returned the drill to the correct slot. Use the specified diameter and a checked chart when selecting a tap drill.

Match the shank to the holder and the hole to the job

A straight shank fits an appropriate chuck or collet. A reduced shank is smaller than the cutting diameter; it does not increase the machine's drilling capacity. A taper shank fits its matching taper socket or approved adapter, rather than being gripped as though it were a straight shank.

Choose enough flute length and reach for the hole, with as little unnecessary projection as the setup permits. A drill's nominal diameter does not guarantee a finished hole's size, location or surface finish. Plan the drilling sequence, then choose a finishing operation if the drawing calls for it.

Locate and secure the work before starting a hole

A drill press feeds a rotating drill along its spindle axis. A mill adds controlled table positioning, which helps place a pattern of holes from drawing datums. On either machine, the hole follows the relationship between spindle, tool and workholding.

Clamp the work or hold it in a suitable vise or fixture rather than by hand; see Machine Hazards for why. Round stock needs support that prevents rolling, such as a properly clamped V-block arrangement. Provide clearance for a through drill without drilling into the table, vise or supports.

For the operating rules, use Machine Hazards and Housekeeping, Personal Protective Equipment and Metal Chips and Swarf. The sequence here assumes those requirements and the machine's operating instructions have been met.

A spot starts the hole; a pilot removes the center material

Spot drilling makes a short starting feature to help locate the next drill. A center drill is primarily designed to produce a center hole for supporting work between centers; its small pilot and conical portion make it different from a spot drill. Select a starting tool compatible with the following drill, rather than treating the two tools as interchangeable.

A pilot hole is a smaller hole drilled before a larger one. It can reduce the thrust required at a conventional drill's chisel edge. It is not automatically required: some drill geometries are intended to enter solid material. Follow the drill maker's starting-hole and pilot recommendations.

Supporting detail: Addendum 2 — Why “always center drill first” is too broad.

Choose speed and feed for this drill and material

Use Feeds, Speeds and Removal Rate for the surface-speed-to-RPM calculation. For drilling, its diameter input is the drill's cutting diameter. Surface speed is a cutting condition; RPM is the spindle setting. They are not the same quantity.

Feed per revolution describes how far the drill advances each turn. Select cutting data for the tool material, work material, diameter, depth and coolant arrangement. A generic material table is a starting reference only when its tool assumptions match. Use an available machine setting consistent with the tool and machine instructions.

Practice drill RPM

Plan chip evacuation and full-diameter depth

Peck drilling advances in stages with retractions to break or evacuate chips. The needed stroke and retraction depend on the drill, material, hole depth and fluid delivery; there is no universal peck distance. Do not add a peck cycle to a tool that calls for continuous feed without checking its instructions.

For a blind hole, distinguish the depth reached by the tip from the depth that has the full drill diameter. The conical point extends beyond the full-diameter portion. A tapped blind hole also needs space for the tap's lead-in and chip clearance. For a through hole, account for breakthrough and the drill point below the work.

If chip shape, sound, thrust or finish changes unexpectedly, stop and inspect the setup before resuming; use Metal Chips and Swarf for chip handling.

Supporting detail: Addendum 3 — Why changes in the cut matter.

Compare advance, retracing and withdrawal paths

Open G-code and Toolpaths. In the playground's Program picker, choose these named examples in order: Drilling path: continuous advance, Drilling path: short in-bore retract, and Drilling path: withdrawal above the mouth. Use Step to follow each G0 and G1 move.

1. Mark where the drill enters material that has not yet been removed. That is new cutting in this geometric model.
2. Mark where the drill returns through the bore it already made. That travel retraces the prior path and removes no additional modeled stock; the separate deeper feed begins after the point reaches the previous bottom. The model does not show possible wall or chip contact, rubbing, force or heat during the return.
3. Compare the retraction heights with the raw top at Z+1. The short retraction stays inside the bore. The other withdrawal carries the point above the hole mouth, creating a clearer opportunity for chips to leave the hole.
4. Compare the finished holes. The three illustrative programs intentionally reach the same final tip depth and geometry even though their travel paths differ.

The playground shows programmed motion and removed geometry. It does not model chip transport or packing, cutting heat or force, coolant delivery, or whether chips actually cleared. A retraction creates an opportunity for chip escape; it is neither proof of chip clearance nor the only way chips can leave. Haas describes its G83 return as a chip-clearing motion and places the R plane above the cut so chips can get out, but these G0/G1 illustrations are not G73, G83 or Q implementations.

The coordinates, spindle speed and feed in these three examples are comparison values for the simulator, not operating recommendations. Select any real drilling cycle, retract amount, speed and feed from the drill maker's guidance, the machine/control manual and the approved shop procedure. Continue to follow the machine instructions and Metal Chips for observation and chip handling.

Primary source: Haas Automation, G83 Normal Peck Drilling Canned Cycle (R-plane return and chip-clearing motion). Controller details differ; use the manual for the machine in front of you.

Read point depth and full-diameter breakthrough separately

Open Milling Operations and its simulator. Choose Job 2 / Pocket and holes. From View, choose 2D sections. Under Drill: choose a size, choose Load the drill Ø6.6. With the tool clear above the block, use the Move to X and Y inputs to place it at X 15, Y 30, then use the Z input and Move to advance to each row below. Watch the Front section and DRO, then scroll to Inspection of the part as it is now and find Ø6.6 through at X 15, Y 30.

These are illustrative coordinates in this simulator: its raw top is Z +1 and its stock bottom is Z −20. They are not operating depths, safe overtravel or an allowance for a real part.

1. Why does a drill-tip DRO of Z −20 not mean the full Ø6.6 body has reached Z −20?
2. Which inspection result changes between Z −21 and Z −22: the measured diameter, the THRU subcheck, or both?
3. Why can the left hole's diameter subcheck pass before its THRU subcheck?
4. Why can the feature row or overall job remain incomplete even after this THRU subcheck passes?

For this feature, THRU checks the bottom opening against a minimum allowed diameter of 6.50 mm. Passing it does not guarantee an exact Ø6.6 opening, and the unfinished top face, pocket or right-hand hole can keep other checks incomplete. Read the Diameter and THRU subchecks separately; do not use the overall job result as the answer to this comparison.

Choose the operation from the finished shape

Ream for size and finish; bore when the axis needs control

A reamer removes a small amount of material with multiple cutting edges. Prepare an undersize hole with enough material for the reamer to cut, rather than rub. Too much allowance overloads the tool; too little may leave the previous surface. Use the reamer maker's allowance for that diameter and material, not one stock allowance for every hole.

A reamer tends to follow the existing hole. Do not rely on it to relocate a badly misplaced or crooked hole. Boring enlarges an existing hole with a cutting edge whose path can be set relative to the machine axis. With a suitable setup and enough material left to clean up, it can correct location and straightness as well as diameter.

Use Tolerances and Fits to interpret the size limits and select inspection methods. See Lathe Operations for boring and threading on the lathe.

Supporting detail: Addendum 4 — A nominal tool size is not a finished-hole guarantee.

Compare the old opening with the final bore envelope

A centered final bore can remove material around a smaller opening when that entire opening lies inside the final bore's removal circle. It cannot add material back where an earlier opening protrudes outside that circle. Setting the boring head to the drawing diameter does not erase the earlier geometry.

Open Milling Operations and choose Job 4 / Boss and bore. From View, choose 2D sections. Before each case, choose Start this job over, then Sure? Start over, so each comparison begins with a fresh block. Use the Move to X, Y and Z inputs and Move. Keep tool and boring-head changes at Z +20 by using Raise to Z +20.

1. In the first case, where is the edge of the Ø10 opening relative to the centered Ø20 removal circle?
2. In the second case, which individual checks show that the result is not simply a centered Ø20 hole: diameter, position, overcut, or all three?
3. Why does a final DRO of X 50, Y 30 not undo the earlier off-axis removal?

These coordinates, depths, offsets and fitted/grid inspection numbers belong only to this idealized simulator. They are not acceptable cleanup allowance, safe boring offset, rework instructions or physical gauge results. The model does not predict boring-bar entry or interrupted-cut behavior, rigidity, deflection, chatter, force, finish, alignment uncertainty or workholding. Geometric containment is necessary here, not sufficient for a real process: use the drawing, measured hole, complete setup, tool-maker guidance and responsible process authority.

The top, boss and chamfers remain unfinished in both cases, so the overall feature row or job may still be incomplete. Read the bore's diameter, position and overcut checks for this comparison.

Match the head seat to the fastener drawing

A counterbore has a cylindrical wall and a flat shoulder. A countersink has a conical seat. The screw head must match that seat's included angle; the thread diameter alone does not determine the head angle or the countersink diameter.

A spot face removes enough surface material to create a local flat seat for a head, nut or washer. It is useful on a rough or uneven surface. A spot face and a counterbore may use similar tools, but their required depth and purpose differ.

Read the specified diameters, depths and angle before cutting. A tool used only to break a sharp edge is not necessarily producing a fastener seat to size. Do not substitute a preferred cutter angle for the drawing requirement.

Test the choice before choosing the cutter

A smooth pin hole already on location suggests reaming. A hole whose axis must be corrected suggests boring, if there is enough material. A socket-head screw recessed into a cylindrical pocket suggests counterboring. A conical flat-head seat suggests countersinking.

Practice choosing hole operations

Read diameter, spacing, series and class separately

In 1/4-20 UNC-2B, 1/4 is the nominal major diameter in inches, 20 is the number of threads per inch, UNC is the Unified coarse series, and 2B identifies the internal thread's fit class. The major diameter is the largest thread diameter; it is not the diameter of the hole drilled before tapping.

UNF identifies the Unified fine series. At a given nominal diameter, fine threads have more threads per inch and therefore a smaller pitch than coarse threads. In M6 × 1, M identifies a metric thread, 6 is the nominal major diameter in millimeters, and 1 is the pitch in millimeters. It does not mean one thread per inch.

Practice reading a callout

Thread class controls fit, not fastener strength

Unified external thread classes are 1A, 2A and 3A; internal classes are 1B, 2B and 3B. A means external, as on a screw; B means internal, as in a tapped hole. Class 1 permits a looser fit, class 2 serves general applications, and class 3 uses closer dimensional control.

The class number is not a material grade or a load rating. A class 3 thread does not by itself make a stronger bolt. Read the drawing for the required class and use the appropriate inspection limits. M6 × 1 alone does not specify a metric tolerance class; do not append an inch A/B class to it.

For the general distinction between a nominal dimension, its tolerance and a mating fit, see Tolerances and Fits. Exact thread acceptance limits require the applicable specification and gauges.

Pitch is spacing; lead is travel per revolution

Pitch is the axial spacing between adjacent thread crests. For an inch thread, pitch in inches = 1/TPI. A 20-TPI thread has a pitch of 0.050 in. Lead is the axial travel in one complete relative revolution.

On a single-start thread, lead equals pitch. On a multiple-start thread, lead equals pitch times the number of starts. Right- and left-hand threads move in opposite axial directions for the same rotation. Look for a left-hand designation rather than forcing a fastener that does not start normally.

The lathe topic owns the process of single-point thread cutting. The tapping topic explains preparing and making internal threads with taps.

Choose the fastener by how it locates and clamps the parts

Engagement, grade and locking are separate decisions

Engagement length is the axial length of mating threads carrying load. There is no single diameter multiplier that establishes adequate engagement for every combination of screw and parent material. Use the joint design or fastener-system requirements, and ensure the screw does not bottom before it clamps.

Strength identification must come from the specified fastener grade or property class and its traceable markings or documentation. Thread fit class and head style are not substitutes. Do not assign a strength grade to an unidentified fastener from its appearance.

A flat washer is not a locking device. A lock washer or thread-locking compound is not a guarantee against loosening in every joint. Use the specified locking method; for a compound, follow its compatibility, preparation, cure and removal instructions.

Supporting detail: Addendum 5 — Check the entire joint before substituting a fastener.

Subtract the pitch to estimate a cutting-tap drill

A tap makes an internal thread in a prepared hole. Start by reading the full thread callout. For common straight Unified and metric cutting taps, a useful roughly 75% thread estimate is:

• Inch: drill diameter ≈ nominal major diameter − 1/TPI. Both diameters are in inches; TPI means threads per inch.
• Metric: drill diameter ≈ nominal major diameter − pitch. Both dimensions are in millimeters.

This is an estimate, not a final hole specification. Use the major diameter, not the minor or pitch diameter. Select the actual drill from the tap maker's chart for the material and required thread. Do not apply this cutting-tap estimate to forming taps, pipe threads or insert-installation taps.

Supporting detail: Addendum 6 — Chart basis and the approximation's limits.

Practice the inch estimate Practice the metric estimate

Thread percentage is not percent of bolt strength

Percent thread describes how much thread height the hole permits relative to a reference profile. With the same cutting tap, a larger prepared hole leaves less thread height; a smaller hole leaves more material for the tap to remove and generally increases tapping torque.

It does not describe how far the screw enters the hole. That is engagement length. Nor does 75% thread mean 75% joint strength. Material, engagement length, thread geometry and loading all affect the joint. More thread height is not automatically a better choice.

Supporting detail: Addendum 7 — Keep percentage and fraction separate.

Practice thread-percentage reasoning

Taper, plug and bottoming describe the tap's lead-in

The chamfer is the gradual lead-in where the first teeth progressively cut the thread. A taper tap has a long lead-in that helps starting; a plug tap has a shorter lead-in; a bottoming tap has the shortest of the three and reaches full thread closer to the bottom of a blind hole.

A bottoming tap still has a lead-in. It cannot produce full thread all the way to the physical bottom. For hand tapping, start with a tap that can establish alignment, then use a bottoming tap when the required depth calls for it. Leave room for incomplete threads, chips and the drill point.

Chamfer style is separate from chip direction. A spiral-point cutting tap generally pushes chips ahead and needs exit space; a spiral-flute cutting tap can draw chips back toward the entrance. Select a tap intended for the material and through or blind hole.

Power tapping needs a machine and holder designed for it

Machine tapping coordinates spindle rotation with axial travel at the thread's lead. Depending on the machine, that may use synchronized rigid tapping or a suitable tapping attachment. The machine, holder, tap, reversal and depth control must work together. An ordinary drill-press setup is not automatically a power-tapping setup.

A cutting tap removes chips. A forming tap displaces suitable ductile material to make the thread without cutting chips. Forming taps require their own, generally larger, prepared-hole sizes and suitable lubrication. A cutting-tap drill can be much too small for a forming tap of the same thread size.

Use the machine's instructions and the approved shop procedure for tapping equipment.

Supporting detail: Addendum 8 — Why the local setup decides what is permitted.