Drilling on a Drill Press or Mill

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.

Why “always center drill first” is too broad

The starting recess determines which part of the next drill touches first. An unsuitable angle or an oversized pilot can load the drill's outer corners before its center is supported. Accurate starting also depends on tool rigidity, alignment and the surface being entered. A center-drilling step alone does not guarantee location.

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.

Why changes in the cut matter

Changes in chip shape, sound, thrust or finish can indicate rubbing, chip packing, a damaged point or unsuitable cutting data. Continuing to force the tool does not diagnose the cause.

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.

Program	Motion to watch	What the model reports
Continuous advance	G1 Z-8	One feed enters new modeled stock to final depth.
Short in-bore retract	G0 Z-1, then G1 Z-4 and G1 Z-8	The first feed back removes no additional modeled stock; the separate deeper feed does.
Withdrawal above the mouth	G0 Z2, then G1 Z-4 and G1 Z-8	The first feed back removes no additional modeled stock; the separate deeper feed does.

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.

Drill-tip DRO	What the Front section represents	Read the individual checks
Z −20	The point reaches the stock bottom, but the full drill diameter stops higher.	Diameter can read Ø6.60 while THRU says Not through yet: full size only to Z −18.02.
Z −21	The point extends below the stock and leaves a partial bottom opening; the full diameter still has not reached the bottom.	Diameter can still read Ø6.60 while THRU says Not through yet: full size only to Z −19.02.
Z −22	The modeled opening at the bottom reaches the inspection's minimum allowed diameter.	THRU changes to Through at the minimum allowed diameter.

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.