CNC drilling and hole-making looks simple until the print calls out a tight diameter, a fine finish, and a true position band measured in thousandths. Getting a hole round, straight, on-size, and in the right place takes the correct sequence of operations, not just a twist drill. This guide covers peck drilling, reaming, boring, and tapping, plus the position tolerance you can realistically expect and the cost behind it.
The Hole-Making Sequence
A quality hole is usually built in stages. Each step removes error left by the one before it.
- Spot drill. A short, rigid spotting tool starts the hole precisely on center so the drill does not walk.
- Drill (or peck drill). The through-hole is drilled to a size just under the finished diameter.
- Ream or bore. A finishing operation brings the hole to final size, roundness, and finish.
- Tap or thread. If the hole is threaded, tapping or thread milling follows.
Skipping the spot drill is the most common cause of a hole drifting off position. On a rigid setup with a proper spot, a drilled hole starts true and stays true.
Peck Drilling and Deep Holes
Peck drilling retracts the drill periodically to clear chips instead of cutting in one continuous plunge. It matters most on deep holes, where chips pack in the flutes, generate heat, and can snap the tool. Guidelines:
- Holes deeper than about 3 to 4 times the drill diameter (3:1 to 4:1 depth-to-diameter) benefit from peck cycles.
- Past roughly 5:1, expect slower feeds, more pecks, and possible drift; specify straightness if it matters.
- Very deep holes beyond about 10:1 call for a dedicated deep-hole or gun-drilling strategy and should be reviewed up front.
Peck drilling trades cycle time for reliability. It is slower per hole but prevents scrapped parts and broken tools on deep work.
Reaming vs Boring for Finished Holes
When a drilled hole is not accurate enough, two finishing routes deliver a precision bore:
- Reaming pulls a multi-flute tool through a slightly undersized hole to hit size and finish. Reaming is fast and repeatable and holds diameter tolerances of +/-.0005 in with a finish around Ra 32 uin or better. It follows the existing hole, so it corrects size and finish but not location.
- Boring uses a single-point tool that can be adjusted precisely. Boring corrects both size and position, holds tolerances down to +/-.0002 in, and produces the roundest, straightest bores. It is slower and costs more per hole.
Choose reaming when you need an accurate diameter in an already well-located hole. Choose boring when position, roundness, and straightness all have to be corrected to a tight band.
Hole Tolerances and Finishes at a Glance
- As-drilled diameter: +.003 / -.001 in typical, and drilled holes tend to run oversize.
- Reamed diameter: +/-.0005 in, finish to Ra 32 uin.
- Bored diameter: +/-.0002 in, finish to Ra 16 uin.
- As-drilled finish: Ra 63 to Ra 125 uin.
True Position Tolerance
True position defines how far a hole center can stray from its nominal location, called out as a diameter zone relative to datums. It is where hole-making gets expensive, because holding tight position depends on setup, spotting, and how many faces the holes share.
- General position: .010 in diameter zone is easy and low cost.
- Precision position: .005 in diameter zone is routine with spot drilling and a rigid setup.
- Tight position: .002 in diameter zone or tighter usually requires boring, minimal setups, and CMM verification.
The biggest lever on position is setup count. Holes drilled in one setup relate to each other tightly. Holes drilled across multiple re-fixtures pick up datum-shift error. A 4-axis horizontal approach that reaches multiple faces in one cycle holds hole-to-hole position far better than repeated re-fixturing. See our CNC milling page for how that works.
Tapping and Threaded Holes
- Cut tapping and form tapping both produce threads; form tapping in ductile materials leaves no chips and a stronger thread.
- Thread milling is preferred for large diameters, hard materials, and blind holes where a broken tap would scrap the part.
- Always specify thread class (for example 2B) and depth of full thread on the print.
What Hole-Making Costs
Hole cost depends on diameter, depth, tolerance, finishing route, and quantity. The table shows typical illustrative ranges per feature. These are planning figures, not binding quotes.
| Operation | What It Buys | Illustrative Added Cost per Hole |
|---|---|---|
| Spot + drill | Located through-hole, as-drilled tolerance | $0.50 to $4 |
| Peck drill (deep) | Reliable deep hole, chip clearing | $2 to $12 |
| Ream | +/-.0005 in diameter, Ra 32 finish | $1 to $6 |
| Bore | +/-.0002 in, tight position and roundness | $4 to $20 |
| Tap / thread mill | Threaded hole | $1 to $10 |
| CMM position report | Verified true position, FAI data | $40 to $150 per lot |
Setup and programming add a fixed $150 to $600 per run on top of per-hole cost, amortized across the batch. A part with twenty general-tolerance holes costs a fraction per hole of a part with four bored, tight-position holes, even though the second part has fewer features.
How to Reduce Hole-Making Cost
- Use standard drill and tap sizes so no special tooling is ordered.
- Loosen position and diameter tolerances on non-critical holes.
- Keep depth-to-diameter under 4:1 where possible to avoid slow peck cycles.
- Group critical holes on one face so they share a datum in one setup.
- Ream instead of bore when only diameter, not position, needs correcting.
Inspection and Quality
Hole diameter, roundness, and true position are verified with in-house Brown & Sharpe CMM inspection, and a documented first article inspection with a full position report is available on request. Our ISO 9001-aligned process delivers dimensional data, material certs, and FAI packages with the parts. More on our inspection and quality page.
Wexmar performs precision CNC drilling and hole-making across turning and milling in Canastota, NY, with in-house CMM verification and nationwide shipping. Send a print through our instant quote tool for pricing on your hole-making requirements.