The short answer
On CNC RFQs, “make this threaded hole” is not one process. Shops usually cut internal threads with a tap (form or cut), or they interpolate the thread with a thread mill. Tapping is often faster per hole on mid-size through holes in friendly materials. Thread milling wins when the hole is large, the material is hard or gummy, a broken tap would scrap an expensive blank, the thread must be incomplete or specialty, or the same tool family must cover many thread sizes. Buyers who only write “M6×1.0 — 4×” leave the process choice—and the scrap-risk story—to the estimator.
State thread class, blind vs through, material/heat treat state, and any “no tap / mill only” preference when you upload STEP and PDF on the 3DWK quote page (quote-new.php). This article is typical buyer guidance only—no invented rates, cycle times, or shop certifications.
What tapping and thread milling actually are
**Tapping** drives a sized tap down the axis of a pre-drilled hole. Cut taps remove chips; form (roll) taps displace material and need a different tap-drill size. Both need chip evacuation or lubrication discipline, especially in blind holes. One tap usually matches one thread size and pitch.
**Thread milling** uses a smaller rotating cutter that interpolates a helical path. One thread mill can often cut several diameters of the same pitch family, can climb out if the tool breaks, and can leave a controlled incomplete thread or a clean stop near a blind bottom. Cycle time per hole is usually longer than a straight tap on common sizes—but programming and risk math change the quote more than raw seconds alone.
Neither process is “always better.” Designing threads and tapped holes covers geometry and engagement length; this article is specifically the **process choice** shops make once the thread exists on the drawing. Helicoil vs tapped holes for CNC aluminum is the insert path when parent material is soft—orthogonal to mill-vs-tap.
When tapping is the shop default
Estimators default to tapping when all of the following roughly hold:
- Common metric or UNC/UNF sizes in the shop’s tap crib (for example M3–M12 / #4–1/2 in many job shops)
- Through holes or generous blind depth with room for chip pack / spiral-flute exit
- Aluminum, free-machining brass, mild steel, or other cooperative alloys in soft or moderate hardness
- Standard thread classes (for example 6H / 2B style callouts) without exotic lead or special form
- Quantity and hole count where a few seconds per hole matters more than tool flexibility
On those jobs, taps are fast to program, easy to peck or rigid-tap on modern CNCs, and cheap to replace relative to a scrapped aerospace blank. Preliminary online quote engines often assume this default when the STEP shows ordinary tapped holes and the material is friendly—see reading a preliminary online quote (min / mid / max) and what needs_manual means when automation cannot infer a safe thread method.
When thread milling is the safer or only practical choice
Thread milling tends to appear—or should be invited on the RFQ—when:
1. **Large diameters**: big taps demand high torque and risk; mills scale more gently
2. **Hard or tough alloys**: hardened steels, titanium, nickel alloys (see Ti-6Al-4V CNC vs SLM and IN625 vs IN718 for CNC vs SLM buyers for material context)—broken taps are expensive events
3. **Blind holes with short unused length**: mills can stop cleanly; taps need chip room and a defined tap drill depth
4. **Expensive blanks or late-stage features**: if the hole is cut after hours of prior machining, mill risk often beats tap risk
5. **Many sizes, one setup**: one pitch-family mill can cover several majors; taps need a tool change per size
6. **Left-hand, special form, or incomplete threads**: easier to program with a mill path than to source a rare tap
7. **Thin walls or interrupted holes**: controlled radial engagement can reduce burst-out compared with an aggressive tap
Deep pockets and tool reach on CNC quotes pairs with this: a thread mill still needs radial and axial clearance for the interpolation. If the boss sits at the bottom of a deep pocket, say so—reach and stick-out affect both methods.
Blind vs through holes change the decision
Through holes favor tapping: chips can exit, coolant can flush, and spiral-point (gun) taps push chips ahead. Blind holes flip the risk:
- Cut taps pack chips at the bottom unless peck cycles and flute style match the depth
- Form taps need correct minor diameter and still need bottom clearance
- Thread mills need a larger pre-drill / bore and a programmed Z stop above the floor
Call **blind vs through** explicitly on every threaded hole—do not leave it only in the 3D model. Counterbore vs countersink vs spotface for CNC bolted joints and edge break / chamfer / deburr callouts also sit next to thread mouths; a missing chamfer on a tapped hole is a common FAIR write-up and a common quote add.
Material, heat treat, and insert paths
Thread process choice follows material state:
- Soft aluminum: taps are common; buyers still choose Helicoil / inserts for wear or assembly cycles (helicoil vs tapped holes for CNC aluminum)
- Stainless: work-hardening and chip stringiness raise tap risk; mills or careful form taps appear more often
- Heat-treated steels / 17-4PH: if threads are cut after harden, mills or carbide tooling dominate; if cut soft then heat treat, call that sequence out (17-4PH H900 vs H1025: what buyers choose)
- Plastics (POM, PA66, PEEK): form taps or careful cut taps; oversized or insert strategies sometimes beat either for repeated assembly—see POM vs PEEK for CNC functional prototypes and PA66 moisture notes
If your drawing says “tap after hard anodize” or “thread after heat treat,” write the sequence on the RFQ. How anodize choice changes CNC RFQ cost and hard anodize vs electroless nickel for wear both change minor diameter and coating growth—thread timing is part of that stack.
How the choice shows up in quotes and lead time
Buyers rarely see a line labeled “thread mill vs tap.” They see:
- Wider min–mid–max bands when hole count is high and material is tough
- Manual review holds when broken-tap scrap risk is obvious from alloy + blind depth + blank cost
- Tooling notes or longer prove-out when specialty mills must be ordered
- Quantity effects: a production lot may invest in rigid tapping cycles; a qty-1 prototype in Ti may mill every hole
What drives CNC machining cost and what affects CNC machining lead time put threading in the broader stack with setups, finishes, and inspection. How quantity breaks change CNC unit cost matters when hole count × method amortizes tool and program time. Prototype vs production CNC quotes is the companion when a first article mills threads and a locked lot switches to high-speed tapping.
Drawing notes that prevent wrong assumptions
Put these on the PDF or RFQ text—not only in CAD cosmetic threads:
1. Thread designation + class (e.g. M8×1.25-6H, 1/4-20 UNC-2B)
2. Blind or through; full thread depth and unused length for blinds
3. Pre-drill / minor diameter if you control it; otherwise “shop standard for method”
4. Material condition at time of threading (annealed / H900 / coated)
5. Preferred method if you have one: “thread mill preferred — no tap” or “shop may tap”
6. Insert callout if applicable (Helicoil / Keensert size and grip)
7. Inspection expectation: Go/No-Go only vs measured pitch diameter on critical holes
What files to send for a CNC quote and the DFM checklist before an online CNC quote both apply: STEP + PDF with thread callouts beat “modeled helix only” every time. GD&T callouts that raise CNC quote bands matter when positional frames on threaded patterns force longer locate and probe cycles—independent of mill vs tap, but stacked on top of them.
RFQ checklist for thread process choice
Before you submit on quote-new.php, confirm:
- Every threaded hole states size, pitch/class, and blind vs through
- Expensive alloy or late-stage holes invite “thread mill OK / preferred” language
- Soft aluminum with repeated assembly asks insert vs parent tap explicitly
- Heat-treat and coating sequence relative to threading is written once
- Deep or pocketed bosses note tool-reach constraints
- Critical holes state Go/No-Go vs quantitative inspection
- Quantity now vs next-buy is clear so shops can amortize taps vs mills sanely
Milled and turned features on one CNC part also affects threads on shafts vs housings: a mill-turn may rigid-tap on-center while an odd radial boss still needs live-tool mill or a second op.
Common buyer mistakes
- Modeling a pretty helix but omitting class and depth on the 2D
- Assuming every shop will tap M1.6 the same way they tap M10
- Forbidding thread mills “to save money” on Inconel blinds—then paying for scrap
- Calling Helicoil after the shop already quoted parent taps in soft aluminum
- Leaving coating growth unstated so finished minor diameters land undersize
Reaming vs boring for CNC hole size control is the cousin topic for the cylindrical hole before the thread exists—wrong minor diameter ruins both taps and mills.
Bottom line
Tapping and thread milling are different risk and cost stories for the same callout on the drawing. Taps dominate common through holes in cooperative materials; thread mills dominate large, hard, blind, high-value, or multi-size cases. Write class, depth, blind/through, material state, and any method preference on the RFQ with STEP and PDF, and shops quote a comparable process instead of three silent defaults. Ready to compare methods on a real part? Start on quote-new.php.