Thread Design for CNC Parts: DFM Rules (2026)

Q: How deep should a tapped hole be for aluminum?

For 6061-T6 and 7075-T6 aluminum, use a minimum thread engagement depth of 1.5× the nominal fastener diameter (1.5D). A 1/4-20 screw needs at least 0.375 in. (9.5 mm) of full thread engagement. Add 2 pitch lengths beyond the engagement zone for tap lead in blind holes, plus 0.060 in. (1.5 mm) clearance at the bottom. This rule comes from the lower shear strength of aluminum relative to steel — at 1.5D, the bolt fails before the threads strip, which is the target failure mode per Machinery's Handbook (31st ed.).

Q: When should I use a Helicoil instead of a tapped hole?

Use Helicoil (wire thread) inserts when the parent material is softer than approximately 30 HRC, the joint will see repeated assembly/disassembly cycles (>10 per product life), or you need to match a steel-strength thread class in a lightweight housing. Typical applications: 6061-T6 aluminum housings with M5 or larger fasteners that get torqued during field service, and any acetal or nylon part requiring threaded connections. A Helicoil adds approximately $0.50–$1.50 per hole in production depending on size, but it prevents the $500+ cost of scrapping a machined housing due to stripped threads.

Scroll to explore

Thread Standards

Thread Standards: Which System and When

Most threading problems start with picking the wrong standard. In the US, Unified Inch (UNC/UNF) per ASME B1.1 is still the default for most commercial hardware. Metric ISO threads per ISO 261/262 dominate European and Asian supply chains — and are increasingly common in US robotics and medical device work. JIS B 0205 is dimensionally identical to ISO metric, so parts designed for the Japanese market are interchangeable.

Assortment of metric and imperial screws and bolts showing different thread standards (UNC, UNF, metric) for CNC part design.

Common thread standards: UNC/UNF (inch) and ISO metric. Choose the standard that matches your hardware and region.

Standard	Governing Spec	Pitch Type	Typical Use	Callout Example	Regional Prevalence
UNC	ASME B1.1	Coarse	General fastening, default for US hardware	1/4-20 UNC-2B	US, Canada
UNF	ASME B1.1	Fine	Vibration-prone joints, thin walls, fine adjustment	1/4-28 UNF-2B	US
Metric ISO (coarse)	ISO 261 / JIS B 0205	Coarse	General fastening, global default	M6 × 1.0 - 6H	EU, Asia, global
Metric ISO (fine)	ISO 261 / JIS B 0205	Fine	High-strength joints, precision adjustment	M6 × 0.75 - 6H	EU, Asia
ACME	ASME B1.5	Trapezoidal	Lead screws, power transmission	1/2-10 ACME-2G	US
Trapezoidal (Tr)	ISO 2904 / DIN 103	Trapezoidal	EU equivalent of ACME	Tr 12 × 3	EU
NPT	ASME B1.20.1	Tapered	US pipe connections (sealing by interference)	1/4-18 NPT	US
BSPP (G)	ISO 228 / DIN 259	Parallel	EU pipe connections (sealing by O-ring/gasket)	G 1/4	EU, Asia
BSPT (R/Rc)	ISO 7 / JIS B 0203	Tapered	EU/Asia tapered pipe (similar function to NPT)	R 1/4	EU, Asia

NPT vs BSPP: Not interchangeable

NPT is tapered (seals by thread interference + sealant). BSPP is parallel (seals by O-ring or gasket on a flat face). They have different thread angles (60° vs 55°) and different pitches at the same nominal size. Mating an NPT fitting into a BSPP port will cross-thread and leak. If your product ships to both US and EU markets, call out the port standard explicitly on the drawing and consider SAE straight thread O-ring boss (SAE J1926) as a universal alternative.

Tapped Holes vs Inserts

Direct Tapping vs Thread Inserts: Decision Framework

Direct tapping is the cheapest option when it works — a single operation, no extra hardware. But in soft metals, plastics, or high-cycle assemblies, tapped threads strip. The question isn't “should I use inserts?” — it's “what's the failure cost if I don't?”

Thread form and relief on turned parts. Use direct tapping for low-cycle, harder materials; choose Helicoil or solid inserts for soft metals and high assembly cycles.

Direct Tapping

Lowest cost per hole ($0.50–$1.00 typical)
Single operation — no extra hardware or installation
Reliable multi-cycle threads in materials ≥25 HRC (steels, stainless, Ti)
Works in softer metals (aluminum, brass) for low-cycle applications — viable when ≤5–10 assembly cycles expected
Thread degradation in soft metals after repeated assembly (<10 cycles in 6061-T6 for M3 and smaller)
Tap breakage risk in blind holes and hard materials

Wire Thread Inserts (Helicoil)

Achieves steel-class thread strength in soft metals
Handles 100+ assembly/disassembly cycles
Repairs stripped threads in existing parts
Adds $0.50–$1.50 per hole (insert + installation)
Requires oversized tap drill (larger hole in the part)

Keyserts / Solid Inserts

Highest pull-out and torque resistance
Locks in place with keys that prevent rotation
Most expensive option ($2.00–$5.00 per hole installed)
Requires specific counterbore geometry

Heat-Set Inserts (Plastics)

Brass knurled insert melted into thermoplastic
Reliable threads in acetal, nylon, ABS, polycarbonate
Handles M3+ fasteners with repeated assembly
Requires controlled installation temperature and pressure

Method	Best For	Material Constraint	Typical Cost/Hole	Assembly Cycles
Direct tap	Any material; multi-cycle durability in ≥25 HRC	Any (limit cycles in soft metals)	$0.50–$1.00	5–10 (soft metals), 50+ (≥25 HRC)
Helicoil (wire)	Soft metals, field service	Any machinable metal	$1.00–$2.50	100+
Keysert (solid)	High-load, vibration, thin walls	Any machinable metal	$2.00–$5.00	500+
Heat-set insert	Thermoplastics (CNC or molded)	Thermoplastics only	$0.30–$1.00	50+

Engagement Depth

Thread Engagement Depth by Material

Engagement depth determines whether the bolt fails before the threads strip — which is the correct failure mode. Too shallow and you strip threads under load. Too deep and you waste machining time and increase blind-hole risk. The right depth depends on the parent material's shear strength relative to the fastener's tensile strength.

Material	Engagement (× nominal ∅)	Example: 1/4-20 UNC	Notes
4140 / 4340 alloy steel	1.0D	0.250 in. (6.4 mm)	High shear strength; bolt fails first at 1.0D
303 stainless steel	1.0–1.25D	0.250–0.312 in. (6.4–7.9 mm)	Sulfur content slightly reduces shear strength vs 304
304 / 316L stainless	1.0D	0.250 in. (6.4 mm)	Austenitic; work-hardens during tapping — use sharp taps
17-4 PH stainless (H900)	1.0D	0.250 in. (6.4 mm)	Precipitation-hardened; shear strength exceeds most bolt grades
6061-T6 aluminum	1.5D	0.375 in. (9.5 mm)	Typical for robotics housings; consider inserts for M3 and smaller
7075-T6 aluminum	1.25–1.5D	0.312–0.375 in. (7.9–9.5 mm)	Higher shear strength than 6061; 1.25D often sufficient
Ti-6Al-4V (Grade 5)	1.0–1.5D	0.250–0.375 in. (6.4–9.5 mm)	Thread milling preferred over tapping to prevent galling; see titanium threading guide
Acetal (POM / Delrin)	2.0–2.5D	0.500–0.625 in. (12.7–15.9 mm)	Coarse pitch only; fine pitch strips easily. Consider heat-set inserts for M4+.
Nylon (PA6 / PA66)	2.0–2.5D	0.500–0.625 in. (12.7–15.9 mm)	Moisture absorption weakens threads over time; inserts strongly recommended for structural fastening
Polycarbonate (PC)	2.0D	0.500 in. (12.7 mm)	Notch-sensitive — chamfer all thread entries to prevent stress cracking

When to Go Deeper vs When to Use Inserts

If engagement depth exceeds 2.0D and the hole is blind, you're fighting diminishing returns — the last few threads carry almost no load (load distribution is non-linear, with the first 3–5 threads carrying ~80% of the clamp force). At that point, a Helicoil at 1.5D engagement is cheaper, more reliable, and produces a shallower hole.

Get a Free DFM Review on Your Threaded Parts

Upload your CAD file and our engineering team will review your thread callouts, engagement depths, and hole specifications — flagging any DFM issues before production starts. Every RFQ includes a free DFM review with tolerance and threading recommendations.

Upload CAD for Free DFM Review

Relief, Runout & Chamfers

Thread Relief Grooves, Runout & Entry Chamfers

Thread relief grooves, proper runout zones, and entry chamfers are the details that separate drawings that work from drawings that cause phone calls from your machinist. They're especially critical on external threads cut by single-point tooling on a lathe.

Machined shaft with threaded section and relief groove between thread and shoulder; external thread design for CNC turning.

External thread with relief groove. The undercut allows the threading tool to run out cleanly and lets the nut seat fully; per ASME B1.1, relief is typically 2–3 pitch widths to minor diameter.

Thread Relief Grooves

Required on external threads that run to a shoulder. The groove gives the threading tool a clean exit zone and ensures the mating nut can seat fully against the shoulder face.

Width: 2–3 pitch lengths (per ASME B1.1). For 1/4-20 UNC: 2 × 0.050 in. = 0.100 in. (2.5 mm).
Depth: To the minor diameter of the thread. For 1/4-20: groove OD ≈ 0.189 in. (4.8 mm).
Corner radius: 0.010–0.015 in. (0.25–0.38 mm) typical. Sharp corners create stress risers.

Entry Chamfers

A 45° × 1 pitch chamfer at the start of both internal and external threads is standard practice. It guides the mating fastener onto the thread and prevents cross-threading during assembly.

Internal (tapped hole): 45° × 1P countersink at the hole entry. Most taps create this automatically if you pre-chamfer the hole.
External (shaft): 45° × 1P chamfer on the leading edge. Critical for blind assembly or automated fastening.
Plastics: Use a 30° chamfer instead of 45° — gentler engagement reduces stress concentration in notch-sensitive materials like polycarbonate.

External thread relief groove (per ASME B1.1). Width = 2–3 pitch lengths, depth = to minor diameter. Required when threads run to a shoulder.

Skip the Relief When You Can

If you can add 3 pitches of unthreaded clearance between the last thread and the shoulder (so the thread doesn't need to run all the way to the face), you can eliminate the relief groove entirely. This saves a secondary machining operation and simplifies the drawing. Many early-career engineers add thread reliefs by default — evaluate whether your nut actually needs to seat against that shoulder before specifying one.

Drawing Callouts

Thread Callouts on Engineering Drawings

A thread callout must be unambiguous. The machinist should never have to guess the standard, pitch, class of fit, or depth. Here's how to write them correctly per ASME Y14.6 (US) and ISO 6410 (EU/global).

Unified Inch — Internal

1/4-20 UNC-2B

1/4: — nominal diameter (0.250 in.)
20: — threads per inch
UNC: — Unified National Coarse
2B: — class 2 fit, internal (B)

Metric ISO — Internal

M6 × 1.0 - 6H

M6: — metric, 6 mm nominal ∅
1.0: — pitch in mm (omit if coarse: “M6 - 6H”)
6H: — tolerance grade 6, position H (internal)

JIS B 0205 uses identical notation.

Pipe Threads — US vs EU

1/4-18 NPT

US tapered — seals by thread interference

G 1/4 (BSPP)

EU parallel — seals by O-ring or gasket

R 1/4 / Rc 1/4 (BSPT)

EU/Asia tapered — ISO 7 / JIS B 0203

Class of Fit Quick Reference

US Class (ASME B1.1)	ISO Equivalent	Fit Description	When to Use
1A / 1B	~8g / 7H (approx.)	Loose — maximum allowance	Quick assembly, dirty/coated threads
2A / 2B ★	6g / 6H	General purpose — default for commercial fasteners	90%+ of all CNC threaded features
3A / 3B	4g6g / 4H5H	Tight — no allowance	Precision assemblies, zero-backlash joints; adds 30–50% threading cost

Common Thread Callout Mistakes

Missing class of fit

Always specify: "1/4-20 UNC-2B" not "1/4-20 UNC." Without a class, the machinist defaults to 2B — which is usually fine, but ambiguity causes RFQ delays and inspection disputes.

Confusing NPT with BSPP

Write the full standard name. "1/4 pipe thread" is ambiguous if the part ships internationally. Specify "1/4-18 NPT" or "G 1/4 per ISO 228."

Omitting depth for blind holes

Call out both thread depth and drill depth: "1/4-20 UNC-2B ↧ 0.375 THRD DEPTH, 0.595 DRILL DEPTH." Two separate dimensions.

Specifying fine pitch without reason

Fine pitch (UNF / ISO fine) increases tap breakage risk, requires tighter hole tolerance, and costs 15–25% more. Use coarse unless vibration, thin walls, or adjustment precision demands it.

Cost Implications

What Drives Threading Cost Up (and How to Keep It Down)

Threading is rarely the dominant cost driver on a CNC part — but poorly specified threads can double the per-hole cost without adding functional value. Here's what matters.

Cost Escalators

Blind holes: +20–30% vs through holes (peck-tapping cycles, spiral-flute taps)
Fine pitch: +15–25% (tighter hole tolerance, higher tap breakage)
Thread milling: +50–100% vs tapping (but required for hard materials and large threads)
Hard materials (Ti, Inconel): +100–200% (specialty taps, TiCN/TiAlN coating, slower feeds)
Class 3B fit: +30–50% (tighter manufacturing tolerance, 100% thread gage inspection)
Non-standard sizes: Custom taps, longer lead times, no off-the-shelf fasteners
Helicoil/insert installation: +$0.50–$1.50 per hole

Cost Reducers

Standard coarse-pitch sizes: M4, M5, M6, M8, 1/4-20, 5/16-18, 3/8-16 — off-the-shelf taps, cheap hardware
Through holes whenever possible: Gun taps, fast cycles, low breakage
Class 2B (default): No inspection surcharge, standard manufacturing tolerance
Consistent thread sizes across the part: Fewer tool changes = faster cycle time
Accessible hole locations: Threads in deep pockets or near obstructions require longer taps and specialized tooling
Form taps for soft metals: Roll-form taps (no chips) in aluminum and brass are faster and produce stronger threads than cut taps

The 80/20 Rule for Thread Cost

On most parts, standardizing all threads to 2–3 coarse pitch sizes (e.g., M5 and M8, or 1/4-20 and 3/8-16) eliminates 80% of thread-related cost premium. The machinist changes the tap once instead of four times, uses off-the-shelf tooling, and runs proven cycle parameters. Save the exotic threads for the one feature that actually needs them.

Common Questions

Frequently Asked Questions

How deep should a tapped hole be for aluminum?

For 6061-T6 and 7075-T6 aluminum, use a minimum thread engagement depth of 1.5× the nominal fastener diameter (1.5D). A 1/4-20 screw needs at least 0.375 in. (9.5 mm) of full thread engagement. Add 2 pitch lengths beyond the engagement zone for tap lead in blind holes, plus 0.060 in. (1.5 mm) clearance at the bottom. This rule comes from the lower shear strength of aluminum relative to steel — at 1.5D, the bolt fails before the threads strip, which is the target failure mode per Machinery's Handbook (31st ed.).

When should I use a Helicoil instead of a tapped hole?

Use Helicoil (wire thread) inserts when the parent material is softer than approximately 30 HRC, the joint will see repeated assembly/disassembly cycles (>10 per product life), or you need to match a steel-strength thread class in a lightweight housing. Typical applications: 6061-T6 aluminum housings with M5 or larger fasteners that get torqued during field service, and any acetal or nylon part requiring threaded connections. A Helicoil adds approximately $0.50–$1.50 per hole in production depending on size, but it prevents the $500+ cost of scrapping a machined housing due to stripped threads.

What is the difference between UNC and UNF threads?

UNC (Unified National Coarse) has fewer threads per inch and is the default for general-purpose fastening in the US per ASME B1.1. UNF (Unified National Fine) has more threads per inch, providing higher tensile strength, finer adjustment, and better vibration resistance — but at the cost of increased tap breakage risk and tighter hole tolerance requirements. Use UNC unless the application specifically demands fine pitch: vibration-prone assemblies, thin-wall sections where you need more threads in a short engagement length, or adjustment mechanisms. For metric equivalents, ISO 261 coarse pitch (e.g., M6 × 1.0) corresponds to UNC, and ISO 261 fine pitch (e.g., M6 × 0.75) corresponds to UNF.

How do I call out a metric thread on an engineering drawing?

Per ISO 6410 (and ASME Y14.6 for US drawings), a metric internal thread is called out as: M6 × 1.0 - 6H, where M = metric, 6 = nominal diameter in mm, 1.0 = pitch in mm, and 6H = tolerance class (6 = grade, H = internal position). For external threads: M6 × 1.0 - 6g (lowercase g = external). If using coarse pitch, the pitch may be omitted: M6 - 6H. JIS B 0205 uses the identical notation. Always include depth for blind holes: M6 × 1.0 - 6H ↧ 12 (12 mm thread depth). Include the drill depth separately if it differs from thread depth.

What thread engagement depth do I need for stainless steel?

For 303, 304, and 316L stainless steel, use 1.0× to 1.25× the nominal fastener diameter (1.0D–1.25D). Stainless has sufficient shear strength that a 1/4-20 thread in 316L only needs 0.250–0.312 in. (6.35–7.94 mm) of engagement to ensure bolt failure before thread strip-out. The higher end of the range (1.25D) is recommended for 303 free-machining stainless, which has slightly lower shear strength due to sulfur content. For 17-4 PH in the H900 condition, 1.0D is sufficient — its shear strength exceeds most bolt grades.

Do I need thread relief on CNC machined threads?

Thread relief grooves are required on external single-point-cut or ground threads where the thread must run to a shoulder or the full thread profile needs to extend to the end of the threaded zone. Per ASME B1.1, a standard relief groove is 2–3 pitch widths long and cut to the minor diameter of the thread. On CNC turned parts, thread relief prevents the tool from crashing into a shoulder and ensures the mating nut seats fully. Internal threads (tapped holes) do not need relief — the tap naturally creates its own lead-in. If you can avoid threading to a shoulder by adding 3 pitches of clearance, you can eliminate the relief entirely and save a machining operation.

How much does threading add to CNC part cost?

A standard tapped through-hole (M6 or 1/4-20, coarse pitch, 2B class) in 6061-T6 aluminum adds approximately $0.50–$1.00 per hole in low-to-mid volume production (10–500 parts). Cost escalators: blind holes (+20–30% vs through), fine pitch (+15–25%), thread milling instead of tapping (+50–100%), hard materials like Ti-6Al-4V or Inconel (+100–200%), tight tolerance class 3B (+30–50%), and Helicoil installation (+$0.50–$1.50 per hole). The most cost-effective threading strategy: standard coarse-pitch through holes in soft-to-medium materials, with 2B class of fit.

Should I use through holes or blind holes for threads?

Use through holes whenever the part geometry allows. Through holes are 20–30% cheaper to thread because chips evacuate freely during tapping, reducing tap breakage risk and eliminating the need for peck-tapping cycles. Through holes also allow standard spiral-point (gun) taps, which are faster and more reliable than the spiral-flute taps required for blind holes. Use blind holes only when the backside of the part is a sealing surface, the hole would break through into an adjacent feature, or the fastener would protrude into a mating component's envelope.

Related Resources

CNC Design Guidelines

Wall thickness, pockets, radii & threads

Titanium Threading Guide

Tapping, thread milling & galling prevention for Ti-6Al-4V

How to Read Engineering Drawings

Title blocks, views, dimensions & thread callouts

GD&T for CNC Machined Parts

Geometric tolerancing for threaded features

Ready to Get Your Threaded Parts Right the First Time?

Upload your CAD files and engineering drawings. Our team reviews every thread callout, engagement depth, and insert specification as part of our free DFM review — before a single tap touches metal.

Get Free Quote Fast

Thread Design for CNC Parts: Engagement, Inserts & Callouts

Quick Reference