What is the difference between tapping and thread milling?

Both tapping and thread milling cut helical grooves (threads) into a pre-drilled hole, but they do it differently. A tap is a multi-flute tool that is driven axially into the hole — it cuts all thread flanks simultaneously on the way in, and on reversal. A thread mill is a smaller, shorter tool that is moved in a helical path around the inside of the hole using the CNC machine's simultaneous 3-axis interpolation. Key difference for titanium: if a tap breaks inside a hole, it is almost impossible to remove (especially in blind holes) and the part is typically scrapped. Thread mills very rarely break catastrophically, and even if they do, the smaller diameter tool is easier to extract. Thread milling also allows the operator to adjust the thread pitch diameter in the CNC program without changing tools — useful in titanium where spring-back affects the finished thread size.

What is "galling" and why does it happen in titanium threads?

Galling is a form of severe adhesive wear where two metal surfaces under pressure bond together at their contact points through a process similar to cold welding, then tear apart as relative motion continues. In titanium threading, galling occurs when: (1) the tap or fastener generates enough frictional heat to activate titanium's chemical affinity for the mating metal, (2) lubrication is insufficient to prevent metal-to-metal contact on thread flanks, or (3) the fit is too tight (not enough clearance on the thread flanks). The result: a seized fastener or damaged thread. Titanium-to-titanium interfaces are especially prone to galling. The fix: use 2B/2A thread class fits (not 3B/3A), apply anti-galling compound (Never-Seez or molybdenum disulfide paste) on assembly, and never thread titanium parts together dry.

What is the best way to thread titanium?

Thread milling is the preferred method for threading titanium (Ti-6Al-4V) in most production applications. Advantages of thread milling over tapping: (1) No catastrophic tap breakage risk — thread mills are spiral flute tools with much higher toughness than a tap; a broken thread mill does not lock in the hole. (2) Adjustable pitch diameter — thread milling allows on-the-fly correction of the major/minor diameter by adjusting the tool path. (3) No chip packing — thread mills use helical interpolation that continuously evacuates chips, which is critical in titanium where chip packing and galling cause tap breakage. (4) One tool for multiple thread sizes — a single thread mill can cut multiple thread sizes (different diameter, same pitch) vs. a dedicated tap per size. Use tapping where thread milling is impractical (very small diameters, deep holes, high-volume production with proven parameters).

What cutting speed should I use when tapping titanium?

When tapping titanium (Ti-6Al-4V), use 30–50 SFM (9–15 m/min) for HSS-E taps and 40–60 SFM (12–18 m/min) for TiCN or TiAlN-coated carbide taps. These are significantly slower than tapping aluminum (80–150 SFM / 24–46 m/min) or steel (40–80 SFM / 12–24 m/min). The low speed is required to: prevent built-up edge (BUE) on the tap flank, minimize heat generation (titanium's poor thermal conductivity concentrates heat at the tap flanks), and allow tapping fluid to reach the cutting zone. Use a dedicated tapping fluid (NOT standard cutting oil) — sulfurized or chlorinated tapping compound, or phosphate ester tapping fluid. Never tap titanium dry or with water-based coolant only.

How do I prevent galling when threading titanium?

Titanium galling (cold welding of the thread flanks) occurs when: (1) The tap runs too fast and generates heat that activates titanium's chemical affinity for the tool material. (2) Insufficient lubrication allows metal-to-metal contact on thread flanks. (3) The minor diameter is too tight (insufficient thread engagement clearance). Prevention: Use TiCN-coated taps (not bare HSS or TiN-coated — TiN reacts with Ti at elevated temperature). Apply sulfurized tapping oil generously before tapping. Maintain 30–50 SFM (9–15 m/min). Use 2B class thread fit for mating titanium components (not 3B) to provide clearance. For high-volume production, consider thread rolling (cold form tapping) rather than cutting taps — form taps do not cut chips and eliminate galling risk entirely.

What tap drill size should I use for UNC threads in titanium?

Use the standard tap drill size per ASME B1.1 for the selected thread series, but apply a tolerance correction: drill to the high end of the drill tolerance to ensure maximum minor diameter clearance, which reduces tap torque and galling risk. Example: #10-32 UNF thread in Ti-6Al-4V. ASME B1.1 / ISO 261 tap drill = #21 (0.159 in. / 4.04 mm) for 75% thread engagement. In titanium, use #19 (0.166 in.) for 65–70% engagement — this reduces tap torque by 15–20% with minimal loss in thread strength. Thread shear strength in titanium is 60–70 ksi (414–483 MPa), making 65% engagement typically adequate for most structural applications. For 100% thread engagement (critical joints), use the standard ASME B1.1 drill size and accept higher tapping torque with the tradeoff of reduced galling clearance.

DFM Guide · 10 min read

Threading Titanium Guide

Threading titanium sounds straightforward — it's just cutting a helical groove. The challenge is that titanium actively fights this process: it galls, it clogs chips, and it'll break a tap in a blind hole if the process isn't controlled.

Key data: thread milling preferred over tapping for most applications. When tapping: 30–50 SFM (9–15 m/min), TiCN coating, sulfurized tapping oil. Galling is the primary failure mode.

By MakerStage EngineeringMarch 10, 2026

See Threading Parameters Get a Quote

Quick Reference

Thread milling80–120 SFM (24–37 m/min)Preferred — no breakage risk

Tapping (HSS-E)30–40 SFM (9–12 m/min)Sulfurized oil required

Tapping (TiCN)40–60 SFM (12–18 m/min)Best for blind holes

Thread rolling30–50 SFM (9–15 m/min)No chips, cold-forms Ti

Thread class2B (UNC/UNF)For Ti-Ti mating joints

Scroll to explore

If you are designing your first threaded titanium part, here is the essential context before diving into parameters. A thread is a helical ridge cut into or onto a cylindrical surface — it is what allows a bolt to screw into a hole. There are three ways to create internal threads (threads inside a hole): tapping, where a hardened multi-flute tool is driven axially into a pre-drilled hole to cut the helical groove; thread milling, where a smaller tool traces a helical path using the CNC machine's 3-axis interpolation; and thread rolling (form tapping), where the tool cold-forms the thread shape without cutting chips.

Two terms you will see repeatedly: thread class and thread engagement. Thread class (e.g., 2B, 3B for inch threads; 6H for metric) specifies the allowable tolerance range on the thread dimensions — a higher number means tighter fit and less clearance. Thread engagement is the percentage of the theoretical full-depth thread that is actually cut — 75% engagement means the thread flanks extend to 75% of the full triangular profile. Higher engagement means more holding force but also higher tapping torque and galling risk.

In titanium specifically, threads fail differently than in aluminum or steel. The same parameters that work fine in those materials will cause tap breakage, galled thread flanks, or oversized pitch diameters in titanium. There are three root causes: titanium's tendency to gall (cold-weld to the tool under pressure), poor chip evacuation in deep holes, and springback that affects the finished thread diameter. Each failure mode has a straightforward countermeasure — but you need to know what to specify on the drawing and what to communicate to the shop.

Key Takeaway

Default to thread milling for titanium. Reserve tapping for small diameters or high-volume production with proven parameters. Always specify thread class and lubrication requirements on assembly drawings.

Threading Challenges

Why Titanium Threading Is Different

Titanium presents three unique challenges when threading that differentiate it from aluminum and steel: galling propensity, tap breakage in blind holes, and spring-back that affects thread pitch diameter. Understanding these challenges drives the method selection and parameter recommendations below.

Galling (Cold Welding)

Titanium's chemical reactivity causes the thread flanks to cold-weld to the tap or mating thread under heat and pressure. Galling can destroy the tap, seize the fastener, or strip the thread — all invisible until the joint is loaded. Prevention: correct SFM, TiCN coating, sulfurized oil.

Tap Breakage Risk

Titanium's high strength and poor chip evacuation cause chip packing in blind holes, which torques the tap beyond its failure point. Standard HSS taps break at higher tapping torques. Mitigation: use spiral-flute taps (chip evacuation), thread milling (no breakage mode), or peck tapping cycles.

Springback

Titanium's intermediate elastic modulus causes thread flanks to spring back after tapping, potentially resulting in a tighter-than-intended pitch diameter. Use 2B class fit for Ti-Ti mating thread pairs; verify with go/no-go gauges. A 3B class may be over-tight after springback.

Tapping Parameters

Tapping Titanium: Parameters and Tooling

Tapping parameters for titanium CNC machining
Parameter	Ti-6Al-4V	CP Grade 2	Notes
Cutting speed (HSS-E)	30–40 SFM (9–12 m/min)	40–50 SFM (12–15 m/min)	Below 30 SFM (9 m/min) increases BUE and galling risk
Cutting speed (TiCN/TiAlN coated carbide)	40–60 SFM (12–18 m/min)	50–70 SFM (15–21 m/min)	TiCN preferred; TiN-coated reacts with Ti at temperature
Tap type (through holes)	Spiral point (gun) tap	Spiral point	Pushes chips forward; reduces chip packing
Tap type (blind holes)	Spiral flute (helical) tap	Spiral flute	Pulls chips up and out; critical for blind holes in Ti
Thread class	2B recommended	2B	3B may be over-tight after springback; use 2B as default
Tapping fluid	Sulfurized or chlorinated cutting oil	Same	Apply generously to tap before entry; water-based alone insufficient
Peck tapping	Recommended for holes ≥ 2× diameter depth	Same	1/3 to 1/2 diameter peck increments; retract fully to clear chips
Thread engagement	65–75% (1.0–1.5× diameter length)	65–75%	65% engagement provides adequate shear strength in Ti; reduces torque 15%

Thread Milling (Preferred)

Thread Milling Titanium (Preferred Method)

Advantages over Tapping

• No breakage mode — thread mills are single-flute interpolation tools; failure is dimensional, not a locked insert
• Adjustable pitch diameter — major/minor diameter corrected by tool path radius; no new tooling required
• One tool, multiple sizes — same-pitch thread mill cuts different diameters; reduces tool inventory
• Better chip control — helical interpolation path continuously clears chips from the bore
• Deeper thread engagement — easier to mill full depth in blind holes vs. peck tapping

Thread Milling Parameters

Cutting speed:80–120 SFM (24–37 m/min)

Feed per tooth:0.001–0.003 in./tooth (0.025–0.076 mm)

Helix direction:Climb milling

Radial engagement:10–20% tool diameter

Coolant:Flood or through-tool HPC

Tooling:Multi-flute carbide, TiAlN

Galling Prevention

Preventing Thread Galling in Titanium

Galling occurs when titanium-to-titanium (or titanium-to-steel) thread surfaces cold-weld under combined heat and pressure during assembly or disassembly. It is distinct from machining galling — this section covers both machining and assembly galling.

Machining Galling Prevention

Use TiCN-coated tap (not TiN — TiN reacts with Ti at elevated temperature)
Maintain 30–50 SFM (9–15 m/min) — exceeding 60 SFM (18 m/min) activates galling mechanism
Apply sulfurized or chlorinated tapping compound, not standard oil
Use 2-flute spiral-flute taps to minimize dwell time at each cutting edge
Prefer thread milling (no tap-to-wall contact on approach and exit)

Assembly Galling Prevention

Apply anti-galling compound: Molykote P-37, Loctite 771, or Jet-Lube SS-30 to threads before assembly
Specify class 2B fit for Ti-Ti thread pairs (not 3B — too tight)
Install titanium fasteners at low RPM with torque control (do not air-ratchet)
Use fluoropolymer-coated titanium fasteners (Xylan, Nylok) for frequent reassembly
Never torque titanium into a titanium tapped hole without lubricant

Thread Callout Guide

Thread Callout Specifications for Titanium

Thread callout specifications for titanium CNC parts
Thread Type	Drawing Callout	Tap Drill	Notes
UNF #10-32	10-32 UNF-2B THRU (or min depth)	#21 (0.159 in. / 4.04 mm) standard; #19 for 65%	Fine thread for small precision fasteners
UNC 1/4-20	0.250-20 UNC-2B ×0.500 MIN FULL THD	#7 (0.201 in. / 5.11 mm) standard	Common structural fastener in titanium brackets
UNF 1/4-28	0.250-28 UNF-2B ×0.500 MIN FULL THD	#3 (0.213 in. / 5.41 mm) standard	Fine thread for vibration-prone or thin-wall applications
Metric M6×1.0	M6×1.0 6H ×12 MIN FULL THD	5.0 mm standard	Per ISO 965 class 6H; 2B UNF equivalent
Metric M8×1.25	M8×1.25 6H ×16 MIN FULL THD	6.8 mm standard	Common in high-performance metric fastener applications
Helicoil insert	#10-32 UNC-2B HELICOIL PER MS21209-F3D10 OR EQUAL	Helicoil tap drill specific	Use Helicoil for repeated assembly Ti threaded holes; recommend for ≥ 5 insertion cycles

Common Questions

Frequently Asked Questions

Related Titanium Machining Resources

Titanium CNC Machining Guide

Complete pillar guide covering grades, speeds/feeds, tooling, and cost.

Titanium CNC Design Guidelines

DFM rules for walls, corners, holes, threads, and cost reduction.

Titanium Machining Tolerances

Achievable tolerance ranges, GD&T guidance, and DFM cost rules.

Quote Threaded Titanium Parts

MakerStage sources CNC machined titanium parts with tapped, thread-milled, or Helicoil-insert holes. Upload your STEP file to review thread strategy, callout risks, and sourcing options before production starts.

Review Titanium Threading Quote