English English 
You've broken three taps this week. Sound familiar? Thread milling could slash your tool costs by 40% while producing threads that actually meet spec. We're talking zero broken tools, adjustable thread sizes, and the ability to cut threads larger than your spindle.
Here's what you'll master:
● Thread milling fundamentals and tooling selection
● Programming techniques for single-point and multi-form cutters
● Speed, feed, and depth calculations that work
● Internal vs. external threading strategies
● Multi-start thread programming shortcuts
● Troubleshooting common thread quality issues
● Cost analysis: when thread milling beats tapping
At TEAM MFG, we've thread milled everything from M2 medical screws to 6-inch pipe threads. Our CNC machining team uses these exact techniques to deliver precision threads across 73 countries. Want us to handle your threading challenges? Let's talk.
Thread milling creates screw threads using a rotating cutter that follows a helical toolpath. Unlike tapping, which forces a thread form into material, this process cuts threads with a smaller-diameter tool moving in a spiral pattern.
Picture drawing circles while slowly lifting your pen. That's thread milling - circular interpolation combined with vertical movement. The cutter shaves material away layer by layer, leaving behind precise thread geometry.
Taps are thread-specific. An M10x1.5 tap cuts only M10x1.5 threads. Thread mills? Totally different game. A single tool handles:
● Multiple thread sizes (adjust your circle diameter)
● Any thread pitch (change your Z-axis movement)
● Both internal and external threads
● Left or right-hand threads
You need thread milling when:
● Threading near the bottom of blind holes
● Working with expensive materials (no broken taps)
● Creating threads larger than your spindle
● Producing interrupted threads (like on a shaft with a keyway)
● Cutting exotic thread forms
Drill or bore the hole to a minor diameter
Position the cutter at the start point
Arc in tangentially to avoid witness marks
Perform helical interpolation for thread length
Arc out tangentially
Retract to clear the part
The beauty? If power fails mid-cycle, you haven't destroyed your part. Just restart where you left off. Try that with a stuck tap.
Thread milling is a helical interpolation process where a rotating cutter moves in a circular path while simultaneously moving along the Z-axis. Think of it like drawing a spiral staircase with a pencil.
Here's the deal. Taps push material. Thread mills cut it. This means:
● One tool, multiple sizes - Adjust your program to cut M6 or M8 with the same cutter
● No more stuck tools in expensive parts
● Cut threads bigger than your machine's spindle
● Left-hand? Right-hand? Same tool does both
You've got three main players:
● Single-Point Thread Mills: One cutting edge profiles any pitch within its range. Perfect for low-volume shops or those oddball thread specs.
● Multi-Form Thread Mills: Multiple teeth matching your thread pitch. These rip through production jobs 3-5x faster than single-point tools. The catch? You need a different tool for each pitch.
● Combination Drill/Thread Mills: Drill and thread in one shot. Saves tool changes but limits your depth options.
Your tool coating depends on what you're cutting:
Material | Best Coating | Why |
Aluminum | Uncoated/ZrN | Prevents built-up edge |
Steel | TiAlN | Handles the heat |
Stainless | TiCN/TiAlN | Fights work hardening |
Titanium | PVD AlTiN | Extreme heat resistance |
Pro tip: Thread mills with eccentric relief grind better in tough materials. The extra clearance prevents rubbing on the minor diameter.
When TEAM MFG switched our medical device client from tapping to thread milling, their reject rate dropped from 8% to 0.3%. Same tools handled metric and imperial threads without missing a beat.
Programming thread mills stumps machinists who think like tap users. Here's the truth: you're creating a toolpath, not forcing a thread. Let's break down both approaches.
Single-point cutters require you to program each thread pass. Your CAM might handle this, but understanding the math saves your bacon when things go sideways.
The basic formula? Helical interpolation = circular motion + Z-axis movement
For a M10x1.5 internal thread:
Position at thread start (X/Y center, Z at top)
Arc in at 90° to avoid tool marks
Complete 360° while dropping Z by pitch (1.5mm)
Repeat for thread depth
Arc out at 90°
What is thread milling if not controlled cutting? You decide the radial depth per pass. Start with 25-30% of pitch for roughing, finish with 10%.
Multi-form thread mills work differently. The cutter length covers your entire thread, so you make one helical pass at full depth. Sounds scary? It's actually safer than tapping.
G02 X_ Y_ Z_ I_ J_ (or G03 for climb milling)
Your Z-move equals one pitch, not the full thread length. The tool's multiple teeth handle the rest.
Thread mill direction matters:
● Climb milling (G03 for right-hand threads): Better finish, less deflection
● Conventional (G02): Use when your machine has backlash issues
Forget the tap speeds you're used to. Thread milling runs 2-3x faster because you're not fighting chip evacuation.
Surface Speed (SFM):
● Aluminum: 600-1000 SFM
● Mild Steel: 150-250 SFM
● Stainless: 100-150 SFM
● Titanium: 50-80 SFM
Calculate your RPM:
RPM = (SFM × 3.82) ÷ Cutter Diameter
Here's where people mess up. Your feed has two components:
Cutting feed (inches per tooth): 0.001-0.004" depending on material
Helical feed: Must maintain constant chip load during the spiral
Most CAM software handles this automatically. If programming manually, reduce your straight-line feed by 20-30% to compensate for the helical path.
Single-point thread mill cutter:
● First pass: 60-70% of full thread depth
● Second pass: 25-30%
● Spring pass: 5-10% (same depth, cleans up deflection)
Multi-form cutters:
● One pass at 100% depth (yes, really)
● Reduce feed rate by 40% compared to the single-point
Never exceed 75% thread engagement in tough materials. You want strong threads? Control your minor diameter, not chase 100% engagement.
Real numbers from our shop floor: switching an aerospace client from 100% to 75% engagement increased their pull-out strength by 15%. Less material stress during cutting meant better thread form.
Quick math for radial depth:
Radial Depth = (Major Dia - Minor Dia) × 0.75 ÷ 2
Your thread milling cutter will thank you with longer tool life and threads that actually gauge correctly.
Internal and external threads demand different approaches with your thread milling cutter. Get this wrong, and you'll wonder why your threads look like they went through a blender.
Internal CNC thread milling follows specific rules to avoid disasters:
Tool Selection Matters: Your thread mill tool needs 20-30% clearance from the minor diameter. Cramming a fat cutter into a small hole? You'll get chatter, a poor finish, and threads that won't gauge.
Rule of thumb for 5-axis CNC mill work:
Max Cutter OD = Minor Diameter × 0.7
Chip Evacuation Strategy
● Start from the bottom, work up (chips fall away)
● Use climb milling for better chip control
● Blast coolant through the spindle if possible
● Add pecking cycles for deep threads
External thread cutting brings different challenges. Your CNC milling operation has more room, but rigidity becomes critical.
● Stick-out should be a minimum of 1.5x thread diameter
● Support long shafts with a tailstock or steady rest
● Consider back-chamfering for clean thread starts
Internal threads (M10x1.5 example):
G02 X10.0 Y0 Z-1.5 I-5.0 J0 (Climb mill, right-hand)
External threads (M10x1.5 example):
G03 X10.0 Y0 Z-1.5 I5.0 J0 (Conventional, right-hand)
Notice the I-value sign change? That's your radial direction flip.
Sometimes you still need taps. Here's the breakdown:
Use Thread Milling When:
● Hole depth exceeds 2x diameter
● Material costs over $50/pound
● You need an adjustable thread fit
● Running a CNC milling services job with multiple thread sizes
Stick with Taps For:
● High-volume, single-size production
● Through holes in soft materials
● Threads under M6 (tool rigidity issues)
Multi-start threads on a thread milling machine used to mean calculator marathons. Not anymore. These tricks cut programming time by 75%.
Instead of calculating new coordinates, use your CNC mill's rotation feature:
(2-START THREAD EXAMPLE)
#100 = 0 (START ANGLE)
WHILE [#100 LT 360] DO1
G0 G90 X0 Y0
G68 R#100 (ROTATE COORDINATE)
(YOUR THREAD MILLING CYCLE HERE)
G69 (CANCEL ROTATION)
#100 = #100 + 180 (360° ÷ 2 STARTS)
END1
This approach to cut a thread works for any number of starts. Just divide 360 by your start count.
For machines without coordinate rotation:
Mill your first thread complete
Rapid to start position
Shift Z up by: Pitch ÷ Number of Starts
Run the same program
Three-start thread with 2mm pitch? Shift up 0.667mm between starts.
Angular Spacing:
Degrees between starts = 360 ÷ Number of starts
Z-Axis Shift:
Z shift = Thread pitch ÷ Number of starts
Lead Calculation:
Lead = Pitch × Number of starts
Your CAM might handle this automatically, but knowing the math saves you when it doesn't.
At TEAM MFG, we programmed a 4-start worm gear that stumped three other shops. Using the index method, we delivered 50 units in half the quoted time. Our CNC milling services team now uses these shortcuts on every multi-start job.
Pro tip: Always cut a test piece in aluminum first. Multi-start threads are unforgiving - one decimal point error ruins everything.
Your threads look like garbage? Let's fix that. Here's what goes wrong and how to solve it.
● Symptoms: Gauge goes in too easy, sloppy fit
● Causes & Fixes:
○ Tool deflection → Reduce radial engagement to 50%
○ Worn insert → Check cutting edges under magnification
○ Wrong compensation → Verify G41/G42 values
○ Thermal growth → Let spindle warm up for 20 minutes
Those ugly waves ruin everything. Attack them with:
● Drop RPM by 20% (breaks harmonic frequency)
● Switch from climb to conventional milling
● Add a spring pass at 70% feed rate
● Check tool stick-out (max 4:1 ratio)
Quick fixes:
● Increase coolant concentration to 8-10%
● Slow feed rate by 30%
● Try a different coating (TiB2 works magic on aluminum)
● Ensure proper speeds for your material
Your threads gauge at top but not bottom? Classic deflection issue.
● Use shorter tools
● Program multiple spring passes
● Consider a tapered pre-bore (0.001" per inch)
● Reduce cutting forces with smaller stepovers
Thread milling costs more upfront, but wins long term.
Thread milling wins when:
(Part value × Scrap risk %) > (Extra cycle time × Shop rate)
Real numbers:
● Titanium aerospace fitting: $800 part value
● Tap breakage risk: 5%
● Risk cost: $40 per part
● Extra thread milling time: 45 seconds
● Shop rate: $150/hour = $1.88 per part
You save $38.12 per part by thread milling.
● High volume + low value: 10,000 aluminum brackets
● Through holes in mild steel under 2x diameter
● Standard threads in soft materials
● Shop rate under $75/hour
Always thread mill when:
● Part value exceeds $200
● Blind holes deeper than 1.5x diameter
● Material harder than 35 HRC
● Need adjustable thread class
● Running exotic materials
● Making multiple thread sizes
People forget these expenses:
● Tap inventory (20 sizes × 3 pitches = $$$$)
● Emergency tap removal ($500 minimum)
● Machine downtime for broken taps
● Quality holds from out-of-spec threads
If you're breaking one tap per 100 parts in anything pricier than cold-rolled steel, switch to thread milling yesterday.
Thread milling isn't complicated once you grasp the fundamentals. You've learned the tools, techniques, and math that separate successful threads from scrap bins.
Key takeaways:
● Thread mills outlast taps in tough materials and blind holes
● Single-point cutters offer flexibility; multi-form delivers speed
● Proper speeds/feeds prevent 90% of thread quality issues
● Calculate true costs, including scrap risk and tool inventory
● Multi-start threads become simple with coordinate rotation tricks
At TEAM MFG, we've thread milled parts that other shops returned with broken taps still stuck inside. Our CNC team applies these exact techniques across aerospace, medical, and automotive projects. Whether you need prototype threads or production runs, we'll deliver threads that gauge right the first time.
Thread milling uses a rotating cutter moving in a helical path to create threads. The tool follows a circular motion while advancing along the Z-axis by one thread pitch per revolution, cutting material away to form precise thread geometry.
Thread mills create internal and external threads in holes, shafts, and specialized parts. They're perfect for blind holes, large diameter threads, expensive materials where broken taps mean scrapped parts, and situations requiring adjustable thread fit.
Taps cut threads using a form tool that matches the exact thread size—one tap per thread. Thread mills use a smaller cutter following a programmed path, allowing one tool to cut multiple thread sizes, pitches, and both left/right-hand threads.
Major benefits include:
● No broken tools stuck in parts
● One tool cuts multiple thread sizes
● Better chip control in blind holes
● Ability to adjust thread fit via programming
● Creates threads larger than spindle capacity
● Works in interrupted cuts
Thread cutting removes material to create a helical groove. The cutting tool advances parallel to the workpiece axis while the part rotates (lathe) or the tool follows a circular path (milling). Each pass deepens the groove until reaching the final thread dimensions.
