In thread milling, a rotating cutter follows a helix to cut internal or external threads on a CNC machine. The cutter is smaller than the thread and cuts it step by step.
One tool can produce different diameters as well as right-hand and left-hand threads. At Vulcanus in Werl, Germany, we use thread milling mainly for tough materials and high-value parts.
This guide shows how thread milling works, which thread mills to choose and how to set reliable cutting data.
Key Takeaways on Thread Milling
- Thread milling is a CNC process for cutting precise internal and external threads.
- The cutter is smaller than the thread. Its diameter should be no more than 70% of the thread diameter.
- One cutter can produce right-hand and left-hand threads and several diameters with the same pitch.
- Most controls program feed at the tool centre. Without feed correction, the load per tooth is often three times too high.
- A broken thread mill can usually be removed. The part is saved.
- Thread milling takes longer per thread. For expensive parts and hard materials it still often pays off.
Thread Manufacturing at a Glance: Where Thread Milling Fits
Threads can be produced by cutting or by forming. Each process has its place in production:
| Process | Principle | Typical use |
|---|---|---|
| Tapping (thread cutting) | A tap cuts the full profile in one pass | Standard threads in series, free-machining materials |
| Thread forming | A forming tap displaces material without chips | Ductile materials such as aluminium and mild steel |
| Thread milling | A small cutter follows a helical path | Large, expensive or hard parts, blind holes, special threads |
| Thread turning | A turning tool follows the pitch on a lathe | Rotationally symmetric parts, shafts |
| Thread rolling | Rolls form the thread without chips | Screws and bolts in mass production |
| Thread whirling and thread grinding | Special processes for long or hardened threads | Lead screws, medical technology, precision threads |
Thread turning is one of the classic types of turning operations. Thread milling is one of the key types of milling operations on a machining centre.
What Is Thread Milling and How Does It Work?
Thread milling combines simultaneous movement on three axes. A 3-axis milling machine with helical interpolation is enough.
The thread mill rotates about its own axis while following a circular path in the X-Y plane. At the same time it moves exactly one pitch along the Z axis per revolution. This creates a helix that cuts the thread.
The circular path in X and Y sets the thread diameter. The Z movement sets the pitch. Because only a small part of the cutting edge is engaged, cutting forces and torque stay low.
Tool Path: Climb Milling for Right-Hand and Left-Hand Threads
Thread milling should use climb milling wherever possible. The chip starts thick and ends thin. This protects the edge and improves the thread flanks.
| Thread | Movement for climb milling (spindle clockwise) |
|---|---|
| Internal, right-hand | from the hole bottom upwards, counterclockwise (G03) |
| Internal, left-hand | from the top downwards, counterclockwise (G03) |
| External, right-hand | from the top downwards, clockwise (G02) |
| External, left-hand | from the bottom upwards, clockwise (G02) |
Our guide to climb milling vs conventional milling explains why climb milling is usually the better choice.
Soft Entry: Arc In Instead of a Radial Approach
The cutter should never move radially straight into the material. A tangential arc entry is better. Z rises by a quarter of the pitch for every quarter turn.
A soft entry prevents force peaks and edge chipping. It reduces vibration and noticeably extends tool life. The same principle applies when exiting the cut.
Types of Thread Mills
Thread mills differ in design and performance. The following three main types are the most widely used in CNC machining:
1. Straight-Flute Thread Mills
These tools have straight flutes between the cutting edges for universal chip removal. All cutting edges engage the workpiece at the same time, which limits cutting speed and feed rate. They are ideal for general applications and free-machining materials.
2. Helical-Flute Thread Mills
Here the flutes are arranged at a helix angle of typically 15° or 30°. The cutting edges engage the material one after another. This reduces lateral forces, improves chip evacuation and allows higher cutting speeds and smoother surfaces.
3. Single-Profile Thread Mills
Single-profile thread mills carry only one thread tooth per cutting edge. They mill the thread turn by turn and need several revolutions to do so. This takes longer but clearly reduces cutting forces, heat and tool deflection.
Single-profile mills suit hard materials, deep threads and fine threads. One tool covers many diameters with the same pitch.
Thread Milling Systems: Solid Carbide, Indexable Inserts and Combination Tools
The choice of thread milling system depends mainly on the thread diameter and the batch size.
- Solid carbide thread mills: the standard for small to medium threads, roughly M3 to M20. They are rigid, precise and often available with internal coolant.
- Thread mills with indexable inserts: economical for large diameters from about M20. When worn, you only replace the insert.
- Drill thread mills: drill, countersink and mill the thread in one tool. This saves tool changes, especially in aluminium and grey cast iron.
- Thread mills with a chamfer step: mill the thread and the chamfer in one pass.
Typical cases for thread milling are asymmetric parts, thin-walled workpieces and blind holes. Other cases are materials with difficult chip formation and expensive parts where a broken tap is not an option. You will find more CNC machining tools in our dedicated guide.
How to Choose the Right Thread Mill
Five questions help you choose a thread mill:
- Which thread type and pitch? ISO metric thread to DIN 13, fine thread, inch or pipe thread. The cutter profile must match the thread type.
- Which cutter diameter? No more than 70% of the thread diameter. A cutter that is too large distorts the profile at the thread root.
- Which thread depth? The usable length must match the thread depth. Every extra millimetre of overhang increases deflection.
- Which material? Coating and edge geometry depend on steel, stainless steel, cast iron, aluminium or hardened steel.
- Which batch size? Multi-row mills are faster in series. Single-row and single-profile mills are more flexible.
An example from Sandvik Coromant shows how much the cutter diameter matters for M30 × 3. A cutter with a 21.7 mm diameter produces about 0.07 mm profile deviation. With an 11.7 mm diameter it is only about 0.01 mm.
Choosing Between Single-Row and Multi-Row Thread Mills
- Single-row thread mills offer high flexibility for different pitches and need less drive power. They are especially suited to small or mixed batch sizes.
- Multi-row thread mills can mill and chamfer a thread in one pass. They are ideal for constant pitches and high volumes.
The Role of Cutting Inserts
- Full-profile inserts produce the complete thread profile (flank, minor diameter, crest) and deliver high-quality threads in fewer passes.
- V-profile inserts cover several pitches with minimal inventory. However, they require a pre-machined minor diameter and usually have a shorter tool life.
Cutting Data for Thread Milling
Starting Values for Solid Carbide Thread Mills
| Material | Cutting speed vc | Feed per tooth fz at the cutting edge |
|---|---|---|
| Mild steel, e.g. S235 | 100 to 150 m/min | 0.04 to 0.08 mm |
| Alloy steel, e.g. 42CrMo4 (AISI 4140) | 70 to 120 m/min | 0.03 to 0.06 mm |
| Stainless steel, e.g. 1.4301 (304) | 50 to 90 m/min | 0.02 to 0.05 mm |
| Grey cast iron, e.g. EN-GJL-250 | 80 to 140 m/min | 0.04 to 0.08 mm |
| Wrought aluminium alloy | 200 to 400 m/min | 0.05 to 0.10 mm |
| Titanium alloy, e.g. Ti6Al4V | 30 to 60 m/min | 0.02 to 0.04 mm |
| Hardened steel, 50 to 62 HRC | 30 to 60 m/min | 0.01 to 0.03 mm |
These values apply to cutters of about 6 to 16 mm diameter under stable conditions. The tool manufacturer’s data always takes priority. Sandvik Coromant recommends not exceeding 0.15 mm feed per tooth.
Our guide to cutting speed covers the basics of the calculation. When machining stainless steel, pay particular attention to sharp edges and small radial steps.
Feed Correction: The Most Common Programming Error
Cutting data refers to the cutting edge at the thread diameter. Most controls, however, expect the feed of the tool centre. In an internal thread, the tool centre travels a much shorter path than the cutting edge.
- Internal thread: vf (centre) = vf (edge) × (D − d) / D
- External thread: vf (centre) = vf (edge) × (D + d) / D
Here D is the thread diameter and d the cutter diameter.
Worked example M16 × 2, internal thread in alloy steel:
- Solid carbide thread mill with d = 11 mm and z = 4. That is just under 69% of D.
- vc = 100 m/min gives n = (100 × 1000) / (π × 11) ≈ 2,890 rpm.
- fz = 0.05 mm gives vf ≈ 0.05 × 4 × 2,890 ≈ 580 mm/min at the cutting edge.
- Corrected for the tool centre: 580 × (16 − 11) / 16 ≈ 180 mm/min.
If you program 580 mm/min here, each tooth carries 3.2 times the intended feed. Tool breakage is then very likely.
Number of Passes
Several radial passes reduce forces and tool deflection. This improves thread tolerance with long overhangs. In hardened and difficult materials, Sandvik Coromant always recommends at least two passes.
Cooling and Chip Evacuation
For thread mills with indexable inserts, Sandvik Coromant recommends dry machining with compressed air. Coolant increases temperature swings there and can cause thermal cracks. Coolant does help when finishing stainless steel, aluminium and heat-resistant alloys.
For solid carbide mills in blind holes, internal coolant or compressed air is useful. It flushes chips out reliably. Our comparison of dry machining vs wet machining covers both options, and our guide to coolant lubricants shows suitable media.
Tap Drill Sizes
Thread mills use the same tap drill sizes as taps. Choose the largest hole within the tolerance. This increases process reliability and tool life.
| Thread (ISO metric coarse) | M6 | M8 | M10 | M12 | M16 | M20 |
|---|---|---|---|---|---|---|
| Tap drill in mm | 5.0 | 6.8 | 8.5 | 10.2 | 14.0 | 17.5 |
Full-profile indexable inserts need a slightly smaller hole so that the thread crest is machined too.
Programming Thread Milling: G-Code Example
Thread milling is programmed with circular interpolation G02 or G03 plus simultaneous Z movement. Many controls offer ready-made cycles. Examples are Cycle 262 THREAD MILLING on Heidenhain and CYCLE90 on Siemens.
The following example mills a right-hand M16 × 2 thread with climb milling. It uses a multi-row solid carbide mill with d = 11 mm that covers the full thread depth. The program follows the tool centre without radius compensation.
(M16x2 internal thread, right-hand, climb milling, cutter D11, multi-row)
N10 G90 G54 G17
N20 S2890 M03
N30 G00 X0 Y0
N40 G43 H1 Z5.0
N50 G00 Z-22.0 (start point at the bottom)
N60 G03 X2.5 Y0 Z-21.0 R1.25 F90 (arc in, half pitch)
N70 G03 X2.5 Y0 Z-19.0 I-2.5 J0 F180 (360 degree helix = 1 pitch)
N80 G03 X0 Y0 Z-18.0 R1.25 F90 (arc out)
N90 G00 Z5.0
N100 M05
The path radius is (16 − 11) / 2 = 2.5 mm. Adjust the Z values to the thread depth and cutter length. Always test a new program in simulation first.
A big advantage: if the thread is too tight, increase the path radius by a few hundredths. This adjusts the fit without a new tool. Read more about programming in our guides to CNC G-code and the CNC programming language. For complex parts, a CAM system with thread milling strategies saves a lot of programming time.
Milling External Threads
External threads follow the same principle. The cutter circles the spigot instead of the hole. For a right-hand thread in climb milling, it moves clockwise from the top downwards.
With external threads, the radial depth of cut is usually smaller. Higher cutting speeds are therefore often possible. The tool centre feed is higher here than at the cutting edge.
Milling external threads pays off especially on parts that are not rotationally symmetric. Examples are spigots on housings, plates or welded assemblies that cannot be turned.
Key Advantages of Thread Milling
Thread milling offers many technical and economic advantages. This makes it an excellent choice for precision manufacturing, especially in mechanical engineering and industrial series production.
1. Superior Thread Quality and Dimensional Accuracy
Thread mills produce short chips that are easy to flush out. Chip packing, a common cause of damaged threads, hardly occurs. The thread flanks are clean and consistent as a result.
The fit can be fine-tuned through the path radius in the program. This reliably achieves tolerance classes such as 6H, even as the tool wears.
2. High Flexibility and Versatility
A single thread mill can produce internal and external threads, left-hand and right-hand threads and different pitches without multiple taps. This versatility reduces tool inventory, simplifies CNC programming and makes it easier to adapt to different parts.
3. Longer Tool Life and Lower Torque Requirement
Solid carbide thread mills need less torque, which generates less heat. This reduces tool wear, extends tool life and lowers the risk of costly scrap.
4. Ideal for Difficult Materials and Complex Geometries
Thanks to lower cutting forces, thread milling is especially suited to hard materials, blind holes and large bores. It also suits asymmetric or thin-walled workpieces that are hard to machine with conventional tapping.
5. High Process Reliability for Expensive Parts
If a tap breaks in a blind hole, the part is often scrapped. A thread mill is smaller than the hole. If it breaks, it can usually be removed and the thread finished.
Thread Milling: Limitations and Key Considerations
Despite its many advantages, thread milling has some practical points to consider:
1. Longer Cycle Times
Thread milling usually takes longer than tapping, especially for simple, small thread diameters. If production speed is the top priority, tapping can be more efficient in terms of cycle time.
2. Higher Demands on Machines and Programming
Successful thread milling requires a CNC machine with helical interpolation, simultaneous multi-axis movement and often a high-speed spindle. Shops without this equipment face higher investment costs.
3. More Complex Programming
Thread milling is more demanding to program than tapping. It requires precise calculation of tool paths, feeds and spindle speeds, as well as G-code for thread milling. Modern CAM systems and calculators can significantly reduce this effort.
4. Cost Factors and Expertise
Thread mills often cost more to buy, and setting up and running the process requires trained staff. For large series with constant thread sizes, tapping can still be the more economical solution.
5. Tool Deflection in Deep Threads
Slender thread mills bend under load. The thread then becomes tighter at the bottom than at the top. Shorter tools, several passes or a spring pass without new stepover solve this.
Thread Milling vs. Tapping: What Are the Differences?
Comparing thread milling and tapping shows that both processes have their own strengths and ideal applications:
| Aspect | Thread milling | Tapping |
|---|---|---|
| Speed | Slower, especially for small standard threads | Very short cycle times; ideal for series production |
| Thread quality & fit | Fit can be fine-tuned through the path radius | Good quality; size is fixed by the tap |
| Tool breakage | Cutter usually removable, part is saved | A broken tap often scraps the part |
| Flexibility | Several diameters, right-hand and left-hand threads with one tool | One tool per thread size and type |
| Chip form | Short comma-shaped chips, easy evacuation | Long helical chips, chip packing in blind holes possible |
| Material & application suitability | Ideal for hard materials, blind holes, large diameters or special threads | Effective for standard applications and free-machining materials |
| Setup & programming | Helical interpolation and feed correction required | Simpler and faster setup |
For a detailed comparison including costs, see our guide to thread milling vs. thread drilling.
When Thread Milling Pays Off: Decision Guide and Cost Example
Thread milling is the right choice when:
- threads must be cut in difficult or hardened materials
- large diameters or blind holes are involved
- flexibility in thread size or pitch is required
- the part is thin-walled or easily deformed
- the part value is high and a broken tap must be avoided
Cost example with assumptions: 2,000 M16 threads per year in stainless steel, machine hour rate €90.
| Item | Tapping | Thread milling |
|---|---|---|
| Extra time per thread | 0 s | + 12 s |
| Extra machine time cost | €0 | 2,000 × 12 s = 6.7 h × €90 = €600 |
| Tool cost | €30 per tap, 150 threads: €400 | €120 per cutter, 2,500 threads: €96 |
| Total | €400 | €696 |
In this example, thread milling costs about €300 more per year. A single avoided tap breakage on a part worth €400 already offsets that. Our guide on how to reduce per part cost shows how to factor such effects into your calculation.
Common Thread Milling Problems and Their Solutions
| Problem | Common cause | Solution |
|---|---|---|
| Thread too tight or too loose | wrong path radius, tool wear | correct the radius, check with a thread plug gauge |
| Tapered thread | tool deflection | shorter cutter, several passes, spring pass |
| Distorted profile at the root | cutter larger than 70% of the thread diameter | choose a smaller cutter |
| Edge breakage at entry | radial approach, feed not corrected | program an arc entry, convert feed to the tool centre |
| Chatter and feed marks | feed per tooth too high, long overhang | reduce fz, clamp the tool shorter |
| Left-hand instead of right-hand thread | wrong Z direction for the arc direction | check the tool path against the table above |
| Chip packing in blind holes | no flushing | use compressed air or internal coolant |
Many causes are the same as for general milling errors. To tackle vibration, read how to avoid vibrations during milling. Runout errors in CNC machining at the tool holder also shorten tool life noticeably.
Internal threads are checked with go/no-go thread plug gauges. Our guide to manufacturing tolerance explains how tolerance classes are defined.
Applications of Thread Milling
Thread milling has become established in many industries where precision, flexibility and material variety are decisive. These qualities fit the demands of mechanical and plant engineering perfectly.
Automotive
In the automotive industry, thread milling is often used for engine components, gearbox housings and chassis parts. The process is especially beneficial for light alloys or parts requiring fine threads and tight tolerances. Thanks to its low torque, it is ideal for thin-walled parts where deformation must be avoided.
Aerospace and Defence
In aerospace, thread milling makes it possible to produce high-precision threads in demanding materials such as titanium, Inconel or stainless steel. Excellent chip control is particularly important in blind holes in safety-critical parts such as turbine housings or structural brackets.
Medical Technology
Medical technology uses thread milling for implants, surgical instruments and device components. Special profiles, fine threads or multi-start threads are often required. Especially in titanium and stainless steel, the process scores with low cutting forces and high repeatability.
General Industrial Applications
In toolmaking and mechanical engineering, thread milling enables custom production of machine parts, tool holders, hydraulic components and much more. It suits small to medium series, prototypes and export threads for international supply chains.
Thread Milling at Vulcanus: Threads from Werl
Vulcanus-Stahl & Maschinenbau has been manufacturing in Werl, North Rhine-Westphalia, since 1984. Our production is ISO 9001 certified. Thread milling is a core part of our CNC milling services.
We mill threads in one-offs, small batches and large welded assemblies. In low volume manufacturing, one thread mill for several sizes saves setup time and tool cost. Through custom spare part manufacturing, you also get special threads made from a sample or drawing.
As a partner for CNC contract manufacturing, we deliver turning, milling, welding and assembly from a single source. Every thread goes through our quality control for CNC machining. That is our standard for precision manufacturing.
Conclusion on Thread Milling
Thread milling is a precise and flexible process for internal and external threads. It shows its strengths with hard materials, large diameters, blind holes and high-value parts.
Three points are decisive: a cutter of no more than 70% of the thread diameter, a corrected feed for the tool centre and a soft arc entry. With these, tool life, thread quality and process reliability all improve together.
Do you need precise ISO metric threads or special profiles? Contact us and send us your drawing for a quote.
Frequently Asked Questions About Thread Milling
1. What is thread milling?
Thread milling is a CNC machining process that creates threads using a rotating tool that follows a helical path. Unlike tapping, it cuts threads with a smaller-diameter cutter, offering more flexibility and precision.
2. When should I use thread milling instead of tapping?
When machining hard materials, thin-walled parts, blind holes or special threads. It is ideal when maximum precision, longer tool life and minimal breakage risk are required.
3. Can one thread mill be used for different thread sizes?
Yes, as long as the pitch stays the same. A cutter for a 1.5 mm pitch can produce M10 × 1.5 and many fine threads with a 1.5 mm pitch. This reduces tool costs and inventory.
4. Is thread milling suitable for blind holes?
Yes. The short chips are easy to flush out with compressed air or coolant. The cutter also mills the thread close to the hole bottom, with a short thread runout.
5. Which materials are suitable for thread milling?
Thread milling suits steel, stainless steel, cast iron, aluminium, titanium and nickel-based alloys. With special solid carbide mills, hardened steels above 60 HRC can be machined too. Plastics and composites are also possible.
6. What machine do you need for thread milling?
A CNC milling machine with at least three axes and helical interpolation is enough. Rigidity, runout accuracy and a stable tool holder matter more than spindle power. A dedicated thread milling machine is usually not necessary.