Tapping vs Thread Milling: CNC Threading Process Guide

Tapping vs thread milling is one of the most important process choices for CNC internal threads. Both methods can produce accurate, functional threads, but they do not create them in the same way. Tapping uses a tool with the full thread form and pitch to cut or form the thread in one axial motion. Thread milling uses a rotating milling cutter and coordinated circular movement to generate the thread progressively.

For a buyer, the best choice is not simply the method with the shortest cycle time. A broken tap in an expensive nearly finished part can cost far more than the tool itself. On the other hand, thread milling every small standard hole may add unnecessary machining time. Hole type, thread size, material, depth, quantity, machine capability, inspection requirements and the cost of a rejected part all influence the decision.

This guide compares tapping and thread milling, explains the main tool types, covers blind and through holes, identifies common defects and gives designers and purchasing teams a practical RFQ checklist for CNC threaded parts.

What Is CNC Tapping?

CNC tapping produces an internal thread by feeding a tap axially into a prepared hole. The tool already contains the pitch and thread profile. As the spindle turns, the machine must advance at a feed that matches that pitch. For a 1.5 mm pitch, for example, the tap advances 1.5 mm per spindle revolution.

In rigid tapping, the CNC synchronizes spindle rotation and Z-axis motion. At the programmed depth, the spindle reverses and the tap follows the same helix out of the hole. Some machines use a tension-compression holder to accommodate a small amount of synchronization error, but the holder cannot correct a fundamentally wrong feed, pitch or program.

Tapping is popular because it is fast. A tap can produce the complete thread in a single entry-and-return cycle. Standard metric and inch taps are widely available, and the process is efficient for repeated small and medium internal threads.

However, the tap occupies most of the hole. Chips, cutting fluid and the tool must share limited space. Torque rises rapidly when chips pack, the pilot hole is undersized, the thread is deep or the material work-hardens. If the tap breaks, removal can be difficult because the tool may be harder than the workpiece and may be locked below the surface.

What Is Thread Milling?

Thread milling generates a thread with a milling cutter that is smaller than the finished thread diameter. After entering the pilot hole, the tool moves in a circular path while also moving axially by one pitch per revolution of the path. This coordinated motion is called helical interpolation.

The cutter removes the thread form progressively rather than engaging the entire circumference at once. Cutter compensation can adjust the toolpath to control pitch diameter and compensate for tool wear. A spring pass or additional radial pass may be used when material springback, tool deflection or a demanding fit requires it.

Thread milling requires a CNC machine capable of simultaneous X, Y and Z interpolation. It also requires enough hole diameter for the cutter and enough control to program the correct helix. According to the Sandvik Coromant threading application guide, the method is especially useful for asymmetric or non-rotating parts, difficult-to-machine materials, threads near the bottom of blind holes and unstable or thin-walled components.

Because the cutter is smaller than the hole, chips have more room to evacuate. If a thread mill breaks, the fragment is often easier to remove than a broken full-diameter tap. The method is usually slower than tapping for a single small thread, but it offers process flexibility and can reduce the financial risk on high-value parts.

Tapping vs Thread Milling at a Glance

This table describes general tendencies. The exact result depends on the machine, tool, holder, material, coolant, thread geometry and production volume.

Types of Taps Used in CNC Machining

The word “tap” covers several tool designs. Selecting the correct type is essential for chip flow and tool life.

Spiral-Point Taps

Spiral-point taps, sometimes called gun taps, push chips forward in the direction of tool travel. They are commonly used for through holes because chips can exit beyond the threaded section. They should not be selected for a blind hole when chips have nowhere to go.

Spiral-Flute Taps

Spiral-flute taps pull chips back toward the hole entrance. They are commonly chosen for blind holes and materials that produce continuous chips. The flute helix, rake and number of flutes should match the material and thread depth. Haas tap guidance distinguishes this chip-lifting action from the forward chip flow of spiral-point taps.

Straight-Flute Taps

Straight-flute taps have relatively simple geometry and may be used for short-chipping materials, hand operations or applications where neither pushing nor pulling a long chip is required. Their suitability depends strongly on material and hole type.

Cutting Taps

A cutting tap removes material to form the thread. It creates chips and therefore needs appropriate flute geometry, lubrication and chip evacuation. The tap drill establishes the approximate minor diameter before tapping.

Form Taps or Roll Taps

A form tap displaces material plastically instead of cutting it. It produces no chips and can create a strong, smooth thread in sufficiently ductile materials. The pilot hole must be larger and more closely controlled than for a cutting tap because the material flows inward to create the thread crest.

Form tapping can be attractive for aluminum, mild steel and some stainless alloys, but it is not suitable for every material. Brittle materials such as gray cast iron generally do not flow as required. Material composition, hardness, ductility, wall thickness and lubricant all need review. A cutting-tap drill chart must never be reused blindly for a form tap.

Tap Chamfer Styles

Taps are also described as taper, plug or bottoming styles. A longer chamfer distributes cutting across more teeth and reduces load per tooth, but it needs more axial room before a complete thread form is reached. A bottoming tap has a short lead that can create full threads closer to the bottom, but the shorter lead places greater load on fewer teeth.

The drawing should state the required full-thread depth, not only the drilled depth. A tap cannot produce a complete thread through its lead section.

Types of Thread Mills

Thread mills also come in several configurations.

Single-Profile Thread Mills

A single-profile cutter has one main row of thread-form teeth. It generates the complete thread by traveling axially through multiple pitches during the helical toolpath. One cutter may produce several thread diameters that share the same pitch and profile, provided the tool fits the pilot hole and the application stays within the manufacturer’s range.

Single-profile tools are flexible and reduce inventory, but their longer path can increase cycle time.

Multi-Row or Full-Profile Thread Mills

A multi-row tool has several teeth distributed along an axial length. It can generate a thread with a shorter helical movement, often approximately one pitch plus entry and exit motion. This improves productivity, but the tool must match the pitch and requires sufficient axial room. Deflection and the simultaneous engagement of several teeth still need control.

Indexable Thread Mills

Larger threads can be milled with an indexable tool body and replaceable inserts. This can be economical for large diameters, special profiles or production work. The tool assembly needs adequate clearance and rigidity.

Solid-Carbide Thread Mills

Solid-carbide tools are common for small to medium threads. Their rigidity and wear resistance support accurate profiles, but runout, holder quality and excessive overhang can still cause taper or premature wear.

Combination Drill, Chamfer and Thread-Mill Tools

Application-specific tools can combine pilot-hole machining, chamfering and thread milling. They reduce tool changes and can improve feature concentricity, but they sacrifice some flexibility and require careful process validation.

When Tapping Is Usually the Better Choice

High Quantities of Standard Small Threads

For many identical M3, M4, M6, 1/4-20 or similar threads, tapping often gives the lowest cycle time. A correct tap can enter, create the complete thread and reverse out quickly. The time advantage becomes significant when a plate or housing contains dozens of threaded holes.

Stable, Proven Production Processes

When the material, pilot hole, tool, holder, coolant and machine have already been validated, tapping can be extremely reliable. Automatic tool-life management and torque monitoring make the process more predictable in production.

Machines Without Helical Interpolation

Older machines may support tapping but not simultaneous three-axis helical interpolation. In that case, thread milling may be unavailable without changing equipment or control capability.

Very Small Threads

Thread mills must fit inside the pilot hole and retain enough core diameter for strength. For very small threads, a suitable thread mill may be fragile, expensive or unavailable. Micro-tapping may be more practical, although it demands excellent runout, hole preparation and process control.

When Cycle Time Dominates Part Risk

On a low-cost component with easy access and a well-established process, the faster tapping cycle may matter more than the lower breakage consequence of thread milling.

When Thread Milling Is Usually the Better Choice

High-Value or Nearly Finished Parts

A broken tap can scrap a costly component after most machining is complete. Thread milling lowers this risk because cutting forces are generally lower and a broken tool is usually smaller than the hole. Aerospace housings, complex prototypes, medical components and low-volume precision parts often justify the additional cycle time.

Large or Nonstandard Threads

Large taps require high torque and are expensive to stock. Thread milling can produce large diameters with a smaller tool. It also suits special diameters, unusual pitch diameters and some nonstandard thread profiles when the correct cutter and programmed path are available.

Multiple Diameters with the Same Pitch

A thread mill may create several internal or external thread diameters that share its pitch. Haas thread-mill guidance also notes the ability to produce right- or left-hand and internal or external threads with suitable programming. This flexibility reduces dedicated tool inventory for prototype and mixed-batch manufacturing.

Tough or Work-Hardening Materials

Titanium, nickel alloys and some stainless steels can create high tapping torque and work-hardening problems. Thread milling divides the cut and gives chips room to escape. The toolpath, coating, cutting data and coolant still need to be designed for the exact alloy.

Blind Holes Close to the Bottom

A tap lead needs extra depth before full-form threads begin, and chips may pack below the tool. A thread mill can often machine usable threads closer to a blind bottom because it does not need a long chamfered lead beyond the full thread. Bottom clearance is still necessary for entry, exit, chip space and the uncut pilot-hole shape.

Thin Walls and Unstable Setups

The progressive cutting action can reduce peak force compared with full-form tapping. This is useful for thin bosses, flexible walls or parts with limited clamping support. The programmer can use multiple radial passes to reduce deflection.

Pitch-Diameter Adjustment

Cutter compensation allows the machinist to adjust thread size without replacing the tool. This is valuable when compensating for wear, material springback, heat-treatment allowance or coating thickness. The adjustment must be validated with a proper thread gauge.

Interrupted or Asymmetric Features

Thread milling can work around some cross holes, interruptions or asymmetric parts that are difficult for a tap. The interrupted cut may still cause vibration, so entry position, cutting direction and radial engagement require planning.

Blind Holes vs Through Holes

Hole type changes both tool selection and the drawing information a supplier needs.

Through-Hole Threads

A through hole provides space beyond the required thread. A spiral-point tap can push chips ahead and out of the hole. The fixture must leave clearance so the tap and chips do not strike a backing plate. Breakthrough burrs may also need deburring.

Thread milling a through hole is flexible because chips can exit either side. The programmer still needs a safe lead-in, sufficient tool overtravel and an approach that avoids leaving a witness mark at the start and end of the interpolation.

Blind-Hole Threads

A blind-hole callout should separate at least three depths:

• Total drilled or cored depth.

• Minimum full-diameter pilot-hole depth.

• Minimum full-thread depth.

The drill point, tap lead, bottom chips and safety clearance all consume depth beyond the last complete thread. Specifying “M6 × 1, 12 mm deep” without identifying whether 12 mm means drill depth or full thread depth creates ambiguity.

For tapping, a spiral-flute or suitable form tap may be used depending on the material. The process must prevent chips from compacting at the bottom. For thread milling, the tool needs room to enter and interpolate, but it can normally control the last full thread more closely.

Do not make a blind hole deeper than necessary without considering cleaning and inspection. Deep threaded holes increase tool reach, chip-removal difficulty and gauge-access problems.

Pilot Hole Size and Thread Percentage

The pilot hole is one of the strongest influences on tapping torque and thread quality. If it is too small, the tap removes or displaces excessive material, increasing torque and breakage risk. If it is too large, thread height and strength may be insufficient.

There is no single correct “percentage of thread” for every application. The functional load, material, engagement length, thread standard, cutting or forming process and supplier data all matter. A high thread percentage can add a large amount of torque while providing little practical strength benefit in some materials. Conversely, an excessively large pilot hole can fail the gauge or joint requirement.

For a cutting tap, use the applicable thread standard and tap manufacturer’s drill recommendation as the starting point. For a form tap, use the form-tap-specific recommendation. Confirm the actual drilled hole because drill runout, material and tool wear can make it differ from the nominal drill diameter.

Thread milling also starts from a pilot hole, but the cutter creates the thread by radial interpolation. The pilot must provide tool clearance while leaving enough material for the complete thread profile. On large threads, the pilot hole may be drilled, bored or circular-interpolated to control location and size.

Rigid Tapping, Feed and Synchronization

In rigid tapping, feed per revolution must equal the thread pitch. If the machine commands the wrong pitch, uses an incorrect unit conversion or loses synchronization during reversal, the tap can stretch, compress, cut an incorrect lead or break.

Important checks include:

• Correct metric or inch pitch in the program.

• Correct spindle direction for right- or left-hand threads.

• Machine control configured for rigid tapping when required.

• Holder and collet suited to the tool shank.

• Minimal tool runout.

• Sufficient acceleration and reversal capability for the selected speed.

• Safe clearance and exact programmed depth.

Increasing spindle speed does not always improve productivity. The machine must decelerate, reverse and accelerate without losing synchronization. Small taps and deep holes may need conservative speed even when the cutting material could theoretically run faster.

Thread-Milling Toolpath and Cutting Direction

Thread milling requires correct helical direction, cutter compensation and entry strategy. A wrong combination can create the wrong hand, cut the wrong diameter or drive the tool into uncut material.

Climb milling is commonly preferred when the machine and setup are suitable. The tool may enter below the thread, arc into the cut, interpolate upward or downward depending on the thread and program, then arc out. Tool suppliers provide recommended methods because the correct path depends on internal or external threading, right- or left-hand form and cutter geometry.

A smooth tangential entry reduces the mark left where the cutter begins. For demanding thread fits, the machinist may rough the profile, measure it, apply cutter compensation and take a finishing or spring pass.

Thread-mill diameter matters. A large cutter is rigid and productive, but it follows a tighter orbital path and may create more profile distortion because the cutter’s nominal form is projected around the thread diameter. Toolmaker guidance should be followed for the allowed cutter-to-thread size ratio.

Chip Control and Coolant

Tapping Chips

Cutting taps create chips in a confined space. A spiral-point tap directs them forward; a spiral-flute tap lifts them backward. The wrong style can pack chips in the hole, chip the tap teeth, damage the new thread or break the tool.

Coolant must reach the cutting zone and provide the necessary lubricity. Tapping is sensitive to friction because multiple teeth contact the thread simultaneously. Through-tool coolant can help in deep holes, but pressure, concentration, filtration and compatibility with the material all affect the result.

Form tapping creates no chips, but it still requires effective lubrication. Sliding and deformation generate heat and friction. An inappropriate lubricant can produce torn crests, pickup or excessive torque.

Thread-Milling Chips

Thread milling creates smaller, more manageable chips and leaves open space around the cutter. Air blast or coolant can clear chips before they are recut. In blind holes, chips should be removed from the bottom before inspection or assembly.

The Sandvik thread-milling troubleshooting guide links poor results to factors such as vibration, tool overhang, cutting data and toolpath. Chip control is important, but it does not compensate for an unstable holder or excessively aggressive engagement.

Material-Specific Considerations

Aluminum

Aluminum is generally easy to tap and thread mill, but built-up edge can affect finish and pitch diameter. Sharp polished tools and suitable lubricant help prevent material from welding to the edge. Form tapping is possible in many ductile aluminum alloys, provided the pilot diameter and wall thickness are controlled.

Carbon and Alloy Steel

Both processes are common. Hardness, heat treatment and alloy content determine tool material, coating and speed. A thread required after hardening may need thread milling with a suitable carbide tool, grinding or another specialized method rather than conventional tapping.

Stainless Steel

Stainless steels can be gummy, work-harden and generate high friction. A dull tap or repeated rubbing can harden the surface ahead of the tool. The process needs correct geometry, positive cutting action, stable feed and effective lubricant. Thread milling is often attractive for difficult grades or expensive parts, but the tool must avoid dwelling and rubbing.

Titanium

Titanium has low thermal conductivity and can cause heat concentration and tool wear. Tapping torque and seizure risk can be high. Thread milling reduces engagement and allows staged radial cuts, making it a common choice for critical titanium parts. Conservative cutting data, short overhang and coolant delivery remain important.

Nickel-Based Alloys

Nickel alloys combine strength, heat and work hardening. Thread milling can reduce catastrophic tool-breakage risk, but it is not automatically easy. The toolmaker should specify coating, cutting speed, radial passes and tool life limits for the exact alloy.

Cast Iron

Cast iron often produces short, abrasive chips. Cutting taps and suitable thread mills can both work. Form tapping is normally unsuitable because the material lacks the required ductility. Dust and fine chips need appropriate machine protection and cleaning.

Engineering Plastics

Plastics can deform, melt, recover elastically or produce stringy chips. A thread may measure differently after it cools or after the tool is removed. Sharp tools, low heat and adequate chip clearance are important. Metal thread inserts may be better for repeated assembly, high clamp load or creep-sensitive polymers.

Thread Accuracy, Fit and Tolerance Classes

Thread size is not defined only by major and minor diameter. Pitch diameter controls how the mating flanks engage and is central to thread fit.

Common drawing callouts include classes such as 2B or 3B for Unified internal threads and tolerance classes such as 6H for ISO metric internal threads. These designations must be interpreted using the applicable standard. A tighter class can increase process control and inspection cost without improving function if the assembly does not need it.

The manufacturing process does not change the specified class. A tapped and a thread-milled M8 × 1.25-6H thread must both satisfy the same functional requirement. However, thread milling offers convenient pitch-diameter adjustment through cutter compensation.

Surface treatment must be considered. Anodizing, plating, coating or paint can reduce internal thread size. Options include machining to an agreed pre-coating allowance, masking the threads, chasing them after treatment when permitted or installing an insert. The drawing and purchase order should state the expected final acceptance condition.

Internal vs External Threads

Taps create internal threads. External threads are normally produced with a die, single-point turning, thread rolling, grinding or thread milling.

Thread milling can create both internal and external threads if the tool and machine access allow it. This is useful on parts that are already set up on a machining center and cannot conveniently move to a lathe. External thread milling also permits diameter adjustment and can create threads on large bosses without a large die.

For an external thread, the designer should provide relief, shoulder clearance and an acceptable runout region. A full thread cannot normally continue into a square shoulder without a groove, undercut or incomplete last thread.

Common Tapping Problems and Solutions

Broken Tap

Possible causes include an undersized pilot hole, packed chips, excessive thread depth, wrong tap style, high runout, poor lubrication, incorrect speed, work hardening or synchronization error.

The corrective action is not simply to slow the machine. Measure the pilot hole, confirm chip direction, inspect the broken tool, verify coolant delivery and review torque. Haas tap-breakage guidance specifically highlights blind-hole chip packing, pilot-hole size, lubrication and the difference between cutting and form taps.

Oversized Thread

An oversized internal thread may result from tap runout, misalignment, built-up edge, an incorrect tool, holder movement or material springback. Verify with a calibrated gauge and inspect tool condition before changing the program.

Undersized Thread or NO-GO Failure

Tool wear, coating buildup, an incorrect tolerance-class tap or material recovery can make the thread tight. Confirm that the gauge and part are clean and at a stable temperature. Do not force the GO gauge.

Torn or Rough Threads

Dull edges, built-up material, poor lubrication, wrong cutting data or chip recutting can tear the flanks. In form tapping, incorrect pilot size and inadequate lubricant can create malformed crests.

Bell-Mouthed Entry

Runout, poor guidance or an unstable holder can enlarge the first threads. An entry chamfer should guide assembly without removing excessive functional engagement.

Common Thread-Milling Problems and Solutions

Tapered Thread

Tool deflection can make the pitch diameter vary with depth. Reduce overhang, use a more rigid holder, select a larger suitable cutter, reduce radial engagement or use multiple passes. A finishing pass can improve consistency after the bulk of material is removed.

Chatter or Faceted Finish

Chatter may come from excessive overhang, weak workholding, aggressive cutting data, poor entry or an unsuitable toolpath. Inspect the pitch-diameter surface and not only the visible crest. Adjust one controlled factor at a time.

Incorrect Pitch Diameter

Wrong cutter compensation, tool diameter, interpolation radius or wear offset can create a tight or loose thread. Measure with the correct gauge and adjust the radial offset according to the machine control and toolmaker’s procedure.

Entry Witness Mark

An abrupt radial move can leave a mark where the cutter enters. A tangential arc-in and arc-out reduces this effect. The start point can also be positioned away from the most functionally sensitive area.

Wrong-Hand Thread or Wrong Lead

Because the thread depends on programmed movement, the toolpath must match internal or external geometry and right- or left-hand direction. Simulate and verify the program before cutting an expensive part.

Inspecting CNC Threads

GO/NO-GO Plug Gauges

For a standard internal thread, a calibrated GO/NO-GO plug gauge provides efficient functional inspection. The GO member checks the combined effect of several thread features and should enter according to the applicable gauge standard. The NO-GO member is limited in how far it may enter.

Gauge acceptance rules depend on the cited thread and gauge standards. “It turns in” is not a complete inspection method. The part and gauge must be clean, damage-free and at an appropriate temperature.

Thread Ring Gauges

External threads are commonly checked with GO/NO-GO ring gauges. Adjustable ring gauges require correct setting and calibration practices.

Pitch-Diameter Measurement

Specialized thread micrometers, three-wire measurement for external threads, indicating gauges or optical systems can quantify pitch diameter. Internal threads may require dedicated internal thread measurement equipment or indirect functional gauging.

Optical and Section Inspection

An optical comparator or microscope can inspect profile, lead and burrs on accessible or sectioned samples. Destructive sectioning is useful for process validation but is not practical for every production part.

CMM Inspection

A coordinate measuring machine can evaluate accessible large threads with an appropriate stylus and strategy, but a few probed points do not always represent full functional fit. CMM inspection should complement, not casually replace, recognized thread gauging.

Cleanliness Before Inspection

Chips, coolant residue, anodizing debris and burrs can cause false gauge failures or damage the gauge. Clean the thread without altering its edges, then inspect under controlled conditions.

Design Guidelines for Machined Threads

Use Standard Sizes and Pitches

Standard threads reduce tool cost, lead time and gauge availability problems. Use a special pitch only when it provides a real functional benefit.

Specify Full-Thread Depth Clearly

For blind holes, state the required full-thread depth and allow additional pilot depth for the tool lead, chip space and drill point. Do not dimension only an ambiguous hole depth.

Avoid Unnecessary Thread Depth

Very deep engagement increases machining and inspection difficulty. Joint strength is governed by material, diameter, pitch and engagement; more depth does not always produce a proportional improvement. Engineering analysis should determine the required engagement.

Add a Practical Entry Chamfer

A controlled chamfer helps start the tap and guides the mating fastener. An oversized chamfer can remove useful engagement or create a thin edge.

Provide Wall Thickness Around the Hole

Thin bosses can expand during form tapping or deflect during cutting. The boss outside diameter, distance to an edge and distance between adjacent holes should support the chosen process and service load.

Consider Runout and Shoulder Relief

Threads near a shoulder or blind bottom need space for the incomplete last thread and tool exit. A relief groove may be needed when the mating part must seat against a face.

Control Perpendicularity When Assembly Requires It

A thread may pass a plug gauge but still point at an angle relative to the mounting surface. If a long stud, connector or fastener alignment is critical, specify the relevant positional or orientation requirement.

Plan for Inserts

Helical wire inserts, key-locking inserts or solid threaded bushings may improve durability in soft materials, support repair or provide locking features. The drawing must identify the insert standard, material, installation depth, tang-removal requirement and final gauge condition.

Define Post-Finish Acceptance

State whether threads are gauged before or after anodizing, plating, passivation or coating. Identify masked areas and whether thread chasing is allowed.

Cost Drivers in a Threaded-Part Quotation

Thread machining cost is affected by more than the number of holes.

• Thread diameter, pitch and tolerance class.

• Cutting, forming or thread-milling process.

• Number of threaded features.

• Blind or through-hole condition.

• Full-thread depth and total pilot depth.

• Material, hardness and heat-treatment state.

• Tool access and required reach.

• Thin walls, interruptions or angled surfaces.

• Standard or custom tool and gauge availability.

• Required inspection frequency and documentation.

• Coating or finishing allowance.

• Part value at the stage when threading occurs.

• Production quantity and repeat-order forecast.

A supplier may choose tapping for production speed and thread milling for prototypes or expensive components. If your application requires one method, state why. Otherwise, specify the functional thread requirement and let the manufacturer select the most reliable process.

RFQ Checklist for CNC Threaded Parts

Provide the following information for an accurate quotation:

1. 3D CAD model and a controlled 2D drawing.

2. Thread standard, nominal size, pitch and tolerance class.

3. Right- or left-hand thread.

4. Internal or external thread.

5. Through hole or blind hole.

6. Minimum full-thread depth and total hole depth.

7. Quantity of each thread per part.

8. Part material, grade, condition and hardness.

9. Heat treatment and machining sequence requirements.

10. Surface finish or coating and final gauging condition.

11. Required thread inserts and installation specification.

12. Critical orientation, position or perpendicularity controls.

13. Gauge standard, inspection level and reporting requirement.

14. Prototype quantity, production quantity and annual demand.

15. Mating fastener information when fit or assembly is unusual.

For a broader quotation package, also use our CNC Machining RFQ Checklist.

Sample Threading RFQ Template

Please quote CNC machining for the attached model and drawing. The part material is 7075-T6 aluminum. The component has six M6 × 1-6H blind threads with a minimum full-thread depth of 12 mm and a total drilled depth of 18 mm. Threads must accept a calibrated GO gauge and reject the NO-GO gauge after Type II anodizing; masking is permitted. The thread axes are controlled by the drawing position tolerance relative to datums A, B and C. Please recommend tapping or thread milling, identify any required pre-coating allowance and include prototype and 500-piece pricing with the inspection plan.

This format separates the functional requirements from the manufacturing method while giving the supplier enough information to plan the process.

Frequently Asked Questions

Is thread milling better than tapping?

Neither method is universally better. Tapping is usually faster for standard small internal threads. Thread milling offers size adjustment, better chip clearance, multiple-diameter capability and a lower consequence if the tool breaks. Part value, material, depth and quantity determine the better choice.

Is thread milling more accurate than tapping?

Thread milling makes pitch-diameter adjustment convenient and can reduce deflection through multiple passes. A well-controlled tap can also produce accurate threads. Final accuracy depends on the complete machine, tool, holder, pilot hole, material and inspection system.

Can one thread mill cut different thread sizes?

Many single-profile thread mills can machine multiple diameters that use the same pitch and profile, within the cutter manufacturer’s allowed range. The cutter must fit the smallest pilot hole, and the CNC program must generate the correct diameter.

Can a thread mill make left-hand threads?

Often yes. A suitable cutter and toolpath can produce right- or left-hand threads and may also produce internal or external forms. Confirm capability with the tool manufacturer and verify the programmed direction.

Why do taps break in blind holes?

Common causes include chip packing, insufficient bottom clearance, an undersized pilot hole, wrong tap geometry, poor lubrication, excessive depth, runout and rigid-tapping synchronization errors. Inspect the failure before changing speed alone.

Does a form tap need a different pilot hole?

Yes. A form tap displaces material and normally needs a larger, more tightly controlled pilot hole than a cutting tap. Use the specific form-tap manufacturer’s data for the material and required thread.

How close can a thread go to the bottom of a blind hole?

It depends on the tap lead or thread-mill geometry, pilot-hole bottom, chip space and inspection requirement. Thread milling can often create a full thread closer to the bottom, but no method eliminates the need for clearance. Specify full-thread depth separately from total hole depth.

Should threads be inspected before or after anodizing?

The purchase specification should define the acceptance stage. Coating can reduce internal thread size. Threads may be masked, machined with an agreed allowance or inspected after finishing. The decision depends on the coating and assembly requirements.

Can thread milling repair an oversized or damaged thread?

It cannot restore material that has already been removed. It may be used to enlarge a damaged hole for an approved repair insert, but the repair must be supported by engineering disposition and adequate remaining wall thickness.

What information is most often missing from a thread callout?

Blind-hole full-thread depth, tolerance class, hand, post-coating acceptance and insert requirements are commonly omitted. A complete 2D drawing should control these details even when a 3D model is supplied.

Final Selection Guide

Choose tapping when the thread is standard, the hole and material are well understood, cycle time is important and tool-breakage risk is acceptable. Choose thread milling when the part is valuable, the material is difficult, the thread is large or nonstandard, bottom clearance is limited, size adjustment is important or one tool must cover several thread diameters.

The most reliable decision comes from the complete application rather than a simple rule. A supplier should review the drawing, material, pilot hole, thread depth, quantity, finishing process and inspection plan before selecting the tool.

AluPrototype provides CNC machining for prototypes and production parts with tapped, form-tapped, thread-milled and insert-reinforced threads. Explore our CNC machining article library or request a quote with your CAD files, drawing, material, thread callouts, quantities and inspection requirements.