Almost every part we machine at SAMSHION has threads: tapped holes for covers and brackets, external threads on turned connectors and the occasional pipe thread on a manifold. We machine metric, UNC/UNF and pipe threads such as NPT and G to the customer’s drawing, and the smallest thread we have machined is M1.2. Every thread is checked with go and no-go thread gauges before the parts ship.
Threads look simple on a drawing, yet a thread can look fine and still fail assembly because its pitch diameter, depth, position or entrance is wrong. This guide explains what to put on the drawing, how we choose between tapping, thread milling and lathe threading, how to design blind holes and threaded inserts, and how we inspect threads and deal with thread problems. For the wider service, see our CNC machining services.
What Information Belongs in a Thread Callout?
A supplier should never have to guess the thread system or the acceptance requirement. A complete callout gives:
- Nominal size and pitch (metric) or threads per inch (UNC/UNF)
- Internal or external thread, and left-hand if it is not a standard right-hand thread
- Tolerance class, for example 6H for an internal metric thread or 2B for a Unified internal thread
- Full thread depth, stated separately from drill depth in blind holes
- The thread standard, when the product or customer requires it
For Unified inch threads, ASME B1.1 defines thread forms, classes and designations. ISO metric thread tolerances are covered by ISO 965. These standards define the thread itself; the drawing still has to show where the thread is, which face it must be square to and how deep it goes.
We Machine to the Depth on Your 2D Drawing
We machine every thread to the depth shown on the 2D drawing. If that depth would break through a wall or leave too little material at the bottom of the hole, we contact the customer before machining instead of changing the depth ourselves. A thread with no depth on the drawing gets the same question.
Untoleranced dimensions around the hole follow ISO 2768-mK, our default general tolerance, which we confirm with each customer before production. The values are listed in our ISO 2768 general tolerances chart.
Show Which Face Controls the Thread Axis
A threaded hole often locates a cover, bracket or connector. In that case, thread position and axis orientation matter more than appearance. Establish functional datums and apply tolerances that reflect the assembly. Our design for manufacturability guide explains why requirements should follow function rather than arbitrary precision.
Tapping, Thread Milling or Single-Point Turning?
There is no fixed thread size at which we switch from a tap to a thread mill. The material is the first deciding factor. As a general pattern, smaller internal threads are tapped and larger ones are thread-milled. On the anodized plate above, the large threads were thread-milled and the small holes were tapped. External threads on turned parts are cut on the lathe with a threading tool.
- Tapping: fast and economical for standard internal threads. Chip evacuation, torque and the risk of a broken tap need attention, especially in blind holes.
- Thread milling: a tool smaller than the thread cuts it along a helical path. Chips stay short, the finished size can be adjusted with tool compensation and one tool can cut several diameters of the same pitch. It takes longer to program and run.
- Single-point turning: a threading tool on the lathe cuts external threads on round parts, concentric with the other turned diameters.
When Tapping Is Efficient
Tapping is usually the fastest method for common internal threads. The tap cuts the complete thread as it advances at a feed synchronized with the spindle. The pilot-hole diameter, tap geometry, coolant and machine synchronization all affect torque and thread quality.
Through holes clear chips more easily than blind holes. Blind-hole tapping needs a deliberate chip strategy and enough clearance below the last full thread. A broken tap in a nearly finished part is costly, so on valuable parts a slower but safer method can be worth it.
When Thread Milling Reduces Risk
A thread mill follows a helical toolpath and cuts the thread progressively. Because the tool is smaller than the finished thread, a broken thread mill is usually easier to remove than a broken tap, and radial compensation can bring the pitch diameter into tolerance without changing the programmed pitch.
Thread milling makes sense where chips are hard to control, where one pitch is needed in several diameters, on expensive parts, and on large threads that would need excessive tapping torque. The trade-off is extra programming and cycle time.
External Threads on the Lathe
External threads on our turned parts are cut with a single-point threading tool on the lathe, usually in the same setup as the diameters and shoulders around them, so the thread stays concentric with the rest of the part. Leave room for the tool to run out before a shoulder, or add a thread relief groove. Rotational features are best reviewed together; see our CNC turning services.
How to Design a Reliable Tapped Hole
Provide Tool Access and Entrance Clearance
The tool must approach along the thread axis. Nearby walls, bosses and overhangs can block the spindle, holder or gauge even when the hole itself is visible. A small entrance chamfer helps start the fastener, protects the first thread and removes a sharp edge, but it should not remove needed engagement.
Avoid Unnecessary Depth
More thread depth does not automatically produce a stronger joint. Required engagement depends on the screw and parent materials, load direction, thread size, fastener grade and how often the joint is assembled. Excessive depth adds drilling and threading time without improving the joint, and deep small threads raise the risk of a broken tap.
Place Threads Away From Fragile Edges
Threads close to a thin wall or free edge can distort during machining or tightening. The remaining material must carry installation torque and service load. If space is restricted, consider a larger boss, a local rib, a through-fastener, an insert or a different joint. For flexible geometry, see our thin-wall CNC machining guide.
Account for Surface Finishing
Anodizing, plating and other coatings add thickness on the thread flanks and can make a thread tight. Decide on the drawing whether threads are masked during finishing or accepted after finishing. When a thread becomes tight after finishing, we normally run a tap through it again; for the next batch we can mask the threads before the parts go to finishing. Available treatments are listed on our surface finishing page.
Blind Holes Need a Complete Depth Stack
A useful blind-hole definition separates four zones: entrance chamfer, full-form thread, incomplete thread or tool runout, and drill-point clearance. The exact stack depends on the drill and threading method, so the drawing should focus on the functional thread depth and avoid an unnecessarily tight hole-bottom requirement.
If the fastener must stop at a precise axial position, use a shoulder, spacer or controlled boss height instead of letting the screw bottom in the drilled hole. A bottomed screw gives unpredictable preload and can damage the incomplete threads.
Threaded Inserts: Wire Thread, Press-In and Heat-Set
We install threaded inserts when the customer’s drawing calls for them. The right type depends on the parent material:
- Wire thread inserts (helical coil inserts) work in both metal and plastic parts. They give a durable steel thread in aluminum or plastic that will be assembled many times.
- Press-in and heat-set inserts are for plastic parts only. Plastic is soft and has a low melting point, so the insert can be pressed or melted in and the plastic locks around its knurls.
Choose the insert before finalizing the boss diameter and hole depth, because the insert needs its own pilot hole, thread and installation access. An insert does not fix every weak joint: edge distance, remaining wall and load path still need review. For aluminum parts, our guide to helical coil and key-locking thread inserts compares the two main options. The plastic parts below have press-in inserts.
How We Inspect CNC Threads
Every thread is checked with thread gauges, and both ends must pass: the go gauge must screw in over the required depth, and the no-go gauge must not enter beyond the limit set by the standard. Internal threads are checked with thread plug gauges and external threads with thread ring gauges. Looking at a thread cannot prove its pitch diameter, so we never accept threads visually.
This short video was filmed during thread gauge inspection in our factory.
A CMM is useful for thread position and its relationship to datums, but it does not replace a functional thread gauge. Our inspection reports guide explains how drawing characteristics connect to gauges, CMM programs and reports, and our quality assurance page covers the wider control plan.
Inspection Questions to Answer Before Production
- Is the thread standard and tolerance class identified?
- Can the gauge reach the full thread depth?
- Must the thread axis relate to a datum or mating feature?
- Will the thread be inspected before or after surface finishing?
- Does the customer require a dimensional report, material certificate or first article package?
Thread Problems and How We Handle Them
- Broken tap in the part: we remove it by EDM, which erodes the hard tap without cutting the part, so a nearly finished part can often be saved. It is the same spark erosion process we use with copper EDM electrodes for cavities and sharp corners.
- Stripped or torn threads: we find out whether a wrong tap size or wrong cutting parameters caused it, scrap the part and machine a new one, and record corrective and preventive actions.
- Go gauge will not enter: we rework the thread, but first check whether the gauge is inaccurate or the tap is worn, so the cause is fixed and not just the part.
- Thread tight after finishing: we re-tap the thread, or mask the threads before finishing the next batch.
- Fastener cross-threads: usually a poor entrance or an axis error; a controlled chamfer and a position check solve most cases.
DFM Checklist for CNC Threads
- State the complete thread designation and standard.
- Separate full thread depth from total drilled depth.
- Provide straight tool and gauge access.
- Use functional tolerances and datums.
- Review edge distance and remaining wall thickness.
- Decide whether threads are masked or re-tapped after finishing.
- Choose the insert type before fixing the boss size.
- Identify the inspection method and documentation level.
Request a Threaded-Part Review
Upload a 3D CAD model and a 2D drawing showing thread callouts, critical datums, material, quantity and finish. Our engineers review tool access, blind-hole depth, thread method, inserts and inspection before machining, and contact you if a thread depth or position needs to change. Request a quote.
Frequently Asked Questions
Is thread milling always better than tapping?
No. Tapping is often faster for standard repeated holes. We choose by material first; thread milling becomes attractive when chip control, broken-tool risk, diameter adjustment or part value matter more than the shortest cycle.
Should a blind tapped hole be drilled only to the thread depth?
Normally no. The drill point and threading tool need extra space beyond the full thread. The allowance depends on the tooling and process plan.
What is the smallest thread you can machine?
The smallest thread we have machined is M1.2. Very small threads need careful tap selection and a realistic depth, so send the drawing for review.
Which thread standards do you machine?
Metric coarse and fine threads, UNC and UNF, and pipe threads such as NPT and G. We machine whichever standard is on your drawing.
Can the same thread mill cut different diameters?
Often it can cut several diameters that share the same pitch and profile, within tool and machine limits. The toolpath sets the finished diameter.
Do coated threads need special planning?
Yes. Coating thickness can make a thread tight. Define whether threads are masked or accepted after finishing; we re-tap tight threads after finishing or mask them in advance.
Can a broken tap be removed without scrapping the part?
Often, yes. We remove broken taps by EDM, which erodes the tap without cutting the surrounding material.
Which threaded insert should I use in a plastic part?
Press-in and heat-set inserts suit plastic because it is soft and melts at a low temperature. Wire thread inserts can be used in plastic and in metal.
Is a CMM enough to inspect every thread?
No. A CMM checks thread position and related geometry, but functional acceptance uses go and no-go thread gauges.


