Rigid tapping
An efficient route for repeated internal threads. For blind holes, select the tap lead and chip evacuation method before fixing the bottom allowance.
Specify the thread standard, full engagement length and final inspection condition before the tool is selected.
Compare tapping, thread milling and single-point turning. Review metric, Unified inch, pipe and STI insert threads together with blind-hole clearance and post-coating gauging.
Review geometry, material and clearance. The route determines tool access, chip evacuation and the way the finished thread is checked.
An efficient route for repeated internal threads. For blind holes, select the tap lead and chip evacuation method before fixing the bottom allowance.
Review helical milling where pitch diameter adjustment, material or bottom clearance matters. Confirm cutter access, reach and the entry path.
Suitable for external threads on shafts and accessible internal threads on turned parts. Review the thread to the turning datum and provide tool runout space.
| Engineering check | Rigid tapping | Thread milling | Single-point thread turning |
|---|---|---|---|
| Bottom or runout allowance | Start with 3P–4P for the tap lead and bottom clearance. | Review 1P–1.5P with cutter geometry and tool path. | Dimension the relief or usable runout at the shoulder. |
| Fit and datum control | Control pilot location and alignment. Match the tap and gauge to the class. | Use cutter compensation where appropriate, then verify pitch diameter and the final finish. | Keep the thread aligned to the functional turning datum; specify geometry separately. |
| Production trade-off | Check chip evacuation and the effect of tool wear in deep holes. | Allow for tool-path time, cutter size and reach relative to the hole. | Review tool access for left-hand, special-pitch or multi-start threads. |
The examples show which thread, seal and inspection details to specify for each type of part.
For a 316L manifold design, identify each port as NPT, BSPP or the specified alternative. Define the sealing interface and the port gauge.
For a 6061-T6 housing, specify the insert part number, installation depth and the required order of finishing and installation.
For Grade 5 titanium, mark the pitch, functional turning datum and thread relief. Agree the gauge and finish condition.
For POM or PEEK, confirm the exact stock grade, wall stiffness and the conditioning or fit check needed after unclamping.
Choose a thread family to review drawing details. Use the calculator below for common coarse metric blind holes.
| Standard and designation | Drawing and acceptance details |
|---|---|
| ISO 261 / GB/T 193 · M1–M64 | Give the diameter, pitch, tolerance class and full thread depth. Use the specified internal or external class, such as 6H or 6g, and identify the final coating condition. |
| Standard and designation | Drawing and acceptance details |
|---|---|
| ASME B1.1 · UNC / UNF | State UNC or UNF, diameter, threads per inch and class. Separate internal classes 2B or 3B from external classes 2A or 3A. |
| Standard and designation | Drawing and acceptance details |
|---|---|
| ISO 228-1 · G / BSPP · G1/16″–G2″ | For a parallel G port, specify the appropriate seat and separate seal. Agree seat geometry and surface texture with the mating part. |
| ASME B1.20.1 / B1.20.3 · NPT / NPTF · 1/16″–2″ | Specify NPT or NPTF explicitly. Agree the applicable gauge, reference position and final surface condition. |
| ISO 7-1 · R / Rc / Rp | Give the full R, Rc or Rp designation and sealing arrangement. Check the mating part against the same specified standard. |
| Standard and designation | Drawing and acceptance details |
|---|---|
| STI · NASM33537 / DIN 8140 | Specify insert type, nominal screw thread, length and depth. Confirm the STI receiving thread, gauge, installation and tang removal if applicable. |
| Masking or pitch diameter allowance | Agree the affected surfaces, thickness and actual buildup for the selected finish. Specify pre-treatment allowance or masking and gauge after finishing when required. |
| Item | Capability and conditions |
|---|---|
| Metric internal and external | ISO 261 / GB/T 193 · M1–M64 · 6H / 6g · 5H / 4h / 6h |
| Unified inch internal and external | ASME B1.1 · #0-80 UNF / #2-56 UNC – 2½″ UNC/UNF · 2B / 2A · 3B / 3A |
| Parallel and taper pipe threads | G / BSPP (ISO 228) · G1/16″–G2″ · R / Rc / BSPT (ISO 7-1) · NPT / NPTF (ASME B1.20.1 / B1.20.3), 1/16″–2″ |
| Thread inserts | STI · NASM33537 / DIN 8140 |
| Blind thread depth and clearance | Start at 1.5D–2.5D. Tapping up to 3D and reviewed thread milling 3.5D–4D. Allow 3P–4P at the bottom for tapping or check 1P–1.5P when milling. |
| Final-condition inspection | Use calibrated plug or ring gauges and taper gauges where required. For coating, agree pitch diameter compensation or masking, then gauge in final condition. |
D is nominal diameter, P is pitch. Confirm thread direction, grade and special fit on the drawing.
Estimate depth from nominal diameter D, pitch P and engagement. These values are for drawing review. Confirm against the actual cutter, chip clearance and tool travel.
The cylindrical depth excludes the drill point. The pilot diameter is a cutting-tap reference. Confirm the pre-hole for the selected thread mill and finished minor diameter.
Set the gauge and sampling plan before machining. Identify the surfaces that must be masked or otherwise protected through delivery.
Use plug gauges for internal threads, ring gauges for external threads, and the applicable tapered gauge for pipe threads. Set gauge insertion limits and inspection coverage by standard and drawing.
Mark surfaces to mask before anodizing or coating. Where needed, pack finished threads in separate pockets or protect them with caps.
Check 2D and 3D revisions, thread designation, full depth and bottom clearance.
Choose the tool, gauge and inspection conditions for the specified thread.
Check full-form depth, gauge fit and specified positional features on the first article.
Apply the specified masking or finish and verify threads in the agreed final condition.
Control tool wear and apply the agreed sampling or full inspection at key features.
Protect threads during transit and retain the released drawing and inspection records for repeat orders.
Add one or more process routes or blind-hole estimates to the brief. Attach it to your drawing inquiry together with the final finish and inspection requirements.
Select a process or add a blind-hole estimate above.
State the standard, pitch or TPI, class, handedness and depth of complete threads. If a mating screw governs the fit, include its specification.
Allow space for tool lead-in and chips. The calculator estimates clearance for tapping and thread milling using typical planning factors. Confirm the actual tool geometry and drill point for the drawing.
Mark the final fit and any protected surfaces. Agree masking or pitch-diameter allowance for the selected treatment, then verify in the final condition.
Provide the insert part number, type, length and installation depth. Request separate prices for the STI receiving thread, insert supply and installation as needed.