Key decisions
- State the full thread designation and the required usable thread length.
- Leave process-specific space for entry, runout and the bottom of a blind hole.
- Inspect threads in their specified final condition, including relevant coatings.
A thread callout needs more than a diameter
A threaded feature connects geometry to assembly behavior. Two holes with the same nominal diameter can differ in pitch, tolerance class, hand, usable length and whether the thread is straight or tapered. A quotation should not infer these details from a generic three-dimensional hole or a note that says tapped.
Sandvik separates thread profile, pitch, size and other thread characteristics when describing process selection. For a drawing, the practical requirement is a complete designation under the governing thread standard, followed by the depth and any special acceptance requirements. Identify left-hand or multiple-start threads explicitly when applicable.
Also describe the joint function. A screw that locates a cover, a repeatedly adjusted mechanism and a sealed fluid connection need different engineering checks. Nominal thread engagement alone cannot establish strength, fatigue resistance or sealing. The responsible designer should assess the mating fastener, material, loads and installation conditions.
Separate the dimensions inside a blind hole
Required full-form thread length is the length that must contain the specified complete thread. Drilled depth describes the prepared hole and needs an unambiguous reference: the full-diameter cylindrical portion and the drill-point tip are not the same endpoint. Actual screw engagement depends on the installed screw, entry chamfer, intervening components and any incomplete thread at the bottom.
The tool also needs space. A tap has an entry portion before it generates complete thread form, while another threading method has its own approach and clearance requirements. A drawing that puts full-form thread exactly against a blind bottom may force a special route or be infeasible as specified. Confirm the selected tool geometry rather than adding an unexplained standard allowance.
| Item | What it describes | What it does not establish |
|---|---|---|
| Nominal thread designation | Size, pitch and the specified thread system and class | The installed engagement or strength of the joint |
| Full-form thread length | Required usable complete thread in the part | The total depth of the drilled preparation |
| Full-diameter drilled depth | Length of the cylindrical hole before the point region | Clearance for every possible tapping or milling tool |
| Screw engagement | Actual mating overlap in the assembled joint | That the screw cannot bottom out elsewhere |
| Bottom or runout clearance | Space beyond usable thread for the selected route | A universal value suitable for all thread tools |
Compare tapping and thread milling in context
Tapping can be productive for suitable thread sizes, materials and quantities. Cutting and forming taps need different preparation and material suitability checks; changing between them is not simply a tool swap into an unchanged hole. Sandvik emphasizes that tap design and application must match the material and task.
Thread milling offers a different way to control size through the programmed path. EMUGE explains that tool-offset adjustment can change the produced diameter and that secure holding, chip evacuation and correct feed calculation remain important. These benefits do not make thread milling automatically faster or safer for every small hole.
For purchasing, process selection can remain with the supplier unless the drawing or qualification requirements mandate a method. Define the accepted thread, required depth and final condition, then request clarification where the geometry creates risk. If a thread insert is proposed, treat it as a design change with its own installation and inspection requirements.
Worked example: an M6 blind hole with limited depth
This illustrative example concerns geometric clearance only. It is not a fastener-strength calculation or a recommended thread specification for an actual assembly.
The assembly needs a separate bottoming check. A screw can reach the blind bottom before clamping the joint, or engage fewer complete threads than the nominal hole length suggests. Include the screw length tolerance, washer or cover thickness and entry geometry in that review. A longer thread is not automatically an improved joint if it creates a clearance conflict.
Do not equate a 12 mm drilled depth with 12 mm of usable thread
Assume an M6 × 1 internal thread needs 9 mm of full-form thread, and temporarily exclude the entrance chamfer from this simplified depth budget. For a candidate process only, suppose the selected tool drawing requires 2 mm beyond that length for its entry geometry, and the process review reserves another 1 mm of bottom clearance. The cylindrical preparation then needs at least 12 mm under those assumptions. If a drawing calls out 12 mm to the drill-point tip, the full-diameter hole is shorter and the assumed route no longer fits. The designer and supplier must resolve the reference, available wall thickness, entrance chamfer and actual tool dimensions before release.
Specify the thread after finishing
A coating or other surface treatment can change the fit of mating threads. Identify whether the acceptance requirement applies before or after the final finish and whether the thread should be masked. Do not ask a supplier to compensate for an unspecified coating while expecting an unchanged final gauge result.
Agree on the gauging method, sampling and any depth verification. A mating production screw can provide useful assembly information but is not automatically a substitute for the specified thread gauge. Conversely, a thread gauge result alone does not prove joint preload, pull-out strength or leak tightness.
For Beigain RFQs, provide a thread schedule when many similar holes occur in one component. Each entry should connect the designation and depth to a feature identifier so repeated sizes with different requirements cannot be confused.
- Give the full thread designation, standard and tolerance class.
- Identify through or blind condition and the required full-form length.
- Distinguish cylindrical drilled depth from drill-point depth.
- Check actual screw engagement and bottoming at assembly extremes.
- State coating, masking and the final thread acceptance condition.
- Specify thread gauges, depth checks and required report coverage.
- Approve changes to thread depth, inserts or sealing geometry before machining.
Questions about this topic
How deep should a threaded hole be?
The joint design determines required engagement; the chosen manufacturing route determines additional preparation and clearance. There is no single depth multiplier suitable for every material, load and thread tool.
Can a bottoming tap make complete threads to a flat blind bottom?
The actual tool still has geometry and clearance requirements. Check its drawing and process allowance rather than interpreting the term bottoming as zero unused space.
Is thread milling always preferable to tapping?
No. It can offer useful size adjustment and process options, while tapping may be productive for suitable features. Compare the real size, material, quantity and available access.
Should threads be inspected before or after anodizing or plating?
The drawing should define the final acceptance condition. In-process checks may support manufacturing, but they do not replace final verification when the surface treatment changes the thread fit.
Technical references
- Sandvik Coromant: Threading — Primary guidance on thread characteristics and selection of threading processes.
- Sandvik Coromant: Tapping — Primary guidance on matching cutting/forming tap designs to their material and application.
- EMUGE-FRANKEN: Three Reasons to Give Thread Milling a Chance — Toolmaker discussion of thread-milling size adjustment and application conditions. The blind-hole allowance example uses explicit hypothetical inputs.
Continue reading
- CNC Turning Services
- CNC Milling Services
- Surface finishing and critical dimensions: a specification guide
- Preparing a CNC RFQ that suppliers can quote accurately
READY TO SOURCE YOUR PART?
Get a machining quote for your drawing.
Send your drawing, material and quantity. Beigain reviews the machining features, finish and inspection requirements with your quotation.
Upload drawing for a quoteDownload the RFQ checklist (PDF)
