How Should You Specify Threaded Holes for a CNC-Machined Part?
Short answer: specify a CNC threaded hole with an unambiguous drawing or model-based callout—not only a threaded-looking cylinder. State the thread standard and form, nominal size, pitch or threads per inch, class/tolerance, quantity and location, through or blind condition, required full-thread depth, total hole depth when needed, entry treatment, and inspection expectation. Also provide the actual mating fastener or its controlled specification.
Customers searching “how do I specify a threaded hole for CNC?” are usually trying to prevent three failures: the right-looking but wrong thread, a bolt that bottoms before clamping, or a blind hole that cannot be manufactured to the depth implied by CAD. A clear callout lets the designer, machinist and inspector discuss the same requirement.
1. Put the full thread identity in the product definition
A thread name must distinguish the system and geometry. For metric threads, nominal diameter and pitch are fundamental. For inch-series threads, nominal size and threads per inch are required, along with the series where applicable. Add the class or tolerance designation that controls fit. State left-hand explicitly when required; otherwise do not rely on a visual helix to communicate handedness.
ASME Y14.6 establishes requirements for representing, specifying and dimensioning screw threads on drawings, while dimensional control belongs to the applicable thread standards. Autodesk’s hole/thread tools similarly separate type, size, designation, class, length and offset. The lesson is practical: “M6 hole” or “1/4 thread” is incomplete.
| Callout element | Question it answers | Common ambiguity if omitted |
|---|---|---|
| Standard/form and nominal size | Which thread family? | Metric versus inch or wrong profile |
| Pitch or TPI | How far between turns? | Coarse/fine mismatch |
| Class/tolerance | What fit limits apply? | Unknown allowance and gauge basis |
| Through/full-thread depth | How much usable engagement? | Bolt bottoms or insufficient thread |
| Quantity and location | Which holes receive it? | Threading the wrong feature set |
2. Separate the thread requirement from CAD appearance
For machined parts, fully modeled threads are often unnecessary. Autodesk notes that cosmetic threads are normally sufficient for milling, while modeled threads may be useful for 3D printing. A detailed helix can increase file complexity and can be wrong even when it looks convincing. The callout is the controlling manufacturing communication.
Use a proper hole or thread feature in CAD when possible because it preserves recognizable intent and can populate drawing notes. Still review the generated note. Confirm that a supplier opening only the STEP file can identify the threaded features from the accompanying drawing or marked-up requirement. Do not encode a thread only in a filename or email sentence separated from the affected hole.
3. Design blind holes with real bottom allowance
A tap does not produce full-profile thread to its extreme tip. A drilled blind hole also commonly ends with a drill-point shape unless a flat bottom is specifically produced. Space is needed beyond the required full-thread length for tool lead, chips and process clearance. Therefore “thread 12 mm deep in a hole 12 mm deep” is not a complete or generally feasible instruction.
State the minimum required full-thread depth and, when controlling, the total hole depth. Leave material below the hole appropriate to the load and part geometry. Consider whether the mating screw can enter without bottoming, including washers and tolerance stack. For very deep blind threads, chip evacuation and tool reach become more demanding.
A through hole usually simplifies chip evacuation and depth, but it may expose the far side, leak, collect contamination or interfere with another feature. Choose through versus blind from function, not from an assumption that one is always cheaper.
4. Provide tool access and a usable entry
The spindle and tool must approach on the hole axis. Nearby walls, ribs, shoulders and deep counterbores can restrict the holder even when the cutting tool itself fits. Show the complete surrounding geometry. If the thread starts beneath a counterbore, verify that the tool and gauge can reach it.
A small entry chamfer can remove burrs and help a fastener start, but its size should not consume the required engagement or sealing surface. Cross-holes and interrupted threads require discussion because they affect cutting and burrs. If the thread is tapered, port-related or sealing, identify the exact standard and any orientation or gauging requirement rather than treating it like a general fastener hole.
5. Decide whether direct threads or inserts serve the application
Directly machined threads can be suitable for many assemblies, but the application may justify a helical-coil, solid or key-locking insert. Repeated service, wear, repair strategy, clamp load, parent material and available boss size all matter. Inserts are not interchangeable decorations: each system requires a specified preparation thread, installation tool, depth and surrounding material.
Provide the insert manufacturer/series or an approved equivalent policy, the installed position, and whether installation is included. Confirm that the mating screw length accounts for the insert and does not bottom in the prepared hole. If inserts are prohibited, state that too; otherwise quotations may not be comparable.
6. Define inspection and send a quote-ready package
Standard internal threads are commonly evaluated with suitable go/no-go plug gauges, supported by visual checks and any required functional verification. The gauge must match the thread standard, size and class. A production screw may confirm assembly but does not by itself establish the complete acceptance limit. Special, tapered or safety-critical threads may require additional methods.
- Mark every threaded hole and its quantity.
- Specify standard/form, nominal size, pitch/TPI and class.
- State right/left hand when nonstandard or relevant.
- Distinguish through, full-thread depth and total blind-hole depth.
- Identify counterbores, chamfers, cross-holes and restricted access.
- Select any insert system and installation responsibility.
- State the inspection/documentation needed.
For a MALIEV CNC quotation request, send STEP/native CAD and a drawing or marked-up view containing this information, plus material, quantity, finish, mating fastener and functional load context. This enables a manufacturability review without inventing a thread specification from a rendered model.
Frequently asked questions
Is a modeled helix enough to specify a CNC thread?
No. The manufacturing requirement should identify the thread standard/form, nominal size, pitch or TPI, class or tolerance, depth/through condition and any inspection requirement. A modeled helix can be ambiguous or unnecessarily heavy.
What is the difference between thread depth and hole depth?
Thread depth is the required length of usable full thread. Hole depth is the total drilled depth, which may need extra space for the tap lead, chip clearance and drill point. They should not be treated as the same value in a blind hole.
When should I use a threaded insert in aluminum?
Consider an insert when the application needs repeated service, wear resistance, repairability, a larger load-bearing thread system or isolation from direct aluminum-thread wear. Select the insert system first because its preparation hole and installation requirements affect the part.
How are internal CNC threads inspected?
The method depends on the requirement. Standard internal threads are often checked with appropriate go/no-go plug gauges and visual/functional checks. Special or critical threads may need additional specified measurement and documentation.