A blind tapped hole has at least two different depths that designers often collapse into one number: the usable full-thread depth needed by the fastener, and the drilled hole depth needed by the manufacturing process.
Those values are usually not identical. A drill has a point. A tap has a lead before it produces full-form threads. Chips and tool overtravel also need room. If the CAD model ends the pilot hole at exactly the required full-thread depth, the shop may have to change the geometry or process.
Start with the functional requirement
Ask what the joint needs: thread size and pitch, thread class or fit where required, minimum full-thread engagement, whether the screw may bottom, whether breakthrough is prohibited, base material, and assembly load.
Do not choose thread depth only from a generic "one diameter" or "two diameters" rule. Required engagement depends on the fastener, internal material strength, loading and the governing design standard.
The drawing or model-based definition should state the functional thread requirement clearly.
Thread depth is not drilled depth
For a blind tapped hole, the drilled cavity normally extends beyond the usable full thread.
The extra depth may need to accommodate the drill-point shape, incomplete threads at the tap lead, chip space, machine or tool overtravel, and the selected tapping or thread-milling strategy.
Renovo CNC's tapping guidance explains the underlying reason: the drilled hole needs additional depth because the tap does not produce full thread form at its leading end. It gives a shop-oriented rule of thumb based on several thread pitches. See Renovo's tapping specification guide. Treat that allowance as manufacturing guidance, not a universal drawing standard.
Model the risk near a thin wall
Blind holes become dangerous when the remaining material below the hole is small.
Suppose a plate is 16 mm thick and the design calls for 12 mm of full thread from the top surface. The process may require a pilot hole deeper than 12 mm. If the designer assumed "4 mm of wall remains," the real drilled point could approach or break through the back face.
Review full-thread depth, pilot depth, drill-point allowance, remaining wall and any opposite-side pocket or channel.
If breakthrough is prohibited, make that requirement explicit instead of hoping the shop infers it from the shaded CAD model.
A flat-bottom CAD hole may not imply a flat-bottom drilling process
CAD systems often model blind holes with a simple flat cylinder. Real drilling commonly leaves a shaped bottom unless another operation creates a flat floor.
If the bottom shape is functionally important, for example for sealing or clearance to another feature, state the requirement. If it is not important, do not force an expensive flat-bottom operation just because the modeling feature happened to show one.
CADProps currently recognizes only bounded cases of simple cylindrical through holes and flat-bottom blind holes. That geometric classification is not a tapping plan and does not establish a thread standard.
Do not infer a thread from the pilot diameter
A cylindrical hole of a certain diameter may be compatible with multiple thread preparations, fits or entirely non-threaded functions.
The threads missing from STEP guide explains why a STEP model can contain useful hole geometry without carrying the complete thread callout.
For quotation, pair the STEP with the controlling drawing or verified PMI when the thread specification is not machine-readable in the receiving workflow.
A useful manufacturing definition
A released definition may need the thread designation, class or fit, minimum full-thread depth, through or blind condition, a no-breakthrough requirement where relevant, positional tolerance, and any functional surface requirement.
The exact syntax depends on ASME, ISO or a company drawing standard. Do not copy a web example into a released drawing without checking the governing standard.
Check deep threads separately from deep drilled holes
A hole can be physically deep without needing full thread to the bottom.
Excessive thread depth can increase cycle time and tool risk without improving the joint after the required engagement has already been achieved. Conversely, a deeper pilot hole can provide process clearance while the full-thread requirement remains modest.
If the drilled depth becomes large relative to diameter, calculate L/D and review the deep-hole drilling guide.
Before sending a CNC RFQ
For each blind threaded hole:
- Confirm the nominal thread requirement.
- Identify the minimum usable full-thread depth.
- Check the modeled or drilled cavity depth.
- Check remaining wall and nearby features.
- Decide whether breakthrough is allowed.
- Verify the drawing or PMI carries the thread callout.
- Do not ask the shop to infer thread size from STEP geometry.
- Let the supplier choose the tapping or thread-milling process unless process is a controlled requirement.
Use the STEP viewer and dimension tool for geometric checks, not as certification of thread strength or manufacturability.
The key distinction is simple: design the joint around usable thread engagement, and give the manufacturing process enough physical space to create it.
Original article: CADProps · https://www.cadprops.com/guides/blind-tapped-hole-depth/