Blind tapped hole thread depth vs drill depth is a distinction worth making before you release a CNC drawing. The full-form thread length determines how much complete internal thread is available for engagement. The drilled cavity must also accommodate the selected threading process and the shape of the bottom. If the drawing shows only one depth, the shop may have to ask whether you mean usable thread, the cylindrical hole, or the deepest point reached by the drill.
The difference matters when a screw must seat without bottoming or when a hole approaches a sealing surface, an internal passage or the back of a thin part. The five checks below show how to dimension a blind tapped hole and what to confirm with the shop before requesting a quote.
1. Blind tapped hole thread depth vs drill depth at a glance
| Term | What it describes | Why it matters |
|---|---|---|
| Minimum full-form thread length | The axial length of complete thread, excluding the entry chamfer and incomplete threads at the bottom. | Establishes the amount of usable internal thread. Actual screw engagement also depends on the fastener and assembly. |
| Full-diameter drill depth | The distance from the specified reference surface to the end of the cylindrical portion of the drilled hole. | Defines the cylindrical space available for the threading tool and screw tip. |
| Depth to the drill point | The distance to the deepest point of the drilled cavity when the drill leaves a cone. | Controls how close the cavity comes to the back face or another feature. |
Call out the geometry that matters. If the bottom must be flat, specify that feature and review the tool access. If the bottom simply needs to stay clear of a passage, a minimum remaining wall or maximum penetration limit can communicate that constraint. Agree which surface establishes the depth reference.
2. Specify the thread requirement and the bottom constraint
A useful blind tapped hole callout includes the thread designation and fit class, the full-form thread length, and the hole location. Mark the drawing as blind where its geometry or notation could be ambiguous. If the drill bottom affects function, add the applicable depth limit or remaining wall separately. Mark any required coating or masking and state the condition in which the thread is to be inspected.
ASME Y14.6 covers thread representation on engineering drawings. For metric M threads, ISO 965-1 describes the tolerance system. Use the convention and edition referenced by your drawing or purchase order. The following note illustrates the information to communicate in plain English.
Example drawing note for one blind hole
M6 × 1–6H. Provide 8.0 mm minimum continuous full-form thread, excluding the entry chamfer and incomplete bottom threads. Measure the full-diameter drilled depth from the top face and keep it within 12.0 ±0.2 mm. Maintain 2.0 mm minimum wall to the back face, including at the deepest point of the cavity.
This example includes a cylindrical drill depth because the designer wants to constrain both the cavity and its usable thread. Where the finished design only needs the minimum thread length and a minimum wall, the supplier can propose a drill depth and tooling route for approval. Provide the 2D drawing and CAD model together so the hole geometry and callout can be reviewed together.
3. Check the remaining wall at worst case
Suppose the drawing describes a 16.0 ±0.1 mm thick plate, with the hole normal to the top and back faces. The cylindrical depth is 12.0 ±0.2 mm. For this illustration, the supplier’s proposed drilling method has a maximum additional point depth of 1.6 mm. Confirm that value from the actual drill and process before using the calculation on a released design.
| Input | Worst-case value |
|---|---|
| Minimum plate thickness | 15.9 mm |
| Maximum full-diameter drill depth | 12.2 mm |
| Maximum additional point depth | 1.6 mm |
| Minimum estimated wall at the tip | 15.9 − 12.2 − 1.6 = 2.1 mm |
The stack leaves 0.1 mm of margin over the drawing requirement. It checks the assumed drilled geometry. The supplier still needs to confirm that its threading tool can produce 8.0 mm of complete thread within that cavity, and that the screw clears the bottom when the parts are assembled. For an angled hole or a nearby internal passage, review the shortest wall in the 3D model and account for hole position and orientation variation.
4. Review tool clearance before locking the drill depth
A tap’s cutting lead forms incomplete threads near the bottom of the hole. The extra space needed depends on the tool chamfer, material, chip behavior and machine process. A shop can assess a suitable blind-hole tap, consider thread milling, or ask whether the drawing can allow a deeper hole. The selected threading process also needs to respect the minimum wall.
Toolmakers provide application guidance for specific tools. For example, Sandvik Coromant’s CoroTap 300 describes spiral flute taps designed to evacuate chips out of blind holes. Ask the shop to confirm the available tool geometry for your thread size and alloy. Easiahome’s thread machining guide explains the differences between several threading processes.
If you cannot satisfy both the usable thread length and the remaining wall, take the conflict back to the design owner. Depending on the assembly, options may include a shorter approved screw, a local change in part thickness, or a different threading process. Verify joint strength and sealing requirements before revising the drawing.
5. Agree how to verify thread fit and depth
Agree on the required gauge, acceptance rule and inspection stage before machining the first article. ISO 1502 covers gauges and gauging for ISO general-purpose metric screw threads. Confirm that the selected method separately verifies the required usable thread length where that length is critical. A basic fit check at the entrance cannot establish how far complete threads extend.
If the part will be anodized or plated, specify whether the thread must meet its requirement after finishing and identify where masking is permitted. If remaining wall is critical, agree how the shop will verify the depth or document the process on the first article. The evidence should match the drawing revision, feature and sample. See Easiahome’s guide to reviewing CNC inspection reports for related acceptance checks.
Frequently asked questions
How much deeper should the drill be than the thread?
Set the depth with the shop after reviewing the tooling, thread pitch, material and the required complete thread length. A tap chamfer and the drill point occupy different parts of the cavity. Allow for both where applicable and check the deepest point against the minimum wall.
Can I put only the minimum full-form thread length on the drawing?
When the cavity bottom is unconstrained, the shop may be able to choose the drill depth. Add a limit if the drill could break through, approach another hole or compromise a functional surface. Specify the depth reference when the entry surface or chamfer makes the measurement ambiguous.
Does 8 mm of full-form thread mean my screw engages all 8 mm?
Actual engagement also depends on the screw length, grip stack, entry chamfer and screw-tip geometry. Check assembly at the tolerance limits to confirm the screw seats without bottoming and has the engagement needed for the design.
Send your blind-hole drawing for a CNC quote
Include the STEP model, 2D drawing, material grade, quantity and finish. Flag the holes with critical thread length, tight bottom clearance or masking requirements. Ask the supplier to confirm the proposed tooling route and how it will verify full thread depth and any critical remaining wall. Send your CNC drawings to Easiahome for a review.
