Get A Quote

Why "Full Thread" Holes Are Never 100% Full Depth

Created on 07.07

If you work with CNC machined parts, you have almost certainly seen “full thread to bottom” written on a drawing for a blind tapped hole. It sounds like a straightforward requirement — but in real-world machining, it is physically impossible to achieve with standard tooling.

This is one of the most common mismatches between design intent and shop-floor reality, and it regularly causes confusion during quote review and first-article inspection. Understanding why full threads cannot reach the very bottom of a hole helps you write clearer drawings, avoid assembly surprises, and cut down on back-and-forth with your manufacturing partner.

Why Every Tap Leaves Incomplete Threads at the Bottom

Every cutting tap has a tapered lead section (chamfer) at its tip. The first few teeth are ground to a smaller diameter, so the tool can enter the hole smoothly, align itself straight, and gradually cut the full thread profile.

These lead teeth do not produce full-height, load-bearing threads. Only the fully formed teeth further up the tap body cut a complete, standard thread form. This is not a quality flaw or a shop limitation — it is fundamental to how taps are designed. Without the chamfer, a tap would not start straight, would bind immediately, and would break almost instantly.

Standard tap chamfer lengths (industry baseline)

Three tap styles are most common in CNC production, each with a different number of incomplete lead threads:

• Plug tap (default): 3–5 incomplete lead threads. The universal standard for most production tapping, balances tool life and speed.

• Bottoming tap: 1–2 incomplete lead threads. Used to maximize thread depth in blind holes, but cannot start a thread on its own.

• Taper tap: 7–10 incomplete lead threads. Used for hand tapping or tough materials, with the gentlest cutting action.

For context: on an M6×1 thread, a standard plug tap leaves 3–5 mm of partial thread at the hole bottom. Even a bottoming tap still leaves 1–2 mm of incomplete thread. No off-the-shelf tap produces full thread all the way to the flat bottom.

How to Calculate the Right Drill Depth for Your Required Threads

A properly specified blind tapped hole has two separate, clearly labeled depths: drill depth and minimum full thread depth. They are never the same number.

Standard industry formula

Total drill depth = required full thread depth + tap chamfer length + chip clearance margin

The extra depth below the last full thread serves three non-negotiable purposes:

1. It accommodates the tap’s chamfered lead section

2. It provides space for metal chips to collect, preventing pack-up and tap breakage

3. It adds a small safety margin for spindle over-travel at the bottom of the machining cycle

As a quick rule of thumb: drill the hole at least 3–5 times the thread pitch deeper than your specified full thread length. Harder materials like stainless steel require more clearance; softer aluminum can use the lower end of the range.

Practical example: M8×1.25 thread, 12 mm full thread required

• Tap chamfer (standard plug tap): ~4 threads = 5 mm

• Chip and safety margin: ~2 mm

• Minimum total drill depth = 12 + 5 + 2 = 19 mm

Specifying 12 mm of full thread in a 12 mm deep hole is one of the most frequent drawing errors. It will always result in shorter usable threads than expected.

How Much Thread Engagement Do You Actually Need?

Many designers over-specify thread depth under the assumption that more depth always equals more strength. In practice, strength gains drop off very quickly beyond a standard threshold.

The widely accepted engineering guideline is:

• Steel / stainless steel assemblies: 1.0× nominal diameter of full thread engagement is sufficient for most loads.

• Aluminum / soft alloy assemblies: 1.5× nominal diameter is the recommended upper limit for high-load joints.

For an M8 screw, this means 8–12 mm of full thread is enough for nearly all applications. Any depth beyond 1.5× the diameter adds negligible pull-out strength, but noticeably increases machining time, tap breakage risk, and cost.

4 Best Practices for Clear, Production-Ready Tapped Hole Drawings

1. Call out full thread depth and drill depth separately

Never write “full thread to bottom.” Instead, specify minimum full thread length and total drill depth as two independent dimensions. This removes all ambiguity and gives the machinist clear, verifiable requirements.

2. Specify bottoming tap only when you truly need maximum depth

If threads must extend as close to the bottom as possible, note that a bottoming tap is required. Keep in mind that bottoming taps cannot start a thread — the hole must first be tapped with a standard plug tap, which adds an operation and slightly increases cost.

3. Add an undercut relief for critical flush-seat applications

If a screw must seat fully against the hole bottom, add a small undercut (thread relief groove) below the threaded section. This guarantees a fully formed final thread and gives the tap tip clearance. This is standard practice for high-reliability assemblies.

4. Catch depth mismatches early with DFM review

Small drawing errors like mismatched thread and drill depths are easy to miss in internal design reviews. At Marigold Rapid, our free DFM check flags these issues automatically before production begins, so you can adjust your drawing before any material is cut.

Frequently Asked Questions

Can you tap a hole all the way to the bottom?

No, not with standard cutting taps. Every tap has a tapered lead section that produces incomplete threads. The closest practical result is 1–2 pitches from the bottom, achieved by following a standard plug tap with a bottoming tap.

What is the minimum drill depth for a blind tapped hole?

As a general rule, drill the hole 3–5 times the thread pitch deeper than your required full thread length. This covers the tap chamfer, chip space, and spindle travel margin. Harder materials need more clearance.

Does thread milling produce full thread to the bottom?

Thread milling can get slightly closer to the hole bottom than tapping, because the cutter has no long chamfered lead. It still cannot reach exactly to a flat bottom, and it is typically slower and more costly than tapping for standard-size threads.

How many threads of engagement do I need?

For most steel and stainless steel joints, 1× the screw diameter of full engagement is sufficient. For aluminum or high-load parts, 1.5× diameter is recommended. Beyond that, additional depth adds almost no strength.

Why do my parts have fewer full threads than the drawing shows?

This almost always happens when the drawing sets full thread depth equal to total drill depth. The machinist must leave room for the tap chamfer, so usable full thread ends up shorter than expected. The fix is to specify drill depth and thread depth as two separate values.

Final Takeaway

“Full thread to bottom” is a common drawing note, but it conflicts with the basic design of all standard tapping tools. Every tap leaves a short section of incomplete thread at the bottom of a blind hole — this is a tooling reality, not a quality defect.

The most reliable way to get consistent, predictable results is to follow standard depth clearance rules and call out full thread depth and drill depth separately on your drawing. This eliminates miscommunication, reduces scrap, and ensures your parts assemble correctly on the first try.

At Marigold Rapid, every quote includes a free DFM review that checks tapped hole depths, thread feasibility, and dozens of other common design issues. We flag potential problems early, suggest practical adjustments, and help you produce parts that meet your functional requirements without unnecessary cost.

To submit your next drawing for a free DFM review and transparent quote, visit our custom CNC machining service page:https://www.marigold-rapid.com.cn/CNC_Machining.html