How Deep to Drill a Blind Hole for Tapping
Work out tap drill depth for blind holes: thread depth plus tap chamfer plus clearance. Plug vs. bottoming taps, drill point length and chip control.
- blind holes
- drill depth
- bottoming tap
- plug tap
- spiral flute tap
- chip evacuation
Quick answer: For a blind hole, drill to full thread depth + tap chamfer length + clearance. The chamfer is the tapered lead on the tap’s tip, which can’t cut a full thread. OSG lists hand plug taps at about 5 threads of chamfer, spiral flute taps at 2.5, and bottoming taps at 1.5. Add at least one more pitch for clearance, plus extra for chips and machine over-travel. For a 1/4-20 with 3/8 in of full thread and a two-thread bottoming chamfer, the minimum full-diameter drill depth is 0.525 in.
Why blind holes need extra depth
A tap doesn’t cut full threads along its whole length. The first few threads at the tip are ground down into a taper called the chamfer (or lead). That’s where all the cutting happens. OSG says the chamfer, usually the first 2–5 pitches, does the entire cutting job, and the full threads behind it just guide the tap.
So the bottom part of any tapped hole has incomplete threads. If your part needs 3/8 in of usable thread, the drilled hole has to go deeper by at least the length of that chamfer.
On top of that you need room for:
- Clearance, so the tap tip never touches the bottom.
- Chips, which collect at the bottom with some tap styles.
- Over-travel, if a machine spindle coasts before it reverses.
- The drill point, which is cone-shaped, not flat.
Step 1: Know your tap’s chamfer
Chamfer length is counted in threads (pitches). OSG publishes these standard lengths:
| Tap type | Chamfer length |
|---|---|
| Hand tap, taper | 9 threads |
| Hand tap, plug | 5 threads |
| Hand tap, bottoming | 1.5 threads |
| Spiral point tap | 5 threads |
| Spiral flute tap | 2.5 threads |
Other makers vary. MSC describes plug chamfers as 3–5 threads, bottoming as 1–2, and modified bottoming as 2–2.5. If you’re cutting it close, measure your actual tap.
To convert to length, multiply by the pitch:
- Inch: pitch = 1 ÷ TPI. A 1/4-20 has a pitch of 0.050 in.
- Metric: pitch is in the size. An M8 x 1.25 has a pitch of 1.25 mm.
So a 5-thread plug chamfer on a 1/4-20 is 0.250 in long, and a 1.5-thread bottoming chamfer is 0.075 in.
Step 2: Add clearance
Cutting Tool Supply’s basic rule is to drill at least one pitch beyond the tap’s chamfer. Tapmatic gives a similar rule: one thread length plus 1 mm beyond the lead.
Then check three more things, again from Cutting Tool Supply:
- Machine over-travel. Newer CNC machines can stop and reverse within half a turn, so one pitch is often enough. Older machines may coast one to three pitches. Add at least one pitch beyond that.
- Chips. Spiral flute taps pull chips out. With straight flute hand taps, chips can get flushed to the bottom, and the tap tip can hit them. In that case, Cutting Tool Supply recommends one tap diameter of extra depth.
- External centers. Plug and taper taps through 3/8 in diameter often have a pointed center on the tip left from manufacturing. Allow about half the tap diameter for it.
Step 3: Account for the drill point
Depth on a drawing is usually measured to where the drill is still full diameter. A standard 118° drill point extends beyond that by about 0.3 × drill diameter (simple geometry: half the diameter divided by tan 59°).
- #7 drill (0.201 in): point adds about 0.060 in.
- 6.8 mm drill: point adds about 2.0 mm.
If you set your drill stop to the tip, add this on top. If the hole is close to breaking through the far side of the part, this is the number that decides whether it does.
Worked examples
1/4-20, needing 0.375 in of full thread
Tap drill: #7 (0.201 in). Pitch: 0.050 in.
| Tap | Chamfer | + 1 pitch | Min. depth (full dia.) | To drill tip |
|---|---|---|---|---|
| Bottoming (1.5 threads) | 0.075 | 0.050 | 0.500 in | ≈0.560 in |
| Bottoming (2 threads) | 0.100 | 0.050 | 0.525 in | ≈0.585 in |
| Spiral flute (2.5 threads) | 0.125 | 0.050 | 0.550 in | ≈0.610 in |
| Plug (5 threads) | 0.250 | 0.050 | 0.675 in | ≈0.735 in |
Those are minimums. For a straight flute plug tap with an external center and chips falling to the bottom, the extra allowances above push the depth well past 0.8 in. If that’s deeper than the part allows, switch tap styles instead of shortening the hole.
M8 x 1.25, needing 12 mm of full thread
Tap drill: 6.8 mm. Pitch: 1.25 mm.
| Tap | Chamfer | + 1 pitch | Min. depth (full dia.) | To drill tip |
|---|---|---|---|---|
| Bottoming (1.5 threads) | 1.9 mm | 1.25 mm | ≈15.1 mm | ≈17.2 mm |
| Spiral flute (2.5 threads) | 3.1 mm | 1.25 mm | ≈16.4 mm | ≈18.4 mm |
| Plug (5 threads) | 6.25 mm | 1.25 mm | 19.5 mm | ≈21.5 mm |
Plug vs. bottoming taps
A plug tap has a longer chamfer, so each tooth takes a lighter cut. That means lower torque and longer life. The cost is more incomplete thread at the bottom, so the hole has to be deeper.
A bottoming tap has a very short chamfer and gets full threads close to the bottom. Tapmatic warns that cutting the lead down to as little as 1.5 threads greatly increases torque and reduces tap life, and that you still need to drill deep enough for clearance.
When tapping by hand, a common approach is to start with a taper or plug tap, which starts straight more easily, then finish with a bottoming tap only if you need threads near the bottom. On a machine with a rigid setup, a bottoming or spiral flute tap can usually go straight in.
If you have the depth, use the longer chamfer. OSG recommends a longer chamfer even in blind holes when the hole is deep enough.
Chip evacuation
Most broken taps in blind holes come down to chips. OSG’s troubleshooting guide lists chip packing and hitting the bottom of the hole among the main causes of tap breakage.
Match the tap to the job:
| Tap style | Chips go… | In blind holes |
|---|---|---|
| Spiral flute | Up and out of the hole | Best cutting-tap choice |
| Straight flute (hand tap) | Stay in the flutes | OK if you back out often |
| Spiral point (gun) | Pushed ahead, toward the bottom | Avoid |
| Form tap | No chips at all | Excellent in ductile metals |
Spiral flute taps
Spiral flute taps pull chips up the flutes like a drill. Tapmatic recommends:
- About 15° helix for blind holes less than 1.5 diameters deep in materials that make short chips.
- A high 40–50° helix for long-chipping materials such as aluminum and stainless steel, in holes up to about 3 diameters deep.
See tapping aluminum and tapping stainless steel for material-specific advice.
Form taps
Thread forming taps make no chips, which removes the biggest blind-hole risk. They need a larger drill, though; see the form tap drill chart and cut vs. form tapping. Form taps also have a chamfer, so you still need depth beyond the full thread.
Hand tapping tips
- Back the tap out regularly to break and clear chips, especially with straight flute taps.
- Blow or flush chips out of the hole before switching to a bottoming tap. Wear eye protection.
- Mark the tap or use a depth stop so you know when you’re near the bottom.
- Stop at the first sign of a hard stop. It’s either chips or the bottom of the hole. Forcing it is how taps break. If it’s too late, see broken tap removal.
Lower thread percentage helps too
Tapmatic notes that blind holes often call for a slightly larger tap drill to reduce loads from chip buildup, and that holes deeper than 1.5 diameters often need one as well. Tapmatic’s deep-hole ranges are 55–65% thread in tough materials and 60–70% in free-cutting ones. See percent of thread for how to pick the drill.
Summary
- Start with the full thread depth you need.
- Add the tap’s chamfer: threads × pitch.
- Add at least one pitch of clearance, plus extra for over-travel, chips, or an external center.
- Remember the drill point adds about 0.3 × drill diameter past the full-diameter depth.
- Use a spiral flute or form tap, and clear chips often.
Find the drill for your thread on the UNC tap drill chart or metric tap drill chart.
Sources: OSG Tap Technical Guide Vol. 1 (section 2.2, Fig. 4 chamfer table, Table 8, Part 12); Cutting Tool Supply, “Determining the Minimum Tap Drill Depth”; Tapmatic, “Tap Recommendations for Specific Materials,” “Drill Size Factors,” and “Tapping Torque vs. Thread Strength”; MSC Industrial Supply, “Types of Taps.”