Tap Drill Size Calculator for Metric, UNC & UNF Threads
Calculate tap drill sizes for cutting or forming taps, check theoretical thread percentage, and estimate full-diameter and drill-tip depths for blind threaded holes. Free, with no sign-in required.
Input Parameters
Select a thread standard, then enter the hole requirements. Advanced settings are optional.
Advanced Settings: Tool Lead & Depth
Initializing calculator. Open the published page if controls do not respond in the editor preview.
Calculation Results
Cutting tap · Aluminum alloy · Blind hole
Blind Hole Depth Breakdown
Schematic distance components, from the hole entrance toward the drill point.
Nearby Standard Drill Sizes
| Drill | Diameter | Theoretical thread % |
|---|
How to Use the Tap Drill Size Calculator
- Choose ISO Metric, UNC, or UNF, then select the nominal thread size and pitch.
- Select cutting or forming. For cutting taps, adjust the theoretical thread percentage; for forming taps, confirm the manufacturer’s pilot-hole recommendation.
- Choose blind or through hole, then enter the required full-profile thread length. For blind holes, confirm the actual tap lead and bottom clearance under Advanced Settings.
- Compare the theoretical diameter with the nearest standard drill. Copy the results or print a calculation sheet.
Metric, UNC and UNF Tap Drill Sizes
The approximate ISO metric cutting-tap guideline is major diameter minus pitch. For example, M6 × 1 commonly uses a 5.0 mm drill and M10 × 1.5 commonly uses an 8.5 mm drill. For 1/4-20 UNC, a common cutting-tap drill is #7 (0.201 in). Actual hole diameter and finished thread class require inspection.
Metric fine threads, Unified Coarse (UNC), and Unified Fine (UNF) have different pitch tables. This calculator keeps the nominal thread data separate from the practical drill-size catalogue, so a theoretical diameter and a stocked drill can differ.
Cutting Taps vs Forming Taps
Cutting taps remove material. Forming taps displace material and generally require a larger pilot hole. Never reuse a cutting-tap drill for a forming tap without checking the tool’s specified pilot-hole range. Material ductility, lubrication, tap geometry, and target thread class are important.
The forming-mode output here is a screening estimate based on an editable pilot-hole factor. It is not a tool-manufacturer-approved size, and the cutting-tap percentage formula is deliberately disabled in forming mode.
How to Calculate Blind Hole Thread Depth
Distinguish three dimensions: required full-profile thread length, full-diameter drilled depth, and depth to the drill point. A tap’s chamfer cannot form complete threads along its full lead length. Blind holes also need clearance for tool geometry, chips when applicable, and machine movement.
The planning relationship is: full-diameter depth = required full thread length + tap lead pitches × pitch + bottom clearance pitches × pitch + any extra allowance. For a conventional conical drill point, point length = drill diameter / [2 × tan(point angle / 2)]. The total depth to the tip is the sum of the full-diameter depth and point length.
Worked Examples
| Thread | Tap | Common Drill | Important Check |
|---|---|---|---|
| M6 × 1 | Cutting | 5.0 mm | Confirm 6H finished thread |
| M10 × 1.5 | Cutting | 8.5 mm | Confirm drill tolerance and tool |
| 1/4-20 UNC | Cutting | #7, 0.201 in | Confirm finished 2B thread |
| M6 × 1 | Forming | Tool-specific | Manufacturer pilot-hole range required |
Calculation Methods and Standards
The cutting-tap percentage display uses a traditional 60° thread-height convention: theoretical drill diameter = major diameter − 1.299 × pitch × (target percentage / 100). This percentage is an estimate of radial thread height, not the axial length of fastener engagement, actual strength, or evidence of thread-class acceptance. Different published percentage conventions can yield different numbers.
Reference standards include ISO 261, ISO 262, ISO 724, ISO 965-1 and ISO 965-2 for metric threads, ISO 2306 for preliminary tapping drills, and ASME B1.1 for Unified inch threads. Tool lead and forming-hole dimensions should be verified against the tap maker’s current technical catalogue.
For detailed thread dimensions, inspection notes, and engineering drawing callouts, see the metric thread chart guide. For manufacturing support, review our CNC machining services overview.
Common Questions
What is the tap drill size for M6 × 1?
A commonly used cutting-tap drill is 5.0 mm. The finished thread’s minor diameter and tolerance class still require verification.
What drill should I use for 1/4-20 UNC?
A #7 drill (0.201 in) is a common cutting-tap starting choice. Verify the required finished thread class and tap manufacturer’s recommendation.
Does a 75% thread mean 75% of the bolt is engaged?
No. The percentage in this tool is a traditional radial thread-height estimate. Axial screw engagement length is a separate dimension.
Can a forming tap use the same drill as a cutting tap?
Generally no. Forming taps displace material and need a larger pilot hole selected for the actual tool, material, and thread tolerance.
Does the blind-hole depth include the drill point?
Yes, the result separates full-diameter depth from the additional conical drill-point length. Confirm your CNC programming reference and tool geometry.
Can I use the result directly for a 6H or 2B acceptance decision?
No. A pilot-hole calculation alone cannot establish finished thread conformance. Check the applicable dimensional limits and use the required thread inspection procedure.
Ready to Quote Your CNC Prototype?
Upload your STEP file and get a DFM review + quote within 12 hours.
No tooling cost. Minimum 1 part.
