Thread Tap Drill Chart for Metric, UNC, and UNF Threads

Q: Can I always calculate a metric tap drill as diameter minus pitch?

No. D - P is a fast approximation for common 60-degree cutting-tap threads. It does not replace the tool manufacturer’s recommendation, especially for forming taps, controlled thread percentages, special tolerance positions, difficult materials, or holes that will be gauged after finishing.

Thread Tap Drill Chart: Metric Coarse Threads

The metric thread designation controls: M is the nominal major diameter in millimeters, and the value after x is pitch P in millimeters. The listed drill is a common nominal size for cutting taps.

Metric Thread	Pitch P (mm)	Common Cutting-Tap Drill (mm)	Quick Check: D - P (mm)
M2 x 0.4	0.40	1.60	1.60
M2.5 x 0.45	0.45	2.05	2.05
M3 x 0.5	0.50	2.50	2.50
M3.5 x 0.6	0.60	2.90	2.90
M4 x 0.7	0.70	3.30	3.30
M5 x 0.8	0.80	4.20	4.20
M6 x 1.0	1.00	5.00	5.00
M8 x 1.25	1.25	6.80	6.75
M10 x 1.5	1.50	8.50	8.50
M12 x 1.75	1.75	10.20	10.25
M14 x 2.0	2.00	12.00	12.00
M16 x 2.0	2.00	14.00	14.00
M18 x 2.5	2.50	15.50	15.50
M20 x 2.5	2.50	17.50	17.50

The D - P column is an arithmetic check, not a tolerance specification. Where the result is not a preferred drill diameter, the chart selects a nearby common drill. Guhring’s calculator returns 5.026 mm for an M6 x 1.0 cutting tap at 75% thread, for example; 5.00 mm is the common nominal chart choice. A designer who needs a controlled internal minor diameter should specify the thread and acceptance criteria rather than dimensioning only the pre-hole.

Metric Fine Thread Tap Drill Chart

Fine-pitch threads can leave more wall thickness around a hole and may suit limited engagement length, but they are not automatically stronger or easier to manufacture. Confirm that the mating fastener and tap use the same pitch.

Metric Thread	Pitch P (mm)	Common Cutting-Tap Drill (mm)	Quick Check: D - P (mm)
M3 x 0.35	0.35	2.65	2.65
M4 x 0.5	0.50	3.50	3.50
M5 x 0.5	0.50	4.50	4.50
M6 x 0.75	0.75	5.25	5.25
M8 x 1.0	1.00	7.00	7.00
M10 x 1.25	1.25	8.75	8.75
M12 x 1.5	1.50	10.50	10.50
M14 x 1.5	1.50	12.50	12.50
M16 x 1.5	1.50	14.50	14.50
M18 x 1.5	1.50	16.50	16.50
M20 x 1.5	1.50	18.50	18.50

These fine-pitch rows are an early DFM reference. The thread designation, class or tolerance position, and gauge requirement remain the controlling product definition.

UNC and UNF Thread Tap Drill Chart

For Unified inch threads, the number after the dash is threads per inch (TPI). The inch drill designation and decimal-inch diameter control in this table. Metric equivalents are rounded to the nearest 0.01 mm for tool-room comparison only; do not use the rounded metric value to impose a tighter hole tolerance.

Thread	Series	Common Drill	Drill Diameter (in)	Metric Equivalent (mm)
#2-56	UNC	#50	0.0700	1.78
#2-64	UNF	#50	0.0700	1.78
#4-40	UNC	#43	0.0890	2.26
#4-48	UNF	#42	0.0935	2.37
#6-32	UNC	#36	0.1065	2.71
#6-40	UNF	#33	0.1130	2.87
#8-32	UNC	#29	0.1360	3.45
#8-32	UNC	#29	0.1360	3.45
#8-36	UNF	#29	0.1360	3.45
#10-24	UNC	#25	0.1495	3.80
#10-32	UNF	#21	0.1590	4.04
1/4-20	UNC	#7	0.2010	5.11
1/4-28	UNF	#3	0.2130	5.41
5/16-18	UNC	F	0.2570	6.53
5/16-24	UNF	I	0.2720	6.91
3/8-16	UNC	5/16 in	0.3125	7.94
3/8-24	UNF	Q	0.3320	8.43
7/16-14	UNC	U	0.3680	9.35
7/16-20	UNF	25/64 in	0.3906	9.92
1/2-13	UNC	27/64 in	0.4219	10.72
1/2-20	UNF	29/64 in	0.4531	11.51
9/16-12	UNC	31/64 in	0.4844	12.30
9/16-18	UNF	33/64 in	0.5156	13.10
5/8-11	UNC	17/32 in	0.5313	13.49
5/8-18	UNF	37/64 in	0.5781	14.68
3/4-10	UNC	21/32 in	0.6563	16.67
3/4-16	UNF	11/16 in	0.6875	17.46
7/8-9	UNC	49/64 in	0.7656	19.45
7/8-14	UNF	13/16 in	0.8125	20.64
1-8	UNC	7/8 in	0.8750	22.23
1-12	UNF	59/64 in	0.9219	23.42

ASME B1.1 defines the Unified thread form, series, class, allowance, tolerance, and designation. It does not turn one tap-drill value into a universal manufacturing requirement. The common drills above should therefore be checked against the tap supplier’s calculator or catalog when tool life, thread class, difficult material, or a gauged production process matters.

How to Estimate a Cutting-Tap Drill Size

Two shop-floor formulas provide a quick reasonableness check for 60-degree cutting-tap threads:

Metric approximation

D_d ~= D - P

Unified inch approximation

D_d ~= D - (1 / N)

Where:

D_d = estimated pre-hole diameter;
D = nominal thread major diameter;
P = metric pitch in millimeters;
N = threads per inch for a Unified thread.

These approximations land near the drill sizes commonly associated with roughly 75% thread, but they do not calculate every thread class, allowance, drill tolerance, material response, or tap manufacturer’s recommendation. For M5 x 0.8, 5.0 - 0.8 = 4.2 mm; Guhring’s 75% cutting-tap calculator gives 4.221 mm. For 1/4-20 UNC, 0.250 - 1/20 = 0.200 in, close to a #7 drill at 0.2010 in.

Why Cutting Taps and Forming Taps Need Different Holes

A cutting tap removes material to create the thread profile. A forming or fluteless tap displaces ductile material into the profile, so it starts from a larger hole and is more sensitive to the selected tap limit, material flow, lubrication, and actual pre-hole size.

The difference is visible even for the same nominal thread:

M5 x 0.8 Example	Guhring Calculator Setting	Calculated Pre-Hole (mm)
Cutting tap	75% thread	4.221
Forming tap	75% thread	4.592

The calculator outputs are shown to 0.001 mm because that is how the source reports them; they are not a ShincoFab process tolerance. YG-1 also publishes separate fluteless-tap drill tables by tap limit, reinforcing that a cutting-tap chart should not be reused for forming taps. Confirm form-tap holes directly from the exact tool supplier and material application data.

How to Use This Chart for Sheet Metal Parts

Identify the exact thread callout. Confirm metric versus Unified, coarse versus fine, right- or left-hand thread, and the specified class or tolerance position.
Choose the thread-making method. Select cutting tap, forming tap, thread mill, extruded-and-tapped hole, weld nut, rivet nut, or self-clinching hardware before freezing the pre-hole.
Check usable engagement. In flat sheet, usable full-thread length is constrained by the material thickness and tap lead. If the available engagement does not support the joint requirement, change the joint rather than forcing a smaller hole.
Define how the hole is made. A laser-cut, punched, drilled, or reamed pre-hole can differ in taper, burr condition, roundness, and size control. The final pre-hole presented to the tap is what matters.
Account for bends and edges. Verify that the tap body, holder, and inspection gauge can reach the hole and that nearby edges or bend zones will not distort the feature.
Set the finish sequence. State whether threads are cut before or after plating, anodizing, paint, or powder coating, and whether masking or post-finish thread restoration is allowed.
Plan inspection. Specify the thread gauge, class, inspection stage, sampling plan, and any functional fastener test needed for the application.

When a tapped hole interfaces with other formed or cut features, use a consistent datum scheme and inspection condition. ShincoFab’s sheet metal tolerance chart explains why a general tolerance should not replace a feature-specific callout for a critical assembly interface.

Design Checks Before Releasing a Drawing

Call out the complete thread designation, including pitch or TPI and thread class where required.
State whether the thread is produced with a cutting tap, forming tap, or another process when that choice is design-critical.
Verify sheet thickness, available full-thread length, joint load, fastener material, and service environment together.
Dimension the hole from functional datums and check clearance to edges, bends, welds, and adjacent hardware.
Define the finished condition for gauging: before coating, after coating, after assembly, or another explicit stage.
Keep burr direction and access side compatible with tapping, deburring, hardware insertion, and inspection.
Confirm that the selected drill is available and that its actual tolerance supports the intended internal minor diameter.
Review whether a replaceable fastener is preferable to a tapped sheet feature for service or repeated assembly.

Common Tap Drill Problems and Corrective Options

Symptom or Constraint	Corrective Option	Trade-Off or Check
Tap torque is high or taps chip early	Evaluate a slightly larger pre-hole or lower thread percentage using the tap supplier's data	Confirm thread strength, minor diameter, and gauge acceptance before release
Thread strips in thin sheet	Add an extrusion, increase local thickness, or use inserted hardware	Changes tooling, access, appearance, and sometimes finish sequence
Form tap is specified with a cutting-tap hole	Replace the hole with the exact form-tap recommendation	Material ductility, tap limit, lubrication, and hole tolerance become critical
Coating fills or tightens the thread	Mask the thread, tap after finish, or define an approved restoration step	Each option changes corrosion protection, cosmetics, handling, or inspection
Hole is too close to a bend or edge	Move the hole, change the bend sequence, or use separate hardware	Requires a drawing-level check of access, distortion, and joint load path
Tapped joint is difficult to service	Use a rivet nut, weld nut, or self-clinching nut	Adds component cost and installation controls but can provide a replaceable or deeper thread

For thin-sheet alternatives, compare the exact hardware family and panel conditions in the self-clinching fastener hole size chart. Production planning should also account for insertion access, finish order, and inspection through the sheet metal hardware insertion service.

Frequently Asked Questions

Find quick answers to common questions about selecting the right tap drill sizes, calculating pre-holes, differentiating between cutting and forming taps, and best practices for threading sheet metal parts.

What tap drill should I use for M6 x 1.0?

A 5.00 mm drill is the common cutting-tap starting size. The D - P check gives 6.00 - 1.00 = 5.00 mm, while Guhring’s calculator gives 5.026 mm at 75% thread. Confirm the final choice against the tap, material, thread tolerance, and gauging plan.

What is the tap drill size for 1/4-20 UNC?

A #7 drill, 0.2010 in (about 5.11 mm), is the common cutting-tap choice. The quick calculation gives 0.200 in. The #7 drill value is the controlling inch size; the metric value is a rounded reference.

Can I always calculate a metric tap drill as diameter minus pitch?

No. D - P is a fast approximation for common 60-degree cutting-tap threads. It does not replace the tool manufacturer’s recommendation, especially for forming taps, controlled thread percentages, special tolerance positions, difficult materials, or holes that will be gauged after finishing.

Is a form-tap drill the same size as a cutting-tap drill?

No. A form tap displaces material and normally needs a larger pre-hole. For the M5 x 0.8 example above, Guhring’s 75% calculator returns 4.592 mm for forming and 4.221 mm for cutting. Use the exact forming-tap supplier’s chart because material and tap limit affect the recommendation.

Is a tap drill the same as a clearance drill?

No. A tap drill creates the pre-hole that will become an internal thread. A clearance drill creates a hole intended to let the fastener pass through without forming mating threads.

Can a laser-cut or punched hole be tapped directly?

It can be a viable process when the resulting pre-hole size, roundness, taper, burr condition, material condition, and tap access satisfy the drawing and tool requirements. For a critical or tightly gauged thread, the production plan may include drilling, reaming, or another finishing operation before tapping.

How much thread engagement is enough in sheet metal?

There is no single engagement length that fits every joint. Fastener size and material, sheet material and thickness, applied loads, vibration, assembly torque, service cycles, and failure mode all matter. If flat sheet cannot provide adequate engagement, evaluate an extrusion, local reinforcement, weld nut, rivet nut, or self-clinching fastener.

Should sheet metal threads be tapped before or after coating?

Either sequence can be appropriate, but the drawing and process plan should define it. Tapping before finish may require masking or controlled restoration; tapping after finish can expose base material or damage a cosmetic surface. Inspect the thread in the condition in which it must function.

Need Help Reviewing a Tapped Sheet Metal Part?

ShincoFab’s engineering team can review the CAD and drawing, thread designation, tap type, sheet material and thickness, quantity, finish sequence, critical datums, gauge requirements, and joint application. Send the part details for a drawing-specific DFM review before locking the tap-drill callout or thin-sheet fastening method.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us