Metric Thread Chart and Tapped Hole Callouts: Sizes, Tap Drills, and Depth Rules

Use this metric thread chart to select an ISO metric thread size, check the selected pitch, plan a cutting tap drill and define an inspectable tapped hole callout. The reference separates basic thread dimensions, manufacturing pilot holes, the usable full-thread length and final 6H thread inspection. A metric tap drill chart is a process reference, while the drawing controls the finished feature.

For an M8 × 1.25-6H blind threaded hole, a designer should state the required full-profile thread depth and the mating fastener requirement. The manufacturer then checks tool lead, bore depth and remaining wall. A drill-bottom dimension is added when the part function or geometry requires it. The GO/NOT GO inspection method is not determined by the drilled-hole diameter alone.

Thread callouts work with the rest of the engineering drawing tolerances on the same drawing; thread acceptance and general dimensional acceptance are separate checks.

1.ISO Metric Thread Standards and Dimensions

An ISO metric thread uses a 60° basic profile. ISO 261:1998 defines the general diameter-and-pitch plan; ISO 262:2023 selects sizes for commercial bolts, screws, studs and nuts; ISO 724:2023 defines metric thread dimensions. ISO 965-1:2026 establishes tolerances and designations, with finished size limits in ISO 965-2:2024 and ISO 965-6:2025. ISO 6410-1:1993 addresses drawing representation, and ISO 1502:1996 addresses gauges and gauging.

Non-thread dimensions can be checked separately with the ISO 2768 general tolerances guide. Do not apply a general linear tolerance to the ISO thread class.

Source	Controls	Does not establish
ISO 261 / ISO 262	Diameter, metric thread sizes, pitch selection and first/second choice	Tap drills, lead time or finished acceptance
ISO 724:2023	Basic D₂, D₁ and external d₃ geometry	6H upper/lower limits or cutting pilot diameter
ISO 965-1:2026	Tolerance classes, S/N/L engagement groups and designation	A universal tapping depth or joint strength
ISO 965-2:2024	6H/6g limits for M1.6–M100	GO/NOT GO operating rules
ISO 965-6:2025	Ten selected internal/external class limits	Pilot drill dimensions or a universal hole-depth rule
ISO 6410-1 / ISO 1502	Drawing conventions / screw and plain gauge checks	Shop pilot-hole selection

The basic pitch diameter is D₂ = d₂ = d − 0.649519P, and the basic internal minor diameter is D₁ = d − 1.082532P. For M8 × 1.25, basic D₂ is 7.188 mm and basic D₁ is 6.647 mm. ISO 724:2023 Clause 5, Table 1 supplies these reference dimensions, not the pre-tap drill size or a finished-part acceptance report.

1.1 Coarse vs Fine Thread and Metric Thread Pitch

A coarse vs fine thread decision starts with the mating fastener and required assembly function. Standard coarse pitches are M6 × 1, M8 × 1.25, M10 × 1.5 and M12 × 1.75. A smaller metric thread pitch reduces axial advance per turn and changes the thread geometry and tap-drill requirement. It does not, by itself, prove improved vibration resistance, fatigue life or stripping strength.

A metric fine thread chart is useful when a reduced advance, limited radial envelope or defined mating fastener makes a fine pitch appropriate. Check the material, minimum wall section, available engagement, bolt loading, tool and gauge availability. ISO 262 designates M8 × 1, M10 × 1.25, M10 × 1 and M12 × 1.5 as selected fine pitches, but says nothing about supplier stock or automatic machining delays.

1.2 Metric Thread Size Chart and Pitch Table

The metric thread size chart below is a selected thread pitch chart covering M1.6–M100. It contains 73 ISO 262:2023 combinations across the displayed nominal diameters. This metric thread pitch chart is a selected-size resource, not every ISO 261 diameter–pitch pairing. For M72–M100, ISO 262 lists 6 mm and 4 mm as fine pitches and no coarse entry.

Nominal × P (mm)	Series	Choice	Cut pilot (mm)	Basic D₁ (mm)
M1.6 × 0.35	Coarse	First	1.25	1.221
M1.8 × 0.35	Coarse	Second	1.45	1.421
M2 × 0.4	Coarse	First	1.6	1.567
M2.5 × 0.45	Coarse	First	2.05	2.013
M3 × 0.5	Coarse	First	2.5	2.459
M3.5 × 0.6	Coarse	Second	2.9	2.850
M4 × 0.7	Coarse	First	3.3	3.242
M5 × 0.8	Coarse	First	4.2	4.134
M6 × 1	Coarse	First	5	4.917
M7 × 1	Coarse	Second	6	5.917
M8 × 1.25	Coarse	First	6.8	6.647
M8 × 1	Fine	First	7 *	6.917
M10 × 1.5	Coarse	First	8.5	8.376
M10 × 1.25	Fine	First	8.8 *	8.647
M10 × 1	Fine	First	9 *	8.917
M12 × 1.75	Coarse	First	10.2	10.106
M12 × 1.5	Fine	First	10.5 *	10.376
M12 × 1.25	Fine	First	10.8 *	10.647
M14 × 2	Coarse	Second	12	11.835
M14 × 1.5	Fine	Second	12.5 *	12.376
M16 × 2	Coarse	First	14	13.835
M16 × 1.5	Fine	First	14.5 *	14.376
M18 × 2.5	Coarse	Second	15.5	15.294
M18 × 2	Fine	Second	16 *	15.835
M18 × 1.5	Fine	Second	16.5 *	16.376
M20 × 2.5	Coarse	First	17.5	17.294
M20 × 2	Fine	First	18 *	17.835
M20 × 1.5	Fine	First	18.5 *	18.376
M22 × 2.5	Coarse	Second	19.5	19.294
M22 × 2	Fine	Second	20 *	19.835
M22 × 1.5	Fine	Second	20.5 *	20.376
M24 × 3	Coarse	First	21	20.752
M24 × 2	Fine	First	22 *	21.835
M27 × 3	Coarse	Second	24	23.752
M27 × 2	Fine	Second	25 *	24.835
M30 × 3.5	Coarse	First	26.5	26.211
M30 × 2	Fine	First	28 *	27.835
M33 × 3.5	Coarse	Second	29.5	29.211
M33 × 2	Fine	Second	31 *	30.835
M36 × 4	Coarse	First	32	31.670
M36 × 3	Fine	First	33 *	32.752
M39 × 4	Coarse	Second	35	34.670
M39 × 3	Fine	Second	36 *	35.752
M42 × 4.5	Coarse	First	37.5	37.129
M42 × 3	Fine	First	39 *	38.752
M45 × 4.5	Coarse	Second	40.5	40.129
M45 × 3	Fine	Second	42 *	41.752
M48 × 5	Coarse	First	43	42.587
M48 × 3	Fine	First	45 *	44.752
M52 × 5	Coarse	Second	47	46.587
M52 × 4	Fine	Second	48 *	47.670
M56 × 5.5	Coarse	First	50.5	50.046
M56 × 4	Fine	First	52 *	51.670
M60 × 5.5	Coarse	Second	54.5	54.046
M60 × 4	Fine	Second	56 *	55.670
M64 × 6	Coarse	First	58	57.505
M64 × 4	Fine	First	60 *	59.670
M68 × 6	Coarse	Second	62	61.505
M68 × 4	Fine	Second	64 *	63.670
M72 × 6	Fine	First	66 *	65.505
M72 × 4	Fine	First	68 *	67.670
M76 × 6	Fine	Second	70 *	69.505
M76 × 4	Fine	Second	72 *	71.670
M80 × 6	Fine	First	74 *	73.505
M80 × 4	Fine	First	76 *	75.670
M85 × 6	Fine	Second	79 *	78.505
M85 × 4	Fine	Second	81 *	80.670
M90 × 6	Fine	First	84 *	83.505
M90 × 4	Fine	First	86 *	85.670
M95 × 6	Fine	Second	89 *	88.505
M95 × 4	Fine	Second	91 *	90.670
M100 × 6	Fine	First	94 *	93.505
M100 × 4	Fine	First	96 *	95.670

Table notes: “Choice” refers to first/second-choice nominal diameters in ISO 262:2023. Basic D₁ is calculated from the ISO 724 profile and shown to 0.001 mm; it is not a drilled-hole recommendation or a finished 6H tolerance table. Unmarked cutting-pilot sizes reproduce the Handbook 32nd edition coarse-thread Table 7 starting recommendations; * identifies a preliminary D − P planning estimate. The asterisked sizes require a manufacturer drill chart, material and tap check before production. No ISO source prescribes these cutting-pilot numbers. The large M72–M100 cutting-pilot values are not represented as handbook table recommendations.

Existing reference download: Download the full chart as PDF.

2.Metric Tap Drill Chart and Tap Drill Size Chart

A tap drill chart is useful after the threading method has been chosen. Cutting-tap entries in a metric drill and tap chart often start with D − P, followed by a drill size available to the shop. A tap drill size chart is a manufacturing aid; it does not supply the finished ISO 965 minor-diameter limits. Hole size also changes with tool wear, runout and material displacement during threading.

2.1 M3 to M12 Tap Drill Sizes

For common coarse cutting taps, the Machinery’s Handbook 32nd edition, Table 7 (printed p. 2174), gives the following practical starting values. The M3 tap drill size is 2.5 mm; M4 tap drill size is 3.3 mm; M5 tap drill size is 4.2 mm; M6 tap drill size is 5.0 mm; M8 tap drill size is 6.8 mm; M10 tap drill size is 8.5 mm; and M12 tap drill size is 10.2 mm. A selected drill is still subject to finished-thread verification.

Cutting thread	Pilot (mm)	Basic D₁ (mm)	Note
M3 × 0.5	2.5	2.459	M3 coarse
M4 × 0.7	3.3	3.242	M4 coarse
M5 × 0.8	4.2	4.134	M5 coarse
M6 × 1	5.0	4.917	M6 coarse
M8 × 1.25	6.8	6.647	M8 coarse
M10 × 1.5	8.5	8.376	M10 coarse
M12 × 1.75	10.2	10.106	M12 coarse

The M6 thread pitch is 1.0 mm, M8 thread pitch is 1.25 mm, M10 thread pitch is 1.5 mm and M12 thread pitch is 1.75 mm for these coarse selections. A percentage of full thread describes geometric tooth-height engagement in a pilot-hole calculation, not the axial thread engagement length or a universal percentage of joint strength.

The Handbook’s metric cutting-tap relation is pilot diameter = D − 1.08253 × P × f, where f is the decimal fraction of theoretical full-thread height. For M8 × 1.25 at f = 0.75, the result is approximately 6.985 mm, not 6.8 mm. Table 7 separately recommends 6.8 mm and reports 78.5% theoretical radial engagement under its tabular convention. Substituting 6.8 mm back into the cited formula yields 88.7%, so these two percentage presentations must not be treated as interchangeable without reconciling their definitions. Neither percentage indicates guaranteed joint strength.

2.2 Cut Tap and Form Tap Drill Selection

In form tapping, ductile workpiece metal is displaced to produce the thread. The forming pilot differs from the cutting pilot. Coating, lubrication, ductility and wall distortion affect the result. The Handbook 32nd edition lists a 6.8 mm cutting pilot for M8 × 1.25 in Table 7 and a 7.4 mm forming pilot in Table 10 (printed p. 2178). A 7.4 mm forming pilot cannot simply be used for an M8 cutting tap.

Tool-manufacturer tables govern the final form-tap diameter. The Handbook’s cold-form formula takes a whole-number percentage, while its cutting-tap relation takes a decimal fraction. Check the numerical input convention before calculating a pilot size. Neither calculation proves final 6H compliance.

3.Tapped Hole Callout on Engineering Drawings

A tapped hole callout identifies a finished threaded feature, not a particular machine program. Where interchangeability matters, specify M × pitch, the correct tolerance class and the required usable thread length. In a threaded hole callout, a process instruction such as “DRILL 6.8 TAP M8” can unnecessarily exclude thread milling or a suitable forming tap. Keep process constraints only when independently required by the design.

3.1 Metric Thread Callout Symbols and Examples

A metric thread callout for a standard coarse internal thread may abbreviate the pitch and default class when the ISO 965-1:2026 Clause 13.2 conditions apply. Nevertheless, writing M8 × 1.25-6H explicitly improves global RFQ interpretation. The thread symbol and depth notation belong to separate functions: the M designation controls the thread, while the drawing depth symbol or text dimension controls the axial limit. This distinction should be visible in the thread callout drawing.

Design intent	Illustrative drawing text	Check
Internal coarse through thread	M8 × 1.25-6H THRU	Thread passes completely through the part
Internal fine blind thread	M10 × 1.25-6H; 12 mm FULL THREAD	Fine pitch and usable full-profile depth explicit
Left-hand internal thread	M8 × 1 with -LH indication	Add the left-hand suffix in the form required by ISO 965-1 Clause 13.4
Coated external matching thread	M8 × 1.25-6g; coating state per drawing	Check before/after coating tolerance condition

The numeric tolerance grade is the width, while the letter is the position of the tolerance zone. For an internal thread above 1.4 mm and pitch other than 0.2 mm, 6H is an ISO 965-1 omission default; external 6g is the corresponding general default. Smaller diameters have defined exceptions. A vendor should not infer a different pitch or a special tolerance from an abbreviated callout.

The mating clearance hole in the other component follows clearance hole fits where a fit is specified; a tap drill is not a substitute for a separate assembly hole requirement.

4.Blind Tapped Hole Depth: Full Threads, Tap Chamfer, and Drill Point

A blind tapped hole contains a drilled termination, a zone of incomplete thread near the bottom and a usable full-profile thread. The stated thread depth must identify the portion that can engage the mating fastener. The hole depth symbol is used when the bottom of the bore must also be constrained because of a minimum floor thickness, adjoining passage, sealing interface, chip clearance or a controlled assembly envelope.

ISO 6410-1:1993 Clause 4.3 allows blind-hole drilled depth to be omitted in ordinary cases while the threaded length is dimensioned. A blanket rule demanding three depth lines on every drawing is therefore incorrect. The machinist must still prove that the selected tool and drill cycle can produce the full-profile length. The design does not become invalid solely because it leaves the manufacturing pilot depth to process planning.

4.1 Bottoming Tap vs Plug Tap for Blind Holes

The bottoming tap vs plug tap choice changes the length of incomplete thread at the bottom. The Handbook 32nd edition (printed p. 2151) describes a plug tap with roughly 3–5 lead threads and a bottoming tap with roughly 1.5 lead threads. These are tool-family descriptions, not a guaranteed dimensional specification for every vendor. Check the actual chamfer geometry, holder approach and chip path.

Worked manufacturing estimate: suppose M8 × 1.25-6H must deliver 15.0 mm of full-profile thread. With an illustrative three-pitch plug-tap lead, nominal incomplete thread length is 3 × 1.25 = 3.75 mm. Allowing an additional 0.50 mm as an assumed process clearance gives a required full-diameter cylindrical bore near 19.25 mm. If the 6.8 mm drill has a 118° included point, its cone height is (6.8/2) / tan(59°) = 2.04 mm, so tip-apex depth becomes about 21.29 mm. The 0.50 mm allowance is an illustrative planning input, not an ISO or Handbook requirement; a supplier must verify the real tool dimensions, minimum bottom wall and method before releasing the drilling depth.

By contrast, a proposed 17 mm drill-tip depth leaves only about 14.96 mm of cylindrical bore under the same drill-point assumption. Even if 17 mm means cylindrical depth, only 2 mm remains below the claimed 15 mm full thread, less than the example plug-tap lead. Neither interpretation demonstrates the required 15 mm full-profile thread. A short-lead tool, bottoming operation or thread mill may change the conclusion and must be reviewed case by case.

5.Metric Thread Inspection: GO/NO-GO Gauges and Acceptance Criteria

ISO 965-1:2026 defines the metric thread class system. ISO 965-2:2024 gives specified 6H/6g size limits for M1.6–M100. ISO 965-6:2025 provides selected additional classes including 4H, 5H, 7H and 6G. The applicable thread tolerance chart must be matched to the exact pitch, nominal diameter, tolerance class and engagement group. A narrower class should be justified by the assembly, not described as inherently “medical grade” or “aerospace grade”.

5.1 Pitch Diameter and 6H Thread Tolerance

For a 6H thread tolerance, the letter H means zero lower fundamental deviation for the internal pitch and minor diameters. The pitch diameter D₂ controls a key part of the thread flank fit; major diameter D refers to the internal crest-envelope convention, while minor diameter D₁ describes the internal thread opening. These dimensions are not interchangeable with the pilot drill. The basic D₁ reference is not a substitute for the finished D₁ upper limit.

Internal 6H	D₂ min	D₂ max	D₁ min	D₁ max
M6 × 1	5.350	5.500	4.917	5.153
M8 × 1.25	7.188	7.348	6.647	6.912
M10 × 1.5	9.026	9.206	8.376	8.676
M12 × 1.75	10.863	11.063	10.106	10.441

Table basis: ISO 965-2:2024 Table 1, dimensions in millimetres for the applicable normal-engagement entries. These size limits define product geometry. A gauge has its own operating rule. Changing from 6H to 4H or 7H requires class-specific limits from ISO 965-6:2025 and a matching gauge scheme; a scaled 6H table is not a valid reference.

5.2 GO NO GO Thread Gauge and Thread Depth Gauge

ISO 1502:1996 separates the go no go thread gauge functions. For internal threads, a GO screw plug checks the functional threaded envelope over the specified full thread length. A NOT GO screw plug tests the opposite pitch-diameter condition under its turn-limit rule, ordinarily not more than two turns, with a short-thread exception. Independent plain GO and NOT GO plugs assess the minor-diameter limits. A thread pitch gauge identifies pitch and is not a finished tolerance acceptance gauge.

Inspection requirement	Method or gauge	Acceptance evidence / limitation
Thread functional envelope	Internal GO screw plug	Pass along defined thread length by hand without undue force; valid gauge condition
Internal pitch diameter upper limit	Internal NOT GO screw plug	Apply ISO 1502 turn rule, including short-thread condition; not a zero-turn requirement
Finished internal minor diameter	Plain GO / NOT GO plugs	Apply ISO 1502 Clause 7.2.3; do not substitute the pilot-drill diameter
Usable full-profile thread depth	Depth-rated gauge or qualified inspection	Define seating datum, entry chamfer exclusion and last full-profile thread
Hole bottom and minimum wall	Depth probe, CMM or section check	Only if dimensioned/functionally required; report independently

A metric thread gauge must match the designation and be within its calibrated condition, with gauge wear and reference temperature controlled as relevant. A thread depth gauge can be useful only after defining what constitutes full-profile engagement. A GO screw plug that starts successfully does not certify the hole bottom, nor does a NOT GO plug establish the complete thread depth. Record separate acceptance results for each drawing characteristic.

Where mating faces also carry surface requirements, check Ra requirements for threaded features separately from ISO thread size and gauge acceptance.

6.Thread Engagement Length and Internal Thread Stripping

Axial thread engagement is the length over which the mating bolt and tapped component transmit load through usable threads. It is different from a 75% radial tooth-height estimate. Thread stripping can occur in a weak tapped substrate, and the limiting mode can change with bolt strength, thread diameter, engagement length, insert geometry, preload and loading history. Do not infer joint capacity from nominal diameter or pilot-hole geometry alone.

6.1 Minimum Thread Engagement for Bolted Joints

A minimum thread engagement decision requires the actual bolt proof/yield basis, mating internal material strength and usable thread length, together with an assessment of tension, shear, fatigue and the required margin. The common “1D” or “1.5D” shortcut is not a universal ISO 965 requirement. A bolt thread engagement calculation should distinguish possible bolt fracture from internal thread stripping and check edge distance and local wall deformation separately.

For example, a 15 mm usable M8 × 1.25 internal thread has an axial full-thread length of 15/8 = 1.875 nominal diameters. That geometric ratio is not a Pass result for a particular joint. The designer still needs the base-material property evidence, bolt grade, loading, contact conditions and a suitable failure-mode calculation before declaring the thread adequate.

7.CNC Tapping and Manufacturing DFM

CNC tapping is one way to produce a specified finished metric thread. In rigid tapping, spindle rotation and axial feed are synchronized; on a single-start thread the nominal feed per revolution equals pitch, while multi-start threads use the full lead. The drawing should distinguish functional geometry from tool setup and specify a process only when the process itself affects the intended result.

Supplier equipment and material range are described on the CNC machining capabilities page; the drawing and inspection plan still establish acceptance.

For hole wall clearance, tool access and layout changes before RFQ, use the DFM manufacturing guidelines with the actual part geometry and mating assembly.

7.1 Thread Milling vs Tapping

A thread milling vs tapping choice depends on hole size, tool accessibility, desired thread length, workpiece value, machine capacity and recovery risk. Thread milling can avoid a long tap chamfer in some blind-hole geometries, but it may require appropriate interpolation access and machine time. It does not automatically solve a thin remaining floor, inadequate full-profile depth or difficult chip control. The vendor should quote the selected strategy against the drawing-controlled feature, not a blanket promise.

7.2 Spiral Flute Tap and Spiral Point Tap

A spiral flute tap often directs chips back toward the entry and is a candidate for blind holes. A spiral point tap tends to push chips forward, which favors through holes with an exit path. Material, helix geometry and coolant can change the choice; the Handbook 32nd edition covers these tools at printed pp. 2151–2152 and 957–958.

7.3 Material Dependent Tap Selection

For tapping stainless steel, particularly an austenitic alloy with work-hardening behavior, review tool wear, torque, lubrication and chip evacuation instead of imposing a uniform 0.1 mm pilot increase. For tapping aluminum, consider the actual alloy, possible material displacement, burr formation and hole roundness. A material and tap supplier combination should be verified with trial holes and finished-thread gauges; the same adjustment must not be assumed valid for titanium, aluminum and 316L.

Material / condition	RFQ / production check	Failure to watch
316L or other austenitic stainless	Actual cutting method, pilot, tool coating, lubricant and cooling	Work hardening, built-up material, tap fracture
6061 aluminum	Alloy/temper, cutting vs forming tap, burr and pilot measurement	Material flow, damaged crests, wrong finished minor diameter
Deep blind hole	Chamfer length, flute direction, chip storage, minimum floor	Incomplete full threads or trapped chips

7.4 Thread Relief and Thread Runout

Thread relief creates room for incomplete threads or tool exit when the design permits it. Runout does not contribute guaranteed usable full-profile engagement. On a blind tapped hole, define the full-thread boundary and any functional relief requirement. The tool supplier must confirm the resulting geometry. ISO 6410-1:1993 distinguishes a conventionally drawn full-thread end from runout; it does not mandate one universal relief dimension.

8.Drawing, Procurement and Inspection Checklist

Before sending an RFQ, state the intended M diameter, pitch, tolerance designation, thread direction and usable full-thread depth. Confirm the substrate, coating state, minimum surrounding wall, mating bolt, access direction and the inspections that demonstrate fit and function. Where bore-bottom location matters, say whether the dimension means cylindrical full-diameter depth or drill-tip apex depth and provide a controlling datum.

Suppliers should document gauge status and inspection evidence. For a broader quality review, see the CNC supplier inspection checklist. Thread results must still be matched to the specific drawing callout.

RFQ field	Customer / supplier decision
Thread designation	M × P, internal/external, class, hand and starts if unusual
Engagement geometry	Usable full-thread depth, mating fastener and entry chamfer
Blind-hole bottom	Functional floor/adjacent-feature limit; if required, defined bore-depth convention
Material and coating	Alloy, product condition, coating before/after thread inspection
Production method	Cut tap, form tap or thread mill; manufacturer confirms pilot and tooling
Inspection and evidence	GO/NOT GO method, minor diameter, depth, gauge status and records
Procurement inputs	Quantity, drawing revision, critical features, delivery and special gage needs

Download the one-page Metric Thread RFQ Checklist before requesting a quote. It captures the thread designation, full-profile depth, material, production constraints, acceptance method and purchasing requirements in one handoff form.

9.Metric Thread FAQ on Depth, Pitch and Inspection

What is thread pitch?

Thread pitch is the axial distance between corresponding points on neighboring thread profiles. For a single-start ISO metric thread, it also equals nominal lead per revolution. For example, M8 × 1.25 has a 1.25 mm pitch. Compare the intended pitch with the mating bolt; the nominal diameter alone is insufficient.

What is a tapped hole?

A tapped hole is an internally threaded feature produced by tapping, thread milling or another suitable method. The drawing controls the intended thread geometry and usable depth; the shop chooses a compatible method unless a process restriction is functionally required.

What is a blind hole?

A blind hole terminates inside the workpiece instead of passing through. For a blind tapped hole, the complete usable thread length, incomplete end threads and pilot-drill tip are different geometries; ISO 6410-1 does not demand a hole-bottom depth on every drawing.

Can a metric callout omit the coarse pitch or 6H class?

Yes, within the applicable ISO 965-1:2026 Clause 13.2 defaults. However, explicitly writing M8 × 1.25-6H on an RFQ avoids ambiguity between internal and external features and helps confirm gauge selection. A fine-pitch requirement must identify its pitch.

Does a GO screw plug prove full thread depth?

Not automatically. Its function depends on proper use over the specified length, and the inspection plan must define the datum and the last acceptable full-profile thread for a blind hole. Separately inspect the minor diameter and any drawing-controlled bottom depth. ISO 1502 is the gauge reference; ISO 965 contains product size limits.

Is 6.8 mm always the M8 tap drill size?

No. The Handbook lists 6.8 mm for M8 × 1.25 cutting taps and 7.4 mm for a listed cold-form tap. Both are starting process references. The correct pilot also depends on actual tool and material, and the finished thread must meet its drawing-specified tolerance and inspection requirements.

10.Related Resources

Related capability: CNC machining tapping capabilities explains relevant materials and manufacturing processes.

Related article: How to tolerance a CNC drawing covers drawing tolerances beyond the threaded feature.

Related standards reference: ISO 2768 general tolerances and the 2026 revision addresses general dimensions outside this ISO thread designation.

Related standards reference: ISO 286 fits for shafts and holes covers mating non-thread cylindrical fits.

Related article: Surface roughness Ra chart for CNC parts covers separate surface-texture requirements.