Thread tolerances define how far the manufactured dimensions of a screw thread may vary while the thread still assembles and performs as intended. They control more than whether a bolt can enter a tapped hole. The selected tolerance class affects interchangeability, assembly clearance, coating allowance, inspection, machining cost, and the risk of stripping or seizure. A thread that is too large may not assemble; one that is too small may feel loose or provide inadequate flank contact. This guide explains metric and Unified thread classes, major and minor diameters, the effect of plating, CNC threading methods, gauge inspection, and a practical process for specifying thread tolerances on engineering drawings.
What Is Thread Tolerance?
Thread tolerance is the permitted dimensional variation between the maximum and minimum limits of a threaded feature. Because tools wear, materials deflect, and cutting conditions vary, no production thread matches its basic mathematical profile exactly. A tolerance system defines an acceptable zone around that profile so separately manufactured internal and external threads remain interchangeable.
Tolerance should not be confused with allowance. Tolerance describes permitted variation within one feature. Allowance is the intentional difference between mating parts at their maximum material limits. In a normal clearance thread fit, that difference prevents the largest permitted external thread from interfering with the smallest permitted internal thread.
| Terim | Anlam | Effect on Thread Fit |
|---|---|---|
| Basic size | The theoretical size from which limits and deviations are established | Provides the common reference for the mating threads |
| Limits of size | The largest and smallest acceptable dimensions | Define the pass/fail boundaries |
| Tolerans | The difference between the upper and lower limits | Controls permitted manufacturing variation |
| Allowance | The intentional minimum clearance or maximum interference at maximum material limits | Establishes the designed relationship between mating parts |
| Clearance | The available space between mating thread surfaces | Affects assembly ease, motion, and coating capacity |
For example, two external threads can have the same nominal diameter but different tolerance positions. The one whose tolerance zone is farther below the basic size provides more minimum clearance when paired with the same internal thread. It is not necessarily manufactured less accurately; its acceptable size zone is positioned differently.
Which Thread Dimensions Are Controlled?
A complete thread specification controls a geometric system rather than one diameter. The principal characteristics include major diameter, minor diameter, pitch diameter, pitch, lead, flank angle, and thread form. Their limits and inspection requirements depend on the thread standard and tolerance class.
Major and Minor Diameter of Threads Explained
The major and minor diameter of threads describe the largest and smallest cylindrical boundaries of the profile. On an external thread, the major diameter passes through the crests and the minor diameter passes through the roots. On an internal thread, the minor diameter passes through the inward-facing crests, while the major diameter lies at the roots. This reversal in physical location is why internal and external limits must not be interchanged.
| Thread Dimension | External Thread Location | Internal Thread Location | Functional Importance | Common Inspection Method |
|---|---|---|---|---|
| Major diameter | Across the crests | Across the roots | Controls the outer envelope and crest/root clearance | Micrometer, caliper, optical measurement |
| Minor diameter | Across the roots | Across the crests | Affects thread depth, root clearance, and section strength | Optical method, internal gauge, bore measurement where applicable |
| Pitch diameter | Imaginary cylinder where nominal thread thickness equals groove width | Strongly influences flank contact and assembly fit | Thread micrometer, three-wire method, calibrated functional gauge | |
| Pitch | Axial distance between corresponding points on adjacent threads | Must match for the threads to advance together | Pitch gauge, optical comparator, CMM | |
| Kurşun | Axial advance in one revolution | Equals pitch for a single-start thread; differs for multi-start threads | Lead measurement system, CMM | |
| Flank angle and form | Shape and angle of the thread flanks, crests, and roots | Affect contact, load transfer, and compatibility | Optical comparator, profile measurement | |
The nominal size alone does not provide the finished limits for the thread major and minor diameter. Those limits depend on the standard, nominal size, pitch or threads per inch, internal or external designation, and tolerance class. A tap-drill diameter also is not the same as the final internal minor-diameter tolerance. The drilled hole influences thread percentage, cutting torque, and tap life, but the formed or cut profile must still meet the specified thread requirements.
Why Is Pitch Diameter So Important?
Pitch diameter is usually the most influential diameter for functional fit because mating thread flanks contact near the pitch cylinder. An oversized external pitch diameter or undersized internal pitch diameter can make assembly tight or impossible. The opposite condition can create excessive clearance, wobble, and reduced flank engagement.
However, pitch diameter is not the only determinant of performance. Lead error, flank-angle error, crest and root interference, engagement length, material strength, preload, surface condition, and thread damage can all affect assembly and load capacity. A part can have an acceptable measured pitch diameter and still fail a functional gauge because cumulative form or lead errors consume the available tolerance.
How to Read ISO Metric Thread Tolerance Classes
ISO metric thread tolerances use a number and a letter to identify the tolerance grade and tolerance position. Consider an internal thread marked M10 × 1.5-6H and an external thread marked M10 × 1.5-6g. M10 is the nominal diameter, 1.5 mm is the pitch, the number 6 identifies the tolerance grade, and H or g identifies the tolerance position relative to the basic profile. Uppercase letters apply to internal threads; lowercase letters apply to external threads.
What Does 6H Mean?
6H is a widely used medium tolerance class for a general-purpose ISO metric internal thread. The grade 6 defines the applicable tolerance width, while position H has zero fundamental deviation at the relevant boundary. It is commonly paired with a 6g external thread. The complete standard tables must still be used to obtain the actual diameter limits for a particular nominal size and pitch.
What Does 6g Mean?
6g is a common ISO metric external-thread tolerance class. Its tolerance zone is displaced below the basic profile, creating allowance relative to an H-position internal thread. This facilitates assembly and can provide room for expected dimensional effects, although coating allowance must still be calculated and specified rather than assumed.
What Is a 6h Thread Tolerance?
A 6h thread tolerance normally identifies an ISO metric external thread. The lowercase h indicates zero fundamental deviation, while 6 gives the tolerance grade. A 6h external thread therefore reaches closer to the basic-size boundary than a comparable 6g thread. It may provide less guaranteed clearance when paired with the same internal thread.
| Özellik | 6h External Thread | 6g External Thread |
|---|---|---|
| Tolerance grade | 6 | 6 |
| Tolerance position | h; zero fundamental deviation | g; zone displaced below the basic profile |
| Relative assembly allowance | Less than 6g when other conditions are equal | More than 6h when other conditions are equal |
| Selection concern | Useful only when the resulting fit and finishing condition are appropriate | Common general-purpose choice, but not a universal coating solution |
The difference between 6g and 6h is mainly the position of the tolerance zone, not a simple ranking of “low precision” versus “high precision.” Neither designation should be selected without considering the mating thread, surface finish, operating temperature, assembly method, and final inspection condition.
How Unified Thread Classes Work
UNC, UNF, and UNEF identify Unified thread series, while Classes 1, 2, and 3 indicate progressively closer tolerance classes. The letter A designates an external thread and B designates an internal thread. A common commercial pairing is a Class 2A external thread with a Class 2B internal thread.
| Unified Class | Thread Type | Relative Fit | Tipik Uygulama |
|---|---|---|---|
| 1A | External | Loose | Quick assembly or conditions where dirt and damage require extra allowance |
| 1B | Internal | Loose | Mates with 1A in selected low-precision applications |
| 2A | External | General-purpose commercial | Standard bolts and CNC-machined external threads |
| 2B | Internal | General-purpose commercial | Standard nuts and tapped or thread-milled holes |
| 3A | External | Close | Applications requiring tighter control of fit and accuracy |
| 3B | Internal | Close | Mates with 3A where closer tolerances provide functional value |
Class 2A and 2B are not two alternative grades for the same feature: one applies to an external thread and the other to an internal thread. Likewise, 3A commonly mates with 3B. A Class 3 thread is not automatically stronger than a Class 2 thread. Joint strength depends on material, engagement, preload, geometry, and failure mode; the tighter class mainly reduces permitted dimensional variation and clearance.
ISO Metric vs. Unified Thread Tolerances
| Karşılaştırma | ISO Metric Threads | Unified Threads |
|---|---|---|
| Size system | Millimeters | Inches |
| Typical callout | M10 × 1.5-6H | 5/16-18 UNC-2B |
| Internal/external identifier | Uppercase letter for internal; lowercase for external | B for internal; A for external |
| Class structure | Grade number plus tolerance-position letter | Class number plus A/B designation |
| Common markets | Global machinery, automotive, medical, and industrial products | Products designed primarily around U.S. inch standards |
| Source for actual limits | Applicable ISO metric thread standard tables | Applicable ASME Unified thread standard tables |
No universal one-to-one conversion turns 6H into 2B or 6g into 2A. The systems use different class structures and limit calculations. When converting a design, engineers should review the actual major-, minor-, and pitch-diameter limits and verify functional requirements. Hole and shaft fit symbols such as H7/g6, H7/k6, and H7/p6 belong to cylindrical fit systems and must not be used as screw-thread tolerance classes.
How to Read a Thread Tolerance Chart
A reliable thread tolerance chart must be tied to a specific standard, thread series, nominal size, pitch, internal or external type, and class. A chart that lists only “M10” or “5/16-18” cannot define all acceptance limits. Use conceptual comparison charts for class selection, but use the governing standard or a controlled engineering table for production dimensions.
- Confirm whether the drawing uses ISO metric or Unified threads.
- Find the exact nominal size and pitch or TPI.
- Select the internal or external table.
- Locate the specified tolerance class.
- Read each controlled diameter limit; do not substitute tap-drill size.
- Confirm whether limits apply before or after coating.
- Use the drawing-specified standard revision when contractually required.
This approach is essential when comparing metric thread tolerances or troubleshooting parts made by different suppliers. A class name without its dimensional context is not an inspection result.
What Are the 5/16-18 Thread Dimensions?
5/16-18 UNC is a Unified coarse thread with a nominal major diameter of 5/16 inch, or 0.3125 inch, and 18 threads per inch. Its basic pitch is 1/18 inch, approximately 0.05556 inch. Those two values describe the thread series, but they do not provide every manufacturing limit.
| 5/16-18 Parameter | Anlam | Basic or Variable? | Tasarım Notu |
|---|---|---|---|
| Nominal major diameter | 5/16 in. (0.3125 in.) | Basic designation | Not the guaranteed measured major diameter of every finished thread |
| Threads per inch | 18 TPI | Basic designation | Defines a pitch of approximately 0.05556 in. |
| External major diameter | Diameter across external crests | Variable within class limits | Depends on 1A, 2A, or 3A requirements |
| External minor diameter | Diameter across external roots | Variable within applicable limits | Do not use an internal-thread value |
| Internal minor diameter | Diameter across internal crests | Variable within class limits | Not identical to the nominal tap-drill diameter |
| Pitch diameter | Functional size near flank contact | Variable within class limits | Use the correct A or B class table |
| Tolerance class | For example, 2A external or 2B internal | Design selection | Must appear in the complete callout |
Therefore, there is no single context-free 5/16-18 minor diameter. Internal and external threads have different minor-diameter definitions and limits, and the allowable values vary with the specified class. A tap chart may recommend a drill size for a desired thread percentage, but that recommendation is not a substitute for the finished internal-thread minor-diameter limits in the applicable ASME standard.
What Is the Tolerance for Thread Holes?
There is no universal answer to what is the tolerance for thread holes. It depends on the thread system, size, pitch, internal tolerance class, engagement length, process, final finish, and inspection standard. An ISO metric internal thread might be specified as M10 × 1.5-6H, while a Unified internal thread might be 5/16-18 UNC-2B.
A note such as “M10 threaded hole” or “5/16-18 tapped hole” may not fully define acceptance. A production drawing should also state the class, effective thread depth, handedness if nonstandard, applicable standard when necessary, surface-treatment condition, and any special gauge requirement. A general title-block linear tolerance does not replace a screw-thread tolerance class.
How Surface Treatments Affect Thread Tolerance
Many coatings reduce available thread clearance because they add material to the flanks. Their effect on functional pitch diameter can be greater than a simple one-surface thickness assumption because deposition occurs on both flanks. Actual compensation depends on the thread geometry and process. For close tolerance plating, the drawing must define whether the thread class applies before processing or to the finished coated part.
| Yüzey İşlemi | Typical Dimensional Effect | Thread Design Consideration |
|---|---|---|
| Çinko kaplama | Adds deposited material; distribution may vary | Allow for specified thickness and verify finished fit |
| Electrolytic nickel plating | Adds material and may be less uniform in recessed areas | Confirm current-density effects and final acceptance condition |
| Elektrolizsiz nikel | Adds a comparatively uniform deposit, including on complex surfaces | Use the supplier’s controlled thickness range for compensation |
| Type II anodizing | Oxide grows partly inward and partly outward | Do not treat the entire coating thickness as external buildup |
| Sert anodizasyon | Thicker conversion layer with inward and outward growth | Mask, compensate, or finish-machine critical threads as specified |
| Paint or powder coating | Relatively thick buildup that can obstruct threads | Threads are commonly masked unless coating is functionally required |
| Pasivasyon | No significant deposited layer like plating | Cleaning and chemistry still require process control, but conventional plating buildup is not expected |
| Dry-film lubricant | Adds a thin functional film | Check film thickness, friction requirement, and final gauge plan |
How Should Close-Tolerance Threads Be Designed for Plating?
First establish the required finished fit. Then obtain the realistic coating-thickness range and distribution from the finishing process. The designer and manufacturer can select a pre-plate size or tolerance strategy that produces the required final condition. Do not assume that changing from 6h to 6g, or from Class 3 to Class 2, automatically supplies the correct compensation.
The drawing should identify whether inspection occurs before or after finishing. Critical coated threads should normally be verified after treatment with the specified functional gauge or measurement method. Masking may be more reliable when the coating is not needed on the thread. If masking is not permitted, sample trials may be required before production to establish machining compensation.
How Materials Influence Thread Fit
The class establishes dimensional limits, but material behavior influences how consistently those limits can be produced and how the thread performs in service.
- Alüminyum: Easy to machine but susceptible to crest damage and stripping. Adequate engagement length or a threaded insert may be necessary.
- Stainless steel: Prone to galling in certain material pairings. Clearance, lubrication, surface finish, and assembly speed matter.
- Titanyum: Galling risk, low thermal conductivity, and tool wear require controlled cutting parameters and careful assembly planning.
- Hardened steel: Provides strength and dimensional stability but can require grinding or other capable finishing processes after heat treatment.
- Brass: Generally machines cleanly, although thin-wall internal threads can distort under clamping or cutting forces.
- Engineering plastics: Thermal expansion, moisture absorption, creep, elastic recovery, and inspection temperature can change measured and long-term fit.
Material name alone does not determine the correct class. Engineers should also consider operating temperature, corrosion, load, assembly frequency, lubricant, engagement length, and the risk of galling between dissimilar or similar materials.
How CNC Machining Processes Affect Thread Accuracy
| Threading Process | En Uygun Olanlar | Tolerance Control | Ana sınırlama |
|---|---|---|---|
| Diş açma | Fast production of common internal threads | Primarily controlled by tap geometry, condition, runout, and hole preparation | Chip evacuation, blind-hole depth, and tap-breakage risk |
| Single-point turning | External and accessible internal threads on turned parts | Offsets can adjust size; repeated passes improve control | Requires suitable access, rigidity, and synchronization |
| Diş frezeleme | Large, special, or high-value internal and external threads | Toolpath compensation permits controlled pitch-diameter adjustment | Higher cycle time and programming requirements |
| Thread chasing | Restoring or finishing existing threads | Can correct limited size or form issues | Not a remedy for severe geometry or lead errors |
| Thread grinding | Hardened components and very accurate threads | High form and dimensional capability | Specialized equipment and greater cost |
| Thread rolling | High-volume external threads with favorable grain flow | Stable when dies, blanks, and material are controlled | Not a cutting process; requires ductile material and dedicated tooling |
Common error sources include tool wear, incorrect offsets, tap runout, spindle synchronization error, machine backlash, workpiece deflection, cutting heat, built-up edge, incorrect pre-drill diameter, poor chip evacuation, hardness variation, and uncontrolled inspection temperature. The process plan must also provide clearance for tap lead, thread-mill entry, or turning-tool runout. Calling out full threads to the bottom of a blind hole without adequate depth is a common design-for-manufacturing error.
How Are Thread Tolerances Inspected?
Inspection can be functional or dimensional. Plug gauges inspect internal threads, and ring gauges inspect external threads. Thread micrometers and the three-wire method measure pitch diameter on accessible external threads. Optical comparators, vision systems, and CMMs can evaluate profiles, angles, pitch, and location when the measurement strategy and uncertainty are appropriate.
What Does a Go/No-Go Gauge Actually Check?
The Go gauge evaluates the thread at its maximum-material functional boundary and should engage as required over the specified thread length. Because it is a functional gauge, it responds to the combined effect of several geometric errors. The No-Go gauge checks the opposite size boundary according to the applicable gauge standard. A plug gauge must match an internal thread; a ring gauge must match an external thread. Size, pitch, class, standard, calibration status, wear, cleanliness, and inspection technique all matter.
Can a No-Go Gauge Enter One or Two Turns?
Do not apply one universal turn-count rule to every thread. Permitted No-Go engagement depends on the applicable ISO or ASME gauging standard, gauge type, thread form, engagement length, and customer requirement. Inspectors should follow the drawing and the standard under which the gauge was manufactured. A shop rule such as “three turns always pass” can accept nonconforming parts when used outside its intended standard.
How to Select the Right Thread Tolerance
- Identify the governing thread standard and series.
- Confirm whether the feature is internal or external.
- Define assembly clearance, alignment, interchangeability, and service needs.
- Evaluate load, vibration, sealing, and engagement length.
- Consider material movement, damage, galling, and temperature.
- Account for plating, anodizing, paint, or lubricant films.
- Confirm that the selected manufacturing process can hold the class.
- Define the final inspection method and acceptance condition.
- Check whether a tighter class creates measurable functional value.
- Place a complete, unambiguous callout on the drawing.
The following chart provides starting points only. Final thread tolerances must be confirmed against the applicable standard, joint analysis, environmental conditions, and product requirements.
| Uygulama | Typical Starting Class | Neden | Ek Dikkat Edilmesi Gereken Hususlar |
|---|---|---|---|
| General metric industrial assembly | 6H internal with 6g external | Common general-purpose fit | Confirm finish and service temperature |
| General Unified industrial assembly | 2B internal with 2A external | Common commercial fit | Verify whether fasteners are coated |
| Frequently assembled component | General-purpose class with validated clearance | Reduces assembly sensitivity | Wear, lubricant, dirt, and galling |
| Coated external fastener | Class determined from final-fit analysis | Coating changes effective size | Coating range, masking, and post-plate gauging |
| Aerospace joint | Drawing- and standard-specific | Traceability and joint performance govern | Preload, fatigue, locking method, and inspection |
| Hydraulic component | Thread-form- and sealing-system-specific | Mechanical and sealing functions may differ | Do not substitute fastening-thread guidance for pipe-thread requirements |
| High-temperature equipment | Selected from thermal fit analysis | Differential expansion changes clearance | Material pair, oxidation, and assembly temperature |
| Plastic threaded component | Application-specific with realistic clearance | Molding or machining recovery and creep affect fit | Moisture, temperature, inserts, and tightening torque |
How Thread Tolerance Affects Manufacturing Cost
Tighter thread tolerances can require more capable tooling, closer offset control, shorter tool-change intervals, slower or more controlled machining, and additional setup trials. Inspection may require dedicated gauges, more frequent sampling, calibrated measurement equipment, post-treatment verification, and lot traceability. Scrap and rework exposure also rises when the process window narrows.
“Tighter” is therefore not automatically “better.” If 6H/6g or 2B/2A meets the functional requirement, moving to a closer class can increase cost without improving joint strength or service life. The correct class is the least restrictive one that reliably satisfies assembly, interchangeability, alignment, sealing, and load requirements.
Common Thread Tolerance Problems and Solutions
| Sorun | Muhtemel Neden | Recommended Check | Corrective Action |
|---|---|---|---|
| Go gauge will not enter | Excessive material, burrs, coating buildup, wrong pitch, or form error | Clean the part and gauge; verify class, pitch diameter, and coating condition | Correct offset or process, deburr, and establish coating compensation |
| No-Go gauge enters too far | Pitch diameter too loose, worn tool, or incorrect offset | Confirm the applicable gauging rule and measure pitch diameter | Adjust the process and replace worn tooling |
| Fits before plating but not after | No or inadequate coating allowance | Measure deposit range and inspect after plating | Revise pre-plate limits, mask the thread, or control coating thickness |
| Bolt feels loose | Excessive clearance, class mismatch, wear, or incorrect mating part | Verify both complete callouts and functional gauges | Correct the specified or manufactured class |
| Tap breaks | Small pre-drill, poor chip evacuation, misalignment, or tool wear | Review hole size, depth, lubricant, runout, and tap condition | Optimize preparation and cutting strategy |
| Internal thread strips | Insufficient engagement, weak material, over-torque, or damaged profile | Review joint calculation and inspect the thread | Increase engagement, use an insert, or change material/torque |
| Stainless threads seize | Galling, inadequate clearance, or unsuitable lubrication | Inspect surfaces and review material pairing | Use a validated lubricant, coating, material pair, and assembly procedure |
| Early parts pass; later parts fail | Tool wear, heat drift, chip buildup, or coating variation | Trend gauge and measurement results over the run | Set tool-life limits and in-process checks |
| Different suppliers’ parts do not mate | Incomplete callout, mixed standards, or different inspection conditions | Compare drawings, gauges, standards, and finish requirements | Standardize the specification and final acceptance method |
What Should Be Included in a Thread Callout?
A production drawing should identify the nominal diameter, pitch or TPI, thread series or form, tolerance class, and thread depth or engagement length. It should also specify left-hand direction when applicable, the governing standard when needed, surface treatment, final inspection condition, and any special gauge or acceptance requirement.
- ISO metric internal example: M10 × 1.5-6H, 15 mm minimum full thread. This identifies a 10 mm nominal metric thread, 1.5 mm pitch, internal 6H class, and required effective depth.
- Unified external example: 5/16-18 UNC-2A. This identifies a 5/16-inch nominal Unified coarse external thread with 18 TPI and Class 2A tolerance.
Additional notes may be required for handedness, coating, start configuration, runout, or inspection. The exact drawing syntax should follow the organization’s drafting standard and the product’s contractual requirements.
Design Checklist for CNC-Machined Threads
- Avoid a tighter class unless it creates a defined functional benefit.
- Provide tool-entry and runout clearance.
- Distinguish drill depth from full-thread depth in blind holes.
- Allow for tap chamfer and incomplete threads.
- Define pre-finish and post-finish acceptance clearly.
- Use realistic engagement length based on the weaker material.
- Consider inserts in soft metals and plastics.
- Specify inspection after final finishing for critical coated threads.
- Confirm gauge standard and class with the manufacturer.
- Review critical threads during DFM before releasing production.
PTSMake supports CNC tapping, thread milling, single-point threading, and the inspection of metric, UNC, UNF, and custom threads. Before machining, the engineering team can review callouts, engagement length, material behavior, tool access, coating condition, and the proposed gauge method. This DFM review helps prevent incomplete specifications and unnecessary close tolerances from turning into avoidable machining and inspection cost.
FAQs About Thread Tolerances
What are the major and minor diameters of threads?
The major diameter is the largest cylindrical boundary of a thread, and the minor diameter is the smallest. For an external thread, the major diameter passes across the crests and the minor diameter across the roots. For an internal thread, the minor diameter passes across the inward crests and the major diameter lies at the roots. Actual limits depend on the standard and class.
What is the tolerance for thread holes?
There is no universal threaded-hole tolerance. It depends on the system, size, pitch, internal class, material, process, finish, and inspection standard. Common examples are 6H for a general ISO metric internal thread and 2B for a general Unified internal thread, but neither should be applied automatically without checking the mating part and service requirements.
What does a 6h thread tolerance mean?
6h normally identifies an ISO metric external thread. The number 6 gives the tolerance grade, while lowercase h identifies an external-thread tolerance position with zero fundamental deviation. Compared with 6g at the same size and pitch, 6h generally provides less allowance relative to the basic profile. It is not an internal-thread designation.
What is the difference between 6H and 6g?
6H normally applies to an ISO metric internal thread, while 6g applies to an external thread. The uppercase H and lowercase g identify different feature types and tolerance positions. They are frequently used as a general-purpose mating combination, but the actual diameter limits still depend on nominal size and pitch.
What are the standard 5/16-18 thread dimensions?
A 5/16-18 UNC thread has a 0.3125-inch nominal major diameter and 18 threads per inch, giving a basic pitch of about 0.05556 inch. Finished major-, minor-, and pitch-diameter limits vary according to whether the thread is internal or external and whether its class is 1, 2, or 3.
What is the 5/16-18 minor diameter?
There is no single 5/16-18 minor diameter that applies to every thread. Internal and external threads use different minor-diameter boundaries, and their limits change with the tolerance class. A recommended tap-drill size is not the same as the finished internal minor-diameter tolerance. Use the specified ASME class table for inspection values.
Does plating change thread tolerance?
Plating does not change the named class by itself, but it adds material and can move the finished thread outside the class limits or eliminate needed clearance. Critical drawings should state whether the class applies before or after plating. Compensation should use the actual process thickness and distribution, followed by final inspection where required.
How do I read a thread tolerance chart?
First identify the governing standard, nominal size, pitch or TPI, internal or external thread, and class. Then read the relevant major-, minor-, and pitch-diameter limits from that exact table. Confirm coating condition and standard revision. Do not take a value from a similarly named class or treat a tap-drill chart as a finished thread tolerance chart.
Is tap drill size the same as the internal thread minor diameter?
No. Tap-drill size is the hole size selected before tapping and influences thread percentage, tap torque, and tool life. The finished internal minor diameter results from the complete tapping or thread-forming process and must fall within the limits applicable to the specified thread class. Material recovery and forming can make the distinction especially important.
Which thread diameter determines whether two parts will fit?
Pitch diameter is often the main dimensional influence on flank fit, but it is not the sole determinant. Major- and minor-diameter interference, lead error, flank-angle error, burrs, damage, and coating buildup can also prevent assembly. A functional Go gauge is valuable because it evaluates the combined effect of several thread characteristics at the functional boundary.
Sonuç
Correct thread tolerances begin with the right standard, complete callout, and clear distinction between internal and external threads. ISO classes such as 6H, 6g, and 6h cannot be treated as direct equivalents of Unified 2B, 2A, or other classes. Major, minor, and pitch diameters each serve different functions, while material behavior, machining method, coating thickness, temperature, and inspection strategy influence the finished fit. A tighter class should be specified only when it produces a measurable assembly or performance benefit. For CNC-machined parts, early DFM review and a defined post-finish gauge plan are the most reliable ways to prevent threads that pass in machining but fail during coating, assembly, or incoming inspection.