ANSI → ISO Tolerance ConversionFrom Inch-Based Limits to ISO 286 Fits
A complete guide to converting ANSI B4.1 inch-based tolerances to ISO 286 metric fits. Learn how to interpret RC/LC/LT/LN/FN classes, choose ISO IT grades, and specify H7/g6 style fits that match real clearance or interference requirements in metric CNC manufacturing.
Table of Contents
Why ANSI→ISO Conversion Matters
Why imperial drawings need ISO fits in metric shops
Go to Section →ANSI vs ISO Basics
Size, limits, fits, and system differences
Go to Section →Conversion Workflow
Step-by-step from inch limits to ISO fits
Go to Section →Practical Examples
Real-world shaft, hole, and press-fit cases
Go to Section →Common Pitfalls
Mistakes that break fits or waste money
Go to Section →Best Practices & FAQ
Design, QA, and supplier alignment tips
Go to Section →Why ANSI → ISO Tolerance Conversion Matters
Many legacy and US-origin drawings use inch units and ANSI-style tolerances, while most high-volume manufacturing today is performed in metric shops that work with ISO-based fits and gauges. If you only convert sizes from inches to millimeters and keep the same numeric tolerances, you often end up with awkward, non-standard metric limits that do not match ISO 286 fits, standard tooling, or inspection practices.
Proper ANSI to ISO tolerance conversion focuses on functional equivalence, not on preserving every micro-inch. The goal is to keep clearance or interference behavior the same while expressing limits as ISO fits such as Φ50 H7/g6 or Φ25 H6/h5. This helps CNC programmers, process engineers, and QC teams work with familiar metric fits, reduces conversion errors, and improves communication with suppliers in Europe and Asia.
ANSI vs ISO Tolerance Basics
Size, Limits, Tolerance, and Fits
Both ANSI and ISO start from the same fundamentals. A basic or nominal size is the target size from which limits are derived. Upper and lower limits define the extreme sizes that are allowed, and the difference between them is the tolerance. When a shaft and hole mate, the combination of their limits defines clearance, transition, or interference fits.
In practice, you will always compute minimum and maximum clearance or interference when converting from ANSI to ISO. This is the only way to verify that the new ISO fit preserves actual functional behavior after unit conversion.
ANSI B4.1 vs ISO 286
ANSI B4.1 uses inch-based fit classes such as RC (running clearance), LC (locational clearance), LT (locational transition), LN (locational interference), and FN (force fit). Drawings often show either those classes or direct dimensions with unilateral or bilateral tolerances.
ISO 286 uses metric tolerance grades (IT5, IT6, IT7, etc.) combined with tolerance zones like H7, g6, or p6. Uppercase letters apply to holes, lowercase letters to shafts. A fit such as 50 H7/g6 fully defines the tolerance width and its position relative to the basic size for both hole and shaft.
Step-by-Step Conversion Workflow
From Inch Limits to ISO Fits
Use this repeatable workflow whenever you convert an ANSI drawing for manufacture in a metric shop. The steps assume you have access to both mating features and can compute clearances or interference values.
Multiply the basic inch size by 25.4 to get the metric basic size. Decide whether to keep the exact metric value, such as 25.4 mm, or to round to a clean metric size like 25 mm or 30 mm when redesigning for fully metric product lines.
From unilateral, bilateral, or limit dimensions, compute max and min sizes for each feature. When fit classes like RC3 or FN2 are specified, reference ANSI tables to understand the intended clearance or interference band before you convert.
Determine if the application requires a clearance fit for free running, a transition fit for accurate location, or an interference fit for permanent assembly. Compute minimum and maximum clearance or interference based on ANSI limits so you have a numerical target.
Match the overall tightness of the ANSI tolerance to a reasonable ISO IT grade. Precision fits typically map to IT5–IT7, general machining fits to IT7–IT9, and non-critical features to IT9–IT11. The goal is to maintain cost-effective manufacturability while preserving functional intent.
Use a hole-basis system by default. Choose H7 or H8 for most machined holes and pair them with shaft zones such as g6, f7, k6, or p6 depending on whether you need clearance, transition, or interference fits. Verify that the resulting min/max clearance or interference in ISO is close to what you had in ANSI.
Confirm that your in-house processes or suppliers can reliably achieve the chosen IT grades at the relevant diameter range. If not, relax the grade or adjust the fit to widen tolerances while keeping functional behavior and safety margins intact.
Practical Conversion Examples
Example 1: Shaft with Bilateral Tolerance
A shaft is specified as 2.5000 ± 0.0050 in on an ANSI drawing. The shaft runs in a bushing, so the intent is a moderate clearance running fit.
2.5000 in × 25.4 = 63.500 mm. The total tolerance is 0.0100 in, which is 0.254 mm. The shaft can vary from 63.373 mm to 63.627 mm after conversion.
This level of control is similar to an IT8 or IT9 tolerance for a diameter around 63.5 mm. For a running clearance fit, a common choice would be Φ63.5 H7/g8 or H8/f7, depending on the hole tolerance and process capability.
Using ISO 286 tables, compute the min and max clearance for the H7/g8 pair and compare them to the original ANSI clearance range. If the ISO fit slightly increases clearance, that usually improves manufacturability and assembly robustness without harming function.
Example 2: Hole with Limit Dimensions
A hole is specified as 1.0000 / 0.9995 in on the drawing. This is a tight tolerance, used for accurate location or a precision slip fit.
The tolerance is 0.0005 in, which is about 0.0127 mm. Converted limits are approximately 25.400 mm max and 25.387 mm min. This points to a high-precision hole, close to an IT6 range at this diameter.
Select Φ25.4 H6 for the hole, pairing it with a shaft fit such as g5 or h5 depending on desired clearance. This expresses the same intent in standard ISO terminology while remaining compatible with reamers and gauge practices in metric shops.
Include a short note in your documentation stating that this is a conversion from the original 1.0000 / 0.9995 in requirement, and that Φ25.4 H6 is chosen as the ISO equivalent fit for metric manufacture.
Example 3: Light Press Fit for Bearing
A bearing outer ring is pressed into a housing. The original ANSI design allows up to 0.001 in interference relative to bearing OD on a nominal 3.1496 in diameter (approximately 80 mm).
0.001 in corresponds to about 0.0254 mm. You want a light press fit with roughly 0 to 0.03 mm interference. This guides the choice of ISO interference fits around the 80 mm diameter range.
A typical choice is Φ80 H7/p6 or H7/n6, depending on the bearing's catalog tolerance. The bearing OD usually follows a standard ISO shaft tolerance, and the housing bore is sized using an H hole and a positive shaft deviation to create the desired interference band.
Check press force, risk of spinning, and thermal expansion in service. If the ISO fit is significantly tighter or looser than the original ANSI design, adjust the selected tolerance zones rather than forcing a mathematically exact unit conversion.
Common Pitfalls When Converting Tolerances
Copying Numeric Tolerances Only
Simply converting ± tolerances from inches to millimeters often produces non-standard limits like 63.500 ± 0.127 mm. These do not map cleanly to ISO tolerance grades, complicate gauging, and may be tighter or looser than needed for the actual function.
Ignoring the Mating Feature
Converting a shaft or hole in isolation can destroy the intended fit. Always compute minimum and maximum clearance or interference from both features and preserve that band when choosing ISO fits.
Over-Tightening Every Fit
Mapping all ANSI tolerances to IT6 or better drives cost without necessarily improving performance. Choose IT grades based on function and proven process capability, not on worst-case precision.
Mixing Standards on One Drawing
Combining inch dimensions, ANSI fits, metric dimensions, and ISO fits on the same drawing leads to confusion and inspection errors. Prefer one primary standard per drawing and document how conversions were performed.
Best Practices & FAQ
Design & Documentation
Choose one primary standard for each drawing and clearly indicate when a part has been converted from ANSI to ISO. Keep a short conversion note in your design files linking the original inch-based limits to the selected ISO fits, so future engineers understand the rationale.
Process Capability
Align tolerance choices with what your machines and suppliers can actually hold. For turning and boring, IT6–IT8 is realistic for many shops. For drilling and reaming, IT7–IT9 is common, while grinding can reach IT5–IT6 when needed.
Supplier Communication
Share both the original ANSI spec and the new ISO fit when you first move a part to a metric supplier. Invite feedback about achievable IT grades and preferred fits for their processes. Adjust designs based on real capability instead of theoretical tables alone.
General Tolerance Blocks
When ANSI drawings use a general ± tolerance, map it to an appropriate ISO 2768 class or a clear metric general tolerance. Document the mapping so CNC programmers and inspectors know which features were tightened or relaxed in the conversion.
Quick Decision Guide
For everyday work, you can remember a few simple rules when converting fits:
- Start from function: clearance, transition, or interference.
- Use a hole-basis system with H7 or H8 for most machined holes.
- Pick IT grades based on required precision and process capability.
- Use g, f, or h shafts for clearance, k or j for transition, and n or p for interference.
- Always verify min/max clearance or interference before releasing the drawing.
Related Tools
Use these tools alongside tolerance conversion
Convert Tolerances with Confidence
Use the workflow and examples in this guide, then pair them with the tolerance converter and machining tools to keep inch-based designs and metric production perfectly aligned.