6.5 Drawing Revisions and Block Tolerances
Key Takeaways
Match the actual job to approved drawing and dataset revisions. Follow revision records before using an older program, setup sheet or gage plan.
Use the drawing’s general tolerance only where its scope applies. Local tolerances and geometric requirements apply to the features they control.
Boxed basic dimensions give theoretically exact geometry for related controls. Reference dimensions provide information and are treated separately from acceptance limits.
6.5 Drawing Revisions and Block Tolerances
Start with the approved revision
Read the part or drawing identifier, issue or revision, applicable sheet or model, units, scale, specifications and general notes. A title block often carries several of these items. A separate revision block or linked change record can identify what changed. This information may differ across drawing formats or electronic datasets. Use the approved job package to identify which drawing, model or revision applies. The newest version available on a shared drive may be for a different job or effective change.
Suppose the work order calls for revision D and the existing operation sheet identifies revision C. Review the controlled change and check related setup, tool paths, fixtures and inspection criteria before using the old program. A changed hole size may need another tool or gage. A changed reference order can affect location and inspection without changing the nominal coordinates. Update associated documents according to the shop’s control process. Verbal agreement with the old dimension is insufficient to decide which job definition governs.
Decide which tolerance applies
General tolerances can be in a title block or in a drawing note. They apply as specified for the class of dimension and may give different defaults for decimals, fractions, angles or other cases. Different prints use different rules. Check the units and which features are included. A print’s precision or formatting alone cannot supply a tolerance.
| Example marking | How to use it |
|---|---|
| 1.250 alone with an applicable .XXX ±0.005 in general rule | The dimension has the stated default. Its limits are 1.245 to 1.255 in. |
| 1.250 +0.002 / −0.000 in | Use its local limits of 1.250 to 1.252 in. The block tolerance does not add to them. |
| Boxed 1.250 locating a hole whose position is geometrically controlled | Use that theoretically exact basic value with the related geometric tolerance. |
| Ordinary (1.250) shown as a reference value | Treat it as supplementary information. Find the controlling dimensions for production or acceptance. |
A surface can have size or location dimensions and a separate geometric control or texture requirement. Passing the dimensional limits does not exempt the geometric check. Similarly, a locally specified surface finish cannot be inferred from the number of decimal places in a nearby size. Read all applicable requirements and notes attached to the relevant features. If the tolerance for a needed dimension is ambiguous or missing, resolve the drawing before assuming a default.
Worked revision and limit check
A released inch drawing shows a 2.000 in overall width governed by its .XXX general tolerance of ±0.005 in. It also shows the width of a locating slot as 0.500 +0.004 / −0.000 in. A boxed dimension of 0.750 in locates the slot relative to the controlling reference, with a separate geometric frame. A parenthesized dimension illustrates the remaining space.
Calculate 1.995 to 2.005 in for the overall width and 0.500 to 0.504 in for the slot size. An overall width of 2.004 in meets the dimensional range. A slot measuring 0.498 in fails the local limits even though the difference from nominal, 0.002 in, would fit the block tolerance if wrongly applied. Slot location is a separate comparison to the relevant geometric control. The parenthesized value cannot overturn a failing required measurement.
Now suppose the released change tightens the slot size to 0.500–0.502 in. The earlier widest accepted slot can now be oversized under the new drawing. Before taking the same cut, check tool wear allowance, process capability and inspection equipment. Save the correct program and inspection revision with the work order. When reviewing a discrepant part, retain the traceability needed to identify which definition and measurement applied.
Keep the reference with the inspection result
Record the feature, units and specified limits in the inspection handoff when the plan requires them. Measure with suitable equipment for the feature and tolerance, and use the applicable rules for decisions close to a specification limit. A nominal coordinate can be reproduced from a controlled model, but a print image may have been resized. Use the documented value and datum structure rather than scaling the page.
ASME Y14.35 revisions, ASME Y14.5 dimensioning and tolerancing and NASA controlled drawing practices
The released drawing for a job is revision C, but the available CNC setup sheet was approved against revision B. What should happen first?
Use the old sheet if the part number matches
Confirm the controlled changes and verify which program, setup and inspection plan are authorized for revision C
Use the most recent looking file without checking its issue
Change only the revision text on the old sheet
An inch drawing gives 1.250 without a local tolerance, and an applicable note says .XXX ±0.005 in. What range applies?
1.250 to 1.255 in
1.200 to 1.300 in
1.245 to 1.255 in
1.249 to 1.251 in
The applicable block tolerance is ±0.005 in, but the local limits for a slot are 0.500 to 0.502 in. The slot measures 0.504 in. How does it compare?
It is within the slot limits
It would pass if the geometric position is within tolerance
It is under the local minimum
It is above the local maximum
A boxed 0.750 defines the nominal location for a hole with a position frame. How do you interpret the box?
It gives the basic location, with permissible variation set by the associated geometric tolerance
It is a supplementary reference dimension only
It gets the same plus/minus default as any other .XXX dimension
It is the hole’s maximum permitted diameter
Sections you finish are checked off in the contents.