Proper coordination of dimensional tolerances, geometric tolerances, and surface roughness is essential for ensuring part accuracy, assembly performance, and manufacturing efficiency.
By applying appropriate tolerance principles, designers can optimize product quality.
They can achieve this by selecting suitable reference features and following established standards for tolerance specification.
These practices also help minimize production costs and reduce inspection complexity.
Relationship Between Geometric Tolerances and Surface Roughness
Although there is no direct numerical or measurement-based relationship between form error and surface roughness, a certain proportional relationship exists between the two under specific machining conditions.
According to experimental studies, at general precision levels, surface roughness accounts for 1/5 to 1/4 of the form tolerance.
To ensure compliance with form tolerance, manufacturers should appropriately limit the maximum allowable values of the corresponding surface roughness height parameters.
Generally, dimensional tolerance, form tolerance, positional tolerance, and surface roughness are related.
The following equation expresses their relationship:
Dimensional tolerance > Positional tolerance > Form tolerance > Surface roughness height parameter.
As can be easily seen from the numerical relationships among dimensions, geometric tolerances, and surface roughness, it is essential to properly coordinate these three factors during the design process.
When specifying tolerance values on drawings, designers should follow the following principle: the surface roughness value specified for a given surface should be less than its geometric tolerance value.
The geometric tolerance value should be less than its positional tolerance value;
And each positional tolerance value should be less than its dimensional tolerance value.
Failure to do so will lead to various manufacturing complications.
However, the most common issues encountered in design work involve tolerance allocation.
These issues include determining how to handle the relationship between dimensional tolerances and surface roughness.
They also involve establishing the relationship between various fit tolerances and surface roughness.
Generally, the following relationships apply:
- When the form tolerance is 60% of the dimensional tolerance (medium relative geometric accuracy), Ra ≤ 0.05IT;
- When the form tolerance is 40% of the dimensional tolerance (high relative geometric accuracy), Ra ≤ 0.025IT;
- When the form tolerance is 25% of the dimensional tolerance (high relative geometric accuracy), Ra ≤ 0.012IT;
- When the form tolerance is less than 25% of the dimensional tolerance (ultra-high relative geometric accuracy), Ra ≤ 0.15Tf (form tolerance value).
The simplest guideline: the dimensional tolerance should be 3–4 times the surface roughness value; this is the most cost-effective approach.
Selection of Geometric Tolerances
Selection of Geometric Tolerance Items
Designers should make full use of comprehensive control items to reduce the number of geometric tolerance items specified on drawings and the corresponding geometric error inspection items.
Provided that the functional requirements are satisfied, designers should select items that are easy to measure.
For example, designers often replace coaxiality tolerances with radial runout tolerances.
However, designers should note that radial runout combines coaxiality error and cylindrical surface form error.
Therefore, when substituting, the specified runout tolerance value should be slightly greater than the coaxiality tolerance value, otherwise the requirements will be too stringent.
Selection of Tolerance Principles
Designers should base the selection on the functional requirements of the feature being measured.
It should fully leverage the role of tolerances while considering the feasibility and cost-effectiveness of adopting a particular tolerance principle.
The independent principle is used when there is a significant difference between dimensional accuracy and geometric accuracy requirements, necessitating separate compliance;
Designers should apply the independent principle when the two are unrelated and in cases involving motion accuracy, sealing performance, or unspecified tolerances.
Engineers primarily use the inclusive principle in situations that require strict assurance of fit characteristics.
Designers use the maximum solid requirement for central features and generally apply it when parts must be assembly-compatible without specific fit requirements.
Engineers primarily use the minimum solid requirement in situations that require guaranteed part strength and minimum wall thickness.
Reversible requirements, when used in conjunction with maximum (or minimum) solid requirements, allow for full utilization of the tolerance zone.
They also expand the range of actual dimensions of the measured feature and improve efficiency.
Designers may select them provided they do not affect performance.
Selection of Reference Features
1. Selection of Reference Locations
(1) Select the mating surfaces used to position the part within the machine as reference locations.
Examples include the bottom and side surfaces of a housing, the axis of a disc-type part, or the support journal or support bore of a rotary part.
(2) Reference features should be of sufficient size and rigidity to ensure stable and reliable positioning.
For example, combining two or more axles spaced far apart to form a common reference axis is more stable than using a single reference axis.
(3) Designers should select surfaces that have been machined with high precision as reference locations.
(4) Unify the assembly, machining, and inspection references as much as possible.
This not only eliminates errors caused by inconsistent references but also simplifies the design and manufacture of fixtures and measuring tools, making measurement more convenient.
2. Determining the Number of Reference Elements
Generally, designers should determine the number of reference elements based on the orientation and positioning requirements of the tolerance items.
Orientation tolerances typically require only one reference element, while positioning tolerances require one or more reference elements.
For example, for parallelism, perpendicularity, and coaxiality tolerance items, generally only one plane or one axis is used as the reference element;
For positional tolerance items, designers may require two or three reference elements to determine the positional accuracy of a hole system.
3. Arranging the Order of Reference Elements
When selecting two or more reference elements, designers must clearly define their order and list them in the tolerance box as the primary, secondary, and tertiary reference elements.
The first reference element is the primary one, followed by the second.
Selection of Geometric Tolerance Values
General Principle: Select the most economical tolerance values while ensuring the part’s functionality.
◆ Based on the part’s functional requirements, taking into account manufacturing economy, part structure, and rigidity, determine the tolerance values for the features according to the table.
Also consider the following factors:
◆ The geometric tolerance specified for a given feature should be smaller than its positional tolerance;
◆ For cylindrical parts (except for the straightness of the axis), the form tolerance value should be smaller than the dimensional tolerance value;
For example, on the same plane, the flatness tolerance value should be smaller than the parallelism tolerance value of that plane relative to the datum.
◆ The parallelism tolerance value should be smaller than the corresponding distance tolerance value.
◆ Approximate proportional relationship between surface roughness and form tolerance: Generally, the Ra value of surface roughness can be taken as (20%–25%) of the form tolerance value.
◆In the following cases, designers may appropriately reduce the tolerance by one or two grades while still meeting the functional requirements of the part.
This adjustment should take into account the difficulty of machining and the influence of factors other than the primary parameters.
○Holes relative to shafts;
○Shafts and holes with a high slenderness ratio; shafts and holes with large distances between them;
○Part surfaces with large widths (greater than half the length);
○Parallelism and perpendicularity tolerances for line-to-line and line-to-surface relative to face-to-face tolerances.
Provisions for Unspecified Geometric Tolerances
To simplify drafting, designers need not specify geometric and positional tolerances on drawings if general machine tool processing can ensure them.
GB/T 1184-1996 governs unspecified geometric and positional tolerances. The general provisions are as follows:
(1) For unspecified straightness, flatness, perpendicularity, symmetry, and circular runout, three tolerance grades—H, K, and L—are specified.
(2) The unspecified roundness tolerance value is equal to the diameter tolerance value, but must not exceed the unspecified tolerance value for radial runout.
(3) The unspecified cylindricity tolerance value is not specified;
It is controlled by the specified or unspecified tolerances for the element’s roundness, generatrix straightness, and parallelism to the relative generatrix.
(4) The unspecified parallelism tolerance value is equal to the greater of two values.
These are the dimensional tolerance between the measured feature and the reference feature, and the unspecified form tolerance value (straightness or flatness) of the measured feature.
The longer of the two features serves as the reference.
(5) The standard does not specify an unspecified coaxiality tolerance value. If necessary, designers may use the unspecified circular runout tolerance value as the unspecified coaxiality tolerance value.
(6) The specified or unspecified linear dimensional tolerances or angular tolerances of the respective features control the unspecified tolerance values for line profile, surface profile, inclination, and positional tolerance.
These dimensional or angular tolerances determine the corresponding unspecified tolerance values.
(7) The standard does not specify an unspecified total runout tolerance value.
Representation of Dimensions and Geometric Features with Unspecified Tolerances in Drawings
If designers use the unspecified tolerance values defined in GB/T 1184-1996, they shall indicate the standard and grade code “GB/T 1184—K” in the title block or the technical requirements.
For working tolerances on drawings that do not specify “Tolerances shall be in accordance with GB/T 4249,” designers shall apply the requirements of GB/T 1800.2-1998.
Conclusion
Proper coordination of dimensional tolerances, geometric tolerances, and surface roughness is essential for ensuring part performance while maintaining manufacturing efficiency and cost-effectiveness.
By applying appropriate tolerance principles, selecting suitable datum features, and specifying economical tolerance values, designers can achieve reliable functionality, simplify inspection, and improve production quality.
Following established standards and best practices helps create accurate, practical, and manufacturable engineering drawings.