I. The numerical relationship between dimensional tolerances, geometric tolerances, and surface roughness:
1. Numerical relationship between form tolerance and dimensional tolerance
Once the dimensional tolerance accuracy is determined, the form tolerance has a corresponding appropriate value. Generally, about 50% of the dimensional tolerance value is used as the form tolerance value; in the instrument industry, about 20% of the dimensional tolerance value is used as the form tolerance value; and in the heavy industry, about 70% of the dimensional tolerance value is used as the form tolerance value. Therefore, the higher the dimensional tolerance accuracy, the smaller the proportion of form tolerance in the dimensional tolerance. Thus, when designing and specifying dimensional and form tolerance requirements, except in special cases, once the dimensional accuracy is determined, generally 50% of the dimensional tolerance value is used as the form tolerance value. This is beneficial for both manufacturing and ensuring quality.
2. Numerical relationship between form tolerance and position tolerance
There is a certain relationship between form tolerances and position tolerances. From the perspective of the causes of error, form errors are caused by machine tool vibration, tool vibration, spindle runout, etc.; while position errors are caused by non-parallelism of machine tool guideways, non-parallel or non-perpendicular tool clamping, clamping force, etc. Furthermore, from the perspective of the tolerance zone definition, position error includes the form error of the measured surface; for example, parallelism error includes flatness error. Therefore, position error is much larger than form error. Thus, under normal circumstances, without further requirements, if a position tolerance is specified, a form tolerance is not specified. When there are special requirements, both form and position tolerances can be specified simultaneously, but the specified form tolerance value should be smaller than the specified position tolerance value; otherwise, the parts cannot be manufactured according to the design requirements during production.
3. Relationship between shape tolerance and surface roughness
Although there is no direct numerical or measurement relationship between shape error and surface roughness, a certain proportional relationship exists between the two under certain processing conditions. According to experimental studies, at general precision levels, surface roughness accounts for 1/5 to 1/4 of the shape tolerance. Therefore, to ensure shape tolerance, the maximum allowable value of the corresponding surface roughness height parameter should be appropriately limited.
Under normal circumstances, the tolerance values of dimensional tolerance, form tolerance, positional tolerance, and surface roughness have the following relationship: dimensional tolerance > positional tolerance > form tolerance > surface roughness (height parameter)
It is clear from the numerical relationships between dimensions, form and position, and surface roughness that the design process must coordinate these relationships. When marking tolerance values on drawings, the following should be followed: the surface roughness value of the same surface should be less than its form tolerance value; the form tolerance value should be less than its position tolerance value; and the positional tolerance values should be less than their dimensional tolerance values. Otherwise, it will cause various manufacturing problems. However, the most frequently involved aspect of design work is how to handle the relationship between dimensional tolerances and surface roughness, as well as the relationship between various fitting accuracies and surface roughness.
Generally, it is determined according to the following relationship:
1. When the form tolerance is 60% of the dimensional tolerance (medium relative geometric accuracy), Ra≤0.05IT;
2. When the form tolerance is 40% of the dimensional tolerance (higher relative geometric accuracy), Ra≤0.025IT;
3. When the form tolerance is 25% of the dimensional tolerance (high relative geometric accuracy), Ra≤0.012IT;
4. 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 reference value is that the dimensional tolerance should be 3-4 times the surface roughness, which is the most economical approach.
II. Selection of Geometric Tolerances
1. Selection of geometric tolerances
The function of comprehensive control projects should be fully utilized to reduce the number of geometric tolerance items and corresponding geometric error detection items given on drawings.
While meeting functional requirements, items that are easy to measure should be selected. For example, coaxiality tolerance is often replaced by radial runout tolerance. However, it should be noted that radial runout is a combination of coaxiality error and cylindrical surface shape error. Therefore, when replacing it, the runout tolerance value should be slightly larger than the coaxiality tolerance value; otherwise, the requirements will be too stringent.
2. Selection of tolerance principles
The function of tolerance should be fully utilized and the feasibility and economy of adopting the tolerance principle should be considered based on the functional requirements of the measured element.
The principle of independence is used when the requirements for dimensional accuracy and geometrical accuracy differ significantly and need to be met separately, or when the two are unrelated, to ensure motion accuracy, sealing, or when tolerances are not specified.
The inclusion requirement is mainly used in situations where strict guarantees of compatibility are required.
The maximum materiality requirement is used for central elements and is generally used when the requirement for accessories is assemblability (no mating requirements).
Minimum material requirements are mainly used in situations where it is necessary to ensure the strength of parts and the minimum wall thickness.
The combination of reversibility requirements and maximum (minimum) material requirements can fully utilize the tolerance zone, expand the range of actual dimensions of the measured feature, and improve efficiency. This method can be used without affecting performance.
3. Selection of benchmark elements
1) Selection of reference location
(1) Select the mating surface of the part in the machine as the reference part. For example, the bottom plane and side of the housing, the axis of the disc part, the support journal or support hole of the rotating part, etc.
(2) The reference element should have sufficient size and rigidity to ensure stable and reliable positioning. For example, using two or more axes that are far apart to form a common reference axis is more stable than using a single reference axis.
(3) Select a surface with relatively precise machining as the reference part.
(4) Try to unify the assembly, processing and inspection standards. This can eliminate errors caused by inconsistent standards and simplify the design and manufacture of fixtures and gauges, making measurement more convenient.
2) Determination of the baseline quantity
Generally, the number of datums should be determined based on the orientation and positioning geometric requirements of the tolerance item. Orientation tolerances mostly require only one datum, while positioning tolerances require one or more datums. For example, for parallelism, perpendicularity, and coaxiality tolerance items, generally only one plane or one axis is used as the datum element; for position tolerance items, it is necessary to determine the positional accuracy of the hole system, which may require two or three datum elements.
3) Arrangement of the baseline order
When selecting two or more datum elements, the order of the datum elements must be clearly defined and written in the tolerance frame in the order of first, second, and third. The first datum element is the primary one, and the second datum element is secondary.
4. Selection of geometric tolerance values
The general principle is to select the most economical tolerance value while ensuring the functionality of the part.
◆Based on the functional requirements of the parts, and considering the economics of machining as well as the structure and rigidity of the parts, determine the tolerance values of the elements according to the table. Also consider the following factors:
◆The shape tolerance given for the same element should be less than the position tolerance value;
◆The form tolerance (excluding the straightness of the axis) of cylindrical parts should be less than its dimensional tolerance; if on the same plane, the flatness tolerance should be less than the parallelism tolerance of the plane to the datum.
◆The parallelism tolerance value should be less than its 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.
◆For the following situations, considering the ease of machining and the influence of factors other than the main parameters, while meeting the functional requirements of the part, the selection level should be appropriately reduced by 1 to 2 levels:
○ The hole is relative to the shaft;
○ Slender shafts and holes with relatively large dimensions; shafts and holes with large distances between them;
○ Surfaces of parts with a large width (greater than 1/2 of their length);
○ Parallelism and perpendicularity tolerances between lines and between lines and opposite sides relative to face-to-face.
5. Regulations for unspecified geometric tolerances
To simplify drafting, for geometrical and positional accuracy that can be guaranteed by general machine tool processing, it is not necessary to indicate geometrical and positional tolerances on the drawing. Geometrical and positional tolerances without indication shall be performed in accordance with the provisions of GB/T1184-1996. The general content is as follows:
(1) Three tolerance grades, H, K and L, are specified for straightness, flatness, perpendicularity, symmetry and circular runout that are not specified.
(2) The unspecified roundness tolerance is equal to the diameter tolerance, but cannot be greater than the unspecified radial runout tolerance.
(3) The unspecified cylindricity tolerance value is not specified and is controlled by the specified or unspecified tolerances of the element's roundness tolerance, straightness of the generatrix, and parallelism of the relative generatrix.
(4) The unspecified parallelism tolerance value is equal to the larger of the dimensional tolerance between the measured feature and the datum feature and the unspecified form tolerance (straightness or flatness) of the measured feature, and the longer of the two features is taken as the datum.
(5) No coaxiality tolerance value is specified. If necessary, the unspecified coaxiality tolerance value may be equal to the unspecified circular runout tolerance value.
(6) The tolerance values of unspecified line profile, surface profile, inclination and position are all controlled by the specified or unspecified linear dimension tolerance or angular tolerance of each element.
(7) No tolerance value for total runout is specified.
6. Drawings without specified tolerance values
If unspecified tolerance values specified in GB/T1184-1996 are used, the standard and grade code should be indicated in the title block or technical requirements: “GB/T1184—K”.
If the drawing does not specify "tolerance principle according to GB/T4249", the working tolerance should be performed in accordance with the requirements of "GB/T1800.2-1998".
Disclaimer: This article is a reprint. If there are any copyright issues, please contact us promptly for deletion (QQ: 2737591964). We apologize for any inconvenience.
