The relationship between dimensional tolerance, geometric tolerance and surface roughness
1. Relationship between shape tolerance and surface roughness
Although there is no direct relationship between shape error and surface roughness in terms of numerical value and measurement, there is a certain proportional relationship between the two under certain processing conditions. According to experimental research, under normal precision, surface roughness accounts for 1/5 to 1/4 of the shape tolerance. It can be seen from this that in order to ensure the shape tolerance, the maximum allowable value of the corresponding surface roughness height parameter should be appropriately limited.
In general, the tolerance values between dimensional tolerance, shape tolerance, position tolerance and surface roughness have the following relationship: dimensional tolerance > position tolerance > shape tolerance > surface roughness height parameter.
It is not difficult to see from the numerical relationship between size, shape and surface roughness that the numerical relationship between the three should be coordinated and handled well during design. When marking the tolerance value on the drawing, it should be followed that the roughness value of the given same surface should be less than its shape tolerance value; and the shape tolerance value should be less than its position tolerance value; and the position difference should be less than its dimensional tolerance value. Otherwise, it will bring various troubles to manufacturing. However, the most involved in design work is how to deal with the relationship between dimensional tolerance and surface roughness and the relationship between various matching precisions and surface roughness.
Generally, it is determined according to the following relationship:
1. When the shape tolerance is 60% of the size tolerance (medium relative geometric accuracy), Ra≤0.05IT;
2. When the shape tolerance is 40% of the size tolerance (high relative geometric accuracy), Ra≤0.025IT;
3. When the shape tolerance is 25% of the size tolerance (high relative geometric accuracy), Ra≤0.012IT;
4. When the shape tolerance is less than 25% of the size tolerance (ultra-high relative geometric accuracy), Ra≤0.15Tf (shape tolerance value).
The simplest reference value: the size tolerance is 3-4 times the roughness, which is the most economical.
2. Selection of geometric tolerances
1. Selection of geometric tolerance items
The functions of comprehensive control items should be fully utilized to reduce the geometric tolerance items and corresponding geometric error detection items given on the drawings.
On the premise of meeting the functional requirements, items that are easy to measure should be selected. For example, coaxiality tolerance is often replaced by radial runout tolerance or radial runout tolerance. However, it should be noted that radial runout is a combination of coaxiality error and cylindrical shape error. Therefore, when replacing, the runout tolerance value given should be slightly larger than the coaxiality tolerance value, otherwise it will be too strict.
2. Selection of tolerance principles
Based on the functional requirements of the measured elements, the functions of tolerances and the feasibility and economy of adopting the tolerance principle should be fully utilized.
The independent principle is used for occasions where the dimensional accuracy and geometric accuracy requirements are quite different and need to meet the requirements separately, or the two are not related, to ensure motion accuracy, sealing, and no tolerance is noted.
The inclusive requirement is mainly used for occasions where the matching properties need to be strictly guaranteed.
The maximum entity requirement is used for the central element, and is generally used in situations where the accessory requirement is assemblability (no matching property requirements).
The minimum entity requirement is mainly used in situations where it is necessary to ensure the strength of the part and the minimum wall thickness.
The reversibility requirement is used in conjunction with the maximum (minimum) entity requirement to make full use of the tolerance zone, expand the range of the actual size of the measured element, and improve efficiency. It can be selected without affecting the performance.
3. Selection of datum elements
1) Selection of datum parts
(1) Select the joint surface where the part is positioned in the machine as the datum part. For example, the bottom plane and side of the box, the axis of the disk-like parts, the support journal or support hole of the rotating part, etc.
(2) The datum 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 datum axis is more stable than using a single datum axis.
(3) Select a surface that is processed more accurately as the datum part.
- Try to unify the assembly, processing and inspection datums. In this way, errors caused by inconsistent datums can be eliminated, and the design and manufacture of fixtures and measuring tools can be simplified, making measurement more convenient.
2) Determination of the number of datums
Generally speaking, the number of datums should be determined according to the orientation and positioning geometric function requirements of the tolerance items. 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 a datum element; for position tolerance items, it is necessary to determine the position accuracy of the hole system, so two or three datum elements may be used.
3) Arrangement of datum order
When more than two datum elements are selected, the order of the datum elements must be clarified and written in the tolerance frame in the order of first, second, and third. The first datum element is the main one, and the second datum element is the second.
4. Selection of geometric tolerance values
General principle: Select the most economical tolerance value on the premise of meeting the function of the part.
According to the functional requirements of the part, consider the economy of processing and the structure and rigidity of the part, and determine the tolerance value of the element according to the table. And consider the following factors:
The shape tolerance given by the same element should be less than the position tolerance value;
The shape tolerance value of cylindrical parts (except the straightness of the axis) should be less than its size tolerance value; on the same plane, the flatness tolerance value should be less than the parallelism tolerance value of the plane to the datum.
The parallelism tolerance value should be less than its corresponding distance tolerance value.
The approximate proportional relationship between surface roughness and shape tolerance: Usually, the Ra value of surface roughness can be taken as (20%~25%) of the shape tolerance value.
For the following situations, considering the difficulty of processing and the influence of other factors other than the main parameters, under the condition of meeting the requirements of part function, appropriately reduce 1~2 levels to select:
Hole relative to shaft;
Slender and relatively large shaft and hole; Shaft and hole with large distance;
Part surface with large width (greater than 1/2 length);
Parallelism and perpendicularity tolerance of line to line and line to face to face.
5. Provisions for unindicated tolerances of form and position
In order to simplify drawing, it is not necessary to indicate form and position tolerances on the drawing for form and position accuracy that can be guaranteed by general machine tool processing. The unindicated tolerances of form and position shall be implemented in accordance with the provisions of GB/T1184-1996. The general contents are as follows:
(1) Three tolerance grades of H, K and L are specified for unindicated straightness, flatness, perpendicularity, symmetry and circular runout.
(2) The unindicated roundness tolerance value is equal to the diameter tolerance value, but cannot be greater than the unindicated tolerance value of radial circular runout.
(3) The unindicated cylindricity tolerance value is not specified and is controlled by the indicated or unindicated tolerances of the element's roundness tolerance, element straightness and relative element parallelism.
(4) The unindicated parallelism tolerance value is equal to the larger of the dimensional tolerance between the measured element and the reference element and the unindicated tolerance value of the shape tolerance (straightness or flatness) of the measured element, and the longer of the two elements is taken as the reference.
(5) The unspecified coaxiality tolerance value is not specified. If necessary, the unspecified coaxiality tolerance value can be taken as equal to the unspecified circular runout tolerance.
(6) The unspecified linear profile, surface profile, inclination, and position tolerance values are all controlled by the specified or unspecified linear dimension tolerance or angle tolerance of each element.
(7) The unspecified total runout tolerance value is not specified.
6. Drawing representation of unspecified geometric tolerance values
If the unspecified tolerance values specified in GB/T1184-1996 are used, the standard and grade code should be indicated in the title bar or technical requirements.
: "GB/T1184-K".
Working tolerances that are not marked with "Tolerance principles in accordance with GB/T 4249" on the drawing should be implemented in accordance with the requirements of "GB/T 1800.2-1998".