Tolerancing
Tolerancing is an essential element in design specification and engineering drawing. It is quoted in both ISO Geometrical Product Specifications (GPS) and ANSI Y 14.5 Geometric Dimensioning and Tolerancing (GD&T) standard but with different emphasis.
Tolerancing is more than a notation requirement on drawing practice, it’s also one of the parameters which formulate functional requirement. There are two important basic ISO GPS standards: ISO 8015 “Fundamentals-Concepts, principles and rules”and ISO 14638 “Matrix model”. These two standards outline the scope of tolerances within GPS and the relationship between the limits of functions and tolerances. The aim of GPS is to develop a common language to specify macrogeometry (size, form, orientation, location) and microgeometry (surface texture) of products or part of products so that it can be used consistent all over the world. Although in ANSI Y14.5 series there are also some similar standards like ANSI B4.2 Preferred Metric Limits and Fits, we will focus on tolerancing principles defined in GPS.
ISO 286 — ISO code system for tolerances on linear sizes
In general, there would be four types of tolerances: size tolerance, form tolerance, positioning tolerance and surface texture tolerance in GPS. Geometrical requirements have historically been defined by zones. This works well for the function of fit to ensure assemblability, but does not lend itself well to the expression of other functional requirements. We can learn this evolution from ISO 286 revision traits.
In the Scope of ISO 286–1, it states clearly “This part of ISO 286 establishes the ISO code system for tolerances to be used for linear sizes of features of the following types: a) cylinder; b) two parallel opposite surfaces”.
ISO 286:1988 was named as “ISO system of limits and fits” and its Annex A “Bases of the ISO system of limits and fits” was no longer available since 2010 edition. In order to understand inherited international tolerance grade today, it’s recommended to have an overview of this archived chapter.
Annex A “Bases of the ISO system of limits and fits”(1988)
For conveniene, the standard tolerance and fundamental deviations are not calculated individually for each separate basic size, but for steps of basic size. The values of the standard tolerances and fundametal deviations for each basic size step are calculated from the geometrical mean (D) of the extreme sizes (D1 and D2) of that step as shown:
D=(D1*D2)1/2
For the first basic size step (less than or equal to 3mm), the geometrical mean, D, according to convention, is taken between sizes 1 and 3mm, therefore D=1.732mm.
The ISO system of limits and fits provides for 20 standard tolerance grades designated IT01, IT0, IT1, …,IT18 in the size from 0 up to 500mm (incl.), and 18 standard tolerance grades in the size range from 500mm up to 3,150mm (incl.), designated from IT1 to IT18.
The system was not developed from a coherent mathematical base, and hence there are discontinuities in the system and differing formulae for the deviation of IT grades up to 500mm.
The values of standard tolerances for basic sizes from 500mm up to 3,150mm (incl.) were subsequently developed for experimental purposes, and since they have proved acceptable to industry they are now given as a part of the ISO system.
Standard tolerance grades IT01 to IT4
The values of standard tolerances in grades IT01, IT0, IT1 were calculated from the formulae in below table. It should be noted that no formulae were given for IT2 , IT3 and IT4 . The values for tolerances in these grades have been approximately scaled in geometrical progression between the values in IT1 and IT5.
Standard tolerance grades IT5 to IT18
The values of standard tolerances in grades IT5 to IT18 for basic sizes up to and including 500mm were determined as a function of standard tolerance factor, i.
i=0.45D1/3+0.001D
where D is in mm mentioned in previous section.
The formula was empirically derived, being based on various national practices and on the premise that, for the same manufacturing process, the relationship between the magnitude of the manufacturing errors and the basic size approximates a parabolic function.
The values of the standard tolerances were calculated in terms of the standard tolerance factor, i, as shown in table below.
It should be noted that from IT6 upwards, the standard tolerances were multiplied by a factor of 10 at each fifth step. This rule applied to all standard tolerances and might be used to extrapolate values for IT grades above IT18.
And deviation of standard tolerances (IT) for basic sizes from 500mm up to and including 3,150mm was factor I, in micrometers, which was calculated from the following formula:
I=0.004D+2.1
where D is the geometrical mean of the basic size step in millimeters.
And the complete IT codes table in ISO-286 is shown below:
ISO 14405–1 -Dimensional Tolerancing-Part1: Linear sizes
This GPS standard is more and compatible to ANSI Y 14.5 by defining tolerances of linear sizes in a conventional way like a + and/or − limit deviation (e.g. 0/−0,019). and also an ISO tolerance class code in accordance with ISO 286‑1 (e.g. 10 h6).
“Envelope Principle” (Taylor Principle) from ISO 14405–1
As there is a “Independency Principle” (section 5.5) in ISO 8015 states
“By default, every GPS specification for a feature or relation between features shall be fulfilled independent of other specifications except when it is stated in a standard or by special indication (e.g. Ⓜ modifiers according to ISO 2692, CZ according to ISO 1101 or Ⓔ modifiers according to ISO 14405–1) as part of the actual specification.” , so if this modifiers Ⓔ applies then it indicates the size tolerance limits of a part control the maximum variation of the form of a part.
ISO 2768–1 and 2768–2 (replaced by 22081:2021)
ISO 2768–1 is intended to simplify drawing indications and it specifies general tolerances for linear and angular dimensions without individual tolerance indications in four tolerance classes (f-fine, m-medium, c-coase, v-very coase). In general, if tolerances in accordance with ISO 2768–1 shall apply, information like “ISO 2768-m” shall be indicated in or near title block. However, now ISO 22081:2021 has been part of GPS set so the scope has been aligned with other GPS and no longer just a series of tables only. For original ISO 2768–2 tables, please refer to this article.
DIN 16901/16742 and ISO 20457: 2018 Plastics molded parts — Tolerances and acceptance conditions
Molding injection plastic parts show significant larger deviations with respect to dimension, form and location compared with metal parts, and considering the application of which plastics are by their properties, less accuracy would be required so the tolearnce applicable for metal parts can’t be adopted and a few separate documents are developed.
DIN 16901 was replaced by DIN16742/ISO 20457 as new plastic materials were keeping developed so rather than listing all materials the new standards asked a series questions to find out vairous properties of material you are going to use. But in addition to that, you still need to know the mold dependency dimenisions by denoting W or NW in new standards like A or B in original DIN 16901. And the production conditions for different accuracy need is considered.
There is an overview blog for detail.
DIN 16742/ISO 20457 Table 2 would be very similar to Table 2 of DIN 16901 but with different tolerance group notation. And you can find the table 2 and table 9 here.
The mission of GLInB is to bring most value by virtualization of your supply chain quality function to fit for challenges in today’s business environment.
Please visit us at http://www.glinb.com for more information.
