The reasons for this transition include the cost of:

These costs are greatly reduced by using a globally recognized standard. The challenge for the corporation is to select a standard that is adequate for their applications and demographics. Many companies are being forced to use ISO standards across the board. There seems to be an assumption that anything ISO is good. Unfortunately, not all ISO standards are mature. This is certainly true in the area of dimensioning and tolerancing. Those being required to adopt the ISO standards for dimensioning and tolerancing should thoroughly understand their current state, direction for the future and current limitations. When a company has only modest design requirements, there is sufficient overlap in the ASME Y14.5 and ISO standards to adequately define undemanding parts. For more complex applications committing to the ASME Y14.5 standard or creating a corporate addendum, which supplements either the ISO or ASME, standards may be required.

Several factors need to be considered when choosing a direction for your company's standard. This matrix illustrates many of these factors.

Whether using ASME Y14.5M-1994 or the ISO standards, you can specify most GD&T requirements while not violating either standard. Here are a few guidelines to follow.

Rules:
All geometric tolerances apply regardless of feature size. The maximum material and least material modifiers may be used as desired and where appropriate.
 
Datums:
The most recent version of the Y14.5 standard agrees with ISO in datum identification and meaning. An exception is the application of a datum triangle in a side view of a cylinder. The Y14.5 standard does not illustrate this option. ISO states that the datum is a line tangent to the feature unless the triangle is in line with the size dimension. In either case, datums are used to establish origins of measurement and arrest the six degrees of freedom.

The current standards reflect the way mating parts contact one another. Caution, the new ISO draft would change the definition of a datum to be a mathematical derivation of the actual feature using a least squares algorithm.
 
Form:
For all intents and purposes, flatness, straightness, circularity and cylindricity are identical in both standards. All points of the surface must lie inside the form tolerance. In order to properly inspect a feature, the inspector would have to use an infinitely small indicator or subtract the uncertainty, resulting from surface roughness, from the allowable form tolerance. There is a draft of the ISO standard that would exclude surface roughness from form controls. If this revision were approved, the definitions for form would not agree.
 
Orientation:
The standards are consistent for perpendicularity, parallelism and angularity.
 
Profile of a Surface:
Simple profile is the essentially same for the two standards. The Y14.5 standard uses profile of a surface to locate flat surfaces as well as contours. ISO traditionally uses position to locate flat surfaces and profile of a surface is used for contours. ISO does not prohibit locating plane surfaces with profile of a surface. There is a move towards minimally dimensioned drawings, making the CAD file BASIC and using a general profile of a surface tolerances to control features unless otherwise specified. This does not violate either current standard. The corner condition of the tolerance zone is not identical.
The concept of composite profile is not found in ISO.

Position:
Position may be used to locate features of size in ISO and Y14.5.
Although composite position is shown in ISO, it is not well developed.
 
Runout:
The circular and total runout definitions are consistent. Both standards default to the indicator being oriented normal to the feature being controlled. ISO allows dimensioning the angle at which an indicator may be oriented relative to the surface.
 
Major differences that exist between the two standards include:
Definition of size:
The Y14.5 standard defaults to the Envelope Principle, which provides the control of form when features are inspected correctly. ISO requires that either the Envelope symbol be placed next to the size dimension or individual form controls be specified.

General and title block tolerances:
Most US companies continue to specify general tolerances in a schedule based on the number of decimal places specified on the dimension. This often requires adding trailing zeros to indicate a tighter tolerance. Adding trailing zeros violates ISO and ASME metric dimensioning standards. ISO uses tolerance grades and a letter to indicate position of the tolerance with respect to the basic (not the same basic used for geometric controls) dimension.

Using general tolerances that apply to locating dimensions have four inherent problems. These problems are:

The next drawing illustrates these four problems. Imagine trying to draw a shadowgraph to inspect the R30 on an optical comparator. The general tolerances do not relate to the datums shown on the part so you would be guessing at where to start. Also, since the 50 and the 75 dimensions would use the +0.2 general tolerance, it is not clear where the center of the R30 is. Anyone who has ever tried to inspect a part such as this will tell you that once the part is produced, it is virtually impossible to reproducibly measure the R30 value and its location. Again, once you have the part in your hand, try to determine what origin to use when measuring the 45° angled surface.

These problems may be overcome by using general geometric tolerances to locate features. By using a general profile tolerance, the tolerances apply to the surface of the part, something you can touch. General + tolerances are often to imaginary points in space.

ISO 2768 invokes a set of general tolerances based on a study of common machine shop practices. If the part does not meet these general tolerances, the part might still be accepted if it seems to work in its' function. This approach may work in Europe, but with our present requirements for Cp and Cpk, it would never fly. Avoid referencing this standard.
 
Coplanarity:
ISO uses flatness and the term "common zone" to control coplanarity.

Locating plane surfaces
Y14.5 uses profile of a surface to locate planes. Although ISO does not disallow using profile of a surface to locate planes, traditionally position is used. In Y14.5, position may only be used to locate features of size and bounded features such as hex, square and 'D' shaped holes. As mentioned earlier, the ISO definition of a profile of a surface tolerance zone creates a rounded corner condition while Y14.5 creates a sharp corner condition.
 
Concentricity and symmetry
Y14.5 requires that all derived median points must be within the specified tolerance for concentricity and symmetry. This makes inspection very time consuming and should be avoided. ISO's definitions of concentricity and symmetry are identical to the Y14.5 definition of position for features shown coaxial or symmetric. Also, ISO permits the use of maximum material and least material for concentricity and symmetry whereas Y14.5 does not.
 
Additional differences in ISO
ISO as yet does not have symbols for all around, between, controlled radius, counterbore, countersink, depth, statistical tolerance and tangent plane. ISO does not include axis or center plane straightness, composite profile and a mathematically defined datum feature. Datum referencing with position is optional. Ambiguous order of datums is permitted in datum referencing if no vertical lines are present in the feature control frame where datums are referenced. Target lines use different symbology. Angular tolerances do not include form control. A leader when specifying a datum feature or geometric tolerance may indicate a centerline. Numbers are separated from decimal fractions by a comma. The application of geometric tolerances to threads is not defined in ISO. First angle projection is the default in ISO whereas the ASME standards default to third angle projection. The definition of composite does not agree in the two standards.
 
Conclusion
The ASME Y14.5 standard continues to be the most comprehensive standard for dimensioning and tolerancing in the world. It is globally recognized and is being translated into other languages as the need arises. Its mathematical definition is used as a basis for coordinate measuring machine and tolerance analysis software. If for political reasons your company is forced to use the ISO standards for dimensioning and tolerancing, consider creating a corporate addendum to help make the ISO standards useable.

Abstract
Today, most manufacturing companies are abandoning their corporate standards on dimensioning and tolerancing in favor of internationally recognized standards. The two major choices in standards today are the Collection of ISO standards or ASME Y14.5M-1994. This presentation will look at the common ground and differences between ISO and ASME and identify topics to include in a corporate addendum. Economic application of tolerances, inspection methods and simultaneous engineering through GD&T will be emphasized.