top of page
Search

# Which mode is better, inch or metric?

Most companies work exclusively in one mode or the other. If the bulk of their prints are dimensioned in inch (as with most companies in the United States), they program and run the machine in the inch mode. If they happen across a print dimensioned in the metric mode, they convert all dimensions to inch (by dividing all millimeter values by 25.4) and still work in the inch mode.

If you are one of the many companies that still work exclusively in the inch mode, you probably don't know about the accuracy advantage of the metric mode. This advantage has to do with the least input increment of the input mode. The least input increment in the inch mode for the vast majority of CNC machines is 0.0001 in. In the metric mode, the least input increment for these machines is 0.001 mm. 0.001 mm is less than half of 0.0001 in (0.001 mm is equivalent to 0.000039 in), meaning your CNC machine will have a much finer resolution when the metric mode is selected.

To get an understanding of this implication, consider a common indexer. A five degree indexer has 72 positions (360 divided by 5). A one degree indexer has 360 positions. Though the one degree indexer is no more accurate than the five degree indexer, you can program it with a finer resolution. You can, of course, index 34 degrees with a one degree indexer and cannot with a five degree indexer. One way to compare this to the inch/metric mode selection is to say that working exclusively in the inch mode when the metric mode is available is like having a one degree indexer but only programming it in five degree increments!

Said another way, a ten inch long linear axis has 100,000 programmable positions in the inch mode. In the metric mode, the same ten inch long axis has over 254,000 programmable positions!

### When can this help?

If the bulk of your work has wide-open tolerances, it is likely that the inch mode will more than suffice. It would be like saying you happen to have a one degree indexer but never have to program it to any finer resolution than five degrees. However, as tolerances get tighter, there are times when you can successfully machine workpieces in the metric mode when you cannot in the inch mode.

Consider how you calculate coordinates in your CNC program. Most programmers will program the mean value for dimensions. For example, if you have a dimension of 3.000 plus or minus 0.001 in, the programmed value will be 3.000. In the case of plus or minus tolerances, determining the mean value is easy and can be easily programmed.

On the other hand, consider a dimension of 3.0000 plus 0.0003, minus nothing. In this case, the mean value is 3.00015. If working in the inch mode (with only four place input), you cannot even program the mean dimension. If you convert 3.00015 in to metric, it comes out to 76.2038 mm, which must be rounded to 76.204. This dimension is within 0.0002 mm (0.0000078 in) of the desired mean value!

This accuracy advantage of the metric mode is also involved with offset setting. A tolerance of plus or minus 0.0002 in has less than four acceptable offset setting positions. The same tolerance in the metric mode is plus or minus 0.005 mm, which allows ten acceptable positions in the offset table! And for SPC purposes, the amount of offset change from one adjustment to the next can be kept smaller.

While people who have never worked in metric mode will find the transition a little cumbersome, if you do tight tolerance work, these accuracy benefits are well worth the effort. In many cases, you'll be able to hold size (or make less scrap) on workpieces that have been previously impossible to machine on CNC machine tools!

## Recent Posts

See All

Actually, the choice between whether the Imperial measurement system or the Metric measurement system is initialized can be done on the Setting display screen page (though it is also a parameter setti

G66 is one of the more misunderstood custom macro B commands. Fanuc calls it a modal custom macro call. It looks just like a G65 command. Consider these two commands: N045 G65 P1000 X3.0 Y3.0 Z0 A45.0

Current model CNC controls make it easy to create circular commands. You simply specify the direction (G02: clockwise or G03: counter clockwise), the end point (usually X and Y), and the radius (with

bottom of page