Reducing a CNC’s Least Input Increment Value
If you work in the imperial (inch) measurement system, reducing the least input increment can help you hold size for workpiece attributes with small tolerances.
I have often said that working in the metric measurement system provides a better resolution for sizing (offset) adjustments than the imperial measurement system. My reasoning is based on the size of the least input increment in each measurement system. In metric, the least input increment that can be entered into an offset is typically one micron (0.001 mm). In imperial, it is typically one ten-thousandth of an inch (0.0001 inch). One micron is less than half of one ten-thousandth of an inch (a micron is equivalent to 0.000039 inch), hence the better resolution.
Consider an overall tolerance of 0.001 inch. With the imperial system, there will be fewer than 10 offset adjustment values that will make the workpiece attribute come out within its tolerance band (and each step is 10 percent of the tolerance band). But with metric, there are 25 adjustment values that will work (and each step is now only 4 percent of the tolerance band). This is especially important with very small tolerances. With a tolerance of 0.0004 inch, there are only three appropriate adjustment values with the imperial measurement system. With metric, there are 10.
Today’s CNCs boast amazing resolution. Internal to the CNC drive system, resolution is often stated in nanometers (billionths of a meter). Even so, most applications for CNC, especially those related to turning and milling, do not require (nor can they achieve) this level of accuracy. Though this is the case, the imperial system’s four-place least input increment (again 0.0001 inch) is rather coarse for many milling and turning applications. Many CNC users are unaware of the potential for improvement.
I compare this to having a one-degree indexer but thinking it is a five-degree indexer. If you never have applications that require indexing to positions smaller than five degrees, you will be happy. But if you do have applications that require a smaller index amount, not knowing that your indexer has a finer resolution will be an issue. In similar fashion, if you never need offset entry resolution smaller than 0.0001 inch (you have no tolerances smaller than 0.001 inch or so), you’ll be happy with the standard offset resolution. But if you work with very small tolerances of less than about 0.001 inch, you can definitely benefit by reducing the least input increment for offset adjustments.
In essence, you can improve the least input increment by one decimal place. For the imperial measurement system, this means the least input increment can be reduced to 0.00001 inch. (With metric, the least input increment will become 0.0001 mm, which means that metric mode still provides a better resolution.)
Changing the least input increment for offset entries with most current CNCs can be done with a parameter change. FANUC specifies this function as simply “Increment System.” Increment System A provides 0.01 mm or 0.001 inch (much too coarse for milling and turning applications). Increment System B, which most machine tool builders set by default, provides 0.001 mm or 0.0001 inch. Increment System C, which is what I’m recommending if you must hold very small tolerances, provides 0.0001 mm or 0.00001 inch.
As with many CNC functions, the parameters related to offset increment systems vary among control models. For a FANUC 0iD control, for example, it happens to be bits one and zero (the two right-most bits) of parameter number 5042. When both bits are set to zero, Increment System B is being selected. Again, this is probably how parameter number 5042 is currently set for your machining centers and turning centers.
To switch to Increment System C (again, with a 0iD control), set bit number one of parameter number 5042 to a value of one (leave bit number zero set to zero). The CNC will likely require you to turn off the power after doing so. After you power back up, check the offset page. Each register will now have five decimal places in the imperial system G20 mode (instead of four).
Note that this parameter only affects offset registers (geometry and wear, as well as workpiece coordinate system offsets). Another parameter controls the increment system for axis-position displays, which, with an 0iD control, is parameter number 1013. This parameter includes one set of registers for each linear axis. With a two-axis turning center, for example, there will be two sets of registers for the parameter, one for X and one for Z.
As with the offset-related parameter, the last two digits for each register set select the desired increment system. To make all axis displays show five places to the right of the decimal point (when the machine is in the imperial measurement system) set bit one of parameter 1013 to a value of one, leaving bit zero set to zero, for all linear axis sets of registers (again, X and Z for a turning center, or X, Y and Z for a machining center). As with the offset-related parameter, you will have to restart the machine to make this parameter change effective. When you do, all axis displays will show five places to the right of the decimal point in the imperial measurement system mode.
While the mistakes listed here will not sound an alarm or cause a program to fail, they will cause confusion, wasted time and scrap parts.
These subjects are the building blocks of training newcomers on a specific CNC machine tool.
They offer benefits that many CNC users overlook.