Parameters Can Make Things Interesting
These function settings can cause identical machines with identical controls to behave differently.
Parameters control countless functions related to the way a given CNC machine tool behaves. Maximum spindle speed, rapid rate, pitch error compensation, communications protocol and backlash compensation are among the countless functions specified by parameters. Two identical machines with identical controls can exhibit dramatically different behaviors based on the way parameters are set.
First and foremost, it is imperative that you keep a backup copy of the parameters for each machine your company owns. I’ve made this point many times before, but it cannot be overstated. As the machine tool user, you—and only you—are responsible for keeping backup copies of parameters. Don’t expect the machine tool builder to do it nor the machine tool distributor who sold you the machine. Take charge and do this important task for yourself, and remember to make a backup copy whenever a parameter is changed.
Current FANUC control models make it easy. You can back up to a memory card, to a USB flash drive or to your company’s direct numerical control (DNC) system. You can even track revisions, having current controls automatically keep a copy of the most recent parameter settings when a parameter is changed (just in case you make a mistake during parameter entry). But this doesn’t protect you from a catastrophic failure. Nothing beats having a set of parameters on an external device when disaster strikes.
Let’s look at a few parameters that can cause identical machines to behave differently.
Decimal Point Non-Usage. Traditionally, new CNC controls tend to maintain compatibility with the old CNC controls. For example, old controls did not allow a decimal point to be used within CNC words. You had to program a fixed format for every word. In the imperial measurement system, an X word of X100000 specifies an X coordinate of 10 inches.
Controls made after about 1980 provide decimal-point programming. An X word of X10.0, of course, specifies an X coordinate of 10 inches. To maintain compatibility with very old machines, many (even new) controls will still interpret X100000 as an X coordinate of 10 inches.
I have always urged programmers to specify a decimal point in every CNC word that allows it. Doing so will ensure that the control will not misinterpret a value.
With current-model FANUC controls, a parameter controls how a real number value will be interpreted if the decimal point is omitted. With the 0iD control, it happens to be parameter number 3401, bit 0. If this parameter bit is set to zero, the control will behave in the traditional manner. In the imperial measurement system, the word X10 will be interpreted as X0.0010. If this parameter bit is set to the number one, however, the control will interpret X10 as X10.0 (10 inches).
If your company owns only new machines that allow this capability, it may make sense to you to take advantage of this new method, setting parameters so that X10 is taken as X10.0. But if your company also owns older machines that behave in the traditional manner, and if programs will be shared among old and new machines, you must be concerned with compatibility issues. It may be wiser to assume decimal-point placement using the older, fixed format. Either way, I still recommend explicitly specifying a decimal point in every CNC word that allows it.
Initialized States Parameters. Certain G codes are automatically executed when the machine’s power is turned on, and you may depend on the control to be in its initialized state when you run a program. If you do, you must ensure that the related parameters are set the same for all of the machines your company owns. Examples include measurement system choice (G20 imperial or G21 metric), absolute or incremental positioning mode (G90 absolute or G91 incremental for machining centers), and federate mode (G98 per minute or G99 per revolution for turning centers).
Canned Cycle Parameters. Parameters control several functions related to how canned cycles behave. Consider, for example, the G73 chip-break peck drilling cycle. A parameter (number 5114 on FANUC 0iD) controls how far the drill will retract (breaking the chip) between pecks. It should be set to a value of about 0.005 inch (about 0.13 mm). As you can imagine, this parameter setting can affect cycle time, since, after each peck, the drill must feed by this amount before it begins cutting again. You could have two identical machines that have identical controls running the same program but experiencing different cycle times. The machine that takes longer may have this parameter excessively set.
The same is true for the G83 deep-hole peck drilling cycle. A parameter controls how far the drill will stay away from previously machined depths during each pass. This parameter (number 5115 on FANUC 0iD) should be set to about 0.05 inch. Excessive setting could cause wasted cycle time.
Here is a list of websites I frequently use to solve CNC-related problems and learn more about the subject.
Tolerances of less than 25 microns can be challenging to achieve and hold. Here are some suggestions for holding them for multiple workpieces.
A custom-macro-based system can predict when a tool will become dull.