Programming parameter changes

There are many parameters that affect the way a CNC machine executes a program. In many cases, one appropriate setting for the parameter will work for an entire program. Indeed, many such parameters will work for all of the programs a company runs.

For example, with the machining center G73 chip-breaking peck-drilling cycle, a parameter controls how far the tool will retract between pecks. A setting of from 0.002 to 0.005 inch will cause the chip to break. And once this parameter is set, there will be no further need to change it.

There are other program-related parameters that may need changing from time to time. With the machining center G83 deep-hole peck-drilling cycle, for example, a parameter controls how far the drill will stay away from its last peck depth position. This distance is related to the material being machined.

Some companies set this parameter excessively. That is, they set it to a large value that will work for the worst case scenario – the material that most allows chips to fall back into the hole during retract. While this is safe, it may not be very efficient. Other companies reset the parameter for the material currently being machined.

In yet other applications, it may be necessary to change parameters even during the execution of a single program. With the turning center threading cycle on some controls, for example, parameters control the minimum depth-of-cut, the final depth-of-cut, and the number of spring passes. If machining two substantially different threads from within one program, the settings for one thread may not be appropriate for the other.

It’s nice to know that program-related parameters can be changed from within a CNC program using the G10 command. For parameters that need to be changed from time to time, and especially when parameters must be changed during a program’s execution, G10 will keep a setup person or operator from having to manually do so.

Here is an example of how G10 works for changing parameters.

  • .

  • .

  • .

  • G10 L50

  • N6218 R0030

  • N6219 R0002

  • N6220 R3

  • G11

  • .

  • .

  • .

The first command (G10 L50) sets the parameter entry mode. The N words specify specific parameter numbers and R words specify the parameter values. You must, of course, know the parameter number/s for the parameter/s you want to set and the related value/s. G11 tells the control to cancel the parameter entry mode.

In our example – and for the specific control model being shows (parameter numbers change for model to model), parameter number 6218 specifies the minimum depth-of-cut (0030 specifies 0.003 inch). Parameter number 6219 specifies the final pass depth (0002 specifies 0.0002 inch). Parameter number 6220 specifies the number of spring passes (three in our example)

41 views0 comments

Recent Posts

See All

Tapping on a turning center (without canned cycles)

Unless your Fanuc controlled turning center came with live tooling, it’s likely that you don’t have canned cycles (G80-G89) like those you find on machining centers. You might have G74 and G75, the mu

Can you speed up your tool change time?

Machining centers, of course, have automatic tool changing devices to automate the tool changing process. Current models boast very fast tool changing times and you may be quite satisfied with tool ch

cnc reverse logo.jpg

44 Little Cahill Road

Cary, IL  60013

Ph: 847-639-8847

  • Facebook Social Icon