What Don’t you Like About that Canned Cycle?

Almost all CNC users take advantage of control-based canned cycles. Even CAM systems commonly output G-code programs that contain canned cycle commands. This includes hole machining canned cycles, such as drilling, tapping, boring and more, and whatever milling cycles the machine may have. For turning centers, it includes roughing and finishing multiple repetitive cycles.


Facebook Share Icon LinkedIn Share Icon Twitter Share Icon Share by EMail icon Print Icon


If you use canned cycles on a regular basis, you’ve probably come up with something about one or more of them that you don’t like. The more of these you use, the more likely there’s something you wish one of them would do differently.
Consider the G83 deep-hole, peck-drilling cycle. Will your control enable you to vary the depth of each peck so that it gets progressively shallower as the hole gets deeper? If you specify a total depth that is not evenly divisible by the peck depth, what happens? Can you control the rate at which the drill reenters the hole after each retract motion? 
When you think about it, you can surely come up with other canned cycle limitations you’d like to overcome. Maybe you wish your drilling cycle would begin the hole at one feed rate—possibly just enough to engage the drill—then machine the balance of the hole at a faster feed rate. Or, maybe you’d like a drilling cycle that would feed through one surface, then rapid to another and feed through it as well.
Does your control provide a canned cycle for the machining operation you need to perform? Maybe you’d like a grooving cycle for turning centers, a pocket milling cycle, a thread milling cycle or a face milling cycle. The potential list of improvements to canned cycles is lengthy.
With custom macro B, you can modify the function of canned cycles or create new ones. You can even make them behave in a modal manner and cancel them with a G80 word.
To achieve this, the custom macro must first be written in the normal manner to perform the machining operation in the fashion you want. The only consideration here will be the program number. If you want the custom macro to be activated by a G code, possibly the same G-code number that is currently being used for the canned cycle you don’t like, you must use a program number that will enable you to do so. Program number O9010 is the first in a series of ten program numbers that enable you to create a user-defined G code.
Once the custom macro is written and verified, it can be called with the standard custom macro calling G code, G65. However, to keep from modifying your current programs, you should call the custom macro using the same G code used to call the canned cycle your custom macro is replacing. To accomplish this, a parameter must be changed.
To find the parameters related to user-defined G codes (they vary from one control model to the next), you must reference the custom macro section of the control’s programming manual. Pick the first available one (currently set to zero), and change it to the G-code number you wish to use to call your custom macro. If you wish the calling G code to be modal, as hole machining canned cycles are, the value must be negative. For example, if parameter number 5061 is the parameter related to the first available user-defined G code program, and you want to change the way G83 behaves, change parameter number 5061 to -83. Again, be sure the program number for your program matches the one used by the parameter (such as O9010). The next time the control sees a G83, it will execute your custom macro instead of performing the normal function of G83.
To cancel your user-created canned cycle with G80, you must also modify the function of G80. Pick another user-defined G-code parameter, and place a value of 80 in it. Finally, match this program number with the program related to the parameter number. This will cancel normal canned cycles as well as your user-defined G code. If choosing the second-available, user-defined G code, the program number will be O9011 — and here it is:

O9011 G80 G67 M99

This program will cancel canned cycles as well as modal custom macro calls.


Related Topics


  • Machining Dry Is Worth A Try

    Reducing cutting fluid use offers the chance for considerable cost savings. Tool life may even improve.

  • Rigid Tapping--Sometimes You Need A Little Float

    One of the most common methods of tapping in use today on CNC machines is 'rigid tapping' or 'synchronous feed tapping.' A rigid tapping cycle synchronizes the machine spindle rotation and feed to match a specific thread pitch. Since the feed into the hole is synchronized, in theory a solid holder without any tension-compression can be used.

  • Non-Traditional Methods For Making Small Holes

    Consider these alternatives when conventional drilling can't do the job.