Most turning centers are equipped with some helpful canned cycles. Fanuc, for example, has three simple, one-pass canned cycles (G90 for turning and boring; G92 for threading; and G94 for facing). Fanuc also offers several multiple-repetitive cycles (G70 for finishing; G71 for rough turning or rough boring; G72 for rough facing; G73 for pattern repeating; G74 for grooving; G75 for peck drilling; and G76 for threading).
If you haven’t learned about these helpful canned cycles, especially the multiple-repetitive cycles, you should pull out your programming manuals and study them. At least master the G71 command for rough turning and rough boring as it truly rivals a good CAM system. It also allows easy modification of the roughing operation at the machine. In like fashion, be sure to master the G76 threading command. This allows you to machine an entire thread (regardless of how many threading passes are required) based upon one command.
Admittedly, proficient programmers already understand the most common applications for these cycles because they are well covered in basic CNC courses. However, here are some special tricks you may not have considered, as you may find them helpful.
Manually boring soft jaws with G90. Though setup personnel must exercise extreme caution, they can use G90 to machine soft jaws. After manually positioning the jaw-boring bar close to the jaws to be bored, the personnel can use manual data input (MDI) to start the spindle and specify a series of jaw-boring passes. If the boring bar’s position has been specified (with a geometry offset), specifying G90 commands is pretty simple. Let's say, for instance, that the boring bar, is currently resting at a diameter of 2.5 inches, and it is 0.1 inch away from the face of the chuck. Again, this position has been manually attained. The command G90 X2.7 W-0.6 F0.010 will machine 0.1inch off the jaws (in diameter), 0.5-inch-deep in Z at a feed rate of 0.010 ipr. To make another 0.1-inch-deep pass, the command X2.9 can be given (G90 is modal—cancelled by G00).
Using G71 or G72 to semi-finish. As you know, these two multiple-repetitive cycles will complete rough-turning, boring or facing a workpiece, leaving a specified amount of stock for finishing. Within the G71 or G72 command, a U-word specifies how much stock must be left for finishing on all diameters. With most Fanuc control models, a W-word specifies the amount of finishing stock to be left on all faces. Specifying U0.04 and W0.005, for example, will leave 0.04-inch stock on all diameters (0.02-inch actual stock to be machined) and 0.005-inch stock on all faces. As you also know, a D-word within the G71 or G72 command specifies the depth of cut (on the side) for each roughing pass. With most controls, a fixed format for the D-word must be used (with most Fanuc models, the D-word does not allow a decimal point). In the inch mode, D1000 specifies a 0.1-inch depth of cut. There are times when you may want the machine to make one sweeping (semi-finish) pass over the entire workpiece—not taking multiple roughing passes. This is commonly the case when the turning operation precedes a heat-treating operation. In this case, make the D-word large enough to rough machine the entire workpiece in one pass. Make U and W the amount of stock you want to leave after semi-finishing. If you have a 2.0-inch diameter workpiece that must be turned down to 1.0 inch, for example, and if you want to leave 0.1 inch on all diameters and 0.02 inch on all faces (after semi-finishing), make the D-word at least 0.5 inch (D5000), U0.1 and W0.02.
Using G70 to repeat commands. Old Fanuc controls (we’re talking back to the 2000C—more than thirty years ago) have a helpful G25 command that allows you to repeat commands in a program. Some current model controls (such as Mitsubishi and Yasnac) have maintained the G25 command. With G70, you to have this capability. While we normally use G70 to finish machine after using G71, G72 or G73, it does work nicely on its own. For example, the command G70 P100 Q200 will cause the control to execute lines N100 through N200. Then the control will go to the command immediately following the G70 command.blog comments powered by Disqus