* indicates optional
G76 Fine Boring Canned Cycles
In addition to boring the hole, this cycle will shift the X and/or Y Axis prior to retracting in order to clear the tool while exiting the part. If Q is used Setting 27 determines the shift direction. If Q is not specified, the optional I and J values are used to determine the shift direction and distance.
* indicates optional
G76 Threading Cycle, Multiple Pass:  Z depth,  Minor diameter,  Major diameter.
Setting 95/Setting 96 determine chamfer size/angle; M23/M24 turn chamfering ON/OFF.
G76 Threading Cycle, Multiple Pass Tapered:  Rapid,  Feed,  Programmed path,  Cut allowance,  Start position,  Finished diameter,  Target, [A] Angle.
The G76 canned cycle can be used for threading both straight or tapered (pipe) threads.
The height of the thread is defined as the distance from the crest of the thread to the root of the thread. The calculated depth of thread (K) is the value of K less the finish allowance (Setting 86, Thread Finish Allowance).
The thread taper amount is specified in I. Thread taper is measured from the target position X, Z at point  to position . The I value is the difference in radial distance from the start to the end of the thread, not an angle.
The depth of the first cut through the thread is specified in D. The depth of the last cut through the thread can be controlled with Setting 86.
The tool nose angle for the thread is specified in A. The value can range from 0 to 120 degrees. If A is not used, 0 degrees is assumed. To reduce chatter while threading use A59 when cutting a 60 degree included thread.
The F code specifies the feed rate for threading. It is always good programming practice to specify G99 (feed per revolution) prior to a threading canned cycle. The F code also indicates the thread pitch or lead.
At the end of the thread an optional chamfer is performed. The size and angle of the chamfer is controlled with Setting 95 (Thread Chamfer Size) and Setting 96 (Thread Chamfer Angle). The chamfer size is designated in number of threads, so that if 1.000 is recorded in Setting 95 and the feed rate is .05, then the chamfer will be .05. A chamfer can improve the appearance and functionality of threads that must be machined up to a shoulder. If relief is provided for at the end of the thread then the chamfer can be eliminated by specifying 0.000 for the chamfer size in Setting 95, or using M24. The default value for Setting 95 is 1.000 and the default angle for the thread (Setting 96) is 45 degrees.
G76 Using an A Value:  Setting 95 and 96 (see Note),  Setting 99 (Thread Minimum Cut),  Cutting Tip,  Setting 86 - Finish Allowance.
Four options for G76 Multiple Thread Cutting are available:
P1:Single edge cutting, cutting amount constant
P2:Double edge cutting, cutting amount constant
P3: Single edge cutting, cutting depth constant
P4: Double edge cutting, cutting depth constant
P1 and P3 both allow for single edge threading, but the difference is that with P3 a constant depth cut is done with every pass. Similarly, P2 and P4 options allow for double edge cutting with P4 giving constant depth cut with every pass. Based on industry experience, double edge cutting option P2 may give superior threading results.
D specifies the depth of the first cut. Each successive cut is determined by the equation D*sqrt(N) where N is the Nth pass along the thread. The leading edge of the cutter does all of the cutting. To calculate the X position of each pass you have to take the sum of all the previous passes, measured from the start point the X value of each pass