G76 Fine Boring Canned Cycle (Group 09)

Classic Control - Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue
F - Feedrate
*I - Shift value along the X-Axis before retracting, if Q is not specified
*J - Shift value along the Y-Axis before retracting, if Q is not specified
*L - Number of holes to bore if G91 (Incremental Mode) is used
*P - The dwell time at the bottom of the hole
*Q - The shift value, always incremental
*R - Position of the R plane (position above the part)
*X - X-Axis location of hole
*Y - Y-Axis location of hole
*Z - Position of the Z-Axis at the bottom of hole

* indicates optional

caution: Unless you specify otherwise, this canned cycle uses the most recently commanded spindle direction (M03, M04, or M05). If the program did not specify a spindle direction before it commands this canned cycle, the default is M03 (clockwise). If you command M05, the canned cycle will run as a “no-spin” cycle. This lets you run applications with self-driven tools, but it can also cause a crash. Be sure of the spindle direction command when you use this canned cycle.

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.

*A - Tool nose angle (value: 0 to 120 degrees) Do not use a decimal point
D - First pass cutting depth
F(E) - Feed rate, the lead of the thread
*I - Thread taper amount, radius measure
K - Thread height, defines thread depth, radius measure
*P - Single Edge Cutting (load constant)
*Q - Thread Start Angle (Do not use a decimal point)
*U - X-axis incremental distance, start to maximum thread Depth Diameter
*W - Z-axis incremental distance, start to maximum thread length
*X - X-axis absolute location, maximum thread Depth Diameter
*Z - Z-axis absolute location, maximum thread length

* indicates optional

G76 Threading Cycle, Multiple Pass: [1] Z depth, [2] Minor diameter, [3] Major diameter.

Setting 95/Setting 96 determine chamfer size/angle; M23/M24 turn chamfering ON/OFF.

G76 Threading Cycle, Multiple Pass Tapered: [1] Rapid, [2] Feed, [3] Programmed path, [4] Cut allowance, [5] Start position, [6] Finished diameter, [7] 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 [7] to position [6]. The I value is the difference in radial distance from the start to the end of the thread, not an angle.

note: A conventional O.D. taper thread will have a negative I value.

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: [1] Setting 95 and 96 (see Note), [2] Setting 99 (Thread Minimum Cut), [3] Cutting Tip, [4] Setting 86 - Finish Allowance.

note: Setting 95 and 96 will affect the final chamfer size and angle.

Four options for G76 Multiple Thread Cutting are available:

  1. P1:Single edge cutting, cutting amount constant

  2. P2:Double edge cutting, cutting amount constant

  3. P3: Single edge cutting, cutting depth constant

  4. 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

G76 Thread Cutting Cycle, Multiple Pass

% o60761 (G76 THREAD CUTTING MULTIPLE PASSES) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD thread tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; G00 G54 X1.2 Z0.3 (Rapid to 1st position) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G76 X0.913 Z-0.85 K0.042 D0.0115 F0.0714 (Begin G76) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.