G82 Spot Drill Canned Cycle (Group 09)

Next Generation 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
*E - Chip-clean RPM (Spindle reverses to remove chips after each cycle)
F - Feedrate
*L - Number of holes if G91 (Incremental Mode) is used.
*P - The dwell time at the bottom of the hole
*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 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.
note: G82 is similar to G81 except that there is the option to program a dwell (P).
% O60821 (G82 SPOT DRILLING CANNED CYCLE) ; (G54 X0 Y0 is at the top-left of part) ; (Z0 is on top of the part) ; (T1 is a 0.5 in 90 degree spot drill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X2. Y-2. (Rapid to 1st position) ; S1000 M03 (Spindle on CW) ; G43 H01 Z0.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G82 Z-0.720 P0.3 R0.1 F15.(Begin G82) ; (Drill 1st hole at current X Y location) ; X2. Y-4. (2nd hole) ; X4. Y-4. (3rd hole) ; X4. Y-2. (4th hole) ; (BEGIN COMPLETION BLOCKS) ; G00 Z1. M09 (Rapid retract, Coolant off) ; G53 G49 Z0 M05 (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

G82 Spot Drilling Example

*C - C-Axis absolute motion command (optional)
F - Feed Rate in inches (mm) per minute
*L - Number of repeats
P - The dwell time at the bottom of the hole
R - Position of the R plane
W - Z-axis incremental distance
*X - X-axis motion command
*Y - Y-axis motion command
*Z - Position of bottom of hole

* indicates optional

This G code is modal in that it activates the canned cycle until it is canceled or another canned cycle is selected. Once activated, every motion of X will cause this canned cycle to be executed.

Also, see G242 for radial live tool spot drilling.

G82 Spot Drill Canned Cycle:[1] Rapid, [2] Feed, [3] Start or end of stroke, [4] Dwell, [5] Starting plane, [R] R plane, [Z] Position of the bottom of the hole.

G82 Y-Axis Drill

% o60821 (G82 LIVE SPOT DRILL CYCLE) ; (G54 X0 Y0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is a spot drill) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G98 (Feed per min) ; M154 (Engage C Axis) ; G00 G54 X1.5 C0. Z1. (Rapid to 1st position) ; P1500 M133 (Live tool CW at 1500 RPM) ; M08 (coolant on) ; (BEGIN CUTTING CYCLE) ; G82 C45. Z-0.25 F10. P80 (Begin G82) ; C135. (2nd position) ; C225. (3rd position) ; C315. (4th position) ; (BEGIN COMPLETION BLOCKS) ; M155 (C axis disengage) ; M135 (Live tool off) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 (Z home) ; M30 (End program) ; %

To calculate how long you should dwell at the bottom of your spot drill cycle, use the following formula:

P = Dwell Revolutions x 60000/RPM

If you want the tool to dwell for two full revolutions at its full Z depth in the program above (running at 1500 RPM), you would calculate:

2 x 60000 / 1500 = 80

Enter P80 (80 milliseconds or P.08 (.08 seconds) on the G82 line, to dwell for 2 revolutions at 1500 RPM.

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.