G70 Bolt Hole Circle (Group 00)

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
I - Radius
*J - Starting angle (0 to 360.0 degrees CCW from horizontal; or 3 o’clock position)
L - Number of holes evenly spaced around the circle

*indicates optional

This non-modal G code must be used with one of the canned cycles G73, G74, G76, G77, or G81-G89. A canned cycle must be active so that at each position, a drill or tap function is performed. See also G-code Canned Cycles section.

% O60701 (G70 BOLT HOLE CIRCLE) ; (G54 X0 Y0 is center of the circle ) ; (Z0 is on the top of the part) ; (T1 is a drill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X0 Y0 (Rapid to 1st position) ; S1000 M03 (Spindle on CW) ; G43 H01 Z0.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G81 G98 Z-1. R0.1 F15. L0 (Begin G81) ; (L0 skip drilling X0 Y0 position) ; G70 I5. J15. L12 (Begin G70) ; (Drills 12 holes on a 10.0 in. diameter circle) ; G80 (Canned Cycles off) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, Coolant off) ; G53 G49 Z0 M05 (Z home and Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

The G70 Finishing Cycle can be used to finish cut paths that are rough cut with stock removal cycles such as G71, G72 and G73.

P - Starting Block number of routine to execute
Q - Ending Block number of routine to execute

G18 Z-X plane must be active

G70 Finishing Cycle: [P] Starting block, [Q] Ending Block.

G71 P10 Q50 F.012 (rough out N10 to N50 the path) ; N10 ; F0.014 ; ... ; N50 ; ... ; G70 P10 Q50 (finish path defined by N10 to N50) ;

The G70 cycle is similar to a local subprogram call. However, the G70 requires that a beginning block number (P code) and an ending block number (Q code) be specified.

The G70 cycle is usually used after a G71, G72 or G73 has been performed using the blocks specified by P and Q. Any F, S, or T codes with the PQ block are effective. After execution of the Q block, a rapid (G00) is executed returning the machine to the start position that was saved before the starting of the G70. The program then returns to the block following the G70 call. A subprogram in the PQ sequence is acceptable providing that the subprogram does not contain a block with an N code matching the Q specified by the G70 call. This feature is not compatible with FANUC or YASNAC controls.

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.