As with G70 Bolt Hole Circle a cnc machinists can machine drills/tap/bore evenly spaced holes in a circle, the same way sometimes you have to drill/tap/bore evenly spaced holes in an arc, so comes G71 Bolt Hole Arc haas cnc command.
With G71 Bolt Hole Arc a cnc mill machinist can easily drill/bore/tap evenly spaced holes in an arc of known Radius.
Easy to program with few parameters.
G71 Bolt Hole Arc is non-modal.
G71 Bolt Hole Arc Format
G71 I J K L
I – Radius of the bolt hole arc
J – Starting angle of first hole ( 0 to 360° CCW from horizontal at the 3 o’clock position).
K – Angular spacing between holes (+ or -)
L – Number of evenly spaced holes around bolt hole arc.
All the parameters of G71 bolt hole arc are self explanatory.
A minus sign with K will reverse angles CW.
Using a K minus value (K-30.0) defines positioning around the bolt hole arc CW starting from the J angle.
Be sure to use a decimal point with angle command codes.
The tool must be positioned at the center of the arc either in a previous block or in the G71 block.
A drill, tap or bore cycle canned cycle must be active to perform the desired operation before the call of G71 bolt hole arc.
Canned cycles G73, G74, G76, G77, or G81-G89 can be used with G71 bolt hole arc.
How NOT to Drill/Tap/Bore in the Center?
1- If an L0 is on the drill, tap or bore cycle canned cycle line, the cycle will not execute that command until the control reads the next line for a G71 command, so as not to drill a hole in the center of a bolt hole arc.
2 – Or you can combine the drill cycle with the G71 on the same line, and it will also not drill a hole in the center.