G62: Automatic Corner Override - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G62: Automatic corner override

Applies the override to the feed speed automatically, and reduces the load on the tool during inside corner cutting or
automatic corner R inside cutting in tool radius compensation.
Code Format
G62
G62
Processing details
• When the G62 command is executed in conjunction with an interpolation command, automatic corner override is
performed. The interpolation command codes that can be used with the G62 command are G01, G02, and G03 only. When
G00 is specified it is invalid. Also, when changing from G00 to G01/G02/G03, or from G01/G02/G03 to G00 on a corner,
automatic corner override is not applied to the G00 block at that corner.
• The G62 command is modal. It remains in effect until any of exact stop check mode (G61), high-accuracy control mode
(G61.1), and cutting mode (G64) from the same group are commanded.
• In the following cases, automatic corner override is not applied.
• When in automatic corner override mode, but not in tool radius compensation mode.
• On a corner where tool radius compensation starts, or cancels.
• On a corner where there are tool radius compensation I and J vectors.
• When an intersection operation cannot be performed. (When movement command blocks are discontinuous for four times or more)
• The deceleration area at an arc command is the length of the arc.
• The angle of an inside corner is the angle of the program path set by the G-code control system parameter settings. When
the parameters are set as follows, automatic corner override becomes invalid.
• When the G-code control system parameter "Automatic Corner Override" setting is "0" or "100".
• When the G-code control system parameter "Automatic Corner Override Maximum Angle" setting is "0" or "180".
• When the G-code control system parameter "Length Before Automatic Corner Override Corner" setting is "0".
■Inside corner
When cutting an inside corner, the machining allowance is large and the load applied on the tool increases. Therefore, to
maintain a good cut, override is automatically applied over the setting range of the corner to reduce feed speed and control
the increase in load on the tool.
θ
P3
P2
P1
Ci
• With no G62 command
When the tool moves in the order of P1P2P3 in the illustration above, the machining allowance increases by the
surface area indicated by
• With G62 command
When the angle  of the inside corner in the illustration above is less than or equal to the angle set in the parameter, the
override set in the parameter is applied automatically over the deceleration area Ci.
Work
Program path (final shape)
Machining allowance
Work surface (before cut)
Tool center path
Deceleration area (IN)
Tool
θ: Inside corner maximum angle
when moving from P2 to P3, thus the load on the tool increases.
5 G-CODE CONTROL PROGRAMS
5.6 G-Code
5
147