G17 To G19: Plane Selection - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G17 to G19: Plane selection

Specify the plane for circular interpolation and the plane for tool radius compensation.
Code Format
G17, G18, G19
G17
G18
G19
Processing details
• Plane selection specifies the plane for performing circular interpolation or tool radius compensation.
G-code
G17
G18
G19
• Set the base axes that make up the plane in [Motion Control Parameter][G-code Control Parameter][G-code Control
System Parameter]"Plane Composition""Base Axis I to K". Refer to Base axis I/base axis J/base axis K for details.
(Page 79 Base axis I/Base axis J/Base axis K)
• The plane selection command (G17, G18, G19) is modal. It remains in effect until another G-code from the same group is
used, and planes cannot be switched at blocks that are not commanded.
• When an axis address is commanded in the same block as a plane selection command (G17, G18, G19), the commanded
axis moves.
• Axis commands that do not exist on the plane determined by plane selection command (G17, G18, G19) have no effect on
plane selection.
Ex.
When registered as the table below, and G17 X100. Z100. is commanded.
The XY plane is selected, and Z moves with no relation to the plane.
Base axis Setting
I 1: X
J 2: Y
K 3: Z
At G-code control start and reset, the plane set in [Motion Control Parameter][G-code Control
Parameter][G-code Control System Parameter]"Modal Initial Setting""Plane Selection" is specified.
Program example
■Program that selects the X-Y plane, and draws an arc
Operation Program
(1) G17
(2) G91 G02 X50. Y50. R50. F500.
Y
50 End point (X50,Y50)
Feed speed
500[mm/min]
Start point 50
Description
X-Y plane selection
Z-X plane selection
Y-Z plane selection
X
[Unit: mm]
Remarks
X-Y plane selection
Circular interpolation positioning
5 G-CODE CONTROL PROGRAMS
5
121
5.6 G-Code