Siemens SINUMERIK 802D sl Programming Manual page 27

04.07
Plane designation
With the commands indicated below, a cutting tool moves along the specified circu-
lar arc in the XY plane, ZX plane, or YZ plane so that the feedrate specified by the
F command will be the tangential velocity of the arc.
S In the XY Plane
G17 G02 (or G03) X⋅⋅⋅Y⋅⋅⋅R⋅⋅⋅ (or I⋅⋅⋅J⋅⋅⋅) F⋅⋅⋅;
S In the ZX Plane
G18 G02 (or G03) Z⋅⋅⋅X⋅⋅⋅R⋅⋅⋅ (or K⋅⋅⋅I⋅⋅⋅) F⋅⋅⋅;
S In the YZ Plane
G19 G02 (or G03) Y⋅⋅⋅Z⋅⋅⋅R⋅⋅⋅ (or J⋅⋅⋅K⋅⋅⋅) F⋅⋅⋅;
To designate the circular interpolation mode (G02, G03), the plane of interpolation
should be selected first by specifying the G17, G18, or G19. For the 4th and 5th
axis, circular interpolation is allowed only when they are linear axes.
The G code designated to select the plane in which circular interpolation is execu-
ted also selects the plane where tool radius offset (G41/G42) is executed. When
the power is turned ON, the XY plane (G17) is automatically selected.
If an optional linear 4th-axis is selected, circular interpolation is possible in the Xα,
Zα, or Yα plane which includes the 4th-axis in addition to the XY, YZ, and ZX pla-
nes. (α=U, V, or W)
S Circular interpolation in Xα plane
G17 G02 (or G03) X ⋅⋅⋅ α ⋅⋅⋅ R ⋅⋅⋅ (or I ⋅⋅⋅ J ⋅⋅⋅) F ⋅⋅⋅;
S Circular interpolation in Zα plane
G18 G02 (or G03) Z ⋅⋅⋅ α ⋅⋅⋅ R ⋅⋅⋅ (or K ⋅⋅⋅ I ⋅⋅⋅) F ⋅⋅⋅;
S Circular interpolation in Yα plane
G19 G02 (or G03) Y ⋅⋅⋅ α ⋅⋅⋅ R ⋅⋅⋅ (or J ⋅⋅⋅ K ⋅⋅⋅) F ⋅⋅⋅;
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
G17
G18
G19
Commands Calling Axis Movements
2.1 Interpolation commands
XY plane, or Xα or Xβ plane
ZX plane, or Zα or Zβ plane
YZ plane, or Yα or Yβ plane
2-27