- G00 - Accelerated movement
- G01 - Linear interpolation
- G02, G03 - Circular interpolation
- G04 - Pause (dwell)
- G10 - Set new coordinates for the origin
- G17, G18, G19 - Plane selection
- G20 - Input inch data
- G21 - Input metric data
- G31 - Movement of axes to a given position
- G38.n - Straight probe
- G50, G51 - Scale mode
- G53 - Disabling the offset of the origin of the coordinate system
- G68 - Rotate coordinate system
- G69 - Cancel Rotation
- G80 - Cancel Canned Cycle
- G81 - Simple Drilling Cycle
- G82 - Drilling Cycle with Dwell
- G90 - Absolute positioning mode
- G90.1 - Absolute distance mode for I , J and K offsets
- G91 - Relative positioning mode
- G91.1 - Incremental distance mode for I, J and K offsets
- G98, G99 - Canned Cycle Return or Feed Rate Modes
- M03, M04, M05 - Spindle rotation control
- M07, M08, M09, M13, M14 - Coolant flow control

In CNC programming, there are 3 G-codes for selecting a plane during NC programming, which are used to define two axes: X, Y or Z. The plane selection is modal and is valid for everyone until you enter a different circular plane command.

The 3 Plane selection G-Codes are:

G17 for XY Plane

G18 for XZ Plane

G19 for YZ Plane

**XY plane selection with G17 code.**

The XY G17 plane selection code is set by default and sets the plane to the circular
interpolation mode G02 and G03.

In the circular interpolation blocks, the words X, Y, Z, I and J. are valid. The word K is
not valid. If the Z word is programmed in a circular interpolation block, then a spiral
forms in the XY plane. The direction of the arc or spiral in the XY plane can be
determined visually: Positive direction X - to the right side, positive direction Y - up.
The XY plane has a right-handed coordinate system. In G17, the endpoint of the arc is
defined in the block by the words X and Y. The center point of the arc is defined in
the block by the words I and J.

G17 is activated by default. Code G17 is canceled by codes G18 and G19.

Example:

**G17**

**G00X0Y0**

**M3 S6000**

**G00Z5**

**G01X14.1421Y-14.1421**

**G01Z-0.5F700**

**G02X14.1421Y14.1421R-20**

**G01X40.0Y-14.1421**

**G03X40.0Y14.1421R-20**

**G01X14.1421Y-14.1421**

**G00Z5**

**M5**

**G00X0Y0**

G17

XZ plane selection code G18 sets the plane to circular interpolation mode G02 and G03. In the circular interpolation blocks, the words X, Y, Z, I and J. are valid. The word J is not valid. If the word Y is programmed in a circular interpolation block, a spiral forms in the XZ plane. The direction of the arc or spiral in the XZ plane can be determined visually: The positive X direction is to the right, the positive Z direction is up. The XZ plane has a right-handed coordinate system. Code G18 is canceled by codes G17 and G19.

Example:

G00X0Z0

M3 S6000

G00z5 G01X14.1421Z-14.1421

G01Y-0.5F700

G02X14.1421Z14.1421R-20

G01X40.0Z-14.1421

G03X40.0Z14.1421R-20

G01x14.1421Z-14.1421

G00Y5

M5

G00X0Y0

G18

The YZ plane selection code G19 sets the plane to circular interpolation mode G02 and G03. In circular interpolation blocks, the words X, Y, Z, I, and K are valid. Word I is not valid. If the word X is programmed in a circular interpolation block, then a spiral forms in the YZ plane. The direction of the arc or spiral in the YZ plane can be determined visually: The positive direction Y is to the right, the positive direction Z is up. The YZ plane has a right-handed coordinate system. In G19, the end point of the arc is defined in the block by the words Y and Z. The center point of the arc is defined in the block by the words J and K. Code G19 is canceled by codes G17 and G18.

Example:

G00Y0Z0

M3 S6000

G00X5 G01Y14.1421Z-14.1421

G01X-0.5F700

G02Y14.1421Z14.1421R-20

G01Y40.0Z-14.1421

G03Y40.0Z14.1421R-20

G01Y14.1421Z-14.1421

G00X5

M5

G00Y0Z0

G19