By specifying a G code from G54 to G59, one of the workpiece
coordinate systems 1 to 6 can be selected.
G54 ; Workpiece coordinate system 1
G55 ; Workpiece coordinate system 2
G56 ; Workpiece coordinate system 3
G57 ; Workpiece coordinate system 4
G58 ; Workpiece coordinate system 5
G59 ; Workpiece coordinate system 6
2. First Tool Load
Tool loading before 1st cutting.
example:
T01 M06
M3 S8000
Format function:
T ; Command to assign tool number.
xx ; number from tool magazine .
M06 ; Command to execute tool change.
M01 ; Option stop - for make sure have right tool.
S xxxx ; RPM of spindle.
M3 ; Spindle rotation clockwise.
3. Feature coordinate system setting (3+2 positioning)
This very important to be check before running program further.
TILTED WORKING PLANE COMMAND
Programming for creating holes, pockets, and other figures in a datum
plane tilted with respect to the workpiece would be easy if commands
can be specified in a coordinate system fixed to this plane (called a
feature coordinate system). This function enables commands to be
specified in the feature coordinate system. The feature coordinate
system is defined in the workpiece coordinate system
Format function:
G68.2 X x1 Y y1 Z z1 Ia Jb Kc ; Feature coordinate system setting.
G69 ; Cancels the feature coordinate system setting.
X, Y, Z ; Feature coordinate system origin.
I, J, K ; Euler's angle for determining the orientation of the
feature coordinate system.
G53.1 ; Controls the tool axis direction.
example:
G69
G68.2 X0.0 Y23.5 Z-23.5 I-90.0 J0.0 K0.0
G53.1
4. First move after tool load
At this section, we should prefer move Rotary axis (A/B & C) first then X, Y.
Example:
G1 A-90.0 C0.0 F3000
X-12.147 Y-27.72
G1 G43 Z40.0 H01 F3000
Format Function:
G1 ; Linear move using Feedrate.
A, C ; Rotary table.
F ; Feedrate.
X, Y ; Actual coordinate.
G43 ; Tool length compensation.
Hxx ; Tool length number.
5. Tool Change
Before we have any tool change, we should switch off all previous modals.
example:
M09
G69
G91 G28 Z0.0
G49 G80 G40
T08 M06
G90
M44
M46
M01
Format Function:
M09 ; Turn collant mode.
G69 ; Cancels the feature coordinate system setting.
G91 G28 Z0.0 ; Return to home machine position.
G49 G80 G40 ; Cancels tool length compensation, cancel drilling cycle.
T08 M06 ; Tool change.
G90 ; Absolute mode ON.
M44 ; UnClamp swivel table.
M46 ; UnClamp rotary table.
M01 ; Option stop.
6. End Program
The end of program that's run after all machining process finished.
example:
G0 Z150.
G49 G80 Z250.
G69
G5.1 Q0
M05
M44
M45
G91 G28 A0.0 C0.0
G91 G28 X0.0 Y0.0 Z0.0
M30
%
## ref: Fanuc Machining Centre User manual
