Fanuc Multiaxis Programming #2

2nd part continued from FANUC control program begin:
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

5 axis Machine

In few pass of year, the machining direction change to use more complex machine. Such as multiaxis machine.

Recently in our country have more population of 5 axis machine such as Deckel Maho, Mazak, Moriseiki, and the new comers are Quaser.




Those machine are using common control to run their mechanical device. The controller such as Fanuc, Heidenhain, Siemens, etc.

Here litle explanation the Fanuc control language as NC Code:
This momment i'll share some function of NC-code languange to control the machine.

1. Program Header
On program header, it containing some NC Code for initialisation:
O8899
G91 G28 Z0.0
G28 A0.0 C0.0
G28 X0.0 Y0.0
G90 G54
M44
M46
T1M6
G5.1Q1
==========

O8899 ; Number program have text "O" at start of program number.
G91 ; Incremental movement.
G28 ; Position of Home machine.
G28 Z0.0 is command to run machine goes to Z home machine position.
G28 X0.0 Y0.0 is command to run machine goes to X, and Y home machine position.
G90 ; Absolut movement.
G54 ; Work offset coordinate
Work offset cooedinate can assign value of 54, 55, 56, 57, 58, 59
M44 ; UnClamp swivel table.
M46 ; Unclamp rotary table.

Next post is Tool change and First Move after tool change position ...