5AXIS HEAD-HEAD 45 deg

This is another configuration of 5 axis machine. Using head and incline head 45° or some of us call it 5axis swivel head.

The main rotation C axis was on Z axis. Then A axis was incline between Z axis and Y axis.

Type of this machine has limitation of their rotation axis, such as:

C axis: limit + 360° and - 360°

A axis: limit +20° and -20°

SEYOON was one of famous machine maker that produce 5 axis machines. Complete with roll cutter to get cutting process much easier for some application.

There is some major equipment that 5 axis machining will result good performance.

1. Machine Constructions
   
2. Machine Control
   
3. Software (external user)
   
4. CAD/CAM Operator
   
5. Tooling
   

With 5 axis software, we can explore the strategy and simulate the 5 axis tool path that we just make.

The 5axis simulation on the software representate the real cutting on the 5 axis machine, so we get more confident.

Safety and accurate, that we want to achieve.

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