Fagor 8040 MC CNC, Руководство пользователя, Страница: 76 / 247

Chapter 2 - page 14
MC work mode 2. Operating in JOG mode
2.5 Tool control
2.5.1 Tool change
2.5.1 TOOL CHANGE
Depending on the type of tool changer, one can have:
Machine with automatic tool changer
Machine with manual tool changer
In both cases the CNC:
Executes the routine associated with the tool change (general machine P60 «TOOLSUB»).
Sends the PLC all the information required for this to handle the tool change.
And assumes the new values for the tool (offsets, geometry, etc. ...).
An example of how a manual tool changer is handled.
Subroutine 55 as associated with the tools. General machine parameter P60 «TOOLSUB» = 55.
Define the general machine parameter P71 "TAFTERS" = YES so that the tool is selected after
executing the subroutine.
The subroutine associated with the tools can contain the following information:
(SUB 55)
(P100 = NBTOOL)
; Assigns the No. of tool requested to P100
(P101 = MS3) ; If spindle clockwise P101=1
(P102 = MS4) ; If spindle counterclockwise P102=1
G0 G53.... XP?? Y?? ZP?? ; Movement to change point
M5
; Spindle stop
(MSG "SELECT T?P100 - THEN PRESS START")
; Message for requesting tool change
M0 ; Program stop and wait until START is pressed
(MSG "" "") ; Erases previous message
(IF P102 EQ 1 GOTO N10) ; Recovers turning direction of spindle
(IF P101 EQ 0 RET)
M3
(RET)
N10 M4
(RET)
After completing the subroutine, the CNC executes function T??, sends the PLC all the
information required for the latter to handle the tool change and assumes the new values for
the tool, (tool offsets, geometry, etc.)
When having a Machining Center, general machine parameter "TOFFM06 (P28) = Yes", the CNC
acts as follows:
If the execution of an operation or cycle involves a tool change, the CNC:
Selects the desired tool in the magazine
Executes the subroutine associated with the tool, general machine parameter "TOOLSUB (P60)"
Executes function M06 to carry out the tool change.
When selecting a new tool in JOG mode or when operating in M mode, the CNC only selects the too
in the magazine and executes the associated subroutine.
The M06 function must be executed by the operator, either by programming an ISO block or by
setting the PLC so it executes the M06 function when pressing a particular key. The following
example uses the [O4] key: DFU B2 R562 = CNCEX1 (M06, M1)
Note: On Machining Centers, the subroutine associated with the tool MUST NOT include the M06.