[deadlykitten]

hello, i just finished my 1st tool change procedure for the mill ; i did not attached it to a G code ( macro ) yet actually, i do not know how

available syntaxes :

CALL OCHG VC190=active tool VC191=next tool
CALL OCHG VC190=active tool
CALL OCHG VC191=next tool
CALL OCHG ( clear everything )

... it moves spindle to right if above senzor
... after "next tool" is prepared, M64 comes in, to avoid magazine "lift up" during cutting
... activates corrections
... it handles EMPTY values, in case a variable gets "nill" ? or how would you call it ? kindly !

ps : the forum editor add extra blank lines well, this makes code easier to view / review / delete ?

OCHG

 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                           ( 0 to EMPTY's )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )



    IF [ VC190 NE EMPTY ] N1
         VC190 = 0
                          N1

    IF [ VC191 NE EMPTY ] N2
         VC191 = 0
                          N2



 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                            ( active tool )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )


    IF [ VC190 EQ VTLCN ] NA1 ( if "desired tool" is allready in spindle  )

    IF [ VC190 NE     0 ] NA2 ( if empty spindle is not desired           )

    IF [ VTLNN EQ     0 ] NA3 ( if there is no "next tool"                )
        M64                   ( lift down                                 )
        NA3 M63               ( find an empty pot                         )
            M6                ( switch > empty spindle                    )
            GOTO NA1

        NA2

                              ( if "desired tool" is allready prepared,or )
                              ( if there is no "next tool"                )
    IF [ [ [ VC190 EQ VTLNN ] OR [ VTLNN EQ     0 ] ] EQ 1 ] NA4
        M64                   ( lift down                                 )
        NA4 T = VC190 M6      ( switch > "desired tool"                   )

    NA1


 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                               ( go play  )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )


    IF [ VTLCN EQ 0 ] NA4
        G56 HA DA
    NA4


 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                       ( spindle to right )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )


    CALL ORGHT


 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                              ( next tool )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )


    IF [ VC191 EQ VTLNN ] NN1 ( if "desired next tool" allready prepared  )

    IF [ VTLNN EQ     0 ] NN2 ( if there is no "next tool"                )
        M64                   ( lift down                                 )
        NN2

    IF [ VC191 EQ     0 ] NN1 ( if no "next tool" is desired              )
        T = VC191             ( "desired next tool" gets prepared         )
        M64                   ( lifting during cutting should be avoided  )

    NN1


 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )
                                                           ( master reset )
 ( ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~ ~  )


    VC190 = 0    VC191 = 0


RTS

ORGHT

    IF [ VTLCN EQ 0 ] GOTO N1
                      GOTO N2

        N1 MOVE = 200
           GOTO N3

        N2 MOVE = 200 + VTOFD [ VTLCN ] / 2
           GOTO N3

        N3

    IF [ VWKAX + VZOFX [ VACOD ] GE - 751 + MOVE ] NSKIP
    IF [ VWKAY + VZOFY [ VACOD ] LE + 331 - MOVE ] NSKIP

    G00 Z9999
    G00 X - 751 + MOVE - VZOFX [ VACOD ]
  ( G00 Y + 331 - MOVE - VZOFY [ VACOD ] )

NSKIP

RTS

[Superman]

We had a little different
( I'd say you could follow the gist of the code )

This is a library file for gauging tool lengths
OTOL2 is registered as a user G code as G114
- usage is G114 T10 D15 A45.
( tool # 10, cutter dia=30mm, tip is 45° from vertical )

OTOL2
(G114 T_ D_ A_)
(THIS PROGRAM SETS MXH TOOL LENGTH OFFSETS)
(USING RADIUS OFFSET AND ANGLE)
(D=RAD A=ANG)
  G15 H20
  IF [PA NE EMPTY] N100
  PA=0
N100
  IF [PT EQ EMPTY] N1100(IF T IS NOT SET GOTO LINE 1100)
  IF [VTLCN EQ PT] N400(IF T=TOOL IN THE SPINDLE GOTO LINE 400)
  IF [VNTOL EQ PT] N300(IF T=NEXT TOOL GOTO LINE 300)
  IF [VNTOL EQ 0 ] N200(IF NEXT TOOL IS VACANT GOTO LINE 200)
     M64               (CANCEL PRE-SELECT TOOL)
N200
     T=PT              (PRE-SELECT COMMANDED TOOL)
N300
     M06               (TOOL-CHANGE)
N400
N1000 G15 H20  (TO SET TOOL OFFSET CENTERLINE)
VFST=129
CALL OO30 PY=PD PRS=PA
G15H0
G56 G0 Z800 H0
X800 Y800
M203 (GET RID OF TOOL)
N1100 RTS

[deadlykitten]

hy why oo30 inside a tool change macro ? means measuring on every change ...

what is the goal for "tip is 45 from vertical" ?

what does VFST ? but M203 ?

is it G15 really required ? kindly !

[Superman]

why oo30 inside a tool change macro ? means measuring on every change ...
As I said....It is a measuring cycle,,if the tool is not in the spindle, it soon will be ( it may have been loaded directly into the pots, or a tip change etc )
CALL = call a subroutine
OO30 = OO prefix is system reserved filename ( you cannot use OO at the start of any sub or filename)...30 is gauging calculations
( refer to autoprobe manual )

It's for a horizontal, that has tool gauging, as well as a measuring probe
what is the goal for "tip is 45 from vertical" ?
- if tool is a boring bar, & the tip is not vertical.......sequence is to rotate spindle to line the tip to 6 o'clock position, & incrementally raise Y to line the tip with the gauging face

what does VFST ? but M203 ?
VFST is Automated tool gauging
M203 is a user M-code to force the spindle to be emptied
- I also have a M-code to clear coolant lines after using thru-coolant

is it G15 really required ?
- gauging cycles cannot be run in G15H0......so used the last one on page

[deadlykitten]

hello, i know , i know ... i raised those questions, because this thread is about tool change macro ; thus, it should not contain oo30 or G15

what is the relevance of your code in this context ?

[Superman]

hello, i know , i know ... i raised those questions, because this thread is about tool change macro ; thus, it should not contain oo30 or G15

what is the relevance of your code in this context ?

so you could see how this section worked in it's entirety

  IF [PT EQ EMPTY] N1100(IF T IS NOT SET GOTO LINE 1100)
  IF [VTLCN EQ PT] N400(IF T=TOOL IN THE SPINDLE GOTO LINE 400)
  IF [VNTOL EQ PT] N300(IF T=NEXT TOOL GOTO LINE 300)
  IF [VNTOL EQ 0 ] N200(IF NEXT TOOL IS VACANT GOTO LINE 200)
     M64               (CANCEL PRE-SELECT TOOL)
N200
     T=PT              (PRE-SELECT COMMANDED TOOL)
N300
     M06               (TOOL-CHANGE)

[deadlykitten]

yup, there is a part that has some conection with active tool, but does not cover all cases ... it good, is a reference so to say, but is just a part; i mean a tool change macro is one thing, a tool measuring/gauging is something else ...

"tool change macro" is before the cut ; after, or during it, you may check if the tool is "broken"

[deadlykitten]

... it moves spindle to right if above senzor

i wish to explain this a bit : if you cut a single part, than this is not necessary, because, in general, spindle is up, moves @ xy, and after that it lowers

on multiples parts, there is no need to raise the spindle to max, but only above the fixtures, and so, "above the fixtures" may be pretty closed to "senzor height", and in this case, such a behaviour, makes things safer

ps : i did not learned it the hard way

[deadlykitten]

    IF [ VC191 EQ     0 ] NN1 ( if no "next tool" is desired              )
        T = VC191             ( "desired next tool" gets prepared         )
        M64                   ( lifting during cutting should be avoided  )
    NN1

hello by using M64, after "next tool" is prepared, the magazine lift goes down, so tools are in vertical position; also, until M64 performs, main spindle does not move

if i remove M64, than tools will be tilted, but main spindle will move imediatly after "active tool" had been clamped

so is there some M64_ignore_response ? or some ATC ignore ? kindly !

[deadlykitten]

hello i just discovered the VTPNO [ tool_numer ], which returns the pot that contains the tool " tool_number "

please, when such a variable is needed ? are there some cases ? if not, than i think i will forget it ... kindly !