[vincent.pomerleau]

There is someone interested by a toolchange macro i created that loop each tool for mutiple parts. IE you set one variable at the program start for the part quantity for example #800=4 and the machine take the tool 1 and make all the operations on G54,G55,G56,G57 and also if you want G54 P1, G54 P2, etc. and then take the tool 2 and do all operations in reverse G57,G56,G55,G54...really usefull when you want to choose part QTY right on the floor.It also support the G5 P10000 (ai Nano HPCC) function that doesn't support macro calculation when activated. If interested reply and i will post all is needed to do it!

[fordav11]

there is always interest in macros that do useful things. please post it here if you want to.

[John_B]

I'd like to check it out as well!

[vincent.pomerleau]

I finally posted it

there's the macro

O9000(TOOLCHANGE*MACRO)
IF[#4113EQ98]THEN#10=1
IF[#4EQ1]GOTO13(GO*BACK*TO*CURRENT*TC)
IF[#5NE#0]GOTO6(WPC*UP)
IF[#6NE#0]GOTO9(WPC*DOWN)
IF[#10EQ1]GOTO14(SEND*TO*END*OF*PROGRAM)
#3=#4114(SEQUENCE*N*FLAG)
#11=#149/100
#11=FIX[#11](CALC*TOOL)
#12=[#149-[#11*100]](CALC*PRELOAD)
IF[#11EQ0]THEN#11=#12(MANUAL*TC)
IF[#11EQ#12]THEN#12=#0
IF[#11EQ30]THEN#11=0(PROBE=T30*FOR*PRELOAD)
IF[#11EQ#702]GOTO5(SAME*TOOL*SKIP)
IF[#703EQ0]GOTO2(SKIP*ROTARY*PROTECT*IF*DISABLED)
IF[#1EQ#0]GOTO1(MANUAL*TC*PROTECTION*WITH*ROTARY)
IF[#7741EQ0]GOTO15(ALARM*IF*FACEPLATE*PROBING*NOT*DONE)
IF[#5021+[#1-#5041]GT#7741]GOTO2(SKIP*IF*TC*IS*SAFE)
IF[#5021+[#1-#5041]LE#7741]THEN#1=#5041-[#5021-#7741](ROTARY*TC*PROTECTION)
G5P0
M9
G91G28Z0M19
G90X#1
GOTO2
N1
IF[#5021LE#7741]THEN#1=#5041-[#5021-#7741]
G5P0
M9
G91G28Z0M19
G90X#1
N2
IF[#3GE2]GOTO3
IF[#4014NE54.1]THEN#801=#4014(SET*FIRST*WPC*G54-G59)
IF[#4014EQ54.1]THEN#801=#4130(SET*FIRST*WPC*G54*P1-P48)
N3
IF[#5021+[#1-#5041]LE0]THEN#1=#0(X-*OT*CHECK)
IF[#5021+[#1-#5041]GE60.7]THEN#1=#0(X+*OT*CHECK)
IF[#5022+[#2-#5042]LE-30.]THEN#2=#0(Y-*OT*CHECK)
IF[#5022+[#2-#5042]GE0]THEN#2=#0(Y+*OT*CHECK)
#700=#4001(MOVE*TYPE*FLAG)
#701=#4003(ABS*INC*FLAG)
M46
IF[#4120NE0]THENGOTO4(PROBE*SPINDLE*LOCK)
S0M47
N4
G5P0
M9
G91G28Z0T#11M19
G90X#1Y#2M6
#702=#4120
T#12
#1=#0
#2=#0
N5
G#700
G#701N#3
#1=#0
#2=#0
M1(OPTIONAL*STOP)
(SET*WPC*MULTIPART*SECTION)
IF[#800LE1]GOTO12(SKIP*SECTION*IF*ONE*PART)
#7=#3/2(CHECK*IF*TC*NWORD*IS*ODD*OR*EVEN)
#8=FIX[#7]
#9=FUP[#7]
IF[#8EQ#9]GOTO9(SEND*TO*WPC*DOWN*IF*ODD)
N6(WPC*UP)
#4=1
IF[#5NE#0]THEN#5=#5+1
IF[#5EQ#0]THEN#5=#801
IF[#5LE48]GOTO7
G#5
GOTO8
N7
G54P#5
N8
IF[#5EQ[[#800-1]+#801]]THEN#5=#0
IF[#5EQ#0]THEN#4=#0
GOTO12
N9(WPC*DOWN)
#4=1
IF[#6NE#0]THEN#6=#6-1
IF[#6EQ#0]THEN#6=[[#800+#801]-1]
IF[#6LE48]GOTO10
G#6
GOTO11
N10
G54P#6
N11
IF[#6EQ#801]THEN#6=#0
IF[#6EQ#0]THEN#4=#0
N12(RETURN*TO*PROGRAM)
M99
N13(GO*CURRENT*TC)
IF[#800LE1]GOTO14
M56
#4=#0
M99P#3
N14(SEND*TO*END*OF*PROGRAM)
#3=#3+1
#10=#0
#800=#0
#801=#0
M99P#3
N15
#3000=1(PROBE*ROTARY*FACEPLATE)
M99
(#1=TC*X*RAPID)
(#2=TC*Y*RAPID)
(#3=CURRENT*TOOL*NWORD)
(#4=RETURN*TO*CURRENT*TC*FLAG)
(#5=CURRENT*UP*WPC)
(#6=CURRENT*DOWN*WPC)
(#7=CURRENT*TOOL*SPLIT*TO*ROUND)
(#8=ROUND*DOWN)
(#9=ROUND*UP)
(#10=END*OF*PROGRAM*FLAG)
(#11=TWORD)
(#12=CURRENT*PRELOAD)
(#700=MOVE*TYPE*FLAG)
(#701=ABS/INC*FLAG)
(#702=CURRENT*TOOL)
(#800=PART*QTY)
(#801=FIRST*WPC)




there's a sample program
%
O6001 (18-19)
#800=1 (PART QUANTITY)
G17 G20 G40 G54 G90 G98
#1=-2.875
#2=-1.25
N1 T0610 (ENDMILL 3/8" CARBIDE 2FL.)
M3 S10000
G5 P10000
G0 X-2.875 Y-1.25 M8
G43 H6 Z-.175
G1 Y.25 F75.
G0 Z.5
X2.875
Z-.175
G1 Y-1.25
G0 Z.5
X2.2813 Y-.5
Z.1
G1 Z-.275 F40.
X2.2822
G3 I-.001
G1 X2.2813
G0 Z.5
X-2.2813
Z.1
G1 Z-.275
X-2.2803
G3 I-.001
G1 X-2.2813
G0 Z.5
G5 P0
#1=0
#2=-.625
N2 T1000 (DRILL 5/32")
M3 S4890
G0 X0 Y-.625 M8
G43 H10 Z.5
G81 X0 Y-.625 R.1 Z-.2719 F29.3
G80
M98 P9000
N3 M9
G53 X30. Y0 Z0 M19
M30
%

[samu]

I was thinking about something like that and i recently wrote my own. It works great for short program but with a 200 block program,that is not very long, the last tool takes almost 5 sec to loop. I have also written a macro that loop a defined number of program on a defined number of work offset. Search for a program is much more faster than search for a block number. But you have to separate each tool on a single prog.

If any interest to see that, let me know

[fdonosos]

I need to put the tool in the same packet from which was take it, for example if I take the T01 from packet # 1 finished work how can I write the program so that the tool T01 back to packet # 1

[samu]

I assume that you have a random tool changer. Why do you want to return the tool in a specific pocket? You can write a macro to track which tool is in a pocket and a reorder macro to return each tool in its initial pocket at the end of the program. But in involve a lot of useless tool change. Maybe if you explain what you really want to do and why you want to do this, with some details on your tool changer, we could find an efficient solution.

[fdonosos]

I assume that you have a random tool changer. Why do you want to return the tool in a specific pocket? You can write a macro to track which tool is in a pocket and a reorder macro to return each tool in its initial pocket at the end of the program. But in involve a lot of useless tool change. Maybe if you explain what you really want to do and why you want to do this, with some details on your tool changer, we could find an efficient solution.

I need put back the tools to the same packet because the diameter of the tool is big.
When the program is running the tools are put in any packet back so when tools of large diameter come together it's lockup each other and how to prevent this from happening is keeping them always in the same packete

[viking73]

You should be able to flag the tool as large or big or heavy in the offset page.

Read your manual to be sure

Sent from my SAMSUNG-SGH-I747 using Tapatalk 2

[samu]

You should be able to flag the tool as large or big or heavy in the offset page.

Read your manual to be sure

If you can do that go this way.

Another way is to call always the same tool before the ''real tool change''.
let a pocket empty, suppose it is T20=empty

O1234
G17 G40 ...
T20 M6 (spindle is empty)
T1 M6 (first tool in spindle pocket 1 empty)
X... Y... M3 s....
T20 M6 (spindle empty first tool back in pocket 1)
T2 M6 (second tool in spindle pocket 2 empty)
X... Y...
T20 M6 (spindle empty second tool back in pocket 2)
T3 M6 (third tool in spindle, pocket 3 empty)
etc. etc. ....

Even if T20 is not empty, it works.

[blkaplan]

Has anyone tried this macro? Results? Sounds like it could be pretty useful!

[samu]

Has anyone tried this macro? Results? Sounds like it could be pretty useful!

Like i said, I tried something similar but with a 10 tool 1000 block program, it is not very fast because when you jump out of the macro, the control have to search from the beginning of the main program for the block you want to loop. The farther the block is, the longer is search time. Maybe with a recent control it doesn't affect so much but with my 0M-D, just for about 180 blocks, it takes about five second!!! The solution is to separate each tool in a sub and search for the program number of this tool which is much more faster than search for a block number. Here is the macro (tested, i use it on a regular basis)

************************************************** ****
* ALLOW TO LOOP MANY PROG ON MANY WORK OFFSET *
* FORMAT: G65 A... B... C... D...F... P9201 *
* A=FIRST WORK OFFSET(G54, G55, G56 ECT) *
* B=QUANTITY OF WORK OFFSET *
* C=FIRST PROG NUMBER TO LOOP *
* D=LAST PROG NUMBER TO LOOP *
* F=SET TO 1 TO BEGGIN BY THE LAST WORK OFFSET *
************************************************** ****
%
O9201
#11=#7-#3 (QUANTITY OF PROGRAM TO LOOP)
#12=#3 (WORKING COPY OF THE FIRST PROG)
#13=0 (PROGRAM COUNTER)
N10DO1
#10=0 (LOOP COUNTER)
IF[#9NE1]GOTO11 (IF YOU DON'T WANT TO BEGIN BY THE LAST WORK OFFSET JUMP TO)
#1=#1+#2-1 (SET LAST WORK OFFSET)
GOTO16
N11DO2
G#1 (SET CURRENT WORK OFFSET)
M98P#12 (CALL CURRENT PROGRAM)
#10=#10+1 (INCREMENT LOOP COUNTER)
IF[#10EQ#2]GOTO15 (IF CURRENT PROG HAS BEEN RUN ON ALL WORK OFFSET JUMP TO)
#1=#1+1 (INCREMENT WORK OFFSET)
END2
N15#13=#13+1 (INCREMENT PROG COUNTER)
IF[#13GT#11]GOTO18 (IF ALL PROG HAVE BEEN RUN JUMP TO)
#10=0 (RESET LOOP COUNTER)
#12=#12+1 (INCREMENT PROG NUMBER)
N16DO2
#9=0 (CLEAR THE BEGIN BY THE LAST OFFSET FLAG)
G#1 (SET CURRENT WORK OFFSET)
M98P#12 (CALL CURRENT PROG)
#10=#10+1 (INCREMENT LOOP COUNTER)
IF[#10EQ#2]GOTO17 (IF CURRENT PROG HAS BEEN RUN ON ALL WORK OFFSET JUMP TO)
#1=#1-1 (DECREMENT WORK OFFSET)
END2
N17#13=#13+1 (INCREMENT PROG COUNTER)
IF[#13GT#11]GOTO18 (IF ALL PROG HAVE BEEN RUN JUMP TO)
#12=#12+1 (INCREMENT PROG NUMBER)
END1
N18M99
%

[blkaplan]

Samu,

With this macro, how should each program be?

Should it start like a normal stand alone program?

for example

G00 G17 G20 G40 G80 G90
G91 G28 Z0.
/ T12
/ M06
G00 G17 G90 G54 X-.1446 Y1.7821 S7000 M03
..
..
..

M09
M05
G91 G28 Z0.
G28 Y0.
G90
M30
%

and then be complete for that tool?

If so, wouldn't I get an error when it runs the second time at the next work offset for the tool being called to the spindle being already loaded?

Thanks

[fdonosos]

Hey Samu thanks it work great I'm sorry so late

[samu]

Samu,

With this macro, how should each program be?

Should it start like a normal stand alone program?

for example

G00 G17 G20 G40 G80 G90
G91 G28 Z0.
/ T12
/ M06
G00 G17 G90 G54 X-.1446 Y1.7821 S7000 M03
..
..
..

M09
M05
G91 G28 Z0.
G28 Y0.
G90
M30
%

and then be complete for that tool?

If so, wouldn't I get an error when it runs the second time at the next work offset for the tool being called to the spindle being already loaded?

Thanks

%
O1234
G0 G17 G40 G49 G80 (AND ALL PREPARATORY CODE YOU WANT)
G91 G28 Z0
G65 A54. B4. C1235. D1238. P9201
G91 G28 Z0 M9
G28 Y0
M30

O1235
M6 T1
G0 G90 X.. Y... M3 S...
G43 H1 Z... M8
X... Y...
X... Y...
.....
.....
G0 Z SAFE HEIGHT TO GO TO NEXT WORK OFFSET
M99

O1236
M6 T2
G0 G90 X.. Y... M3 S...
G43 H2 Z... M8
X... Y...
X... Y...
.....
.....
G0 Z SAFE HEIGHT TO GO TO NEXT WORK OFFSET
M99

O1237
M6 T3
G0 G90 X.. Y... M3 S...
G43 H1 Z... M8
X... Y...
X... Y...
.....
.....
G0 Z SAFE HEIGHT TO GO TO NEXT WORK OFFSET
M99

O1238
M6 T4
G0 G90 X.. Y... M3 S...
G43 H1 Z... M8
X... Y...
X... Y...
.....
.....
G0 Z SAFE HEIGHT TO GO TO NEXT WORK OFFSET
M99
%

This example do each prog from O1235 to O1238 on G54 to G57 work offset
Program number have to follow each other except the main that doesn't matter
there is no tool change in the main, each tool change is in the sub of each tool. (I don't know how your machine act if you call the tool already in the spindle but if the tool change is well constructed, it should skip the tool change with no alarm. If you have a tool change macro, it is easy to make it act this way if it doesn't already do)
There is no work offset written in any program, this is the macro that assign the work offset

Keep me informed if you have any question or problem or even if it works perfectly

[samu]

Hey Samu thanks it work great I'm sorry so late

Thank you for the feedback, I'm happy that it works for you

[blkaplan]

My machine will throw and error and stop if i call a tool that is already in the spindle.

It is a Mori Seiki running Fanuc 10M.

Do you have any suggestions for that?

[samu]

My machine will throw and error and stop if i call a tool that is already in the spindle.

It is a Mori Seiki running Fanuc 10M.

Do you have any suggestions for that?

Does it use a tool change macro? if so, post the tool change macro and I'll check possible edit to fix it. Another solution is to set a variable after the tool change that allow to jump over the subsequent tool change and reset this variable by the macro when program number change.

%
O9201
#11=#7-#3 (QUANTITY OF PROGRAM TO LOOP)
#12=#3 (WORKING COPY OF THE FIRST PROG)
#13=0 (PROGRAM COUNTER)
#130=0(FIRST TOOL CHANGE FLAG)
N10DO1
#10=0 (LOOP COUNTER)
IF[#9NE1]GOTO11 (IF YOU DON'T WANT TO BEGIN BY THE LAST WORK OFFSET JUMP TO)
#1=#1+#2-1 (SET LAST WORK OFFSET)
GOTO16
N11DO2
G#1 (SET CURRENT WORK OFFSET)
M98P#12 (CALL CURRENT PROGRAM)
#10=#10+1 (INCREMENT LOOP COUNTER)
IF[#10EQ#2]GOTO15 (IF CURRENT PROG HAS BEEN RUN ON ALL WORK OFFSET JUMP TO)
#1=#1+1 (INCREMENT WORK OFFSET)
END2
N15#13=#13+1 (INCREMENT PROG COUNTER)
IF[#13GT#11]GOTO18 (IF ALL PROG HAVE BEEN RUN JUMP TO)
#10=0 (RESET LOOP COUNTER)
#130=0
#12=#12+1 (INCREMENT PROG NUMBER)
N16DO2
#9=0 (CLEAR THE BEGIN BY THE LAST OFFSET FLAG)
G#1 (SET CURRENT WORK OFFSET)
M98P#12 (CALL CURRENT PROG)
#10=#10+1 (INCREMENT LOOP COUNTER)
IF[#10EQ#2]GOTO17 (IF CURRENT PROG HAS BEEN RUN ON ALL WORK OFFSET JUMP TO)
#1=#1-1 (DECREMENT WORK OFFSET)
END2
N17#13=#13+1 (INCREMENT PROG COUNTER)
IF[#13GT#11]GOTO18 (IF ALL PROG HAVE BEEN RUN JUMP TO)
#130=0
#12=#12+1 (INCREMENT PROG NUMBER)
END1
N18 #130=0
M99
%


O1235
IF[#130 EQ 1] GOTO 5
M6 T1
#130=1
N5 G0 G90 X.. Y... M3 S...
G43 H1 Z... M8
X... Y...
X... Y...
.....
.....
G0 Z SAFE HEIGHT TO GO TO NEXT WORK OFFSET
M99


I use variable #130 to jump over problematic tool change
at the beginning of the macro and before each sub change, macro reset #130 to 0
At the beginning of each sub, i check for the value of #131
if #130=0, that means that it is the first time the sub is executed
right after the tool change block, I set #131 to 1 (in the sub ) so, for the subsequent execution of this sub, i will jump over the tool change.

I use that trick for rigid taping to avoid computing the M29 code at each work offset. (in that case you must have a G80 following #130=0 in the macro)
But I think in your case, it will be easier to work on the tool change logic and avoid hand coding. Do you know if you have a tool change macro?? If you don't have,no problem, we will create a macro called by M6 to watch if we need to call a tool change(M6 inside this macro will act as usual so we can call the tool change the way you already done)

[blkaplan]

When i unlocked the 8000 and 9000 programs on mill there is no macro tool change visible.

So to my knowledge there is no tool change macro.


It uses a randomly assigned pots.

[samu]

so i think the problem is with the T number and not with M6. M6 just swap the tool in spindle with the tool in the tool changer , but logically you cannot ask to prepare the pocket containing the tool in the spindle. More complicated than i thought! At least, the solution exposed in my previous post should work according that you jump above the M6 and the next tool Txx.
%
O1 (main)
T1 (TOOL FOR THE FIRS SUB )
G65 A54. B4. C2. D4. P9201
G91 G28 Z0 M9
G28 Y0
M30

O2
IF[#130=1] GOTO 5
M6
T2(TOOL FOR THE NEXT SUB)
N5 #130=1
(REST OF THE SUB)
M99

O3
IF[#130=1] GOTO 5
M6
T3(TOOL FOR THE NEXT SUB)
N5 #130=1
(REST OF THE SUB)
M99

O4
IF[#130=1] GOTO 5
M6
T1(TOOL FOR THE FIRST SUB)
N5 #130=1
(REST OF THE SUB)
M99
%

Give it a try and give me feed back! I'll continue thinking a way to avoid hand coding of the "IF GOTO ........."