Sample Fanuc Tool change macro

[dpuch]

I'm offering up a version of our tool change macro that we use to make tool changes easier and less code intensive in programs. Note this also makes MDI tool changes MUCH easier. This will activate the tool length offset and work offset G54 as well. This requires macros to use.
I'd appreciate any comments or suggestions for improving this.
And a disclaimer: Check the G and M codes against what your machine uses!


Usage:
T12
M98 P9006 (or just and M6 if you register the program, see below)

Yep that is all it takes to get T12 called to the spindle, with the tool length active.


You may replace the M98 P9006 with a simple M6 if you register program O9006 as M6 This may vary some for different controls, on our machine we have to set parameter 6046 = 6

parameter 6041 matches O9001
6042 matches O9002
Ect.
What ever number is assigned to the 604x is the M code that runs the 900x program

O9006 (TOOL CHANGE) 
G80
M9
G91G30Z0M5
G30X0Y0M15
IF[#[2000+#4120]LE11.0]GOTO10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG) 
N0010
G90
T#4320M6
G53 (SUPPRESS MULTI-BUFFER)
IF[#4320EQ0]GOTO9999
POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
IF[#[2000+#4120]GE1.0]GOTO20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT) 
N0020
IF[#[2200+#4120]LT1.0]GOTO30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE) 
N0030
G90G0G43G54Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
G53 (SUPPRESS MULTI-BUFFER)
IF[#4320NE#500]GOTO50
M0
M99
N0050
M1
N9999
M99

Now for the breakdown of the code

O9006 (TOOL CHANGE)
G80
M9
G91G30Z0M5
G30X0Y0M15
End previous activities and go to tool change position. Make sure automatic cycles are canceled and coolant is off, stop and orient the spindle.

IF[#[2000+#4120]LE11.0]GOTO10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG)
N0010

This is a quick check that the tool isn't too long for the machine/tool change, and will stop with error 97 and ",YIKES, TOOL LENGTH IS TOO LONG" as the message.

G90
T#4320M6

The actual tool change. this machine uses the T# on the same line as the M6 not all will. #4320 recalls the last T# used previously

G53 (SUPPRESS MULTI-BUFFER)
IF[#4320EQ0]GOTO9999
If T0 is called exit without activating any tool length ect.


POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
Outputs on the com port a line with the date and time, program number, and tool number separated by the @ symbol. I couldn't figure out how to output a comma or tab...

IF[#[2000+#4120]GE1.0]GOTO20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT)
N0020
IF[#[2200+#4120]LT1.0]GOTO30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE)
More tool length and length wear checks to make sure something stupid wasn't put in the offset table. This will also catch a missing offset


N0030
G90 G0 G43 G54 Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
Here we activate the tool offset. Home position is at Z25.0 This calculates the tool length and moves to Z24.99 (0.010 move) The move is required to activate the tool offset.


G53 (SUPPRESS MULTI-BUFFER)
IF[#4320NE#500]GOTO50
M0
M99
A number in macro variable 500 will cause the program to pause after changing to that tool number. cycle start will continue normal operation.


N0050
M1
N9999
M99
And finally turning on optional stop stops after any/all tool changes.

Here is a simple version with very little of the fancy stuff

O9006 (TOOL CHANGE) 
G80
M9
G91G30Z0M5
G30X0Y0M15
T#4320M6
G53 (SUPPRESS MULTI-BUFFER)
G90G0G43G54Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
G53 (SUPPRESS MULTI-BUFFER)
M99

Similar Threads:

• Fanuc OM, lost tool change macro
• Fanuc OM tool change macro for a Kiwa/Excel
• EDIT O9000 tool change macro fanuc 0M
• A sample tool change macro.
• Need Help!- Fanuc OM - How do I display the tool change macro?

[inthezone]

I get an error with my Fanuc OM controller saying there is an ilegal use of the minus sign when I try to upload the simple version of your tool change macro.

Any ideas why I might be getting this error? Perhaps I will have to write my macro differently?

[dpuch]

I would guess it has to do with the G90G0G43... line to activate the tool length offset.

Possibly you don't have fanuc macro B enabled on your control, or you don't have tool length wear offsets.

[dpuch]

An update to solve an issue about using G54 and a fixed number in the line to activate the tool offset.

N0030
G91 G0 G43 G54 Z-[#[2000+#4120]+#[2200+#4120]] H#4120
G90

[romer]

dpuch,

Thanks for sharing, very helpful, but could you please explain the

G53 (SUPPRESS MULTI-BUFFER)

line?

Is that some sort of resetting command line?

Thanks,
romer

[dpuch]

G53 on our machines stops the read ahead buffer until that line is actually finished.
M20 is the equivalent on another machine.

The point is to keep the buffer from reading and processing macro statements ahead of the actual execution.

I think the default read ahead is 3 lines, and there is an option that is 20 or more lines. It is mainly a safety to make sure the variables can't get the wrong values from later in the g-code. I (over) use them sometimes to be on the safe side.

[dpuch]

For some reason I got a post update message today, and I thought I would clean up the code posted here. It would not let me edit the original, so I am re-posting the code with better formatting, and the updated offset line. Nothing else was changed.

Code:

O9006 (TOOL CHANGE) 
G80
M9
G91 G30 Z0 M5
G30 X0 Y0 M15
IF [#[2000+#4120] LE 11.0] GOTO 10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG) 
N0010
G90
T#4320 M6
G53 (SUPPRESS MULTI-BUFFER)
IF [#4320 EQ 0] GOTO 9999
POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
IF [#[2000+#4120] GE 1.0] GOTO 20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT) 
N0020
IF [#[2200+#4120] LT 1.0] GOTO 30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE) 
N0030
G91 G0 G43 G54 Z-[#[2000+#4120]+#[2200+#4120]] H#4120
G90
G53 (SUPPRESS MULTI-BUFFER)
IF [#4320 NE #500] GOTO 50
M0
M99
N0050
M1
N9999
M99

Now for the breakdown of the code

O9006 (TOOL CHANGE)
G80
M9
G91 G30 Z0 M5
G30 X0 Y0 M15
End previous activities and go to tool change position. Make sure automatic cycles are canceled and coolant is off, stop and orient the spindle.

IF [#[2000+#4120] LE 11.0] GOTO 10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG)
N0010
This is a quick check that the tool isn't too long for the machine/tool change, and will stop with error 97 and ",YIKES, TOOL LENGTH IS TOO LONG" as the message.

G90
T#4320 M6
The actual tool change. this machine uses the T# on the same line as the M6 not all will. #4320 recalls the last T# used previously

G53 (SUPPRESS MULTI-BUFFER)
IF [#4320 EQ 0] GOTO 9999
If T0 is called exit without activating any tool length ect.


POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
Outputs on the com port a line with the date and time, program number, and tool number separated by the @ symbol. I couldn't figure out how to output a comma or tab...

IF [#[2000+#4120] GE 1.0] GOTO 20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT)
N0020
IF [#[2200+#4120] LT 1.0] GOTO 30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE)
More tool length and length wear checks to make sure something stupid wasn't put in the offset table. This will also catch a missing offset


N0030
G91 G0 G43 G54 Z-[#[2000+#4120]+#[2200+#4120]] H#4120
G90
Here we activate the tool offset. This makes a -Z incremental move Equal to the tool length+wear This activates the tool offset without physically moving the machine.


G53 (SUPPRESS MULTI-BUFFER)
IF [#4320 NE #500] GOTO 50
M0
M99
A number in macro variable 500 will cause the program to pause after changing to that tool number. cycle start will continue normal operation.


N0050
M1
N9999
M99
And finally turning on optional stop stops after any/all tool changes.

Here is a simple version with very little of the fancy stuff
Code:

O9006 (TOOL CHANGE) 
G80
M9
G91 G30 Z0 M5
G30 X0 Y0 M15
T#4320 M6
G53 (SUPPRESS MULTI-BUFFER)
G91 G0 G43 G54 Z-[#[2000+#4120]+#[2200+#4120]] H#4120
G90
G53 (SUPPRESS MULTI-BUFFER)
M99

[tem44ik]

Hello. I do have similar problem on my Leadwell TDC-510 - Fanuc O-M RoboDrill Tool Change CNC milling machine- after failure part of code is missing.
Maybe someone have similar machine and could share backup of tool change macro? If you have this machine please contact me. Any help appreciated - backup, manuals as text or pictures - any related information will help.

I'm offering up a version of our tool change macro that we use to make tool changes easier and less code intensive in programs. Note this also makes MDI tool changes MUCH easier. This will activate the tool length offset and work offset G54 as well. This requires macros to use.
I'd appreciate any comments or suggestions for improving this.
And a disclaimer: Check the G and M codes against what your machine uses!


Usage:
T12
M98 P9006 (or just and M6 if you register the program, see below)

Yep that is all it takes to get T12 called to the spindle, with the tool length active.


You may replace the M98 P9006 with a simple M6 if you register program O9006 as M6 This may vary some for different controls, on our machine we have to set parameter 6046 = 6

parameter 6041 matches O9001
6042 matches O9002
Ect.
What ever number is assigned to the 604x is the M code that runs the 900x program

O9006 (TOOL CHANGE) 
G80
M9
G91G30Z0M5
G30X0Y0M15
IF[#[2000+#4120]LE11.0]GOTO10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG) 
N0010
G90
T#4320M6
G53 (SUPPRESS MULTI-BUFFER)
IF[#4320EQ0]GOTO9999
POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
IF[#[2000+#4120]GE1.0]GOTO20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT) 
N0020
IF[#[2200+#4120]LT1.0]GOTO30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE) 
N0030
G90G0G43G54Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
G53 (SUPPRESS MULTI-BUFFER)
IF[#4320NE#500]GOTO50
M0
M99
N0050
M1
N9999
M99

Now for the breakdown of the code

O9006 (TOOL CHANGE)
G80
M9
G91G30Z0M5
G30X0Y0M15
End previous activities and go to tool change position. Make sure automatic cycles are canceled and coolant is off, stop and orient the spindle.

IF[#[2000+#4120]LE11.0]GOTO10
#3000=97 (,YIKES, TOOL LENGTH IS TOO LONG)
N0010

This is a quick check that the tool isn't too long for the machine/tool change, and will stop with error 97 and ",YIKES, TOOL LENGTH IS TOO LONG" as the message.

G90
T#4320M6

The actual tool change. this machine uses the T# on the same line as the M6 not all will. #4320 recalls the last T# used previously

G53 (SUPPRESS MULTI-BUFFER)
IF[#4320EQ0]GOTO9999
If T0 is called exit without activating any tool length ect.


POPEN
DPRNT [TIMES@#3011[80]@#3012[60]@P#120[40]@T#4120[20]]
PCLOS
Outputs on the com port a line with the date and time, program number, and tool number separated by the @ symbol. I couldn't figure out how to output a comma or tab...

IF[#[2000+#4120]GE1.0]GOTO20
#3000=98 (,YIKES, TOOL LENGTH IS TOO SHORT)
N0020
IF[#[2200+#4120]LT1.0]GOTO30
#3000=99 (,YIKES, TOOL WEAR IS TOO LARGE)
More tool length and length wear checks to make sure something stupid wasn't put in the offset table. This will also catch a missing offset


N0030
G90 G0 G43 G54 Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
Here we activate the tool offset. Home position is at Z25.0 This calculates the tool length and moves to Z24.99 (0.010 move) The move is required to activate the tool offset.


G53 (SUPPRESS MULTI-BUFFER)
IF[#4320NE#500]GOTO50
M0
M99
A number in macro variable 500 will cause the program to pause after changing to that tool number. cycle start will continue normal operation.


N0050
M1
N9999
M99
And finally turning on optional stop stops after any/all tool changes.

Here is a simple version with very little of the fancy stuff

O9006 (TOOL CHANGE) 
G80
M9
G91G30Z0M5
G30X0Y0M15
T#4320M6
G53 (SUPPRESS MULTI-BUFFER)
G90G0G43G54Z[24.99-[#[2000+#4120]+#[2200+#4120]]]H#4120
G53 (SUPPRESS MULTI-BUFFER)
M99

[toranacar]

Hi dpunch

I hope you can help me out a little here.
A bit of history with my Leadwell MCV OP, Fanuc OM. I purchased a few years ago (Unpowered for a few years) but seems the Parameters and Diagnostics have erased so I have punched in manually into the machine all the Parameters and Diagnostics.
The machine is now partially functional thanks the the great help from the guys here, unfortunately the ATC is not changing tools.
This is basically what happens.

[wendtmk]

Hi dpunch

I hope you can help me out a little here.
A bit of history with my Leadwell MCV OP, Fanuc OM. I purchased a few years ago (Unpowered for a few years) but seems the Parameters and Diagnostics have erased so I have punched in manually into the machine all the Parameters and Diagnostics.
The machine is now partially functional thanks the the great help from the guys here, unfortunately the ATC is not changing tools.
This is basically what happens.

You need to ask this question in the Fanuc forum. This forum is for G Code.

Mark

[toranacar]

thank you

[marsheng]

Hi Just wondering if this is still active. Just refurbished a YANG SMT500 It has an OMD controller and the tool offset has been a real problem. Nearly broke my machine when I used G43 H2 with a 30 mm offset as it lifted the spindle into the tool change area while it was spinning. No option to disable axis move on tool offset implementation.

I'm wondering if
IF[#[2000+#4120]LE11.0]GOTO10
is compatible with my machine.

My tool is held in
T#20 (LOAD TOOL NUMBER)

Not sure where the offset is ?


.

[dpuch]

If the 0MD has macro B enabled, it will probably work fine but I can't say for sure without knowledge of that machine.
#4120 is the last T number called #2001 is the length geometry for T1 So after a T12, #[2000+#4120] becomes #[2000 + 12] then #2012 then the length geometry offset for T12
Change 11.0 to a max value you want to allow so tools fit thru the tool changer.

An easy way to test bits of code is with MDI
T12
#100 = #4120
#101 = #[2000+#4120]

#100 should = 12
#101 should = the length offset for T12

[marsheng]

Thanks for the reply.

I'm still learning and still to find info on the # numbers. Any suggestions where to look ?

I know that #20 is my next tool number.

Here is my macro for my auto Tool changer.

I've added 50mm for the tool offsets to make sure there are no crashes. 50 is a guess. It will be the based on the biggest tool offset.

I'm sure that I could substitute tool offset value from a variable for the 50 mm, however if the machine does not remember the tool offset, then there could be a problem. Not sure whether the G49 moves the Z when activated in the macro.


[QUOTE]%
%
:9020(AUTO TOOL CHANGE 23-06-10)
N0010 M9 (COOLANT OFF)
N0020 G94 (FEED M/MIN)
N0030 IF[#1015EQ1] GOTO50 (MACHINE LOCK)
N0040 IF[#20EQ#0] GOTO40 (NO TOOL)
N0050 #106 = BIN[#1032]
N0060 IF[#106EQ#20] GOTO30 (TOOL IS CURRENT)
N0070 #1100 = 1 (TOOL CHANGE ACTIVE)
N0080 #101 = #4001 (SAVE MODES 01)
N0090 #102 = #4002 (SAVE MODES 02)
N0100 #103 =#4003 (SAVE MODES 03)
N0105 G53 Z-50.0 (MOVE TO SPACE BELOW Z HOME)
N0107 G49 (REMOVE TOOL OFFSET)
N1018 G53 Z0.0 (MOVE TO MACHINE ZERO)
N0110 G17G91G80G0 (XY PLAIN, INC, CAN CAN)
N0120 M19 (ORIENT SPINDLE)
N0130 M86 (TOOL CHANGE)
N0140 M07 (AIR BLAST)
N0150 G1 Z60.0 F2000.(FEED TO CHANGE)
N0160 G30 Z0.0 (TOOL CHANGE)
N0170 T#20 (LOAD TOOL)
N0180 M07 (AIR BLAST)
N0190 G28 Z0. (RETURN REF)
N0200 G#101 G#102 G#103 (RESTORE MODES)
N0210 #1100 = 0 (TOOL CHANGE INACTIVE)
N0220 M87 (FINISH TOOL CHANGE)
N0222 G53 Z-50.0 (MOVE TO SPACE BELOW Z HOME)
N0252 G43 H#20 (SET TOOL OFFSET)
N0230 N30 M99 (RETURN MAIN PROGRAM)
N0240 N40 #3000=1 (M06-NO-T-Code)
N0250 M99 (RETURN MAIN PROGRAM)
N0260 N50 #3000=2 (MACHINE LOCK /Z AXIS LOCK)
N0270 M99 (RETURN MAIN PROGRAM)
%

[dpuch]

The fanuc manuals list all the variables for your control. System variables vary some with different generations of controls. Common variables #100-199 and #500-999 may not all be available based on control options purchased.
#1-#33 are local macro variables and the #20 is just passing the T## number used to call the macro ie. 'M6 T14' to a variable usable inside program 9020

A summary from the CNC Cookbook site.
See also the local variables associated letter list

[marsheng]

I'm missing something here

In my macro have

#106 = BIN[#1032]

I assume that #1032 is the next tool number

IF[#106EQ#20]

If the next is the same as current, jump to end.

I don't understand how to do this

> An easy way to test bits of code is with MDI

Is my #20 a parameter or diagnostic value ?

Need to find where the tool offset value.is stored.

[dpuch]

I think #1032 would have been setup by your machine tool builder. It does seem to be storing the T# as a binary value based on the code posted.
Inside that macro, #20 should work in place of #4120 ie #[2000+#20] instead of #[2000+#4120] to get the tool length geometry offset value (without the wear value)

Did #4120 work in this MDI example?

An easy way to test bits of code is with MDI
T12
#100 = #4120
#101 = #[2000+#4120]

System parameter list
Macro programing PDF book

[marsheng]

Tried various options but can't enter # in MDI mode directly. Can in a line like below.

Tried G65 H1 P#100 Q20 (#100=20)

but get an error. From memory 078, something like cant find program number.

I think it is seeing the P as a program prompt.

Man this Fanuc is overly difficult to follow.

[dpuch]

Yes, G65 is macro program call so P#110 will try to run program 20 if there is one on the machine.

Just write a short program instead of MDI and try the same thing. Your tool change program uses macro programming, so that isn't an issue. But will #100 = #4120 write the last T number used to #100 and then will #101 = #[2000+#4120] write the correct offset length to #101?

[marsheng]

Don't know what I'm doing wrong.

For a test I ran

%
:0040 (OFFSET ADDRESS)
#100=100
#101=#4120
#102=#2000
M30
%

Looked up Variables on the screen and all were blank.

Hope I'm looking in the right place.

When I page through, Offset button I get

Offset Wear W001-W400
Offset Geometry G001-G400
Variable 100-199 ------------------All showed blank
Var 500-531 (Name Data Comment)
Variable 532-999
Variable 1-33

I presume this is correct.

What was also strange was, I had a tool offset of 20 mm. First time I ran the program, all good, second time the tool offset was cancelled and the Z moved the 20 mm.

This Fanuc stuff is convoluted !!!