Need Help!- Tool Change not working after reset

[mrneelix]

I am relatively new to CNC so please bear with me.

I am running an Anderson Stratos Router with a Fanuc 0-M controller. Everything was going great until last night when it came up with a P/S 101 Alarm and nothing would function. I checked the Operator Manual and found that the only way to clear it is to clear the memory completely by turning on the power to the controller while holding down <Delet>. I did so and lost all programs in memory (obviously what it was supposed to do). Unfortunately it also took out all the O9000 programs as well. When I brought it back up, I could manually jog the position, etc but I could not run any programs (getting a P/S 078). Long story short, I found the code for the Tooling Change Macro for the Stratos, entered it and sent it over after figuring out how to disable the protection/etc. The code I used is below. Once I had put those in I was able to run one program, but the tool change wouldn't work...I had to manually change them at the proper times. After that I went to run a second program, and the head moved to the correct start point, but as soon as the code indicated what tool to grab, the program stalled and would go no further (i.e the tool would not change, the tool already in the spindle would not lower to start the cut, etc.) Any help that anyone can give me would be VERY appreciated.

Thanks in advance.


Here is the programs that it said to load

%
:O9000
G65 H81 P2000 Q#1003
M52
G65 H01 P#1114 Q0
G65 H01 P#144 Q#4001
G65 H01 P#145 Q#4003
G65 H81 P1002 Q#4006 R21
N2 G65 H01 P#146 Q-32704
N3 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G65 H03 P#147 Q#149 R10
G65 H02 P#148 Q#147 R60
G65 H85 P950 Q#149 R19
G65 H84 P950 Q#149 R10
G65 H83 P910 Q#149 R10
N20 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M60
G04 P10
G65 H81 P900 Q#1001 R1
G91 G00 Z#146 F20000
G04 P10
G65 H82 P950 Q#5023 R#146
G65 H01 P#1100 Q1
M71
M73
G91 G00 Z-#146 F20000 M53
G65 H01 P#1100 Q0
M54
G04 P10
G65 H82 P950 Q#5023 R0
G65 H01 P#1101 Q1
M74
M72
N900 M70
G28 Z0
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G#145
G#144
M51
M99
N910 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M#148
G04 P10
G65 H81 P930 Q#1000 R1
G65 H82 P940 Q#1001 R1
G65 H81 P920 Q#1002 R1
T#149
N920 G91 G00 Z0
G04 P10
G65 H82 P950 Q#5023 R0
G65 H01 P#1101 Q1
M71
M73
G91 G00 Z#146 F20000 M53
G65 H01 P#1101 Q0
M54
G04 P10
G65 H82 P950 Q#5023 R#146
G65 H01 P#1100 Q1
M74
M72
N930 M70
G65 H01 P#1100 Q0
G28 Z0
G#145
G#144
M51
M99
N940 G91 G00 Z#146 F20000
G04 P10
G65 H82 P950 Q#5023 R#146
G65 H01 P#1100 Q1
M71
M73
G91 G00 Z-#146 F20000 M53
G65 H01 P#1100 Q0
G04 P10
G65 H82 P950 Q#5023 R0
G65 H01 P#1101 Q1
T#149
G91 G00 Z#146 F20000
G65 H01 P#1101 Q0
M54
G04 P10
G65 H82 P950 Q#5023 R#146
G65 H01 P#1100 Q1
M74
M72
M70
G65 H01 P#1100 Q0
G28 Z0
G#145
G#144
M51
M99
N950 M51
G65 H99 P1
M99
N1002 G65 H01 P#146 Q-83070
N1003 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G65 H03 P#147 Q#149 R10
G65 H02 P#148 Q#147 R60
G65 H85 P1950 Q#149 R19
G65 H84 P1950 Q#149 R10
G65 H83 P1910 Q#149 R10
N1020 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M60
G04 P10
G65 H81 P1900 Q#1001 R1
G91 G00 Z#146 F6000
G04 P10
G65 H82 P1950 Q#5023 R#146
G65 H01 P#1100 Q1
M71
M73
G91 G00 Z-#146 F6000 M53
G65 H01 P#1100 Q0
M54
G04 P10
G65 H82 P1950 Q#5023 R0
G65 H01 P#1101 Q1
M74
M72
N1900 M70
G28 Z0
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G#145
G#144
M51
M99
N1910 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M#148
G04 P10
G65 H81 P1930 Q#1000 R1
G65 H82 P1940 Q#1001 R1
G65 H81 P1920 Q#1002 R1
T#149
N1920 G91 G00 Z0
G04 P10
G65 H82 P1950 Q#5023 R0
G65 H01 P#1101 Q1
M71
M73
G91 G00 Z#146 F6000 M53
G65 H01 P#1101 Q0
M54
G04 P10
G65 H82 P1950 Q#5023 R#146
G65 H01 P#1100 Q1
M74
M72
N1930 M70
G65 H01 P#1100 Q0
G28 Z0
G#145
G#144
M51
M99
N1940 G91 G00 Z#146 F6000
G04 P10
G65 H82 P1950 Q#5023 R#146
G65 H01 P#1100 Q1
M71
M73
G91 G00 Z-#146 F6000 M53
G65 H01 P#1100 Q0
G04 P10
G65 H82 P1950 Q#5023 R0
G65 H01 P#1101 Q1
T#149
G91 G00 Z#146 F6000
G65 H01 P#1101 Q0
M54
G04 P10
G65 H82 P1950 Q#5023 R#146
G65 H01 P#1100 Q1
M74
M72
M70
G65 H01 P#1100 Q0
G28 Z0
G#145
G#144
M51
M99
N1950 M51
G65 H99 P1
N2000 M99
%

--------------------------------------------------------------------------

%
:O9004
G65 H81 P2000 Q#1003 R1
G65 H81 P1000 Q#4006 R21
M52
G65 H01 P#1114 Q1
G65 H01 P#144 Q#4001
G65 H01 P#145 Q#4003
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G65 H82 P20 Q#1015 R1
G91 G01 Z-#5023 F6666
G65 H80 P500
N20 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M60
G04 P10
G65 H01 P#1100 Q1
M73
M53
N30 G91 G01 Z-#5023 F6666
G65 H01 P#1100 Q0
G65 H01 P#1101 Q1
M54
G04 P10
M74
M72
N500 M70
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G#145
G#144
G65 H01 P#1114 Q0
M51
M99
N1000 M52
G65 H01 P#1114 Q1
G65 H01 P#144 Q#4001
G65 H01 P#145 Q#4003
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G65 H82 P1020 Q#1015 R1
G91 G01 Z-#5023 F2000
G65 H80 P1500
N1020 G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
M60
G04 P10
G65 H01 P#1100 Q1
M73
M53
N1030 G91 G01 Z-#5023 F2000
G65 H01 P#1100 Q0
G65 H01 P#1101 Q1
M54
G04 P10
M74
M72
N1500 M70
G65 H01 P#1100 Q0
G65 H01 P#1101 Q0
G#145
G#144
G65 H01 P#1114 Q0
M51
M99
N2000 G65 H99 P2
%

---------------------------------------------------------------------

%
O8999
M98 P9004
M30
%

[mrneelix]

Ok, quick update....talked to Anderson and they found 1 missing parameter in the O9000 program so now the tool changer is working (YAY!) but it is still going to the start point of a production program, grabbing the tool (which is good) but then stalling out on the line below the tool call.

Here is the part of the code in bold where it is stalling plus 20 lines above and below in case they are the cause.

Thanks all!

%
O7303 (ANC9A0A)
(07 MAY 10 - 14:40)
(RUN TIME=5:35)
(SPOILBOARD 0.5)
(MATERIAL 0.875)
G17 G90 G20 G40
G08 P1
M06
'(OP 5 CONTOUR POCKET TOOL 16 T-6 ENGRAVING BIT TEST ENGRAVING AT .1 D
'(EFFECTIVE DIAMETER 0.015, WIDTH OF CUT 0.0075)
T16
G00 G90 G54 X25.5775 Y35.0175 M13 S0
G43 H16 Z4.375
G0 Z5.375
X25.5775 Y35.0175
X12.792 Y39.0448
Z5.125
G1 Z1.275 F0.
G3 X12.8396 Y39.0367 R0.1425
G1 X13.0253
G3 Y39.0362 R0.42
G1 X12.8396
G3 X12.792 Y39.028 R0.1425
G1 Y39.0448
X12.8019 Y39.0495
G3 X12.8396 Y39.0442 R0.135
G1 X13.0324
G3 X13.0335 Y39.0287 R0.4125
G1 X12.8396
G3 X12.7845 Y39.0169 R0.135
G1 Y39.0559

[timlkallam]

Mat be no spindle speed and no feed rate. may be T16 M06

[sinha_nsit]

Which program M06 is calling?
Are you calling tool-change macro by M06 or a T-code?

[gwarble]

i think you're program is flawed no matter what...

if you're using program o9000 as the macro, then the T-code is calling it and you shouldnt have an M06

if you're using macro program either o9001-o9009 (case A) or o9020-o9029 (case B) then you need to either call the T-code before the M06 or simultaneously with the M06

CaseA: toolchange macro is a subprogram, so you can call T6;M6; or T6M6; or M6T6; and the macro uses the system's T-code (internally system var #4120)

CaseB: macro mode, so the call most likely has to be M6T6; or T6;M6; but not T6M6 (as the macro is ran without a T argument (ie T#0) and the T6 is processed after the macro, at least in my experience on fanucs 0-MC and later

hope that helps, otherwise, do as others requested and post your macro's program number, the macro itself, or your 6050+ params

- gwarble

[mrneelix]

Hi everyone!

Finally got an answer to the issue from Anderson themselves.

The Tool Change macros that I used (O9000 and O9004) were the right ones and were not the reason for the continuing issue.

They took a look at the program and agreed with timlkallam...I went back in through the program and realized that in the mess one of the times it got resent to the controller the spindle speed and feed rates had zeroed....once I added them back in it worked like a charm!

As to your question gwarble, I am not sure why the M06 calls the tool even though the macro is O9000...the macros I used came with the documentation on the unit so I am not sure if there is a conversion going on in the post processer or...? I know that we use the T# when we select the tool and because of the changer it winds up being Tool 1 = T11, Tool 2 =T12, etc...maybe that has something to do with it?

Thank you all for your help and suggestions....you have no idea how great it is to have people that I can ask when these little "gremlins" pop up

Cheers!

[sinha_nsit]

An ordinary T-code does not change the tool on a milling machine. It has to be used with M06.
You may call O9000 by a T-code. But it does not disable M06 on a milling machine. In fact, O9000 would still use M06 for tool change (M06 T#149) on a milling machine. (Note that a T-code inside O9000 is treated as an ordinary T-code; it would not cause circular reference.)

Edit:
If you have already used M06 in the O9000 calling-block (e.g., M06 T20), M06 in 9000 may not be needed. The other way would be to use just T20 in the calling block, and include M06 in O9000.