[sm2000]

Hello all, I hope someone can help me with this problem?

First - I had an 101 PS alarm and was able to clear this alarm

101 PS = while writing to part program the power was turned off (didn't happen but this alarm just showed up)

Second - I then recieved a 078 PS alarm

078 PS alarm = A program number or a sequence number which was specified by address P in the block whcih includes an M98, M99, G65 or G66 was not found

1- I just noticed that all my part programs have been deleted
2- I reloaded the part program in the machine
3- I then recieved the 078 PS alarm still
4- went to MDI and called up a manual tool change M6T# and then recieved the same alarm
5- I am assuming that the tool change macros where probably lost as well?
6- I do not have any back ups of the macros
7- does anyone know what could cause this? The 09000 programs are hidden, I have been reading on how to turn off the write protect.
8- If the O9000 programs are lost - does anyone have a copy of this or do I have to call fanuc?
9- I would really appreciate it someone could help me with this.
10- are there any other macros that I need (more than 1 O9000 programs)

2000 YCI Supermax Rebel
20 tool changer umbrella style
Fanuc om control
just a basic 3 axis machine

If I am in the wrong forum then I aplologize

[dcoupar]

I would check parameter #230 through #239. One of them should contain a 6 or 06. Let/s say #239 is 6. That means that the tool change macro that runs when M6 is called should be O9029. If #233 is 6, then it would be O9026.

Then check parameter #10 bit 4. If it is set to 1 then you can't edit programs 9000 through 9999.

You have to be in MDI to change parameters. First go to SETTING, then page down until you see PWE (Parameter Write Enable). Change it to 1; you'll get an alarm but ignore it. then go to SYSTEM - PARAM page down until you find 0010, then set bit 4 to 0 (they're numbered 76543210). Now go back to settings and turn off PWE.

If you don't see O9029 in the directory you'll have to create one.

I think for the Rebel it should be something simple like:

O9029 (ATC MACRO)
G91 G28 Z0
T#20 M06
G90
M99

Once you've got it working, be sure and set parameter 0010 bit 4 back to 1 to lock the 9000-9999 programs.

[sm2000]

thank you very much - I will give it a try today

[sm2000]

-I tried and entered the the information but it did not work

-I found a macro for the tool changer in my fanuc manual but it does not work either? I ended up with a 114 alarm

This is what i found in my fanuc manual - but gets a 114 alarm

%
O9020(20T M6 TOOL CHANGE)
#3003=1
IF[#20EQ#0]GOTO100(WITHOUT T ALARM)
M70T#20(TF CHECK)
G4X0.1
IF[#1008EQ1]GOTO300(TF ON SPINDLE)
IF[#20EQ0]GOTO100(T=0 ALARM)
IF[#20GE100]GOTO90(T-LIFE T3 CODE)
IF[#20GE21]GOTO100(T>MAGAZINE ALARM)
N90IF[#1012EQ1]GOTO101(SP=EMPTY ALARM)
#140=0
#149=#4003
#148=#4001
#147=#4006
G0G91G80G49M19
M6(TOOL CHANGE IN PLC)
IF[#1009EQ1]GOTO10(ATC POSITION 1)
WHILE[#1009EQ0]D01(ATC POSTION 1 CHECK)
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
#140=0
N10M71(MAG. FORWARD)
M72(SPINDLE TOOL UNCLAMP)
WHILE[#1010EQ0]D01(ATC POSITION 2 CHECK)
#140=#140+1
IF[#140GE4.]GOTO98
G30P3Z0
END1
#140=0
M73T#20(MAG.ROTATE)
WHILE[#1009EQ0]D01(ATC POSITION 1 CHECK)
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
M74(SP. TOOL CLAMP)
G#148G#149G#147
M75(MAG. BACK)
GOTO300
N98#3000=20(ATC POSITION 2 ERROR)
N99#3000=21(ATC POSITION 1 ERROR)
N100#3000=22(T/M6 ERROR)
N101#3000=28(SP=EMPTY ERROR)
N300
#3003=0
M99
%

[sm2000]

YCI was pretty good about sending it to me and i posted it below - thanks

%
:9020(20M6TOOLCHANGE)
#3003=1
IF[#1015EQ1]GOTO300
IF[#20EQ#0]GOTO100(WITHOUTTALARM)
M70T#20(TFCHECK)
G4X0.1
IF[#1008EQ1]GOTO300(TFONSPINDLE)
IF[#20EQ0]GOTO100(T=0ALARM)
IF[#20GE100]GOTO90(T-LIFET3CODE)
IF[#20GE21]GOTO100(T>MAGAZINEALARM)
N90IF[#1012EQ1]GOTO101(SP=EMPTYALARM)
#140=0
#149=#4003
#148=#4001
#147=#4006
G0G91G80M19
M6(TOOLCHANGEINPLC)
IF[#1009EQ1]GOTO10(ATCPOSITION1)
WHILE[#1009EQ0]DO1(ATCPOSITION1CHECK)
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0M19
END1
#140=0
N10M71(MAG.FORWARD)
M72(SPINDLETOOLUNCLAMP)
WHILE[#1010EQ0]DO1(ATCPOSITION2CHECK)
#140=#140+1
IF[#140GE4.]GOTO98
G30P3Z0
END1
#140=0
M73T#20(MAG.ROTATE)
WHILE[#1009EQ0]DO1(ATCPOSITION1CHECK)
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
M74(SP.TOOLCLAMP)
G#148G#149G#147
M75(MAG.BACK)
GOTO300
N98#3000=20(ATCPOSITION2ERROR)
N99#3000=21(ATCPOSITION1ERROR)
N100#3000=22(T/M6ERROR)
N101#3000=28(SP=EMPTYERROR)
N300
#3003=0
M99
%

[Thawatchai_Tiw]

Hello all, I hope someone can help me with this problem?
Alarm 078 : Number Not found

For Machine
MNC : MAKINO FNC -128 40A (40tools)
Control : Professional 3