[dung_ninhbinh]

Hello everyone!
I am Nguyen from Vietnam. Who can help me repair some problems? My CNC’s serial is Fanuc 18M. (Anderson Industrial Corp)
Machine Type: NC-2525TC2+G/PT
Machine Number: FAANCPT92077
I have machine’s parameter. The last time, machine had an error 915 SRAM PARITY and I repaired it. But after, when I write M100 (Call subprogram waiting) then “078 NUMBER NOT FOUND” message on screen. I can not use M100 code.
M00, M01, M02, M03, M11, M12…. M98, M99... OK. Problem with M100 code.
0078 NUMBER NOT FOUND on help menu description:
“Function: Subprogram call
Alarm: the program number or sequence number designated by P in block M98, M99, M65, and M66 cannot be found. Or sequence number designated by goto cannot be found.”
What can I do now? Can you help me?
And I need file post processor for CNC FANUC Oi-TC in AlphaCAM, who can share for me?
Thank you very much!

[bborb]

Possibly when you repaired the SRAM you lost parameters and the option parameter for subprograms was not turned back on. I do not know which parameter that is.
Hope this helps.

[dung_ninhbinh]

Hi Frank,
My CNC change tool Ok. It has two spindles and change tool by ATC arm. M06 enable vacuum for Y table, M07 disable vacuum for Y table. M08, M09 for V table. M05 change tool for two spindle. M51 change tool spindle number one. M53 change tool spindle number 3. I think O9001 is a system program, when i format the RAM and upload data then disable this program i will test to enable it on parameter 3202 bit 4. Tell you later. Thank you.

[sinha_nsit]

I have not seen the use of M100. What does it do? Possibly it is machine specific.

If M98/M198/G65/G66 are working, it should be enough.

[dung_ninhbinh]

hi all,
I checked parameter 3202 and change bit 4 to 0. But have not O9001 in my memory. Can you show me how to write this program? Can i get it?
Thank you very much.
M00: STOP, M01: STOP, M02: STOP, M05: CHANGE TOOL(2 SPINDLES), M06: ENABLE VACUUM NUMBER1 TABLE, M07: DISABLE VACUUM M06, M08: ENABLE VACUUM NUMBER2 TABLE, M09: DISABLE M08, M11: SPINDLE 1 DOWN, M12: SP1 UP, M13: SP1 ROTATE CW, M14: CCW, M15: TURN OFF SP1, M21: SPINDLE 2 DOWN, M22: UP, M23: ROTATE, M25: SP2 TURN OFF (NUMBER2 IS A SAW). M30: FINISH PROGRAM, M31: SPINDLE 3 DOWN, M32:UP, M33: ROTATE CW, M34: CCW, M35: TURN OFF SP3, M40: Y&V OPERATION NORMAL, M50 AND M60 (FOR M100), M51: CHANGE TOOL NUMBER1, M53: CHANGE TOOL NUMBER2, M56: ENABLE PIN 1 AREA, M57: DISABLE M56, M71: SP1&SP3 DOWN, M72: UP, M73: ROTATE CW, M74: ROTATE CCW, M75: TURN OFF, M92: ALL SPINDLE UP, M95: ALL SPINDLE OFF, M98: CALL SUBPROGRAM, M99: FINISH SUBPROGRAM (REPEAT).

[dung_ninhbinh]

Hi FrankCNC,
Thank you for your help,
I wrote program from your information, i post here
That is Macro to change table for Fanuc 18M
%
O9001
IF[#1003 NE 1] GOTO100
N5 IF[#1000 EQ 1]GOTO10
IF[#1001 EQ 1] GOTO10
IF[#1101 EQ 0] GOTO5
G91 G09 G00 Z[0-#5023]
G91 G09 G00 X[#501-#5021]
G04 P300
GOTO5
N10 G91 G17 X0 Y0
M50
#1101=1
#1102=0
M60
M99
N100 IF[#1000 EQ 1] GOTO120
IF[#1001 EQ 1] GOTO130
IF[#1101 EQ 0] GOTO100
IF[#1102 EQ 1] GOTO110
G91 G09 G00 Z[0-#5023]
G91 G09 G00 X[#501-#5021]
G04 P300
GOTO100
N110 G91 G09 G00 Z[0-#5023]
G91 G09 G00 X[#502-#5021]
G04 P300
GOTO100
N120 G91 G17 X0 Y0
M50
#1101=1
#1102=0
M99
N130 G91 G17 X0 V0
M60
#1101=1
#1102=1
M99
%

[FrankCNC]

Hi Nguyen,

Good to hear you've been successful, I'm surprised that the User Inputs for the Daewoo are the same as the Anderson, I would have thought they would have been machine specific. I only listed them as a guide to show what to look for in you Anderson literature and machine.

I worked out the Pallet User Inputs for our machine by going into CNC/PMC then PCDGN then searching for UI31.G to bring up the User Input screen then seeing which User Inputs changed from 0 to 1 or 1 to 0 when I changed the pallets on the machine.

Regards,
Frank.

[dcoupar]

Maybe M100 is an macro or subprogram call, and the program it's calling is no longer in memory?

Check parameters 6050-6059, and 6080-6089 to see if one of them = 100.

6050 > O9010
...
...
6059 > O9019

6080 > O9020
...
...
6089 > O9029

[sinha_nsit]

Maybe M100 is an macro or subprogram call, and the program it's calling is no longer in memory?
...
...

This is the only possibility.

If he is not sure what the macro/subprogram called by M100 is supposed to do, he possibly does not need to use M100.

[dung_ninhbinh]

I will check parameter. M100 is a macro. I use it for subprogram.
M100 call subprogram. I write a program when use M100 follow:
O7000 (MAIN PROGRAM);
M100;
IF [#1102 EQ 1] GOTO1000;
M98 Pxxxx (PROGRAM FOR Y TABLE);
M99;
N1000;
M98 Pxxxx (PROGRAM FOR V TABLE);
M99;
that is M100 in my program, i dont know to repair this problem. Sometime i use this code on top program when i do on a table to wait ready button. M100 is a macro line. If i use it, i can do auto. We work on 2 table and program run if one of 2 tables ready.
I will check parameter 6050-6089 and tell you later
Thanks alot

[guru]

Do you have pallet changer on that machine?, that #1102 must be for checking pallet or table number. Can you post last few lines of sub Pxxxx.

[dung_ninhbinh]

i just check parameter, do you know to modify the PLC? What can i do now?

PARAMETER (CUSTOM MACRO)
6030 SUB CALL (FLPY) 0
6031 0
6032 0
6033 0
6034 0
6035 0
6036 0
6037 0

6050 MACRO CALL G 0
6051 0
6052 0
6053 0
6054 0
6055 0
6056 0
6057 0
6058 0
6059 0

6071 SUB CALL M 100
6072 101
6073 0
6074 0
6075 0
6076 0
6077 0
6078 0
6079 0

6080 MACRO CALL M 0
6081 0
6082 0
6083 0
6084 0
6085 0
6086 0
6088 0
6089 0
6090 SUB CALL ASCII 0
6091 0
6092 0

[dcoupar]

M100 is calling program O9001 - is this program stored in memory? If not, M100 will cause alarm 078.
M101 is calling program O9002 - is this program stored in memory? If not, M101 will cause alarm 078.

[dung_ninhbinh]

Hi Dcoupar,
Can you show me about that program? 9001 and 9002. My memory is empty.
Thanks

[dcoupar]

Your 9000 programs may be hidden? Check parameter 3202 bit 4. If it's 1, then the 9000 programs are locked. Change it to 0 and see if programs O9001 and O9002 are in the memory.

What should M100 and M101 do on your machine?

[dung_ninhbinh]

Dear Dcoupar,
M100 and M101 use to call subprogram. That code on the top of program. When use it, it wait we push OK button on the table then machine will run. Repeat program until finish item i want to do. (999999999 times ok)

[FrankCNC]

Hi Nguyen,

O9001 macro should be the tool change macro which is normally called with M06,
Parameter #7071 is the M code used to call macro program O9001

O9002 macro should be the pallet change macro which is normally called with M60,
Parameter #7072 is the M code used to call macro program O9002

Macro Programs O9001 & O9002 must be in your machines memory.

Do you have a backup copy of your machines macro's that you can reload into the machine.

[FrankCNC]

,
M100 and M101 use to call subprogram. That code on the top of program. When use it, it wait we push OK button on the table then machine will run. Repeat program until finish item i want to do. (999999999 times ok)

Hi Nguyen,

Is M100 used to call a subprogram which checks which Table is setup and ready to be machined.

On our twin pallet machine when the operator has finished setting up the job on the pallet not being used by the machine the 'Setup' button needs to be activated so the machine knows it can change pallets and carry on machining on the new pallet.

This is controlled in our pallet change macro O9002 by user input #1020, if #1020=1 pallet is setup, if #1020=0 machine waits till pallet setup button has been pushed before continuing.
N30 IF[#1020 NE1]GOTO30 (Loops until setup button pushed).

It's possible M100 only calls a subprogram which checks if a table is ready to be machined by checking which tables vacuum is enabled (only a thought).

It would then be a matter of checking user inputs/outputs in the PMC to see which variables are used for function checks and then writing a subprogram
to do these checks and associate M100 to call this subprogram.

Hope this helps,
Frank.

Below is a list of User Inputs/Outputs from our machine that might give you a hint on what to look for.

DAEWOO ACE H-100 USER DATA INPUTS.

G051.0 UI00.G #1000 APC MACRO START/FINISH

G051.1 UI01.G #1001

G051.2 UI02.G #1002 PALLET ON B AXIS

G051.3 UI03.G #1003 PALLET #1 ON CHANGE TABLE

G051.4 UI04.G #1004 PALLET #2 ON CHANGE TABLE

G051.5 UI05.G #1005

G051.6 UI06.G #1006 B AXIS SECOND REF POINT RETURN IN POSITION

G051.7 UI07.G #1007 MACHINE LOCK SWITCH

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

G050.0 UI08.G #1008 AUX FUNCTION LOCK SWITCH

G050.1 UI09.G #1009 REPEAT SWITCH

G050.2 UI10.G #1010 ATC TOOL CHANGE SECOND REF POINT RETURN IN POSITION

G050.3 UI11.G #1011 APC REF POINT RETURN IN POSITION CHECK

G050.4 UI12.G #1012 APC CHANGER 1/5 SELECT

G050.5 UI13.G #1013 APC NOT INITIAL CHECK

G050.6 UI14.G #1014

G050.7 UI15.G #1015

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

G049.0 UI16.G #1016 AUTO B AXIS CLAMP/UNCLAMP SELECT

G049.1 UI17.G #1017 360 ROTATE B AXIS SAME COMMAND

G049.2 UI18.G #1018 360 ROTATE B AXIS CCW DIRECTION

G049.3 UI19.G #1019 ATC MACRO START/FINISH

G049.4 UI20.G #1020 SETUP BUTTON CHECK

G049.5 UI21.G #1021

G049.6 UI22.G #1022

G049.7 UI23.G #1023

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

G048.0 UI24.G #1024

G048.1 UI25.G #1025

G048.2 UI26.G #1026

G048.3 UI27.G #1027

G048.4 UI28.G #1028

G048.5 UI29.G #1029

G048.6 UI30.G #1030

G048.7 UI31.G #1031



DAEWOO ACE H-100 USER DATA OUTPUTS.

F051.0 UO00.G #1100 APC MACRO START

F051.1 UO01.G #1101 APC MACRO START

F051.2 UO02.G #1102

F051.3 UO03.G #1103 AXIS APC POSITION/APC POSITION

F051.4 UO04.G #1104

F051.5 UO05.G #1105

F051.6 UO06.G #1106

F051.7 UO07.G #1107

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

F050.0 UO08.G #1108

F050.1 UO09.G #1109

F050.2 UO10.G #1110

F050.3 UO11.G #1111

F050.4 UO12.G #1112

F050.5 UO13.G #1113

F050.6 UO14.G #1114

F050.7 UO15.G #1115

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

F049.0 UO16.G #1116

F049.1 UO17.G #1117

F049.2 UO18.G #1118 ATC MACRO END/ATC MACRO START

F049.3 UO19.G #1119 ATC MACRO START

F049.4 UO20.G #1120 PALLET SETUP BUTTON CANCEL AUX

F049.5 UO21.G #1121

F049.6 UO22.G #1122

F049.7 UO23.G #1123

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

F048.0 UO24.G #1124

F048.1 UO25.G #1125

F048.2 UO26.G #1126

F048.3 UO27.G #1127

F048.4 UO28.G #1128

F048.5 UO29.G #1129

F048.6 UO30.G #1130

F048.7 UO31.G #1131

[MysticMonkey]

Your home made macro works then, did the manuals help ?

dung_ninhbinh

Contact your local Doosan CNC dept,
DOOSAN MECATEC Co Ltd.
DOOSAN VINA (CPE PLANT)
DUNG QUAT ECONOMIC ZONE
BINH THUAN BIN SON
QUANGNGAI PROVINCE, VIETNAM

TEL: 84 553 618 900
FAX: 84 553 618 955


They need to know
1. Machine Model number
2. Machine Serial number
3. Control Model

Tell them that you have lost all 9000 macros and please help to get new ones

[sinha_nsit]

Why do you insist on using M100? The program it is referring to appears to have somehow got deleted from your machine. Nobody can write it for you because others do not know what it was doing. So, use M98/G65 for calling subprogram/macro. Analyze your list of M-codes on your machine, and command as required.