Fanuc 6t control won't start program again

[MaintManAndy]

Hi everyone,

I have a Hitachi Seiki 3NE 300 with a Fanuc 6T control. We have had no problem with it for years, but it's been pointed out to me that this machine does not want to start the program from the beginning now, despite there being an M30 at the end of the program.
Once the program has finished, you can open the door to swap jobs perfectly well. But you cannot cycle start and start the program again. Switching off the machine solves this issue but is not ideal.

Any help is much appreciated.

Thanks in advance

 

[sinha]

This is unusual. Check if M02 works.

 

[MaintManAndy]

I will try that tomorrow, the awkward part is that we haven't had any previous problems with the M30 code.

 

[DouglasJRizzo]

Make sure there is a ";" after the M30 and a "%" at the bottom of the program.

 

[Vancbiker]

This is probably caused by the completion conditions for M30 not being met. Those conditions are determined by the machine builder and HS were good at making simple things complex.

 

[MaintManAndy]

Make sure there is a ";" after the M30 and a "%" at the bottom of the program.

Yep, both of those are in the program, everything with the program seems to be ok, and has been for a while. The program jumps back to the start, and after loading a new job in, it won't then start the program again.

 

[DouglasJRizzo]

Any alarms?

 

[beege]

Is there a parts counter comparing cycles complete with cycles needed?

 

[wrustle]

Is your door switch not working correctly preventing the program from running?

 

[sinha]

Can you run a small MDI program?
Cycle start button remains green?

 

[MaintManAndy]

Can you run a small MDI program?
Cycle start button remains green?

Yes, there's two main programs in the machine, let's call them 1 and 2. Program 1 can run and will run over and over again, hand loading new jobs, clamping/unclamping Chuck and tailstock. But program 2 will finish the program, jump back to the beginning, but then won't start the program.

 

[MaintManAndy]

Is your door switch not working correctly preventing the program from running?

We have another program that will run perfectly fine. It will begin cycle again after hand loading a new job. It's the current program we are having trouble with

 

[wrustle]

Why don't you post the first few lines of code on your program along with the last few lines for everyone to look at for issues?

If it's not a large program, post it all.

 

[sinha]

If all the problem is with a particular program only, then the problem is not with the machine.

 

[MaintManAndy]

Why don't you post the first few lines of code on your program along with the last few lines for everyone to look at for issues?

If it's not a large program, post it all.

Ok, here goes.

O2000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z46.5 F.12 M08 ;
G00 X40. Z253. ;
.....

So then it's cut, cut, cut, change tools, cut, cut, cut etc.

.....
T0909 ;
M03 S90 ;
X40. Z253. M08 ;
G01 X17.7 F.25 ;
G01 X18.4 Z250.1 F.1 ;
G28 U0 W0 M05 ;
M09 ;
M30;
%

 

[MaintManAndy]

If all the problem is with a particular program only, then the problem is not with the machine.

I agree, but comparing this to program O1000, which runs perfectly, it is not much different.
O1000 goes as follows.

O1000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z38. F.15 M08 ;
.....

.....
T0505 ;
M03 S80 ;
G00 X21. Z184.7 F.25 ;
G01 X16.1 F.1 M08 ;
G01 Z103.7 F.25 ;
G00 X21. Z184. ;
G01 X13.3 F.1 ;
G01 Z103.7 X13.5 F.25;
G00 X100. Z253. M05 ;
G28 U0 W0 M09 ;
M30;
%

 

[sinha]

So, essentially you are saying that O2000 runs perfectly for the first time, but does not run thereafter unless you cycle power.
Please run it block-by-block and check where it stops.

 

[angelw]

I agree, but comparing this to program O1000, which runs perfectly, it is not much different.
O1000 goes as follows.

O1000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z38. F.15 M08 ;
.....

.....
T0505 ;
M03 S80 ;
G00 X21. Z184.7 F.25 ;
G01 X16.1 F.1 M08 ;
G01 Z103.7 F.25 ;
G00 X21. Z184. ;
G01 X13.3 F.1 ;
G01 Z103.7 X13.5 F.25;
G00 X100. Z253. M05 ;
G28 U0 W0 M09 ;
M30;
%

The FS6 control and others of that period, the axes slides would move the amount of the registered X and Z offset if the offset was applied when calling the tool, as in your case. If the control happened to be in G01 and Feed Per Revolution Mode when the tool was being called, then the axes slides can't move and therefore, the program will appear not to be running.

In the program you have listed in your Post #15, the last Block before the G28 Reference Return is a Linear Interpolation Block (G01 X18.4 Z250.1 F.1); and therefore, the control will be in G01 mode when an attempt to start the program again. At the beginning of that program, Feed Per Revolution Mode has been specified, therefore, the Axes Slides can't move the Offset amount and the program will appear to have stalled.

In Program O1000, the last Block executed before the Reference Return Block is a Rapid Traverse movement (G00 X100. Z253. M05) and therefore, when the program is attempted to be started again, the control is in G00 Mode. In this case, there is no requirement for there to be a specific movement Block, nor for the spindle to be running and therefore, the Axes Slides will move the amount of the registered offset in Rapid Traverse mode, with the program running as normal.

The reason the first program can be made run again by cycling the power to the control, is that there are certain "G" codes that can be set via parameter to default when the control is turned on. In the case of your control, when the control is turned on, one of the default "G" codes is G00.
If you were to add G00 to the first Block in the program, as in the following example

G00 G21 G40 G99
that will fix your problem. However, a better solution is to include G00 in your Tool Call Up Block as in the following:
G00 T1111

When I was teaching clients programming and use of 6T controls, I disliked calling the new tool and its offset at the same time. The reason is that the axes slides would be moving during the Tool Change action. My preferred method was to call the new tool without the offset and then apply the offset during the next movement block as in the following example:

G50 X200. Z300. ;
G00 T1100 ;
G96 S80 M03 ;
G00 Z253. T1111;

In this way, there is no slide movement during the tool call up and the offset is applied seamlessly in the first movement Block.

Try any of the above suggestions and I suspect that you issue will be solved.

Regards,

Bill

 

[MaintManAndy]

If all the problem is with a particular program only, then the problem is not with the machine.

I agree, but comparing this to program O1000, which runs perfectly, it is not much different.
O1000 goes as follows.

O1000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z38. F.15 M08 ;
.....

.....
T0505 ;
M03 S80 ;
G00 X21. Z184.7 F.25 ;
G01 X16.1 F.1 M08 ;
G01 Z103.7 F.25 ;
G00 X21. Z184. ;
G01 X13.3 F.1

Ok, here goes.

O2000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z46.5 F.12 M08 ;
G00 X40. Z253. ;
.....

So then it's cut, cut, cut, change tools, cut, cut, cut etc.

.....
T0909 ;
M03 S90 ;
X40. Z253. M08 ;
G01 X17.7 F.25 ;
G01 X18.4 Z250.1 F.1 ;
G28 U0 W0 M05 ;
M09 ;
M30;
%

G01 Z103.7 X13.5 F.25;
G00 X100. Z253. M05 ;
G28 U0 W0 M09 ;
M30;
%

Ok, here goes.

O2000
G21 G40 G99 ;
G28 U0 W0 ;
G50 X200. Z300. ;
T1111 ;
G96 S80 M03 ;
G00 Z253. ;
T1111 ;
G00 X50. ;
G01 X32. F.5 ;
G01 Z46.5 F.12 M08 ;
G00 X40. Z253. ;
.....

So then it's cut, cut, cut, change tools, cut, cut, cut etc.

.....
T0909 ;
M03 S90 ;
X40. Z253. M08 ;
G01 X17.7 F.25 ;
G01 X18.4 Z250.1 F.1 ;
G28 U0 W0 M05 ;
M09 ;
M30;
%

So the program on cycle 2 gets hung up on on the 1st T1111 of the program. No alarms on display.

So, essentially you are saying that O2000 runs perfectly for the first time, but does not run thereafter unless you cycle power.
Please run it block-by-block and check where it stops.

Yes, on the second run, it stops at the 1st tool call ' T1111 ;' in the program

 

[sinha]

Can you execute T1111 in the MDI mode?