Additional information after M30 code?

[cossiegaz]

What do i need to alter to allow my Fanuc Oi-MC controller to read in additional lines of programme after the M30 code?
The reason i ask is that i would like to add a renishaw probing cycle after the M30 in the programme so we can just search down to it and probe the tools straight away then have this cycle ignored when running the main programme due to it being after the M30, this will save us a hell of a lot of time on set-ups as we would no longer have to write out a probing cycle every time we set up a job.
Currently, when reading a programme into its directory the machine will stop reading when it sees an M30, is this due to the way the Fanuc controller is set up? i.e a parameter setting? Or is it to do with the set up of the system that sends the programme to the machine? We use a "Seiki" system if that means anything to anyone.

I know i could add it into the main programme and use block skip but some of our programmes already use block skip for other reasons and i dont really want to have to create seperate probing programmes either, would be far simpler to just keep it all in one programme, i have operated other machines that will read information after the M30 code.

[psychomill]

Never tried reading beyond M30 on a O control but there are many controls that can read past M30. Not sure on the O control but many do have a parameter that can shut off the I/O at the M30/M2... even M99. On most, you can switch this to a timer shut off value for when the control stops seeing a data flow. It can also be on the DNC side. Many DNC systems have similar parameters for turning off the I/O.

"probe the tools" ... so I take it this a tool setter? Why not just have a generic program that stays in the machine to set tools with instead of being in the part program? A relatively simple macro could accomodate to any tool count depending on the set up. Or just keep the probing program seperate of the part program and bring it in the machine like its a sub program. The operator just simply runs the program by itself then switches to the part program for the operation.

If you have macros then you could do this by a counter. Have a variable control whether or not the probing routine gets run. Once the probe cycle runs, it sets a number. When the control gets there, it simple looks at the variable then "GOTO" to a block number to skip the probing routine or sub call.

[dcoupar]

I believe Parameter 3201 bit 6 is what you're looking for. Try setting it to 1.

[cossiegaz]

There is a generic program that stays in the machine but it has to be hand edited each time we set a job to suit whatever tools we are using, this takes up valuable machining time. And to have a seperate programme would mean having to get the programming department to create a seperate file in the DNC for every different part that we manufacture and as we make so many different parts they quite simply cannot be bothered to go through and do this.
Having the cycle after the M30 is definitely the easiest way as it is just a case of me editing the cycle on the end of the programme and returning it to the DNC.

dcoupar, thanks for the information, how easy is it to alter this parameter, i have very limited experience of parameter alteration having only seen other people do it a few times before

[dcoupar]

In MDI, go to OFFSET/SETTING, then [SETING], then cursor to PARAMETER WRITE = and key in 1 then INPUT. You'll get an alarm... ignore it.

Press SYSTEM, then [PARAM], then key in 3201 and [NO. SRH]

Parameter bits are numbered left to right: 7 6 5 4 3 2 1 0

Cursor right to bit 6. Key in 1 and INPUT.

Go back to OFFSET/SETTING and set PARAMETER WRITE = 0. RESET the alarm and try to load your program.

[stevo1]

Cossiegaz,
So what you are saying is you don't have a standard way of touching off a tool? You setup your tools around a specific part? Why would you have to edit the tool touch off program?

A tool lenght is a tool length. If you put a tool in the machine and touch it off you should never have to offset it again unless it is crashed or worn. If you probe every tool in your machine all you would have to do is specify the part height in the program and run. If you put a different part on, the tool length should remain the same. An 6" long spot drill is 6" long no matter if your part is 1" tall or 100" tall.

Stevo

[Boots]

Have you thought about ending your part program with an M00 ? This is a dwell till you hit cycle start again. Write your edits and end with an M30. go back to the M00 and hit cycle start 2 times. There ya go.....on yer way.

[ChattaMan]

You could always use a goto statement.....

O0001
M6T1
.....
your prog
.....
G53Z0Y0
GOTO999
N1
your probing prog
N999 M30

Search for N1 to do probing
Running machining prog will "skip" probing prog.

[cossiegaz]

Thanks dcoupar, i shall try this when i am back at work.

stevo1, What i am saying is that we have a tool probing cycle that stays in the machine all the time, when setting up a job we would go through and edit this cycle to suit the tools in the job being set so if tool 1 was an 80mm square corner facemill without cutter compensation we would edit the probing cycle to offset the tool by 40mm and probe the length then after running and completing that job we would then set up the next job - a completely different part which would be using completely different tools so tool 1 could now be a 20mm endmill using cutter compensation so we would have to edit the probing cycle to offset the tool by 10mm to probe the length and then to move over and go down the side of the probe to measure the diameter of the tool, i want to have a probing cycle in the main programme after the M30 to suit the tools in that programme so as not to have to write one out every time that particular job is set up.

Boots, we did try this but the problem with this was that you would either have to re-set to the beginning of the programme once you reached the M00 at the end or alter it to an M30 which is what i think you are suggesting, this worked fine until it came to having to return the programme to the DNC if any edits had been made to the main programme, operators were forgetting to change the M30 back to M00 before returning the programme and the probing cycle was then lost as it would not return to the DNC because it was after an M30.

ChattaMan, I am not familiar with using GOTO commands, am i right in thinking that you are saying everything between the lines "GOTO999" and "N999M30" will be ignored? If this is the case and if i have no luck with the advice dcoupar has given me then your suggestion sounds like something that may be a good option.

Thanks for all the replies.

[g-codeguy]

Originally Posted by cossiegaz ChattaMan, I am not familiar with using GOTO commands, am i right in thinking that you are saying everything between the lines "GOTO999" and "N999M30" will be ignored?

That is exactly what it means. When the control reads a GOTO statement, it jumps to the block in the GOTO statement ignoring everything in between. Very useful in your case. You wouldn't have to mess with setting any parameters either.

[Superman]

Why not leave your probing in the correct spot in the program, and insert a Block Skip at the front of the codes used in probing

block skip ON when running a program will miss any probing

or

use a "JUMP" or "GOTO" with a block skip
eg

/N1 GOTO N999
N2 M00
.... (probing)
M01
()
N999
T1 M6
... ( your program)
...
M30

Block skip ON = do probing, then do program ( miss reading line #N1 )
block skip OFF = do program only

2nd version may be best, as a default, when machine is fired up in the mornings, all switches are OFF, and the probe won't be called out accidently.

[beege]

Remember that M99 does the same thing as GOTO in the main program.

In other words
In a main program

M99P3 == GOTO3