Issue with FANUC 18i-M controller

[TeleGuy]

Our shop has a Machining Systems HMC 200 with a FANUC 18i-M controller. The problem I'm having is intermittently the machine will read the values in the G10 offsets lines in the program but when you look at the work offset screen, the values will be tripled. The machine most often will over travel at this point. Hitting reset and reading the G10 lines again will most always resolve the issue for that instance.

Has anyone seen this type of issue before and have any suggestions for what is causing this? Every program has a M30 at the end and the programs all go back to the top.

[dcoupar]

Do you have a G90 in the G10 block?

Maybe you could post your program here.

[TeleGuy]

The G10 blocks are written as:

G10L2P2X...Y...Z...


A sample of the way the programs are written is like:

G10L2P2X...Y...Z...
G10L2P3X...Y...Z...
G10L2P4X...Y...Z...
G10L2P5X...Y...Z...
T1M6
G04P100
S300M3
G90G55G0X...Y...T48
G43Z.5H1
G81Z-1.5F2.M8
G0Z15.M9
M6
G91G28X0Y0Z0
M30

Thanks for your reply dcoupar!

[stevo1]

What Dave is getting at is there a possiblility that you are in G91 incremental mode before the G10 lines are read? If you were then this would add to the existing numbers that are already in G54-G57. Then by resetting the program it will default back to G90 and read the proper values.

Also are the X...Y...Z... hard numbers or are they being set by variables ex X#100Y#101Z#102?

Stevo

[TeleGuy]

Ok That makes sense being in incremental. I think I'll try a G90 before my M30 and see what happens. And yes Stevo, those are hard numbers. Thanks guys for your help so far!

[Jaxbubba]

Always hard copy in your post a Clear Block to cancel everything and start from new. Example for head of program. Do this before every tool change and you won't have any problems.
O0001:
G00G40G80G90:
This cancels any leftover cutter comp, canned cycles, and puts the control back in absolute. Then do your tool change, and run the program.

[christinandavid]

Safest to put in G90 G10 for each instance. You never know where G91 might be lurking (eg our M6 macro used to finish in G91 mode as it had a home positioning move at the end).

DP