Problem- Restarting Fanuc 21i-TB in prog middle or after tool break

[underdog]

Hi. Thanks in advance for the help!

We purchased a new lathe with Fanuc 21i-TB controller. Question is; if we want to stop the operation and pull the tool away to check/change it and then restart (or as our G&L's say, "toolpath recovery", that recovers and re-enters the same cut perfectly) - How do we do it?

I can't believe 1980's G&L's and Mazaks have a feature that 2009 Fanuc's do not, but the field engineer is a great mechinical guy, but not an operator or programmer.

[Capt Crunch]

Hi Under dog

what i do is have N001 at the first toll and N002 for the 2nd tool and so on down thru my program. if i have to restart in the middle of a toolpath, reset prgm, type in the N00?? that you need to go to, forward search. this tells the machine where it is and such. SINGLE BLOCK on, then cycle start 'til it reads the tool offset (T0101) for example, and the G96S????, without resetting the program, go into edit and bring up the
program and search for where you need to resatart your tool, go into memory and single block for the first few lines and if it looks good, let'er go. that is what i do for our 20 T control. on our Oi control, search for the N???? have it read the T???? and G96, turn selector knob to edit and simpley scroll down to where i want to statrt again, turn selector to memory and single block to make sure everything looks safe then go full auto. hope this helps.

Cheers
Gerry

[underdog]

Thansk - we'll give it a whirl!

[cossiegaz]

You should find that the method given by Capt Crunch will work perfectly, although is only really needed if you have had to come out of the program and press 're-start' which will cancel any offsets and codes that are active which you will probably have to do if it is neccessary to replace your tool.
You should also be able to single block it mid-cycle, wait for it to reach the end of the required block, then go into 'jog' or 'manual' mode, press 'spindle stop' open the door move the tool away and check whatever you want to check, then if all is O.K just close the door, re-start the spindle, go back into 'auto' mode and press cycle start, the machine will know where it is as it should have a 'manual absolute', be careful though as under some circumstances you may have to handwheel the tool back to where it was before you moved it away which is the safest way of using this technique anyway (just zero the 'relative' figures before moving tool away) and then press cycle start, this will depend on what positional information is specified on the next line in the program, also if a G01 is still active then you will have to wait for it to feed all the way back to the job so in this case you would be better off moving it closer back to the part before pressing cycle start.

[Dan Fritz]

I don't know if you have the option or not, but even the old Fanuc 6 controls had a "Program Restart" feature. You could search to any point in the program, and while doing this, the control would scan the program and remember the last executed M-code, S-code, T-code, tool offset, and all the modal G-codes. When you pressed Cycle Start, it would pick up from the middle of the program. You may want to look in the table of contents of your operator's manual for "Program Restart" and see if you have it.

If you press RESET on any Fanuc, it not only dumps the 1-block buffer in memory, but it also sets all the G-codes back to their initial state and cancels tool offsets. That's why a "Program Restart" feature is nice to have. Once you stop a program and press RESET, you can't just do a simple search to that spot and start again. There are many parameters that affect how RESET works also, so not all machines are going to be the same.