Fanuc Program Restart

[Rocketmachinist]

We have a Laser with a Fanuc control. Does it have program restart like the Haas control. I haven't gotten into it yet but is there a setting I need to turn on?

[huskermcdoogle]

I wish I understood the Fanuc program restart function on most conventional machines.  I have not been able to make heads or tails of it.  My feeling is that there really needs to be some level of MTB integration for it to work, along with proper program format and syntax, plus very specific instructions on how it functions along with its limitations...  Not as simple as the fanucese manuals make it out to be.

I have never used the Fanuc or Haas restart function, though I have used the Okuma sequence restart, it work beautifully.

My best suggestion is to make sure the program is formatted such that you have logical restart points built into the program wherever you might need them.  All modal and non-modal codes needed are applied at these points such that you can safely start the program from those points.

What series Fanuc control is it?  The 30i series controls have a setting that throws a warning message if you aren't starting the program from the top.  Forces you to press cycle start twice.  If you can, I suggest that you enable/use that setting, it is buried in one of the offset/setting pages (operator limits maybe?) (it's not a parameter).

[jeff]

All of the Fanuc controls I've ran (all have been 0 models) the only way to restart was to go into Edit, scroll down to the line you wanted to start at, then back into Auto and Cycle Start from there.

The only issue with that is, your starting points have to have the G54 code, M03, S codes, T codes, etc... 

That's why I have my Fanuc post set up to spit that info out for every toolpath.

 

[Ewood42]

23 hours ago, jeff said:

That's why I have my Fanuc post set up to spit that info out for every toolpath.

 

Pretty sure the "Force toolchange" checkbox does the same thing.

[jeff]

1 minute ago, Ewood42 said:

Pretty sure the "Force toolchange" checkbox does the same thing.

Yes, but doesn't that also spit out an M06? Or is that dependant on how the post is edited?

[Ewood42]

2 minutes ago, jeff said:

Yes, but doesn't that also spit out an M06? Or is that dependant on how the post is edited?

Depends on the post, and the control. On a lot of machines with newer Fanuc controls, if the tool currently in the spindle is called with an M6, it just returns to home, calls all modal commands again,  then continues along. For older controls you could add a logic check in the post that omits the M6 if current tool is same as tool being called.

[Colin Gilchrist]

The restart sequence does vary by control model, and sometimes by vintage of control. I usually Google the specific control and find some good info on Practical Machinist (forum).

Typically on older controls (example: Mazak M-32), you go to the search page, and enter 4 pieces of data:

The Subroutine Number (can be 0), the N Block to search for (required), Block number ("0" typical; any positive number is a number of lines past the N Block), and Number of Loop Repetitions (0 Typical).

Press 'Enter' and wait. And wait. And wait. Eventually the control will display the "previous block number" on the display. Then when you press Cycle Start, the tool will move to the "last position" of the previous block, before the N Block you called.

Due to modality, some codes may not be active, so it helps to go into MDI, and turn the Jog Speed, all the way up. This makes it so the tool moves at 80 IPM, to the previous position, before moving to the called N block.

[Leon82]

On FANUC find the line you want to start on and add a search able character. Could be a comment, n number or even z depth or spindle speed.

 

Single block thru the beginning of the tool path thru the g43 line. Now you can switch to edit and search your comment, or if in the manual guide i. hit n search to go to the n number you added.

 

It will proceed to correctly.

 

If you feed isn't modal or not called out every time you should type it in in mdi before all this.

 

If you don't start in single block it will look ahead and after you search and go back to memory it it will jump back to the top and not work.

 

I do this on the matsuura fanuc controls and regular fanuc controls. Works on tilting work plane too.

[Leon82]

They know how do do it because on a fanuc wire you hit reset then restart and it will continue where it left off.

 

It is probably an option for cancellation machines

 

[Del.]

On 8/18/2018 at 8:42 PM, Leon82 said:

They know how do do it because on a fanuc wire you hit reset then restart and it will continue where it left off.

 

It is probably an option for cancellation machines

 

I love that feature but you must be at the " Hold point return" to do so accurately.

[mkd]

Not aware of Fanuc restart capabiltiy.

GOTO 66

 

N66

.

.

.

.

 

[Tim Johnson]

If I remember correctly, search for the block needed while in Memory mode. You will see the program moving quickly on the screen. When the search stops every modal command is set and ready to go.

[Leon82]

The ihmi control has a button to save restart info, then the utility icon has a restart button.

I'll have to see if it actually works