Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Restarting a long program on a Fanuc


Recommended Posts

Hi All,

 

I am after the forums thoughts on a problem that people would face reasonably often.

 

OK lets say we are running a long die mould program, At a given point the tool extracts from the cavity to reposition itself somewhere else. At this point the operator stops the machine to have a look at the tool. He decides that the tool needs replacing. SO he writes down the programs coords and/or the block number.

 

I generally open the file in the editor and delete the blocks that have been run, rename the file then run the new one, What do you guys do?

Link to comment
Share on other sites

Well On a Haas I use a M97 P??, and I put a N?? in front of the line I want to start at. It will jump down to the line with the N?? in front of it. Make sure to use the M97 after the Modals are started (Fixture, spindle speed, and tool length offset). For safety sake I change my initial Z 2 0r 3" above my part and feed into my part then let it rip.

Link to comment
Share on other sites

What I do on my Fanucs is put a block number in where I want to restart then jump back to the start of that tool. I will then start at the beginning until my G43 is commanded which I stop using single block. Switch to Edit type in the block number I inserted and press the arrow down hard key to jump ahead to my block number. Then switch back to Auto and hit start. Probably is a easier way but this is what I do.

  • Like 1
Link to comment
Share on other sites
Guest CNC Apps Guy 1

Ditto within a thou...

 

Also, I've added GOTOxxxx after the G43 and it will do a program search, slower than within's method, but more automatic. Be sure your G43 is high enough to avoid anything, and make sure you have all the positions you need on the restart line.

Link to comment
Share on other sites

One thing to be careful with using the GOTO approach is if you ever plan to make more then one off. If the operator misses it on the next piece you may find a cutter trying to get through material that is still there before the line you are restarting on which could be over ran using block delete but once again if this program comes up a month down the road I would atleast add a /M00 (make sure block delete is on); Before the start of that tool or you may run into problems. If you add the /M00 and block deleteis on the machine doesnt get stopped and most operators are no more the wise, if it isn't on the machine stops and your operator has a note telling him why you are making him stop.

  • Like 1
Link to comment
Share on other sites
Guest CNC Apps Guy 1

^^^ WHat you could do to prevent that is to set a MACRO variable to 1 manually, then after it executes the GOTO, then reset that MACRO variable to 0 and you won't have to worry. :D

Link to comment
Share on other sites
  • 2 weeks later...

This is on a FANUC control???? Why edit anything in the program? You can use the search function to restart a program anywhere. No need to edit, delete, insert GOTO or anything else. Just write down the line where you stopped at.

 

Then, I just simply go into single block mode at the start of the toolpath, ... single block the program to pick up some codes like work offset, spindle on, coolant on, Tool length, Lookahead.... whatever you need. Then take the machine out of MEMORY mode and go into a HANDLE/jog mode and without pressing anyother keys, type into the control the line information you want to jump to and press the DOWN arrow key (or search down button on i controls), put the control back into MEMORY mode and hit the start button.

 

This is called Manual Interrupt. All FANUC controls can do this.... at least every one that I've used in the last few decades through numerous MTBs. It only takes about 2 seconds and you don't have to worry about leaving behind edits in a program. With Manual interrupt, you jump into sub routines, use toolpaths paths from a totally different tool.... all kinds of stuff. The only thing to be careful of is to not move any of the machine axes unless you need to because the control is not tracking the any changes to axes position in Manual Interrupt. This is another way you can take a "deeper" cut without reprogramming.

  • Like 2
Link to comment
Share on other sites
The only thing to be careful of is to not move any of the machine axes unless you need to because the control is not tracking the any changes to axes position in Manual Interrupt.

 

Not move the axes? Usually your stopping / re-starting to change a tool and thus have to move machine.

Link to comment
Share on other sites
Guest CNC Apps Guy 1

What will happen if you have run 8000 blocks of a 50,000 block program from the HDD/Server? How long will the search take, and will it do it?

It'll do it and it'll take a while.

Link to comment
Share on other sites

I think the "quickest" can be debated.... Certainly you can edit code but you have to get in there and do that. For HDD or DS programs, you'd have to download, edit, reload, restart....

 

You can jump and search inside of HD so for me, this is the quickest and I don't have to change any codes or programs...or worry that me (or someone else) left something behind to mess up the next part. And I hate having a "junk" program simply to restart and finish..... But that's me....

Link to comment
Share on other sites

If you are restarting at the beginning of the tool after your G43 line everything you need should be there. Manual interrupt shouldn't be a worry you are restarting after a reset. But you don;t use handle mode to do this. You use edit.

 

Greg the best way is like Psychomill says a debate. Is this a one off part? or is this a program that will be ran many times? Do you archive all proven programs or just repost them?

 

One off edit the code because who cares. If this is a program you want to archive or rerun, then just add a block number where you need the restart follow the same approach Psychomill explained but do it in edit not handle. If we are talking about speed and limiting mistakes it is a lot easier to add a block number to a program and then search for the block number then it is to write down an entire block on a piece of paper then do a search using the arrow down key.

 

Keep it simple add a block number and follow what I put above. Why mess with a good program. It will take you longer to cut and paste original code, then resave and try to explain this to the operator then it will for the search to take place. Cutting a program up may seem faster but guess what you just cut up your program making it useless for future parts.

  • Like 1
Link to comment
Share on other sites
Guest CNC Apps Guy 1

On an i series FANUC with Manual Guide i program search is much more functional when the program redides on a Dataserver. No Manual Guide i cutting up a program is fastest.

 

 

Link to comment
Share on other sites
Well On a Haas I use a M97 P??, and I put a N?? in front of the line I want to start at.

 

Waste of time. Turn on setting 36. Go to the line you want to start from and hit the button. Just be careful cause it will actually come down a line or 2 before then move into position and go to the Z depth. Use it all the time works flawlessly.

Link to comment
Share on other sites
  • 5 months later...

When I have long program and need to change inserts, I just put the machine on single block mode on some retract move, stop the spinde and zero the relative coordinates to that point, then I can jog the tool to better position, remove the tool and chance inserts, put the tool back, start spindle and jog back to relative zero, change to program mode and continue machining.

 

Does Fanuc 18 i-mb store the line number somewhere when the program is stopped in the middle of the run?

Link to comment
Share on other sites
  • 3 weeks later...

Hi All,

 

I am after the forums thoughts on a problem that people would face reasonably often.

 

OK lets say we are running a long die mould program, At a given point the tool extracts from the cavity to reposition itself somewhere else. At this point the operator stops the machine to have a look at the tool. He decides that the tool needs replacing. SO he writes down the programs coords and/or the block number.

 

I generally open the file in the editor and delete the blocks that have been run, rename the file then run the new one, What do you guys do?

 

My FADAL allows starting at any cursor position, I place cursor on appropriate line and use the search moduls and restart command.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...