G60 and Fanuc 0i-MC Control

[DavidSV]

G60 does not appear to be working. Is there a parameter to turn it on or set the distances or something?

 

Thanks

David

[Mike S @ S4A]

can you elaboate?

[DavidSV]

I can program a G60 on the position lines for a boring bar cycle, but it doesn't seem to do anything special. From the descriptions on the forum, its suppose to position off center and then move on center of the hole from the same direction every time. It just seems to go to the hole without going off center first.

[Mike S @ S4A]

You mean like a G76 milling bore cycle?

[generaldisarray]

G60 must be on a line with the axis moves.It is not modal.It must be the only command in the block.It must be first in the block.If you are already Coming at a position from that direction you may not see any difference.

[Zoober]

I think he is talking about positive approach.

Are you using it in a modal or non modal way. IRC There is a parameter for that, but is usually a one shot command, so you need to put it on every move line.

 

edit: what General said.

Too slow

[Guest CNC Apps Guy 1]

G60 is not listed in my FANUC manual for the 0i Control. If you're talking about Exact Stop, that would be G61 and you'll have to consider what generaldisarray said. After you're done with it, you should command a G64 to put it back in cutting mode so you don;t get erratic machine behaviour.

 

HTH

[generaldisarray]

G60 single direction positioning.It looks like any other rapid on our Dura Vertical.On our Monarch with a 15M The control looks like it is executing a macro.The movement looks the same on the X&Y but on the W axis it always finishes a move in the positive (up) direction.That is the only place I ever use it is on that Monarch W axis BTW.

[DavidSV]

I noticed that it was listed as optional. I am now wondering if its not turned on in our control.

[DavidSV]

Just to update this, I got it to work. The problem was that the position amount was set to 0 in the parameters from the factory. After I added a value it now positions from the same direction every time now that I use a G60.

[Zbuilder]

Please post what the parameter is. We are trying to find it also.

[Zbuilder]

Never mind. Just found it. Fanuc Parameter# 5440

[Roger Peterson]

What is our machine model and age?  Have you done any testing to see if this improves accuracy on your machine?  I had setup a custom drill cycle to do this manually for an old clapped out machine and it made a real difference.  Being that rapid moves are all exact stop mode I'm just curious if you are seeing any tangible benefits.

 

 

[Zbuilder]

Yes it did work for us. We had a different problem that this method solved. The machine gibs were worn and that made the table move out of square... depending where the center of gravity was on the far X- travel or far X+ travel. Using single direction positioning helped enough to make a passable part until the tech came in and fixed the problem. Single direction positioning is not used when the machine positioning/repeatability is in spec.

[Zbuilder]

I forgot to mention the Toyoda's age is 12 years now but we noticed the problem last year. The machine has a heavy super spacer set up on the left end and a vacuum jig on the right.
the X travel is 55". That heavy weight on the far left end is pretty much what caused the problem.

[Roger Peterson]

sounds familiar with similar results.  There was one place where they used to remove the 4th axis that was mounted on one end of the table every time a specific job was run so they could make parts in spec!  I hate it when the real world and the laws of physics get in the way of making good parts...  using a single axis approach definitely has it's place and can make a big difference, and it can be done manually if you don't have G60.

[Leon82]

We use it sometimes for tight bored holes .

 

We use approach in the ref points. And the post was modified to position x and y individually