Tool Offsets for 8L

Do I need to set the tool offset for the reference tool every time I power up the Lathe (8L).
The position is off by about .01 inches every time I power cycle the machine.


1 Like

@Sandeep_Dutta welcome to the Tormach user forums - thank you for posting!

The proximity limit switches on the 8L provide an acceptable reference position for limits of travel but not for holding tight tolerances on a part. To ensure accurate diameters you should take a skim cut (using any tool) and mic the result after a power cycle. Don’t change the tool offset to match the diameter - change the work offset diameter value. Changing the tool offset only works for the one tool whose offset you change. Changing the work offset will affect all tools’ positions.

More info here:

1 Like

Thank you . This was very helpful.
I also found this video very help as well.

well, that would have been good to know. I am experience a variance of +/- .025 on the x when referencing then turning diameters. I just tested a piece, turning, setting, referencing and checking - total crap shoot on what size I would get. My expectations on a CNC lathe was .0002. The Z seems to repeat ok, the X is really crappy. I have spent a couple of hours trying to see what is wrong with my lathe, not realizing it all 8L lathes that have a poor reference system. I have a 1100 Mill which has really good repeatability so I expected the same or better seeing the 8L is 10 years newer. Now that I know to lower my expectations and set the offsets every time I power off that will help.

@Tom_Carr ,

Limit switches on any machine only get you so far. Will milling you are often removing more that 0.025" from your rough stock, so a roller limit switch like on the PCNC and M milling machines is acceptable for a home reference. The MX machines use servo motors which home to an encoder index which is much more accurate.

With a lathe it’s a different story - the machine’s understanding of X axis distance to spindle centerline influences the final part in a way that doesn’t happen on a mill. If your work offset is off your part comes out under or over-sized. The Z reference seems better to you because the X reference is a radius value but you measure a resulting diameter - magnifying any error 2X. Even a lathe with servo motors that home to an index pulse suffers from this. In my experience most machinists measure the first part that comes off a lathe after power cycle and adjust the offset accordingly regardless of the type of reference switch.

There is another option if you don’t want to go through a skim cut/offset adjustment on power cycles. Some users prefer to mount a dial indicator on X that can measure against a reference surface, then on power up they jog the machine until zero is reached on that indicator, disable the limit switches on the settings screen, and click the ‘ref x’ button. With limit switches disabled ‘ref x’ will set ‘machine home’ to the machine’s current position. I know we have a few 15L customers who do this. I’ve always taken the skim cut approach.

Best of luck.

Thanks for the detailed reply. I have been looking at some videos of tricks, the one I like the best is the person that mounted a LED edge finder in a tool holder and uses it like a probe. I could do the same with an indicator in a tool holder that I know what diameter is I am touching off on.

I have an old 1100 series III and the limits are really accurate - when checking with my probe it has always been right on. I expected the lathe to have the same repeatability. Just an extra step which means making sure the students do it if when they fire up the lathe or crash a tool and have to reset. Servos would be nice. :wink: