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.
Sandeep
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.
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. 
Would be interested to see if any of you would try this on your 8L. This problem of the limit switches producing different values from one time to the next after cycling the machine got me thinking. If we think it will be different each time, one easy way to check and to know for sure if that’s happening would be to indicate on the back of the quick change in the Z and X when referencing each axis after an E-Stop.
What I found, is that my machine is repeating the referencing location to within 3 tenths max and I’ve done the test numerous times. Often it will be dead on.
Check out the 2 tests below.
Let me know if you think this testing methodology is flawed…
X-Axis check
Z-Axis check
Looks good to me! Or, you’re 0.100" off. I have bad eyesight. Hahahaha!
I just watched your videos and am wondering if you have tried this test after actually cycling the power off and back on? I’ve done essentially the same thing that you have and it comes up really close every time, but I have noticed that after a power cycle lots of times the offset will be off a pretty significant amount just based on the size it’s cutting compared to what it was cutting the previous day. I’m just wondering if actually cycling the power makes a difference in the outcome.
While I didn’t show that in either of these videos, I did power cycle at least once and had similar results. However, I did all of these tests without actually having the maching perform any operations/cuts. As I get a bit more time on the machine I’ll come back and update my findings.
I’m a member of a Makerspace in Dallas where we’re trying to come up with a solution to have a shared physical tool library of 6-8 tools with each of the offsets defined in a tool library file that users can download into their pathpilot profile from a network drive. All of the tools are insert tools so repeatability should be quite good. As for users moving the tools in the holders, we have what we think is a unique solution to this. Each of the tools either stick out of the back of the holder or are recessed from the back of the cutter by some amount. That distance is rather easy to measure accurately. Our rule for the tools will be to leave the tools in their original position (the position they were in when I first setup the tool offsets) but if they must move a tool for a specific clearance need, they should put the tool back to the measured offset from the butt of the tool holder. We will have these measurements posted next to the machine which will make it very easy to check when you arrive at the machine if you want to be sure no tool has been moved.
I even have an idea for a tray the tools can sit in with each slot having it’s own index to match the offset that tool needs. This could even eliminate the need for users to need to measure if it works how i’m thinking…
From here we will need to teach how to zero the z when putting new stock in but i’m hopeful this will be something repeatable and will help all of the members who have gone through the training, get more value out of the machine.
Any comments/suggestions would be welcome.