Re: "0" reference point on CNC lathe

Scott,

I'll try to explain some of this, but I'm not completely sure what
you're asking. Most of this stuff is determined by your control
software.


Everybody (almost) sets the part's Z zero at the end of the part and
part center as X zero. Negative Z's are into the part and positives
Z's are off the part. X & Z values in your Gcode program are
relative to the part's offsets.


The following are the way two of my lathes operate, each is quite a
bit different than the other. Both have advantages in certain cases.

On one lathe the tool offsets are set by touching off the part.
However far the part protrudes from the chuck or collet determines
part and Z tool offsets. On this machine when you reference it the
screen readout indicates X0.0000 & Z0.0000, which is far to the right
and away from the operator. This is an easy system to setup with
multiple tools. All offsets can be set by touch or taking a skim
cut. Note, without a part the Z tool offsets are meaningless, once
set the X offsets would still be valid for different parts unless the
tool is moved. To set a tool touch the end of the part (or skim
cut), go to the tool offset function and enter Z0.0, then touch or
skim the OD and enter the diameter value. Nothing needs to be
specified in the Gcode program to establish part offset, just calling
up a tool is all that's required.

On the other lathe the tool offsets are set with respect to their
position from the face and center of the tool holding turret, so tool
offsets can be set independent of any part being made (they can also
be set by touching off part, but not so easy on this machine) and the
tools can be removed and re-installed while maintaining their offsets
since they register in the tool turret pockets accurately. On this
machine the reference positon has values, something like X4.0123,
Z7.8967, again far to the right and away from operator. The machines
X0.0 & Z0.0 is the center and face of the spindle. The control
establishes the actual position of the part's Z offset by adding an
offset for chuck (G54) or collet holder (G55) and a G92/G59 value
which must be specified in your Gcode program.

I've probably totally confused you. I even get confused when I start
thinking about this stuff, once I'm standing in front of the machine
it's second nature, explaining it is the hard part.

As I said before, most of this should be determined by your control
software. There is no set way these things work, however the control
is designed to use the tool offsets is how you have to do it.

Doug

--- In CAD_CAM_EDM_DRO@y..., fuddham@a... wrote:
> I am just getting into programming and running CNC lathes. Where
do
> most of you set your "0" reference point for your tool offsets on
the
> lathe? At the chuck face or somewhere beyond the end of the work?
> Do you change this point for different parts? My software has a
home
> position whick is at the far right and tool back toward the front
> which is also where the axis readouts are "0.0". The tool
reference
> point can be set anywhere from this point.
>
> Thanks
>
> Scott Hamilton