Re: [CAD_CAM_EDM_DRO] EMC Lathe mode.

this aint as easy as it might look at first

the G-Code interpreter would need to be redone in some areas for a
turning center ,many of the codes do different things and most lathes have
some extra canned cycles for rough turning and facing that will take several
passes and leave some stock for the finish pass
often the parts finished profile is given in a subroutine and the control
will run that section of code twice ,once to rough it down and again as
a constant contouring finish pass (another canned cycle)

tool nose radius comp is done slightly differently and the
standard 8 TNR vectors would need to be added to the tool table ,
maybe in place of some of the extra work offsets (lathes only use one)
also many lathes do not use M03 to change tools,you first move to
a preset tool change position (X positive limit) and just use T020202
(tool 2 , pocket 2 , offset 2) calling that tool with a 2nd offset would be
T020222

the default cutting plane for arcs will need to be set to XZ rather than
the mills default of XY (naturally)

the spindle encoder should have a fairly high resolution both for threading
and as the C axis ,the encoder is often driven from a small timing belt pulley
separate from the spindle drive pulleys
in fact most mills have a spindle encoder for rigid tapping and tool indexing
during tool changes
so you should really think of the spindle as a full blown rotary axis on ANY
machine tool not just the lathe
oh yea, even with a high resolution encoder at several thousand RPM the
encoder counts will only be coming in at a few hundred Khz ,this shouldn't be
a problem for a reasonably fast computer to keep up with

constant surface speed was already mentioned

and I don't remember if EMC has a feed per rev setting or just feed per min

looks like you've got your work cut out for ya :-)

Brian

On Monday 01 October 2001 17:28, you wrote:
> Hi All:
>
> I seem to be hearing from a few people lately who would like to see
> lathe capability added to my software. Since it is based very much on the
> EMC code kernel, I thought I'd ask the EMC guru's what would be required to
> add lathe capability. I have never used a lathe CNC before, what is
> necessary? what would be nice? Would C-Code just be a translation of the
> input coordinate system, or is it necessary to use different G-Code
> translations? Can Mill software not be used on a lathe or is it a matter of
> apples and oranges? Is EMC not usable on a lathe?
>
> Any input would be appreciated,
> Art
>