Re: EMC Lathe mode.

--- In CAD_CAM_EDM_DRO@y..., "Art Fenerty" <fenerty@h...> wrote:

> >
> Why, does the spindle slow down to any signifigant degree?? This is
> beginning to sound like lathe CNC really require a VERY tight

control of

> stepper motor speed versus Spindle speed. Wouldn't any PC have a

latency in


You got it! Most lathe feedrates are in inches per rev or MM per
rev. If the revs slow down because of heavy cutting, the feed must
stay in sync. Yes, it is very usual to take big hogging cuts to
remove lots of material at the absolute top hp and material removal
rates possible. There is an acceptable range of variation from the
programmed feedrate, but if it gets to be significant the spindle may
stall or the tool will break. If you just take baby cuts who cares,
but if you want to do any serious cutting, precise feed control is
required.

Threading is related in that you need to have about .0002 inch pitch
accuracy over the length of the thread to make accurate threads over
the size ranges that most people need. Even then you may not be able
to hold some standard and common classes of fits. Many controls have
a start and end zone in which they do not guarantee pitch accuracy,
as the controller checks where it is and tweaks the Z feed rate to
hold the pitch tolerance. The feedrate for threading is the pitch of
the thread ie. 1/4-20 would be .05000 ipr and yes they usually are
programed to at least 5 decimals in inches. The leanin and exit
error rates are usually defined with a formula that takes into
account the rpm of the spindle, and they define how far in front of
the part you must start to get a good thread.


The other thing is that usually the spindle speed is programmed in
constant surface speed. That means that the spindle rpm is changed,
based on the programmed X location of the tool tip. Example. 2 inch
diameter cut at 100 SFM is approx 190 rpm, a 1/4 inch diameter would
be about 1500 rpm at 100 sfm. If you cut a taper from 1/4 to 2
inches in diameter, you would want the spindle speed to change from
1500 rpm to 190 rpm while you are cutting. This will create a nice
smooth surface and a constant chip load. The feed should be .006 per
rev no matter what the rpm was.

This is similar to the surface speed that you would calculate for
different cutter sizes in a mill, except that you get the option to
make changes within the full range of the radius swing of your
lathe. I used one of the slide rule calculators as that is close
enough for most work. That's why I say "about" when indicating the
rpms.

Best Regards,

Fred Smith IMService

Listserve Special discounts and offers are at:
http://209.69.202.197/cced.html

imserv@... Voice:248-486-3600 or 800-386-1670 Fax: 248-486-
3698