Converting a lathe to CNC seems pretty straight forward. A few mods to the
compound so primary cross feed is driven by a stepper or servo and a better
screw and nut. Throw a good screw on the saddle with a servo or stepper and
disengage the feed screw.
My question is in regards to the spindle motor. Just use the regular
spindle motor and feed back RPM to the control, or change it to a servo for
more precise spindle position control like a 4th axis on a mill?
I converted a lathe with Anilam CNC control to EMC2. I just needed a
spindle encoder with an index pulse and EMC2 threads great. The threading
is fast compared to threading on a manual lathe. I was able to turn down 1"
dia Stainless to 3/4" Dia X 3" L and thread ~1-1/2" length with 3/4 -16
thread (for a cylinder rod end) in around 3 minutes, turning, manual tool
change, & threading, all within 3 minutes.
You do not need a servo motor and drive unless you plan to use the spindle
as a C axis, with live tooling. For threading, you need a spindle
encoder, and the CNC control will adapt the Z feed to stay in sync
with the spindle.
Add an encoder to the spindle with a single index point and a
number of pulses per revolution for the rest, so the controller can keep
track of spindle position. Always start the threading pass when the
primary index passes its sensor. A lot better than trying to guess
where it is purely based on RPM.
Kind of a test post here. I'm at a new location.
A VFD with three phase spindle motor is a REAL HANDY addition. Then
you can program speed changes.
I believe nobody else on this NG uses my control, Camsoft. But this
may apply to EMC, they work about the same for threading.I got
improved control threading at high RPM by adding a slot sensor and
high speed Opto22 input. This allowed cutting on one side of the
thread (30 degree input angle) at 1000+ RPM. At the time my son had a
large job for fine threads in titanium rods.
I have seen only one lathe running Mach 3. The owner showed me how it
cut threads. The lathe used only 1 pulse per revolution for thread
timing. This seemed to me to be inadequate for accurate threads. Every
CNC lathe I've ever run or owned in over 30 years of machining has had
some type of multiple pulse output from the spindle. Watching the Mach
3 lathe thread a 10 pitch thread with the tool cutting on both sides
made me think about how the spindle must have spun slower when the
tool dug in. I have wondered about Camsoft. I see it's about 4 grand
for the software capable of threading and IPR on the lathe. This seems
high to me. Are you quite happy with Camsoft?
First, I am quite happy with Camsoft. I started with CNC when Mach and
EMC didn't exist with a DOS control called AHHA. It didn't do servos
so I upgraded to Camsoft twelve years ago. Couldn't be happier. But
because of the high cost, I don't suggest it to hobby types. You're
looking at nearly 10K if you buy all new hardware.
Threading on all these controls is done about the same. Trigger thread
start with a spindle input then move the Z axis. The devil is in the
details: - how accurate is your spindle RPM - will Z speed instantly
adjust to a dip in spindle speed (electronic high speed gearing) - how
quick is your start pulse - how fast(hi acceleration) and accurate is
your Z axis servo move - can you move X for taper and quick withdraw
The custom G76 cycle I wrote for Camsoft with special high speed
hardware may set the standard for threading on refit controls.
I don't see why speed of withdraw should be an issue. Even 20 or 30
IPM is quite fast when you are talking about the depth of a thread.
Acceleration is only limited by the inertial mass of the cross slide.
Lets say you need to pull out of 50 thou depth at 1000 RPM in one half
a spindle revolution for easy math. That's 100 IPM with some serious
acceleration. If you need to thread to a shoulder and not leave a
groove to weaken the part, you need this.
Not hardly true with modern servos, at least not on the X axis. The
slide itself is the major component. X screws are normally small by need
of the fit requirements. One has to deal with the maximum dynamic load
the screw/nut assembly can take, not the mass of the screw itself or the
In fact, the big deal with AC servos is "tuning" the drive to match the
inertia of the screw and couplings/pulleys to the motor inertia so that
unwanted oscillations don't occur.
On Tue, 29 Nov 2011 12:47:44 -0600, "Lloyd E. Sponenburgh"
Let's throw some numbers at it: Assume a 1 inch dia x 48" long x 5 TPI
screw and a low inertia 2kW motor. The polar inertia of the motor and
screw will be around .015 lb-in-sec^2. The slide would have to weigh
over 5000 lb in order for its reflected inertia to equal that of the
motor + screw. I didn't do the math too carefully, but it doesn't look
out of line based on personal experience.
If you have pulleys and belts in the drive path of a servo system
you'll have to make big compromises in tuning regardless of inertia
On Tue, 29 Nov 2011 15:04:22 -0600, "Lloyd E. Sponenburgh"
No, I was only worried about how the screw + motor inertia affects the
ability to accelerate the carriage, and just plugged in a motor and
screw based on a SWAG for components for a machine I was imagining,
probably considerably heavier than an import 13x40. (My 13x30 Monarch
weighs 5500# <g>)
Thanks for the info Karl. Most of the threads I cut are class three
threads. A pitch error of just a tiny amount can really cut down on
the effective pitch diameter tolerance. The CNC machines I now own
cut good threads. They better because that's what they're supposed to
do. But I want to add CNC to a manual lathe for various reasons. I
think that only 1 pulse per rev is not enough for accurate threading.
I have been considering using a larger Z axis servo than would be
needed for turning just to make sure I can change the Z motion fast
enough. I'm still looking at EMC to see if is something I'll be
If you have to be producing parts right now for money, go the higher $$
turn key solutions. If not, the EMC solution is the way I would recommend
to go. EMC doesn't use 1 pulse per revolution, the speed can change as the
cutter enters the work and puts it under load. EMC does something more like
slaving the feed to the spindle axis. For example, a 100 line quadrature
encoder produces 400 counts per revolution, EMC generates the command on
where the tool bit should be based on the counts from the encoder. In this
way it doesn't matter all that much if the spindle slows down a little, EMC
will detect it in 1/400th of a turn with only a 100 line quadrature encoder.
If you choose a 500 line encoder, there are 2000 counts per revolution for
EMC to attempt to gear to.
EMC can seem intimidating at first because there are so many ways you can go
with it. Once you pick the hardware and encoders it is much easier to get
help with getting things set up. For example when you don't know what pitch
of lead screws you will have, or what encoder counts you will have, or how
many pulses per revolution you will have on the spindle, no one can suggest
the proper setup. But once you have the machine and say for example it has
5TPI axis screws, 2000 count encoders, and 1000 counts per revolution of the
spindle, it's not difficult to set up 10,000 counts per inch of axis travel
and 1000 counts per spindle revolution. So for example, a 20 TPI thread
would need 500 axis encoder counts per 1000 spindle encoder counts.
Reading about the numerous configurations available with EMC seems much more
intimidating than when you actually pick your hardware and set up your
machine for EMC. I think it's well worth the effort to have a machine you
know inside out and can fix yourself in minutes versus paying someone high
$$$ for an emergency repair.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.