CNC Lathe Question

My thought is to set up some macros for quick threading.

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.

RogerN

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.

Jon

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.

Enjoy, DoN.

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.

Karl

Greetings Karl, 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? Thanks, Eric

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 at end_of_cut.

The custom G76 cycle I wrote for Camsoft with special high speed hardware may set the standard for threading on refit controls.

Karl

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.

Karl

In a leadscrew driven system, the inertia of the slide is usually insignificant compared to the inertia of the leadscrew and motor.

Ned Simmons fired this volley in news: snipped-for-privacy@4ax.com:

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 motor's rotor.

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.

Lloyd

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 matching.

Ned Simmons fired this volley in news: snipped-for-privacy@4ax.com:

If your numbers are correct, I'll concede the inertia being more than the screw's, but did you ignore the dynamic loads on (say) a 16mm ball screw/nut? (fairly typical for -say- a 13x40 lathe)

Lloyd

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# )

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 comfortable learning. Eric

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.

RogerN