Hardinge CHNC retrofit. ASD drive (old school) and threading...

[natefoerg]

Hello!

I have a Hardinge CHNC lathe that I have running steppers, smoothstepper, G203V's and mach 3.

I have not had good results using a inverter duty motor and a VFD, probably has to do with the fact that I'm not willing to spend big money to get a really nice big VFD and motor.

Since my motor was bogging down under any mild or greater cut, I have decided to go old school with the spindle control. I have a Adjustable Speed Drive, like the drive found in a bridgeport series 1 2hp mill head.

This ASD will allow me to rotate the ASD dial and change the speed manually. I don't need computer control of the speed. what I really need is torque for cutting...the ASD should give me what I need.

Since this lathe does not have backgear or changeable pulley ratios, the ASD should give me enough torque at lower speeds to let me thread without losing spindle sync.

OK, enough background, here is my question-

I will have manual control of the spindle rpm.
If I use my tach (optical pickup) on the spindle, I should be able to dial the ASD to a set speed for threading. lets just say 300RPM. the ASD should hold the 300rpm fairly well, and only vary +/- 5 or 10 RPM.
I can then tell the mach threading wizard that I want to thread at 300RPM.

With the Tach pickup sending pulses into mach, will mach have enough info to keep the feeds synced with the spindle RPM, and not loose the threads position?

I guess what I don't understand, is with mach threading normally, the spindle speed is controled via a 0-10V signal. If that signal is not present, and the spindle speed is set manually and fixed, how can mach know where to keep the bit. How, if it cannot alter the spindle speed can mach keep the thread synced? Can mach see the spindle speed as stable at 300 and just keep the timing correct to cut the thread?

now that I think about it, how does mach keep the thread synced with the spindle? does it modify the spindle speed (0-10V) or does it modify the feed speed of X and Z and when it leads into the cut? does Mach modify both?

[Peter Homann]

Hi,

Yes, what you are suggesting will be fine.

When, threading, Mach3 does not vary the spindle speed, it varies the Z axis feedrate to match the speed of the spindle.

So, if the spindle slows slightly, the Z axis will also slow to ensure that the thread pitch being cut is maintained.

What Mach3 does need is to know how fast the spindle is actually rotating. It gets this from the spindle index sensor, and not from what S word is in the Gcode.

So you can set the spindle speed manually. If the spindle is rotating too fast such that the Z axis can't move fast enough to cut the thread. Mach3 will halt giving you a warning message of this.

Cheers,

Peter.

[natefoerg]

Thanks peter!

[RICH]

Mach takes readings of the spindle rpm before the Z is allowed to move / trigger for the threading cycle. If you have spindle speed averaging on it will
average the readings, if the index debounce is set to 0 it will accept any signal even if it is noise. The more accurate the rpm the more accurate the the thread.  The user should always calculate the thread when using the threading wizard as it will tell you if the accel and velocity as set in motor tuning is adequate for the input rpm to be used and will inform you if your exceeding it. Mach will compensate from say 10 to 25% rpm difference,
maybe more, but again the quality of the thread is only as good as your stable rpm.
Since threading is a real test of the "lathe system" one should do some testing by scribing the thread  to know before hand just what to expect
from their lathe. Have a read of Threading on the Lathe write up which is is included with Mach's installation or can be found in Members Doc's
RICH