[uberlinuxgeek]

Hello,
I am looking to find out how far someone with a shopmaster with center x axis ballcrew has pushed the x and y axis velocity and acceleration settings in motor tuning screen in mach 3. My 2014 model was set for 25 in/min for both axis. I am working to speed these up, I have been able to get to 50 in/min and 2 for acceleration on the x axis in mill mode/ z in lathe mode and 35 in/min and 2 for acceleration on y in mill mode and x in lathe mode. But have others been able to push these further? I ran into an issue threading course threads and spindle speed using mach3 threading wizard. What I found was that I needed to speed up z in lathe mode for increased spindle speed past 300rpm, 25 in/min was too slow past that rpm or the pitch would not match settings and with aluminum threads I needed higher spindle speeds for a good thread so I started increasing the axis speed to match higher spindle speeds. In fine threads this was not as bad but with course ones the cutter would not move fast enough to match. So would love to hear what others have been able to achieve, if you have a center x ballscrew. This would help me push the machine faster in both lathe and mill mode. That would save me time over experimenting.
Thank you

Sent from my SM-N910V using Tapatalk

[BlackICE1]

I'm running 75 on the X & Y about 50 on this Z these g0 only I don't use them for cutting or it will lose steps.

[sharpshooter90]

Guys, I'll jump in here with what I remember- anyone who spots an error please correct me.
Stepper motors usually run about 200 rpm max, and with microstepping that goes up to about 2000. But the big drawback is that steppers lose all their power at max rpm, so running down around 30% of max is generally the best torque/rpm compromise. I think Shoptask still uses the 2-1 pulley ratio and the 5 pitch ballscrews, so doing my math, the max feed rate would be around 200 inches per minute. Using the 30% rule, that would put your usable range around 60 IPM. You would probably have to keep your acceleration pretty low to allow the motors to come up to speed. That would also mean giving yourself plenty of lead before your tool engaged to be sure the motors were up to full speed before the cut started. The other variable is the VFD drive spindle motors. People say that they can maintain 80-90% of torque right down to near zero rpm, and I can't dispute that. But in my old school mentality I believe that the mass of a spinning rotor is the real key to high torque, so the faster you turn that motor, the less chance you will have that it stalls a bit. So with these newer style machine which rely on the motor and feed rate to maintain a constant ratio, you need to find that "sweet spot" where the spindle motor is turning fast enough to keep a steady rpm and the feed rate is set to the other " sweet spot" where the steppers can keep the carriage moving under cutting loads and not loses steps. Then you need to find the proper setup to cut your desired threads- As a simple easy to calculate sample, let's say you want to cut a 10 pitch thread 1" long.
If your spindle was turning at 1 rpm, then your carriage would have to travel 1" in 1 minute, so your feed rate of 1 IPM would have all the power it needs to cut the threads without losing steps, but most likely your spindle would stall and get out of synch. So now if we increase the spindle to 1000 rpm where it has a ton of torque, we need to increase our feed rate to 1000 IPM-which is way beyond our usable range. Using the 60 IPM from before as the maximum usable feed rate, then our matching spindle rpm should be 60. Now you need to know exactly how stable your VFD spindle is at 60 rpm- does it have plenty of torque to keep turning under cutting loads and does it vary by more than 1-2%. A lot of that depends on the motor-spindle drive ratio. For general lathe work an rpm range of 0-1500 is pretty good, so a 1500 rpm motor would run a 1-1 drive ratio. However trying to get 60 RPM at a 1-1 ratio would put your motor speed at 60 rpm as well, so we get back to the question of how efficient are VFD drives at low speeds. With a CNC machine you can do some compensation by setting the number of passes high- maybe 30 passes and the depth of cut in small increments to reduce the chances of spindle or stepper stalling. Figuring this out will be a trial and error method unique to every different machine.

[Fiero Addiction]

Check your motor wiring. The motors on my 2007 were wired bipolar series. Changing them to bipolar parallel provides more torque at high speeds. There is no drawback other than higher current draw. The power supply and Gecko drives can handle the additional current so I'm not sure why they were not wired parallel to begin with. If you make this change you will also need the change the current set resistors on the drives. I also switched to 1:1 drive ratio on the screws. With 2:1 at 50 ipm you are asking those big nema 34 motors to spin over 500 rpm, way outside their usable torque curve, especially if they are connected in series. By driving at 1:1 you cut motor speed in half and put the motor back into usable range, and still have resolution of .000098" per step with 10x microstepping drives. With these two changes you can double the rapid speeds while maintaining resolution that exceeds the mechanical ability of the machine. It will also put the motors into a better speed range where they are making more torque at normal feedrates. I can rapid at 100 inches per minute and 50 inches per minute squared acceleration. That's above the motor's ideal rpm but that's a fairly conservative setting that I ended up with after some testing.

[smallblock]

Fiero,
I did the same thing on my Mill Turn- changed to a 1-1 ratio and got a lot better overall carriage response and rapids. I don't know about my motor wiring, but I think I'll just leave it alone for now- " if it ain't broke don't fix it " I was almost tempted to bump it up to a 2-1 motor- screw ratio to double the feeds again just to find the torque limits of those steppers.

Sharpshooter,
By increasing the feed rates it allows you to run your spindle motors faster and get that " inertia" power. I have found that the spindles are more consistent in rpm the higher they go. My machine came with a 1.20-1 ratio on the lathe drive and the motor is rated at 1390 RPM at 50Hz. So at 50Hz the spindle was turning 1160 rpm which is a good range for a lathe of this size. However, you can boost the Hz settings in the VFD up to as much as 120 before the motor can't keep up, so you can actually run the lathe spindle as high as 2800 rpm. That might be OK for a Sherline, but its way faster than the Shopmaster needs. So I also put a smaller pulley on my lathe motor - the original was 3.75 and my new one is 2.125- a reduction of almost 1/2. So now I have my VFD set at 120Hz and my max rpm is 1600 and when I set it for the lower speed for threading- around 300, the motor is spinning about 600 so its gets your inertia power.
I spoke to JT about these mods and sent him some video and he is considering making the same changes in the production.
I also found that in the threading wizards, you need to edit your G code to the actual RPM as opposed to your " requested " rpm in the wizard. For example, my machine will run at about 494-498 rpm as tested with a laser tachometer when I give it an M3S500 command. That is not an issue in turning, but when threading, especially if you run a lot of light cuts, the accumulated difference between the RPM in your G code and the actual RPM can cause errors in the threads until they begin to wipe themselves out, so you need to keep tweaking the spindle pulley settings until you can get the least possible error. Also in Mach 3, be sure to set your de-bounce to a high number like 500. That has to do with the size of the magnet and the diameter of the pulley- on the lathe its not a real issue, but the mill has a real small diameter pulley and those little magnets are strong. They are pressed into a countersunk hole in the steel pulley, so you don't really know how big that magnetic field is. Also set the Shuttle wheel setting to a small number- mine is 0.0001 as opposed to the factory 1.0000

[uberlinuxgeek]

Hello,
This is all great info. When you mention to tweet the gcode smallblock I am not sure what I would be looking at, as when the wizard generates the code it is like you said, 500 rpm and if i use the laser tach on the spindle it will vary between 495 and 502 and never stable it keeps varying so what would I actually use? For the debounce it contains 2 lines, my debounce interval was set at 400 and index debounce at 0. Also where is the shuttle wheel speed setting, have not seen it? Funny you would mention threads being wiped out as I have been fighting that but thought was my x start and end values for the thread type I am working on, I start my thread an inch before I touch the actual stock. I see you guys are achieving some high rapids, would you mind sharing how high of mill and turn feed rates you are getting on say aluminum stock?
Thanks for all the info guys

Sent from my SM-N910V using Tapatalk

[uberlinuxgeek]

Thanks to the info, and a couple talks earlier with JT, he is sending me new belt and pulley to get to 1:1 like mentioned here. He remembered someone mentioning using it, he just wasn't sure where so I let him know about this thread

Sent from my SM-N910V using Tapatalk

[uberlinuxgeek]

Fiero Addiction, did you change to 1:1 drive on both x and y? Where did you get the pulley for the y axis? JT is sending me for my x.
Thanks

Sent from my SM-N910V using Tapatalk

[Fiero Addiction]

Mine was an older machine (TriPower) with the gearboxes and manual controls. It was a factory CNC, but the CNC stuff was just sort of cobbled on in those days. It was all worn out and it wasn't a good design to begin with so I tore it all off and redesigned all three axis to be much simpler and more rigid. I actually just sold the machine this week. I had finally gotten it to the point where it could do some decent work, then I bought some other machines and lost interest.

[uberlinuxgeek]

Smallblock, I found the shuttle wheel setting but what does it do exactly?
Thanks

Sent from my SM-N910V using Tapatalk

[smallblock]

Read the Mach 3 manual and if you understand it, let me know. Sometimes the more I read it the less I understand, but the Mach forums have some guys who speak plain ol' English and can offer advice on what to do.

[uberlinuxgeek]

Well the shuttle acceleration setting is used in backlash movements and a Mpg shuttle controll. Have set for .004 on both mill which was original setting and now lathe creates a less jerky backlash at higher percentage of backlash speed. I now have installed a new belt and pulley so the x axis is a 1 to 1. In lathe mode I can cut at 60in/min for 1200 rpm 20tpi. What I found for threading issue was that with the shopmaster running the rpm by manual mode and feeding that into threading wizard works well. When using vfd under mach3 control it was mashing threads as it would adjust speed of z axis based on last read rpm which varies within 5 rpm which is too much for a good thread, by manual controll is within 1-.5 rpm which does work. Just an fyi

Sent from my SM-N910V using Tapatalk

[BlackICE1]

If you turn off the PID control of the motor speed it should work like manual VFD control. However the RPM won't track as well.

[smallblock]

BlackIce,
How do you turn off the PID ? In PORTS & PINS> SPINDLE SETUP, do you un check the Closed Loop Spindle control or just set all the values at zero? Or do you go to FUNCTION CONFIGS> CALIBRATE SPINDLE and turn it off somehow. I am still a bit in the dark about how Mach 3 arrives at their default settings. Below is a definition of PID I found on line.

(2) (Proportional-Integral-Derivative) The most common control methodology in process control. It is a continuous feedback loop that keeps the process flowing normally by taking corrective action whenever there is any deviation from the desired value ("setpoint") of the process variable (rate of flow, temperature, voltage, etc.). An "error" occurs when an event (valve opened, closed, etc.) or a disturbance changes the load, thus causing a change in the process variable.

The PID controller receives signals from sensors and computes corrective action to the actuators from a computation based on the error (proportional), the sum of all previous errors (integral) and the rate of change of the error (derivative).

The Mach 3 default settings were-
P 0.25
I 1
D 0.3

Maybe someone can explain each of these settings in relation to the RPM.

[BlackICE1]

BlackIce,
How do you turn off the PID ? In PORTS & PINS> SPINDLE SETUP, do you un check the Closed Loop Spindle control or just set all the values at zero? Or do you go to FUNCTION CONFIGS> CALIBRATE SPINDLE and turn it off somehow. I am still a bit in the dark about how Mach 3 arrives at their default settings. Below is a definition of PID I found on line.

(2) (Proportional-Integral-Derivative) The most common control methodology in process control. It is a continuous feedback loop that keeps the process flowing normally by taking corrective action whenever there is any deviation from the desired value ("setpoint") of the process variable (rate of flow, temperature, voltage, etc.). An "error" occurs when an event (valve opened, closed, etc.) or a disturbance changes the load, thus causing a change in the process variable.

The PID controller receives signals from sensors and computes corrective action to the actuators from a computation based on the error (proportional), the sum of all previous errors (integral) and the rate of change of the error (derivative).

The Mach 3 default settings were-
P 0.25
I 1
D 0.3

Maybe someone can explain each of these settings in relation to the RPM.

Either method should work, but I just uncheck the box.

[uberlinuxgeek]

If you turn off the PID control of the motor speed it should work like manual VFD control. However the RPM won't track as well.

Actually I did not turn off PID, I just changed the vfd settings to allow for manual controll using the knob. Then I adjust to desired rpm and fed back the turn rpm value using the laser tach into the mach3 threading wizard. I get within 1 to .5 rpm and have no issues and a good thread. I am going to start looking into PID values in the future for automatic control but for now this is a very simple solution.

Sent from my SM-N910V using Tapatalk

[BlackICE2]

I think the rpm sensor automatically adjust the Z movement to match the real RPM to get the desired tread pitch. The difference between the real vs commanded RPM isn't a big deal, but the hunting (oscillation of RPM) is. Having PID on cause more hunting at low RPMs, at higher RPMs it dead on. But most threading will happen in the lower RPM range because the X axis can't move fast enough. I find it hard to keep the RPM stable at < 250 RPM. At 1000 no problem. That said I have successfully cut thread without problems at around 200 to 300 RPM. They probably would be cleaner if the RPM was more stable.

[jlmccuan]

How did you speed your steppers up? I get 25ipm and haven't been able to set any faster.

[BlackICE1]

It's in the motor config settings. If you go too fast you will lose steps with possible bad side effects.

I found that I could go 75 in/sec in the x and y, but the Z would lose steps when peck drilling so I lowered it to 50. Even then the higher speeds I use just for G0 moves and not under load while cutting. Under load you probably will lose steps and ruin parts at the very least.

[uberlinuxgeek]

BlackICE1, was right on in motor configuration and this is done per axis. I found in lathe mode doing threading operations I can hold 60 under load since it is such a light cut, and was needed so that with softer metals I needed higher rpm which requires faster axis. I only cut that fast on lathe z. All other are rapids for higher speed, I don't usually exceed 15ipm in normal cutting.

Sent from my SM-N910V using Tapatalk