Servo spindle advice...

Post anything you want to discuss with others about the software.

Servo spindle advice...

Postby spumco » Sat Mar 16, 2019 8:36 pm

Hi All,

In the beginning stages of planning my spindle motor swap. Changing from a 3p induction motor to an AC servo.

First decision that came up is how to command the spindle. I am currently using 0-10V to the VFD, and my servo amplifer can be set up with the same control scheme in velocity mode.

On the other hand, I could change to a step/direction command system with the amplifier in position mode. If need be, I could adjust the electronic gearing so that I can reach max spindle speed (7500RPM) given the UC300ETH 400khz step limit.

I don't intend to use the servo amplifier index pulse for orientation as I haven't decided on a 1:1 (or other) belt ratio. A simple proxy on the spindle will be used as spindle homing (for peck tapping & drive key orientation) via UCCNC. I'll get to the macros later for that stuff.

So... anyone have a recommendation on 0-10v vs. step/direction for the spindle?

Thanks,
Ralph
spumco
 
Posts: 255
Joined: Mon Oct 03, 2016 10:10 pm

Re: Servo spindle advice...

Postby Vmax549 » Mon Mar 18, 2019 5:36 pm

HI Ralph, For the most flexability I would do step and direction. This gives the option of running the Spindle as a spindle or as Caxis. Spindle orientation is as simple as ref home the C axis then move to index position.

Also running as c axis gives you the ability of doing a true rigid tapping with precise Z depth (blind hole tapping)

Just a thought, (;-) TP
Vmax549
 
Posts: 91
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: Servo spindle advice...

Postby Battwell » Mon Mar 18, 2019 5:49 pm

i have mine set as step/direction spindle- seems to work ok now the deceleration is fixed at m30 .
we had a bit of discussion regarding this before- setting spindle step/direction to the same pin numbers as c axis. (i havnt tried this as yet)
mine works fine with rigid tapping etc- using a single pulse direct off spindle- not off encoder z pulse ( z pulse was too short)
i used a programable drive to get the spindle to home and orient itself at an exact encoder position for tool changes- where the tool must be aligned properly for the drive dogs to match the carousel.

the only annoying thing ive found- today- while posting out of fusion 360 for the first time is that the rigid tap cycle posts out m3 and m5 commands for every hole- which delays the cycle by the dwell times set for m3 m5 in uccnc. deleting the m5 stops this delay. (im going to see if i can modify the pp but havnt looked if its possible yet.)
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 441
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Servo spindle advice...

Postby spumco » Mon Mar 18, 2019 10:37 pm

Thanks gents, step & direction it is.

As to the F360 PP doing the M3/M5 thing, I think that was me. F360 would start the spindle with an M3 and the G33.x would start then reverse to the R plane and move on to the next hole with the spindle stopped.

Then it just sat there doing nothing.

I found that UCCNC needed an M5 command to stop and then another M3 to start the G33.x cycle again on the next hole.

I send Autodesk a request to edit the Generic UCCNC PP which they did - about a year & change ago.

Does it just need an M3 before each hole and not the M5 as well? If that's the case feel free to contact F360 and they'll edit the PP for everyone. I wish you could subscribe to the PP library and get alerts when they update.

-R
spumco
 
Posts: 255
Joined: Mon Oct 03, 2016 10:10 pm

Re: Servo spindle advice...

Postby Battwell » Mon Mar 18, 2019 10:52 pm

i left the m3 in there- just deleted the m5's and it ran ok without delays.
im sure when i hand wrote my rigid tap test code before i only had a single m3 with s300 and m5 at the end- il check it out tomorrow.
7 seconds delay between each hole of delays was annoying me!

in the pp i can see where the m3,m4 are written but couldnt find the m5 for rigid tap.

it was my first posts out of fusion so i thought it was me doing something wrong. - but now i can blame you :-)
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 441
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Servo spindle advice...

Postby spumco » Tue Mar 19, 2019 2:30 am

Line 939 or so in the latest PP I think is the culprit. The (COMMAND_STOP_SPINDLE) line is the bunny, I think.

That's generating the M5 rather than simply letting the tool spin backwards until the move to the next hole followed by an M3. Just a guess, however. Comment it out and let me know how it works.

Function onCyclePoint(x, y, z) {
var forceCycle = false;
switch (cycleType) {
case "tapping":
case "left-tapping":
case "right-tapping":
case "tapping-with-chip-breaking":
case "left-tapping-with-chip-breaking":
case "right-tapping-with-chip-breaking":
if (!isFirstCyclePoint()) {
onCommand(COMMAND_STOP_SPINDLE);
}
forceCycle = true;
}
spumco
 
Posts: 255
Joined: Mon Oct 03, 2016 10:10 pm


Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 4 guests

cron