Odd G01 behavior in Mach3?

[mactec54]

Is the video in slow motion?

The program is attached with Video, run it your self and see Mach 3 in the Video has the same settings as you are using, and was run at the same speed, I even put the acceleration up to 200in/sec and it made it jerky at each direction change so put it back down to 80 in/sec is where this one normally runs

Change your IPM not your acceleration, 20 in/sec is already quite low for a servo machine

Your problem is, you are right on the edge of your low Voltage Servo Drive, most don't get 300IPM from Low Voltage Drives

[eldata]

The program is attached with Video, run it your self and see Mach 3 in the Video has the same settings as you are using, and was run at the same speed, I even put the acceleration up to 200in/sec and it made it jerky at each direction change so put it back down to 80 in/sec is where this one normally runs

Change your IPM not your acceleration, 20 in/sec is already quite low for a servo machine

Your problem is, you are right on the edge of your low Voltage Servo Drive, most don't get 300IPM from Low Voltage Drives

After further reading, my problem is that I'm decelerating too fast for CV motion mode (the default) to synchronize stop with the beginning of the next move in the opposite direction. My assessment here was spot on;

The drive faulted during the acceleration phase at the beginning of the G1 Z0 move as though the deceleration phase of the G1 Z-9 F300 move never occurred or didn't complete properly. In other words, the start of the G1 Z0 move was not synchronized with zero velocity. If the same thing happened using G0, instead of G1 commands, then I would have simply concluded that the acceleration setting was too high.

Edit:

The red underlined setting in the following image is the best solution to this problem;



The following code, with nine 180 degree direction changes, took 12.48 seconds to complete. The same code, except using G0 instead of G1, took 12.28 seconds.

G1 Z0 F300
Z-9
#100=0
#101=-9
M98 P1 L4
Z0
M30
O1
#100=[#100-1]
#101=[#101+1]
Z#100
Z#101
M99

Regarding your video....I'm lost for words, but the "uncanny resemblance" between the debated code here and what appears to be obfuscating CAM software output, is probably worth mentioning. BTW, was there a crash at the end?

[mactec54]

Regarding your video....I'm lost for words, but the "uncanny resemblance" between the debated code here and what appears to be obfuscating CAM software output, is probably worth mentioning. BTW, was there a crash at the end?

No crash, the program is attached with the video, so you can look and see what's at the end, it does an arc off the part, and a very short 2 axes rapid move, it was also moving 600Lbs of iron

One of the main differences was to show you, not just one axes, but 2 axes where able to move G1 at 300 IPM simultaneously and the Z axes was also moving down at a feed rate related to the movement of the cut, so 3 axes where moving simultaneously, and with no fancy computer, plus using the PP port

The difference you are seeing with your G0 and G1 G0 is not controlled like a G1 G2 G3 is a G0 Rapid can move freely, a G1 G2 G3 are more restricted as they have to be exact, and are tightly controlled G0 is not as it just Rapidly move your machine around from position to postion, you would never use a G0 for cutting something as it would not be accurate and you would have no control over what speed it could run at, it would run at what ever the settings are for your machine

Feed rate and acceleration/deceleration work hand in hand, either one can be adjusted and will have the same affect

[eldata]

ger21 (or another mod), you can add [SOLVED], or something similar, to the title of this thread if that sort of thing is appropriate here. Thanks!

[samco]

ok - thought I would chime in... When I was testing linuxcnc's new trajectory planner - I played around with mach. So - I fired up the test setup again... I am using linuxcnc as a logger with mesa hardware counting the steps coming from both linuxcnc and mach (on the same computer - dual boot)

Here are 2 screen shots of what linuxcnc logged (this is averaging accelleration over 60ms - that is why the stepped acceleration graph) you can see that at the reversal - mach3 seems to not obey the acceleration constraint... (20in/s^2) (you can also see how steep the velocity lines are..) Probably almost 2 times the acceleration constraint. (I have seen worse)




The next 2 are linuxcnc




sam

[eldata]

I'm guessing that constant velocity path control mode (G64 code active) is the culprit as it was in my case. Mach3 has this mode set by default. Change the motion mode from CV to Exact Stop in general configuration and take measurements again. Or, better still, leave the default CV mode set and check the "Stop CV on angles >" option, setting it to 179 degrees. See post #42 above.