Try this code:
G00 A000 Z250
G01 A180 F12
I've been reading and attempting everything I have found. My 4th axis is working surprisingly well, but its very jerky. I'm using fusion 360 with usb smoothstepper and have tried various smoothing settings, slower feed rates and it all yields the same results. Theres a video below with some sample code.
I see lots of people with harmonic drive 4th axis and mach3 and they all seem so smooth. The pausing is adding a decent amount of machining time and leaving marks on my finish. Does anyone have any ideas what's causing the jerkiness/stuttering?
Code:Z0.6334 A-6.574 F2836.3323Z0.6395 A-9.401 F2653.4703 Z0.642 A-10.341 F7665.2579 Z0.6468 A-12.217 F3861.3871 Z0.6488 A-13.152 F7937.2541 Z0.6507 A-14.087 F7996.3277 Z0.6523 A-15.02 F8146.2995 Z0.6538 A-15.953 F8273.91 Z0.6551 A-16.884 F8360.7096 Z0.657 A-18.745 F4297.0773 Z0.6582 A-20.603 F4442.1249 Z0.6585 A-21.531 F9124.6597 Z0.6584 A-23.387 F4677.8014 Z0.6582 A-24.315 F9147.9255 Z0.657 A-26.171 F4444.8371 Z0.655 A-28.029 F4297.6506 Z0.6537 A-28.958 F8398.9712 Z0.6522 A-29.888 F8277.2542 Z0.6506 A-30.818 F8155.041 Z0.6487 A-31.75 F8035.2122 Z0.6467 A-32.682 F7924.6533 Z0.6445 A-33.616 F7856.4056 Z0.642 A-34.55 F7700.0207
Similar Threads:
Try this code:
G00 A000 Z250
G01 A180 F12
Take a look at the feed speeds in the G code, they are all over the map. Every line has a different speed. The action in the video looks like it is following the G code commanded speed.
Jim Dawson
Sandy, Oregon, USA
Looks like Jim is the winner!
Wow. I wonder how that happened?.
Need to figure out how to stop that happening, wouldn't fancy having to edit every line of code to delete the F rates!
Must be something in Fusion. Different feedrates for smoothing, roughing, finishing, plunging, cornering etc must have been set.
Hi, I have the same problem with the rotary extension in fusion360. I set :cutting feed rate, lead in and lead out, ramp and plunge all to the same feed rate. When I generate the gcode every line has it's own different feed rate and gives a jerky cut. Its also quite a bit slower then what I had running before where I added the rotation numbers manually. Anyone have any suggestions?
here are a few lines of the code:
O0001(ROTARY1 2)
G0 A-90.
X0.4 Z19.798
G1 X0.392 Z19.417 F1000.
Z17.798
X0.38 Z17.702
X0.342 Z17.605
X0.278 Z17.518
X0.192 Z17.452
X0.096 Z17.412
X0. Z17.398
G93 Z17.395 A88.833 F18.4136
Z17.398 A267.749 F18.4053
Y-1.998 A270.35 F1262.6583
Y-1.993 Z17.395 A271.173 F3915.5086
Y-1.986 Z17.398 A272.445 F2537.1061
Y-1.98 Z17.395 A273.517 F3007.2727
A273.526 F355836.3751
Y-1.973 Z17.398 A274.771 F2591.9728
Y-1.967 Z17.394 A275.906 F2839.2202
A275.915 F356034.426
You could edit the code, searching and replacing all those A axis speed commands. Or get DeskProto and write better A axis code.
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]
The G93 is the cause of this problem as when using a G93 this will require each line of code to have a feed rate
This G code specifies that all F (federate) values are interpreted as strokes per minute. In other words, the time (in seconds) to complete the programmed motion using G93 is, 60 (seconds) divided by the F value.
See if you can use a G94
Feed Per Minute (G94)
G94 G-code is a modal G-code. G94 instructs the control to interpret feed commands as
Inches/minute or mm/minute for linear moves.
degrees/minute for rotary moves.
Inches/minute or mm/minute for a combination of linear and rotary moves.
When a combination of linear and rotary moves is programmed, the rotary moves match the time it takes to make the linear moves.
Mactec54