I just got my system switched over to Linux EMC and i'm having some issues with the standard G1 command producing straight lines at high feed rates. When I slow it down it works fine, but i'm trying at 120IPM just to do a square (rotated 45 degrees so it looks like a diamond.. kinda). At slow feed rates it's fine, but once I bump it I can hear it accelrate and decelrate incorrectly.

The backplot actually shows the curves too, i'm not sure how they do backplotting, but it shows the curves on the corners.... I assumed maybe this was just due to a sampling rate of some kind but it looks identical what is produced, and it ain't straight.

It's not a backlash issue, not that i don't have some, but i have very minimal, and it's only on X axis, around 0.05 inches. Which i'm getting a 1/4 to 1/2 inch curve... makes no sense.

I'm cutting foam if anyone is wondering why i'm trying to move so fast... Mainly I want to do 3d cnc foam cutting.

I'm just wondering if I need any other prepending G codes to set something else up differently. Also maybe there is something in the ini file that is doing this.. i dunno.

Also the curves would make sense if I was doing a G41 G42, i'm not.. and I do issue G40, not that it matters since all I do is G1 moves.

Background on machine:
Gecko servo drives, regulated 36volt power supply with amperage usage output (the whole system never goes over 1.5amps, small gantry). It was originally a hobbycnc design with completly rebuilt gantry and Z axis. Servos are us digital encoders with a nice DC motor (100watt, nice magnets good torque).

Thanks for any help,
Ross

Hi I don't really know if this helps but can you put in a stop pont at the end of the lines 10 nanoseconds to make sure it goes to the corner. Or put a radius of .1mm at the corners.

Hi, Ross.

AFAIR you get this emc behaviour when using emc in G64 (continuous mode)
with low acceleration values in emc.ini. So you can try to increase
DEFAULT_ACCELERATION and MAX_ACCELERATION.
Or try to use G61 (exact path mode) or G61.1 (exact stop mode).

I would suggest G61, because G61.1 slows down machining to much.


Regards
Frank


--

Homepage (http://www.fjungclaus.de)

Ross, the minimum radius of a corner in G64 mode is feedrate^2/accel.
What are your .ini values?

Les

Thanks for all your responses... I've modified the ini file to have much faster acceleration settings in the TRAJ section and it seems to help a lot. I also read up on the G64 G61 modes, haven't tried them yet, but I understand why I would use them.

Really i was testing rapid movments for foam, there's no way I could mill at 120IPM doing any kind of real material, I just did some 3d foam tests though at 120ipm (i really dont' think it was going quite that fast) It was hauling though compared to the old stepper motors, at least 8 times faster. It was quite cool.

Heres what I changed my ini file to, the TRAJ section at least:
[TRAJ]

AXES = 3
COORDINATES = X Y Z
HOME = 0 0 0
LINEAR_UNITS = 0.03937007874016
ANGULAR_UNITS = 1.0
CYCLE_TIME = 0.010
DEFAULT_VELOCITY = 0.0167
MAX_VELOCITY = 2
DEFAULT_ACCELERATION = 30
MAX_ACCELERATION = 30
PROBE_INDEX = 0
PROBE_POLARITY = 1

I had acceleration set at 4 and 4 before, I set them low just because really i didn't know what to set anything too, 30 seems a bit high, the motors can handle it, but the machine isn't quite as strong as I thought it was eheh.

Thanks for your help though, i'll obviously use G61 when I need the exact path, course when i'm milling a piece like that i'm usually running no where near 120ipm, so it isn't a problem.

Thanks,
Ross

Program tip.
Using G4 dwell at corners of contours can signifgantly sharpen your profiles. This is a big help on lathes.

Machine setup Tip.
You seem to have found the main problem though in your .ini file. 120 IPM is cruising. Even the Haas machines that I run don't go that fast. I machine aerospace plastics and have pushed the feeds way up sometimes. The feed rate shows on the status display but it really never gets there. It has to do with the accel and decel rates of the motors as you found on your setup. The max feeds and rapids etc. are only reached when traveling a relatively long distance as the machine has to be able to slow back down in time to stop at the presrcibed point in the program. This is the function of the settings in your .ini file.