My x and y speeds on my plasma table are not following the gcode. I cut a 60mm diameter circle and it takes 27 seconds. That is about 500 mm/min. The g-code has F2000 for speed. Attached are the g-code and settings. Nema 23 stepper motors. Black Box 4x. Any help would be appreciated.
Are you using OB Control? If so, double check your feed rate slider. The max feed rate settings look fine, but since its a bunch of small moves, it may have to do with acceleration. Someone smarter than me will know. Also noticed that your steps per mm for each axis is set to 250. Its a sign that you probably havent calibrated your machine.
Ok. Calibrated the steps per mm. It was the arc issue; I drew a rectangle in Openbuilds and it was must faster. I downloaded Sketchup Maker 2017 and Sketchup CAM. I'm struggling to figure out how to setup my z axis touch off with the switch from openbuilds. The g-code I use in openbuilds is below. I'm not sure what settings to change in sketchup CAM G38.2 Z-30 F100; Probe G10 L20 Z-2; Set Z Zero
Acceleration is set quite low too: $120=10.000 ; X-axis acceleration, mm/sec^2 $121=10.000 ; Y-axis acceleration, mm/sec^2 $122=10.000 ; Z-axis acceleration, mm/sec^2 Have a read through github.com/gnea/grbl/wiki at some point.
SketchUcam has a laser mode but not a plasma mode. To get plasma touchoffs you will have to do some searchandreplace in the gcode file. I don't understand what you mean by having M5? M3 is 'spindle on' M5 is 'spindle off' in 'GRBL power mode' M4 is spindle on (read the GRBL wiki to learn how power mode works with acccleration., you DO NOT want this with plasma) On the hole featureoptions menu you want to turn power mode and feedrate in arcs off (false). Also make sure you set the spinde RPM in the parameters dialog to the correct value for 'fully on', depend son your GRBL settings for max spindle speed Sketchup Menu Tools|Phlatboyz|Options|Hole Feature Options do read the help, the plunge hole dwell time is also used for laser output. (big blue question mark in the toolbar) Here is my quick sample in laser mode with the above settings, I drew 3 rectangles and outside cut them, nothing fancy. Code: (Generated by SketchUcam V1.5c-fc1fbff) (Bit diameter: 1.0mm) (Feed rate: 750.0mm/min) (Plunge Feed rate: 450.0mm/min) (Material Thickness: 6.0mm) (Material length: 780.0mm X width: 450.0mm) (Overhead Gantry: false = Climb Cut) (Plunge Depth first) (Optimization is ON) (Arc Feedrate scale is OFF) (LASER is ON) (www.PhlatBoyz.com) G90 G21 G49 G17 F450 G00 X30.978 Y35.435 M05 ; ensure laser off M03 S12000 ; laser on, 12000 is my max rpm set in GRBL setting $30 G01 Y82.635 F750 G01 X78.178 G01 Y35.435 G01 X30.978 M05 ; laser off G00 X83.51 Y68.564 ; move to next rectangle M03 S12000 ; laser on G01 Y112.164 F750 G01 X177.71 G01 Y68.564 G01 X83.51 M05 ; off G00 X97.335 Y51.346 ;move M03 S12000 ; laser on G01 X177.735 F750 G01 Y18.846 G01 X97.335 G01 Y51.346 M05 (home at end of job) M05 G00 X0.0 Y0.0 M05 M30 to convert this to plasma code you will need to search for the M3 lines and replace with your touchoff code and then the M3 line again, thus inserting the touchoff code before all the M3 lines.
