Hello everyone, as the title states I'm having some problems with the workstations in Control. I have a turning/4th axis station for my cue making. And I have g55 set for that. The problem is after I run a program it changes back to g54. I have to constantly change it back otherwise my program starts to run completely off from its zeros. How do I get it to stay on the set station. Thanks for any help you guys can provide.
EVERY program you run must set the Work Coordinate System it expects to be using. ALL programs, without fail, it is the only safe way to operate. Similarly they must also always set any modes they expect, like G90 G17 G46 etc, and also G20 or G21 for inch/metric mode . The controller boots in G54 mode, so to switch to G55 you can create a macro that runs at startup (may confuse other operations) , but CONTROL does have a button for switching WCS systems
Not sure if I put the right code in or put it in the right spot but when I added a line of G55 to the program it f'ed everything up. To the point where I had to remove control and start over. Every time I zero something out my work station was changing.
then there is something wrong with your process (-: to work in WCS G55: home the machine (defaults to G54 at switch on!) select G55 in CONTROL jog to origin point and 'setZero' or use a probe to find the workpiece origin, this sets the offsets for G55. load Gcode that uses G55 and has G55 in the gcode. check that you have G55 selected and that 'goto X0 Y0' goes to the correct origin on the workpiece run Gcode I have done jobs using all 6 offsets (G54 to G59) in one Gcode file, this does work.
at what spot do i add the g55. later today i can screen shot the program and upload it for you to look at.
no screenshots, thanks, just upload the file itself. even easier is to look at Gcode generated by any CAM system, for example SketchUcam, the Gcode plugin for Sketchup (Generated by SketchUcam V1.5a-241a161) (Bit diameter: 3mm) (Feed rate: 2540mm/min) (Material Thickness: 6mm) (Material length: 550mm X width: 1000mm) (Overhead Gantry: true = Conventional Cut) (Plunge Depth first) (Optimization is ON) (Arc Feedrate scale is ON) (Origin offset ~ 22mm, ~ 25mm) (www.PhlatBoyz.com) G90 G21 G49 G17 F2540 G54 G53 G00 Z0.0 G00 X0 Y0 M3 S15000 G00 Z3.0 X-1.5 Y-1.5 G00 Z0.5 G01 Z-6.0 F2540 X101.5 Y56.5 X-1.5 Y-1.5 G00 Z3.0 G00 X0 Y0 (home) G53 G00 Z0.0 M05 M30 Just replace the G54 with whatever you need. All Gcode should have a header like the one you see just above the G54, setting modes that this code expects (since modal settings stay set between jobs, every file must set its own modes, never assume the mode is correct) G90 absolute coordinates will be used G21 metric coordinates and feedrates G49 remove tool offsets G17 use XY plane for arcs F2540 default feedrate
