Hi, When I make simple component ( circle with smaler circle inside ) and I want to cut with plasma all simulation are ok but... when I post gcodes only one M3 commande ( firing torche ) are at beginning and one M5 ( stop firing ) at the end ? I use the last Openbuildsfusionpostgrbl.cps post processor and try with generic GRBL post processor and same result but langmuir firecontrol seems to work ok for M3 command. Link for my video : Gcodes : I use student version of Fusion 360. I try to make 2 setup 1 for each cut and same result. This is the gcodes: (This file contains the following operations: ) (1 : 2D Profile4) ( Work Coordinate System : G54) ( Tool 2: Plasma Cutter Diam = 1.2mm) ( Machining time : 10 sec) (2 : 2D Profile2) ( Work Coordinate System : G54) ( Tool 2: Plasma Cutter Diam = 1.2mm) ( Machining time : 2 sec) G90 G94 G17 G21 (Operation 1 of 2 : 2D Profile4) G54 (Plasma cutting with GRBL.) M3 S1000 G0 X55.93 Y28.5 F1000 G1 X51.6 Y26 G2 X0.4 Y26 I-25.6 J0 X51.6 Y26 I25.6 J0 G1 X55.93 Y23.5 (Operation 2 of 2 : 2D Profile2) (Plasma cutting with GRBL.) G0 X26.07 Y23.5 F1000 G1 X30.4 Y26 G3 X21.6 Y26 I-4.4 J0 X30.4 Y26 I4.4 J0 G1 X26.07 Y28.5 M5 G0 X0 Y0 M30 % Can you help me please. Best regards
That post has only been written and tested for router and laser cutting (-: but let me get this straight, you want an M3 at the beginning of every cut and an M5 at the end of every cut when in plasma mode? let me see what I can do.....
ok, grab the latest code from OpenBuilds/OpenBuilds-Fusion360-Postprocessor (not the release, you want the green button and the .zip file download) and your plasma cut should be happy.
Thank you for your fast reply (-: I try your updated post processor and it work great for my test model but at second M3 command S1000 don't appear after M3 but its not a big problem I can add S1000 manually. In another test with plasma cutting... when I used gcodes on Openbuilds control many lines are missing ? Can you help me ? Regards Syl
Hi @Sylvain Michaud - the gcode is there, CONTROL is just failing to display it correctly. @Peter Van Der Walt this is that display bug on CONTROL (I thought you had fixed that!?) yet bCNC shows all of it, exact same input file..
This does not matter, the S command is modal, GRBL remembers the last setting and uses it for the next M3 command. I have just run your code through my test controller and it acts exactly as expected with the torch coming on for each letter and going off in between the letters.
I remember working on it, was something to do with the states when something preceded a G2/3 right? You wouldn't happen to remember where the old discussion was, did a couple searches can't find it off hand. Will check from this sample gcode in the meantime
it wanted a G word after an S word, a comment in my code says Code: // force a G word after a spindle speed change to keep CONTROL happy but now there is something else going on because we have M3/5 sprinkled through the code.
Please update again as I have just uploaded an improved version. I noticed in your drawing that the tool routes around some letters when moving to the next letter to avoid crossing an already cut area. Those moves were so, now they are rapids. If you turn off 'keep nozzle down' in the toolpath and turn on 'Use Z movements' in the post then the torch will lift up for those moves. also, your S will cut better if you turn on smoothing in the toolpath. Without smoothing it is thousands of small line segments, with smoothing it is a few arcs and a handful of line segments.