I’m getting a G28 at the top of the program, which I’m assuming is causing the behavior you’re describing. Mine also goes to the top of z, then to the first x,y location, then down to my clearance plane.
I don’t mind, since I’m usually over the tool setter when I touch start, so it raises high enough to clear anything before moving to start position.
Try this.
When you post process, in the post properties section, change “safe retracts and home positioning” to clearance height.
I believe @microarms nailed this one. It looks like the retract you’re seeing is from the first few lines in the gcode. Here’s a quick run-down through the first few lines and what they are telling the machine to do.
G90 G94 … -G90 absolute positioning and G94 feed mode “units per minute”
G17 … -G17 plane selection “X/Y”
G20 … -G20 Coordinates are in Inches"
G28 G91 Z0 … ***THIS IS THE LINE -G28 Go to reference position(zero, home, etc) -G91 relative positioning (telling the machine to use machine references not work 0) -Z0 Move z-axis to zero (straight up) This is done since this is usually the safest start position in order to clear any fixtures, parts of the work piece, etc.
G90 … -G90 return to absolute positioning
…Continues on to the actual job from here
As @FabLabRacing mentions as well, you can change this in the post process stage and by choosing clearance height instead of G28, the post output will remove the G28 line completely.
However, the machine should not error out when going to machine Z zero. Before running the job does the machine home fine and are the soft limits enabled? If the soft limits are set correctly with the .050" offset, the machine should stop before even hitting the limit switches.
Sorry guys my job calleth me. YOU ARE EXACTLY CORRECT. I thought the G28 was the rapid move speed and the retraction was what you get for the height. The post shows G28 and I really thought that was correct but WOW was I off. Thank you guys for helping me on this. This will not be forgotten to soon:). I am just learning Fusion so I am sure I will mess up again but I am 1 step closer!!
The G18 is being generated based on one of the lead-in moves in Fusion 360. G17, G18, and G19 are used to define the work plane. The common table top is G17 (G18 and G19 define vertical planes). If you look closely at the toolpath simulation, you can see the arc that is triggering the work plane change. Enter 0 as radius in this lead-in and the work plane change will be eliminated.