This is about the torch height issue. You might look at this posting on another topic.
And to clear up some questions with gcode: SheetCAM generates a xxx.tap file and Fusion 360 generates a xxx.nc file. They are basically the same thing to FireControl.
If you would like a brief start on understanding the gcode (I know you said you have some experience with it, so I will give you the nearly complete listing of gcode commands):
G-Code Cheat Sheet of Common Commands.pdf (186.4 KB)
G-Codes Explained_ An Introduction to Common G-Code Codes.pdf (201.6 KB)
I get lost in this one:
Every G Code for Your CNC [The Complete List] - Machinist Guides.pdf (1.6 MB) (some do not apply to plasma cutting)
Here are the most important/often used g-code commands:
G-code explanations with information compiled from notations from @DS690, Langmuir
document (G-Code Command Sheet) and www.thomasnet.com.
This is how the gcode will look at the beginning of each cut loop:
G92 Z0. - Set Z axis zero at the current location
G38.2 Z-5.0 F100.0 - Drive the Z axis down (up to 5 inches) @ 100 inches/min until it opens the
IHS switch on the Z axis
G38.4 Z0.5 F20.0 - Raise the Z axis (up to .5") @ 20 inches/min until it closes the IHS switch
G92 Z0.0 - Set the Z axis zero at the current location
G0 Z0.02 (IHS Backlash) - Raise the Z-axis .02" to account for backlash
G92 Z0.0 - Set the Z axis zero at the current location
G0 Z0.15 (Pierce Height) - Raise the Z axis to pierce height
M3 - Torch on
G4 P1 - Pause (in this case 1.0 seconds for Pierce Delay)
G1 Z0.06 F70.0 (Cut Height) - Lower the Z axis to cut height @ 70 inches/min
H1 - turn on the Torch Height Controller
Additional commands you might see include:
G00 Fast move
G01 Linear interpolation
G02 Circular interpolation CW
G03 Circular interpolation CCW
G17 XY plane designate
G20 Set English units (inches)
G21 Set metric units (mm)
H0 - turn off THC
M5 -torch off
Langmuir adds:
H0 is written into the preamble of every program to ensure that the machine controller has
control of the Z-Axis to perform the IHS sequence:
(v1.6-af)
G90 G94
G17
G20
H0
H1 is written once the torch has fired, delayed, and moved to Cut Height - before starting a cut
loop. Once the cut loop has finished and the torch must retract for the rapid to the next cu, the
Machine controller needs to be in control of the Z-Axis so an H0 is again written, generally
before the Torch Off (M5) command.
And the last line of code must be: M30 - end program
The very last line needs to be the program speed (cut speed) in parenthesis like (PS120) so this
will appear as:
M30
(PS120)
Pre-amble
Version Comment
The first line in a FireControl Posted Program contains a comment that identifies the version
of the post processor that generated the program. This comment is intended for use with the
two Langmuir Systems supported Posts: Autodesk Fusion and SheetCAM.
Note: If you are developing your own post, be sure to use either (v1.6-af) or (v1.6-sc) in the Wrst
line of your program to ensure that FireControl will accept it. If you publish your post online,
please make Langmuir Systems aware by contacting our support team and we can assign a
character code for your post so that future versions of FireControl will accept it without
needing to mask as Fusion or SheetCAM.
Ex.
(v1.6-af)
G90 G94
G17
G20
H0