Error multiple commands

[akillion]

Good afternoon,
I have been trying to run a file out of fusion 360 as well as inventor. Everytime I try to run the file through win cnc I get "Error multiple commands" or file not found. I am using the wincnc_noatc postprocessor. I have been searching all over trying to get this taken care of but can't figure out what I need to do to get a post processor in inventor or fusion to work with win cnc. I could not attach the whole file so I copied and pasted some of the code below.
Thanks a ton in advance

[1001]
[T1 D=0.25 CR=0. - ZMIN=-2.582 - ball end mill]
G90
G20
G53
[Adaptive1]
S7330
M3
G0 X0.0312 Y2.0739
Z0.6
Z0.2
Z0.1
G3 X-0.0312 Y2.075 Z0.0966 I-0.0312 J0.0006 F55
X0.0312 Y2.0739 Z0.0931 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0897 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0863 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0829 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0794 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.076 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0726 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0691 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0657 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0623 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0589 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0554 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.052 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0486 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0451 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0417 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0383 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0349 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0314 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.028 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0246 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0211 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0177 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0143 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.0109 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0074 I-0.0312 J0.0006
X0.0312 Y2.0739 Z0.004 I0.0312 J-0.0006
X-0.0312 Y2.075 Z0.0006 I-0.0312 J0.0006

[Gary Campbell]

If you want a correct answer, attach the file that produced the error. The only issue I see with the included text is that there is a "G53" call with no axis parameters.

[jmd_82]

Add the line: g2modal=1 (without quotes) to the WinCNC.ini file

[emriffle]

Hey all, just wanted to share the resolution I managed to get to when I had this same error.

It took many days of researching and learning for my novice rear end to get this figured. I tried literally everything i could find on these forums and others, and just couldnt get the clean gcode that Wincnc was looking for.

What Wincnc wants to see, is a Gcode and coordinates...on every line. It will not read stacked coords under the same operation:

Here we see multiple coordinates for the g1 operation. This popped the multiple commands error for me.
S18000M3
M37T4
G0X8.1199Y44.2536
G43Z1.95
Z0.95
G1Z0.8F40
X8.0074Z0.7862F100
X8.7968Z0.6893
X8.0074Z0.5923
X8.7968Z0.4954
X8.0074Z0.3985
X8.4021Z0.35

Here is a different code, but made with one singular change to the Post coding.This reads and runs fine through Wincnc...because every bloody line has its g mode.

N18 S18000
N20 M3
N22 G0X19.075Y12.7
N24 G43
N26 G0Z0.795
N28 G0Z0.395
N30 G1Z0.2344F250
N32 G1Z-0.0125
N34 G1Y38.9187F500
N36 G3X17.2Y40.7939I-1.8751J0.0001
N38 G1X14.7615
N40 G1X14.6365Z0.05F500
N42 G1X14.3865
N44 G1X14.2615Z-0.0125F250
N46 G1X10.7625F500
N48 G3X8.8875Y38.9187I0.0001J-1.8751

This is all probably more than is necessary for the point of this...
if youre getting the multiple commands error because your gcode spits out like the first example, this is the change:


variOutput=createReferenceVariable({prefix:"I",force:true},xyzFormat);
varjOutput=createReferenceVariable({prefix:"J",force:true},xyzFormat);
varkOutput=createReferenceVariable({prefix:"K",force:true},xyzFormat);

vargMotionModal=createModal({force:true},gFormat);// modal group 1 // G0-G3, ...
// var gPlaneModal = createModal({onchange:function () {gMotionModal.reset();}}, gFormat); // modal group 2 // G17-19
vargAbsIncModal=createModal({},gFormat);// modal group 3 // G90-91

the bolded {force:true} behind the motionmodal command

This is located ~200 lines down, under the various formats.

Sorry if this doesnt make much sense, im still building my understanding of all this. This one command fixed the issue entirely for me though.