Qtplasmac M3 detected error.

Start
Prev
1
Next
End

paulsao
Topic Author
Offline
Elite Member

25 Apr 2022 15:30 #241212 by paulsao

Qtplasmac M3 detected error. was created by paulsao

Greetings to all. I was trying to make some parts with punching, but I have the following error in Qtplasmav v1.222.172
**-M3 command detected before movement
**-Lines: 39,48,57,66
The code is the following:

(1001)
N10 G21
N15 G90 G40
N20 G17 G91.1
N25 G64 P0.254 Q0.254
N30 M52 P1.
N35 M65 P2.
N40 M65 P3.
N45 M68 E3 Q0.

(HOLES TO CENTERPUNCH)
()
(- THIS SECTION IS SET UP TO CENTER PUNCH THE SELECTED HOLES. -)
(- ANY OTHER TYPE OF OPERATIONS IN THIS SECTION WILL NOT WORK CORRECTLY -)
()
N50 F999999.
(PLASMA CUTTING)
(THROUGH CUTTING)

N55 M190 P1.
N60 M66 P3. L3 Q1.
N65 F#<_hal[plasmac.cut-feed-rate]>
N70 G0 X76.34341 Y24.10845
N75 G0 X80. Y20.
(CENTER PUNCH THE HOLE ONLY)
N80 M3 $2 S1
N85 G91
N90 G1 X0.00001
N95 G90
N100 M5
N105 X76.34341 Y24.10845
N110 X50. Y38.
N115 Y50.
(CENTER PUNCH THE HOLE ONLY)
N120 M3 $2 S1
N125 G91 //////////***/////////
N130 G1 X0.00001 ///////////***////////
N135 G90
N140 M5
N145 X50. Y38.
N150 X22.53924 Y24.87876
N155 X20. Y20.
(CENTER PUNCH THE HOLE ONLY)
N160 M3 $2 S1
N165 G91
N170 G1 X0.00001
N175 G90
N180 M5
N185 X22.53924 Y24.87876
N190 X23.65659 Y75.89156
N195 X20. Y80.
(CENTER PUNCH THE HOLE ONLY)
N200 M3 $2 S1
N205 G91
N210 G1 X0.00001
N215 G90
N220 M5
N225 X23.65659 Y75.89156
N230 X74.51456 Y79.60001
N235 X80. Y80.
(CENTER PUNCH THE HOLE ONLY)
N240 M3 $2 S1
N245 G91
N250 G1 X0.00001
N255 G90
N260 M5
N265 X74.51456 Y79.60001
N270 F#<_hal[plasmac.cut-feed-rate]>

(PERFIL 2D3)
()
(- THIS SECTION IS SET UP TO CUT SMALL HOLES ONLY. -)
(- IT WILL AUTOMATICALLY SLOW THE CUT SPEED FOR THE HOLES BASED ON THE SETTING IN THE PARAMETERS. -)
(- IT WILL ALSO CREATE AN ARC LEAD-IN FOR EACH HOLE STARTING AT THE CENTER OF THE HOLE. -)
(- ANY OTHER TYPE OF OPERATIONS IN THIS SECTION WILL NOT WORK CORRECTLY -)
(- THIS SETUP HAS OCCURRED DUE TO DISABLING LEAD IN ON THE LEADS PAGE -)
(- BE CERTAIN YOU HAVE ALSO SET PIERCE CLEARANCE TO 0 OR YOU WILL NOT GET THE CORRECT RESULTS -)
()
N275 G0 X100.5 Y80.
N280 G1 Y20.
N285 G2 X80. Y-0.5 I-20.5
N290 G1 X20.
N295 G2 X-0.5 Y20. J20.5
N300 G1 Y80.
N305 G2 X20. Y100.5 I20.5
N310 G1 X80.
N315 G2 X100.5 Y80. J-20.5
N320 M5

N325 G0 X0. Y0.
N330 G90
N335 G40
N340 M65 P2.
N345 M65 P3.
N350 M68 E3 Q0.
N355 M5
N360 M30

Please Log in or Create an account to join the conversation.

snowgoer540
Offline
Moderator

25 Apr 2022 17:11 #241222 by snowgoer540

Replied by snowgoer540 on topic Qtplasmac M3 detected error.

The g-code filter currently expects to see G0 or G1 in the line before the M3 command. You just have the X and or Y values currently (because you had already specified G1. I will discuss with Phill and see if we need to change the thought process here a bit on our end.

In the meantime, you can work around this by adding G1 to the lines that don't currently have it.

So as an example, change this:

N105 X76.34341 Y24.10845
N110 X50. Y38.
N115 Y50.
(CENTER PUNCH THE HOLE ONLY)
N120 M3 $2 S1

to this:

N105 G1 X76.34341 Y24.10845
N110 G1 X50. Y38.
N115 G1 Y50.
(CENTER PUNCH THE HOLE ONLY)
N120 M3 $2 S1

If you make the similar changes to the other 3 places this shows up, it should get you through until we can take a closer look to see if/how we want to handle this situation on our end.

The following user(s) said Thank You: paulsao

Please Log in or Create an account to join the conversation.

paulsao
Topic Author
Offline
Elite Member

25 Apr 2022 17:43 #241226 by paulsao

Replied by paulsao on topic Qtplasmac M3 detected error.

Thank you very much for your timely help.

The following user(s) said Thank You: snowgoer540

Please Log in or Create an account to join the conversation.

snowgoer540
Offline
Moderator

26 Apr 2022 10:22 #241276 by snowgoer540

Replied by snowgoer540 on topic Qtplasmac M3 detected error.

I looked at this a bit more last night; I don't believe there's anything to "fix" on our end.

It seems like the post processor/process lead ins, lead outs, etc. might need some attention. After each M5 there are 3 X/Y moves, which really only needs to be one (to get to the next pierce spot). It also occurred to me that these should be G0 moves and not G1 moves as I suggested earlier. If you're using Fusion360, I know that they remove some rapid moves on output for the free "hobbyist" license. So that explains why they are missing (and normally would be there). If that's the case you'll just have to manually add them back.

I suggest looking into sheetcam if you plan to do any kind of production work, etc. and can work it into the budget

. You can still use Fusion for the dxf design and then send it to sheet cam for all the process manipulation. In the long run it will likely save you a lot of grief.

The following user(s) said Thank You: Clive S, paulsao

Please Log in or Create an account to join the conversation.

Start
Prev
1
Next
End

Moderators: snowgoer540

Time to create page: 0.129 seconds