Cutting issues on a DIY Table

[Pyrotech]

Running into an issue where the Test part is not cutting properly. the Fusion360 simulation shows the inner circle cutting, along with the Mach4 tool path display. The machine traces the outline of the inner circle but fails to fire the torch. the outer profile cuts with no issue.

https://www.youtube.com/watch?v=eiI27aQekOY

Not sure if it is a G-code issue or if its a hardware issue.


The table is not 100% done there are issues with the THC so the ARC Ok is forced on for testing and the torch mount is broke an needs replace, and of course the water table is not done yet. Just testing the machine in the various stages of construction


Specs:
Primeweld Cut60
16g Mild steel
30 Amps
110 IPM
55 PSI
Mach4 with ESS control Board

The G-code:

N10 G90
N20 G70

(Circle)
N30 G0 Z0.6161
N40 G0 X0.2562 Y-0.168
N50 G0 Z0.0161
M62P5 (+++ P=Output5, Turn Torch ON +++)
N60 G4 P0.5
N70 G1 Z0. F50.
N80 G1 X0.4267 Y-0.0696
N90 G3 X0.4742 Y0.0127 I-0.0475 J0.0823
N100 G3 X-0.4708 I-0.4725 J0. F110.
N110 G3 X0.4742 I0.4725 J0.
N120 G3 X0.4267 Y0.095 I-0.095 J0.
N130 G1 X0.2562 Y0.1934
M63P5 (--- P=Output5, Turn Torch OFF ---)

N140 G0 Z0.6161

(Outer Profile)
N150 G0 Z0.6161
N160 G0 X1.3193 Y1.2455
N170 G0 Z0.0161
M62P5 (+++ P=Output5, Turn Torch ON +++)
N180 G4 P0.5
N190 G1 Z0. F50.
N200 G1 X1.4177 Y1.075
N210 G3 X1.5 Y1.0275 I0.0823 J0.0475
N220 G2 X1.5275 Y1. I0. J-0.0275 F110.
N230 G1 Y-0.5
N240 G2 X1. Y-1.0275 I-0.5275 J0.
N250 G1 X-1.5
N260 G2 X-1.5275 Y-1. I0. J0.0275
N270 G1 Y1.
N280 G2 X-1.5 Y1.0275 I0.0275 J0.
N290 G1 X1.5
N300 G3 X1.5823 Y1.075 I0. J0.095
N310 G1 X1.6807 Y1.2455
M63P5 (--- P=Output5, Turn Torch OFF ---)

N320 G0 Z0.6161
N330 M30

[weldguy]

That is very odd, the timing of everything is off and your M62P5 command doesn't appear to turn the torch on when that line is executed. What post processor are you using?

[acourtjester]

I have not used Mach 4 but Mach 3 had a fire button on the main screen used to test firing the torch. Since this is a new DIY table could you have a wiring problem ( intermittent break in the fire circuit)?

[Pyrotech]

That is very odd, the timing of everything is off and your M62P5 command doesn't appear to turn the torch on when that line is executed. What post processor are you using?

this one

https://warp9td.com/index.php/faq/faq-m ... lasmaSetup

[weldguy]

OK chances are the pp is fine.

Not sure what plasma cutter your using but there could be some delay time between when it gets the fire signal and when it actually fires.

Many plasma cutters do this to provide enough time for the air to flow to the torch head prior to initiating the arc.

Many plasma table controllers accept an "OK to move" signal from the plasma cutter however your plasma cutter likely doesn't output that signal.

In this case you may just need to introduce some delay times. Do you see any delays that you can mess with in Fusion 360?

[Pyrotech]

Figured out the problem, with some help from CNC plasma table builders Facebook group. it was originally suggested that I change M62P5 to M64P5 and that change to cutting the inner circle first and not the outer profile. so I tried using the original M62P5 for the second cut. still same as before, but it did lead me to an interesting little bit information on the warp9 webpage ( the makers of my control board).

"To make sure the M10/M11 or M62/M63 works as desired, it is best to follow these guidelines:

The M10Px, M11PX, M62PX or M63PX command should be by itself on the line immediately before the subsequent G0, G1, G2 or G3 command. Don't mix other commands in between!"
well, I was curious about how to add a pierce delay if I need an axis movement right after firing the torch so Aa search on M62X with pierce delay led me to another page for the warp9 THC board.

Pierce Delay
Typically, most plasma users just use a G04 P# after firing the torch, to get a pierce delay. The provided SheetCam post processor would generate output which would look something like this:

...

N2170 M62P3 (>>>Torch ON<<<)

N2180 Z0.1500 (Force a small move in Z to make M62 fire the torch)

N2190 G04 P0.4 (DELAY)

N2200 G01 Z0.0600 F20.0 (Drop to cut height)

(Move X and Y here to make the cut)


After making the change in the G-code I was able to make 3 cuts that turn out as they should, minus the tuning that is needed to cut a the circle clean, it is a bit "off"

[weldguy]

That's great, glad you got it sorted out. Always learn a lot and save a lot going the DIY route