Create a pause or rest in fusion360 for duty cycle

[blackdogironworks]

I’m cutting a rather large and complex part from 1/4" plate. Before the part is finished it will surpass the duty cycle of my razorcut 45. I can and have continued the part after the plasma cutter resets, but I am wondering if there is a way in Fusion360 to create a rest or pause in the cut path so if I know a part will exceed the cutters duty cycle I can pause in between some of the cuts so that it can rest and continue on its own. Anyone know of a way to do this? Thanks in advance.

[nicaDd]

search for PAUSE in the this forum. someone created an app where you can insert your tap file and add pauses after each cut and/or after a certain amount of cuts.

[JA6]

You can do this 2 ways.

1). STOP is M00. It will stop the program. Use cycle start to resume when you’re ready. I haven’t used this in Fire control, but it’s a universal command… So post result if you go this way.

2). Dwell is the cnc term for a pause with precision time. If you know your plasma unit needs a 2 min rest, then just insert this:

G04 P120

The P sets the time unit to seconds. (U is for milliseconds)

You don’t have to do anything… Machine will dwell for 120 sec, then resume program.

I would use the second method… Hands free, you can program for perfect match to cut and duty cycle.

[AultFab]

Have a long 10 minute cut with only one start and need the machine to pause and cool half way through as its beyond the machines duty cycle, the G04 pxx code pauses the torch but my torch stays on?

How to i implement this half way through a cut?

Thanks

[toolboy]

do not get upset…but I trust the old and simple way of hitting Pause…just the old spacebar…then resume when I am ready…

As fuxion360…or G-code adjustments…beyond me…

sorry…

[ds690]

You need to insert an M5 command on the line before the G04 command. The M5 turns the torch off. You will then need to insert an M3 command to fire the torch again after the pause.

If you have a THC, you may also need to insert an H0 command before the M5 to turn off the THC or it may throw an error when the torch shuts off.

Its much easier to just hit the pause button during the cut and then resume.

[KX9M]

Not sure if this works with FireControl but, some were inserting an M01 in their code for pauses… I think Sheetcam allows for this as well… It did work with Mach3…

M06 for beginners

you can also add an M01 below the M05 to pause before the next cut. I believe that will cut first, torch off, go to next cut and pause there until you hit cycle start again to cut the next part. I was doing that at first before i found the sheetcam PAUSE. I would add an M01 after every 5 or so M05’s so it’ll cut a few pieces then pause at the end of the 5th one. example: M05 M05 M05 M05 M05 M01 and so on…

Here’s one more thread to check out----->

Adding Pauses to G Code Files for duty cycle (Solved Slowed down rapids instead of adding pauses)

I had a need to add pauses between cuts to my g code files for a couple of reasons. I wanted to extend consumable life and also to allow my compressor to catch up after several cuts as it is a little undersized. I wanted to add a short pause after each cut to keep the nozzle cool and also a longer pause every 5 cuts to allow the compressor to catch up. I edited the files manually by adding a ‘G4 PXXX’ line after every ‘G0 Z1’ line where xxx is the pause time in seconds. This was ok to start …

[ds690]

It’s pretty easy to add pauses between cut loops, but he wants to add a pause in the middle of a cut loop and then start again on that same cut loop. It’s much more difficult, because you have to add commands to turn the THC off, turn the torch off, pause, turn the torch back on, turn the THC back on.

If you add pauses between cut loops, those commands are already there and you just add a pause between the loops.

[TomWS]

@ds690

turn the THC off, turn the torch off, pause, turn the torch back on, turn the THC back on.

It seems to me that THC isn’t necessary if you’re cutting thick material.

[JA6]

Totally Agree with ds690 on his assessment and advise. Once I have a file I trust cutting, I like to walk away and do other stuff. A PAUSE (M01) command will require the user to give input to continue. So I get why it would be convenient to have the auto stop and restart halfway through.

It might take a little trial and error to get the movement to stop, thc to not get confused, torch stopped, then let the pause run— then restart it all up. You need to set feed to 0 to stop movement just before you do the torch commands.

F0.0
H0
M5
G4 P120
M3
H1
F60.0

That snippet of code should let you paste it anywhere and work. Just change the F60.0 to whatever your cut speed for the file is. Since you’re already over a pierced portion of metal, you shouldn’t need to do a torch retract and pierce height to cut height change.

[AultFab]

Much appreciated, This is exactly what im looking for and dont want to baby sit parts to hit the pause button, I wont need to add this code very often but its nice to have a program completely automated.

[TomWS]

Is the first ‘F0.0’ necessary? If you don’t do that then you won’t have to issue the subsequent Fxx command to reset the speed.

[JA6]

Not sure if it’s necessary… I wouldn’t use it for myself, but I can read Gcode. I was going for a cut / paste for any location if you know nothing but the N line. F0.0 will allow deceleration to stop before torch turns off, so no gaps in cut result from delay.

I think fire control read ahead would deal with it fine, but doesn’t hurt to have it there…

[TomWS]

@JA6

but doesn’t hurt to have it there…

Good points and I agree. The only reason I questioned it was that the code is no longer ‘cut and paste’. You need to modify it to match the current cut speed.