Pausing for plasma cool down

Hi,

Im making a table tops out of 6mm stainless steel plate in the design of a monsteria leaf. As the outside edge is rather long I need to pause the job at least three times to let the plasma cutter cool down. Im hoping someone can give me some advice on the best way to do it other then messing with the g code. I was thinking about just leaving some small tabs then manually snipping them afterwards that way I can pause machine between on and off sequence. Any advice would be appreciated.

Cheers from West Oz.

1 Like

I would add the tabs in sheetcam and add a pause after cut for a few minutes.

Not sure if that would work though since I don’t think sheet cam generates another start point when you have it create the tabs for you. If that’s the case I’d make the original file with tabs in it and use pause after cut in sheetcam.

1 Like

Messing with the Gcode would be the easiest way to do I think. I use sheetcam for my toolpath generation so if you use fusion the process will be different but same concept. On your final cut you can do tabs like your saying, run the post processor and then open the Gcode in note pad and fire control. Use fire control to find the Gcode line where your cut ends at a tab. It should say something along the lines of…

G1 X25.00 f150
M5

Your really just looking for that M5 command because thats what shuts the torch off, after the M5 command add a line that says G4 pxxx and replace the 3 x’s with the time in seconds you want the plasma to dwell and cool off before continuing. You can also use sheetcams native code editor to do the same, whatever you prefer. Hope that helps some.

You could also setup a code snippet you have sheetcam automatically insert with the tabs but Im not super familiar with the process to do this

1 Like

Hi Thanks for the info,

Shame sheetcam doesn’t have a command that after x amount of time it could automatically pause then restart from same spot. Will have a crack at g code have read a little about adding G4 after M5.If its one continuous cut line however there won’t be a m5 until the end. I guess I can just insert a m5 halfway through the code but also need to know how to pause the x and y movement… rabbit hole haha.

Think just adding tabs might be easier.

I am not sure but if you select only parts of the geometry and generate that g-code will that work. Example: If your cutting a large square and it is thick metal and you do not want to destroy the tip and shield. Can you select each side and do a separate sequence? You would have 4 programs (square 1, square 2 and so on). I have had to do something similar. I select the geometry I want, post it. And then to the next. I have three programs with the same start point on the same part and cut all three one after the other giving time for the cool down. You said you have paused the program so I was wondering if this may work for you?

You can if they are separate lines. If they’re a closed shape it’s one object & path. For your example of a square I’d make 4 lines that extend past the corners so you’d still get a square but could control the sequence & timing of cutting each line.

I understand that. I was just using that as an example. If the leaf he is working on isn’t a complete geometry if he could select the geometry in segments? But I guess it is one full line.

To Langmuir Systems Tech guys: could you add an option for this in the patterning section of fire control? I’ve designed parts and then use that patterning section instead of doing the pattern in fusion and having to have the computer process all that code so now I’ve got now way to edit the code and add a pause. seems like a simple thing to add though? Maybe a button with an editable time section next to it??

I may be jumping the gun…or misreading your post…I am known for that…

but is there not a button called PAUSE on the firecontrol screen that …pauses the torch where ever you want…then the as most torches do they go into post flow…often adjustable…then when you press pause after what ever time you want…it starts again…

seems easy

1 Like

yes, that works… I was looking for a way to automate that. One the parts I’m currently cutting out if I could have a whole sheet set up where it would automatically pause and let the torch cool then I wouldn’t have to keep coming back and wasting time on it. I could be working on countless other things while it’s cutting for me and not overworking the machine

the problem of walking away…you could have a tip up…and THC issue…and ruin a whole sheet…

just saying…I know…it happens…

1 Like

You can do that in sheetcam 2 different ways. The easiest is to extend the delay before cut in the settings, that way it will move to the pierce location but won’t start till the timer expires. You can have 10 seconds, shorter or longer. Just note that if you still have post air flowing it maybe splashing water everywhere!

The other way I do it sometimes if I want to make sure there is no slag stuck to the tip when cutting thick stuff, also helps with cool down. This way is not automated, you have to click resume although rather then using the M code for pause, There is probably M code for delay.

On the left there is a button for custom code. I think it’s called custom code, if not it’s something very similar. In that code add your M?? Command. Then using the contour selection create a different layer for every line or group of lines. That’s as easy as clicking on the lines holding shift (or dragging a box) right click and create new layer. Now on the bottom left when you to start creating your commands. Select cut and then your tool and layer etc. After that insert your custom code. Then select cut again for the next layer, then another custom code etc etc.

That way after every cut, fire control will pause until you press resume. Gives you machine time to cool down, check out the tip or even replace it and remove tip ups.

I’ve never tried pausing fire control mid cut. I was under the impression you can’t as it has no code to start another pierce location. You could go back in the code and start that cut over but I haven’t had much luck running over a already cut line. If I have to, to save a piece. Reduce the pierce time and speed up the movement. When you get close to the fresh material click reset. That’s assuming your speeds and set in your g code. Plan B is to load the file back in sheet cam and move the piece point to the location that the arc went out then load it back into fire control, assuming you have not moved the metal in the table. If your halfway though your cuts you can deselect the previous completed cuts.

unfortunately I’m running on Mac and not using sheet cam so I don’t think I can use any of that… also, I’m currently set up using a Hypertherm 30 air so I need a delay time of about 7.5 minutes the its running at max capacity. I think I’ve sorted out how to do it by just setting up multiple cuts from fusion using the same setup so that FireControl doesn’t lose its location. Haven’t tried it on anything huge yet but it seems like it should work