Programing a delay

[phil240]

I am new to this and an overall newbie. I just successfully programed multiple cuts and was able to successfully do the cut, however my machine turned off 3/4 through the cut.

I am learning as I go and beginning to understand what the duty cycle is. So is there a way that I can program in with sheetcam a pause for say 10 seconds prior to each pierce or say let it run for 2 minutes then pause for 45 seconds to cool down before resuming the cut?

[toolboy]

strange way of posting…

depends on what software you are using for post processing…
I believe sheetcam has one you can add for a pause after each cut…

you can stand by the table and tap the “pause” button and hit resume after a bit.

you have to be careful with your computer…if Firecontrol is loaded/paused and the computer goes to screen saver or to sleep…Firecontrol has been known to freeze up and require a complete PC reboot.

[phil240]

duplicate for some reason

sorry

[phil240]

I have no idea why it posted that way. I found it strange as well.

Post processing is being done in sheetcam. I just load the tap file from sheetcam into firecontrol.

By chance do you know where in sheetcam that would be? If not I’ll hit up the old youtube to help me find out.

[toolboy]

I said I believe…not sure though…not at my table right now so I can not answer properly…

[MechanicJon]

It’s in the edit tool

[nicaDd]

its in the toolset you create towards the bottom. That adds the delay at the end of each cut prior to moving to the next.

I believe if you do a search, someone created a program where you load your tap file and it’ll add a pause after a specified amount of cuts that you input and it adds the pause after the last cut but prior to cutting the next one.

I downloaded it but haven’t tried it yet.

[phil240]

Thank you for the help guys

[phil240]

Just for anyone who reads in the future. When you create the tool there is a setting for pause at end of cut.

I just don’t know if that’s for the end of each part when you group them or before each pierce. I will let you know the results.

[bobdobqb]

Here’s a link to the thread for the app that @S_Oates wrote and made available for adding pauses. Works great for me with either Fusion .NC or Sheetcam .TAP files. Also lets you add longer pauses as well every XX cuts.

Certainly helps for those of us with “less than industrial” setups

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 …

[nicaDd]

it’s for after each cut. It’ll complete the cut, PAUSE at that moment for the specified time (spraying water everywhere) then continue to the next and PAUSE again after that cut.

[TomWS]

I hesitate to jump into this learned thread, but, with very little effort (or knowledge for that matter), one could modify your Sheetcam post processor to insert either M0 or M1 into your code after each cut is finished. I would use M1 since I use the vastly superior Mach3 controller (JK) but I don’t think EmberControl recognizes or responds to M1. Mach3 has a button to ignore or honor M1 commands, very useful. Dunno about EmberControl.
Just sayin…

[phil240]

I am way to new to try and write in my own code. I wouldn’t even attempt that once experienced.

[MechanicJon]

Old post but I wanted to share what Les from Sheetcam shared with me. I use the pause after cut quit often and it makes a mess boiling the water because it pauses at the cut height. Edit the post proccesor code with this code and it will lift to rapid movement height then pause, lessing the mess.
Attached text file zipped up with proper formating of code.

In SheetCam go to Options->machine->post processor and click on the ‘Edit post’ button.
Look for function OnPenUp() near the end of the file. Replace the function with this version:

function OnPenUp()
ihs = pierceHeight ~= 0 and cutHeight ~= 0 --enable IHS if both pierce and cut are non-zero
post.Text (“H0\n”) – thc OFF, Machine in control of Z
post.Text (“M5\n”)
if (ihs) then
post.TextDirect (“G0 Z” … post.FormatNumber(25.4 * scale, “0.0##”) … “\n”) – Z to rapid height
end
if (endDelay > 0) then
post.Text (“G4 P”)
post.Number (endDelay,“0.###”)
post.Eol()
end
post.CancelModalNumbers()
end

post processor mod.zip (417 Bytes)