Program Pause

[CosmosK]

It would be so cool if I could insert a pause into a program in VCarve.

I'm doing it manually now, adding

(text to display)
G4

into my G code.

The problem is, when I am programming and need to make a pause, I'm not ready to compile everything down to G code yet. It would be so cool if you could do this in VCarve!!

[Leo]

I don't know if you have an optional stop switch on your control panel, but M1 is the code for optional stop.

[CosmosK]

What does that do, one step at a time?

[Leo]

When you put a M1 in the program and you turn on the switch for optional stop - the program will stop at the location of the optional stop - and stay stopped until you press the cycle start. It could be used for a variety of reasons - maybe to clear chips away before proceeding.

[CosmosK]

Cool, can you program an M1 from VCarve? I'm trying to pause without having to edit the g-code manually (and remember to) when it's all done.

[Leo]

I don't know how to put it in using V-Carve. I have so many years of manual G-coding that I could edit the program if I needed to very easily.

The may be a way to edit the post processor but to enter it in a location to give a satisfactory output may be a challenge. It would be a trial and error basis.

First though would to be sure there is a way on your control to turn it on and off.

[martin54]

What is it you are trying to achieve? If you could give a bit more detail about why you need this or what you hope to achieve then I am sure one of the experts on the forum would be able to give you an answer. It's easy for someone like Leo with years of experience reading & writing G code to look through the code & make the changes he wants, unfortunately it's not so easy for some of us.

[rscrawford]

I'm not sure the M1 command will pause with WinCNC. Unless you write a macro that uses the G4 command (and you'd be better off just using the G4)

Is there a particular spot you'd like the pause, like a tool change? If so, you can add it to your post processor at the end of the tool change.

It it is random spots, then I don't think there is a way to add it unless you go in and edit the g-code. Might be easier to just split into two separate cuts so you aren't searching through lines of G-code to find the spot you want to add a G4 every time you generate a .tap file.

[Leo]

M1 is an optional program stop

G4 is a dwell command generally associated with a time.

It is not a program stop.

G4 could be used for example, when you want to dwell for a few seconds to let the spindle come to speed before starting the cutting.

M1 would stop the program to allow the operator to do something in the machine - then press cycle start again to restart the program.

I would not use a G4 - particularly if my fingers were going to be anywhere near the sharp cutter. Depending on the "time" associated with the G4 the spindle and machine could start without warning.

I have been programming for 30 years as a CNC programmer, and have used G4 and M1 more times than I care to count.

I don't know what the OP is trying to achieve, but to me it sounds like the OP wants to stop the program to do something.

http://www.cnccookbook.com/CCCNCGCodeRef.html ---- this is a list of G and M codes

[CosmosK]

Yes, just trying to insert a pause in a random spot. In a program, this ends up something I do a lot. An example is when I need to bolt something down before the next cut, but using the same tool. I'm doing it manually through G-code, but every time I go back into Vcarve to tweak a toolpath, then resave the .tap, the manual edits are gone.

Right now I manaully enter:

(text to display)
G4

This works great. Many times, I bail out of the program and reset my Z zero, the restart from last position. It would be cool if there was a way to insert this type of thing from Vcarve. Pocket, Profile.. Pause

I'll have to dig into to post processor and see if I can try something there. Maybe if it sees a particular tool # I can have it dub in the pause comands.. I'v done a little with the PP, but not much.

I suppose another way is just break up the program into multiple segments, but it's nice just having one. Thanks

[rscrawford]

Leo, M commands are more specific to the control software you are using. In WinCNC, there is no M1 command. You can program 'M1' to be whatever you want, but if you just insert an M1 into the file it WILL NOT stop the program unless you have previously set it up to do that.

In WinCNC, the G4 command on its own will pause until you hit 'ENTER'.

You can specify a time, for example G4X2, which will pause for 2 seconds.

Unfortunately Gcode and the M commands are not always the same in different control software. Its too bad - it should be universal, but its not.

[Leo]

In the years I have been programming on a multitude of machines the g-codes are pretty much universal. G0 through G4 particularly.

Yes, M-codes are somewhat machine specific, but M0, M1, M3, M4, M5, M8, M9 are pretty universal.

I have programmed machines that use unique coding, but those machines are very unique and don't use G and M codes at all.

I looked in the WinCNC at the G-code and M-code list.

It is unfortunate that WinCNC does not follow convention and include the basic M-codes of which M1 - optional stop is a member of. Mach3 has it and it is a very useful code.

However the WinCNC manual does warn about the use of G4 to change parts, which is very similar to my warning.

I have never used WinCNC, but I can understand why many users will convert to something that follows CNC convention.

************************************************************
From the WinCNC manual

WinCNC Controller
WinCNC Users Guide Page 93

G4 Dwell - G4 X#

Stops movement for the time specified by the X value in seconds. There is no limit to delay time. If no time is specified, then the machine will be stopped until the operator pushes ENTER. Place a comment after the dwell to prompt the operator. Example: G4 [Ready To Start Section 2]

WARNING: Never use Dwell to stop the machine while changing parts!

Instead program a single part and use the TAB key at the Program prompt. This will repeat the last part cut.

[CosmosK]

Yup, I always hit escape and jog the machine out of the way. but, then I can restart from that point. Thanks for the info!

[CosmosK]

Well I did some looking around. I hadn't looked into Mach 3, but I know Camaster used to use it. I don't see myself switching to it although I do appreciate it follows convention more than WinCNC.

I think at the end of this I'm realizing I should split up my program at the pauses instead of trying to insert something that's probably a bad habit.

I appreciate the discussion, thanks!

[bravesoul]

Just a thought, break it up into separate toolpaths but using the same bit, then save each file separately. You can then create a single file and use a gosub to call each cut file with a Pause in between the files. I know this can be done with shopbot's but not sure about others. Leo, can this be done with basic gcode??

Just a thought.

Joe