How can I continue g-code tomorrow ?

[FriendOfGhost]

Dear friends,

I want to stop (pause) mach3 while running and shutdown eveyything and tomorrow I want to continue where I stopped the system.

I wonder how do you do it. I get the last coordinates, last line of gcode that will be processed and "tomorrow" I try to continue.

but... "Radius to end of arc differs from radius to start on Line #" messages are making this operation impossible.

Can you suggest some way to do it ?

best regards...

[Hood]

Sounds to me your default  IJ mode may be different to what you have in the code. How are you restarting, if doing a Run From Here then I think it should change the IJ mode to what is in the code so it sounds like you are not doing that. Either MDI the correct IJ mode or change the default on General Config and see if that helps.
Hood

[FriendOfGhost]

Nope my friend,

IJ mode is correct. I tried that. also if I change IJ mode my gcode never runs and directly gives that error.

 gcode is running perfectly.Problem is after I pause gcode, press reset button, exit from mach3....
and...
re-run mach3, open my gcode, set old coordinates and run the gcode that error rises. I believe when  run gcode starting from the middle of it, arcs could not be completed...

never mind, real problem is:  how I stop gcode, shurdown everything  and continue tomorrow ?

[Hood]

How are you trying to restart the code?
Do you home to switches?
Can you attach your xml and code and also say which line you stop at?
Hood

[BR549]

The first problem is that the machine will loose its exact position when you shut it down. You will need to Rereference the machine to home on startup. That will place you back to a known position +/- the accuracy of your referencing switches.

The second option is to reference the machine to a KNOWN point on the material or table and then set the dros to those values. That will reference you BACK to the part. A edge reference in X and Y or a simple center of a hole will do.


THen the easy way toRESTART is to use RUN FROM HERE. There are some quirks to this as well but for the most part it works fine on simple Gcode. Just follow the prompts to restart. NOTE it will take you BACK to the line BEFORE the one you select. So check your tool/fixture clearances to allow a safe move to the start point.

The Run Next Line can work BUT you cannot restart in an arc or you will get that message(;-) at that point mach does NOT know where the last move was from so it cannot determine where the arc should end.

If you want to use Run next line you HAVE to make sure your MODES are set correct for where you are at in the Gcode. Then start from the beginning of a line not an arc.

Just some thoughts, (;-)TP

[FriendOfGhost]

The Run Next Line can work BUT you cannot restart in an arc or you will get that message(;-) at that point mach does NOT know where the last move was from so it cannot determine where the arc should end.

this is exactly my point my friend. So you say I cannot continue arcs tomorrow...
that means I need to pause mach3 EXACTLY after finising the arc.

Can you tell me please, if there's a way for stopping mach3 in some exact line ? like breakpoint ? like "stop at line number *********"

[BR549]

Easy Just restart at a point that is a line not an arc "previous" to the arc where you stopped. All modal values have to be set. G1/G0? Feedrate, SpindleSpeed,G20/21, G90/91.etc,etc.

Run from here works well and does all that for you based on the Gcode and gives you the option to restart the spindle.

NOW note: None of these options will work well with SUBs or macros or parametric Gcode as in most cases there are no Know values until the function actually runs and Variables are calculated.

Also with tool comp you MUST allow room on your restart for the machine to cycle the comp before it can restart or else you may crash the tool into the part or machine table.

(;-) TP

[agguilar]

Can some one here make a video tutorial this will help us all new members

[djc]

I want to stop (pause) mach3 while running and shutdown eveyything and tomorrow I want to continue where I stopped the system.

Do you know in advance where you want to stop or do you just stop "somewhere" when you run out of time or when the wife calls you home?

If you know in advance, put in an optional stop (M01). If you ever want t run the program through from start to finish, tell Mach to ignore optional stops.

In a way, G-code is like driving a car - it is not wise to just jam on the brakes in the middle lane of the motorway and jump out leaving the car where it stands. You have to indicate, slow down, pull over to the hard shoulder and park up nicely. Further, you stand a much higher chance of restarting in a graceful fashion if you follow the latter procedure.

[BR549]

COme on guys just try it in the air with no part or tools loaded. It is not rocket science.

Load a program  move to line inside the program and press run from here and then start and SEE what happens. Follow the prompt from the Message box that will appear. It tells you where you are at position wise and where it will go to get to the part position and gives you some restart options like start spindle.

It will not blow a fuse or cause warts to appear on your finger, just try it  (;-) TP