Material zero reference after power outage

[MS76]

For those of you that have installed a UPS backup on your tables computer, how do you record your starting point or material reference if you need to restart a cut after an electric outage?

[robertspark]

Home your machine before you start.

Record your machine co-ordinates at the start of a cut operation to a log file.
(depending upon what cnc software you are running you could create a macro to log the machine co-ordinates when the macro is called). So if using sheetcam, just insert a macro as part of the post processor to be called at the start of the job "OnInit()" or "Operation".

You can then use G53 to jog to the machine co-ordinates location once the machine is rehomed and start from that location. (this could be automated from a macro to reopen the log file and call the last co-ordinates via a button on screen)

[robertspark]

Its probably a bit more helpful if you list / explain your setup (i.e. Mach3 / Linuxcnc / uccnc / sheetcam / fusion360 etc etc) as someone may have what you want in macros to automate the process for you

[MS76]

Thanks for the responses. I have written down my coordinates at the start but am not in the habit of it. I am running sheetcam, command cnc linux on an arclight dynamics table. I frequently use inkscape on my drawings

[MS76]

I'll have to look into that on sheetcam roberspark, that sounds interesting.

[robertspark]

I can help with sheetcam (that's easy)...
I have not written macros under linuxcnc so cannot help there (I keep trying to dabble with linuxcnc with a Mesa + thcad card but I've got too many other projects that are work in progress.... plus if you have a working setup that you are happy with why change....)

[Rodw]

On Linuxcnc, you could log every probe event very simply with comments at the beginning and end of every job. You might be able to use the file gcode name as the basis of the log file within the sheetcam post.
(LOGOPEN,probe-results.ngc)
; cut here
(LOGCLOSE)


See http://linuxcnc.org/docs/html/gcode/g-c ... #gcode:g38
and an example file mentioned above:
https://github.com/LinuxCNC/linuxcnc/bl ... tprobe.ngc

[robertspark]

Rod,

its not after probing that the OP wants to log the current machine co-ordinates, however, thanks very much for the info as I think I may have the right direction below.

it looks like you could do the following:

Code: Select all

G30.1 (stores the current absolute position into parameters 5181-5186)
(LOGAPPEND,startcoordinates.txt)
(----)
G53 G0 X#5181
G53 G0 Y#5182
G53 G0 Z#5183
(LOGCLOSE)

I would suggest placing the above code in an *.ngc file and running it and seeing if it saves your current machine co-ordinates for you. where I placed the (---) this will act as a marker so that you know that the last co-ordinates will be at the end of the file. I added the G53 G0xxxx so that cou could just copy and paste them into the MDI and the machine will move to those co-ordinates. It should not move the machine when the co-ordinates are logged, given the machine won't move anywhere given that is where it is located as the G30.1 is given just before the (LOGAPPEND)

The LOGAPPEND was used so that you have one file with all the info added to it so the last info is the most current (i.e. if you have a power outage that is the place to go to for a restart).

[Rodw]

@Robert, My thinking was if you logged the probing event, you would get a log of the coordinates on every pierce. But yes the logappend is also a good solution

[MS76]

Thank you both for your responses! So many members on here amaze me with their knowledge and willingness to help those of us that have so much to learn. As it would have it by coincidence, I've had a 7 hour power outage today although I wasn't running my table only my powder coat oven at the time.

[robertspark]

maybe the probe event is better on second thoughts it will just log every pierce point


I guess it's some options to play with

where on the planet are you ?

[MS76]

I'm from north east Ohio robertspark

[beefy]

.

[Thor]

If you have Command CNC you dont need to write it down. I home my machine and then use fixture offsets to auto locate the corner of a sheet off some machined blocks that fit my table sides. I use G55 for cold rolled sheets and G56 for hot roll (I think its like .075" farther inward then G55 is).

Even if you dont use fixture offsets Command Cnc remembers where you zeroed last, given that your machine has homing switches.

Thats one thing they did great on Command Cnc is its tracking of machine zero and work zero (G54) and the use of Fixture offsets. If I have to modify a part I move to a good spot on a sheet of steel pushed into the corner of the table, then cut an outline that the part fits into. And record that same Zero posistion into a new Fixture offset, and make sure the program calls it up in the beginning before any movement. Then I can still come back to it months later, provided I keep track of which Fixture offset I was using and dont need it for something else (In which case a quick camera pic of the offset page and throw the pic in the appropriate file. Much the same as I do on my CNC turning and machining centers. If I know its going to be a long term job I'll write the fixture offset numbers into some human readable notes at the beginning of the program along with any other setup info needed.

[beefy]

.

[Rodw]

If my PC and my smartphone with the photo die at the same time, then I guess I'm just doomed.

Keith.

Nah, if you use Google Android your photo will be backed up to the cloud in Google photos before it dies.

[beefy]

Hey Rod,

what I meant though, was that I wouldn't go buying a lottery ticket.