Re: CNC PRO

> From: Jon Anderson <janders@...>
>
> > Tim Goldstein wrote:
>
> > If I remember correctly, Jon Elson or Matt Shaver was telling
> > me there is a g-code that you can use to run the same program
> > repeated a number of times for the same purpose.
>
> M99 will cause a loop back to start. I use this all the time, at the end
> of the program using a pause or tool change, then looping back to start
> . In production, it's faster than having to restart the program.

The EMC software doesn't implement this feature.

> However, I wasn't aware of any ability to use this to loop a finite
> number of times.
> This however, isn't the same thing. When using subroutines as I
> mentioned, the part geometry is generally programmed in incremental
> mode. I only have to lay out a single part and program in incremental.
> This becomes the subroutine. The main program moves to the starting
> point for the first part, and calls the subroutine, which then goes into
> incremental, machines the part, switches back to absolute, then returns
> to the main program which in turn moves to the starting point of the
> next part. Sometimes I will use G92's instead. I can follow absolute
> code, mentally tracing the toolpath, but I find it harder to do this
> with incremental code.

Then you'll like how it's done with the EMC! We have 8 independent work
coordinate systems that you can call out in your program using G54 through
G59.2 and which can be offset from machine zero using the command:

G10L2P<p_value>X<x_value>Y<y_value>Z<z_value>

where <x_value>, <y_value>, <z_value> are the respective distances from
machine zero for each axis.

What you would do is go to the XYZ zero point on the first fixture and enter
the G10 command in MDI mode to set the offset for the G54 coordinate system.
Something like:

G10L2P1X.3254Y-1.2847Z-2.9385

Repeat this for up to eight fixtures on your machine table. Note that there
doesn't need to be a particular distance between the fixtures known when you
write the program. You can then write the code to make your part in absolute
coordinates. Your program would look like:

G54 (first fixture)
<part program>
G55 (second fixture)
<part program>
G56 (third fixture)
<part program>

etc...

Offset Command P Value for G10

Machine G53 Can't be offset
1 G54 1
2 G55 2
3 G56 3
4 G57 4
5 G58 5
6 G59 6
7 G59.1 7
8 G59.2 8

The G54 offset is the default offset which is in effect when the machine is
powered up. G54 through G59.2 are modal, which means that once invoked they
stay in effect until another offset is commanded. G53 is non-modal and refers
to the machine coordinate system.

> I sort of straddle the lines here. I'm self
> employed and can't afford a full size CNC mill, so I do what I can with
> my MAXNC, always looking to get the biggest bang for my buck, but I
> really like the DIY approach. I need more power than a strict hobbyist
> and jumping through too many hoops starts to diminish the already
> marginal usefullness of the MAXNC in a commercial application. Heck, for
> all I've invested in this thing, time and labor, I probably could have
> put half down on a nice new CNC knee mill. However, I've got more time
> than money....

I have profound empathy with your circumstances. You are not alone!

Matt Shaver