Help programming a Boss 5 Loop

I've been reading the programming manual but I'm lost on this one. Say I have 2 vises on my machine 10" on center and I've got stock in each that I want to run a program like the following on. I want to loop the program with a 10" step in the X over to the second vise so I can cut that part. Assume I've got X0Y0 centered over the first part. I figure I need a G91 line with an incremental X for the 10" move but I don't want it to move before it does the first piece. Here's my base code:

%N5G0G90X0Y0T1M6
N6G00X0 . 0Y3 . 0
N10G00Z-0 . 980
=N30/10
N11G01G91Z-0 . 020F200
N15G03G90X-3 . 0Y0 . 0I0 . 0J3 . 0F320
N20G03X0 . 0Y-3 . 0I3 . 0J0 . 0
N25G03X3 . 0Y0 . 0I0 . 0J3 . 0
N30G03X0 . 0Y3 . 0I3 . 0J0 . 0
N50G0G90X0Y0M2
E


And what I think I need to do:

%N5G0G90X0Y0T1M6
=N40/1
N6G00X0 . 0Y3 . 0
N10G00Z-0 . 980
=N30/10
N11G01G91Z-0 . 020F200
N15G03G90X-3 . 0Y0 . 0I0 . 0J3 . 0F320
N20G03X0 . 0Y-3 . 0I3 . 0J0 . 0
N25G03X3 . 0Y0 . 0I0 . 0J3 . 0
N30G03X0 . 0Y3 . 0I3 . 0J0 . 0
N40G0G91X10 . 0
N50G0G90X0Y0M2
E


This would be a nested loop of course with the circle loop in there. Do I have this correct or am I off somehow. I believe it will follow the loop for N30 to completion then set over incremental 10" for N40 and repeat the N30 loop finally skipping N40 and going to N50 to stop the program and return to X0Y0.

If this works it will make a bunch of parts easier to make since I'll have less stock changes. In one case I cut 2" disks out of 0.0250" steel plate and I'd like to loop 8-10 times rather than move the stock manually after each disk. I unsure in this case whether the line =N40/1 should actually be =N40/0 so it skips N40 on the second part.

The machine in a Bridgeport Boss 5 CNC and has to do circles in quadrants. Also isn't there a way to turn off the decel between quadrants? Max feedrate is 38 IPM (380) and I'd love for it not to slow down at the end of each quadrant.

The Boss 5 will do 360 degrees with one line

You have to call G75 first

I and J are different than single-quadrant mode - I've forgotten the specifics, but the BP programming manual is very good. I think that I and J are the absolute coordinates of the arc center when in G75 mode.

Why not have this logic in a loop sequence:

manually set X0 on l.h. vise

Start loop
machine l.h. vise using a subroutine
go to X0
G92X-10. sets X0 on r.h. vise
call the same machining subroutine - does the r.h. vise
go to X0
G92X10. sets X0 on l.h. vise
End loop

loop as many times as you want for continuous running

The major disadvantage is that if you pop a tool or have to stop while machining the r.h. vise, you have to manually reset X0. Not a big deal.

Thanks, got it figured out with help from another forum. Just like you suggested, put the program in a macro and call it up after positioning and G92. Actually I was guessing on the vises, they are 11" on center apart. Here's the new code, cuts air just fine! This is for a different part, the circle above was just an example.

%N10G0G90X0 . 0Y0 . 0T1M6F100
#1
N20G00X0 . 0Y0 . 0S2000
N30G00X-3 . 400Y-2 . 000
N40G00Z-3 . 1
N50G01Y2 . 000F40
N60G00X3 . 400
N70G01Y-2 . 000
N80G00X-3 . 380
N90G01Y2 . 000F150
N100G00X3 . 380
N110G01Y-2 . 000
N120G00Z-1 . 950
N130G00X1 . 750Y0 . 010
.N140G83Z-1 . 100Z0 . 050F20
N150X1 . 750Y-0 . 010
N160X-1 . 750Y-0 . 010
N170G00Z-1 . 950
N180G00X2 . 2Y-1 . 0
N190G01Z-2 . 050F40
N200G77X-4 . 4Y1 . 75Y0 . 250F320
N210G00Z-2 . 0
N220G00X2 . 250Y-1 . 250
N225G01Z-2 . 050
N230G01X2 . 250Y0 . 800
N240G01X-2 . 250Y0 . 800
N250G01X-2 . 250Y-1 . 250
N260G00Z-1 . 9500
N270G00X0 . 0Y0 . 0
$
N400G90X0 . 0Y0 . 0
=#1
N410G90X-11 . 0
N420G92X0 . 0Y0 . 0
=#1
N430G0X11 . 0
N440G92X0 . 0Y0 . 0
N450M2
E