I am having problem with my program. It was mad in Bob-cad and it runs fine there. When I get it to the mill it is not doing what it shoud be. I have no manual for the G-code part for mill. I am fumbling thru the offset and tool offset sceens but I feel that is not my problem. I think it is with the G02 and the G03. Here is the beginning of my program where I am having problems...
N2%
N4G00
N6G90
N8G70
N10M25
N12T01 M06 D01$(None)
N14M25
N16S3500 M3
N18 Z0.1
N20 X0.75 Y0.75 Z0.1
N22 G01 Z-0.25F3.
N24G41
N26 Y0.5 Z-0.25F30.
N28 G03 X1. Y0.25 Z-0.25 I0.25 J0.
N30 G01 X5.5 Z-0.25
N32 G02 X6.25 Y-0.5 Z-0.25 I0. J-0.75
N34 G01 Y-1.3964 Z-0.25
N36 G02 X6.1036 Y-1.75 Z-0.25 I-0.5 J0.
N38 G01 X6.0732 Y-1.7803 Z-0.25
N40 G03 X6. Y-1.9571 Z-0.25 I0.1768 J-0.1768
N42 G01 Y-3.5429 Z-0.25
N44 G03 X6.0732 Y-3.7197 Z-0.25 I0.25 J0.
N46 G01 X6.1036 Y-3.75 Z-0.25
N48 G02 X6.25 Y-4.1036 Z-0.25 I-0.3536 J-0.3536
N50 G01 Y-5.85 Z-0.25
N52 G02 X5.5 Y-6.6 Z-0.25 I-0.75 J0.
N54 G01 X0.5 Z-0.25
N56 G02 X-0.25 Y-5.85 Z-0.25 I0. J0.75
N58 G01 Y-4.1036 Z-0.25
N60 G02 X-0.1036 Y-3.75 Z-0.25 I0.5 J0.
N62 G01 X-0.0732 Y-3.7197 Z-0.25
N64 G03 X0. Y-3.5429 Z-0.25 I-0.1768 J0.1768
N66 G01 Y-1.9571 Z-0.25
N68 G03 X-0.0732 Y-1.7803 Z-0.25 I-0.25 J0.
N70 G01 X-0.1036 Y-1.75 Z-0.25
N72 G02 X-0.25 Y-1.3964 Z-0.25 I0.3536 J0.3536
N74 G01 Y-0.5 Z-0.25
N76 G02 X0.5 Y0.25 Z-0.25 I0.75 J0.
N78 G01 X1. Z-0.25
N80 G03 X1.25 Y0.5 Z-0.25 I0. J0.25
N82G40
N84 G01 Y0.75 Z-0.25
N86 G00 Z0.1
N88 X0.75 Z0.1

N12T01 M06 D01$(None)

W I remove this line it runs ok, I think!
This line calls for tool one and what else I can't make out?? ???

When you removed that line it ran ok on your mill?

Also it runs with that line bob cad.

Not being a programmer I don't know what it does but without that lime Mach 3 will cut a strangely shaped parallelogram all in one pass.

Does it do funny z travel in mach 3

It plunges to 1/4" deep and stays there till the pattern is cut then returns to 1" above zero and quits!

thanks, let you know how it turns out.

Ok so I took that line out and at machine all it does is spindle retract and thats it. Any help would be great.

What software are you using to run your machine?

Hyper terminal on pc

Proprietary software? Their machine, their software, their controller?

I don't know...............
Good luck!

Try removing just the D01$(None) from line 12. The T01 is telling you tool1 and the Mo6 means tool change. As far as a book for programing in G code for the KMB!, I don't think there is one.

If you post a dxf drawing of your part I'll post a sheetcam/Mach3 version of the g code for you to try.

Have you run other parts on this machine? Give us some background so we aren't just bumping blindly into walls.

When I generate geometry from your code in my Bobcad v17 it makes a mess.

This code should make a 6x6.35 rect. w/.5 radi. corners at .25 deep it should ramp in at x.75 y.75 I am running bobcad v21. it runs fine in there.

Since there's been no activity on this thread for several days it may be too late to help, but....
1) As already suggested, remove all or part of line "N12" if you dont have a tool changer. The "M06" does really bad things to at least one of my controllers that doesn't have a tool changer.
2) Make sure your machine understands M25 (line "N10" and "N14", spindle retract). You may want to leave it out in order to keep things simple until you get the bugs out.
3) Make sure your tool offset tables or lists have a valid value for tool "1" because line "N24" is calling for G41 which is left cutter comp.
4) Now this is very important for some controllers, if your machine does not do helical interpolation you may not be able to have "X","Y","Z", and "I","J","K" or "R" on the same line, or this may be the wrong format for your helical interpolation. In your sample program you don't need it either way.

Just to make things simple: Remove from line "N12", the "M06 D01$(none)". The "T01" part may be ok. Remove lines N10 and N14 if you're not sure about M25 (make sure clamps aren't in the way because the cutter will only be .100 inches above the part when it's done running.) Go thru line by line and remove the "Z-0.25" from any line that has an "I" and / or "J" value, like lines "N28", "N32", "N36", etc., down to "N80". If you're not sure about your tool offsets for the cutter comp called out in "N24", change the G41 to G40 which will turn the cutter comp off for now. And last (but maybe least), after everything else is fixed, add line "N90 M5" to the end of the program to turn the spindle off.
I too have BobCadCam. I have versions 19, 20, 21, 22, 2007 and it's terrible at creating posts for my machines with a Fagor 8040 controller and even worse for my Hurco VM2! Beware of Crop Circles (otherwise known as crap circles). Everything look nice on the BobCad simulation screen and on the Predator simulator but then it tries to cut BIG circles in your part, thru your vise, thru your clamps, etc. If you're lucky you'll just get an axis over-run or limit error.
With the mods I suggested, your program runs on both my VM2 and my Fagor controllers. I did let the machine make the moves with the spindle running and the tool cutting air. The part is a 6x6 square (approx) with recesses on two opposite sides and a radiused(sp?) lead in and out near one corner....
Good luck.

Thanks for your help, still trying to work at it.

Hi mmachining.

ran your programme through my backplotter and it would not run when set up for hurco. but when i changed to fanuc configuration it did. which suggests to me that you are using incremental circle centres and as far as i remember th kmb1 uses absolute co-ordinate centres. if this is the case tere must be a setting in bobcad to set the type of circle centre output.

Regards Stu.