Just had a program generate the following G-code segment. I can't tell if the code is bad or if Mach3 (latest) is misinterpreting it.
1) The code is producing two small circles where arcs are supposed to be. I have the circle code set to incremental. It is getting all of the other arcs right.
2) This particular segment is supposed to spiral down five loops. Without actually cutting a piece, I can't tell if it is doing it. I don't see it on the tool path window when I change the perspective
3) The G03 code lines 331,345,359,etc. only reset the speed and it looks as though it should also set the new depth. Is this proper usable code? Every 5 passes the code does set a new depth.

What is the solution to this?

Thanks.
Bill

Sorry wrong picture.

It is a bad Gcode...
  The lines flanking the problem circles are drawn without "fillets" or they are just intersecting with a IJ move in between them.
also at line 329 although there is an arc, the lines surrounding this arc are out of position for the arc (it seems to me).

What program are you using to draw/generate this code?

I haven't investigated the spiral down yet.

Bloy,
Item 3) has been resolved by by changing a parameter that I though was unrelated. There is a parameter that is used to link chains together. It is apparently is also used when generating tool offsets. I had it set very large and it was closing up the arcs with lines and then cramming in the arc

I am using BOBCAD, probably a bad investment, since it is not going to be much faster at generating code.

I now have Z values where they belong but now the Mach 3 does not like the codes it's generating for a G83 peck drill. If I peck a single hole before cutting the part outline, the first arc of the part outline chokes with a "Radius to end of arc differs from radius to start on line. .(N14).  (No peck no error)
N  1 G90
N  2 G80
N  3 G40
N  4 G49
N  5 G91.1
N  6 G0 X0.0000  Y0.0000
N  7 M6 T1
N  8G83 Z-.5 R0 F15 I.01 P.1
N  9 X2.8230 Y0.5195
N 10G80
N 11 Z0.1000
N 12 X0.6000 Y1.1625
N 13 G01 Z-0.0100F15
N 14 G03 X0.0375 Y0.6000 I0.0000 J-0.5625F45
N 15 X0.6000 Y0.0375 I0.5625 J0.0000
N 16 G01 X4.1000
N 17 G03 X4.1442 Y0.0558 I0.0000 J0.0625

Thanks.

Bill

I have BobCadCam. It is used so infrequently by me that I am always in the learning mode, but it does what I need.  Whatever the drawing, I just keep re-generating the code and back checking to see what causes what to happen.  To see how your drawing turns into Gcode, I would need to have the drawing file as well.  I remember making a drill cycle with a dozen holes and a multi-cycle profile for the same part(similar in ways to yours), but I had separate files that I just ran after changing tools. Probably, they could have been combined into one file but impatience made me pass on that and just ran them separately.

tool path and selection order always seemed important.

Bloy,
I now know what the problem is. The code generator is forgetting to add a G00 to line 11 and Mach does not know what to do with data that follows the G80.

Now to fix the code generator.

One problem that Bob Cad has is that it is click intensive. There are a few flexibilities that should never exist that are constantly in the way. The big one I notice is being able to reverse a single element in a chain. Another is that it forgets settings on some functions that tend to be repeat items.   

Thanks.

Bill

This tool might help clean up all your errant element directions..

Bloy,
I use that function. It works pretty fair at solving chaining problems. Trouble is that it is too easy to screw it up again. Once a chain is formed, the direction of all of the segments should be locked together, changing one should change them all by default.
 
I tried to make a gear (using the gear function) and then convert it to a surface to extrude it into a solid and it wouldn't do it. I'm not sure what I did wrong or if it can be done. I had a devil of time trying to close the chain, because the segments are all very small, and I could not easily organize them. "Reorganize" helped with it, but every time I tried to select the gear, I would wind up reversing a segment or two, which broke the chain again.

I will get used to the program someday.  I have the 10 CD training series and that helps, providing I can find what I am looking for.

I now have a patch for the G83 function, and that seems to work for me for the problem below.

Thanks.

Bill

here's a link to some videos that BobCadCam's Sorin has put out free. He really makes things look easy.  Maybe you have already seen this.
http://cadcamtrainer.com/forums/showthread.php?p=2439#post2439


I'm also assuming that you have the Mach3mill post processor offered at BobCam's main sight.  In support