[md63825]

BurrMan,

Did your toolpaths look anything like the toolpath pics I have attached when you ran my program?

[dwood]

in your post see what lines 204 & 205 are

[md63825]

Both are "n" currently. I have changed them both to "y" and then 204 to "n" and 205 "y" and then 204 "y" and 205 "n". I have added "z_f" to line 64, "x_f" to line 65, "y_f" to line 66, changed line 203 to "n". Nothing seems to be working. I have even tried other post processors from other machines and get the same exact thing. I think my BobCAD software is screwed up. I have even had others run the program that BobCAD created and it has these crazy sweeping arcs that it shouldn't. And of course BobCAD won't help until I pay their service support fee. Think I will uninstall and reinstall the software and see if that works.

[dwood]

maybe burr will hit on something
i ran your file as it uploaded your tools etc in preditor, part looked ok
only i thing changed was the post to my haas
set 203,204,205 to yes and try
can you turn off g18&g19 in your control ?
i will try on a machine if i get time

[BurrMan]

I wasnt backplotting the part.. I was just paying attention to your requirement to have the G18 output on that line and why it doesnt on those line...

The 2 different lines are a feed move and an arc move.. The feed move with the G01 outputs the G18 but the arc move and the G02 dont...

I couldnt get it to output a G02 G18 as you want, and dont know enough about it to make it happen or tell you it cant.

The backplot circles are the post issue that dwood is refering too. Although, you are mentioning that it is the lack of a G18 on your arc output moves, so I think that is your answer.

The only way I can get the subsequent G18's that you want to output is to hardcode the G18 into Line 66.

But I dont know enough about it to know the longterm affects of this along with other ops, with your controller.. Seems that if your controller needs it there, then putting it there "ALWAYS" wont be a bad thing. The only other thing with that, is you then get the first line with 2. But you could also put a NUL value as the identifier for the G18 and just have the hardcode output it always....

[BurrMan]

BurrMan,

Did your toolpaths look anything like the toolpath pics I have attached when you ran my program?

And just to answer this, I can post it out with my post processor and backplot it ok.



For the backplot, it will be a combination of the post output along with the machine/reverse post used to do the backplot.

I dont know enough about this type of code to help set something up for you that works. A request to the BobCad post creation may be in order:

Post Request | BobCAD-CAM

Along with some discussion about what RP you are using.

[BurrMan]

I just ran the code from your post processor and used a different program to backplot the output.. The only odd arcs I got were on those slice planar parts with a vertical loop.... Let me look at that a little closer.

[BurrMan]

So I removed the "arc fit" check from those slice planar toolpaths, and they then backplot ok:



Lets take a look at that vaue being used with this output.

[BurrMan]

Ok, so I can change the arc fit value to something other than .0005, like .0004 and get a good backplot, or I can change my machining tolerance, under current settings, from .0005 to .0001 and it will backplot those planar toolpaths ok...

Please try either of these.
(I have no selected as break arcs at quads or <180.)

[md63825]

BobCAD finally responded to my request and provided me the following:

They modified the post processor line 64,65 and 66 as follows:
64. Arc move XY.
n,program_block_1,g_arc_move,x_f,y_f,arc_center,fe ed_rate
65. Arc move YZ.
n,program_block_1,g_arc_plane,g_arc_move,y_f,z_f,a rc_center,feed_rate
66. Arc move XZ.
n,program_block_1,g_arc_move,x_f,z_f,arc_center,fe ed_rate

And they modified line 222 to "b" which b=incremental

Seems to be running correctly now but I also noticed changes in the behavior of the posted program when I monkeyed with the arc fit value. Never got around to changing the machining tolerance. Where is the setting for changing the machining tolerances? Just in case I need to make some more adjustments.

[BurrMan]

CAM-Part-milling tools-current settings-Machine parameters.