[ToolChatter]

Hey folks,
I'm using BC for Solidworks V4. I'm trying to do a 2D profile with contour ramping. Everything simulates the way I want, but the Post (Centroid_M_Series_Rev1.MillPst) is doing something weird. For every arc where the toolpath is supposed to be ramping, it takes out the Z move and puts it into the next linear move. This results in extreme plunging and broken tools. I thought it was a bug so I contacted BC support, but they told me it is a problem with the way I have my Post set up, and since I'm not paying for support they won't help. I've looked at all the Post settings and don't see anything that suggests it would fix this problems. Anyone have any thoughts? (besides paying BC for support)

Thanks!
Tom

[LeWhite]

Allow circulr or helical interpolation. Or arc move XY (add Z here). Somewhere around paragraph 60. Use the search function in the word processor. Circular interpolation allow Z? Y/N
If you havent fixed it, I'll look tomorrow and check back

[ToolChatter]

Thanks! I'm not sure I follow exactly what you're saying. I opened the postprocessor in notepad and found "Arc move XY" on line 64. I changed it to "Arc move XYZ" (see picture) but that didn't seem to have any effect. I searched for "helical," "interpolation," "circular," and "allow," but none of those seem to be in there. What should I try next?
Attachment 277824
Thanks again!
Tom

[LeWhite]

As I remember paragraph 64 arc move XY is just the title (sets G17) dont put Z there, Try x_r y_r z_r. The other way is to put the post processor in debug mode something like 8. debug YN. When you put the pp in debug mode it will post your code and the pp paragraph that generated that line. So your code will read G03 Xn, Yn and no Zn, but right next to that line will be the pp paragraph that generated that line. That paragraph wont have a Z_ that is needed to do helical. I'll check back tomorrow cause I'm in bed.

[SBC Cycle]

You guys got the right line (Block 64). It's lacking a z_f which will output the Z feed move in the same line as the arc. There are quite a few posts on the BobCAD web site that are missing this critical function. Doesn't seem to me to be a user problem if the post was downloaded from the "Downloads" section of BobCAD.

I'm not familiar with your control so make sure this is the correct way to format a line for helical output. It is fine for both my Fadal and Haas controls.

[LeWhite]

As long as you are there mod pp paragraph 65.& 66 which sets G18 & G19. Make sure they all read X_f Y_f Z_f . This will allow Bob to do planer offset, radial and some others (allow arcs) when the lace angle isnt 0 90 180 or 270. Have fun!

[ToolChatter]

BOOM! That seems to have done it. Thanks for all the help! Looking forward to keeping my tools intact...