[jimmyjames1981]

Hi guys, as all of you know helix bores in mastercam generate a crapload of lines of code, ive been making some aluminum parts 1 piece at a time in the vice and now im building a fixture to hold 28 parts, 2 counterbored flat bottomed holes in each part, 1st operation is ith a 3/8" 2 flute going .875" deep on a .52" diameter hole, next operation for the counterbore is with a 1/2" 2 flute 90 degree drill point drill mill at a depth of .25" to the shoulder with the step on the bore being 45 degrees, hence the reason for using the drill mill. My problem is, the program is way to big, how do i can the helix bore cycles in mastercam so it only has 2 different sets of helix bore code rather than 112 seperate helix bore codes. machine is a haas vf4.

[jimmyjames1981]

thinking of just using a contour, depth cut(not 2d ramp) plunging at 30-40ipm with a 40ipm feed .125 depth cuts and finish pass at bottom at 30% speed and feed and lead out to center of bore. thoughts? If i used 2d ramp the program would still be way too big.

[Superman]

curious, is your NC code point to point ( small lines ), or arcs with a Z move ?
or are you surfacing ?


Couple of ways to do it
1-.......bit of manual editing....runs a risk of programmer error..... program each helix bore at X0. Y0 in INCREMENTAL and change it to be a sub-program....ends with M99
Then have the main program go-to the bore centre then call-up the correct sub.

2- let Mastercam do it.....say 10 holes....run it.....next 10 holes.........probably faster, & less chance of fat finger errors

[fizzissist]

This is where subroutines shine. Write the tool paths in a single subroutine, and the main program indexes the part location. If you have macro on your control you could use that to index the part. Writing macros is more complex (more fun too, IMHO), but either way, editing a single subroutine is far safer than wading through 28 iterations and risking missing one single ... whoops.