On Wed, Nov 07, 2012 at 04:47:01PM -0600, Daniel Rogge wrote: > > Trying to mill a 1" diameter hole with a 1/2" diameter endmill using G42 > radius offset compensation: > > % > G40 G49 G54 G80 G90 > G10 L1 P1 R.25 > T1 M6 > G43 H1 > M3 S750 > G0 X0 Y-.25 Z0 > G1 Z-.1 F10 > G41 X0 Y.5 D1 > G3 J-.5 > G40 G1 X0 Y0 > M5 > %
At the risk of making a pun, this is a corner case for the entry move. The CRC code tries to start at the given point, and over the entry move it applies the full offset, ending inside the concave corner made by the nominal entry move and the nominal subsequent move. By "inside the corner" I mean tangent to both. In the case you present, you don't really have that inside corner at all - or you just barely do, depending on how you look at it: See my picture of where the corner might barely be: [The preview is showing the NOMINAL path because I disabled G41/G40 with block delete so it would load. Otherwise it is your program.] http://timeguy.com/cradek-files/emc/barely-entry.png Now see what happens if I change your last G3 from J-.5 to J-.51, enlarging that corner just a bit, so the tool definitely fits. Reducing the tool diameter a tad would do the same thing. It does now run, but you don't cut a full circle like you surely want. [This is showing the compensated path now that it loads] http://timeguy.com/cradek-files/emc/entered-but-not-what-you-want.png If you must do your entry move inside what will eventually be the hole, I recommend using tangent arc entry like this: % G40 G49 G54 G80 G90 G10 L1 P1 R.25 T1 M6 G43 H1 M3 S750 G0 X0 Y-0.1 Z0 G1 Z-.1 F10 G41 G3 J0.3 X0 Y.5 D1 G3 J-.5 G40 G1 X0 Y0 M5 % Not only will you get your full circle cut, you'll also get much better finish at the Y+ edge of your hole if you enter tangentially. Ideally you'd exit with a tangent arc too, so you don't ever rub against the edge of the hole. http://timeguy.com/cradek-files/emc/nice-arc-entry.png The docs cover this a bit: http://linuxcnc.org/docs/html/gcode/tool_compensation.html#_overview As you can see from the example, even if you're cutting an outside profile, if you make a concave corner when you enter, you may not get your full profile cut. A tangent arc entry could be used here too, in the same way. Or, you could fix it by using a corner like in figure 4. You might also want to see the hole milling subroutine in useful-subroutines.ngc, which does CRC entry using a line above the workpiece (which is probably the most standard practice) and avoids making any concave corners at all. This makes it awfully foolproof. It is safest to do your entry move totally away from the work, so you are fully compensated before you come into contact with the workpiece. Also, it's best to move fully away from the work before you turn off compensation. The move immediately after turning off compensation can be surprising because the tool must get back onto the nominal path. Imagine you've cut an inside profile and then while still against the work, turn off CRC and program a Z-only move upward. The resulting move will slant "outward", so the endpoint is on the nominal path again, centered above the edge you just cut (which now has a little gouge in it). Chris ------------------------------------------------------------------------------ Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_nov _______________________________________________ Emc-developers mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-developers
