[japco43]

I am trying to program a series of hole that have a drill bit/countersink built in. I would like to have 2" of z height clearance. How do i make the spindle rapid down to about .200" and slowly drill to depth, and then rapid back up to 2." then move to the next hole?

[Brian L]

With G-code it is pretty simple, set your Z0 tool lengths at 2.0" above the part, then your drilling cycle would look like this:

G98 G81 X___ Y___ Z-3.0 R-1.8 F20.0
X____ Y_____
X____ Y_____
and so on until you complete your holes, then you will need a G80 line to cancel the canned cycle.

How any of this is done with the conversational side, I can't tell you, I never use it.

[sportybob]

Conversationally, in the drill set up, set the R plain to .200 then do a position move to Z +2.00

sportybob

[ZZZZ]

On the Enable Drill Cycle event, you have the option of Initial or Clearance on the Return Point line. Initial means the Z height when the cycle starts, Clearance means the programmed Return Plane in the Clearance line.

The way to use this is to do the Tool Change, then have a Position Event to move Z down to Z+2, then a Drill Start event with the Initial return point programmed. When you run the program, the machine will complete the TC, then rapid down to the +2 inches, then rapid down to the value in the R Plane, then feed down to depth, then rapid back to the Initial point, then move to the next hole, and do it again, etc.

In Brian's example, it's the G98 that tells the control to use the Initial Return Point, a G99 would tell it to return to the Clearance point ( R Plane) after drilling the hole.