Reference Section > Touchcut G Code Reference > Notes on Using G-Codes:

All settings for drilling are stored on the machine in a tooling database- no feed or speed informations needs to be included in the program

Select a spindle type tool: eg T1(DI30) selects the spindle and loads the settings for a "DI30" drill, which might be a 30mm diameter insert drill. If the machine has an automatic toolchanger then it will automatically locate the "DI30" tool in its magazine and load it into the spindle, otherwise the operator will be prompted to manually load the "DI30" drill.

A series of rapid G0 and Tool-On M30 instructions. M30 is all that is required to activate a through-plate drill cycle (rapid down to initial height, feed down, rapid up). No M3 (tool off) code is required.

To drill to a given depth, add a depth specifier to the tool on command. For example M30D10 will drill a hole 10mm deep on a metric machine, while M30D1 will drill a hole 1" deep on a machine running inches. Depth is specified to the deepest part of the hole, ie the tip of the drill. If the specifier is zero, M30D0, or not present at all, M30, then the machine will drill through the plate, adding an overshoot as specified in the on-machine drill library.

Boring and Tapping work the same as drilling; TouchCut6 identifies tapping or boring tools by switches in its tooling library. For example to drill and tap an M12 hole, and counter-bore it 10mm deep and 22mm in diameter we might have:

T1(DI10)

M30

T1(M12)

M30

T1(BORE22)

M30D10