There are three basic plane selection commands:
G17 – XY plane selection
G18 – XZ plane selection
G19 – YZ plane selection
When you first power up a Fanuc-controlled CNC machining center, G17 is automatically selected, meaning the machine will be in XY plane selection mode unless you select a different plane by commanding G18 or G19.
There are several CNC functions that are affected by your plane selection choice. But frankly speaking, almost everything commonly done on a machining center requires the selection of the XY plane, so there aren’t many times when you’re required to switch planes. But let’s discuss a few of the times when plane selection is necessary.
As you know, G02 and G03 are used to specify clockwise and counter-clockwise circular motions. When milling in the XY plane, as is commonly required, it is the X and Y axes that are moving during the circular motion. And by the way, we evaluate the direction (cw or ccw) by looking at the motion from the plus side of the uninvolved (Z) axis.
Again, most circular motions require the X and Y axes to be moving to form the motion. But consider placing an end mill in a right angle head, maybe one that points the tool in the X minus direction (tool facing to the left on a vertical machining center). In this case, a circular motion will require a YZ motion and prior to making such a motion, the YZ plane (G18) must be selected. If the right angle head points the tool along the Y axis, the tool will be machining in the XZ plane, and G19 must be commanded prior to this motion.
Another time plane selection must be considered with circular motions is when using a ball end mill. It’s possible that a circular motion with a ball end mill will be in the XZ or YZ plane, and the appropriate plane selection G code must be commanded prior or within the circular motion command.
Most holes are machined in the Z axis with CNC machining centers. That is, the hole centerline coordinates are specified with positions along the X and Y axes. But again, consider placing a hole machining tool (drill, tap, reamer, etc.) in a right angle head that is pointing the tool in the X minus direction. This tool will have the ability to machine holes along the X axis – and believe it or not – using the appropriate plane selection command (G18 for YZ plane selection in this case) will allow you to use canned cycles (G81, G82, G83, etc.) to machine the holes. This dramatically simplifies the task of programming.
When this is done, the canned cycle-related letter addresses will change in meaning. If YZ plane selection is chosen (drilling along X), The hole center will be specified with Y and Z. The rapid plane will still be specified with R. But the hole bottom position will be specified with X.
What about odd angles?
With G17, G18, and G19, the planes are, of course, ninety degrees apart, which is why these commands can be helpful with right angle heads on standard three-axis machining centers. But these commands won’t help with other planes – those that are not at right angles with the three axes of the machining center (X, Y, or Z).
There are, however, machines that have the ability to machine in any plane. Five axis machining centers can machine in planes other than just XY, XZ, and YZ. For this reason, most five axis machining centers come with a special feature called user-defined plane selection. With this feature, the programmer can define any plane – and still use circular interpolation, canned cycles, and other coordinate manipulation features (like rotation and mirror image) in any defined plane.