CNC Machine Overview

Any CNC machine has one or more Axes. Different types of CNC machines have different combinations. For instance, a 4-axis milling machine may have XYZA or XYZB axes. A lathe typically has XZ axes. A foam-cutting machine may have XYUV axes. In LinuxCNC, the case of a XYYZ gantry machine with two motors for one axis is better handled by kinematics rather than by a second linear axis.
[If the motion of mechanical components is not independent, as with hexapod machines, the RS274/NGC language and the canonical machining functions will still be usable, as long as the lower levels of control know how to control the actual mechanisms to produce the same relative motion of tool and workpiece as would be produced by independent axes. This is called kinematics.]

The X, Y, and Z axes produce linear motion in three mutually orthogonal directions.

The U, V, and W axes produce linear motion in three mutually orthogonal directions. Typically, X and U are parallel, Y and V are parallel, and Z and W are parallel.

The A, B and C axes produce angular motion (rotation). Typically, A rotates around a line parallel to X, B rotates around a line parallel to Y, and C rotates around a line parallel to Z.

A CNC machine typically has a spindle which holds one cutting tool, probe, or the material in the case of a lathe. The spindle may or may not be controlled by the CNC software.

If a CNC machine has components to provide mist coolant and/or flood coolant they can be controlled by G codes.

A CNC machine can have separate feed and speed override controls, which let the operator specify that the actual feed rate or spindle speed used in machining at some percentage of the programmed rate.

A CNC machine can have a block delete switch. See the Block Delete Section.

A CNC machine can have an optional program stop switch. See the Optional Program Stop Section.

The X, Y, and Z axes form a standard right-handed coordinate system of orthogonal linear axes. Positions of the three linear motion mechanisms are expressed using coordinates on these axes.

The U, V and W axes also form a standard right-handed coordinate system. X and U are parallel, Y and V are parallel, and Z and W are parallel (when A, B, and C are rotated to zero).

The rotational axes are measured in degrees as wrapped linear axes in which the direction of positive rotation is counterclockwise when viewed from the positive end of the corresponding X, Y, or Z-axis. By wrapped linear axis, we mean one on which the angular position increases without limit (goes towards plus infinity) as the axis turns counterclockwise and deceases without limit (goes towards minus infinity) as the axis turns clockwise. Wrapped linear axes are used regardless of whether or not there is a mechanical limit on rotation.

Clockwise or counterclockwise is from the point of view of the workpiece. If the workpiece is fastened to a turntable which turns on a rotational axis, a counterclockwise turn from the point of view of the workpiece is accomplished by turning the turntable in a direction that (for most common machine configurations) looks clockwise from the point of view of someone standing next to the machine.
[If the parallelism requirement is violated, the system builder will have to say how to distinguish clockwise from counterclockwise.]

The controlled point is the point whose position and rate of motion are controlled. When the tool length offset is zero (the default value), this is a point on the spindle axis (often called the gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool holder that fits into the spindle. The location of the controlled point can be moved out along the spindle axis by specifying some positive amount for the tool length offset. This amount is normally the length of the cutting tool in use, so that the controlled point is at the end of the cutting tool. On a lathe, tool length offsets can be specified for X and Z axes, and the controlled point is either at the tool tip or slightly outside it (where the perpendicular, axis-aligned lines touched by the front and side of the tool intersect).

To drive a tool along a specified path, a machining center must often coordinate the motion of several axes. We use the term coordinated linear motion to describe the situation in which, nominally, each axis moves at constant speed and all axes move from their starting positions to their end positions at the same time. If only the X, Y, and Z axes (or any one or two of them) move, this produces motion in a straight line, hence the word linear in the term. In actual motions, it is often not possible to maintain constant speed because acceleration or deceleration is required at the beginning and/or end of the motion. It is feasible, however, to control the axes so that, at all times, each axis has completed the same fraction of its required motion as the other axes. This moves the tool along same path, and we also call this kind of motion coordinated linear motion.

Coordinated linear motion can be performed either at the prevailing feed rate, or at traverse rate, or it may be synchronized to the spindle rotation. If physical limits on axis speed make the desired rate unobtainable, all axes are slowed to maintain the desired path.

The rate at which the controlled point moves is nominally a steady rate which may be set by the user. In the Interpreter, the feed rate is interpreted as follows (unless inverse time feed or feed per revolution modes are being used, in which case see Section G93-G94-G95-Mode).

Flood coolant and mist coolant may each be turned on independently. The RS274/NGC language turns them off together see Section M7 M8 M9.

A machining center may be commanded to dwell (i.e., keep all axes unmoving) for a specific amount of time. The most common use of dwell is to break and clear chips, so the spindle is usually turning during a dwell. Regardless of the Path Control Mode (see Section Path Control) the machine will stop exactly at the end of the previous programmed move, as though it was in exact path mode.

Units used for distances along the X, Y, and Z axes may be measured in millimeters or inches. Units for all other quantities involved in machine control cannot be changed. Different quantities use different specific units. Spindle speed is measured in revolutions per minute. The positions of rotational axes are measured in degrees. Feed rates are expressed in current length units per minute, or degrees per minute, or length units per spindle revolution, as described in Section G93 G94 G95.

The controlled point is always at some location called the current position, and the controller always knows where that is. The numbers representing the current position must be adjusted in the absence of any axis motion if any of several events take place:

There is always a selected plane, which must be the XY-plane, the YZ-plane, or the XZ-plane of the machining center. The Z-axis is, of course, perpendicular to the XY-plane, the X-axis to the YZ-plane, and the Y-axis to the XZ-plane.

Zero or one tool is assigned to each slot in the tool carousel.

A machining center may be commanded to change tools.

The two pallets may be exchanged by command.

The machining center may be put into any one of three path control modes: (1) exact stop mode, (2) exact path mode, or (3) continuous mode with optional tolerance. In exact stop mode, the machine stops briefly at the end of each programmed move. In exact path mode, the machine follows the programmed path as exactly as possible, slowing or stopping if necessary at sharp corners of the path. In continuous mode, sharp corners of the path may be rounded slightly so that the feed rate may be kept up (but by no more than the tolerance, if specified). See Sections G61/G61.1 and G64.

The Interpreter will interpret RS274/NGC commands which enable M48 or disable M49 the feed and speed override switches. For certain moves, such as the traverse out of the end of a thread during a threading cycle, the switches are disabled automatically.

LinuxCNC reacts to the speed and feed override settings when these switches are enabled.

See the M48 M49 Override section for more information.

If the block delete switch is on, lines of G code which start with a slash (the block delete character) are not interpreted. If the switch is off, such lines are interpreted. Normally the block delete switch should be set before starting the NGC program.

If this switch is on and an M1 code is encountered, program execution is paused.