This section gives a brief description of how a CNC machine is viewed from the input and output ends of the Interpreter.
1. Mechanical Components
A CNC machine has many mechanical components that may be controlled or may affect the way in which control is exercised. This section describes the subset of those components that interact with the Interpreter. Mechanical components that do not interact directly with the Interpreter, such as the jog buttons, are not described here, even if they affect control.
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 EMC, 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.]
1.1.1. Primary Linear Axes
The X, Y, and Z axes produce linear motion in three mutually orthogonal directions.
1.1.2. Secondary Linear Axes
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.
1.1.3. Rotational Axes
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. See Section [sub:Feed-Interaction].
A CNC machine can have a block delete switch. See Section [sub:Block-Delete-Switch-Interaction].
A CNC machine can have an optional program stop switch. See Section [sub:Optional-Program-Stop-Interaction].
2. Control and Data Components
2.1. Linear Axes
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).
2.2. Rotational Axes
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 or the axes move is nominally a steady rate which may be set by the user. In the Interpreter, the interpretation of the feed rate is as follows unless “inverse time feed” or “feed per revolution” modes are being used (see Section -G94:-Set).
If any of XYZ are moving, F is in units per minute in the XYZ cartesian system, and all other axes (ABCUVW) move so as to start and stop in coordinated fashion.
Otherwise, if any of UVW are moving, F is in units per minute in the UVW cartesian system, and all other axes (ABC) move so as to start and stop in coordinated fashion.
Otherwise, the move is pure rotary motion and the F word is in rotary units in the ABC “pseudo-cartesian” system.
Flood coolant and mist coolant may each be turned on independently. The RS274/NGC language turns them off together (see Section -M8).
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 [sub:Path-Control-Mode]) 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 [sub:Feed-Rate].
2.9. Current Position
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:
Length units are changed.
Tool length offset is changed.
Coordinate system offsets are changed.
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.
2.11. Tool Carousel
Zero or one tool is assigned to each slot in the tool carousel.
2.12. Tool Change
A machining center may be commanded to change tools.
2.13. Pallet Shuttle
The two pallets may be exchanged by command.
2.14. Feed and Speed Override Switches
The feed and speed override switches may be enabled (so they work as expected) or disabled (so they have no effect on the feed rate or spindle speed). The RS274/NGC language has one command that enables both switches and one command that disables both (see Sections [sub:M48-Both-Override] and [sub:M49-Neither-Override]). See Section [sub:Feed-Interaction] for further details.
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 Section [sec:G61-G61.1-G64].
3. Interpreter Interaction with Switches
The Interpreter interacts with several switches. This section describes the interactions in more detail. In no case does the Interpreter know what the setting of any of these switches is.
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.
EMC2 reacts to the speed and feed override settings when these switches are enabled.
If the block delete switch is on, lines of RS274/NGC 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.
A tool table is required to use the Interpreter. The file tells which tools are in which tool changer slots and what the size and type of each tool is. The name of the tool table is defined in the ini file:
[EMCIO] # tool table file TOOL_TABLE = tooltable.tbl
The default filename probably looks something like the above, but you may prefer to give your machine its own tool table, using the same name as your ini file, but with a tbl extension:
TOOL_TABLE = acme_300.tbl
TOOL_TABLE = EMC-AXIS-SIM.tbl
For more information on the specifics of the tool table format, see the [sec:Tool-Table-Format] section.
In the RS274/NGC language view, a machining center maintains an array of numerical parameters defined by a system definition (RS274NGC_MAX_PARAMETERS). Many of them have specific uses especially in defining coordinate systems. The number of numerical parameters can increase as development adds support for new parameters. The parameter array persists over time, even if the machining center is powered down. EMC2 uses a parameter file to ensure persistence and gives the Interpreter the responsibility for maintaining the file. The Interpreter reads the file when it starts up, and writes the file when it exits.
All parameters are available for use in G Code programs.
Subroutine local parameters of call arguments. These parameters are local to the subroutine. See [cha:O-Codes]
G-Code user parameters. These parameters are global in the G Code file.
Result of "G38.2" Probe for X, Y, Z, A, B, C, U, V & W.
"G28" Home for X, Y, Z, A, B, C, U, V & W.
"G30" Home for X, Y, Z, A, B, C, U, V & W.
"G92" offset for X, Y, Z, A, B, C, U, V & W.
Coordinate System number 1 - 9 for G54 - G59.3.
Coordinate System 1, G54 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 2, G55 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 3, G56 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 4, G57 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 5, G58 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 6, G59 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 7, G59.1 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 8, G59.2 for X, Y, Z, A, B, C, U, V & W.
Coordinate System 9, G59.3 for X, Y, Z, A, B, C, U, V & W.
Result of M66 - Check or wait for input
Tool X Offset
Tool Y Offset
Tool Z Offset
Tool A Offset
Tool B Offset
Tool C Offset
Tool U Offset
Tool V Offset
Tool W Offset
Tool Front Angle
Tool Back Angle
Current Position including all offsets and in the current program units for X, Y, Z, A, B, C, U, V & W.
The format of a parameter file is shown in Table [cap:Parameter-File-Format]. The file consists of any number of header lines, followed by one blank line, followed by any number of lines of data. The Interpreter skips over the header lines. It is important that there be exactly one blank line (with no spaces or tabs, even) before the data. The header line shown in Table [cap:Parameter-File-Format] describes the data columns, so it is suggested (but not required) that that line always be included in the header.
The Interpreter reads only the first two columns of the table. The third column, "Comment," is not read by the Interpreter.
Each line of the file contains the index number of a parameter in the first column and the value to which that parameter should be set in the second column. The value is represented as a double-precision floating point number inside the Interpreter, but a decimal point is not required in the file. All of the parameters shown in Table [cap:Parameter-File-Format] are required parameters and must be included in any parameter file, except that any parameter representing a rotational axis value for an unused axis may be omitted. An error will be signalled if any required parameter is missing. A parameter file may include any other parameter, as long as its number is in the range 1 to 5400. The parameter numbers must be arranged in ascending order. An error will be signalled if not. Any parameter included in the file read by the Interpreter will be included in the file it writes as it exits. The original file is saved as a backup file when the new file is written. Comments are not preserved when the file is written.