This section gives a brief description of how a machining center is viewed from the input and output ends of the Interpreter. It is assumed the reader is already familiar with machining centers.
Both the RS274/NGC input language and the output canonical machining functions have a view of (1) mechanical components of a machining center being controlled and (2) what activities of the machining center may be controlled, and what data is used in control.
The view here includes some items that a given machining center may not have, such as a pallet shuttle. The RS274/NGC language and canonical machining functions may be used with such a machine provided that no NC program used with the controller includes commands intended to activate physical capabilities the machine does not have. For such a machine, it would be useful to modify the Interpreter so it will reject input commands and will not produce output canonical function calls addressed to non-existent equipment.
A machining center 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.
A machining center has independent mechanisms1.1 for producing relative linear motion of the tool and workpiece in three mutually orthogonal directions. These are the X, Y and Z axes.
Three additional independent mechanisms produce relative rotation of the workpiece and the tool around an axis. These mechanisms (often a rotary table on which the workpiece is mounted or a drum on which the spindle is mounted) are called rotational axes and labelled A, B, and C. The A-axis is parallel to the X-axis. B is parallel to the Y-axis, and C parallel to the Z-axis1.2. Each rotational mechanism may or may not have a mechanical limit on how far it can rotate.
A machining center has a spindle which holds one cutting tool, probe, or other item. The spindle can rotate in either direction, and it can be made to rotate at a constant rate, which may be changed. Except on machines where the spindle may be moved by moving a rotational axis, the axis of the spindle is kept parallel to the Z-axis and is coincident with the Z-axis when X and Y are zero. The spindle can be stopped in a fixed orientation or stopped without specifying orientation.
A machining center has components to provide mist coolant and/or flood coolant.
A machining center has a pallet shuttle system. The system has two movable pallets on which workpieces can be fixtured. Only one pallet at a time is in position for machining.
A machining center has a tool carousel with slots for tools fixed in tool holders.
A machining center has a mechanism for changing tools (fixed in tool holders) between the spindle and the tool carousel.
A machining center has a device that can display messages.
A machining center has separate feed and speed override switches, which let the operator specify that the actual feed rate or spindle speed used in machining should be some percentage of the programmed rate. See Section .
A machining center has a block delete switch. See Section .
A machining center has an optional program stop switch. See 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 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 machine1.3
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.
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. 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 rate mode is being used in the RS274/NGC view (see Section ).
Flood coolant and mist coolant may each be turned on independently. The RS274/NGC language turns them off together (see Section ).
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 ) 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 in degrees per minute, as described in Section .
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 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 Section ). See Section 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 .
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. It is useful to be able to override these switches for some machining operations. The idea is that optimal settings have been included in the program, and the operator should not change them.
EMC2 reacts to the setting of the speed or feed override switches on the control panel, 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.
The Interpreter runs in two stages (read and execute). The driver tells the Interpreter when to perform each stage. When the Interpreter reads a line starting with a slash, it informs the driver, ``I just read a line starting with a slash.'' The driver checks the setting of the block delete switch. If the switch is off, it tells the Interpreter, ``Execute that line.'' If the switch is on, the driver does not tell the Interpreter to execute the line. Instead, it tells the Interpreter to read another line, with the result that the line starting with the slash is not executed.
The optional program stop switch works as follows. If this switch is on and an input RS274/NGC code line contains an M1 code, program execution is supposed to stop until the cycle start button is pushed.
EMC2 checks the optional stop switch when the OPTIONAL_PROGRAM_STOP canonical function call is executed and either stops (if the switch is on) or not (if the switch is off).
A tool file is required to use the Interpreter. The file tells which tools are in which carousel slots and what the length and diameter of each tool are.
The format of a tool file is exemplified in Table .
The file consists of any number of header lines, followed by one blank line, followed by any number of lines of data. The header lines are ignored. 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 describes the data columns, so it is suggested (but not required) that such a line always be included in the header.
Each data line of the file contains the data for one tool. Each line has five entries. The first four entries are required. The last entry (a comment) is optional. It makes reading easier if the entries are arranged in columns, as shown in the table, but the only format requirement is that there be at least one space or tab after each of the first three entries on a line and a space, tab, or newline at the end of the fourth entry. The meanings of the columns and the type of data to be put in each are as follows.
The ``Pocket'' column contains an unsigned integer which represents the pocket number (slot number) of the tool carousel slot in which the tool is placed. The entries in this column must all be different.
The ``FMS'' column contains an unsigned integer which represents a code number for the tool. The user may use any code for any tool, as long as the codes are unsigned integers.
The ``TLO'' column contains a real number which represents the tool length offset. This number will be used if tool length offsets are being used and this pocket is selected. This is normally a positive real number, but it may be zero or any other number if it is never to be used.
The ``Diameter'' column contains a real number. This number is used only if tool radius compensation is turned on using this pocket. If the programmed path during compensation is the edge of the material being cut, this should be a positive real number representing the measured diameter of the tool. If the programmed path during compensation is the path of a tool whose diameter is nominal, this should be a small number (positive, negative, or zero) representing the difference between the measured diameter of the tool and the nominal diameter. If cutter radius compensation is not used with a tool, it does not matter what number is in this column.
The ``Comment'' column may optionally be used to describe the tool. Any type of description is OK. This column is for the benefit of human readers only.
The units used for the length and diameter of the tool may be in either millimeters or inches, but if the data is used by an NC program, the user must be sure the units used for a tool in the file are the same as the units in effect when NC code that uses the tool data is interpreted. The table shows a mixture of types of units.
The lines do not have to be in any particular order. Switching the order of lines has no effect unless the same slot number is used on two or more lines, which should not normally be done, in which case the data for only the last such line will be used.
In the RS274/NGC language view, a machining center maintains an array of 5400 numerical parameters. Many of them have specific uses. 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.
The format of a parameter file is shown in Table . 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 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 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.
In the RS274/NGC language view, a machining center has an absolute coordinate system and nine program coordinate systems.
You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of the coordinate system) with values for the axes in terms of the absolute coordinate system. See Section .
You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or G59.3 (see Section ). It is not possible to select the absolute coordinate system directly.
You can offset the current coordinate system using G92 or G92.3. This offset will then apply to all nine program coordinate systems. This offset may be cancelled with G92.1 or G92.2. See Section .
You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or G1. See Section .
Data for coordinate systems is stored in parameters.
During initialization, the coordinate system is selected that is specified by parameter 5220. A value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220 to be anything but a whole number between one and nine.
The RS274/NGC language is based on lines of code. Each line (also called a ``block'') may include commands to a machining center to do several different things. Lines of code may be collected in a file to make a program.
A typical line of code consists of an optional line number at the beginning followed by one or more ``words.'' A word consists of a letter followed by a number (or something that evaluates to a number). A word may either give a command or provide an argument to a command. For example, ``G1 X3'' is a valid line of code with two words. ``G1'' is a command meaning ``move in a straight line at the programmed feed rate'', and ``X3'' provides an argument value (the value of X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for General and Miscellaneous). The words for these commands are called ``G codes'' and ``M codes.''
The RS274/NGC language has no indicator for the start of a program. The Interpreter, however, deals with files. A single program may be in a single file, or a program may be spread across several files. A file may demarcated with percents in the following way. The first non-blank line of a file may contain nothing but a percent sign, ``%'', possibly surrounded by white space, and later in the file (normally at the end of the file) there may be a similar line. Demarcating a file with percents is optional if the file has an M2 or M30 in it, but is required if not. An error will be signalled if a file has a percent line at the beginning but not at the end. The useful contents of a file demarcated by percents stop after the second percent line. Anything after that is ignored.
The RS274/NGC language has two commands (M2 or M30), either of which ends a program. A program may end before the end of a file. Lines of a file that occur after the end of a program are not to be executed. The interpreter does not even read them.
A permissible line of input RS274/NGC code consists of the following, in order, with the restriction that there is a maximum (currently 256) to the number of characters allowed on a line.
Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the line, except inside comments. This makes some strange-looking input legal. The line ``g0x +0. 12 34y 7'' is equivalent to ``g0 x+0.1234 y7'', for example.
Blank lines are allowed in the input. They are to be ignored.
Input is case insensitive, except in comments, i.e., any letter outside a comment may be in upper or lower case without changing the meaning of a line.
A line number is the letter N followed by an integer (with no sign) between 0 and 99999 written with no more than five digits (000009 is not OK, for example). Line numbers may be repeated or used out of order, although normal practice is to avoid such usage. Line numbers may also be skipped, and that is normal practice. A line number is not required to be used, but must be in the proper place if used.
A word is a letter other than N followed by a real value.
Words may begin with any of the letters shown in Table . The table includes N for completeness, even though, as defined above, line numbers are not words. Several letters (I, J, K, L, P, R) may have different meanings in different contexts.
The following rules are used for (explicit) numbers. In these rules a digit is a single character between 0 and 9.
Numbers used for specific purposes in RS274/NGC are often restricted to some finite set of values or some to some range of values. In many uses, decimal numbers must be close to integers; this includes the values of indexes (for parameters and carousel slot numbers, for example), M codes, and G codes multiplied by ten. A decimal number which is supposed be close to an integer is considered close enough if it is within 0.0001 of an integer.
A parameter value is the pound character # followed by a real value. The real value must evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the parameter value is whatever number is stored in the numbered parameter.
The # character takes precedence over other operations, so that, for example, ``#1+2'' means the number found by adding 2 to the value of parameter 1, not the value found in parameter 3. Of course, #[1+2] does mean the value found in parameter 3. The # character may be repeated; for example ##2 means the value of the parameter whose index is the (integer) value of parameter 2.
An expression is a set of characters starting with a left bracket [ and ending with a balancing right bracket ]. In between the brackets are numbers, parameter values, mathematical operations, and other expressions. An expression may be evaluated to produce a number. The expressions on a line are evaluated when the line is read, before anything on the line is executed. An example of an expression is [ 1 + acos - [#3 ** [4.0/2]]].
Binary operations appear only inside expressions. There are four basic mathematical operations: addition (+), subtraction (-), multiplication (*), and division (/). There are three logical operations: non-exclusive or (OR), exclusive or (XOR), and logical and (AND). The eighth operation is the modulus operation (MOD). The ninth operation is the ``power'' operation (**) of raising the number on the left of the operation to the power on the right. The relational operators are equality (EQ), inequality (NE), strictly greater than (GT), greater than or equal to (GE), strictly less than (LT), and less than or equal to (LE).
The binary operations are divided into three groups. The first group is: power. The second group is: multiplication, division, and modulus. The third group is: addition, subtraction, logical non-exclusive or, logical exclusive or, and logical and. If operations are strung together (for example in the expression [2.0 / 3 * 1.5 - 5.5 / 11.0]), operations in the first group are to be performed before operations in the second group and operations in the second group before operations in the third group. If an expression contains more than one operation from the same group (such as the first / and * in the example), the operation on the left is performed first. Thus, the example is equivalent to: [((2.0 / 3) * 1.5) - (5.5 / 11.0)] , which simplifies to [1.0 - 0.5] , which is 0.5.
The logical operations and modulus are to be performed on any real numbers, not just on integers. The number zero is equivalent to logical false, and any non-zero number is equivalent to logical true.
A unary operation value is either ``ATAN'' followed by one expression divided by another expression (for example ``ATAN/[1+3]'') or any other unary operation name followed by an expression (for example ``SIN''). The unary operations are: ABS (absolute value), ACOS (arc cosine), ASIN (arc sine), ATAN (arc tangent), COS (cosine), EXP (e raised to the given power), FIX (round down), FUP (round up), LN (natural logarithm), ROUND (round to the nearest whole number), SIN (sine), SQRT (square root), and TAN (tangent). Arguments to unary operations which take angle measures (COS, SIN, and TAN) are in degrees. Values returned by unary operations which return angle measures (ACOS, ASIN, and ATAN) are also in degrees.
The FIX operation rounds towards the left (less positive or more negative) on a number line, so that FIX[2.8] =2 and FIX[-2.8] = -3, for example. The FUP operation rounds towards the right (more positive or less negative) on a number line; FUP[2.8] = 3 and FUP[-2.8] = -2, for example.
A parameter setting is the following four items one after the other: (1) a pound character # , (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign = , and (4) a real value. For example ``#3 = 15'' is a parameter setting meaning ``set parameter 3 to 15.''
A parameter setting does not take effect until after all parameter values on the same line have been found. For example, if parameter 3 has been previously set to 15 and the line ``#3=6 G1 x#3'' is interpreted, a straight move to a point where x equals 15 will occur and the value of parameter 3 will be 6.
Printable characters and white space inside parentheses is a comment. A left parenthesis always starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left parenthesis is placed on a line, a matching right parenthesis must appear before the end of the line. Comments may not be nested; it is an error if a left parenthesis is found after the start of a comment and before the end of the comment. Here is an example of a line containing a comment: ``G80 M5 (stop motion)''. Comments do not cause a machining center to do anything.
A comment contains a message if ``MSG,'' appears after the left parenthesis and before any other printing characters. Variants of ``MSG,'' which include white space and lower case characters are allowed. The rest of the characters before the right parenthesis are considered to be a message. Messages should be displayed on the message display device. Comments not containing messages need not be displayed there.
A comment can also be used to specify a file for the results of G38.2 probing. See section .
A line may have any number of G words, but two G words from the same modal group (see Section ) may not appear on the same line.
A line may have zero to four M words. Two M words from the same modal group may not appear on the same line.
For all other legal letters, a line may have only one word beginning with that letter.
If a parameter setting of the same parameter is repeated on a line, ``#3=15 #3=6'', for example, only the last setting will take effect. It is silly, but not illegal, to set the same parameter twice on the same line.
If more than one comment appears on a line, only the last one will be used; each of the other comments will be read and its format will be checked, but it will be ignored thereafter. It is expected that putting more than one comment on a line will be very rare.
The three types of item whose order may vary on a line (as given at the beginning of this section) are word, parameter setting, and comment. Imagine that these three types of item are divided into three groups by type.
The first group (the words) may be reordered in any way without changing the meaning of the line.
If the second group (the parameter settings) is reordered, there will be no change in the meaning of the line unless the same parameter is set more than once. In this case, only the last setting of the parameter will take effect. For example, after the line ``#3=15 #3=6'' has been interpreted, the value of parameter 3 will be 6. If the order is reversed to ``#3=6 #3=15'' and the line is interpreted, the value of parameter 3 will be 15.
If the third group (the comments) contains more than one comment and is reordered, only the last comment will be used.
If each group is kept in order or reordered without changing the meaning of the line, then the three groups may be interleaved in any way without changing the meaning of the line. For example, the line ``g40 g1 #3=15 (foo) #4=-7.0'' has five items and means exactly the same thing in any of the 120 possible orders (such as ``#4=-7.0 g1 #3=15 g40 (foo)'') for the five items.
In RS274/NGC, many commands cause a machining center to change from one mode to another, and the mode stays active until some other command changes it implicitly or explicitly. Such commands are called ``modal''. For example, if coolant is turned on, it stays on until it is explicitly turned off. The G codes for motion are also modal. If a G1 (straight move) command is given on one line, for example, it will be executed again on the next line if one or more axis words is available on the line, unless an explicit command is given on that next line using the axis words or cancelling motion.
``Non-modal'' codes have effect only on the lines on which they occur. For example, G4 (dwell) is non-modal.
Modal commands are arranged in sets called ``modal groups'', and only one member of a modal group may be in force at any given time. In general, a modal group contains commands for which it is logically impossible for two members to be in effect at the same time - like measure in inches vs. measure in millimeters. A machining center may be in many modes at the same time, with one mode from each modal group being in effect. The modal groups are shown in Table .
For several modal groups, when a machining center is ready to accept commands, one member of the group must be in effect. There are default settings for these modal groups. When the machining center is turned on or otherwise re-initialized, the default values are automatically in effect.
Group 1, the first group on the table, is a group of G codes for motion. One of these is always in effect. That one is called the current motion mode.
It is an error to put a G-code from group 1 and a G-code from group 0 on the same line if both of them use axis words. If an axis word-using G-code from group 1 is implicitly in effect on a line (by having been activated on an earlier line), and a group 0 G-code that uses axis words appears on the line, the activity of the group 1 G-code is suspended for that line. The axis word-using G-codes from group 0 are G10, G28, G30, and G92.
It is an error to include any unrelated words on a line with O- flow control.
G codes of the RS274/NGC language are shown in Table 5 and described following that.
In the command prototypes, the hypen (-) stands for a real value. As described earlier, a real value may be (1) an explicit number, 4, for example, (2) an expression, [2+2], for example, (3) a parameter value, #88, for example, or (4) a unary function value, acos, for example.
In most cases, if axis words (any or all of X-, Y-, Z-, A-, B-, C-) are given, they specify a destination point. Axis numbers are in the currently active coordinate system, unless explicitly described as being in the absolute coordinate system. Where axis words are optional, any omitted axes will have their current value. Any items in the command prototypes not explicitly described as optional are required. It is an error if a required item is omitted.
In the prototypes, the values following letters are often given as explicit numbers. Unless stated otherwise, the explicit numbers can be real values. For example, G10 L2 could equally well be written G[2*5] L[1+1]. If the value of parameter 100 were 2, G10 L#100 would also mean the same. Using real values which are not explicit numbers as just shown in the examples is rarely useful.
If L- is written in a prototype the ``-'' will often be referred to as the ``L number''. Similarly the ``-'' in H- may be called the ``H number'', and so on for any other letter.
For rapid linear motion, program G0 X- Y- Z- A- B- C-, where all the axis words are optional, except that at least one must be used. The G0 is optional if the current motion mode is G0. This will produce coordinated linear motion to the destination point at the current traverse rate (or slower if the machine will not go that fast). It is expected that cutting will not take place when a G0 command is executing.
It is an error if:
For linear motion at feed rate (for cutting or not), program G1 X- Y- Z- A- B- C-, where all the axis words are optional, except that at least one must be used. The G1 is optional if the current motion mode is G1. This will produce coordinated linear motion to the destination point at the current feed rate (or slower if the machine will not go that fast).
It is an error if:
A circular or helical arc is specified using either G2 (clockwise arc) or G3 (counterclockwise arc). The axis of the circle or helix must be parallel to the X, Y, or Z-axis of the machine coordinate system. The axis (or, equivalently, the plane perpendicular to the axis) is selected with G17 (Z-axis, XY-plane), G18 (Y-axis, XZ-plane), or G19 (X-axis, YZ-plane). If the arc is circular, it lies in a plane parallel to the selected plane.
If a line of RS274/NGC code makes an arc and includes rotational axis motion, the rotational axes turn at a constant rate so that the rotational motion starts and finishes when the XYZ motion starts and finishes. Lines of this sort are hardly ever programmed.
If cutter radius compensation is active, the motion will differ from what is described here. See Chapter .
Two formats are allowed for specifying an arc: Center Format and Radius Format.
In the center format, the coordinates of the end point of the arc in the selected plane are specified along with the offsets of the center of the arc from the current location. In this format, it is OK if the end point of the arc is the same as the current point. It is an error if:
That means to make a clockwise (as viewed from the positive z-axis) circular or helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=16, and Z=9, with its center offset in the X direction by 3 units from the current X location and offset in the Y direction by 4 units from the current Y location. If the current location has X=7, Y=7 at the outset, the center will be at X=10, Y=11. If the starting value of Z is 9, this is a circular arc; otherwise it is a helical arc. The radius of this arc would be 5.
In the center format, the radius of the arc is not specified, but it may be found easily as the distance from the center of the circle to either the current point or the end point of the arc.
In the radius format, the coordinates of the end point of the arc in the selected plane are specified along with the radius of the arc. Program G2 X- Y- Z- A- B- C- R- (or use G3 instead of G2). R is the radius. The axis words are all optional except that at least one of the two words for the axes in the selected plane must be used. The R number is the radius. A positive radius indicates that the arc turns through less than 180 degrees, while a negative radius indicates a turn of more than 180 degrees. If the arc is helical, the value of the end point of the arc on the coordinate axis parallel to the axis of the helix is also specified.
It is an error if:
Here is an example of a radius format command to mill an arc: G17 G2 x 10 y 15 r 20 z 5.
That means to make a clockwise (as viewed from the positive Z-axis) circular or helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=15, and Z=5, with a radius of 20. If the starting value of Z is 5, this is an arc of a circle parallel to the XY-plane; otherwise it is a helical arc.
For spindle-synchronized motion, code G33 X- Y- Z- K- where K gives the distance moved in XYZ for each revolution of the spindle. This syntax is subject to change (In particular, to use F- instead of K-). For instance, G33 Z1 K.0625 produces a 1 inch motion in Z over 16 revolutions of the spindle. This command might be part of a program to produce a 16TPI thread.
All the axis words are optional, except that at least one must be used. This will produce coordinated linear motion to the destination point at a rate dependant on the speed of the spindle.
It is an error if:
For a dwell, program G4 P- . This will keep the axes unmoving for the period of time in seconds specified by the P number. It is an error if:
The RS274/NGC language view of coordinate systems is described in Section.
To set the coordinate values for the origin of a coordinate system, program G10 L2 P - X- Y- Z- A- B- C-, where the P number must evaluate to an integer in the range 1 to 9 (corresponding to G54 to G59.3) and all axis words are optional. The coordinates of the origin of the coordinate system specified by the P number are reset to the coordinate values given (in terms of the absolute coordinate system). Only those coordinates for which an axis word is included on the line will be reset.
It is an error if:
The coordinate system whose origin is set by a G10 command may be active or inactive at the time the G10 is executed.
Example: G10 L2 P1 x 3.5 y 17.2 sets the origin of the first coordinate system (the one selected by G54) to a point where X is 3.5 and Y is 17.2 (in absolute coordinates). The Z coordinate of the origin (and the coordinates for any rotational axes) are whatever those coordinates of the origin were before the line was executed.
Program G17 to select the XY-plane, G18 to select the XZ-plane, or G19 to select the YZ-plane. The effects of having a plane selected are discussed in Section and Section
Program G20 to use inches for length units. Program G21 to use millimeters.
It is usually a good idea to program either G20 or G21 near the beginning of a program before any motion occurs, and not to use either one anywhere else in the program. It is the responsibility of the user to be sure all numbers are appropriate for use with the current length units.
Two positions are defined (by parameters 5161-5166 for G28 and parameters 5181-5186 for G30). The parameter values are in terms of the absolute coordinate system and the machine's native coordinate system.
To return to the predefined position by way of the programmed position, program G28 X- Y- Z- A- B- C- (or use G30 ...). All axis words are optional. The path is made by a traverse move from the current position to the programmed position, followed by a traverse move to the predefined position. If no axis words are programmed, the intermediate point is the current point, so only one move is made.
G28 and G30 do not use home switches to find the predefined position. They merely command a rapid motion to the position defined by the parameters, assuming that the machine has already been homed.
Program G38.2 X- Y- Z- A- B- C- to perform a straight probe operation. The axis words are optional, except that at least one of them must be used. The tool in the spindle must be a probe.
It is an error if:
After successful probing, parameters 5061 to 5066 will be set to the coordinates of the location of the controlled point at the time the probe tripped.
A comment of the form (PROBEOPEN filename.txt) will open filename.txt and store the coordinate of each successful straight probe in it. The file must be closed with (PROBECLOSE).
To turn cutter radius compensation off, program G40. It is OK to turn compensation off when it is already off.
Cutter radius compensation may be performed only if the XY-plane is active.
To turn cutter radius compensation on left (i.e., the cutter stays to the left of the programmed path when the tool radius is positive), program G41 D- . To turn cutter radius compensation on right (i.e., the cutter stays to the right of the programmed path when the tool radius is positive), program G42 D- . The D word is optional; if there is no D word, the radius of the tool currently in the spindle will be used. If used, the D number should normally be the slot number of the tool in the spindle, although this is not required. It is OK for the D number to be zero; a radius value of zero will be used.
It is an error if:
To use a tool length offset, program G43 H-, where the H number is the desired index in the tool table. It is expected that all entries in this table will be positive. The H number should be, but does not have to be, the same as the slot number of the tool currently in the spindle. It is OK for the H number to be zero; an offset value of zero will be used.
It is an error if:
It is OK to program using the same offset already in use. It is also OK to program using no tool length offset if none is currently being used.
For linear motion to a point expressed in absolute coordinates, program G1 G53 X- Y- Z- A- B- C- (or use G0 instead of G1), where all the axis words are optional, except that at least one must be used. The G0 or G1 is optional if it is the current motion mode. G53 is not modal and must be programmed on each line on which it is intended to be active. This will produce coordinated linear motion to the programmed point. If G1 is active, the speed of motion is the current feed rate (or slower if the machine will not go that fast). If G0 is active, the speed of motion is the current traverse rate (or slower if the machine will not go that fast).
It is an error if:
To select coordinate system 1, program G54, and similarly for other coordinate systems. The system-number-G-code pairs are: (1-G54), (2-G55), (3-G56), (4-G57), (5-G58), (6-G59), (7-G59.1), (8-G59.2), and (9-G59.3).
It is an error if:
Program G61 to put the machining center into exact path mode, G61.1 for exact stop mode, or G64 P- for continuous mode with optional tolerance. It is OK to program for the mode that is already active. See Section for a discussion of these modes.
Program G80 to ensure no axis motion will occur. It is an error if:
Program G76 P- Z- I- J- R- K- Q- H- to perform a threading canned cycle. It is an error if:
The ``thread pitch'', or distance per revolution, is given by the P- value.
The ``thread peak'' is given by the I- value, which is an offset from the drive line. Negative I values indicate external threads, and positive I values indicate internal threads. Generally the material has been turned to this size before the canned cycle.
The ``initial cut depth'' is given by the J- value. The first threading cut will be J beyond the ``thread peak'' position. J- is positive, even when I- is negative.
The ``full thread depth'' is given by the K- value. The final threading cut will be K beyond the ``thread peak'' position. K- is positive, even when I- is negative.
The ``depth degression'' is given by the R- value. R1.0 selects constant depth on successive threading passes. R2.0 selects constant area. Values between 1.0 and 2.0 select decreasing depth and increasing area. Values above 2.0 select decreasing area.
The ``compound slide angle'' Q- is the angle (in degrees) describing to what extent successive passes should be offset along the drive line. This is used to cause one side of the tool to remove more material than the other. A positive Q value causes the leading edge of the tool to cut more heavily. Typical values are 29, 29.5 or 30.
The number of ``spring passes'' is given by the H- value. Spring passes are additional passes at full thread depth. If no additional passes are desired, program H0.
Each pass begins at a position on the drive line. It consists of
The exit move (traverse to original X) is not synchronized to the spindle speed. With a slow spindle, the exit move might take only a small fraction of a revolution. If the spindle speed is increased after several passes are complete, subsequent exit moves will require a larger portion of a revolution, resulting in a very heavy cut during the exit move. This can be avoided by providing a relief groove at the exit, or by not changing the spindle speed while threading.
The sample program g76.ngc shows the use of the G76 canned cycle, and can be previewed and executed on any machine using the sim/lathe.ini configuration.
The canned cycles G81 through G89 have been implemented as described in this section. Two examples are given with the description of G81 below.
All canned cycles are performed with respect to the currently selected plane. Any of the three planes (XY, YZ, ZX) may be selected. Throughout this section, most of the descriptions assume the XY-plane has been selected. The behavior is always analogous if the YZ or XZ-plane is selected.
Rotational axis words are allowed in canned cycles, but it is better to omit them. If rotational axis words are used, the numbers must be the same as the current position numbers so that the rotational axes do not move.
All canned cycles use X, Y, R, and Z numbers in the NC code. These numbers are used to determine X, Y, R, and Z positions. The R (usually meaning retract) position is along the axis perpendicular to the currently selected plane (Z-axis for XY-plane, X-axis for YZ-plane, Y-axis for XZ-plane). Some canned cycles use additional arguments.
For canned cycles, we will call a number ``sticky'' if, when the same cycle is used on several lines of code in a row, the number must be used the first time, but is optional on the rest of the lines. Sticky numbers keep their value on the rest of the lines if they are not explicitly programmed to be different. The R number is always sticky.
In incremental distance mode: when the XY-plane is selected, X, Y, and R numbers are treated as increments to the current position and Z as an increment from the Z-axis position before the move involving Z takes place; when the YZ or XZ-plane is selected, treatment of the axis words is analogous. In absolute distance mode, the X, Y, R, and Z numbers are absolute positions in the current coordinate system.
The L number is optional and represents the number of repeats. L = 0 is not allowed. If the repeat feature is used, it is normally used in incremental distance mode, so that the same sequence of motions is repeated in several equally spaced places along a straight line. In absolute distance mode, L > 1 means ``do the same cycle in the same place several times,'' Omitting the L word is equivalent to specifying L = 1. The L number is not sticky.
When L > 1 in incremental mode with the XY-plane selected, the X and Y positions are determined by adding the given X and Y numbers either to the current X and Y positions (on the first go-around) or to the X and Y positions at the end of the previous go-around (on the repetitions). The R and Z positions do not change during the repeats.
The height of the retract move at the end of each repeat (called ``clear Z'' in the descriptions below) is determined by the setting of the retract mode: either to the original Z position (if that is above the R position and the retract mode is G98, OLD_Z), or otherwise to the R position. See Section
It is an error if:
At the very beginning of the execution of any of the canned cycles, with the XY-plane selected, if the current Z position is below the R position, the Z-axis is traversed to the R position. This happens only once, regardless of the value of L.
In addition, at the beginning of the first cycle and each repeat, the following one or two moves are made
The G81 cycle is intended for drilling. Program G81 X- Y- Z- A- B- C- R- L-
The first move is a traverse along the Z-axis to (1,2,4.8), since old Z < clear Z.
The first repeat consists of 3 moves.
The G82 cycle is intended for drilling. Program G82 X- Y- Z- A- B- C- R- L- P-
The G83 cycle (often called peck drilling) is intended for deep drilling or milling with chip breaking. The retracts in this cycle clear the hole of chips and cut off any long stringers (which are common when drilling in aluminum). This cycle takes a Q number which represents a ``delta'' increment along the Z-axis. Program G83 X- Y- Z- A- B- C- R- L- Q-
This code is currently unimplemented in EMC2. It is accepted, but the behavior is undefined.
The G85 cycle is intended for boring or reaming, but could be used for drilling or milling. Program G85 X- Y- Z- A- B- C- R- L-
The G86 cycle is intended for boring. This cycle uses a P number for the number of seconds to dwell. Program G86 X- Y- Z- A- B- C- R- L- P-
This code is currently unimplemented in EMC2. It is accepted, but the behavior is undefined.
This code is currently unimplemented in EMC2. It is accepted, but the behavior is undefined.
The G89 cycle is intended for boring. This cycle uses a P number, where P specifies the number of seconds to dwell. program G89 X- Y- Z- A- B- C- R- L- P-
Interpretation of RS274/NGC code can be in one of two distance modes: absolute or incremental.
To go into absolute distance mode, program G90. In absolute distance mode, axis numbers (X, Y, Z, A, B, C) usually represent positions in terms of the currently active coordinate system. Any exceptions to that rule are described explicitly in this Section .
To go into incremental distance mode, program G91. In incremental distance mode, axis numbers (X, Y, Z, A, B, C) usually represent increments from the current values of the numbers.
I and J numbers always represent increments, regardless of the distance mode setting. K numbers represent increments in all but one usage (see Section ), where the meaning changes with distance mode.
See Section for an overview of coordinate systems.
To make the current point have the coordinates you want (without motion), program G92 X- Y- Z- A- B- C- , where the axis words contain the axis numbers you want. All axis words are optional, except that at least one must be used. If an axis word is not used for a given axis, the coordinate on that axis of the current point is not changed. It is an error if:
Here is an example. Suppose the current point is at X=4 in the currently specified coordinate system and the current X-axis offset is zero, then G92 x7 sets the X-axis offset to -3, sets parameter 5211 to -3, and causes the X-coordinate of the current point to be 7.
The axis offsets are always used when motion is specified in absolute distance mode using any of the nine coordinate systems (those designated by G54 - G59.3). Thus all nine coordinate systems are affected by G92.
Being in incremental distance mode has no effect on the action of G92.
Non-zero offsets may be already be in effect when the G92 is called. If this is the case, the new value of each offset is A+B, where A is what the offset would be if the old offset were zero, and B is the old offset. For example, after the previous example, the X-value of the current point is 7. If G92 x9 is then programmed, the new X-axis offset is -5, which is calculated by [[7-9] + -3].
To reset axis offsets to zero, program G92.1 or G92.2. G92.1 sets parameters 5211 to 5216 to zero, whereas G92.2 leaves their current values alone.
To set the axis offset values to the values given in parameters 5211 to 5216, program G92.3.
You can set axis offsets in one program and use the same offsets in another program. Program G92 in the first program. This will set parameters 5211 to 5216. Do not use G92.1 in the remainder of the first program. The parameter values will be saved when the first program exits and restored when the second one starts up. Use G92.3 near the beginning of the second program. That will restore the offsets saved in the first program. If other programs are to run between the the program that sets the offsets and the one that restores them, make a copy of the parameter file written by the first program and use it as the parameter file for the second program.
Two feed rate modes are recognized: units per minute and inverse time. Program G94 to start the units per minute mode. Program G93 to start the inverse time mode.
In units per minute feed rate mode, an F word is interpreted to mean the controlled point should move at a certain number of inches per minute, millimeters per minute, or degrees per minute, depending upon what length units are being used and which axis or axes are moving.
In inverse time feed rate mode, an F word means the move should be completed in [one divided by the F number] minutes. For example, if the F number is 2.0, the move should be completed in half a minute.
When the inverse time feed rate mode is active, an F word must appear on every line which has a G1, G2, or G3 motion, and an F word on a line that does not have G1, G2, or G3 is ignored. Being in inverse time feed rate mode does not affect G0 (rapid traverse) motions. It is an error if:
When the spindle retracts during canned cycles, there is a choice of how far it retracts: (1) retract perpendicular to the selected plane to the position indicated by the R word, or (2) retract perpendicular to the selected plane to the position that axis was in just before the canned cycle started (unless that position is lower than the position indicated by the R word, in which case use the R word position).
To use option (1), program G99. To use option (2), program G98. Remember that the R word has different meanings in absolute distance mode and incremental distance mode.
To stop a running program temporarily (regardless of the setting of the optional stop switch), program M0.
To stop a running program temporarily (but only if the optional stop switch is on), program M1.
It is OK to program M0 and M1 in MDI mode, but the effect will probably not be noticeable, because normal behavior in MDI mode is to stop after each line of input, anyway.
To exchange pallet shuttles and then stop a running program temporarily (regardless of the setting of the optional stop switch), program M60.
If a program is stopped by an M0, M1, or M60, pressing the cycle start button will restart the program at the following line.
To end a program, program M2. To exchange pallet shuttles and then end a program, program M30. Both of these commands have the following effects.
To start the spindle turning clockwise at the currently programmed speed, program M3.
To start the spindle turning counterclockwise at the currently programmed speed, program M4.
To stop the spindle from turning, program M5.
It is OK to use M3 or M4 if the spindle speed is set to zero. If this is done (or if the speed override switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle speed is set above zero (or the override switch is turned up), the spindle will start turning. It is OK to use M3 or M4 when the spindle is already turning or to use M5 when the spindle is already stopped.
To change a tool in the spindle from the tool currently in the spindle to the tool most recently selected (using a T word - see Section ), program M6. When the tool change is complete:
To turn mist coolant on, program M7.
To turn flood coolant on, program M8.
To turn all coolant off, program M9.
It is always OK to use any of these commands, regardless of what coolant is on or off.
To enable the spindle speed and feedrate override switches, program M48. To disable both switches, program M49. See Section for more details. It is OK to enable or disable the switches when they are already enabled or disabled. These switches can also be toggled individually using M50 and M51 as described in the sections and .
To enable the feedrate override switch, program M50 or M50 P1. To disable the switch program M50 P0. While disabled the feed override will have no influence, and the motion will be executed at programmed feedrate. (unless there is an adaptive feedrate override active).
To enable the spindle speed override switch, program M51 or M51 P1. To disable the switch program M51 P0. While disabled the spindle speed override will have no influence, and the spindle speed will have the exact program specified value (using the S-word as described in ).
To use an adaptive feed, program M52 or M52 P1. To stop using adaptive feed, program M52 P0. When adaptive feed is enabled, some external input value is used together with the user interface feed override value and the commanded feed rate to set the actual feed rate. In EMC2, the HAL pin motion.adaptive-feed is used for this purpose. Values on motion.adaptive-feed should range from 0 (feed hold) to 1 (full speed).
To enable the feed stop switch, program M53 or M53 P1. To disable the switch program M53 P0. Enabling the feed stop switch will allow motion to be interrupted by means of the feedstop control. In EMC2, the HAL pin motion.feed-hold is used for this purpose. Values of 1 will cause the motion to stop (if M53 is active).
To control a digital output bit, program M- P-, where the M-word ranges from 62 to 65, and the P-word ranges from 0 to an implementation-defined maximum.
To invoke a user-defined command, program M- P- Q- where P- and Q- are both optional. The external program ``Mnnn'' in the directory [DISPLAY]PROGRAM_PREFIX is executed with the P and Q values as its two arguments. Execution of the RS274NGC file pauses until the invoked program exits.
It is an error if
O-codes provide for flow control in NC programs. Each block has an associated number, which is the number used after O. Care must be taken to properly match the O-numbers.
The behavior is undefined if
Subroutines extend from a O- sub to an O- endsub. The lines inside the subroutine (the ``body'') are not executed in order; instead, they are executed each time the subroutine is called with O- call.
O- call takes up to 30 optional arguments, which are passed to the subroutine as #1, #2, ..., #N. Parameters from #N+1 to #30 have the same value as in the calling context. On return from the subroutine the previous values parameters #1 through #30 (regardless of the number of arguments) will be restored to the values they had before the call.
Because ``1 2 3'' is parsed as the number 123, the parameters must be enclosed in square brackets. The following calls a subroutine with 3 arguments:
Subroutines do not have ``return values'', but they may change the value of parameters above #30 and those changes will be visible to the calling code.
The ``while loop'' has two structures: while/endwhile, and do/while. In each case, the loop is exited when the ``while'' condition evaluates to false.
Inside a while loop, O- break immediately exits the loop,
and O- continue immediately skips to the next evaluation
of the while condition. If it is still true, the loop begins
again at the top. If it is false, it exits the loop.
The ``if'' conditional executes one group of statements if a condition is true and another if it is false.
The O- value may be given by a parameter or calculation.
To set the feed rate, program F- . The application of the feed rate is as described in Section , unless inverse time feed rate mode is in effect, in which case the feed rate is as described in Section .
To set the speed in revolutions per minute (rpm) of the spindle, program S- . The spindle will turn at that speed when it has been programmed to start turning. It is OK to program an S word whether the spindle is turning or not. If the speed override switch is enabled and not set at 100%, the speed will be different from what is programmed. It is OK to program S0; the spindle will not turn if that is done. It is an error if:
To select a tool, program T-, where the T number is the carousel slot for the tool. The tool is not changed until an M6 is programmed (see Section ). The T word may appear on the same line as the M6 or on a previous line. It is OK, but not normally useful, if T words appear on two or more lines with no tool change. The carousel may move a lot, but only the most recent T word will take effect at the next tool change. It is OK to program T0; no tool will be selected. This is useful if you want the spindle to be empty after a tool change. It is an error if:
The order of execution of items on a line is critical to safe and effective machine operation. Items are executed in the order shown below if they occur on the same line.
Use at least 3 digits after the decimal when milling in millimeters, and at least 4 digits after the decimal when milling in inches. In particular, arc tolerance checks are made to .001 and .0001 depending on the active units.
G-code is most legible when at least one space appears before words. While it is permitted to insert whitespace in the middle of numbers, there is no reason to do so.
Center-format arcs (which use I- J- K- instead of R-) behave more consistently than R-format arcs, particularly for included angles near 180 or 360 degrees.
When correct execution of your program depends on modal settings, be sure to set them at the beginning of the part program. Modes can carry over from previous programs and from the MDI commands.
As a good preventative measure, put a line similar to the following at the top of all your programs:
Perhaps the most critical modal setting is the distance units-If you do not include G20 or G21, then different machines will mill the program at different scales. Other settings, such as the return mode in canned cycles may also be important.
Ignore everything in Section , and instead write no line of code that is the slightest bit ambiguous. Similarly, don't use and set a parameter on the same line, even though the semantics are well defined. (Exception: Updating a variable to a new value, such as #1=#1+#2)
Line numbers offer no benefits. When line numbers are reported in error messages, the numbers refer to the line number in the file, not the N-word value.