| |
|
|
|
3 Input: the RS274/NGC Language
This section describes the input language, RS274/NGC. This section is intended for NC programmers, machine operators, developers and researchers. SAI installers can skip it.
3.1 Overview
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 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 SAI does not even read them.
3.2 RS274/NGC Language View of a Machining Center
The RS274/NGC language is based on a particular view of what a machining center to be controlled is like. The view is as described in Section 2.1, with the changes described below. The RS274/NGC language view includes one mechanical component not known to the canonical machining functions: a cycle start button. The use of the button is described in Section 3.6.1.
The RS274/NGC language contains commands that change the way subsequent commands are to be interpreted, but do not tell the machining center to do anything. These are not covered in this section, but are dealt with as they arise in Section 3.5.17, Section 3.5.19, and Section 3.5.20.
3.2.1 Parameters
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 should persist over time, even if the machining center is powered down. The RS274/NGC language makes no provision regarding how to ensure persistence. The EMC project 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 2. 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 2 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 2 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.
3.2.2 Coordinate Systems
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 3.5.5.
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 3.5.13). 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 3.5.18.
You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or G1. See Section 3.5.12.
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.
3.3 Format of a Line
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.
- 1. an optional block delete character, which is a slash "/" .
- 2. an optional line number.
- 3. any number of words, parameter settings, and comments.
- 4. an end of line marker (carriage return or line feed or both).
Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error.
To make the specification of an allowable line of code precise, we have defined it in a production language (Wirth Syntax Notation) in Appendix E.
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.
3.3.1 Line Number
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.
3.3.2 Word
A word is a letter other than N followed by a real value.
Words may begin with any of the letters shown in Table 3. 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.
A real value is some collection of characters that can be processed to come up with a number. A real value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a unary operation value. Definitions of these follow immediately. Processing characters to come up with a number is called "evaluating". An explicit number evaluates to itself.
3.3.2.1 Number
The following rules are used for (explicit) numbers. In these rules a digit is a single character between 0 and 9.
· A number consists of (1) an optional plus or minus sign, followed by (2) zero to many digits, followed, possibly, by (3) one decimal point, followed by (4) zero to many digits - provided that there is at least one digit somewhere in the number.
· There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in it; a decimal does.
· Numbers may have any number of digits, subject to the limitation on line length. Only about seventeen significant figures will be retained, however (enough for all known applications).
Notice that initial (before the decimal point and the first non-zero digit) and trailing (after the decimal point and the last non-zero digit) zeros are allowed but not required. A number written with initial or trailing zeros will have the same value when it is read as if the extra zeros were not there.
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.
3.3.2.2 Parameter Value
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.
3.3.2.3 Expressions and Binary Operations
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[0] - [#3 ** [4.0/2]]].
Binary operations appear only inside expressions. Nine binary operations are defined. 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 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.
3.3.2.4 Unary Operation Value
A unary operation value is either "ATAN" followed by one expression divided by another expression (for example "ATAN[2]/[1+3]") or any other unary operation name followed by an expression (for example "SIN[90]"). 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.
3.3.3 Parameter Setting
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.
3.3.4 Comments and Messages
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.
3.3.5 Item Repeats
A line may have any number of G words, but two G words from the same modal group (see Section 3.4) 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.
3.3.6 Item order
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.
3.3.7 Commands and Machine Modes
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.
3.4 Modal Groups
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 4.
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.
3.5 G Codes
G codes of the RS274/NGC language are shown in Table 5 and described following that.
The descriptions contain command prototypes, set in helvetica type.
In the command prototypes, three dots (-) stand 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[0], 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.
3.5.1 Rapid Linear Motion - G0
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.
If cutter radius compensation is active, the motion will differ from the above; see Appendix B. If G53 is programmed on the same line, the motion will also differ; see Section 3.5.12.
3.5.2 Linear Motion at Feed Rate - G1
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).
If cutter radius compensation is active, the motion will differ from the above; see Appendix B. If G53 is programmed on the same line, the motion will also differ; see Section 3.5.12.
3.5.3 Arc at Feed Rate - G2 and G3
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 Appendix B.
Two formats are allowed for specifying an arc. We will call these the center format and the radius format. In both formats the G2 or G3 is optional if it is the current motion mode.
3.5.3.1 Radius Format 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 180 degrees or less, while a negative radius indicates a turn of 180 degrees to 359.999 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 not good practice to program radius format arcs that are nearly full circles or are semicircles (or nearly semicircles) because a small change in the location of the end point will produce a much larger change in the location of the center of the circle (and, hence, the middle of the arc). The magnification effect is large enough that rounding error in a number can produce out-of-tolerance cuts. Nearly full circles are outrageously bad, semicircles (and nearly so) are only very bad. Other size arcs (in the range tiny to 165 degrees or 195 to 345 degrees) are OK.
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.
3.5.3.2 Center Format Arc
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:
· when the arc is projected on the selected plane, the distance from the current point to the center differs from the distance from the end point to the center by more than 0.0002 inch (if inches are being used) or 0.002 millimeter (if millimeters are being used).
When the XY-plane is selected, program G2 X- Y- Z- A- B- C- I- J- (or use G3 instead of G2). The axis words are all optional except that at least one of X and Y must be used. I and J are the offsets from the current location (in the X and Y directions, respectively) of the center of the circle. I and J are optional except that at least one of the two must be used. It is an error if:
When the XZ-plane is selected, program G2 X- Y- Z- A- B- C- I- K- (or use G3 instead of G2). The axis words are all optional except that at least one of X and Z must be used. I and K are the offsets from the current location (in the X and Z directions, respectively) of the center of the circle. I and K are optional except that at least one of the two must be used. It is an error if:
When the YZ-plane is selected, program G2 X- Y- Z- A- B- C- J- K- (or use G3 instead of G2). The axis words are all optional except that at least one of Y and Z must be used. J and K are the offsets from the current location (in the Y and Z directions, respectively) of the center of the circle. J and K are optional except that at least one of the two must be used. It is an error if:
Here is an example of a center format command to mill an arc: G17 G2 x 10 y 16 i 3 j 4 z 9.
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.
3.5.4 Dwell - G4
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:
3.5.5 Set Coordinate System Data - G10
The RS274/NGC language view of coordinate systems is described in Section 3.2.2.
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.If origin offsets (made by G92 or G92.3) were in effect before G10 is used, they will continue to be in effect afterwards.
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.
3.5.6 Plane Selection - G17, G18, and G19
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 3.5.3 and Section 3.5.16.
3.5.7 Length Units - G20 and G21
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.
3.5.8 Return to Home - G28 and G30
Two home 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, but are in unspecified length units.
To return to home 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 home position. If no axis words are programmed, the intermediate point is the current point, so only one move is made.
3.5.9 Straight Probe - G38.2
3.5.9.1 The Straight Probe Command
Program G38.2 X- Y- Z- A- B- C- to perform a straight probe operation. The rotational axis words are allowed, 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. The linear axis words are optional, except that at least one of them must be used. The tool in the spindle must be a probe.
In response to this command, the machine moves the controlled point (which should be at the end of the probe tip) in a straight line at the current feed rate toward the programmed point. If the probe trips, the probe is retracted slightly from the trip point at the end of command execution. If the probe does not trip even after overshooting the programmed point slightly, an error is signalled.
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.
3.5.9.2 Using the Straight Probe Command
Using the straight probe command, if the probe shank is kept nominally parallel to the Z-axis (i.e., any rotational axes are at zero) and the tool length offset for the probe is used, so that the controlled point is at the end of the tip of the probe:
· without additional knowledge about the probe, the parallelism of a face of a part to the XY-plane may, for example, be found.
· if the probe tip radius is known approximately, the parallelism of a face of a part to the YZ or XZ-plane may, for example, be found.
· if the shank of the probe is known to be well-aligned with the Z-axis and the probe tip radius is known approximately, the center of a circular hole, may, for example, be found.
· if the shank of the probe is known to be well-aligned with the Z-axis and the probe tip radius is known precisely, more uses may be made of the straight probe command, such as finding the diameter of a circular hole.
If the straightness of the probe shank cannot be adjusted to high accuracy, it is desirable to know the effective radii of the probe tip in at least the +X, -X, +Y, and -Y directions. These quantities can be stored in parameters either by being included in the parameter file or by being set in an RS274/NGC program.
Using the probe with rotational axes not set to zero is also feasible. Doing so is more complex than when rotational axes are at zero, and we do not deal with it here.
3.5.9.3 Example Code
As a usable example, the code for finding the center and diameter of a circular hole is shown in Table 6. For this code to yield accurate results, the probe shank must be well-aligned with the Z-axis, the cross section of the probe tip at its widest point must be very circular, and the probe tip radius (i.e., the radius of the circular cross section) must be known precisely. If the probe tip radius is known only approximately (but the other conditions hold), the location of the hole center will still be accurate, but the hole diameter will not.
In Table 6, an entry of the form <description of number> is meant to be replaced by an actual number that matches the description of number. After this section of code has executed, the X-value of the center will be in parameter 1041, the Y-value of the center in parameter 1022, and the diameter in parameter 1034. In addition, the diameter parallel to the X-axis will be in parameter 1024, the diameter parallel to the Y-axis in parameter 1014, and the difference (an indicator of circularity) in parameter 1035. The probe tip will be in the hole at the XY center of the hole.
The example does not include a tool change to put a probe in the spindle. Add the tool change code at the beginning, if needed.
3.5.10 Cutter Radius Compensation - G40, G41, and G42
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.
The behavior of the machining center when cutter radius compensation is on is described in Appendix B.
3.5.11 Tool Length Offsets - G43 and G49
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.
To use no tool length offset, program G49.
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.
3.5.12 Move in Absolute Coordinates - G53
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).
See Section 3.2.2 for an overview of coordinate systems.
3.5.13 Select Coordinate System - G54 to G59.3
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).
See Section 3.2.2 for an overview of coordinate systems.
3.5.14 Set Path Control Mode - G61, G61.1, and G64
Program G61 to put the machining center into exact path mode, G61.1 for exact stop mode, or G64 for continuous mode. It is OK to program for the mode that is already active. See Section 2.1.2.16 for a discussion of these modes.
3.5.15 Cancel Modal Motion - G80
Program G80 to ensure no axis motion will occur. It is an error if:
· Axis words are programmed when G80 is active, unless a modal group 0 G code is programmed which uses axis words.
3.5.16 Canned Cycles - G81 to G89
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 3.5.20
When the XY plane is active, the Z number is sticky, and it is an error if:
When the XZ plane is active, the Y number is sticky, and it is an error if:
When the YZ plane is active, the X number is sticky, and it is an error if:
3.5.16.1 Preliminary and In-Between Motion
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:
- 1. a straight traverse parallel to the XY-plane to the given XY-position,
- 2. a straight traverse of the Z-axis only to the R position, if it is not already at the R position.
If the XZ or YZ plane is active, the preliminary and in-between motions are analogous.
3.5.16.2 G81 Cycle
The G81 cycle is intended for drilling. Program G81 X- Y- Z- A- B- C- R- L-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Retract the Z-axis at traverse rate to clear Z.
Example 1. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the following line of NC code is interpreted.
This calls for absolute distance mode (G90) and OLD_Z retract mode (G98) and calls for the G81 drilling cycle to be performed once. The X number and X position are 4. The Y number and Y position are 5. The Z number and Z position are 1.5. The R number and clear Z are 2.8. Old Z is 3. The following moves take place.
- 1. a traverse parallel to the XY-plane to (4,5,3)
- 2. a traverse parallel to the Z-axis to (4,5,2.8)
- 3. a feed parallel to the Z-axis to (4,5,1.5)
- 4. a traverse parallel to the Z-axis to (4,5,3)
Example 2. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the following line of NC code is interpreted.
G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3
This calls for incremental distance mode (G91) and OLD_Z retract mode (G98) and calls for the G81 drilling cycle to be repeated three times. The X number is 4, the Y number is 5, the Z number is -0.6 and the R number is 1.8. The initial X position is 5 (=1+4), the initial Y position is 7 (=2+5), the clear Z position is 4.8 (=1.8+3), and the Z position is 4.2 (=4.8-0.6). Old Z is 3.
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.
- 1. a traverse parallel to the XY-plane to (5,7,4.8)
- 2. a feed parallel to the Z-axis to (5,7, 4.2)
- 3. a traverse parallel to the Z-axis to (5,7,4.8)
The second repeat consists of 3 moves. The X position is reset to 9 (=5+4) and the Y position to 12 (=7+5).
- 1. a traverse parallel to the XY-plane to (9,12,4.8)
- 2. a feed parallel to the Z-axis to (9,12, 4.2)
- 3. a traverse parallel to the Z-axis to (9,12,4.8)
The third repeat consists of 3 moves. The X position is reset to 13 (=9+4) and the Y position to 17 (=12+5).
- 1. a traverse parallel to the XY-plane to (13,17,4.8)
- 2. a feed parallel to the Z-axis to (13,17, 4.2)
- 3. a traverse parallel to the Z-axis to (13,17,4.8)
3.5.16.3 G82 Cycle
The G82 cycle is intended for drilling. Program G82 X- Y- Z- A- B- C- R- L- P-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Dwell for the P number of seconds.
- 3. Retract the Z-axis at traverse rate to clear Z.
3.5.16.4 G83 Cycle
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-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate downward by delta or to the Z position, whichever is less deep.
- 2. Rapid back out to the clear_z.
- 3. Rapid back down to the current hole bottom, backed off a bit.
- 4. Repeat steps 1, 2, and 3 until the Z position is reached at step 1.
- 5. Retract the Z-axis at traverse rate to clear Z.
3.5.16.5 G84 Cycle
The G84 cycle is intended for right-hand tapping with a tap tool.
Program G84 X- Y- Z- A- B- C- R- L-
- 0. Preliminary motion, as described above.
- 1. Start speed-feed synchronization.
- 2. Move the Z-axis only at the current feed rate to the Z position.
- 3. Stop the spindle.
- 4. Start the spindle counterclockwise.
- 5. Retract the Z-axis at the current feed rate to clear Z.
- 6. If speed-feed synch was not on before the cycle started, stop it.
- 7. Stop the spindle.
- 8. Start the spindle clockwise.
The spindle must be turning clockwise before this cycle is used. It is an error if:
With this cycle, the programmer must be sure to program the speed and feed in the correct proportion to match the pitch of threads being made. The relationship is that the spindle speed equals the feed rate times the pitch (in threads per length unit). For example, if the pitch is 2 threads per millimeter, the active length units are millimeters, and the feed rate has been set with the command F150, then the speed should be set with the command S300, since 150 x 2 = 300.
If the feed and speed override switches are enabled and not set at 100%, the one set at the lower setting will take effect. The speed and feed rates will still be synchronized.
3.5.16.6 G85 Cycle
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-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Retract the Z-axis at the current feed rate to clear Z.
3.5.16.7 G86 Cycle
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-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Dwell for the P number of seconds.
- 3. Stop the spindle turning.
- 4. Retract the Z-axis at traverse rate to clear Z.
- 5. Restart the spindle in the direction it was going.
The spindle must be turning before this cycle is used. It is an error if:
3.5.16.8 G87 Cycle
The G87 cycle is intended for back boring.
Program G87 X- Y- Z- A- B- C- R- L- I- J- K-The situation, as shown in Figure 1, is that you have a through hole and you want to counterbore the bottom of hole. To do this you put an L-shaped tool in the spindle with a cutting surface on the UPPER side of its base. You stick it carefully through the hole when it is not spinning and is oriented so it fits through the hole, then you move it so the stem of the L is on the axis of the hole, start the spindle, and feed the tool upward to make the counterbore. Then you stop the tool, get it out of the hole, and restart it.
This cycle uses I and J numbers to indicate the position for inserting and removing the tool. I and J will always be increments from the X position and the Y position, regardless of the distance mode setting. This cycle also uses a K number to specify the position along the Z-axis of the controlled point top of the counterbore. The K number is a Z-value in the current coordinate system in absolute distance mode, and an increment (from the Z position) in incremental distance mode.
- 0. Preliminary motion, as described above.
- 1. Move at traverse rate parallel to the XY-plane to the point indicated by I and J.
- 2. Stop the spindle in a specific orientation.
- 3. Move the Z-axis only at traverse rate downward to the Z position.
- 4. Move at traverse rate parallel to the XY-plane to the X,Y location.
- 5. Start the spindle in the direction it was going before.
- 6. Move the Z-axis only at the given feed rate upward to the position indicated by K.
- 7. Move the Z-axis only at the given feed rate back down to the Z position.
- 8. Stop the spindle in the same orientation as before.
- 9. Move at traverse rate parallel to the XY-plane to the point indicated by I and J.
- 10. Move the Z-axis only at traverse rate to the clear Z.
- 11. Move at traverse rate parallel to the XY-plane to the specified X,Y location.
- 12. Restart the spindle in the direction it was going before.
When programming this cycle, the I and J numbers must be chosen so that when the tool is stopped in an oriented position, it will fit through the hole. Because different cutters are made differently, it may take some analysis and/or experimentation to determine appropriate values for I and J.
3.5.16.9 G88 Cycle
The G88 cycle is intended for boring. This cycle uses a P word, where P specifies the number of seconds to dwell. Program G88 X- Y- Z- A- B- C- R- L- P-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Dwell for the P number of seconds.
- 3. Stop the spindle turning.
- 4. Stop the program so the operator can retract the spindle manually.
- 5. Restart the spindle in the direction it was going.
3.5.16.10 G89 Cycle
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-
- 0. Preliminary motion, as described above.
- 1. Move the Z-axis only at the current feed rate to the Z position.
- 2. Dwell for the P number of seconds.
- 3. Retract the Z-axis at the current feed rate to clear Z.
3.5.17 Set Distance Mode - G90 and G91
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 3.5.
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 3.5.16.8), where the meaning changes with distance mode.
3.5.18 Coordinate System Offsets - G92, G92.1, G92.2, G92.3
See Section 3.2.2 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:
When G92 is executed, the origin of the currently active coordinate system moves. To do this, origin offsets are calculated so that the coordinates of the current point with respect to the moved origin are as specified on the line containing the G92. In addition, parameters 5211 to 5216 are set to the X, Y, Z, A, B, and C-axis offsets. The offset for an axis is the amount the origin must be moved so that the coordinate of the controlled point on the axis has the specified value.
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.
3.5.19 Set Feed Rate Mode - G93 and G94
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 (no, not that F word; we mean feedrate) 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:
· inverse time feed rate mode is active and a line with G1, G2, or G3 (explicitly or implicitly) does not have an F word.
3.5.20 Set Canned Cycle Return Level - G98 and G99
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.
3.6 Input M Codes
M codes of the RS274/NGC language are shown in Table 7.
3.6.1 Program Stopping and Ending - M0, M1, M2, M30, M60
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.
- 1. Axis offsets are set to zero (like G92.2) and origin offsets are set to the default (like G54).
- 2. Selected plane is set to CANON_PLANE_XY (like G17).
- 3. Distance mode is set to MODE_ABSOLUTE (like G90).
- 4. Feed rate mode is set to UNITS_PER_MINUTE (like G94).
- 5. Feed and speed overrides are set to ON (like M48).
- 6. Cutter compensation is turned off (like G40).
- 7. The spindle is stopped (like M5).
- 8. The current motion mode is set to G_1 (like G1).
- 9. Coolant is turned off (like M9).
No more lines of code in an RS274/NGC file will be executed after the M2 or M30 command is executed. Pressing cycle start will start the program back at the beginning of the file.
3.6.2 Spindle Control - M3, M4, M5
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.
3.6.3 Tool Change - M6
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 3.7.3), program M6. When the tool change is complete:
· The tool that was selected (by a T word on the same line or on any line after the previous tool change) will be in the spindle. The T number is an integer giving the changer slot of the tool (not its id).
· If the selected tool was not in the spindle before the tool change, the tool that was in the spindle (if there was one) will be in its changer slot.
· The coordinate axes will be stopped in the same absolute position they were in before the tool change (but the spindle may be re-oriented).
· No other changes will be made. For example, coolant will continue to flow during the tool change unless it has been turned off by an M9.
The tool change may include axis motion while it is in progress. It is OK (but not useful) to program a change to the tool already in the spindle. It is OK if there is no tool in the selected slot; in that case, the spindle will be empty after the tool change. If slot zero was last selected, there will definitely be no tool in the spindle after a tool change.
3.6.4 Coolant Control - M7, M8, M9
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.
3.6.5 Override Control - M48 and M49
To enable the speed and feed override switches, program M48. To disable both switches, program M49. See Section 2.2.1 for more details. It is OK to enable or disable the switches when they are already enabled or disabled.
3.7 Other Input Codes
3.7.1 Set Feed Rate - F
To set the feed rate, program F- . The application of the feed rate is as described in Section 2.1.2.5, unless inverse time feed rate mode is in effect, in which case the feed rate is as described in Section 3.5.19.
3.7.2 Set Spindle Speed - S
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:
As described in Section 3.5.16.5, if a G84 (tapping) canned cycle is active and the feed and speed override switches are enabled, the one set at the lower setting will take effect. The speed and feed rates will still be synchronized. In this case, the speed may differ from what is programmed, even if the speed override switch is set at 100%.
3.7.3 Select Tool - T
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 3.6.3). 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:
On some machines, the carousel will move when a T word is programmed, at the same time machining is occurring. On such machines, programming the T word several lines before a tool change will save time. A common programming practice for such machines is to put the T word for the next tool to be used on the line after a tool change. This maximizes the time available for the carousel to move.
3.8 Order of Execution
The order of execution of items on a line is critical to safe and effective machine operation. Items are executed in the order shown in Table 8 if they occur on the same line.
| |
|
|
|
