APPLICATIONS SUPPORT

User Manuals

Drill Fundamentals

Drill Parameter

Part Programs

Unix Help For UCS

Machine Setup Commands

MANUALS

Keyboard commands

This chapter describes the various CNC-7 keyboard commands whose functions are not available through the touchscreen. Commands which are available through the touchscreen are described in the definition of the button. You can look up the keyboard command by name in the index, located at the rear of this manual. Keyboard commands are supported in the CNC-7 for a variety of reasons. First of all, to retain compatibility with the CNC-6 keyboard commands. A trained CNC-6 operator can begin operating a CNC-7 almost immediately BECAUSE he can use virtually all of the CNC-6 keyboard commands on the CNC-7. He will find after a short time, however, that the touchscreen is must easier for many functions. There also may be certain functions you perform often (due to your particular application) which make it easier to use particular keyboard commands from time to time than to use the touchscreen menus. The keyboard command line is located in the lower left-hand corner of the display. This command line consists of two parts, the command line and the message line. When you begin typing, the command line will appear, using the current operator's name as a prompt. The letters you are typing appear after the prompt. During the time you are entering a command, notice that the screen continues to update as items change in the system, for example, XY coordinates, hit counters, or tool data. You can also use buttons to execute other functions or even change pages while you are entering the command, and the command line will remain displayed. This is a unique function of the CNC-7. When you press RETURN, the command will be executed. If there is a problem, the command line stays displayed, and the message appears on the next line of the display. The command and message lines will remain displayed until you change pages, or start entering a new command.

spcfunc

Special keyboard functions

The keyboard command system of the CNC-7 includes some other unique features which make use of commands simpler. These functions are described in the following sections. They will normally be used by intermediate to advanced users of the system.

Command queue

The system contains a command queue, which holds up to 20 commands. Pressing the "up" arrow will cause the previous command to be displayed. Pressing "up" again displays the one before that, etc, until the queue wraps around. The down arrow will take you back to the next command after the current one. Let's say that you were doing a test, and commanding the table to move between two corners (e.g.: J,XY followed by J,X18Y24 followed by J,XY followed by...). Instead of typing the commands in over and over again, you could simply enter the two commands the first time, and then on the third command, simply hit the "up" arrow twice (re-displaying J,XY), and then hit RETURN. The fourth command could be entered the same way, "up" arrow twice, and then RETURN.

Command line editing

The DELETE key is used to delete characters which are to the left of the cursor. The left and write arrow keys are used for line editing. The left arrow will move the cursor backward in the command WITHOUT ERASING. You can then type new characters over the old data to replace it. The right arrow moves you to the right in the command. You do NOT have to move the cursor to the end of the line before pressing RETURN, the system will use all characters on the line unless you erase them. Let's say that you typed a command which read METRIC,000/00,TZ. This command contains a typo, in that the "/" should be a ".", and the system will complain and give you a message. You now have three choices, you can give up, you can reenter the whole command, or you can press the "up" arrow to re-display the line, press the left arrow five times until the cursor is to the immediate right of the "/", press DELETE to delete the "/" character, then press "." to enter the correction and press RETURN.

Last page toggle

The ESCAPE key is used to toggle between the last two displayed pages. For example, if you're working on the TMS and Tool and Router pages, and need to work back and forth between them, going through the Machine Setup page would be a waste of time after about the third time. To resolve this, the system keeps track of the last TWO page displays (excluding the Front Page). Pressing ESCAPE allows the system to toggle between the last two page displays. e.g.: on the first press, ESCAPE will display the TMS page, on the second press will display the Tool and Router display, on the third press the TMS page... Also, if you go to a page and then return to the Front Page, ESCAPE will take you right back to the page. This function can be very useful for more advanced operators - give it a try after you're more familiar with the basic system.

Page presets

Function keys

The CNC-7 keyboard allows you to preset the function keys of the system to specific page displays. This works much like the preset button on a car's radio. To use this function, simply go to a page you wish to preset, then press and hold the function key to be assigned to this page. When you let go (after about 2 seconds), the console will "beep" to let you know that the button has been preset. You can continue with this to set other pages you want preset. Whenever you press a function key which has been previously preset, the page display will change to that page. You can use this feature to set up a series of screens that you want your operator to look through in verifying automatic setup, or to guide him through pages during manual setup.

Automatic feeds and speeds

AFS,on/off

This command is included only for compatibility with part programs from CNC-4 and earlier systems, and is ignored by CNC-5 and later control systems, since all feeds and speeds are "automatic".
See also: TP
Keyboard command: AFS,on/off

Routing related commands

The following commands are used to assist in the setup of the machine for routing, primarily from the M48 header. These commands are special functions beyond the basic functioning of the Routing software which allow you to calibrate and further customize the Routing machine setup. This section describes commands with functions such as Calibrating the table velocity for Routing, and setting the Table Feedrate override percentage.

BOARD_SENSOR command

BOARD_SENSOR,on/off

This command will disable the board sensor feature when the autoload machine operates in manual mode. This command is for maintenance purpose. NOTE: Use this command only when you operate the machine in some unusual situation. When the machine is powered up, it will go back to default value that means board sensor function is on.
Format: BOARD_SENSOR,on/off

Calibrate table velocity for routing

CALV

This command is used to calibrate the table velocity used in routing. When you enter this command, the table will move to the zero corner, and then travel diagonally from one corner of the table to another. During these moves, it will change speed several times, and will display the velocity variance detected as the calibration progresses. The message is displayed in the machine status box. The calibration will stop after five complete passes (back and forth), or if the velocity variance exceeds 25%. Routing systems will request a table calibration in the machine status box until one is performed, which includes the initial load, or after installation of new software. A CALV will also be requested after calibrating the tachometer for the X or Y axes. Although CALV is not required, it is highly recommended to improve the accuracy of routing moves.
Keyboard command: CALV

Radius Adjustment Band

RAD command

This command is used to set the 180 degree arc radius adjustment band. The band is used to adjust for minor part program errors or NC system round-off errors that may occur while performing routing calculations. The adjustment band handles cases where a 180 degree arc is programmed using the G02/G03 commands, but the calculated distance between the beginning and end points results in an arc slightly less than 180 degrees. If uncompensated, this results in a flatter arc than desired. The default band is set to .0015 inches. This means that if half the distance between the beginning and end points is less than the radius within .0015", the radius is automatically adjusted to rout a 180 degree arc. The command may be used to increase or decrease the band as desired. A smaller band may be needed in cases where a 180 degree arc is programmed, but after applying cutter compensation the actual position of the cutter at the beginning of arc is less than 180 degrees from the end point. In this case too large a band could result in the arc radius being adjusted when it should not be, resulting in an elongated arc. The RAD command parameter specifies the size of the adjustment band. Entering the command without a parameter causes the current setting to be displayed inside the 10-key popup window, where it may be changed if desired. The RAD command may be added to the MACH.DAT file, or it may be included in the M48 header or set-up files.
Keyboard command: RAD,#

Table Feedrate override percentage

TBFR

This command is used to set up the Table Feedrate Override Percentage used to override the programmed or default table feedrates. This command has the effect of adjusting the Feedrate value displayed on the Manual Operations page which also affects JOG. A common use of this command is to add it to the M48 header to assure that a leftover adjustment of the Table Feedrate by a previous operator will not impact the routing table feedrates. This command can be used from the Keyboard, or from the MACH.DAT file, Login file, or M48 header. The provided value may range between 1% and 150%.
Keyboard command: TBFR,#

Returning to NC mode

NC

This command returns the system to NC mode. NC mode (and it's displays) are exited when the system is put into Maintenance or Programmer modes. Entering the command (or pushing a button if applicable) will result in a "please wait" message while the system loads the NC system screen definitions in from disk. Once loaded, the Front page of the NC system will be displayed.
See also: MAINT, PROG
Keyboard command: NC

Safety hood override

HOOD,on/off

This command is used to do a one time override of the Safety hood (if the machine is so equipped). Entering the command "HOOD,OFF" will allow the system to override ONE opening of the Safety hood. This is intended for use primarily during servicing or troubleshooting of the machine. After entering this command, you will get an "Are You Sure?" popup to make sure that this is really what you wanted to do. The override command will NOT override restrictions on the START button. The START button can ONLY be used when the hood is closed. Otherwise, once this command has been entered, the machine can be operated with the hood open until it is closed again. As soon as the hood is closed, the hood is re-enabled, and opening it will again stop the machine. If you wish to further restrict use of this command, you can change the operator access privileges for this command in the COMMANDS.TAB file.
Keyboard command: HOOD,on/off

Override table clamps

OTCLMP,on/off

This command overrides the table clamps (if turned on) so that the machine may be run with the clamps open. Normally, open table clamps will inhibit the part program from being started, although table movements in non automatic mode (such as PARK and JOG) are allowed. Turning OTCLMP off again will restore the systems normal operation, inhibiting the START button until the clamps are closed. This command may be useful in special circumstances, such as pneumatic or sensor problems with clamps that would otherwise take the machine out of production.
Keyboard command: OTCLMP,on/off

Purge Broken Tool Detector

PURG,on/off

This command is included only for compatibility with part programs from CNC-6 and earlier systems, and is ignored by the CNC-7, which does not come equipped with optical Broken Tool Detector systems.
See also: TSI
Keyboard command: PURG,on/off

Confidence Check enable/disable

TSI Confidence Check enable/disable

RCHK,on/off

This command enables the Confidence Check, which causes picked up tools to be compared with a previous history of tools of the same size. If the tool "looks" to TSI like the same tool, it is assumed good. If not, it is indicated as bad before the first hole is drilled. The Confidence Check in the CNC-7 defaults to ON. This command should be used only on machines equipped with Microwave Tool Detectors. This command may be placed into the MACH.DAT file.
See also: DETECT, LTBL
Keyboard command: RCHK,on/off

Reset Diameter page

R,DIAP

This command is used to clear the Diameter Page from memory. The diameter page is the page which contains feeds, speeds, retract rates, max hit counts, and Z-axis offsets for various tool sizes. After the Diameter page has been cleared, attempting to display it will result in a message. Entering tool diameters (from the console or part program) will not result in any access to any diameter table.
See also: DIAP
Keyboard command: R,DIAP

Reset Excellon Frequency Converter

R,EXFC

This command is used to reset the Excellon Frequency Converter after a trip. If the converter trips due to a fault or other failure, this command must be issued from the system console in order to reset the converter for further use. In the case of a trip, the CNC-7 will display a message in the machine status box telling you to wait for the spindles to stop, and then to execute this command.
See also: R
Keyboard command: R,EXFC

Reset button disable

RSB,on/off

This command is included only for compatibility with part programs from CNC-6 systems, and is ignored by CNC-7 systems, since the CNC-7 does not display the Reset button while the machine is running, which is what the RSB command was intended to protect against in the CNC-6.
See also: R
Keyboard command: RSB,on/off

Spindle Group Select

SG,on/off

SG,group#,#,#...

This command allows you to enable and to set up spindle group mode, in which six spindle groups replace the spindle select buttons. These groups may contain up to six spindles each. All spindles of a group are selected simultaneously when the spindle select button is used, all spindles of any other group are automatically deselected. Spindle group mode enables the M96 part program code, which can be used to select and deselect spindles during the part program. This is useful when drilling a large board on more than one station. The SG,on/off form of the command enables and disables spindle group mode. The SG,group#,#,#... form of the command is used to define the spindles assigned to a particular group numbers. Both forms of the SG command may be included in the M48 header or the MACH.DAT file.
See also: M96, SETSP, Spindle select
Keyboard command: SG,on/off or SG,group#,#,#,#

TMS group diameter declaration

DIAM,diam,#,#,#...

This command is used to declare the diameters of the given groups. The first parameter if the tool diameter, all other parameters beginning with the second are group numbers to be set to the specified diameter. The DIAM command is only useful in TMS Mode 2, and is typically included in an M48 header to define the layout of the cassette. This gives the part program (via the header) complete control over which tool sizes are loaded into which groups, which can vary greatly from job to job (number of tools of a particular size required). Please note that in TMS mode 2, tool groups of the same tool size are automatically "linked" such that one expired tool group will cause the next tool of the same size to be picked up in the next group of the same tool size.
See also: TMS, MODE
Keyboard command: DIAM,diam,#,#,#...

Diameter Dwell

DIAMDWELL

This command is used to specify a dwell time for a range of tool diameters. For tool sizes that fall within the specified range, the machine will delay an additional amount of time beyond the normal worktable dwell time before performing a drill stroke. Although a standard worktable dwell time has been established at the factory for each machine type, it may be desirable to alter the dwell time to fine tune a particular machine. For example, a dwell time may be established (refer to the DWELL keyboard command) to achieve the maximum hit rate for larger sized tools. To accommodate the smaller tool sizes, the DIAMDWELL command may be used to specify additional settling time before the drill stroke. Each DIAMDWELL command specifies a tool diameter range and a dwell time. The first and second parameters specify the minimum and maximum diameters defining the range, the third parameter is the dwell time in milliseconds. Multiple commands may be entered to specify up to ten diameter ranges and dwell times as in the following example:
DIAMDWELL,.000,.009,24 DIAMDWELL,.009,.020,16 DIAMDWELL,.020,.030,8 The dwell table display keyboard command DTBL may be used to view the current settings (refer to the DTBL keyboard command description).
Please note the following conventions: Entering a diameter range clears all higher diameter ranges. Multiple diameter ranges must therefore be entered from smallest to largest range. The maximum diameter of the previous range is automatically set to the minimum diameter of the range presently being entered. This insures there are no unintentional gaps in the range specification and also insures ranges do not overlap one another. The drilling machine searches the diameter table for the current tool size beginning with the smallest diameter range. In the above example, a .020 diameter tool will use the 16 msec dwell value. To avoid ambiguity the range boundary could be set at an unused diameter.
See also: DTBL, DWELL
Keyboard command: DIAMDWELL,mindiam,maxdiam,dwell

Display Diameter Dwell data table

DTBL

This command is used to display the Diameter Dwell data table. The table provides a method to establish different worktable settling times before each drill stroke based upon the tool diameter. Values are inserted into the table using the diameter dwell keyboard command DIAMDWELL (refer to the DIAMDWELL keyboard command description). Each line of the display consists of a minimum and maximum diameter, and a dwell time in milliseconds. For tool sizes that fall within the minimum/maximum diameter range, the machine will delay an additional amount of time beyond the normal worktable dwell time before performing a drill stroke. The table allows up to ten diameter ranges and dwell times to be specified. Table entries for which no diameter or dwell have been given contain zero. The table is displayed via the Display program (same as that used during HELP or TYP).
See also: DIAMDWELL, DWELL
Keyboard command: DTBL

Operator ID command

OPID,idstring

This command is used to enter an operator ID string which will be used to replace asterisk characters ("*") found in M97 or M98 part program codes. The OPID string is displayed on the Options and Switches page, so that the string can be checked. This string replaces the "*" character in an M97, M98 part program command, and is usually used to drill an operator's ID (initials, employee number, etc) into a corner of the board. See also: M97, OPSP
Keyboard command: OPID,idstring

DNC related commands

The following commands are used to control the DNC system (DNC-1.3). These commands are special functions beyond the basic functioning of the DNC device which allows you to transfer files between this machine and another machine. This section describes commands with functions such as sending a message to a remote host, sending a control command to the host, or resetting the DNC system on this machine.

Operator message

OM,message

This command is used to send an operator message to a remote host. If the machine is connected to a FileServer or DataWorkshop, the OM command will send the message via the DNC-1.3 system to the remote host for display on that system.
See also: DNC chapter
Keyboard command: OM,message

Remote control command

CTRL,command

This command is used to send a command to a remote host system to be executed on that system. For example, you may want to send a directory command to the host to get that system to take a directory of a portion of it's disk, and then write it to a file. You could then transfer the file back from the host to your own system using a standard COPY function. It is important to remember that the specified command will be executed on the host system, not on your own, so you should avoid commands which would require direct operator input, such as editors or other commands doing operator prompting.
See also: DNC chapter
Keyboard command: CTRL,command

Reset DNC

R,DNC

This command is used to reset the DNC of the local machine. This is useful where problems (hardware, software, application) might cause the DNC system to get "stuck". The R,DNC command will cause all of the software and related hardware to be reset and will generally recover from whatever the problem might be. Note that this command is a way to get out of a problem, and should not ever be necessary under normal circumstances.
See also: DNC chapter
Keyboard command: R,DNC

Paper tape related commands

The following commands are used to control the paper tape system. These commands are special functions beyond the basic functioning of the Paper tape devices which allow you to read and punch paper tape. This section describes commands with functions such as turning the paper tape reader parity on and off, selecting the code type (EIA or ASCII) for data sent to the punch, tape feed, man readable header, and tape duplication.

Paper tape parity

PAR,on/off

This command is used to turn the parity of the paper tape reader on or off. Normal operation of the system is to have the parity of the system turned on, which allows the reader software to detect most data errors, and allows the system to automatically tell the difference between EIA and ASCII tape. However, some CAM systems which generate paper tapes create different forms of non-parity ASCII, which may have the parity bit on or off, depending on how that system is set up. PAR,OFF allows the tapes to be read, ignoring the parity track. Although this allows the tapes to be read, it also increases the possibilities that an error will happen and not be detected by the parity check (which wouldn't be done).
See also: COPY, CT
Keyboard command: PAR,on/off

Printer control commands

The following commands are used to control the printer system. These commands are special functions beyond the basic functioning of the printer device which allows you to print files. This section describes commands with functions such as listing the printer queue to see what print jobs are pending, and to delete print jobs from the queue.

Printer queue

LPQ

LPQ displays the status of the printer queue, indicating which jobs are in the printer queue, in which order, and their size. For each job in the queue, the following information is given: User, Print device, Job ID, Size, Status, Filename.
See also: PRINT, LPRM
Keyboard command: LPQ

Printer job delete

LPRM

LPRM allows you to remove a print job from the printer queue. When you type LPRM, the system will list for you all available print jobs, one at a time, and ask you if you want to remove that job from the queue. Answering "y" or "Y" will remove that print job.
See also: PRINT, LPQ
Keyboard command: LPRM

Display TSI data table

LTBL

This command is used to display the TSI data table, which will indicate the normal readings for all of the tool diameters known by the CNC-7 for each spindle. This table is consulted when a tool is picked up to see if the TSI reading for the new tool is within a normal range for tools of that size. The table is displayed in a multiple column display, with the tool diameter indicated first, followed by the stored readings for each spindle. If there is no reading for a particular spindle, the entry for that spindle will be blank. The display is sorted by diameter, and displayed via the Display program (same as that used during HELP or TYP). Table entries are created the first time that a tool of a particular size is picked up. Only the readings from selected spindles are entered or updated. The table is continuously updated as tools are picked up, with new readings incorporated using a moving average method. This makes the system less sensitive to minor normal variations of the hardware. This table is affected also by the commands ROVR, RTBL, RDIA, and RSPN. This command should be used only on machines equipped with Microwave Tool Detectors.
See also: ROVR, RTBL, RSPN, RDIA
Keyboard command: LTBL

Log a message manually to the log files

LOG,message

This command is used to log any explanatory message to the CONSOLE and STATS log files. The command can be used to log comments explaining some of the conditions recorded by the machine. It can also be used to record other significant events, such as taking the machine down for preventive maintenance.
See also: Using the System Log files
Keyboard command: LOG,message

Commands File Processor

This command provides a fast and convenient way to execute system commands which otherwise would require lengthy and time consuming keyboard typing. It is especially useful in those cases where a sequence of many commands needs to be entered into the machine on a periodic basis, for example during job set up. Another common case of issuing many commands is after a new user logs into the machine and he needs to configure it to fit his particular work requirements. It is for this reason that the system, as part of the logging procedure, automatically looks for a commands file and if found, executes it (See Logging into the CNC-7 for a detailed explanation) every time a new user logs in. A commands file is simply another file similar to a part-program file that instead contains command lines to be executed by the system. The syntax of these lines is the same as if they were to be typed from the console keyboard. Only one command is allowed per line. Also, some special characters and keywords are supported to indicate the Commands Processor to handle some functions specific to it. They are explained below.

Comments

Comment lines are permitted as long as they start with a semicolon. All text after the semicolon is ignored. No comments allowed in the same line as the one that has the command itself.

Keywords

Keywords are not commands to the drilling system but to the commands processor itself. They tell it how to interface with the operator and also execute some functions of its own. These keywords are always preceded by a dot, like in .QUIET . This dot must be at the beginning of the line in the first column. keywords followed by text, such as CALL, ASK, etc. must have a space between the keyword itself and the subsequent text. Keywords currently supported are:
QUIET - Tells the processor not to display on the screen the commands as they are executed. Any messages returned by the system will not by displayed either. This is the default mode.
NOQUIET - It is the opposite of QUIET. When found, this keyword will force the screen to be cleared and all following commands printed as they are processed along with possible messages.
POPUP - Tells the processor to display on the screen the popup windows that prompt the operator to confirm or reject a command execution. This is the case with commands such as ZEXT, disk initialization etc, which due to their nature require the user to be sure of what it is being done in order to prevent irreversible changes. However, while this is a necessary safeguard for commands started from keyboard or a button, it may not be convenient when the same command is initiated from a commands file. Therefore, by default these popups are not displayed and the specified command is executed avoiding the dialog with the operator. In those cases where popups are still desired, the use of this keyword will force the commands file to interrupt execution and wait for user confirmation.
NOPOPUP - This is just the opposite from the previous keyword POPUP. After this keyword is found, commands that normally display a confirmation popup will no longer do so, but instead execute the command directly. This is the default set, so unless POPUP is included in a file, popups will not be displayed.
DELAY - This causes the processor to delay execution of the following commands by an amount of time equal to the number that follows it. For example the line .DELAY 1000 indicates the processor to wait one second before continuing execution. Note that the time is specified in milliseconds, with allowed ranges from 1 millisecond to 30 seconds. Values out of range will be ignored.
PRINT "text" - With this, a line of text may be printed on the screen. Please note that "text" may be entered in any supported language, including Kanji, Korean, etc.
ASK "text" - This keyword will cause the system to print "text" on the screen and then wait for the operator to hit a key in response to it. This response (only one character) may be any key; but only "Y" (yes) or "N" (no) are interpreted by the commands "IFYES" and "IFNO". "text" may also be in any supported language including Kanji characters, Korean, etc.
IFYES "text" - This will look at the keyboard answer entered in response to the previous keyword ASK. If it was "Y" (yes), "text" is executed. Here "text" must be either a drilling system command, or another keyword. This keyword does not necessarily have to follow an ASK. Rather it may be placed later on in the file after any number of lines. The answer entered in response to ASK is saved until a following IFYES or IFNO is satisfied, at which point it is destroyed. This means that an answer requested while executing a called macro (see CALL) may be returned back to the caller.
IFNO "text" - Operation of this keyword is similar to IFYES except that "text" is executed when the response from ASK is "N" (no).
REPLACE %# "text" - This keyword allows for variable substitution. During execution, upon finding a 'replace' key, "text" will be displayed on the screen and the system will wait for the operator's keyboard entry, which will be saved into the variable number that follows the symbol '%'. The variable number may be any one digit number from 0 (zero) thru 9 (nine). Any subsequent occurrence of '%#' will cause the symbol '%' and variable number to be substituted by the previous operator's entry.
CALL "text" - When this keyword is found, another macro is called for immediate execution. After the called file completes, the caller macro resumes execution with the next line in the file. The called macro's name and directory is indicated by "text".
CLS - This will cause the screen to be cleared.
This is a simple commands file with a description of every line:
; Test file This is a comment line .QUIET Do not display executed commands atc,off Turn automatic tool change off dn,.5 Set lower limit fsb,on Enable feeds and speeds log,This is a test Log text into log files r Reset machine .delay 2000 Halt execution 2 seconds .ask Do you want to enable Diameter Check (Y/N): Ask user .ifyes dchk,on Turn diameter check on .ifno dchk,off Turn diameter check off .cls Clear the screen .replace %0 Enter cassette file name Variable substitution cas,%0.cas .ask Execute "Login check list"? Ask user .ifyes .call /usr/data/check.cmd Call next command file .print End of this commands file Print text on the screen
Besides the usual application of command files as a way to execute many commands contained in one file by simply calling the file's name, they also provide a convenient mean to run a machine/operator dialog to ensure that certain operations are done at predefined states like before or after a job run, upon user login, etc. For instance, after a new user logs in, the system looks for a commands file with the same name as the user name. In this file, or another file called from this one, an entire sequence of questions and reminders may be executed with the help of the macro keywords CALL, ASK, IFYES, IFNO, PRINT and CLS.
A portion of a file of this kind would look similar to this:
; User login check list macro .cls .print LOGIN CHECK LIST .print .ask Is the work table clean? .ifyes log,Table was clean .ifno .print Clean the table .print Check spindle's collets for any tools . . . .
See also: Logging Into the CNC-7
Keyboard command format: @filename

End of Program Command file

The system allows for a command file to be executed automatically at End of Program. This is intended as an automatic way to return the system to a known state, so that M48 headers or operator setup need only deal with things different from normal. For example, if you are using soft tooling, and are often switching between drilling of tooling holes and drilling of product, you may find yourself turning the Extended Z-axis mode on and off a lot. It may be desirable to have Extended Z-axis mode turned OFF at the End of Program so that you're sure it's off before setting up the next job. To do this, you create a file in the SYSTEM directory called ENDOFPROGRAM. This file is a command file (please see Commands File Processor section), and may contain any valid commands. In this case, the file might contain only one command, ZEXT,OFF. Whenever the machine reaches End of Program, it will look for the existence of this file. If it exists, it will be executed. Notes:
1) The decision of whether or not to execute the ENDOFPROGRAM command file is made when the program is loaded, so if you create it after the program has been loaded, the ENDOFPROGRAM command file will be ignored until the program is cleared from memory.
2) The Commands File Processor will execute all commands in the file, and will not abort if there are problems. Problems are not reported, because it is assumed that the command file has already been tested. To test the command file, add a ".NOQUIET" line to the top of the file, and then execute it by entering the keyboard command "@/cnc/data/ENDOFPROGRAM" - each command and any messages will display on the screen as they are encountered. BE SURE TO REMOVE THE ".NOQUIET" FROM THE FILE WHEN TESTING IS COMPLETE.
See also: Commands File Processor, Logging into the CNC-7

Ethernet related commands

The following commands are used to provide access to more advanced Ethernet functions. These commands are special functions beyond the basic functioning of the Ethernet software, which is fully integrated into the CNC-7 human interface. This section describes commands such as remote login, remote copy, and remote shell. In order to use any of the commands in this section, the machine and software must be equipped with the Ethernet option.

Remote Login

RLOGIN

This command is used to log into a remote system via the Ethernet link. You specify the host to log into, and optionally the user name to use at login time. RLOGIN will take control of the screen, and will not release it until you log out of the remote system, at which point the standard CNC-7 pages will re-display.
See also: DNC chapter (Ethernet)
Keyboard command: RLOGIN host (-l username)

Remote Copy

RCP

This command allows you to copy files between the CNC-7 and a remote system. Protections should be set on the RCP command in /cnc/data/commands.tab, and on the HOSTS and RHOSTS files on both systems. With this command, you specify the hosts at either end (RCP can copy between two remote machines) and the filenames involved. In order for this command to succeed, the HOSTS and RHOSTS files must be correctly set up. The local host name (the CNC-7) should not be specified.
See also: DNC chapter (Ethernet), Setting up Operator Accounts
Keyboard command: RCP (host:)/dir/file (host:)/dir/file

Remote Shell

RSH

This command allows you to execute commands on a remote system without logging into the remote system. Protections should be set on the RSH command in /cnc/data/commands.tab, and on the HOSTS and RHOSTS files on both systems. With this command, you specify the hosts on which to execute the command, optionally the user name under which to execute it, and the command to be executed. In order for this command to succeed, the HOSTS and RHOSTS files must be correctly set up.
See also: DNC chapter (Ethernet), Setting up Operator Accounts
Keyboard command: RSH host (-l username) command

Pecking related keyboard commands

PCKPARAM

The PCKPARAM keyboard command is a quick way to set up several pecking parameters. This command gathers features from the Pecking Depth Button, Pecking Infeed Button and Pecking Retract Button and combines them into a single command for a specific tool. The depth, infeed and retract values of the entered peck step is continued into all subsequent pecks as with other pecking buttons.
Keyboard command: PCKPARAM,toolno,peckno,depth,infeed,retract
See also: PCK_DPTH, PCK_INF, PCK_RET and PCK_TOOL

REMPFT command

REMPFT,on/off

This command indicates to the CNC-7 that the Removable Pressure Feet feature is installed and enabled on the machine. The command can be used by VSB to enable this feature, or by the operator to temporarily enable or disable it. NOTE: Use this command only when the machine is equipped with the required software and hardware. Be sure to check that the large insert is installed before disabling the function. When REMPFT is turned OFF, the system indicates to itself that it does not know which pressure foot is installed. For this reason, when REMPFT is truned back ON, the system will again display the popup requesting the operator to identify which pressure foot insert is currently installed. This command cannot be used when there is a tool in the collet. NOTE: A machine equipped with multiple pressure foot inserts will automatically select the correct insert based upon the diameter of the requested tool. The system will select the large insert if no diameter is specified, OR if the tool being picked up is a router tool. This allows drilling and routing operations to be intermixed within the same part program and still allows fully automatic use of the automatic pressure foot insert changer. This command is normally included in the system software "SYS" file and should not be added to the machine data file. Instead, add the line "W/REMPFT" to the MACH.DAT file. "W/REMPFT" will enable this function and load all required parameters.
Format: REMPFT,on/off

SET command

This command determines the mode of data packing when writing to a ZOS (CNC-6) format diskette. Method of data packing when READING from an existing ZOS disk file is determined by the file itself, no special commands are needed. However, when CREATING a ZOS disk file, there are two primary choices. 1) Data can be written in an unpacked format which can directly be read without further interpretation. This is the default. 2) Data can be packed in a binary format according to the current INCH/METRIC/LZ/TZ setup of the CNC. These INCH/METRIC formats are set using the standard INCH or METRIC commands. Packed format will pack all lines of data containing only an XY coordinate. It takes three bytes to pack a single axis, or six to pack a coordinate pair. In some cases, this can significantly reduce the amount of floppy disk space required to store a part program. However, packed format also has disadvantages in that it can change the original data (e.g. by dropping trailing zeros), and can be confusing if you are switching often between CNC measurement modes. SET,AF will cause the system to create any new ZOS files in unpacked format. This command should ONLY be needed after the system has been operating in packed format, and you wish to return the system to unpacked mode. SET,CF will cause the system to pack data in newly created ZOS disk files according to the CNC's current INCH or METRIC setting.
Format: SET,AF or SET,CF
See also: INCH, METRIC

Tooling Plate Rotation Angle

Single Spindle Machine Tooling Plate alignment

The ROTANGLE keyboard command can be used to rotate all part program coordinates based on an origin, a second point, and an offset measured from the second point. This command is useful to align the tooling plate on either a single spindle machine or on System 1000 stations.
There are two ways to use this command. Entering the ROTANGLE keyboard command followed by six proper parameters will enable the rotate angle feature.
The six parameters are defined as (1) the first point X coordinate nominal position, (2) the first point Y coordinate nominal position, (3) the second point X coordinate nominal position, (4) the second point Y coordinate nominal position, (5) the second point X coordinate offset ( difference from nominal position and actual position ) and (6) the second point Y coordinate offset.
Entering the ROTANGLE keyboard command followed by the parameter ON will turn on the rotate angle feature if it was OFF. A message will be displayed in the machine status box. Entering the ROTANGLE keyboard command followed by the parameter OFF will turn off the rotate angle feature while it is setting ON. The message will be removed from the machine status box.
In order to obtain the above mentioned parameters, the following procedures are suggested in order to measure the last two offset parameters.
Set the machine to version 1 and INCH mode. Prepare a panel with it's size as close to the maximum panel-handling size as possible. For SYSTEM 1000 machines, the panel size is 18x24 .
Prepare panel with proper backup material and insert (size 0.125") registration pins on each end.(top and bottom). Lock this panel in the tooling plate using pin clamp and edge clamps.
Write a part program to drill 16 holes around each of the two registration pins and four other holes on the the back right corner on the stack. All holes should be 0.054 inch diameter.
Zero set machine work zero at the front edge pinning hole. For example, set zero at X10.004Y0.254 while using 0.125" size 1/8 BUSH pins or set zero at X10.191Y0.379 while using SFTPL6 pins, which is the front pin.
The part program should be as follows.
M48 T01C.054F090B0700S43 VER,1 % T01 X-0.15Y0.5 R3Y0.1 X-0.05Y0.8 R3Y-0.1 X0.05Y0.5 R3Y0.1 X0.15Y0.8 R3Y-0.1 X-0.15Y22.5 R3Y-0.1 X-0.05Y22.2 R3Y0.1 X0.05Y22.5 R3Y-0.1 X0.15Y22.2 R3Y0.1 X8.1Y22 X7.9 X8.0Y22.1 Y21.9 M30
After the program has executed and panel is drilled, carefully remove the two registration pins from the stack. Now this panel is ready to be measured on a good measurement machine such as the Zeiss to find out the two offset values.
While doing the measurement, use those two sets of reference points, sixteen points each, to first align the two registration positions and then use these two registration positions to align the Y axis. Assume the front edge pinning hole as the ( 0, 0 ) point, and measure the four actual positions on those four drilled holes close to the ( 8, 22 ) location and then take an average of them.
For example, the calculated average position from the measurement machine for this point might be ( 8.0032 , 22.0019 ). Then the calculated offset will be ( -0.0032, -0.0019 ). The input value to the ROTANGLE keyboard command at this time ( with the work zeros ) will be:
ROTANGLE,0,0,8,22,0.0032,0.0019
The Zeiss can also report to you the actual measured pin position of the desired ( 0,0 ) location base on the sixteen drilled reference points next to it. For example, if the Zeiss measured first pin location is at ( -0.00185, -0.00048 ) then ZERO SET the machine at ( 10.00585, 0.25448 ) while using the 1/8" BUSH pin will align the center of the registration pin locations very close to ( 0, 0 ) . To zero set key in the keyboard command as Z,X10.0059Y00.2545 .
The machine work zero and the coordinate version can be reset at any time after the ROTANGLE command is invoked without impacting the functioning of the rotation angle compensation.
The ROTANGLE keyboard can also be included in the MACH.DAT file after the measurement. In this case, the work zero offset must be added to the first four parameters when the ROTANGLE command in invoked from the MACH.DAT file. For example, the front pin location is at ( 10., 0.25 ), then the ROTANGLE command in the MACH.DAT file will be described as follows:
ROTANGLE,10.0059,0.2545,18.0059,22.2545,0.0032,0.0019
The first four parameters are calculated as follows: 1st parameter = 0 + 10.0040 + 0.0019 = 10.0059 2nd parameter = 0 + 00.2540 + 0.0005 = 0.2545 3rd parameter = 8 + 10.0040 + 0.0019 = 18.0059 4th parameter = 22 + 00.2540 + 0.0005 = 22.2545
Remember, always use VERSION 1 scale and INCH mode to measure the offsets. This will prevent you from entering the offset value sign incorrectly.
Format: ROTANGLE,ON/OFF Format: ROTANGLE,X1,Y1,X2,Y2,X,Y X1 - First Point (Rotate Point) X coordinate position Y1 - First Point (Rotate Point) Y coordinate position X2 - Second Point X coordinate position (Nominal Point) Y2 - Second Point Y coordinate position (Nominal Point) X - Second Point X coordinate offset Y - Second Point Y coordinate offset

learn_cmd

Learn Mode Commands and Files

Learn Mode consists of three keyboard commands which comprise a very powerful mechanism for the "learning" of setup sequences for later recall and reuse by an operator or user at a later date. Learn mode uses thre keyboard commands, LEARN, SAVE, and USE as described further on in this section. Learn Mode operates by recalling sequences of keyboard commands and buttons as stored in the CONSOLE log file. The LEARN command places a marker into the log file which indicates the start of the learn sequence. At the end of the learn sequence, a SAVE command causes the system to extract all relevant commands and buttons from the log file. USE causes the system to recall and replay the learn sequence. The learn sequences are stored in files in the SYSTEM directory. If the command LEARN MLB8 had been used to start the learn session, then when the SAVE command is later used, the system will create and store a learn sequence file in the SYSTEM directory called USE.MLB8. This sequence can be recalled and replayed later with the command USE MLB8. When the learn sequence file is created, all useable keyboard commands and buttons are remembered and stored. There are several functions which the system chooses not to remember, but these are mostly functions which would not be useful or wise to use in the learn sequence anyway. Examples would be buttons which increment and decrement a data value (like a tool number), and functions like HOME, PARK, etc. If commands or buttons contain parameters, the learn sequence will learn and save the parameters. For example, "T,1" will be saved as "T,1". However, if a command or button does not include a required parameter, then just as the original command would cause a popup to get the missing information, the learned sequence will cause a popup when the sequence is replayed. So, "T" would be saved as "T". Commands stored in the learn sequence file will be commented by extracting their HELP title from the corresponding HELP entry. For example, a learn sequence which goes to the Status page, sets NODRILL, and then returns to the Front page will look like this:
; Machine Setup page SP ; No Drill Mode button NODRILL,ON ; System Front page FP
The comments are added only for your convenience should it become necessary for you to fine tune the learn sequence by editing it with the normal EP editor. Finally, although only one learn session may be active at any one time, multiple USE commands may be entered during the learn session, which will execute and therefore remember all commands that result from the USE command. You can therefore create more complex learn sequences by combining USE and other individual commands and buttons.

Learn a New Sequence

LEARN,name

The LEARN command causes the system to enter learn mode and begin saving all entered commands and buttons for later recall. The LEARN command requires on parameter, the name of the learn sequence. This is a portion of a filename, and may be no more than 8 characters in length. The LEARN command causes an entry to be made into the CONSOLE log files, noting the start of the learn sequence, and sent some internal software flags. Other than that, it causes no other action. The commands and buttons that you use during the learn sequence will continue to function in the same manner as normal. The only difference is that they are being recorded as part of the learn sequence as well. Please note that in some cases, you may have to pay attention to the sequence of operation in order for it to be remembered properly. For example, if you want to assure that QuickDrill is turned on, you cannot just ignore it if it is already on. If you ignore it, so will the learn sequence. In order to make sure that QuickDrill is set to the state that you want, turn it OFF and then back ON. The learn sequence will do the exact same thing.

Terminate and Save a Learn Sequence

Save a Learn Sequence

SAVE

When you are all done with the sequence that you want the system to lean, the SAVE command causes the sequence to be processed and saved. After entering SAVE, the system will release the log files, locate the last LEARN command within the CONSOLE log file, extract all useable commands and add comments, and then finally, will give you a chance to edit the learn sequence file that has just been created. If you wish, you may answer YES to this question, and you will be entered into the EP editor to edit and make final modifications on the learn seuqnce file. Please note that at any time you may go back and make further edits to the file - this is just one chance that you get without an extra step. You may wish to add additional comments, delete commands or buttons used by mistake, or perhaps, delete unnecessary actions like turning QuickDrill OFF before turning it ON.

Use a Learn Sequence

USE,name

Finally, in order to recall and replay the learn sequence, enter the command USE followed by the basic name of the learn sequence. If the name of the file created by SAVE was USE.MLB8, then you would enter USE,MLB8. The "USE." prefix simply identifies a learn sequence file. As the commands in the learn sequence file are replayed, the comments will be ignored and the commands will behave exactly as if they had been entered from the keyboard. In fact, they actually echo through the keyboard command line exactly as if they had been entered through the keyboard. This method gives the commands used in the learn sequence a great deal of flexibility. For example, commands can be used which require popups (T, UP, DN), commands which provide all necessary data (T,0, UP,0.125), commands which create popups (TMSGPH, TSUMRY), commands which cause page changes (FP, SP, TP), commands which require file selections (EP, COPY), and commands which require interaction with the user (EP, OP). Learned commands are subject to all of the same protections, restrictions, and error conditions as if the commands were entered directly.

Registration Station Location

Alternate Registration Station Location

Reg. Station location for different size of panel

This command will change the registration station location to load/unload either large or small panel. Type REGPANELSIZE at the command line will popup a panel size selection window on the screen. If there is any need to implement this command in the M48 header or setup file. The command can be invoked by REGPANELSIZE,SMALL or REGPANELSIZE,LARGE which will not cause the popup window to display. The command required the REG-STA-POS-SMALL and REG-STA-POS-LARGE command set up the location in the MACH.DAT file.

MPR popup

Multi Panel Registration Popup

This command will display a popup with all possible panel size defined in the MPR.DAT file. By choosing the desired panel size, it sets up the registration stop pin and it's location during loading operation. This command can also be used the the command file by following the panel size as the second parameter. In this case, the popup will not appear.
Format: MPR Format: MPR,20X18

MPR Stop Pin Operation

Multi Panel Registration Stop Pin Operation

This command will eject any one of the three stop pin up or down. The second parameter is the stop pin listed from left to right. The third parameter ON will eject the stop pin up and OFF will lower the stop pin. At any given time, it allows only one stop pin to eject up and others will automatically lowering down.
Format: MPRPIN,1/2/3,ON/OFF

Double Side & Multilayer Panel Operations

This keyboard command will control the SYSTEM 2000 to switch between drilling Double Side panel and Multilayer panel. This command only works while PINS_AND_CLAMPS feature has configured in the vsb.
Format: DSRPANEL,ON/OFF

M97/98 canned text drilling offset

These commands allow the user to shift the position of the text away from the edge clamps. Add the offset to the original X, Y coordinate for M97/98.
CAN_TEXT_OFF,#,# : The first parameter is X coordinate, and the second parameter is Y coordinate.
CAN_TEXT_OFF,# : Modify the X coordinate only.
CAN_TEXT_OFF : Show the current offset of X, Y in machine status window.

Coupon drilling setup commands

These commands allow the user to have more control on the coupon drilling. These commands can be in setup file or MACH.DAT file. In the following commands, if no parameter specified, it will show the current value in machine status window.
CPN_MAX_SIZE,# : To specify the maximum diameter of the tool to be used in the coupon drilling. The default value is 0.25 inch( 6.35mm ).
CPN_SEQ,# : To specify how many holes have to be drilled before inserting a gap free of holes in the coupon. The default value is 100.
CPN_GAP,#,# : To specify the size of this gap free of holes. The first parameter is X value, and the second one is Y value. The default X, Y value is 0, 0.

Binary map drilling setup commands

These commands allow the user to setup different mode for binary map drilling. In order for binary map drilling to take effect, there should have a line of code M19 inside the part program. If you specify BINARY_MAP_INPUT,2, you need to put some characters you want to drill inside the code, example "M19,12345ABC". If you specify BINARY_MAP_INPUT,0 (default), the characters you want to drill are coming from bar code scanner, you only need to put "M19" in your part program. These commands can be in setup file or MACH.DAT file. In the following commands, if no parameter specified, it will show the current value in machine status window.
BINARY_MAP,#,# : To specify the binary map location relatived to work zero. The first parameter is X value, and the second one is Y value. The default X, Y value is 10.0, 10.0.
BINARY_MAP_DIAM,# : To specify the diameter of the tool to be used in the binary map drilling. The default value is 0.031" ( 0.8mm ).
BINARY_MAP_SPACE,# : To specify the spacing between each hole. The default value is 0.05" (1.27MM).
BINARY_MAP_MAP,# : To specify the direction of sub_sequent characters.
1 : Upward 0,2 : Downward, default 3 : Leftward 4 : Rightward
BINARY_MAP_CONV,# : To specify the location of MSB of each character.
1 : at up 2 : at down 0, 3 : at right, default 4 : at left
BINARY_MAP_COUNT,# : To specify the maximum number of characters for binary map. The default value is 16.
BINARY_MAP_MODE,# : To speciy what kind of method to pick up tool for binary map drilling.
1 : Using current tool in part program. 0, 2 : Using the tool specified by BINARY_MAP_DIAM command, default.
BINARY_MAP_INPUT,# : To speify the source of characters to be drilled.
0,1 : From bar code scanner, default. 2 : From part program.

Adjust Tooling Plate

This command will select and adjust the tooling without displaying any popups. The machine will begin to adjust the tooling as soon as the command is entered.
The first parameter is the type of panel. MLB : Multilayer DSR : Double sided
The second parameter is the number of pinning holes 0 : DSR pannels without pinning holes # : Panels loaded over # number of fixed or adjustable pins.
The third parameter is the overall board size 24X30 : Describes the size of the board and it's orientation on the drilling machine. From left to right, the first number is the side to side dimension, the second is the front to rear dimension.
Format: TCADJ,#,#,# Example: TCADJ,DSR,0,24x17, TCADJ,MLB,4,24x20

Unclamp Tooling Plate

This keyboard command will unclamp the panels on all stations.
Format: UNCLAMP

Binary Map Location

This command will move the tooling plate to the location for binary map drilling. This command confirms the location.
Format: MOVE_BINARY_MAP

Set Quickdrill Border size

This command can alter the quick drill border size. if only one parameter is specified in this command, this parameter will be applied to both the X and the Y axes' quick drill board size. If two parameters are specified, the first parameter will be applied to the X axis' quick drill border size
Format: QBRDR,#,[#]

Update Cassette File

This command will force an immediate update of the current cassette configuration file. It will then copy the tooling data associated with the specified cassette number into the location specified by the command CRPLCFG.
Format: UPDCAS,#

Combine Cassette Files

This command will combine the contents of two cassette configuration files to create a new cassette configuration file with the same filename as that specified in the command. First, it copies all the data information contained in the specified number of cassette files from the specified filename to a temporary file. The system will then copy the remaining data information necessary to complete the cassette configuration file from the current cassette configuration file into the temporary file. A new XTMS configuration line will be generated. The file specified in the command will then be overwritten with the contents of the temporary file. The temporary file is then erased.
Format: COMBINE_CAS,filename,#