T-Series Operator`s Manual v3.04

CENTROID
T-SERIES
Operator's Manual
CNC11 Version 3.04
Rev. 110520
U.S. Patent #6490500
© 2011 Centroid Corp. Howard, PA 16841
™
READ THIS MANUAL BEFORE USING THIS PRODUCT.
FAILURE TO FOLLOW THE INSTRUCTIONS AND SAFETY
PRECAUTIONS IN THIS MANUAL CAN RESULT IN
SERIOUS INJURY OR DEATH.
All operators and service personnel must read this manual before operating
CENTROID CNC control equipment and all connected machine tools.
Keep this manual in a safe location for future reference.
Throughout this manual and on associated products where applicable, in accordance with
ANSI Z535, the following symbols and words are used as defined below:
DANGER
“DANGER” with or without a red background =
Hazard WILL cause death or serious injury if
ignored.
WARNING
“WARNING” with or without an orange
background = Hazard COULD cause death or
serious injury if ignored.
CAUTION
“CAUTION” with or without a yellow
background = Hazard MAY cause minor to
moderate injury if ignored.
NOTICE
“NOTICE” with or without a blue background =
Indicates an action to prevent damage to the
product or other materials used with product.
Information provided by CENTROID relating to wiring, installation, and operation of CNC
components is intended as only a guide, and in all cases a qualified technician and all
applicable local codes and laws must be consulted. CENTROID makes no claims about the
completeness or accuracy of the information provided, as it may apply to an infinite number of
field conditions.
As CNC control products from CENTROID can be installed on a wide variety of machine tools
NOT sold or supported by CENTROID, you MUST consult and follow all safety
instructions provided by your machine tool manufacturer regarding the safe operation
of your machine and unique application.
CENTROID CNC controls provide facilities for a required Emergency Stop circuit which can
be used to completely disable your machine tool in the event of an emergency or unsafe
condition. Proper installation of your CNC control MUST include the necessary wiring
to disable ALL machine tool movement when the Emergency Stop button is pressed.
This includes machine, servo motors, tool changers, coolant pumps, and any other moving
parts. DO NOT disable or alter any safety feature of your machine or CNC control.
Never alter or remove any safety sign or symbol from your machine or CNC control
components. If signs become damaged or worn, or if additional signs are needed to
emphasize a particular safety issue, contact your dealer or CENTROID.
CNC Control Operating Specifications
Operating Temperature
Ambient Humidity
Altitude
Minimum
Maximum
40°F (5°C)
104°F (40°C)
30% relative, non-condensing
90% relative, non-condensing
0 Ft. (Sea Level)
6000 Ft. (1830m)
Input Voltage (110, 220, 440 VAC,
-10% of Specified System Input
+10% of Specified System Input
System Dependent)
Voltage
Voltage
Note: Your machine may have operating conditions different than those shown above. Always consult your
machine manual and documentation.
Safety signs and labels found on your machine tool, and on CNC system
components typically follow the following examples:
CNC Machine Tool Safety
•All machine tools contain hazards from rotating parts; movement of belts, pulleys, gears, and chains;
high voltage electricity; compressed air; noise; and airborne dust, chips, swarf, coolant, and lubricants.
Basic safety precautions must be followed to reduce the risk of personal injury and property damage.
•Your local safety codes and regulations must be consulted before installation and operation of your
machine and CENTROID CNC control. Should a safety concern arise, always contact your dealer or
service technician immediately.
•Access to all dangerous areas of the machine must be restricted while the machine is in use. Ensure
that all safety guards and doors are properly in place during use. Automatically controlled machine
tools may start, stop, or move suddenly at any time. Do not enter the machining area when the
machine is in motion; death or severe injury may result.
•Personal protective equipment, particularly ANSI-approved impact safety glasses and OSHAapproved hearing protection must be used. Proper handling, storage, use, and disposal of materials
in accordance with manufacturer's instructions and Material Safety Data Sheets (MSDS, or your local
equivalent) must be followed.
•DO NOT operate your machine or CNC control in explosive atmospheres or in environmental
conditions outside of the manufacturer's specified ranges. Electrical power must meet the
specifications provided by your machine and CNC control manufacturer.
•DO NOT operate your machine or CNC control if any safety systems are damaged or missing.
Excessively scratched or damaged windows and guards must be replaced.
•ONLY authorized personnel should be allowed to operate the machine and CNC control. Improper
operation can cause injury, death, and machine or control damage, and may void applicable
warranties.
•All electrical enclosures and panels MUST be closed and secured at all times except during
installation and service. Only qualified electricians and service personnel should have access to these
locations. Hazards arising from high voltage electricity and heat exist in the control cabinet, and may
exist even after the main disconnect is turned OFF.
•Improperly clamped or fixtured parts; improperly secured tooling; and broken parts, fixtures, and
tooling resulting from machining operations at unsafe feedrates and spkeeds may result in projectiles
being ejected from your machine, even through safety systems such as guards and doors. Always
follow safe and reasonable machining practices and follow all safety precautions provided by your
tooling and machine manufacturer.
•Ultimate responsibility for safe operation and maintenance of your machine and CNC control rests
with shop owners and machine operators. Before performing any work or maintenance all individuals
should be thoroughly acquainted with the safe operation of BOTH machine tool AND CNC control.
•Shop owners and operators are responsible for ensuring that shop and machine safety systems such
as Emergency Stop and fire suppression systems are present and functioning properly, as required by
local codes and regulations.
CNC Control Warning Labels
High Voltage Electrocution
Hazard.
Death by electric shock can occur.
Turn off and lock out system power before
servicing.
High Voltage Electrocution
Hazard.
Death by electric shock can occur.
Turn off and lock out system power before
servicing.
Table of Contents
CHAPTER 1 - Introduction
Window Description
Conventions
Machine Home
Lathe M and G Codes
CHAPTER 2 - Operator Panels
T-Series Jog Panel
Keyboard Jog Panel
Keyboard Shortcut Keys
CHAPTER 3 - Main Screen
Option Descriptions
CHAPTER 4 - Tool Setup
Tool Wear Offset Adjustment Screen
Tool Geometry Offset Adjustment Screen
Tool Orient
Procedures for Setting Tool Offsets
Setting the Nose Radius
Setting the Nose Vector
CHAPTER 5 - Part Zero and WCS
Part Zero Menu
Setting Part Zeros
WCS Configuration Menu
Using Work Coordinate Systems
CHAPTER 6 – Running a Job
Job Running Menu
Canceling a Job in Progress
Resuming a Canceled Job
Run Menu
Power Feed
1-1
1-3
1-4
1-5
2-1
2-5
2-7
3-1
4-1
4-2
4-4
4-6
4-15
4-15
5-1
5-3
5-6
5-7
6-1
6-2
6-2
6-3
6-5
CHAPTER 8 - Lathe Intercon Manual
Lathe Intercon Main Menu
Lathe Intercon File Menu
Insert Operation
Linear
Arc
Drill
Tap
Thread
Profile
Turning
Groove
Cutoff
Other Operations
Graphics
Math Help
Intercon Lathe Tool Library
CHAPTER 9 - Lathe Intercon Tutorials
Lathe Intercon Tutorial #1
Lathe Intercon Tutorial #2
8-1
8-5
8-8
8-9
8-11
8-14
8-16
8-17
8-21
8-24
8-27
8-29
8-30
8-34
8-35
8-41
9-1
9-9
CHAPTER 10 - CNC Program Codes
Miscellaneous CNC Program Symbols
User and System Variables
Advanced Macro Statements (Optional)
10-1
10-4
10-8
CHAPTER 11 - G Codes
G-Code Quick Reference
G-Code Descriptions
11-1
11-2
CHAPTER 12 - M-functions
Macro M-functions
12-2
CHAPTER 13 - CNC Program Example
CHAPTER 7 - The Utility Menu
F2 – Update, F3 – Backup, F4 – Restore
F5 - File Ops
F6 - User Maint., F7 - Report, F8 - Options,
F9 - Log
7-1
7-2
7-3
7-3
CHAPTER 14 - Configuration
Password
Control Configuration
User-Specified Paths
Machine Configuration
Machine Parameters
PID Menu
CHAPTER 15 – CNC11 messages
CNC11 Message Descriptions
14-1
14-2
14-3
14-4
14-8
14-32
15-1
Chapter 1
Introduction
Window Description
The T-Series display screen is separated into five areas:
DRO Display
Status Window
Message Window
User Window
Function Key
Options
DRO display
The DRO display contains the digital readout for the current position of the tool. The display is configurable
for number of axes and desired display units of measure (see Chapter 14). The bars under each axis are the
load meters and represent the amount of power being supplied to the drive for that axis. The display of axis
load meters is configured by machine parameter 143 – see Chapter 14 for specific information. The symbol
next to the X-axis DRO indicates diameter or radius mode. See “Hot Keys” in chapter 2 for changing
between machine position and the current WCS position.
Distance to Go DRO
The distance to go DRO is located below the main DRO. This display shows the distance to go to complete
the current move. The display of the distance to go is controlled by parameter 143. See Chapter 14 for
details or it can be turned on by using Ctrl+D, see “Hot Keys” see chapter 2 for more details.
Status window
The first line in the status window contains the name of the currently loaded job file (see Chapter 3).
Below the job name are the Tool Number and Tool Offset, Program Number, Feedrate Override, Spindle
Speed, and Feed Hold indicators. The Feedrate Override indicator displays the current override percentage
set on the Jog Panel. If your machine is equipped with a variable frequency spindle drive (inverter), the
Spindle indicator will display the current spindle speed. The Feed Hold indicator displays the current status
of the FEED HOLD button located on the Jog Panel. If FEED HOLD is on, then the Feed Hold indicator
will indicate 'On' and can only be turned off by pressing CYCLE START.
T-Series Operator’s Manual
5/18/11
1-1
The Part Count and Elapsed Time indicators are not always displayed. Pressing CYCLE START while a
job is running will cause the indicators to appear. The Part Count indicator displays the number of times the
current part has been run and upon the completion of each run, it can increment/decrement by one. If a job is
canceled prematurely, the Part Count will not be incremented. The Part # counter shows how many parts
have been run, with an up/down arrow displayed to indicate the counting direction. See the run menu for
more information on the Part Count and Part# setting.
The Elapsed Time indicator displays the amount of time passed since CYCLE START was pressed. The
indicator will help you to determine how long it takes to cut a particular part. The timer will not stop until
the job is finished or canceled for any reason. It will continue to count for optional stops, tool changes,
FEED HOLD, etc.
Message window
The message window is divided into a message section and a prompt section. The prompt section is the
lowest text line in the window and will display prompts to the user. For example, the prompt 'Press CYCLE
START to start job' is displayed on the prompt line after power up.
The message section is the top four text lines of the message window. This section will display warnings,
errors, or status messages. The newest messages always appear at the bottom of the four lines. Old
messages are shifted up until they disappear off the top of the message window. When this happens, a scroll
bar appears. When the scroll bar is visible, use the up and down arrow keys to view older messages. See
Chapter 15 for a description of the T-Series error and status messages.
Function Key Options
Options are selected by pressing the function key indicated in the box. For example, on the Main Screen,
pressing the function key F5-CAM selects the CAM option.
User window
The information contained in this window is dependent on the operation you are performing on the control.
Enter the part zeros and the tool library setup information in this window. The window is empty if you are
performing no action.
For example, when the CYCLE START button is pressed and a job is processed correctly, up to 11 lines of
G-code will be displayed in this window.
1-2
5/18/11
T-Series Operator’s Manual
Conventions
● There are 10 function keys used by the control. They are represented by F1, F2,… F10. Keystrokes other
than the function keys are represented by the capitalized name of the key in bold font. For example, the A
key is written as A and the “Enter” key is written as ENTER. The "Escape" key is written as ESC. Key
combinations such as ALT+D mean that you should press and hold ALT then press D.
● Data entry menus on the T-Series Control usually use F10-Save to save changes and ESC to discard
changes.
● Any menu in the T-Series Control can be exited by pressing ESC. This will take you back to the previous
menu, pressing ESC enough times will eventually take you back to the main screen. This also usually
discards any changes you have made in that menu.
● The Centerline of the part (and Spindle) is usually considered to be X=0.
● The orientation of the axes are as follows: X+ always points away from the Centerline and Z+ always
points to the right and away from the Spindle. Although the T-Series Control is able to display the X+
direction as either oriented up or down (set in Machine Parameter 1), most of the illustrations in this manual
will show X+ as pointing upward, as if the tool turret is mounted behind the centerline of the spindle.
Tool turret mounted
behind centerline
X+
Z+
Centerline (X = 0)
Z+
Spindle
Chuck
X+
Tool turret mounted
in front of centerline
● Tools move in X and Z directions. The work piece remains in a stationary location relative to X and Z.
● CW stands for clockwise and CCW stands for counterclockwise.
● The work piece physically spins in the Spindle Chuck, the CW and CCW directions refer to the chuck
spinning in those directions when viewed in the Z+ direction (Through the spindle towards the tailstock).
● ID means Inner Diameter, and OD means Outer Diameter.
T-Series Operator’s Manual
5/18/11
1-3
Machine Home
When the T-series control is first started, the Main Screen will appear as below.
Before you can run any jobs, you must set the machine home position. If your machine has home/limit
switches, reference marks or safe hard stops, the control can automatically home itself. If your machine has
reference marks, jog the machine until the reference marks are lined up (see below). Then press CYCLE
START to begin the automatic homing sequence. The control will execute the G-codes in a file called
cnct.hom in the c:\cnct directory. By default, this file contains commands to home X to its plus limit and
home Z to its plus limit.
Typical Reference Marks
If your machine does not have home/limit switches or safe hard stops, the following message will appear
instead.
In this case you must move the machine to its home position yourself, using either the jog keys or the
handwheels. Once all axes are at their home positions, press CYCLE START to set machine home.
1-4
5/18/11
T-Series Operator’s Manual
Lathe M and G Codes
M00 Stop For Operator
M01 Optional Stop for Operator
M02 Restart Program
M03 Spindle On Clockwise
M04 Spindle On Counterclockwise
M05 Spindle Stop
M07 Mist Coolant On
M08 Flood Coolant On
M09 Coolant Off
M10 Clamp On
M11 Clamp Off
M26 Set Axis Home
M29 Set Tap Mode for G84
M50 C Axis Disable
M51 C Axis Enable
M91 Move to Minus Home
M92 Move to Plus Home
M93 Release/Restore Motor Power
M94/M95 Output On/Off
M98 Call Subprogram
M99 Return from Macro or Subprogram
M100 Wait for PLC bit (Open, Off, Reset)
M101 Wait for PLC bit (Closed, On Set)
M102 Restart Program
M103 Programmed Action Timer
M104 Cancel Programmed Action Timer
M105 Move Minus to Switch
M106 Move Plus to Switch
M107 Output BCD Tool Number
M108 Enable Override Controls
M109 Disable Override Controls
M115,M116,M125,M126 Protected Move Probing
M120 Open data file (overwrite existing file)
M121 Open data file (append to existing file)
M122 Record position(s) in data file
M123 Record value and/or comment in data file
M124 Record machine position(s) in data file
M127 Record Date and Time in a data file
M128 Move Axis by Encoder Counts
M150 Set Spindle Position to 0 on Next Index Pulse
M151 Unwind C axis
M200 Stop for Operator, Prompt for Action
M223 Write Formatted String to File
M224 Prompt for Operator Input Using Formatted String
M225 Display Formatted String for A Period of Time
M300 Fast Synchronous I/O update
M1000-M1015 Graphing Color for Feedrate movement
T-Series Operator’s Manual
G00
G01
G02
G03
G04
G10
G20
G21
G22
G23
G28
G29
G30
G32
G40
G41
G42
G50
Rapid to Position
Linear Move
CW Arc Move
CCW Arc Move
Dwell
Set Parameter
Inch Units
Metric Units
Work Envelope On
Work Envelope Off
Return to Reference Point
Return from Reference Point
Return to Secondary Reference Point
Constant Lead Thread Cutting
Cancel Cutter Compensation
Cutter Compensation Left/Right
Cutter Compensation Left/Right
Coordinate System Setting OR
Maximum Spindle Speed for CSS mode
G52 Offset Local Coordinate System Origin
G53 Rapid Positioning in Machine Coordinates
G54-G59 Select Work Coordinate System
G65 Call Macro
G70 Finishing Cycle (after Stock Removal)
G71 Stock Removal in Turning
G72 Stock Removal in Facing
G74 End Face Peck Cutting Cycle
G75 Outside/Inside Diameter Peck Cutting Cycle
G76 Multi-Pass Threading Cycle
G80 Canned Cycle Cancel
G83 Deep Hole Drilling (Canned Cycle)
G84 Tapping (Canned Cycle)
G85 Boring (Canned Cycle)
G90 Outside/Inside Diameter Cutting Cycle
G92 One-Pass Thread Cutting Cycle
G94 End Face Turning
G96 Constant Surface Speed (CSS mode)
G97 Cancel Constant Surface Speed
G98 Feed per minute
G99 Feed per revolution
5/18/11
1-5
How to unlock software features or unlock your Control
The following are necessary to unlock software features:
1.
2.
3.
4.
5.
6.
7.
If you are at the "Demo mode expired" screen, start at step 4.
Go to the Main screen of the Control software.
Press F7 "Utility" and then F8 "Option"
Press F1 "Unlock Option". (You may need to enter the password – usually 137)
Next, type in the Unlock # and press ENTER.
Then, type in the Unlock Value and press ENTER.
Repeat step 4, 5, and 6 for each new Unlock.
1-6
5/18/11
T-Series Operator’s Manual
Chapter 2
Operator Panel
The operator panel is a sealed membrane keyboard that
enables you to control various machine operations and
functions. The panel contains momentary membrane
switches, which are used in combination with LED
indicators to indicate the status of the machine
functions.
Axis Jog Buttons
X+ X- Z+ ZThe yellow X and Z keys are momentary switches for
jogging the two axes of the machine. There are two
buttons for each axis (+/-). Only one axis can be jogged
at a time.
* NOTE: The jog buttons will not operate if the TSeries CNC software is not running, or if a job (a CNC
program) is running.
Slow/Fast
The slow/fast key is located in the center of the Axis
Motion Controls section and is labeled with the turtle
and rabbit icon shown to the right. The turtle
represents slow jogging mode. When SLOW jog is
selected (LED on) and a jog button is pressed, the axis
moves at the slow jog rate. If FAST jog is selected, the
axis will move at the fast jog rate. See Chapter 14 for
information on setting the fast and slow jog rates for
each axis.
Inc/Cont
INC/CONT selects between incremental and
continuous jogging. Pressing the key will toggle
between these two modes. The LED is lit when INC is
selected. If CONT jog is selected and an axis jog button
is pressed, the axis will move continuously until the
button is released.
Fig 1 - T-Series Jog Panel
T-Series Operator’s Manual
5/18/11
2-1
x1, x10, x100
Press any one of these keys to set the jog increment amount. The amount you select is the distance the control will
move an axis if you make an incremental jog (x1=0.0001", x10=0.0010" and x100=0.0100"). You may select only one
jog increment at a time, and the current jog increment is indicated by the key that has a lit LED. The jog increment
you select is for all axes; you cannot set separate jog increments for each axis. The jog increment also selects the
distance the control will move an axis for each click of the MPG handwheel.
MPG
The MPG is housed in a separate hand-held unit. Press the MPG key to set the control jog to respond to the MPG hand
wheel, if equipped. When selected, the LED will be on. Select the Jog Increment and desired axis and slowly turn the
wheel. When the LED is not lit, the MPG is disabled and the jog panel is on.
NOTICE
Do not spin the handwheel too quickly. Damage to the machine or part may result.
Single Block
The SINGLE BLOCK key selects between auto and single block mode. When the SINGLE BLOCK LED is on, the
single block mode has been enabled. Single Block mode allows you to run a program line by line by pressing CYCLE
START after each block. While in block mode you can select auto mode at any time. While in auto mode and a
program is running you cannot select single block mode. Auto mode runs the loaded program after CYCLE START is
pressed. Auto mode is the default (LED off).
Cycle Start
When the CYCLE START button is pressed, the T-Series Control will immediately begin processing the current
program at the beginning and will prompt you to press the CYCLE START button again to begin execution of the
program. After an M0, M1, M2, or tool change is encountered in the program, the message
Press CYCLE START to continue
will be displayed on the screen, and the T-Series Control will wait until you press the CYCLE START button before
continuing program execution.
WARNING
Pressing CYCLE START will cause the T-Series Control to start moving the
axes immediately without further warning. Be certain that you are ready to start
the program when you press this button. Pressing the FEED HOLD button, ESTOP, or the CYCLE CANCEL button will stop any movement if CYCLE
START is pressed accidentally.
Feedrate Override
This knob controls the percentage of the programmed Feedrate that you can use during feedrate cutting moves: lines,
arcs, canned cycles, etc. This percentage can be from 0% to 200%.
CAUTION
The Feerate Override knob will not work during tapping cycles (G84) and
threading moves (G32).
Feed Hold
Feed Hold decelerates motion of the current movement to a stop, pausing the job that is currently running. Pressing
CYCLE START will continue the movement from the stopped location.
CAUTION
2-2
FEED HOLD is temporarily disabled during tapping cycles (G84),
threading moves (G32), and automatic tool changes (M6).
5/18/11
T-Series Operator’s Manual
Tool Check
Pressing TOOL CHECK while a job (a CNC program) is not running will move the table to its tool change (G28)
position. Pressing TOOL CHECK while a job is running will stop normal program movement, clear all M-functions,
and automatically display the Resume Job Menu. From the Resume job menu, you will be able to change tool settings.
● NOTE: When a job is running, pressing TOOL CHECK once stops the job and allows you to manually jog the tool
clear. Pressing TOOL CHECK a second time will cause the tool to move to its tool change (G28) position.
Cycle Cancel
Press CYCLE CANCEL to abort the currently running program. The control will stop movement immediately, clear
all M-functions, and return to the Main Screen. It is recommended that you press FEED HOLD first before CYCLE
CANCEL. If you press CYCLE CANCEL, program execution will stop; if you wish to restart the program you must
rerun the entire program or use the search function. See search function operation in Chapter 6.
Emergency Stop
EMERGENCY STOP releases the power to all the axes and cancels the current job immediately upon being pressed.
EMERGENCY STOP also resets certain faults if the fault condition has been fixed or cleared.
Spindle CW/CCW
The SPINDLE CLOCKWISE/COUNTERCLOCKWISE keys determine the direction the spindle will turn if it is
started manually. If the spindle is started automatically, the direction keys are ignored and the spindle runs according
to the program. The default direction is CW.
Spindle Speed +
Pressing this key will increase the spindle speed by 10% of the commanded speed in Auto spindle mode, limited by the
maximum speed or 200% of commanded speed, whichever is less. For manual spindle mode, the spindle speed is
increased by 5% of the maximum spindle speed (up to the maximum speed). The LED is on if the spindle speed is set
above the 100% point.
Spindle Speed 100%
Pressing this key will set the spindle speed at the 100% point, which is defined as the commanded speed in Auto
spindle mode, or ½ the maximum spindle speed in manual mode. The LED will be on when the spindle is at the 100%
point.
Spindle Speed Pressing this key will decrease the spindle speed by 10% of the commanded speed in Auto spindle mode, limited to
10% of commanded speed. For manual spindle mode, the spindle speed is decreased by 5% of the maximum spindle
speed down to 5% of maximum. The LED is on if the spindle speed is set below the 100% point.
T-Series Operator’s Manual
5/18/11
2-3
Spindle (Auto/Man)
This key selects whether the spindle will operate under program control (automatic) or under operator control
(manual). When the LED is lit, the spindle is under automatic control. If the LED is off, the spindle is under manual
control. Pressing the SPINDLE (AUTO/MAN) key will toggle it from AUTO to MAN and back again. The default
is AUTO mode.
Spin Start
Press the SPIN START key when manual spindle mode is selected to cause the spindle to start rotating. Press SPIN
START when automatic mode is selected to restart the spindle if it has been paused with SPIN STOP.
Spin Stop
Press the SPIN STOP key when manual spindle mode is selected to stop the spindle. Press SPIN STOP when
automatic mode is selected to pause spindle rotation and can be restarted with SPIN START.
NOTICE
SPIN STOP should only be pressed during FEED HOLD or when a program is NOT
running.
Coolant Auto/Manual
This key will toggle between automatic and manual control of coolant. In automatic mode, M7 (Mist) and M8 (Flood)
can be used in G-code programs to select the coolant type to be enabled. In manual mode, flood coolant and mist
coolant are controlled by separate keys. Note: When switching from automatic to manual mode, both flood and mist
coolants are turned off automatically.
Coolant Flood
In manual coolant control mode, flood coolant can be toggled off and on by pressing this key. The LED will be on
when flood control is selected in either automatic or manual mode.
Coolant Mist
In manual coolant control mode, mist coolant can be toggled off and on by pressing this key. The LED will be on
when mist control is selected in either automatic or manual mode.
Auxiliary Function Keys (AUX1 – AUX12)
The T-Series jog panel has nine auxiliary keys, some of which may be defined by customized systems.
T-Stock In, T-Stock Out,
Quill In, Quill Out, Turret Index
These buttons currently have no settings but can be added to one of the Aux keys and then programmed to control
hydraulic stock clamps, Quills, or Turret index functions through the PLC. Your installer will provide you with the
necessary documentation explaining the operation and functions these keys perform.
2-4
5/18/11
T-Series Operator’s Manual
Keyboard Jog Panel
The PC keyboard may be used as a jog panel. Press Alt-J to display and enable the keyboard jog panel. The jog panel
appears as shown below:
Some controls, such as coolant on/off, spindle on/off, feedrate and spindle override will work without the “jog panel”
being displayed but for full functionality (and jogging) of the keyboard jog panel, the “jog panel” must be displayed on
the screen. To enable keyboard jogging, parameter 170 must be set to “1”.
The status window in the upper right corner of the screen displays the jogging mode (continuous/incremental),
incremental step size, and jog speed (fast/slow). In continuous mode, the jog keys start movement when pressed and
movement stops when you release the key. In incremental mode, the axis will move the indicated incremental step
amount.
As shown in the picture above, the jog keys are located in the cursor key block to the right of the main keyboard and to
the left of the numeric keypad. If a jog key controls an axis, it will be overlaid with the axis symbol (“X”, “Z”, etc.)
The jog keys are the arrow keys, Insert, Delete, Home, End, Page Up, and Page Down.
The remaining keys are described below:
Legend
Key(s)
Ctrl S
Function
Cycle Start
Description
Same as Cycle Start.
Availability (Notes)
Always, with few
exceptions.
Esc
Cycle
Cancel
Same as Cycle Cancel.
Space
Feed Hold
Turns Feed Hold on and off
During a job run;
otherwise, Esc is
used to exit menus.
Always, with few
exceptions.
Alt J
Start/Exit
Panel
Aux 1 –
Aux 12
Invokes or exits the jog panel.
Ctrl F1
Ctrl F12
T-Series Operator’s Manual
Executes the corresponding Aux function and
signals the PLC. A custom PLC program is
required to act upon jog panel signals.
5/18/11
Always, with few
exceptions.
Always, with few
exceptions.
2-5
Legend
Feedrate
Override
+
Feedrate
Override
-
2-6
Key(s)
Ctrl M
Function
Toggle Auto
Coolant
Description
Toggles coolant mode between auto and
manual.
Availability (Notes)
Always, with few
exceptions.
Ctrl N
Turns on/off
Flood
Toggles Flood coolant if in manual mode
Always, with few
exceptions.
Ctrl K
Turns on/off
Mist
Toggles Mist coolant if in manual mode
Always, with few
exceptions.
Increase
feedrate
override
Increase feed rate override by 1% while held.
Jog panel, job run,
graphing, and some
other times
Decrease
feedrate
override
Decrease feed rate override by 1% while held.
Jog panel, job run,
graphing, and some
other times.
Ctrl C
Selects CW
Spin
Selects CW Spin dir in man mode
Always, with few
exceptions.
Ctrl W
Selects CW
Spin
Selects CCW Spin dir in man mode
Always, with few
exceptions.
Ctrl A
Toggles between automatic and manual
spindle operation.
Always, with few
exceptions.
Ctrl S
Toggle
Spindle
Auto/
Manual
Spin Start
Starts spindle in selected direction if in
manual mode
Always, with few
exceptions.
Ctrl Q
Spin Stop
STOPS spindle regardless of auto or manual
mode.
Always, with few
exceptions.
Ctrl >
Spindle
Override
+1%
Increase the spindle override by 1% while
held.
Always, with few
exceptions.
Ctrl <
Spindle
Override 1%
Decrease the spindle override by 1% while
held.
Always, with few
exceptions.
Ctrl T
Tool Check
Performs a tool check.
Always, with few
exceptions.
Ctrl I
Incremental/
Continuous
Jog
Selection
Toggles incremental or continuous jog mode.
Ctrl +
Ctrl -
5/18/11
Available most times
that jogging is
available.
T-Series Operator’s Manual
Legend
Key(s)
Ctrl F
Function
Toggles
Fast/Slow
Jog mode
Description
Toggles between Fast and Slow Jog mode
Availability (Notes)
Always, with few
exceptions.
Ctrl B
Selects
Single
Block Mode
Decrease
Jog
increment
Selects single block mode
Always, with few
exceptions.
Decreases current jog increment to the next
lower available increment
Always, with few
exceptions.
Increase current jog increment to the next
higher available increment
Always, with few
exceptions.
Delete
Insert
Increase Jog
Increment
Left
arrow
Z - Jog
With on screen jog
panel displayed
Right
Arrow
Z+ Jog
With on screen jog
panel displayed
Up
Arrow
X+ Jog
With on screen jog
panel displayed
Down
Arrow
X- Jog
With on screen jog
panel displayed
MDI and the Keyboard Jog Panel
Many of the keys used by the keyboard jog panel are also possible commands to MDI. To use the keyboard jog panel
functions in MDI, you must press Alt J. You may jog; use the handwheels, or any other jog panel function. Press Alt
J or Esc to return to MDI.
Keyboard Shortcut Keys
A computer style keyboard is supplied with most systems. This keyboard can be used as a jog panel. The keyboard
jog panel has many “hot keys”. Hot keys are keys that can be used at almost any time, with few exceptions. Some
menus may prohibit their use. The CNC software has many other hot keys in addition to the jog panel hot keys. The
hot keys are listed below.
Hot Keys
Hot Key
Ctrl A
Ctrl N
Ctrl M
ALT D
CTRL D
CTRL K
ALT F
ALT I
ALT J
ALT K
Action
Spindle auto/manual
Flood coolant on/off*
Toggle Auto Man Coolant
Switch between current position and machine position
Switch DRO between position and distance to go
Mist coolant on/off*
Displays available system memory
PLC diagnostics
Enables keyboard jogging*
Displays current ATC tool bin location
T-Series Operator’s Manual
5/18/11
2-7
Hot Key
ALT M
Ctrl T
ALT P
CTRL P
Ctrl C
Ctrl W
Ctrl S
Ctrl Q
ALT S
ALT T
ALT V
ALT W
ALT + / ALT ALT 1 - ALT 0
ALT Tab
CTRL F1 - CTRL F12
CTRL V
CTRL I
Notes:
2-8
Action
MDI
Tool check*
Live PID display
Clear max and min error display
Spindle CW*
Spindle CCW*
Start Spindle*
Stop Spindle
Cycle start
Displays current motor temperature estimates
Displays current software version #
MPG on/off*
Selects next/previous WCS, cycles through WCS 1-18**
Selects WCS 1 – WCS 10**
Cycle through currently running applications
Executes Aux function 1 – 12*
Enables/disables Stall detection in PID Configuration
Creates plcstate.txt when PLC diagnostics is displayed***
* This is a keyboard jog panel function.
** Not available during jobs or on jog panel.
5/18/11
T-Series Operator’s Manual
Chapter 3
Main Screen
When the T-Series control is started, the first menu to appear is the Main Screen.
Option Descriptions
F1 - Setup
When you press F1-Setup from the Main Screen, you will be shown the Setup menu containing options related to
setting up various aspects of the machine.
F1 – Part
This key displays the Part Setup menus, which are explained in Chapter 5.
F2 – Tool
This key displays the Tool Setup menus, which are explained in Chapter 4.
F3 – Config This key displays the Configuration menu, which is explained in Chapter 14.
F4 – Feed
This key displays the Feed menu, which is discussed in Chapter 6.
T-Series Operator’s Manual
5/18/11
3-1
F2 – Load Job
Job Name: c:\cnct\ncfiles\bracket.cnc
Use arrow keys to select file to load and press F10 to Accept.
arcs.cnc
bracket.cnc
flange.cnc
test fixture plate.cnc
Job to load? bracket.cnc
G code
/ICN
F1
Floppy
/USB/LAN
F2
Details
On/Off
F3
Show
Recent
F4
Date/
Alpha
F5
Edit
F6
Help
On//Off
On
F7
Graph
F8
Advanced
F9
Accept
F10
F1
0
*Note: The path and/or file name may also be selected by typing the path or path and file name. A window
will open automatically when you begin typing.
F1 – G code
/ICN
F2 – Floppy
/USB/LAN
F3 – Details
F4 – Show
Recent
F5 – Date/Alpha
F6 – Edit
F7 - Help
F8 - Graph
F9 - Advanced
Page Up
Page Down
END
HOME
Arrow Keys
Allows the user to change which types of files are displayed.
Select a different drive from which to load files.
Displays file details including: Programmer, Description and Date Modified.
Displays a list of the 15 most recently loaded jobs.
Toggles the current view of files to be sorted alphabetically or by date modified.
Opens selected file in editor.
Displays on screen help for the load screen.
Back plots (graphs) the selected file.
Displays a unified file and device browser similar to Windows Explorer.
Move the cursor backward one page.
Move the cursor forward one page.
Select the last file in the list.
Select the first file in the list.
Move the cursor in the selected direction.
F3 –MDI - MDI mode allows you to directly enter M and G-codes one line at time.
After entering the M
and G-codes you wish to run, press cycle start to have the controller execute the command. When the
command has finished executing the command, it will prompt you for another line. When you are finished
entering commands, press ESC.
Examples:
Block? G50X0Z0
; Set the current XY position to 0,0
Block? M26 /Z ; Set the current Z position as Z home
.
3-2
5/18/11
T-Series Operator’s Manual
F4 - Run
Press F4-Run to change the way your part program will run. See chapter 6 for more information concerning the
run menu.
F5 - CAM
Choose F5-CAM from the Main Menu to enter Intercon (Interactive Conversational) software. When you exit
Intercon software, you will return to the Control Main Screen. The posted Intercon program will be automatically
loaded into CNC11.
Current Position ( Inches )
X
Z
+4.0000
+2.0000
Job Name :
Tool :
Feedrate :
Spindle :
pawn.cnc
pawn.cnc
T0700
100%
0
M
Stopped
Waiting for PLC operation
Pres
Press
ess CYCLE START to start job
CAM Selection
ICN
Help
ICN
F1
F1- ICN
F2- Help
- Intercon Lathe
- Operators Manual
Help
F2
Lathe Intercon conversational programming
Allows you to access the operator manual on the control
F6 - Edit
Loads the current job into a text editor for editing. Some of the commands available in the editor are:
Alt-f = Opens the File Menu
Alt-e = Opens the Edit Menu
Alt-s = Opens the Search Menu
Alt-p = Opens the Preferences Menu
Alt-c = Opens the Macro Menu
Alt-w = Opens the Window Menu
Ctrl-o = Open file
Ctrl-n = New file
Ctrl-s = Save file
Ctrl-q = Quit
Shift-Ctrl-f = Find
Shift-Ctrl-g = Find next
Shift-Ctrl-r = Replace
Shift-Ctrl-l = Goto line number
*Note: Alt key combos work only when Num Lock is OFF.
T-Series Operator’s Manual
5/18/11
3-3
Attempting to edit files that contain non-printable characters may cause unexpected results. DO NOT edit the
CNC11 files cnctcfg.xml, cnct.prm.xml, cnct.job, cnct.ttl, and cnct.wcs. These files will be destroyed and all
information lost if they are edited.
F7 - Utility
From the utility menu you can view available software options, perform diagnostics, backup part and
configuration files, create new directories and import or export files to and from external locations. For further
information please see chapter 7.
F1 – Format
F2 – Update
F3 – Backup
F4 – Restore
F5 – File Ops
F6 – User Maint
F7 – Report
F8 – Options
F9 – Logs
Format a high-density floppy disk. Only available if a floppy drive is installed.
Update your control software from a floppy disk or USB Storage device
Backup your CNC and ICN files
Restore your CNC and ICN files
Use this menu to perform file and directory operations.
Perform user maintenance.
Generates a backup of system configuration files called report.zip.
Shows the software options that you have purchased or added to your control.
Shows the messages and errors that have been logged by the control.
F8 – Graph
In addition to the Main Screen, the Graph feature can be accessed from other menus like the Load Job Screen and
the various Run Job menus. Use the Graph feature to show a tool path of the current program loaded. The
following is a sample graph of a part:
A wire frame tool path of your part should appear. Each axis is indicated by the X or Z marker, along with scales to
indicate the current location of the part. Here is a list and the function of the F-Keys located on the bottom of the
screen:
F3 - Set Range
Press this key to set the range of line numbers or block numbers to graph.
3-4
5/18/11
T-Series Operator’s Manual
F4 - Time Estimation
Press this key to estimate the time needed to create the part. It takes into account accelerations and decelerations,
but neglects tool change times.
F5 - Redraw
Press this key to redraw the graphics at any time.
F6 - Pan
Press this key to move the part around the graph. Once pressed, use the crosshatches to pick a location of the part
that will pan to the center of the graph. Once a section is selected, press F6-Pan again to continue panning.
F7 - Zoom In
Press this key to zoom into the part relative to the center of the graph.
F8 - Zoom Out
Press this key to zoom away from the part relative to the center of the graph.
F9 - Zoom All
Press this key to view the entire part fit inside the graph.
F10 - Shutdown
Press F10-Shutdown to enter the Shutdown menu. This menu allows you to park the machine, poweroff the
control, start a command window or exit CNC11.
F1 - Park
Press F1-Park to park the machine at the end of the day for quicker machine homing at startup. Once F1-Park is
selected, The Cycle Start key must be press to start machine movement. The park feature homes each axis, at the
maximum rate, to ¼ motor revolutions from its home position. The Z-axis is moved first, and then all the other axes
are done.
F2 - Poweroff
Press F2-Poweroff to properly shutdown the control. With most controls, this action turns off the control once the
system has prepared itself to be shutdown. Just like a desktop computer, the control should be properly shutdown
before turning off the power in order to reduce the risk of corrupting data on the hard drive.
NOTE: This option will only turn off the control. The machine itself will still need to be manually turned off. Once
the screen says Power Off it is safe to turn off the main disconnect.
F6 - System Prompt
Press F6-System Prompt to start a command window. From this window you can type CNC Linux commands at a
prompt. Pressing Alt+F6 at any time will display a command window. Type the command exit to exit the
command window.
F9 - Exit CNC11
Press F9-Exit CNC11 to exit CNC11 software.
T-Series Operator’s Manual
5/18/11
3-5
3-6
5/18/11
T-Series Operator’s Manual
Chapter 4
Tool Setup
Four menus are involved in tool setup:
● Tool Wear Offset Adjustment Screen – allows operator to make tool wear adjustments for each tool
● Offset Library – specifies offset definitions to be associated with each tool
● Tool Orient – miscellaneous tool offset specifications
● Lathe Intercon’s Tool Library – Lathe Intercon’s version of the Tool and Offset Libraries
Only the first three menus will be discussed in this chapter. See Chapter 8 for a description of Lathe Intercon’s Tool
Library. For information on setting up tool offsets see the section “Procedures for Setting Tool Offsets” later in this
chapter.
Tool Wear Offset Adjustment Screen
To get to the Tool Wear Offset Adjustment Screen from the Main Screen, press F1-Setup ➞ F2-Tool. This screen
allows you to make tool wear adjustments for each tool. Adjustment values entered here will be added to the
corresponding fields in the Offset Library to obtain the final offset value to be used by the control during a job run.
The Tool Offset Adjustment table fields and screen elements are described below:
Tool: This field is considered the offset number if you access the Offset X, Offset Z, or Nose Radius fields of this
table. However, this field is considered the Tool Number if you look at the Description field of this table. This
field is just a display label and cannot be modified.
Offset X: This is the distance adjustment for the Offset X field in the Offset Library radius or diameter (described
later in this chapter).
Offset Z: This is the distance adjustment for the Offset Z field in the Offset Library (described later in this
chapter).
Nose Radius: This is the size adjustment for the Nose Radius field in the Offset Library (described later in this
chapter).
T-Series Operator’s Manual
5/18/2011
4-1
(Description): This field is displayed on this screen for your convenience. It cannot be modified here. To modify
this field, go to the control’s Tool Library (see the Tool Library section later in this chapter) or go into Lathe
Intercon’s Tool Library.
F4 – Abs/Inc
This toggles the Entry Mode between Absolute and Incremental.
Entry Mode: You can toggle between absolute input and incremental input using the F4-Abs/Inc key. The Entry
Mode affects values entered in the Offset X, Offset Z and Nose Radius adjustment fields. If the Entry Mode is
Incremental, then the value that you enter will be added to current value in that field. If the Entry Mode is
Absolute, then the value that you enter will be the value entered in that field.
F5 – Increment by small amount
To make small incremental adjustments to an Offset X, Offset Z, or Nose Radius adjustment value, use the arrow
keys to select the value to be adjusted and press this key. A small amount (as defined in Machine Parameter 70)
will be added to the affected field.
F6 – Decrement by small amount
To make small decremental adjustments to an Offset X, Offset Z, or Nose Radius adjustment value, use the arrow
keys to select the value to be adjusted and press this key. A small amount (as defined in Machine Parameter 70)
will be subtracted from the affected field.
F7 – ATC (Automatic Tool Change)
If you have an automatic tool changer installed, you can press this key to change tools.
F10 – Save
When you are done with modifications press this key to save the changes.
Tool Geometry Offset Library
To get to the Offset Library from the Main Screen, press F1-Setup ➞ F2-Tool ➞ F1-Offset Lib. On this screen,
you can define the offsets to be associated with each tool.
Elements of the Offset Library and its fields are described below:
4-2
11/18/02
T-Series Operator’s Manual
Tool: This is the offset number. Although this number is appended to a “T”, this is not a tool number. However,
if you only associate tool numbers with the same numbered offset, and then this field would correspond to the tool
number. This field is just a display label and cannot be modified.
Offset X: This field defines the X offset distance away from the tool measurement radius or diameter. (See X
Diam/Radius as described below.)
Offset Z: This field defines the Z offset distance away from the Z reference position. (See Z Ref as described
below.)
Nose Radius: This field tells the control the distance to adjust when cutter diameter compensation (G41 or G42) is
activated.
Nose Vector: This field tells the control how the tool is oriented in the machine. See the section titled “Setting the
Nose Vector” later in this chapter for a more in-depth explanation.
X Diam/Radius: This field defines the diameter or radius from which the X offsets of tools are to be measured.
This diameter is usually created by a skim cut as part of the tool measuring procedure. (See the Procedures for
Setting Tool Offsets section later in this chapter.) To set the X diameter field, cursor over to the Offset X column
and press F1 – X Diam. and follow the instructions.
Z Ref: This field is the Z reference position from which the Z offsets of tools are to be measured. To set the Z
reference field, cursor over to the Offset Z column and press F1 – Z Ref. and follow the instructions.
Entry Mode: You can toggle between absolute input and incremental input using the F4-Abs/Inc key. The Entry
Mode affects values entered in the Offset X, Offset Z, Nose Radius, X Diam/Radius, and Z Ref fields. If the Entry
Mode is Incremental, then the value that you enter will be added to currently affected field. If the Entry Mode is
Absolute, then the value that you enter will change the field to that value.
F1 – X Diam/Rad or Z Ref
Press this key to establish the X Radius or Diameter for Tool measurement or to establish the Z reference. To
establish the X Radius or Diameter, cursor over to the Offset X column and press this key and then follow the
instructions. To establish the Z reference, cursor over to the Offset Z column and press this key and then follow the
instructions.
F2 – Manual Measure
Press this key to make an offset measurement of a tool. This key is used in the part tool measuring procedure. (See
the Procedures for Setting Tool Offsets section later in this chapter.)
F4 – Abs/Inc
This toggles the Entry Mode between Absolute and Incremental. (See “Entry Mode” as described above.)
F5 – Increment by small amount
To make small incremental adjustments to an Offset X, Offset Z, or Nose Radius value, use the arrow keys to select
the value to be adjusted and press this key. A small amount (as defined in Machine Parameter 70) will be added to
the affected field.
F6 – Decrement by small amount
To make small decremental adjustments to an Offset X, Offset Z, or Nose Radius value, use the arrow keys to
select the value to be adjusted and press this key. A small amount (as defined in Machine Parameter 70) will be
subtracted from the affected field.
F7 – ATC (Automatic Tool Change)
If you have an automatic tool changer installed, you can press this key to change tools.
F10 – Save
When you are done with modifications press this key to save the changes.
T-Series Operator’s Manual
5/18/2011
4-3
Tool Orient
To access the Tool Orient screen from the Main Screen, press F1-Setup ➞ F2-Tool ➞ F2-Tool Orient. This
screen allows you to view and change miscellaneous tool offset descriptions used by Lathe Intercon.
The Tool Detail fields and screen elements are described below:
Tool (Offset): This field is the tool offset number. It is selected in lathe CNC programs by the third and fourth
digits of the T number. For example, T0122 selects tool offset 22 and turret station 01. For convenience in editing,
you may jump directly to any offset number by entering the new number in the Tool field.
Station: This field contains the station number (turret position) of the tool that uses this offset. This field
corresponds to the first two digits of the T number in CNC programs and the “Tool Loc” (Tool Location) field in
Lathe Intercon’s version of the Tool Library. To change the station number, type a new number and press ENTER.
Normally, you should try to keep this number the same as the offset number. However, if you want to use 2 or 3
different offsets for one tool, this is the field that you should change. For example, T0101, T0122, T0123 specify
different offsets for the same tool station position. In the tool details, you would enter “1” in the station field of
offsets 1, 22, and 23. When you choose an offset from the Intercon Tool Library, Intercon automatically inserts the
selected station/offset combination. This way, when you map multiple offsets to a single tool, it is likely that most
of the information in the respective offsets will be very similar with minor differences.
Description: This field contains a text description of the tool. The description will appear in a prompt message on
the screen when the control software reaches a tool change during a job run.
Type: This field specifies a general class of tool. It is supplied for your reference only. CNC11 does not make use
of this information. Possible values are “Turning”, “Threading”, “Grooving/Parting”, “Boring”,
“Drill/Tap/Reamer”, and “Custom”. To change the value, press the SPACE bar until the desired type is shown.
Operation: This field specifies whether the tool is an “Outer Diameter” or “Inner Diameter” tool. CNC11 does not
use this information at the present time. In future releases of CNC11, it may be necessary to set this field correctly
on systems that are configured for gang tooling.
Approach: This field specifies the tool approach direction for a gang tool type or dual tool turret type lathes. It is
an essential input to the “most likely nose vector” calculation. To be able to change this value parameter 163 (gang
tool parameter) must be set to a 1, otherwise this field should display the direction of all tool approaches as
determined by parameter 1.
4-4
11/18/02
T-Series Operator’s Manual
Spindle Direction: This field specifies the spindle direction. Possible values are “CW (M3)”, “CCW (M4)”,
“NSP” (no spindle) and “Off”. It is an essential input to the “most likely nose vector” calculation.
Spindle Side: This field specifies whether the spindle is mounted on the left or right side of the machine. It is an
essential input to the “most likely nose vector” calculation.
Mount Direction: This field specifies how the tool is mounted. Possible values are “Vertical” and “Horizontal”. It
is an essential input to the “most likely nose vector” calculation.
Mount Reversal: This field specifies how the tool is mounted. Possible values are “Normal” and “Reversed”. It is
an essential input to the “most likely nose vector” calculation.
Hand of Tool: This field specifies whether the tool is left-handed, right-handed or neutral. The hand of tool is
defined as the general direction the insert points when the tool is held flat in your hand; insert side up and facing
you. It is an essential input to the “most likely nose vector” calculation. Due to the geometry of some inserts such
as grooving and cutoffs, you should use the direction of cut as a guide to setting the hand rather than using the strict
definition of handedness. To get the “most likely vector” to match your actual nose vector, you should choose
“Neutral”.
Vector: This field specifies how the tool is oriented in the machine. It is the same as the Nose Vector field in the
Offset Library screen. See the section titled “Setting the Nose Vector” later in
this chapter for a more in-depth explanation. To the right of the vector field are
two pictures that display the most likely orientation and most likely nose vector,
respectively. These pictures are chosen based on the values that you selected for
Approach, Spindle Direction, Spindle Side, Mount Direction, Mount Reversal and Hand of Tool. The most likely
nose vector is shown in black. The next most probable vectors are shown in red. This feature is provided as an aid
to selecting the correct nose vector. It should be used as a guide and secondary check only. Never blindly set the
vector based on this value. You must select the actual nose vector and enter it into the vector field. The value that
you enter will most probably be exactly what is displayed as the “most likely” nose vector. If not exact, the vector
that you enter will probably be a vector with a similar orientation, such as the vectors displayed in red. As
discussed in “Hand of Tool”, the most likely vector for grooving and cutoffs will not match the true nose vector if
the strict definition of handedness is used.
Nose Radius: This field tells the control the distance to adjust when cutter diameter compensation (G41 or G42) is
activated. It is the same field found in the Tool Offset library.
Coolant: This field specifies a default coolant type to use with each tool. Possible values are FLOOD, MIST, or
OFF. Lathe Intercon uses this information to automatically insert M7 or M8 after a tool change. To change the
value, press SPACE bar until the desired value is shown.
X Offset: This field defines the X offset distance away from the tool measurement radius or diameter. (See X
Diameter/Radius as described below.) The field is the same as the Offset X field in the Offset Library but the
automatic measurement procedure is slightly different. Either cursor over to the X Offset field or press F1 to jump
directly to it. Follow the instructions.
Z Offset: This field defines the Z offset distance away from the Z reference position. (See Z Ref as described
below.) The field is the same as the Offset Z field in the Offset Library but the automatic measurement procedure
is slightly different. Either cursor over to the Z Offset field or press F2 to jump directly to it. Follow the
instructions.
X Diameter/Radius: This field defines the diameter or radius from which the X tool offsets are to be measured.
This diameter is usually created by a skim cut as part of the tool measuring procedure. (See the Procedures for
Setting Tool Offsets section later in this chapter.) To change this field, cursor over to the X Diameter/Radius field
(or press F3) and follow the instructions.
T-Series Operator’s Manual
5/18/2011
4-5
Z Ref: This field is the Z reference position from which the Z offsets of tools are to be measured. To change this
field, cursor over to the Z Offset field (or press F4) and follow the instructions.
Note: Instructions are displayed when you move the cursor to the X Offset, Z Offset, X Diam/Radius and Z Ref.
Fields. These instructions cannot be dismissed. Use the arrow keys to move to another field.
F1 – X Offset / Set X Off
When the cursor is anywhere except the X Offset field, the F1 button reads “X Offset”. Press F1 in this case to
jump directly to the X Offset field and display instructions. When the cursor is on the X Offset field, the F1 button
changes to “Set X Off”. Press F1 in this case (per instructions) to set the current position as the X offset.
F2 – Z Offset / Set Z Off
When the cursor is anywhere except the Z Offset field, the F2 button reads “Z Offset”. Press F2 to jump directly to
the Z Offset field and display instructions. When the cursor is on the Z Offset field, the F2 button changes to “Set
Z Off”. Press F2 in this case (per instructions) to set the current position as the Z offset.
F3 – X Diam/Rad
Press this key to jump directly to the X Diameter/Radius field and display instructions.
F4 –Z Ref / Set Z Ref
When the cursor is anywhere but the Z Ref field, the F4 button reads “Z Ref”. Press F4 in this case to jump
directly to the Z Ref field and display instructions. When the cursor is on the Z Ref field, the button changes to
“Set Z Ref”. Press F4 in this case (per instructions) to set the current position as the Z Reference.
F7 – Prev Tool
Displays the information for the previous tool, to confirm settings or make changes.
F8 – Next Tool
Displays the information for the next tool, to confirm settings or make changes.
F10 – Save Changes
When you are done with modifications press this key to save the changes and return to the Offset Adjustment
screen. F10 will save all changes to all offsets, not just the one currently displayed.
Esc – Abandon Changes
Esc will abandon edits to all offsets that you changed, not just the one currently displayed.
Procedures for Setting Tool Offsets: Introduction
Follow these five steps to successful CNC turning:
1.
2.
3.
4.
5.
Determine the tools necessary to machine the part by analyzing the print.
Set the X and Z offsets for each tool. (This Chapter)
Program the part-using Intercon. (Chapter 8, Lathe Intercon Manual)
Set the X and Z Part Zero positions on the stock to be machined. (Chapter 5)
Graph the part to check for programming errors, and machine the part.
Tool offsets let the control know the difference in position for each tool being used. Since different tools are at
different positions, each tool will have its own specific offset value in X and Z. For a multi-tool job, it is critical
that the X and Z offsets for each tool are set at the proper values.
We will use the control to determine the difference in location of each tool by simply defining a position from
which to measure each individual tool. The easiest method is to make a skim cut and then touch each tool off of the
4-6
11/18/02
T-Series Operator’s Manual
newly measured skim cut diameter. The control will record the distance that each tool had to move to touch off the
known diameter. Once the X and Z offset information is known for each tool, a multi-tool program can be run with
success.
Before doing the procedures in the ensuing sections, make sure:
1. The “Entry Mode” field in the Offset Library is toggled to “absolute”.
2. The control is in Diameter mode (set Machine Parameter 55 to 0)
3. The adjustment values in the Tool Offset Adjustment Screen (described earlier in this chapter) are all
zeroed out for the tools, which will be involved in the measurement process.
The following instructions show how to set offsets using the Offset Library screen. You may also use the Tool
Details screen to set offsets. The details of entering the offset values are different on the Tool Details screen.
Otherwise, the procedures are identical.
Setting X-Axis Tool Offsets for OD Tools.
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be all zeroed out for the tools which will be involved in the steps below.
STEP 1:
Chuck up a piece of stock, and use the Jog buttons to make a skim cut (Figure 1). Leave the tool set at this X
position.
● NOTE: Start spindle by switching to manual mode, press Spin Start button, and adjust RPM with the spindle
override knob.
=1.8721”
Figure 2
Figure 1
STEP 2:
Measure the new skim cut diameter, as shown in Figure 2.
STEP 3: Open the Offset Library
On the T-Series Control Main Screen, press: F1-Setup ➞ F2-Tool ➞ F1-Offset Lib.
STEP 4: Set the X Measurement Diameter
Press F1-X Diam and enter the diameter measured in Step 2 into the “Establish the X Diameter field”, then press
F10-Save to accept. The X-Measurement Diameter for OD tools is now set.
T-Series Operator’s Manual
5/18/2011
4-7
Figure 3
STEP 5: Measure the X-Offset
Press F2-Meas. to measure the X-offset of the tool used to make the skim cut. The value appears in the X Offset
field.
Figure 4
NOTES:
● Always make sure the cursor is on the X offset field for the offset number that you are measuring. For instance, if
you are using tool #1, make sure the cursor is in the X offset T01 position BEFORE pressing F2-Meas.
● Press F2-Meas. while the tool is STILL at the skim cut diameter.
● Any piece of stock can be used to set tool offsets. It is not necessary to use the actual part blank.
STEP 6: Measure the Next Tool
Touch the next tool to the new skim cut OD (the X Measurement Diameter) as shown in Figure 5, and press F2Meas. Repeat this step for the rest of your OD tools.
4-8
11/18/02
T-Series Operator’s Manual
For each new OD tool:
Touch off X diameter
and press F2-Measure
Figure 5
NOTES:
● Verify you are clear of any obstacles, then use “Tool Check” to withdraw the tool from its current position.
● Use a piece of paper to touch off the next tool to the skim cut diameter. Slow jog close to the work piece, switch
to Incremental jog mode and jog in close at small increments until the tool just pins the paper to the work piece.
● If you are using an ATC, be sure that you are clear of any obstacles, then use the ATC button in the Tool Library
to rotate the ATC to the next tool position.
Setting X-axis Tool Offsets for ID Tools
After setting all OD Tool Offsets, a new Internal X Measurement Diameter should be set to measure the X offsets
for all ID Tools.
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be all zeroed out for the tools which will be involved in the steps below.
STEP 1:
Chuck up a piece of stock, and use the Jog buttons to make a skim cut (Figure 6). Leave the tool set at this X
position.
● NOTE: Start spindle by switching to manual mode, press Spin Start button, and adjust RPM with the spindle
override knob.
= 1.3344”
Figure 7
Figure 6
STEP 2:
Measure the new skim cut diameter, as shown in Figure 7.
STEP 3: Open the Offset Library
On the T-Series Control Main Screen, press: F1 - Setup ➞ F2 - Tool ➞ F1 - Offset Lib.
STEP 4: Set the X Measurement Diameter
Now press F1 - X Diam, enter the diameter measured in Step 2 into the Establish the X Diameter field, and press
F10 - Save to accept. The X-Measurement Diameter for ID tools is now set.
T-Series Operator’s Manual
5/18/2011
4-9
Figure 8
STEP 5: Measure the X-Offset
Press F2 - Meas. to measure the X-offset of the tool used to make the skim cut. The value appears in the X Offset
field.
Figure 9
NOTES:
● Verify the cursor is highlighting the X offset field for the offset number that you are measuring. For instance, if
you are using tool #5, make sure the cursor is in the X offset T05 position BEFORE pressing F2 - Meas.
● Press F2 - Meas. while the tool is STILL at the skim cut diameter.
4-10
11/18/02
T-Series Operator’s Manual
STEP 6: Measure the Next Tool
Touch off all internal tools on this new internal diameter and press F2 - Meas. to measure each one. Repeat this
step for all the remaining ID tools (Figure 10).
For each new ID tool:
Touch off X diameter and
press F2[measure].
Figure 10
NOTES:
● Make sure you are clear of any obstacles, then use “Tool Check” to withdraw a tool from its current position.
● Use a piece of paper to touch off the next tool to the skim cut diameter. Slow jog close to the work piece, switch
to Incremental jog mode and jog in close at small increments until the tool just pins the paper to the work piece.
● If you are using an ATC, move the ATC away from any obstacles, then use the ATC button in the Tool Library to
index to the next tool position.
Special Cases: Sometimes it might be difficult to touch a new tool off the X Measurement
Diameter set in Step 2. If this is the case, you can repeat each step from Step #1 through 5 for
EACH tool, reading in a new reference position for EACH tool! In this case, you will make a new
skim cut Measurement Diameter for each tool and enter in that new skim cut diameter as a new
reference position for that tool. This method is more work, but if touching off a new tool to an
existing reference position is very difficult, this method may be used for both OD & ID tools.
T-Series Operator’s Manual
5/18/2011
4-11
Setting X-Axis Offsets for Drills, Center Drills, and Taps
To set drills, center drills, taps, and boring tools, sweep the tool in with an indicator to find the spindle center.
Remember that the X Measurement Diameter should be set to ‘ 0 ‘ before proceeding with step 1. (See the section
“Setting X-Axis Tool Offsets for OD Tools” earlier in this chapter for directions on setting an X Measurement
Diameter)
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be all zeroed out for the tools which will be involved in the steps below.
STEP 1: Set the Indicator
Mount the indicator base on the spindle or put the indicator in the chuck. Move the tool towards the approximate
center of the spindle. (Figure 11)
Figure 11
STEP 2: Center the Drill
Touch the indicator probe to the shank of the tool, and rotate the chuck by hand. Jog the X-axis in incremental
mode until the indicator reads the same around the circumference of the tool.
STEP 3: Measure the X Offset
Press F2 – Meas. to measure the X-offset of the tool. The value appears in the X Offset field.
● NOTE: This procedure may also be used in setting ID tool offsets in cases where an initial ID skim cut is not
possible.
Setting X-Axis Offsets for Boring Tools
Since boring tools come with a manufactured offset, setting a boring tool is just like setting a drill, with a few added
steps. Follow Steps 1 to 3 in the previous section above, and then do the following steps:
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be all zeroed out for the tools which will be involved in the steps below.
STEP 4: Find the Tool Offset
Look up the tool manufacturer’s offset for the tool being measured.
STEP 5: Switch to Incremental mode
With the X Offset field highlighted for the tool being measured, press the F4 - Abs/Inc key until the “Entry Mode:”
field on the screen reads “incremental”.
STEP 6: Enter the Given Offset
Multiply the manufacturer’s offset by negative two (–2), and type the number into the X Offset field. The value
you type should appear as being added to the measured X offset already measured.
● NOTE: Remember to press the F4 - Abs/Inc key to toggle the Entry Mode back to “absolute” when you are
done.
4-12
11/18/02
T-Series Operator’s Manual
Setting Z-Axis Tool Offsets
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be all zeroed out for the tools which will be involved in the steps below.
STEP 1:
Chuck up a piece of stock, and use the Jog buttons to make a skim cut (Figure 12) OR if the surface is true, touch
off the end as shown in Figure 13.
Z Reference
STEP 2: Open the Offset Library
From the T-series Control Main Screen, press: F1 - Setup ➞ F2 - Tool ➞ F1 - Offset Lib.
STEP 3: Set the Reference:
Make sure the Z column is highlighted, press F1 - Z Ref. and then F10 - Save to accept this as the reference.
STEP 4: Measure the Tool Offset
Without moving the Z-position of the tool that you just used to set a reference point, press F2 - Meas. to measure
the Z-offset of that tool (it should result in 0 as its offset), as seen in figure 14.
Figure 14
T-Series Operator’s Manual
5/18/2011
4-13
STEP 5: Measure the Next Tool Z-Offset
Load the next tool and bring it to the reference point (as shown in Figure 13). Press F2 - Meas., and then repeat for
all remaining tools.
● NOTE: Make sure the cursor is on the Z-Offset field for the Offset number being measured before pressing F2 Meas.
Setting Part Cutoff Tool Z-Offset:
● NOTE: Before you begin, the adjustment values in the Tool Offset Adjustment Screen (described earlier in this
chapter) should be zeroed out for the tools that will be involved in the setup as described below.
Load the part cutoff tool and bring it to the stock face (Figure 15). With the menu highlighted in the Z Offset
column at the correct offset number, press the F2 – Meas. key.
Figure 15
If the part cutoff tool is 0.125 wide and you want the back side of the tool to be set at Z-Zero, then highlight the Zoffset of the tool being adjusted and press the F4 - Abs/Inc key to toggle to incremental mode.
Figure 16
Type in -.125 and press ENTER. The value of -0.125 will be added to the value measured in Step 1.
● NOTE: Remember to press the F4 - Abs/Inc key to toggle the Entry Mode back to “absolute” when you are
done.
4-14
11/18/02
T-Series Operator’s Manual
Setting the Nose Radius
The Offset Library also has a field for the tool Nose Radius. This field tells the control the distance to adjust when
cutter compensation is used (G41 or G42). For more details, see Chapter 11.
Figure 17
To edit these entries, first press the F4 - Abs/Inc until the “Entry Mode” field reads “absolute”. Move to the
desired Nose Radius field using the arrow keys and type in the nose radius of the tool, and press Enter.
Setting the Nose Vector
Entering Nose Vector for your tool will tell the control how that tool is oriented in the machine. This is needed for
calculating cutter compensation and for determining how to retract the tool during cutting cycles.
First, highlight the nose vector column for the number of the tool being used. Then enter the correct nose vector as
indicated by the graphic display on the right side of the screen.
Figure 18
T-Series Operator’s Manual
5/18/2011
4-15
For tools approaching from the +X direction nose vectors 3, 8, and 4 are used for OD turning and nose vectors 2, 6,
and 1 are for ID boring. For machines that have both front and rear mount tooling (+X and –X tooling), such as
gang tool lathes, the tools approaching from the -X direction use nose vectors 2, 6, and 1 for OD turning and nose
vectors 3, 8, and 4 are for ID boring. Nose vector 5 is used for back facing and nose vectors 7 and 0 are used for
drilling. Nose vectors 5, 7 and 0 will stay the same even if your tool post is mounted on the front or the rear of the
machine.
4-16
11/18/02
T-Series Operator’s Manual
Chapter 5
Part Zero and WCS
Part Zero Menu
To get to the Part Zero menu from the Main Screen press F1 – Setup then F1 – Part.
The Part Zero menu fields and screen elements are described below:
Axis: This field shows which axis the Part Zero is being set up for. When the Part Zero menu is first brought up,
the Z axis will be shown. Press F8 – Set X to access the Part Zero menu for the X axis.
Position: This field allows you to establish a non-zero offset between where the tool is and where you want the
origin to be. On the X-axis, this is either a diameter or radius distance away from the part centerline that the tool tip
is touching.
● NOTE: The part centerline is usually considered to be where the X axis position is 0.
Tool Number: This field allows you to tell the control what tool offset number (see the Offset Library in Chapter 4)
is being used while setting the Part Zero position. Although this number is called a “Tool Number”, this is not a
tool number. However, if you only associate tool numbers with the same numbered offset, then this field would
correspond to the tool number.
● NOTE: The Offset Library must be up to date before setting the Part Zeroes.
T-Series Operator’s Manual
5/18/2011
5-1
Set All WCS: This field appears only if you are modifying the Part Zero for the X axis.
Press <SPACE> to toggle between “Yes” and “No”. If this field is toggled to “Yes” then this field specifies that
the position that you enter will be copied to all the X axis Part positions in every Work Coordinate System. This
will cause all Work Coordinate systems to have the same X axis Part Zero. This feature is a convenience, since the
centerline position of a part is usually set at X=0, regardless of which WCS is currently active. If this field is
toggled to “No” then only the currently selected WCS will be affected.
F6 – Previous WCS
This key will select the previous Work Coordinate System. If you will be using multiple work coordinates, you
must set up a new set of Part Zeros for each work coordinate. Each work coordinate represents a different Part
Zero. You can use this key to cycle through all available Work Coordinate Systems. Note that WCS #1-6 are
standard, but WCS #7-18 are an extra-cost option.
F7 – Next WCS
This key is like the F6 – Prev WCS key (see above) except that this key will cycle forward to the next work
coordinate system. You can use this key to cycle through all available Work Coordinate Systems. Note that WCS
#1-6 are standard, but WCS #7-18 are an extra-cost option.
F8-Set X
To get access to the Part Zero menu for the X axis, press F8 – Set X. Setting the X axis Part Zero is given special
treatment in a sub-menu because it is not done very often (See the section titled “Setting X Axis Part Zero” later in
this chapter).
F9 - WCS
Pressing this key will bring up the WCS Configuration menu, which will let you conveniently view and modify the
Work Coordinate Systems. See the WCS Configuration Menu section for a further explanation.
F10 – Set
Pressing this key will cause the part position that you entered to be set.
5-2
5/18/2011
T-Series Operator’s Manual
Setting Part Zeros - Introduction:
Setting the Part Zero for a part establishes a local coordinate system with its origin at the centerline of the part. In
T-Series controls, this coordinate system considers X+ as always pointing away from the centerline and Z+ always
pointing to the right and away from the spindle.
Setting Z-Axis Part Zero (Z0)
STEP 1:
Jog the tool to the stock surface and take a skim cut across the face (Figure 1), or touch off of the known surface
(Figure 2) and leave the tool setting at this Z position.
● NOTE: In the case of Figure 1, start the spindle by switching to manual mode, press Spin Start button, and adjust
RPM with the spindle override.
STEP 2:
On the T-Series Control, from the Main Screen, press F1 – Setup then F1 – Part. This will bring you to the Z-axis
Part Zero menu.
STEP 3:
Type 0.000 (or the known position of the surface you are touching off) into the Part Position field. Press Enter.
● NOTE: If, for example, you need to take a 0.05” face cut off of your part, type 0.05 into the Part Position field on
the menu. Z-Zero will now be 0.05” deeper into the part from the existing face.
T-Series Operator’s Manual
5/18/2011
5-3
STEP 4:
Enter the Tool Number of the tool being used, and then press the F10 – Set key. Part Zero is now set for the Z-axis.
All the other tools set up in the Tool Library (Chapter 4) are now automatically set to this new Z-axis Part Zero.
Setting X-Axis Part Zero (X0)
● NOTE: Since the X axis Part Zero is usually defined to be the Centerline of the part, there is usually no need to
set it up again when doing a different part. An ideal situation would be that you program all parts to have a
Centerline of X=0, and thus you would need to set up the X axis Part Zero for every WCS only one time during the
whole life of the machine.
STEP 1:
Chuck up the stock to be machined. Jog the reference tool (in this case, an OD turning & facing tool) to the stock
surface and take a skim cut across the surface (Figure 3), or touch off of the known surface (Figure 4) and leave the
tool setting at this X position.
● NOTE: In the case of Figure 3, start the spindle by switching to manual mode, press Spin Start button, and adjust
RPM with the spindle override.
STEP 2: Measure the resulting diameter
On the T-Series Control, from the Main Screen, press F1 – Setup, F1 – Part, then F8 - Set.
F6 – Prev WCS and F7 – Next WCS keys can be used to select the work coordinate.
● NOTE: There are 18 different work coordinates that can be used (1 through 6 are standard; 7 through 18 are an
extra-cost option). See “Setting a WCS” later in the chapter.
5-4
5/18/2011
T-Series Operator’s Manual
STEP 3:
Enter the OD measurement taken in Step 2 into the Part Position field, and press Enter.
● NOTE: Depending on how your control is set, this value can be a diameter or a radius. See Chapter 14, Machine
Parameter 55 for further details.
STEP 4:
Enter the Tool Number of the tool being used, and then press the F10 - Set key. Part Zero is now set for the X-axis.
All the other tools set up in the Tool and Offset Libraries (Chapter 4) are now automatically set to this new X-axis
Part Zero.
OPTIONAL STEP:
If you want all Work Coordinate systems to have the same X axis Part Zero, then toggle the “Set all WCS” field to
“Yes” and press F10 - Set. This will copy the position that you entered to all the X axis Part positions in every
Work Coordinate System. This feature is a convenience, since the centerline position of a part is usually set at
X=0, regardless of which WCS is currently active.
T-Series Operator’s Manual
5/18/2011
5-5
WCS Configuration Menu
To get to the WCS Configuration menu from the Main Screen, F1 – Setup, F1 – Part, then F9 – WCS Table.
When you enter this screen, the DRO display will automatically switch over to machine coordinates as an aid to
entering numbers. All the values on this screen are represented in machine coordinates. X values are radius
dimensions, even if the machine is in diameter mode (set in Machine Parameter 55). Note that WCS #1-6 are
standard, but WCS #7-18 are an extra-cost option.
There are 2 sections in this menu, Reference Return Points and the Work Coordinate Systems, which define the
individual Part Zeros.
F1 – Reference Return Points 1, 2, 3, and 4
This option will let you modify the positions of the reference return points (in machine coordinates). See G30 in
Chapter 11 for more information on how to use these return points.
The G28 position (Return #1) is of interest because it specifies the Tool Check position and the usual Tool Change
position. The Tool Check position is the machine coordinate position that the machine will move to when the
TOOL CHECK button is pressed. Also, the G28 position is the usual position at which tool changes occur during
a job run. You can change the G28 position if you would like the Tool Check position and tool changes to occur
somewhere else.
F2 – Origins of Work Coordinate Systems
This option lets you specify the locations (in machine coordinates) of the origins of the work coordinate systems.
However, the preferred method for setting these values is to use the Part Zero Setup screen. The other 12 work
coordinate systems are viewed by pressing F1 – Next Table.
5-6
5/18/2011
T-Series Operator’s Manual
Using Work Coordinate Systems
These different part zero positions are typically used to reduce setup and/or programming time. There are a number
of creative ways the WCS can be used to simplify lathe machining. The 18 work coordinates and the G-codes are
shown below. Regular WCS #1-6 are standard, but extended WCS #7-18 are an extra-cost option.
Regular WCS
WCS
G-Code
G54
WCS #1
G55
WCS #2
G56
WCS #3
G57
WCS #4
G58
WCS #5
G59
WCS #6
Extended Work Coordinate Systems
WCS
G-Code
WCS
G-Code
G54 P1
G54 P7
WCS #7
WCS #13
G54 P2
G54 P8
WCS #8
WCS #14
G54
P3
G54 P9
WCS #9
WCS #15
G54 P4
G54 P10
WCS #10
WCS #16
G54 P5
G54 P11
WCS #11
WCS #17
G54 P6
G54 P12
WCS #12
WCS #18
At any time that you see the Digital Read Out (DRO) for the X and Z current position, you will see a display of
which WCS the control is currently using in the upper left hand corner of the screen right above the DRO (See the
figure below). The DRO always displays the tool position from the WCS that is being used.
T-Series Operator’s Manual
5/18/2011
5-7
WCS currently in
use is shown on
most menus
F6 – Prev WCS
and
F7 – Next WCS
switch to another
WCS
To change the WCS being used:
● From the T-series control Main Screen, press: F1 – Setup, F1 - Part.
● Now press F6 – Prev WCS or F7 – Next WCS, and the WCS number will change in the upper left corner of the
display.
The WCS will change to the next position - if you were on WCS#1 and press F7 – Next WCS, it will change the
DRO to WCS#2. Simply press F6 – Prev WCS or F7 – Next WCS until the WCS displayed is the one you want to
use. After that you can set up the new WCS using the part setup menus for X and Z to define a new Part Zero
position with this WCS. See the section “Setting Part Zeros” in this chapter and the two sections after that for stepby-step instructions of how to zero out your part. Once a WCS is set, the control will remember this position as the
Part Zero for that WCS until you change it, even if the control is shut off.
F3 – Work Envelope
Use the F3 – Work Envel key to specify the ‘+’ ‘-‘ work envelope locations (in machine coordinates) used in
conjunction with the G22 G code. The Z, X and I, J parameters specified in the G22 code are stored here, so
subsequent G22 codes do not need to specify the limits unless they change.
Note: The work envelope will only work in programmed moves. You will still be able to jog outside of the work
envelope.
5-8
5/18/2011
T-Series Operator’s Manual
Chapter 6
Running a Job
To run the current job, press the CYCLE START button on the jog panel. See Chapter 2 for a description of the
CYCLE START button. If your control is not equipped with a jog panel, press ALT-S on the keyboard. The
following menu is available, while the job is running.
Job running menu
The following keys are available while the job is running.
F1 – Feed (-1%)
Decrease feedrate override by 1%. This key only appears if jog panel is set to keyboard jogging.
F2 – Feed (+1%)
Increase feedrate override by 1%. This key only appears if jog panel is set to keyboard jogging.
F3 – Repeat On/Off
Toggle job repeat property.
F4 – Skips On/Off
Enable/Disable block skips.
F5 – Auto
Disable single block mode.
F6 – Stops off
Disable optional stops.
F7 – Feed Hold
Turn feed hold on/off. This key only appears if jog panel is set to keyboard jogging.
T-Series Operator’s Manual
5/18/11
6-1
F8 – Graph
Return to run-time graphics screen. This key only appears if the run-time graphics option is turned on.
F9 – Rapid On/Off
Turn rapid override on/off.
Canceling a Job in Progress
There are three conventional ways to cancel a currently running job (CNC program). When a job is canceled using
any of the following methods, the job's progress will be recorded. This allows the user to restart the job using the
Resume Job option or the Search and Run option.
CYCLE CANCEL
Pressing this key while a job is running will cause the control to abort the currently running job. The control will
stop movement immediately, clear all M-functions, and return to the main screen. Hitting the escape key on the
keyboard is the equivalent to hitting “CYCLE CANCEL.”
TOOL CHECK
Pressing this key while a job is running will cause the control to stop the normal program movement, turn off the
spindle, clear all M-functions, and go the Run menu screen. Make sure the tool will clear the part before pressing
Tool Check a second time, which will move the X and Z-axes to their home position. The control will then
automatically go to the resume job screen.
EMERGENCY STOP (E-Stop)
Pressing the EMERGENCY STOP button while a job is running will cause the control to abort the currently
running job. The control will stop movement immediately, clear all M-functions, and return to the main screen.
Also, the power to all axes will be released.
Resuming a Canceled Job
If a job is canceled using one of the methods described above, it can be resumed in one of three ways.
CYCLE START
Pressing the CYCLE START button will restart the job at the BEGINNING of the part program.
Note: Before performing a F1-Resume Job or F2-Search the tool may need to be positioned in X and Z for cycles
that start down inside an ID or behind a shoulder.
Resume Job – F1 from the Run menu
Restart the canceled job at or near the point of interruption. See the next section in this chapter entitled “Run
menu” for more information.
Search – F2 from the Run menu
Restart at a specified point in the part program. See the next section in this chapter entitled “Run menu” for more
information.
6-2
5/18/11
T-Series Operator’s Manual
Run menu
Press F4-Run from the main screen to access the Run menu. From this menu, the operator can restart a canceled
job or change the way the job will run.
F1 - Resume Job
Press F1-Resume Job in the run screen to go to the resume job screen. If the job was canceled by pressing Tool
Check, the control will go to the resume job screen automatically. From this screen, the user can modify tool
offsets and the tool library, turn single block mode on and off, turn optional stops on or off, graph the partially
completed job, or start the partially completed job.
The resume job option is not always available. The following situations will cause the resume job option to be
unavailable:
Loading a new job.
Running a job to completion.
Parse errors in the job.
Editing or reposting the job file.
Loss of power while a job is running.
F2 - Search
Invoking this option will bring you to the “Search and Run” menu. This menu will allow you to specify the
program line, block number, or tool number at which execution of a program is to begin. Program lines are
numbered from the top of the file down with the first line numbered 1. To enter a block number place an "N" in
front of the number. To enter a tool number place a "T" in front of the number. Pressing CYCLE START from
here would start the program at the point you specified.
An extra option unique to the “Search and Run” screen is the F1-Tool Change “Do Last Tool Change” function.
This key toggles the tool change option as shown on screen. A "YES" tells the control to perform a tool change so
that the tool specified for the line or block has the tool indicated in the program. A "NO" uses the currently loaded
tool, regardless of what tool is specified for the line or block being searched.
NOTE: You cannot search into a subroutine.
T-Series Operator’s Manual
5/18/11
6-3
F3 – Repeat On/Off
This key toggles the repeat feature for part counting. When part counting is in effect and Repeat is on, the job will
be automatically run again until the specified number of parts have been run. The On or Off label indicates the
state to which the repeat feature will toggle to when pressed. It does not indicate the current state. The current
state is indicated in the user window above.
Part Count: this prompt is used to set the required number of parts. Positive values set the part counter to count up
and negative values configure the part count to count down. For example, if 10 is entered in the Part Count prompt,
the Part Cnt in the status window changes to 10 and the Part # changes to 0 with an upward arrow indicator. When
a job is completed, the Part # will increment to 1. If repeat is on, the job will automatically start again and keep
running until the Part # has reached the Part Cnt. If a –10 is entered in the Part Count prompt, the Part Cnt in the
status window changes to 10 and the Part # changes to 10 with a downward arrow indicator. When a job is
completed, the Part # will decrease to 9 and if repeat is on, the job will automatically start again and keep running
until the Part # has reached 0.
F4 - /Skips On/Off
This function toggles the block skip feature. When block skipping is on, G-code lines that start with a forward
slash character ‘/’ are skipped (not processed). The On or Off label indicates the state the /Skips feature will toggle
to when pressed. It does not indicate the current state. The current state is indicated in the user window above.
F5 - Block Mode
Turns single block mode on and off. This is similar to pressing AUTO/BLOCK. If single block mode is on,
CNC11 will stop after each block in your part program and wait for you to press CYCLE START. The current
state is indicated in the user window above.
F6 - Optional Stops
Turns optional stops on and off. If optional stops are on, any M1 codes that appear in your program will cause a
wait for CYCLE START (just like M0). If optional stops are off, M1 codes will be ignored. The current state is
indicated in the user window above.
F7 - Manual Run
Turns manual run option on and off. This option allows you to manually run a G-code file by turning a single axis
MPG.
F8 - Graph
Graphs the part. For more information, see the "F8 - Graph" section in chapter 3. If this feature is invoked from
the Run and Search screen or the Resume Job screen, then the graphics will show exactly where the searched line or
block begins. Dotted lines indicate the portion of the part that is skipped. Solid lines indicate the portion of the part
that will be machined.
F9 – Rapid On/Off
This function key toggles Rapid Override. The On or Off label indicates the state to which the Rapid Override
feature will toggle to when pressed. It does not indicate the current state. It has the same effect as the Rapid Over
key discussed in Chapter 14.
F10 – RTG On/Off
This function key toggles the Run-Time Graphics option. If the option is turned on, Run-Time Graphics
automatically starts when the CYCLE START button is pressed. This option must be turned on for Run-Time
Graphics to be used. If the option is turned off, Run-Time Graphics cannot be started while a job is running.
6-4
5/18/11
T-Series Operator’s Manual
Power Feed
Press F4-Feed from the Setup menu to access the Power Feed screen. This screen is used to command axis
movement. All the operations available on the Power Feed screen may also be performed in MDI with the
appropriate M and G codes.
F1 - Absolute Power Feed
Press F1-Abs to move an axis to an absolute position, at a specified feedrate.
F2 - Incremental Power Feed
Press F2-Inc to move an axis an incremental distance, at a specified feedrate.
F3 - Free XZ
Press F3-Free to release power to the X and Z motors, allowing you to use your machine manually.
F4 - Power XZ
Press F4-Power to apply power to the X and Z motors, allowing you to use your machine in CNC mode.
T-Series Operator’s Manual
5/18/11
6-5
6-6
5/18/11
T-Series Operator’s Manual
Chapter 7
The Utility Menu
To get to the Utility Menu, press F7 - Utility at the CNC software Main Screen. The model will vary depending on
your M-Series Control model.
F2 – Update
This option is generally used as a facility for updating software. This option can also be
used to restore a previously saved report of the system configuration (See F7 – Report).
F3 – Backup
Use this option to backup your data files such as CNC program files and Intercon
programs.
F4 – Restore
Use this option to restore the data previously backed up with F3 – Backup.
T-Series Operator’s Manual
5/18/11
7-1
F5 – File Ops
Use this menu to perform file and directory operations such as: Importing and
Exporting (copying) files to and from the control, rename or delete files, create or delete
directories.
F1 – Toggle
Press once to select or press again to unselect a single file.
F2 – All /None
Press once to select all or press again to unselect all files.
F3 – Import/
Export
F4 – Edit
Import or Export selected files.
F5 – Refresh
Refresh file list. Use after inserting a new USB storage device
F7 - Rename
Rename selected file or directory.
F8 - New Dir
Create a new directory in the current folder.
F9 - Delete
Deletes selected file or directory.
Page Up
Move the cursor backward one page.
Page Down
Move the cursor forward one page.
End
Select the last file in the list.
Home
Select the first file in the list.
Arrow Keys
Move the cursor in the selected direction.
Opens selected file in editor.
T-Series Operator’s Manual
5/18/11
7-2
F6 – User Maint
Use this menu to perform user maintenance such as checking an axis for excessive drag or setting
backlash
F1 – Drag The Drag Factor utility is used to determine if an axis has an excessive amount of drag. To
run a drag test, use the F1 key to select the axis which you wish to test, position the axis at or near
the home position and press CYCLE START. The axis will move back to the home switch then
traverse the entire range of travel for the axis moving to the opposite limit and returning to home
while moving the slow jog rate. If excessive friction (drag) is encountered an error message will
be displayed. When the test completes, use F8-Graph to display the results. The red horizontal
lines indicate the bounds acceptable limits for the machine as it is currently configured.
F2 - Lash (Backlash Compensation) In order to insure an accurate measurement always set the backlash
compensation in the control to zero before attempting to measure the physical lash in an axis.
F7 – Report
Generates a backup of system configuration files called report.zip and copies it to the
specified location. Your dealer may then use the disk for servicing and troubleshooting purposes.
To restore the configuration files from the report disk, press F2 - Update from the Utility menu.
F8 – Options
Shows the software options that you have purchased or added to your control. On this
screen you can also enter unlock codes for software options that you have purchased. This page
will also display the PLC programs, PIC type, and System ID #.
F9 – Logs
Shows the messages and errors that have been logged by the control.
F1 – Errors Displays the error/message log. Use PgUp, PgDn, Home, & End to view and ESC to exit.
F2- Stats Displays counts of errors logged. Use PgUp, PgDn, Home, & End to view and ESC to exit.
F3 – Export Exports the log to a destination of your choosing.
T-Series Operator’s Manual
5/18/11
7-3
T-Series Operator’s Manual
5/18/11
7-4
Chapter 8
Lathe Intercon
Introduction
Intercon (Interactive Conversational) software for Lathes allows you to quickly create a lathe part program right at
the control without having to be a G-code expert. Intercon will prompt you to enter values from your print that
describes the geometry of the part. Intercon will display graphics of the part as you are creating it, helping you to
quickly proceed through part programming.
Lathe Intercon Main Menu
When you access Intercon through the F5-CAM option in the CNC11 Main screen, the part program will be
displayed if the current job loaded in CNC11 has an associated Intercon program. If the job file in CNC11 did not
have an associated Intercon program, the F1-File menu will be displayed. See the “Lathe Intercon File Menu”
section later on for a description of the file menu.
Intercon Lathe
Current Part: pawn.lth
Operation
End
#
Type
X (D)
Z
0001 ;Demo Lathe Part
0002 ; tool #8 – 55 degree turning tool
0003 ; tool #7 - .125 wide cut off tool
0004 ; not .125 wide change Z tool 7
0005 Facing
0.850
0.1
0.8500
8500
0.1000
0006 G50s4000
0007 Profile
0.7500
0.1000
.7500
1000
- 0.05
0008 Linear
0.1000
.1000
.0500
- 0.0500
0009 Linear
0.0000
0000
0010 Linear
0.0000
0.0000
0.0000
0011 Arc CCW
- 0.3198
0.2658
0012 Arc CCW
- 0.4088
0.3264
0013 Linear
- 0.4837
0.2400
0014 Arc CW
- 1.0375
0.5000
0.5000
0015 Linear, CR
- 1.0375
0.6250
0016 Linear
- 1.1625
0.6250
0017 Linear, CR
- 1.1625
0.7400
0018 Linear
- 1.4850
0.7400
Finish Pass
0019 Finish
0.1000
0.9500
0020 Profile End
0.7500
0.1000
0021 Cutoff
- 1.4750
0.8400
0022 End Prog
- 1.4750
0.8400
Tool
08
07
07
07
07
07
07
07
07
07
07
07
07
08
08
07
07
Status
Stock Diameter
Stock Length
Tool Num/Offset
Nose Vector
Feedrate
Spindle Speed
Spindle Dir.
Cutter Comp
Coolant Type
File
Modify
Insert
Cut
Paste
Copy
F1
F2
F3
F4
F5
F6
Copy
Menus..
F7
X:
Z:
:
:
:
:
:
:
:
0.9000
1.4500
T0808
0
0.0100 F/R
500 CSS
CW
None
Off
Graph
Setup
Post
F8
F9
F10
While in the Lathe Intercon Main Menu, use the up and down arrow keys to highlight the desired operation.
F1 - File
Press F1-File to display the File Menu. See the “Lathe Intercon File Menu” section later in this chapter for a
description of the file menu.
T-Series Operator’s Manual
5/18/2011
8-1
F2 - Modify
Press F2-Modify (or the ENTER key) to make changes to the highlighted operation. This will display the
Edit Operation Menu for the highlighted operation. Use the Page Up and Page Down keys to move
between operations and highlight the operation you want to modify while in the Edit Operation Menu. See
the “Insert Operation” section later in this chapter for a description of each operation type.
F3 - Insert
Press F3-Insert to insert an operation above the currently highlighted operation. See the “Insert Operation”
section later in this chapter for details.
F4 - Cut
Choosing F4-Cut will cut (remove) the highlighted operation from the program. The operation that is cut is
placed onto the clipboard stack. Attempting to cut a profile start or end operation will cut the entire
profile.
F5 - Paste
Choosing F5-Paste will paste the last operation that was cut or copied into the clipboard stack into the
current program line that is before the highlighted operation. A number on the second line of the Paste key
indicates the number of operations that are currently in the clipboard stack. If the top of the clipboard
contains a profile, the entire profile will be pasted.
F6 - Copy
Choosing F6-Copy will copy the highlighted operation into the clipboard stack and advance the cursor to
the next operation.
F7 – Copy Menus…
Choosing F7-Copy Menus… will display these options:
F1-Copy Menu - allows a range of operations to be copied. Specify the Start Block, End Block, and
Destination in the prompts that appear in the Copy Menu. The range of operations is copied into a location
that precedes the destination block.
F2-Move Menu - allows a range of operations to be moved. Specify the Start Block, End Block, and
Destination in the prompts that appear in the Move Menu. The range of operations is moved into a location
that precedes the destination block.
F3-Cut, F4-Paste, F5-Copy perform the same actions as described above.
F9-Clear Clipbrd - removes all operations in the clipboard stack.
F8 - Graph
Press F8-Graph to display a graphic preview for the part. See the “Graphics” section later in this chapter
for details.
8-2
5/18/2011
T-Series Operator’s Manual
F9 - Setup
Press F9-Setup to change the part setup. The following window will be displayed on the screen. Use the up and
down arrow keys to select between fields. Press F1-Toggle to toggle between options when necessary and press
F10-Accept to accept the setup when you are finished. Press the ESC key to cancel and return to the File menu.
Intercon Lathe
Current Part: pawn.lth
Intercon Setup
Comment Generation
Clearance Amount
G71/G72 Cut Depth
G71/G72 Retract Amount
Peck Retract Amount
G74 X Relief Amount
G75 Z Relief Amount
Thread Min. Cut Depth
Thread Chamfer Amount
Chamfer Blend Radius
Spindle Coolant Delay
Max Spindle Speed (G50)
Modal Linear
Modal Arc
Modal
Modal Drill/Bore/Tap
Use G28 for tool change
Help Icons always on
X Coordinate Input Mode
Taper Angle Input Fields
Modal Input Fields
Dro Units
Machine Units
Stop spindle during tool change
Stop coolant during tool change
: Enabled
:
0.10
0.10000
:
0.02500
:
0.00200
:
0.05
0.05000
:
0.00000
:
0.00000
:
0.00100
:
0.00000
:
0.01000
:
3.00
:
0
: No
: No
: No
: No
: No
: Diameter
: No
: No
: Inches
: Inches
: No
: No
Toggle
Accept
F1
F10
Comment Generation: Toggle between Enabled and Disabled. When comment generation is enabled, Intercon
will insert a comment before each block describing the operation type. Disabling comment generation reduces the
size of the file.
Clearance Amount: Set the distance away from the part you want to position when changing from a rapid to a
feedrate move. This amount applies to both the X and Z-axes. Adjust this value to adjust the retract amount in a
threading cycle (G76).
G71/G72 Cut Depth: Enter the amount of material to remove per pass in a profile cycle. Value is always a radius
amount.
G71/G72 Retract Amount: Enter the distance to retract after a cutting pass has been made in a profile cycle. The
values are always a radius amount.
Peck Retract Amount: Enter the distance to retract after a cutting move has been made in the peck drilling cycle,
peck cut off cycle and grooving cycle.
G7x X Relief Amount: Enter the relief amount for the X-axis in a Grooving cycle. This is the amount the tool
moves away from the material in the X-axis direction before making rapid moves to position for the next cut.
T-Series Operator’s Manual
5/18/2011
8-3
F9 – Setup (continued)
G7x Z Relief Amount: Enter the step over amount for the Z-axis in a Grooving cycle. This is the amount the
tool moves away from the material in the Z-axis direction before making rapid moves to position for the next
cut.
Thread Min. Cut Depth: Enter the minimum amount you want removed for a pass in the threading cycle.
Thread Chamfer Amount: Enter the number of turns to taper from the thread depth to the surface of the
work piece.
Chamfer Blend Radius: Enter the radius to use when rounding the corners of a chamfer when blend chamfer
is selected.
Spindle/Coolant Delay: Enter the amount of time in seconds that you want the lathe to wait for the spindle to
get up to speed and the coolant to begin flowing.
Max Spindle Speed (G50): Enter the maximum spindle speed for posted Intercon programs. Posts a G50 at
the beginning of the program if the value entered is greater than zero.
Modal Operations (Linear, Arc, Drill/Tap): Toggle between yes or no. Entering yes will cause the same
type of operation to be automatically inserted after the initial operation has been accepted.
Use G28 for Tool Change: Toggle between yes or no. Entering “yes” will cause Intercon to post a G28 on a
tool change operation to return the tool to the G28 position. Gang tooling setups usually require this option to
be set to “no”.
Help Icons always on: Toggle between yes or no. Selecting “yes” means that help information will always
be displayed when editing operations. “No” means that you will have to press a key to get help. Whether set
to “yes” or “no”, help screens can always be toggled on or off by pressing the F5-Help key when editing an
operation.
X Coordinate Input: Toggle between radius and diameter. You can select to enter the coordinates as radius
amounts or as diameter amounts.
Taper Angle Input Fields: Toggle between hide and display. When you select hide, the fields that
correspond to polar coordinates will not be shown. When you select display, the fields that correspond to
polar coordinates will be shown.
Modal Input Fields: Toggle between hide and display. When you select hide, modal fields will not be
shown. When you select display, modal fields will be shown.
Stop Spindle During Tool Change: Toggle between Yes and No. Select “Yes” if you want the spindle to be
shut off during a tool change. Select “No” if you want the spindle to be left on while doing a tool change.
Stop Coolant During Tool Change: Toggle between Yes and No. Selecting “Yes” will cause the coolant to
be shut off during a tool change. Selecting “No” will cause the coolant to be left on while doing a tool change.
F10 - Post
Press F10-Post to post a part program. Posting a part program generates the G-codes for the program. After the
program is posted, you will be returned to the control software’s Main Screen where the G-code program will be
loaded and you can press CYCLE START to run the job. The Intercon program will be automatically saved.
8-4
5/18/2011
T-Series Operator’s Manual
Esc - Quit
Press Esc to quit Intercon. You will be prompted to save changes if any were made. You will be returned to the
control software’s Main Screen.
Teach Mode
The X and Z keys will fill in a field with the current position for the related axis. This feature works when editing
most fields in an operation. Press F9-Teach Mode when editing an operation to display a DRO.
Lathe Intercon File Menu
Press F1-File while in the Intercon Main Menu to access the File Menu. The screen will look something like the
example below:
Intercon File Menu
Intercon Lathe
Directory: c:\
c:\icn_lathe
File
[[ c:\
c:\]
[[..]
Pawn
Shaft
Pipethread
Current Part: pawn.icn
Programmer
Description
John Q. Public
John Q. Public
John Q. Public
Drive
Parent directory
Demo Pawn Part
Demo Shaft Part
Demo Pipe Thread Part
New
Load
Save
F1
F2
F3
Save
As
F4
Date Modified
0606-OctOct-2006
0606-OctOct-2006
0606-OctOct-2006
Details
On/Off
F9
Delete
F5
F1 - New
Press F1-New to create a new file; you will be prompted to save changes to the currently loaded part program.
Press “Y” to save changes or”N” to continue without saving changes. Choosing F1-New will display the “New
file:” prompt above the function keys. Type the name of the new file, then press F10-Accept or the ENTER key to
accept the new name. After accepting the new name, the program header information can be entered.
T-Series Operator’s Manual
5/18/2011
8-5
F2 - Load
Press F2-Load to load an existing program. You will be prompted to save changes to the currently loaded
part program. Press “Y” to save changes or “N” to continue without saving changes.
p
p
pp
Load file from CNC hard drive c:\
c:\icn_lath
Use arrow keys to select file to load and press F10 to Accept.
File
[..]
pawn
annyanny-en2
pipethread
Programmer
Description
Date Modified
John Q. Public
John Q. Public
John Q. Public
Parent directory
Demo Pawn Part
Demo Encoder Shaft
Demo Pipe Thread
0606-OctOct-2006
0606-OctOct-2006
0606-OctOct-2006
1919-NovNov-2006
Job to load? bracket.cnc
G code
/ICN
F1
Floppy
/USB/LAN
F2
Details
On/Off
F3
Show
Recent
F4
Date/
Alpha
F5
Edit
F6
Help
On//Off
On
F7
Graph
F8
Advanced
F9
Accept
F10
F1
0
Load Menu
To navigate the files in the load menu, use the arrow keys to move the cursor around and highlight the file
to be loaded. The HOME, END, PAGE UP and PAGE DOWN keys can be used to navigate the list of
files. Names that are bracketed, for example [..], are the names of directories in the current directory, which
is displayed at the top of the screen.
It is also possible to load a file by typing the name of the program to be loaded. When typing has started,
the characters appear in the “File to load:” prompt above the function keys. Different drives and directories
can be accessed by typing in the path at the “File to load:” prompt, or by pressing F10 or ENTER on a
bracketed directory name. When loading a new file, a prompt will be displayed asking whether to save the
existing file if there was one.
Additional viewing and loading options are available through the F-Key menus which are detailed below:
F1 – G code/ICN
Allows user to toggle the view between the Intercon files present in either c:\icn_lath or c:\cnct\ncfiles.
F2 – Floppy USB/LAN
Provides options for loading Intercon files from USB devices, floppy and LAN drives.
F3 – Details On/Off
The F3 - Details On/Off option changes the format of the display such that each file or directory is on a
separate line and there are columns displayed for Programmer, Description, and Date Modified, i.e., the
information that is contained in the program header operation.
8-6
5/18/2011
T-Series Operator’s Manual
Load Menu (continued)
F4 – Show recent
Use the F4 – Show Recent option to show the 15 most recently loaded Intercon and g-code files. It is important to
remember that even though g-code files are displayed on this screen, ONLY Intercon files should be loaded from this
screen. WARNING!!! Attempting to load a g-code file from the “Show Recent” screen will cause an error which will
discard the current Intercon program. All unsaved changes will be lost. If you should accidently load a g-code file,
press escape to return to the main Intercon menu.
F5 – Date/Alpha
Use F5 Date/Alpha to view files either alphabetically or by date modified. By default, programs are listed in
ascending alphabetical order.
F6 – Edit
Opens the selected file in Intercon for editing.
F7 – Help On/Off
Displays on screen help for the load menus.
F8 – Graph
Graphs the selected file.
F9 - Advanced
Displays file menu in a comprehensive “all in one” format similar to Windows Explorer
File Menu (continued from pg 7-6)
F3 - Save
Press F3-Save to save the current part program under its current name.
F4 - Save As
Press F4-Save As to save the current part program under a different name or to a different drive/directory. This
allows you to make changes to a program and save the file under a different name so the original program remains
unchanged. The name can be up to 8 characters long, but it cannot contain the symbols +=\[]'.";/<>? in the
filename. If the new name already exists, a prompt will be displayed as a warning and will give the option to
overwrite the existing file or return to enter a different name.
F5 - Delete
Press F5-Delete to delete a file. After F5-Delete is pressed, the screen will appear as in the F2-Load option where
the same keys can be used to navigate the files. A yes/no prompt will appear after accepting a file for deletion for
final confirmation.
F9 – Details On/Off
Turns Intercon part file information display on or off.
T-Series Operator’s Manual
5/18/2011
8-7
Insert Operation
Press F3-Insert or Insert key to access the Insert Operation Menu. From this menu, you can add operations to a
part program.
The operation is added before the currently highlighted operation. The block number is shown to the left. The
operations you can insert are listed at the bottom of the screen. Pressing the function key that corresponds to an
operation will bring up the Edit Operation Menu for that operation.
NOTE: For operations that use negative side tooling (see chapter 4) X values will be negative, such as starting and
ending diameters in a turning cycle. Roughing and finishing tools are the same and the user is required to do tool
positioning for tool changes.
8-8
5/18/2011
T-Series Operator’s Manual
F1 - Linear
Press F1-Line at the Insert Operation Menu to insert a linear operation.
End
(X,Z)
X+
Z+
Press F1-Toggle or Space key to toggle between "Rapid" and "Feedrate" options when necessary and then use the
Up and Down arrow keys to move between fields and fill in the rest of the required information. Once complete
press F8-Graph to check your work and F10-Accept to accept the entries. Use the up and down arrow keys to
move between fields. Press ESC to cancel and return to the Insert menu.
The destination of the linear move can be given in terms of the end point coordinates or as the counterclockwise
angle from the 3 o'clock position to the line and the length of the line (polar coordinates). Press F3-Modal Display
to hide modal fields. Press this key again to show those fields. Press the F4 key to hide the polar coordinates.
Press this key again to display those fields.
Linear Type: Enter the type of linear move you want to make (Rapid or Feedrate). This field can be toggled
between Rapid and Feedrate. A rapid move is a non-cutting positioning move made at the maximum rate. A
feedrate move is a cutting move made at the programmed feedrate. When performing a cutting operation, this must
be toggled to Feedrate.
End X: Enter the X coordinate of the end position of the linear move. You can toggle between absolute and
incremental position. When toggled to absolute, enter the absolute position, with reference to the part zero. When
toggled to incremental, an INC will appear next to the entry. In this mode, enter the X distance from the preceding
end position.
End Z: Enter the Z coordinate of the end position of the linear move. You can toggle between absolute and
incremental position. When toggled to absolute, enter the absolute position, with reference to the part zero. When
toggled to incremental, an INC will appear next to the entry. In this mode, enter the Z distance from the last
preceding end position.
Angle: The destination can also be determined with an angle from the three o'clock position. Enter this angle in
conjunction with the length to determine the end point of the linear move.
Length: Enter the length of the linear move. The length, along with the previously entered angle, will be used to
calculate the end point of the move.
T-Series Operator’s Manual
5/18/2011
8-9
Connect Type: When two feedrate moves are performed consecutively, you can choose the style in which they are
connected. You can toggle this field between the following options: None, Bl Chamf (Dist), Chamf (Dist), Bl
Chamf (Len), Chamf (Len), or Radius. When set to none, the linear operations are connected at the point of
intersection. There are now two chamfer types: Distance and Length. For Distance Chamfers the operator specifies
the amount of distance to be removed from the ends of the two linear segments. The chamfer connects the two
shortened segments. If a Length Chamfer is chosen, the linear moves are connected by a chamfer of a specified
length. Both chamfer types have a blended version. When blend chamfer is chosen, the linear moves are connected
by a chamfer with rounded corners. When radius is chosen, a rounded corner connects the two linear moves.
● NOTE: Chamfers and blend chamfers in programs created with pre 8.10 Intercon are Length chamfers.
● NOTE: Chamfer and blend chamfer cannot be used to connect to an arc.
Connect Radius: Enter the radius of the rounded corner used to connect two feedrate moves.
Chamfer Distance: Enter the Distance to be removed from the end of each linear segment.
Chamfer Length: Enter the length of the chamfer you want to connect two linear feedrate moves.
Tool Num/Offset: Enter the tool number and offset number used. The first two digits is the tool number; the last
two digits is the offset number. You can also press F2 to go to the tool library to select another tool and/or make
changes to the tool library. Then, press F10 to accept.
Feedrate: Enter the desired cutting feedrate. You can toggle between feed/min and feed/rev.
Spindle Speed: Enter the desired spindle speed. You can toggle between RPM or CSS. When toggled to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
8-10
5/18/2011
T-Series Operator’s Manual
F2 - Arc
Press the F2-Arc to insert an arc operation.
R
Center (X,Z)
End (X,Z)
CW
CCW
X+
Z+
Use the up and down arrow keys to move between fields. Press F1-Toggle or Space bar to toggle between options
when necessary and press F10-Acept to accept the information entered. Press ESC to cancel and return to the Insert
Menu. Press F3-Modal Display to hide modal fields. Press this key again to show those fields.
Type: Intercon allows you to specify the arc in one of four ways. You can specify the arc by its end point and radius
(EP&R), by its center point and angle (CP&A), by its center point and end point (CP&EP), or by its mid point and
end point (3-Point). The fields displayed will depend on the type specified.
EP&R – End Point and Radius
End X: Enter the X coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the X distance from the preceding end position.
End Z: Enter the Z coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the Z distance from the preceding end position.
Radius: Enter the radius of the arc. Blend chamfer and chamfer cannot be used to connect to arc or to connect an
arc to another item.
Direction: Enter the direction you want the arc to be cut. Toggle between clockwise and counterclockwise.
Connect Radius: Enter the radius to use when blending an arc with another arc or a linear cut. Entering a value in
this field will cause the moves to be connected by a rounded corner with this radius.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Feedrate: Enter the desired cutting feedrate. You can toggle between feed/min and feed/rev.
Spindle Speed: Enter the desired spindle speed. You can toggle between RPM or CSS. When toggled to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
T-Series Operator’s Manual
5/18/2011
8-11
CP&A – Center Point and Angle
Center X: Enter the X coordinate of the center of the arc. You can toggle between absolute and incremental
position. When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to
incremental, an INC will appear next to the entry. In this mode, enter the X distance from the last point.
Center Z: Enter the Z coordinate of the center of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the Z distance from the last point.
Angle: Enter the angle of the arc.
Direction: Enter the direction you want the arc to be cut. Toggle between clockwise and counterclockwise.
Connect Radius: Enter the radius to use when blending an arc with a linear cut or another type of arc. Entering a
value in this field will cause the arc and a linear move to be connected by a rounded corner with this radius.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Feedrate: Enter the desired cutting feedrate. You can toggle between feed/min and feed/rev.
Spindle Speed: Enter the desired spindle speed. You can toggle between RPM or CSS. When toggled to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
CP&EP – Center Point and End Point
End X: Enter the X coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the X distance from the last point.
End Z: Enter the Z coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the Z distance from the last point.
Center X: Enter the X coordinate of the center of the arc. You can toggle between absolute and incremental
position. When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to
incremental, an INC will appear next to the entry. In this mode, enter the X distance from the last point.
Center Z: Enter the Z coordinate of the center of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the Z distance from the last point.
Direction: Enter the direction you want the arc to be cut. Toggle between clockwise and counterclockwise.
Connect Radius: Enter the radius to use when blending an arc with a linear cut or another type of arc. Entering a
value in this field will cause the arc and a linear move to be connected by a rounded corner with this radius.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Feedrate: Enter the desired cutting feedrate. You can toggle between feed/min and feed/rev.
8-12
5/18/2011
T-Series Operator’s Manual
Spindle Speed: Enter the desired spindle speed. You can toggle between RPM or CSS. When toggled to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
3-POINT (Start Point, Mid Point, and End Point)
Mid X: Enter the X coordinate of a point on the arc between the start point and the end point. You can toggle
between absolute and incremental position. When toggled to absolute, enter the absolute position, with reference to
the part zero. When toggled to incremental, an INC will appear next to the entry. In this mode, enter the X distance
from the last point.
Mid Z: Enter the Z coordinate of a point on the arc between the start point and the end point. You can toggle
between absolute and incremental position. When toggled to absolute, enter the absolute position, with reference to
the part zero. When toggled to incremental, an INC will appear next to the entry. In this mode, enter the Z distance
from the last point.
End X: Enter the X coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the X distance from the last point.
End Z: Enter the Z coordinate of the end of the arc. You can toggle between absolute and incremental position.
When toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental,
an INC will appear next to the entry. In this mode, enter the Z distance from the last point.
Direction: Enter the direction you want the arc to be cut. Toggle between clockwise and counterclockwise.
Connect Radius: Enter the radius to use when blending an arc with a linear cut or another type of arc. Entering a
value in this field will cause the arc and a linear move to be connected by a rounded corner with this radius.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Feedrate: Enter the desired cutting feedrate. You can toggle between feed/min and feed/rev.
Spindle Speed: Enter the desired spindle speed. You can toggle between RPM or CSS. When toggled to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
T-Series Operator’s Manual
5/18/2011
8-13
F3 - Drill
Press the F3-Drill key to insert a Drill operation. This operation allows you to either do normal Drilling or offcenter Boring operations. Both the Drilling and Boring type operations are actually the same, except in the types of
tools used and position X field.
Centerline
Drilling
Off-Center
Boring with
an Insert Drill
Press F1-Type to toggle between Bore and Drill and their various options (i.e. peck, & deep hole). If the operation
is toggled into Bore mode, then you can modify the Position X coordinate, which can be specified to be off-center
(usually by the tool diameter).
NOTE: Insert drills and end mills can be used to drill and bore holes into a part. In order to bore with a specific
tool, it will need an offset value for that tool so diameters can be controlled. If for example a .750 diameter insert
drill is used to drill a hole in a part, but the final diameter of the hole needs to be 1.250, toggle to the boring cycle
and for Position X enter .750. This will offset the center of the drill to the center of the part. After the hole is in the
part, use a profile or a turning cycle to finish the hole to the 1.250 diameter, using the same tool.
Press F1-Type to toggle between options when necessary and the F10-Accept key to accept the entries. Use the up
and down arrow keys to move between fields. Press ESC to cancel and return to the Intercon Main Menu.
Z Surface Height
Clearance Amount
X+
Z+
Drill or Bore
Rapid move
Peck Drill or
Peck Bore
Feed move
Retract Amount
Deep Hole Drill
or
Deep Hole Bore
Rapid Clearance
Depth Z (Dwell occurs here)
8-14
Depth Increment
5/18/2011
T-Series Operator’s Manual
Surface Z: Enter the position of the front face of the work piece.
Type: Enter the type of Drilling or Boring you want to perform. You can toggle between Drill, Peck Drill, and
Deep Hole Drill, Bore, Peck Bore, Deep Bore using the F1-Type key.
Position X: (Valid only while in Bore mode) Enter the diameter for the tool being used.
Depth Z: Enter the depth of the hole to drill. This is the Z distance from the surface height.
Depth Increment: Enter the cut depth increment used during the cycle. This field only applies when the type field
has been set to Peck Drill, Deep Hole Drill, Peck Bore, or Deep Hole Bore.
Retract Amount: Enter the amount the drill should retract before making another incremental depth cut. This field
only applies when the type field has been set to Peck Drill or Peck Bore.
Rapid Clearance Enter the amount above the uncut material the drill will rapid to on subsequent cuts. This field
only applies when the type field has been set to Deep Hole Drill or Deep Hole Bore
Dwell Time: Enter the amount of time in seconds that the drill should dwell at the bottom of the hole.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Plunge Rate: Enter the feedrate at which you want to drill the hole. Toggle between feed/min and feed/rev.
Spindle Speed: Enter the spindle speed in RPM
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or a
position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
T-Series Operator’s Manual
5/18/2011
8-15
F4 - Tap
The tap operation allows you to tap into the parts centerline (cutting in the negative Z direction). The operation may
use a floating tap holder or rigid tap, with spindle reversal, or a self-reversing tap head. Press the F4-Tap key to
insert a center tapping operation.
X+
CW
Z+
CCW
Clearance Amount
Z Surface Height
Depth Z (Dwell occurs here)
Press the F1-Type key to toggle between options when necessary and the F10-Accept key to accept the entries.
Use the up and down arrow keys to move between fields. Press the Esc key to cancel and return to the Insert Menu.
Tap Head Type: Enter the type of tap head you will be using. You can toggle between floating and reversing.
Z Surface Height: Enter the Z position of the surface you are tapping.
Depth Z: Enter the depth of the hole you want to tap. You can toggle between absolute Z and an incremental value
from the parts surface. This is the Z distance from the surface height.
Thread Pitch: Enter the desired threads/unit.
Thread Lead: Enter the desired units/thread.
Dwell Time: Enter the time in seconds the tap should dwell at the bottom of the hole. This is to allow time for the
spindle to reverse rotational direction. Used for Floating Tap only.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Spindle Speed: Enter the spindle speed in RPM. A constant RPM value will be maintained.
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or a
position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
8-16
5/18/2011
T-Series Operator’s Manual
F5 - Thread
Press the F5-Thread key to insert a threading cycle. This cycle allows you to create a thread on the outside or
inside of your part. When you first insert a threading cycle, the screen looks something like the picture below.
Press F7-Details to skip thread lookup and manually enter custom thread data. Press the F1-Type key to toggle
between options when necessary and the F10-Accept key to accept the entries. Use the up and down arrow keys to
move between fields. Press the ESC key to cancel and return to the Insert Menu.
Thread Lookup
This cycle has a lookup feature that simplifies the process of creating threads. The data for standard threads have
been entered into a database. You can add custom threads to this database. You can recall any previously stored
thread by specifying a few key criteria:
Thread Type: Enter the thread type desired. Toggle between external, internal, external pipe, internal pipe. You can
view database entries for internal/external or pipe threads but not both at the same time.
Designation: Type any part of the beginning of a standard or custom designation to view a list of matching database
entries. Leave blank to match all entries from the database.
Class: Type any part of the beginning of the class to view matching entries. Leave blank to match all classes.
When you have typed anything in Designation or Class, the screen will display the first matching entries. For
example, typing “10” in the Designation field would show all entries in the database whose designations start with
“10”. If there is only one thread listed, simply press Enter to select it. If more than one is listed, you can choose
any thread shown by using the arrow keys to move up and down in the list. If the cursor is somewhere in the thread
list, you can press Page Up or Page Down to change to a different page of the thread list. When the desired
thread is highlighted, press Enter to accept. Below left is an example of selecting from the list. Below right is an
example of accepting the single match.
T-Series Operator’s Manual
5/18/2011
8-17
When you press Enter, you can view the thread details. The fields will have been filled in with the values from the
selected thread.
You can modify any of the values, if desired. If you do, an asterisk (*) will appear next to the Designation field and
it will be appended with “Custom”. You may change the designation and class fields to any name that you wish.
Press F4-Save to save the new thread in the database. If the designation and class already exist, you will be
prompted to overwrite the values.
X+
Thread (Compound) Angle: Enter the desired thread
compound angle to shift the chip load to be heavier
towards one side of the thread cutter. A thread
compound angle of 0 means that the chip load will
be even on both sides of the thread cutter. A typical
value is 55°. The default value is taken from
parameter 51. (See Chapter 14.)
Threads/Unit: Enter the number of threads per inch
or threads per millimeter you want to cut. This field
affects the Thread Lead field.
8-18
5/18/2011
Z+
First Pass
Next Pass
Thread
Lead
Thread
Compound
Angle
T-Series Operator’s Manual
Thread Lead: Enter the width of a thread for one complete turn. This field affects the threads/unit entry.
External Thread
Internal Thread
External Pipe Thread
Internal Pipe Thread
Major Diameter: Enter the major diameter of the thread you want to cut.
Minor Diameter: Enter the minor diameter of the thread you want to cut.
Note: Non-pipe threads are referenced at the thread face. Pipe thread diameters are referenced according to
ANSI/ASME B1.20.1-193 (R1992). External pipe threads are referenced at E0, the diameter at the external thread
face. For internal pipe threads, this is E3, the diameter at the end of the wrench make-up length (3 turns past the
nominal diameter of the external pipe thread.) For external and internal pipe threads, this should be the smallest
diameter on the taper.
T-Series Operator’s Manual
5/18/2011
8-19
Chamfer Amount: Enter the number of turns to take to withdraw the tool from the maximum depth to the surface.
This produces a thread that tapers to the surface.
Taper Amount: Enter the amount the surface rises over the length of the surface you want to thread – normally
negative amount for external, positive amount for internal. This field affects the thread angle field. For pipe
threads, this value is calculated from the preset angle of 1.2812 degrees.
Taper Angle: Enter the angle that the surface tapers to – normally negative angle for external, positive angle for
internal. This field affects the taper amount entry. The taper angle of pipe threads is preset at 1.2812 degrees.
Clearance Z: Enter a clearance amount, or “run-up” distance from the thread face. This clearance helps get the
cutting tool is up to speed before it contacts the thread face.
The main screen contains the following fields:
Thread Face Z: Enter the Z coordinate where the threading tool will first make contact with the thread. (Use the
Clearance Z field to get a run-up to this point.)
Ending Z: Enter the Z coordinate for the end of the threading cycle.
Minimum Cut Depth: Enter the minimum amount of material to remove during a pass. The threading cycle will
remove larger amounts of material initially but will work down to this value.
First Cut Depth: Enter the amount of material to be removed during the first cut.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Spindle Speed: Enter the desired spindle speed for the threading cycle. You can toggle between RPM or CSS.
When toggled to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed will be
maintained.
Finish Pass Amount: Enter the amount of material to leave for a finishing pass.
Num Spring Passes: Enter the number of passes to make at the finish diameter.
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or a
position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
8-20
5/18/2011
T-Series Operator’s Manual
F6 - Profile
Press the F6-Profile key to insert a profile.
The profile operation allows you to define a profile with lines and arcs that will be produced with a cleanout cycle.
NOTE: Do not move Z until the 2nd line of the profile to avoid over and under cutting of part.
Example Profile
Press the F1-Type key to toggle between options when necessary. When at least one operation is present in the
profile, you can press the F10-Accept to accept the profile.
Profile Type: Enter the type of profile you want to produce. Toggle between diameter and end face. Choosing
diameter will cause the cleanout cycle to be performed along the diameter while choosing end face will cause the
cleanout cycle to be performed along the face.
Start X: Enter the X coordinate of the start of the profile. Allow for clearance.
Start Z: Enter the Z coordinate of the start of the profile. Allow for clearance.
Start X and Start Z are where the tool rapids to before it starts the cleanout cycle.
● NOTE: Intercon determines whether the cleanout cycle is external or internal by the start position of the profile
and the end position of the first move in the profile. If the end position of the first move is lower than the start
position of the profile, the cleanout cycle is external. For external cleanout cycles, all profile operations must be
lower than the start point. If the end position of the first move is higher than the start position of the profile, the
cleanout cycle is internal. For internal cleanout operations, all profile operations must be higher than the start point.
Depth of Cut: Enter the amount to remove per pass per side in the cleanout cycle.
Rough Tool: Enter the tool number and offset number you want to use during the roughing portion of the cleanout
cycle. The first two digits is the tool number; the last two digits is the offset number.
Rough Feedrate: Enter the desired feedrate for the roughing portion of the cycle. You can toggle between Feed Per
Revolution (f/r) or Feed Per Minute (f/m). Note that this Rough Feedrate is different from the Finish Feedrates
specified within each of the Line and Arc operations inside the profile.
T-Series Operator’s Manual
5/18/2011
8-21
Rough Spin Speed: Enter the desired spindle speed for the roughing portion of the cycle. You can toggle between
RPM or CSS. When toggled to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface
speed will be maintained. Note that this Rough Spin Speed is different from the Finish Spindle Speeds specified
within each of the Line and Arc operations inside the profile.
Stock to Leave X: Enter the amount of stock to leave on the X-axis to be removed by the finishing pass(es).
Stock to Leave Z: Enter the amount of stock to leave on the Z-axis to be removed by the finishing pass(es).
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
After entering these fields, define the profile you want to cut out with lines and arcs. Intercon allows you to insert
Lines, Arcs, and Finish Passes within a profile. Lines and Arcs are described earlier. The Finish Pass is described
later.
Rapid Between Cuts: Choose whether or not the moves between rough passes are to be done as Rapid or Feedrate.
You can toggle between Yes and No.
● NOTE: The Spindle Speeds and Feedrates specified within each of the individual Line and Arc operations inside
the profile are not used by the roughing portion of the cycle. However they will later be utilized by the Finish Pass,
if it is defined.
Finish Pass (For Profiles Only)
The Finish Pass is a special operation that only applies to profiles. At least two operations must be present in the
profile before you can insert a finishing pass. Multiple finishing passes can be inserted. Once a finish pass is
inserted, you can no longer make changes in the profile without going back out to the Insert Operations Menu.
● NOTE: The number of passes made for a finish operation is determined by the greater of
Stock to leave x (Profile Operation)
OR
stock to leave z (Profile Operation)
Depth of cut x (Finish Operation)
depth of cut z (Finish Operation)
8-22
5/18/2011
T-Series Operator’s Manual
Start Block: Enter the block number in the profile that the finishing pass should start on.
End Block: Enter the block number in the profile that the finishing pass should end on.
Depth of Cut Z: Enter the amount of material to remove from the Z-axis per pass. 0 will be one pass.
Depth of Cut X: Enter the amount of material to remove from the X-axis per pass. 0 will be one pass
●If both are 0, there will only be one pass.
Tool Num/Offset: Enter the tool number and offset number you want to use for the finish pass. The first two digits
is the tool number; the last two digits is the offset number. This field is disabled if G28 is not used for tool
changes.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
● NOTE: The Spindle Speeds and Feedrates specified within each of the individual Line and Arc operations
defined inside the profile will determine the Spindle Speeds and Feedrates for the Finish Pass. That is why there is
no way to specify a Spindle Speed or Feedrate on the Finish Pass Operation page.
T-Series Operator’s Manual
5/18/2011
8-23
F7 – Turning
A turning cycle is a repetitive cycle used to cut an outside or inside diameter to a specified dimension within a
specified Z range. Press the F7-Turning key to insert a turning cycle into your part program.
Diameter/Radius
Turning
End Face Turning
X+
Rapid move
Feed move
Z+
Press the F1-Type key to toggle between options when necessary and the F10-Accept key to accept the entries.
Use the up and down arrow keys to move between fields. Press the ESC key to cancel and return to the Insert
menu.
Turning Type: Enter the type of turning you want to use. Toggle between diameter/radius and end face. Choosing
diameter/radius will cause the cycle to remove material in a direction parallel to the Z-axis, along the diameter or
radius. Choosing end face will cause the cycle to remove material in a direction parallel to the X-axis, along the
face.
Starting Diameter/Radius: Enter the diameter at which you want the cycle to start.
Ending Diameter/Radius: Enter the diameter at which you want the cycle to finish.
● NOTE: When turning an inside diameter, the starting diameter must be less than the ending diameter. When
turning an outside diameter, the starting diameter must be greater than the ending diameter.
Starting Z: Enter the starting Z value for the turning cycle.
Ending Z: Enter the ending Z value for the turning cycle.
8-24
5/18/2011
T-Series Operator’s Manual
Taper Amount: Enter the amount that you want to taper from the starting diameter to the ending diameter. This
entry affects the taper angle. For diameter turning, enter a positive value to taper from the ending diameter + taper
amount to the ending diameter. Enter a negative value to taper from the ending diameter - taper amount to the
ending diameter amount. For end face turning, enter a positive value to taper from end Z taper + taper amount to
end Z. Enter a negative value to taper from end Z- taper amount to end Z.
● NOTE: The taper amount must be less than the depth of cut.
Taper Angle: Enter the angle you want to use to taper. This angle is used to determine the taper amount. For
diameter turning, enter a positive value to taper from the ending diameter + taper amount to the ending diameter.
Enter a negative value to taper from the ending diameter - taper amount to the ending diameter amount. For end
face turning, enter a positive value to taper from end Z taper + taper amount to end Z. Enter a negative value to
taper from end Z- taper amount to end Z.
End Face Turning
Radius/Diameter Turning
4
1
3
Taper
Angle (+)
1
2
Ending Z
Taper
Amount (+)
2
4
3
Ending Radius/Diameter
X+
Ending Z
Z+
Ending Radius/Diameter
● NOTE: Only one pass is shown in each of the illustrations.
Depth of Cut: Enter the amount to remove per pass
Rough Tool: Enter the tool and offset number to use for the roughing portion of the cycle. The first two digits is the
tool number; the last two digits is the offset number.
Rough Feedrate: Enter the cutting feedrate for the roughing portion of the cycle. You can toggle between feed/min
and feed/rev.
Rough Spin Speed: Enter the spindle speed for the roughing portion of the cycle. You can toggle between RPM and
CSS. When toggled to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed
will be maintained.
Finish Pass Amount: Enter the amount you want the roughing portion of the cycle to leave to be removed by the
finish pass. This is a radial amount. If the amount entered is zero, a finish pass will not be performed.
Finish Tool: Enter the tool and offset to use during the finishing pass. The first two digits is the tool number; the
last two digits is the offset number. This field is disabled if G28 is not used for tool changes.
Finish Feedrate: Enter the cutting feedrate for the finishing pass. You can toggle between feed/min and feed/rev.
T-Series Operator’s Manual
5/18/2011
8-25
Finish Spin Speed: Enter the spindle speed for the finishing pass. You can toggle between RPM and CSS. When
toggled to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed will be
maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
Return Feed Amount: This is a special field that activates 3-sided turning. If the value is 0, then the normal 2-sided
turning will be performed. If this value is more than 0, then 3-sided turning will be performed. On 3-sided turning,
this field specifies the length of the returning feedrate move.
Normal 2-sided Turning Cycle
3-sided Turning Cycle
(Return Feed Amount = 0)
4
Return Feed
Amount > 0
5
4
1
1
3
3
2
2
Rapid move
Feed move
X+
Z+
● NOTE: Only one pass is shown in each of the illustrations.
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or
a position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
8-26
5/18/2011
T-Series Operator’s Manual
F8 - Groove
Groove Cut on Outside Diameter
The grooving operation allows you to cut a groove of specified width and depth in a specified location. Press the
F8-Groove key to insert a grooving operation.
Press the F1-Type key to toggle between options when necessary and the F10-Accept key to accept the entries.
Use the up and down arrow keys to move between fields. Press the ESC key to cancel and return to the Insert
menu.
Type: Toggle between four options for the type of grooving. The four options are outside, inside, front and back
Choosing outside will cause the operation to cut the groove on the outside diameter of the work piece. Choosing
inside will cause the operation to cut the groove on the inside diameter of the work piece. Choosing front will cause
the operation to cut the groove on the front face of the work piece (see example below). Choosing back will cause
the operation to cut the groove on the back face of the work piece.
Groove Cut on Face of Part
T-Series Operator’s Manual
5/18/2011
8-27
Starting Diameter/Radius: Enter the position of the surface on which the groove will be produced.
Ending Diameter/Radius: Enter the grooves ending dimension.
Depth Increment: Enter the depth increment for the grooving cycle. This is the amount removed per plunge in the
peck cutting cycle used to produce the groove.
Starting Z: Enter the starting position of the groove.
Ending Z: Enter the ending position of the groove. For the outside or inside diameter, it will be a Z value. For the
front or back face, this will be an X value. You can toggle between absolute and incremental position. When
toggled to absolute, enter the absolute position, with reference to the part zero. When toggled to incremental, an
INC will appear next to the entry. In this mode, enter the X distance from the last point.
Width Increment: Enter the width increment for the grooving cycle. This is the step over amount for the cleanout
cycle used to produce the width.
Corner Finish: Enter the type of corner finish you want.
Toggle between square, radius, chamfer (Distance or
Length), and blend chamfer (Distance or Length).
Shown below is each type of corner that will be
produced for the groove.
Corner Radius: Enter the radius for the rounded corner
when corner finish is set to radius.
Chamfer Distance: Enter the Distance to be removed
from the end of each linear segment.
Chamfer Length: Enter the length of the chamfer you want for the corner finish.
Rough Tool Number: Enter the tool number and offset number to use for the roughing portion of the cycle. The first
two digits is the tool number; the last two digits is the offset number.
Rough Feedrate: Enter the cutting feedrate for the roughing portion of the cycle. You can toggle between feed/min
and feed/rev.
Rough Spin Speed: Enter the spindle speed for the roughing cycle. You can toggle between RPM and CSS. When
toggled to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed will be
maintained.
Finish Pass Amount: Enter the amount you want the roughing portion of the cycle to leave to be removed by the
finish pass. This is a radial amount. If the amount entered is zero, a finish pass will not be performed.
Finish Tool Number: Enter the tool number and offset number to use during the finishing pass. The first two digits
is the tool number; the last two digits is the offset number. This field is disabled if G28 is not used for tool
changes.
Finish Feedrate: Enter the cutting feedrate for the finishing pass. You can toggle between feed/min and feed/rev.
Finish Spindle: Enter the spindle speed for the finishing pass. You can toggle between RPM and CSS. When toggle
to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or a
position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
8-28
5/18/2011
T-Series Operator’s Manual
F9 - Cutoff
The cutoff operation allows you to cut off the part with a cutoff
tool.
Press the F1-Type key to toggle between options when
necessary and the F10-Accept key to save changes. Use the up
and down arrow keys to move between fields. Press the ESC
key to cancel and return to the Insert Menu.
Type: Enter the type of cut to cut off the work piece. You can
toggle between continuous and peck. Choosing continuous will
cause the work piece to be cutoff with a continuous cut.
Choosing peck will cause the work piece to be cutoff in
incremental moves.
Peck Increment: When the type field is set to peck, enter the increment amount used in cutting the part off. When
the type field is set to continuous, this field will not be shown.
Z position: Enter the Z position of the cut.
Starting Diameter: Enter the diameter at which the cutoff is to start.
Ending Diameter: Enter the diameter at which the cutoff is to finish.
Corner Finish: Enter the type of corner finish you want.
Toggle between square, radius, chamfer (Distance or
Length), and blend chamfer (Distance or Length). Shown
below is each type of corner that will be produced for the
cutoff. Corner finish will be on the start diameter.
Corner Radius: Enter the radius of the corner you want for
the corner finish. This field is only shown when radius is
chosen for the corner finish.
Chamfer Distance: Enter the Distance to be removed from the end of each linear segment.
Chamfer Length: Enter the length of the chamfer you want for the corner finish. This field is only shown when
chamfer is chosen for corner finish.
Tool Num/Offset: Enter the tool number and offset number you want to use. The first two digits is the tool number;
the last two digits is the offset number.
Feedrate: Enter the cutting feedrate to cutoff the work piece. You can toggle between feed/min and feed/rev.
Spin Speed: Enter the spindle speed for the work piece cutoff. You can toggle between RPM and CSS. When toggle
to RPM, a constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Pre/Post Cycle Pos.: Allows you to select if you want to move to a specified position before the cycle and/or a
position after the cycle. Once toggled from “None” 2 fields appear to enter the desired position.
T-Series Operator’s Manual
5/18/2011
8-29
F10 - Other
The F10-Other key displays additional operations.
If the 3rd axis label in the machine configuration is set to ‘C’ and parameter 93 is set for C axis operation, or if the
4th axis label in the machine configuration is set to ‘C’ and parameter 94 is set for C axis operation, there will be
options for C Axis and C Indexing operations shown.
The options shown at the bottom of the screen are described below. Press the ESC key to cancel and return to the
Insert Operation Menu.
F1 - Comment
Press the F1-Comment key to enter a comment. The comment can be up to 35 characters long and will be
displayed in the generated CNC program.
F2 – M&G Code
Press the F2-M&G Code key to enter M and G codes directly into the part program.
After entering the M and G codes you may press the F10-Accept key to accept the entry or the ESC key to cancel
and return to the Insert Operation Menu.
F3 – C Axis
Press the F3-C Axis key to enter the C Axis edit operation screen.
8-30
5/18/2011
T-Series Operator’s Manual
Press the F1-Toggle key or space bar to toggle between on and off. Press the F10-Accept key to accept the entry
or the ESC key to cancel and return to the Insert Operation Menu.
F4 – C Index
Press the F4-C Index key to enter the C Indexing operation screen.
Press the F1-Abs/Inc key to toggle between incremental (INC) and absolute (ABS) positioning.
Press the F3-Brake Off-On key to toggle the brake fields off and on.
Degrees: The number of degrees you want to move the C axis. This value can be positive or negative.
Minutes: The number of minutes you want to move the C axis. Values for this field are between 0 and 59.
Seconds: The number of seconds you want to move the C axis. Values for this field are between 0 and 59.
Move Mode: Rapid positioning or Feedrate move.
Feedrate: This is the degrees per minute at which to move if the aforementioned Move Mode is set to Feedrate.
Otherwise this field is not used.
Decimal degrees: This is another method of entering the number of degrees. If you choose to enter the movement
of the C axis with the fields listed above, the value of this field will be calculated automatically. If you choose to
enter the number of degrees with this field or make changes to it, then the degrees, minutes, and seconds will be
calculated or changed automatically. Values for this field can be positive or negative.
Brake On M code: The number of the M code to output for the braking function. The brake fields must be toggled
on to allow the editing of this field. When the brake fields are on, code will be output to turn off the brake, position
the C axis, and then turn on the brake.
T-Series Operator’s Manual
5/18/2011
8-31
Brake Off M code: The number of the M code to output for the braking function. The brake fields must be toggled
on to allow the editing of this field.
Press the F10-Accept key to accept the entry or the ESC key to cancel and return to the Insert Operation Menu.
F9 – Chamfer
Press the F9-Chamfer key to enter the chamfer operation screen. This is a one-shot operation. It generates a
cutting move from the current position at one of four angles as shown in the picture, below.
Chamfer Angle: Press the space bar or keys 1 through 4 to choose one of four angles: 135, 225, 315, and 45.
Length: If you know the length, enter it here. Intercon will calculate the End X and Z for you.
End X, End Z: Enter either X or Z; Intercon will calculate the other axis end position and length based on the
selected angle.
Tool Num/Offset: In one-shot mode, this will be filled in with the current tool number.
Feedrate: Enter the cutting feedrate for the chamfer. You can toggle between feed/min and feed/rev.
Spindle: Enter the spindle speed for the chamfer. You can toggle between RPM and CSS. When toggle to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
Press the F10-Accept key to accept the entry or the ESC key to cancel and return to the Insert Operation Menu.
8-32
5/18/2011
T-Series Operator’s Manual
F10 – Radius
Press the F9-Radius key to enter the radius operation screen. This is a one-shot operation. It generates an arc
move from the current position in one of eight directions as shown in the picture, below.
Center Line Axis: This chooses four of the eight possible arcs. X selects a center point on the X axis; Z selects a
center point on the Z axis. Press the space bar to toggle or press the X and Z keys.
Direction: The direction to move on the selected axis. It is also the direction of the center point from the current
position. Press the space bar to toggle between “+” and “-“. This chooses two out of four possible arcs.
Radius: The radius of the arc.
End X, End Z: If known, the end position of the arc. Intercon will calculate the other axis end point, arc direction,
and angle automatically.
Arc Direction: Use the space bar to select CW (clockwise) or CCW (counter-clockwise).
Tool Num/Offset: In one-shot mode, this will be filled in with the current tool number.
Feedrate: Enter the cutting feedrate for the arc. You can toggle between feed/min and feed/rev.
Spindle: Enter the spindle speed for the arc. You can toggle between RPM and CSS. When toggle to RPM, a
constant RPM will be maintained. When toggled to CSS, a constant surface speed will be maintained.
Cutter Compensation: Set cutter compensation in Chapter 11 for more details. You can toggle between None, Right
and Left.
Press the F10-Accept key to accept the entry or the ESC key to cancel and return to the Insert Operation Menu.
T-Series Operator’s Manual
5/18/2011
8-33
Graphics
Press the F8-Graph key from the Intercon Main Menu, the File Menu, or from any Edit Operation Menu to view
graphics. A wire frame of your part will appear.
F3 - Range
Press the F3-Range key to graph a portion of a part program.
Start Block: Enter the start block number of the portion of the part program you
want to graph.
End Block: Enter the end block number of the portion of the part program you
want to graph.
Press the F10-Accept key to accept entries and the ESC key to cancel.
F4 - Time
Press the F4-Time key to get an estimate of the time it will take to produce the part.
F5 - Redraw
Press the F3-Redraw key to redraw the graphic.
F6 - Pan
Press the F6-Pan key to move the part around the graph window. After pressing this key, crosshatches will appear.
Move the crosshatches around with the arrow keys. Pick a location on the part with the crosshatches and press the
F6-Pan key to pan this to the center of the graph window.
F7 - Zoom In
Press the F7-Zoom In key to zoom into the part. You will zoom in to the center of the graph window.
F8 - Zoom Out
Press the F8-Zoom Out key to zoom out from the part. You will zoom out from the center of the graph window.
F9 - Zoom All
Press the F9-Zoom All key to fit the entire part within the graph window.
1 – 9, 0, Space – Feed Rate Override & Hold
If no jog panel is attached (or “Keyboard” has been selected as the jog panel type) the number keys 1 – 9 and 0
choose feed rate overrides 10% - 90% and 100%, respectively. The space bar toggles feed hold on and off.
8-34
5/18/2011
T-Series Operator’s Manual
Math Help
Intercon provides a math assistance function to solve the trigonometric problems common in part drawings. To
enter Math Help, press F6-Math Help from any Edit Operation screen. The first time that you invoke Math Help,
the following screen appears which shows all available solvers:
The figures on the right are a graphical representation of the highlighted solver on the left. Pressing ENTER will
display another menu that has various fields particular to the type of problem that is being solved. The graphic
below displays the Right Triangle Calculator menu. The options that are available on the function keys are the
same for every type of math help solver and perform the following operations:
T-Series Operator’s Manual
5/18/2011
8-35
F1 – Prev Soln
F2 – Next Soln
The Prev Soln and Next Soln options will cycle backward and forward, respectively, through the available solution
sets for math solvers that may have multiple solutions. A status line near the bottom left of the screen appears once
a valid solution has been found. The solution status line indicates the total number of solutions and the solution
number that is currently represented by the graphic display on the right. For example, in an Arc Tangent Arcs math
help, the display solution status may be “- Solution 1 of 8 -“. In this case, the Prev Soln and Next Soln can be used
to cycle through all eight of the solutions.
F3 – Clear All
The Clear All option removes all solutions. It sets all fields for a particular solver to UNKNOWN.
F4 – Prev Solver
F5 – Next Solver
The Prev Solver and Next Solver options cycle backward and forward, respectively, through the various math help
solvers. These options are shortcuts which have the same effect as pressing ESC to reach the main math help
menu, navigating to the previous or next math help option, and then pressing ENTER.
F6 – Hide Math
The Hide Math option exits math help mode and returns to the operation edit menu. Pressing F6-Hide Math to
invoke Math Help again will restore Math Help exactly as you left it.
F7 – Copy <<<
F8 – Copy >>>
The Copy <<< option will move the value from the selected edit operation field into the selected math help menu
field and the Copy >>> operation will move the value from the selected math help menu field into the selected edit
operation field. For both options, the selected fields in the math help menu and the operation edit menu are
advanced. If the graphical display is visible when choosing one of these options, the effect is to turn off the
graphics display. Only when the graphics display is off will the Copy operations actually copy values and advance
field selections.
The currently selected fields have either a box drawn around them or are highlighted depending upon which menu
is active. The active menu, which is either the math operation menu on the left hand side or the operation edit
menu on the right hand side, depicts the selected field by highlighting the entire field. The non-active menu
displays the active field with a box drawn around it. Use the arrow keys to select fields as described below.
F9 – Graphic On/Off
The Graphic On/Off option will remove the graphical representation of the math help menu from the display. This
is helpful before copying data between Intercon operations and Math Help.
 (Arrow Keys) – Select Fields
The LEFT and RIGHT arrow keys are used to navigate between the math menu and the edit menu. The UP and
DOWN arrow keys are used to navigate within a menu. To choose fields for the “Copy” option, above, use the UP
and DOWN arrow keys to highlight the desired field in the menu and use the LEFT or RIGHT arrow keys to
switch menus.
8-36
5/18/2011
T-Series Operator’s Manual
Other features common to all Math help operations
In some math help operations, there will be an asterisk ‘*’ character that appears immediately to the right of a field.
This character marks the field as a “given” field, which means that the value of this field will be held constant in the
process of solving the math equations.
F1 –Triangle: Right
F2 –Triangle: Other
The screen will show UNKNOWN if the value of each parameter is not known. Math Help waits for known values
to be entered, where:
Point a, b, or c is the coordinate value for each corner of the triangle.
Angle A, B, or C is the angle at each point of the triangle.
Length of values are the distances between the points indicated.
Continue adding all the known parameters. Select parameters using the arrow keys. When Math Help solves the
remaining unknown values, the screen will display them.
F3 – Tangent: Line Arc
T-Series Operator’s Manual
5/18/2011
8-37
Given the center (C1) and radius of an arc and 1 point (LP) on a line, find the lines tangent to the arc (defined by
the tangent point (T1)). You must enter the X and Y coordinates for the circle's center point, the circle's radius, and
the X and Y coordinates for a point on the line.
F4 – Tangent: Arc Arc
Given the center points (CP1 and CP2) and radii (R1 and R2) of two arcs, find the point (T) at which they are
tangent. You must enter the X and Y coordinates for the first circle's center point, the radius of the first circle, the
X and Y coordinates for the second circle's center point, and the second circle's radius.
F5 – Tangent: Line Arc Arc
Given the center points (CP1 and CP2) and radii (R1 and R2) of two arcs, find the lines (defined by T1 - T8)
tangent to both arcs. You must enter the X and Y coordinates for the first circle's center point, the radius of the first
circle, the X and Y coordinates for the second circle's center point, and the second circle's radius.
8-38
5/18/2011
T-Series Operator’s Manual
F6 – Tangent: Arc Arc Arc
Given the center points (C1 and C2) and radii of two arcs and the radius of a third arc, find the center point of the
third arc and the tangent points (T1 and T2). You must enter the radius of the tangent arc, the X and Y coordinates
for the first circle's center point, the radius of the first circle, the X and Y coordinates for the second circle's center
point, and the second circle's radius.
F7 – Intersection: Line Line
You must enter the X and Y coordinates for 1 point on each line, and also one of the following:
* The X and Y coordinates for a second point
* The X coordinate for a second point and the angle from horizontal
* The Y coordinate for a second point and the angle from horizontal
* The angle from horizontal only
T-Series Operator’s Manual
5/18/2011
8-39
F8 – Intersection: Line Arc
Given the center (CP) and radius (R) of an arc, 1 point (LP1) and either a second point (LP2) or one coordinate
(LP2 X or Y) and the angle from horizontal, find the intersection point(s) (I1 and I2).
You must enter the X and Y coordinates for the circle's center point, the circle's radius, the X and Y coordinates for
one point on the line, and one of the following:
* The X and Y coordinates of a second point on the line
* The X coordinate of a second point and the angle from horizontal
* The Y coordinate of a second point and the angle from horizontal
F9 – Intersection: Arc Arc
Given the center points (CP1 and CP2) and the radii (R1 and R2) of two arcs, find the intersection point(s) (I1 and
I2) of the arcs.
You must enter the X and Y coordinates for the first circle's center point, the radius of the first circle, the X and Y
coordinates for the second circle's center point, and the second circle's radius.
8-40
5/18/2011
T-Series Operator’s Manual
Intercon Lathe Tool Library
You can press F2-Tool lib in most Edit Operations screens to enter the Tool Library Screen.
Use the up and down arrow keys to select which tool offset to edit. When editing a tool, press ENTER to accept
the entry and to move onto the next field for that tool, or use the left and right arrow keys to move from field to
field. You can also use F5-+.001 or F6- -.001 to adjust the offsets and nose radius values by a small increment.
Absolute/Incremental entry mode for the offset values and nose radius values can be toggled with the F4-Abs/Inc
key.
Press F10-Acept to accept the highlighted offset for the current operation and save any changes. Press Esc to
cancel the offset selection. If you made changes, you will be asked if you wish to save them.
Tool Off (Tool Offset): Use the up and down arrow keys to select a tool offset.
Tool Loc (Tool Number): Enter the tool number (01-99) that you want to associate with the tool offset number.
Usually the Tool Location would be associated with the same numbered Tool Offset. For example, Tool #1 would
have Location T01 and Offset 01, therefore T0101. However, there may be situations where you may want to
specify 2 or 3 different offsets for tool #1. For instance, T0102 would be Location T01 and would use Offset 02
and T0103 would be location T01 and use offset 03.
X Offset: Enter the amount to adjust the X-axis position when tool offsets are used.
Z Offset: Enter the amount to adjust the Z-axis position when tool offsets are used.
Nose Radius: Enter the nose radius of the tool. This field is used by cutter compensation, if it is turned on.
Nos Vec (Nose Vector): Enter the nose vector of the tool. This tells Lathe Intercon how the tool is oriented in the
machine. This field affects the behavior of cutter compensation, and also affects the tool retraction moves when a
tool change occurs in a program.
T-Series Operator’s Manual
5/18/2011
8-41
Spin Dir (Spindle Direction): Enter the spindle direction for the tool. Toggle between off, clockwise, and
counterclockwise.
Max Spin (Max. Spindle Speed (G50)): The maximum spindle speed for the tool. A G50 is posted with the tool
change using this value as the S parameter. If the value is zero, the G50 value from the Setup screen is used.
Coolant: Specify the coolant for each tool. Toggle between off, flood and mist
Description: Enter a description of the tool.
8-42
5/18/2011
T-Series Operator’s Manual
Chapter 9
Lathe Intercon Tutorials
Lathe Intercon Tutorial #1
This is a step-by-step example of creating a part from a blueprint using Intercon. The tool path to be created is for
turning a ball end onto a one-inch diameter piece of stock. Before beginning, be sure you are following these five
steps to successful turning:
● Determine the tools necessary to machine the part by analyzing the print.
● Set the X and Z offsets for each tool. (T-Series Operator’s Manual, Chapter 4)
● Program the part using Intercon. (Lathe Intercon Manual)
● Set the Part Zero position on the stock to be machined. (T-Series Operator’s Manual, Chapter 5)
● Graph the part to check for programming errors, and machine the part.
This exercise begins after the print has been analyzed, the tools have been chosen, and the X and Z offsets have
been set. For this particular example, the end face coordinates of the part are chosen to be X0 and Z0. The
procedure outlined in the following pages will give you step-by-step instructions for programming the part (Figure
1) using Intercon.
R0.5000
1.0000
2.0000
Figure 1 - Part to be Programmed
Each feature of the part will become an operation in your program. Beginning from the T-Series Control Main
Screen, the following series of keystrokes will describe the step-by-step process of programming the part shown in
Figure 1.
A. Create a New Part Program:
PRESS
ACTION
F5
CAM
F1
ICN
F9
Setup
F10
Accept
F1
File
F1
New
F10
Accept
F10
Accept
9-1
COMMENTS
CAM Selection menu.
Starts Lathe Intercon.
Modify setup parameters. (See the next page.)
Save modified setup parameters.
Opens the File Menu.
Creates a new program. Enter “demo1” as the name for the file.
Accept the file name. Fill in the dialog box exactly as shown in
Figure 2.
Creates a new part file using the data entered.
5/18/11
T-Series Operator’s Manual
These tutorials assume the options Modal Linear and Arc are turned on in Intercon Setup (F9 on Intercon main
menu). When these options are turned on, accepting a Linear or Arc operation automatically inserts new Linear or
Arc operation after it. The Esc key can be used to cancel the new operation if it is not desired and return to the
operation menu. If these options are not turned on, the user must press F1 or F2 to insert a new Linear or Arc
operation. The operations shown in the examples have the taper angle and modal input fields turned on. To make
your entry screens look like the examples, go to the Setup screen to make sure that the parameters match the ones
below.
Enter your name as
programmer.
You may enter a description
of the part.
In this field, hit <SPACE> to
toggle between End
Chucked and Between
Center.
Figure 2 - New Part Dialog Box
B. Insert the First Cycle:
PRESS
ACTION
F7
Turning
F8
Graph
Esc
Escape/Cancel
COMMENTS
Creates a repetitive cycle used to cut an outside or inside
diameter to a specified dimension within a specified Z range. Fill
in the Edit Operation side of the screen as shown in Figure 3.
Generates a graph of the part to this point, as shown in Figure
4. This preview can be used to detect problems that may occur
if the part was cut now.
Returns to the Editing window.
F10
Accept
Saves the data.
9-2
5/18/11
T-Series Operator’s Manual
In this field, hit <SPACE> to toggle
between End Face, and Diameter.
Your cycle will begin at X=1.1 in. and
end at X=-0.05 in.
Your cycle will begin at Z=0.1 in.
and end at Z= 0.01 in.
Press F2 to set up tools. Enter 0.0321
for nose radius, 3 for nose vector, and
CW for spdinle direction.
Figure 3 - Turning Cycle Operation
Figure 4 - First Graph of Turning Cycle
C. Create A Profile:
PRESS
ACTION
F6
Profile
9-3
COMMENTS
Defines a profile with lines and arcs that will be produced with a
cleanout cycle. Fill in the Edit Operation portion of the screen
as shown in Figure 5. The first profile command will create the
move shown in Figure 6.
NOTE: The line number displayed in the Edit operation window
is the line number for the end of the profile (which is currently
line 40).
5/18/11
T-Series Operator’s Manual
In this field, hit <SPACE> to toggle
between End Face, and Diameter.
The profile will begin at X=1.0 in., Z=0.1
in., removing .05 in.
These values set how much stock the
Rough Pass will leave for the Finish pass.
In this field, hit <SPACE> to toggle
between Right, Left, and None.
Figure 5 - Beginning of Profile Cycle.
Note: For T1 press F2-Tool and enter 0.321 for nose
radius, 3 for nose vector, and CW for spindle
direction.
Figure 6 - First Profile
PRESS
F1
ACTION
Line
COMMENTS
Inserts a line into your profile (Figure 8). Fill in the Edit
Operation portion of the screen exactly as shown in Figure 7.
Figure 8 - First Line in Profile.
Figure 7 - Line 1 Edit Screen (Modal and Taper displays on)
PRESS
F10
ACTION
Accept
9-4
COMMENTS
Saves the data for Line 1, and automatically inserts another line
operation. This line will be the second line in Figure 10. Fill in the
Edit Operation portion of the screen exactly as shown in Figure 9.
Notice that End X is 0 incremental.
5/18/11
T-Series Operator’s Manual
Figure 10 - Second Line in Profile.
Figure 9 - Line 2 Edit Screen (Modal and Taper displays on)
PRESS
F10
ACTION
Accept
COMMENTS
Saves the data for Line 2 and automatically inserts another line
operation. This next line will be Line 3 in Figure 12. Fill in the Edit
Operation portion of the screen exactly as shown in Figure 11.
Figure 12 - Third Line in Profile.
Figure 11 - Line 3 Edit Screen.
PRESS
F10
ACTION
Accept
Esc
Escape/Cancel
F2
Arc
F10
Accept
9-5
COMMENTS
Saves the data for Line 3 and automatically inserts another line
operation
Cancel current line operation. Return to the profile edit menu.
Inserts an arc into the profile (Figure 14). Fill in the Arc Edit
Operation portion of the screen exactly as shown in Figure 13.
Saves the data, automatically inserts another arc operation.
5/18/11
T-Series Operator’s Manual
Figure 14 - Arc (0.5” Dia.) in Profile.
Figure 13 - Arc Edit Screen (Modal displayed)
PRESS
ESC
ACTION
Cancel Arc
COMMENTS
Cancel current arc. Return to profile edit screen.
F1
Line
Inserts a fourth line into your profile (Figure16). Fill in the Line
Edit Operation portion of the screen exactly as shown in Figure
15.
Figure 16 - Last Line in Profile.
Figure 15 - Line 4 Edit Screen
9-6
5/18/11
T-Series Operator’s Manual
D. Include a Finish Pass:
PRESS
ACTION
F10
Accept
COMMENTS
Saves the data for Line 4, and automatically inserts another line
operation.
Esc
Escape/Cancel
Cancel current line operation. Return to profile edit screen.
F3
Finish
Creates a finish pass through the whole profile to remove
material left by the rough pass (Figure 18). If no Depth of Cut is
set here, the finish pass will remove all the material in one pass.
Fill in the Edit Operation portion of the screen exactly as shown
below in Figure 17.
● Note: The depth of material left to be removed by the Finish Pass is defined in the beginning of the
Profile, (shown in Figure5) in the fields marked ‘Stock to Leave’.
These numbers refer to the lines
in the program that mark the
beginning and end of the profile.
Figure 17 - Full Screen View of Finish Pass Edit Screen.
Figure 18 - Finish Pass Over Whole Profile.
E. Graph the Final Part:
PRESS
ACTION
F8
Graph
9-7
COMMENTS
Generates a graph of the finished part, as shown in Figure19.
This preview can be used to detect problems that may occur if
the part was cut now.
5/18/11
T-Series Operator’s Manual
Figure 19 - Graph of Finished Part
F. Post the Part and Exit
PRESS
ACTION
Esc
Escape/Cancel
F10
Accept
Ecs
Escape/Cancel
F10
Post
9-8
COMMENTS
Returns you to the Editing window.
Saves the data, and returns to the profile editing screen.
Returns you to the Main Programming window.
Saves and posts the job to the control, creating G-codes for the
program.
5/18/11
T-Series Operator’s Manual
Lathe Intercon Tutorial #2
This is a step-by-step example of creating a part from a blueprint using Intercon. The tool path to be created is for
the part shown in Figure 1. Before beginning, be sure you are following these five steps to successful turning:
● Determine the tools necessary to machine the part by analyzing the print.
● Set the X and Z offsets for each tool. (T-Series Operator’s Manual, Chapter 4)
● Program the part using Intercon. (Lathe Intercon Manual)
● Set the Part Zero position on the stock to be machined. (T-Series Operator’s Manual, Chapter 5)
● Graph the part to check for programming errors, and machine the part.
This exercise begins after the print has been analyzed, the tools have been chosen, and the X and Z offsets have
been set. For this particular example, the end face coordinates of the part are chosen to be X0 and Z0. The
procedure outlined in the following pages will give you step-by-step instructions for programming the part shown
below.
Figure 1 - Part to be Programmed.
Beginning from the T-Series Control Main Screen, the following series of keystrokes will describe the step-by-step
process of programming the part shown in Figure 1.
A. Create a New Part Program:
9-9
5/18/11
T-Series Operator’s Manual
PRESS
F5
F1
F1
F1
F10
ACTION
CAM
ICN
File
New
Accept
F10
Accept
COMMENTS
CAM Selection menu.
Start Lathe Intercon interface.
Opens the File Menu.
Create a new program. Enter a name for the file.
Accept the file name. Fill in the dialog box exactly as shown in
Figure 2.
Creates a new part file using the data entered.
Enter your name.
You may enter a description of the part.
In this field, hit <SPACE> to
toggle between End Chucked
and Between Center.
Figure 2 - New Part Dialog Box
B. Insert the First Cycle:
PRESS
ACTION
F7
Turning
COMMENTS
Creates a repetitive cycle used to cut an outside or inside
diameter to a specified dimension within a specified Z range. Fill
in the Edit Operations side of the screen as shown in Figure 3.
The cycle will begin at X = 2.1 inches, and
end at X = –0.05 inches.
The cycle will begin at Z = 0.10 inches, and
end at Z = 0.0 inches.
9-10
5/18/11
T-Series Operator’s Manual
PRESS
F2
ACTION
Tool
F10
F10
Accept
Accept
COMMENTS
Opens the Tool Library. For Tool Offset 1, set the following
values:
Tool Location (Tool Number) = T01
Nose Radius = .0312
Nose Vector = 3
Spin Dir = CW (See Figure 4)
Sets the Tool Library for Tool Offset #1.
Keeps selected values for the turning cycle.
For this example, only
these four values
need to be set before
continuing.
Figure 4. Setting values for Tool #1, Offset #1
C. Create A Profile:
PRESS
ACTION
F6
Profile
9-11
COMMENTS
Defines a profile with lines and arcs that will be produced with a
cleanout cycle. You can accept the values when at least two
operations are present within the profile. Fill in the Edit
Operation side exactly as shown in Figure 5.
NOTE: The line number displayed in the Edit operation window
is the line number for the end of the profile (which is currently
line 40).
5/18/11
T-Series Operator’s Manual
0003 PROFILE
Figure 5 - Beginning of Profile Cycle – Program Line #0003
PRESS
F10
F1
ACTION
Accept
Line
COMMENTS
Accept the entered values for the Profile.
Inserts a line into your profile. Fill in the Edit Operation portion of
the screen exactly as shown in Figure 6.
0004 LINE
Figure 6 - First Line within the Profile Cycle – Program Line #0004
PRESS
F10
ACTION
Accept
9-12
COMMENTS
Keep selected values for first line in profile. Automatically insert
another line operation. Fill in the Edit Operation portion of the
screen exactly as shown
in Figure 7.
5/18/11
T-Series Operator’s Manual
0005 LINE
Figure 7 - Second Line within the Profile cycle – Program Line #0005
PRESS
F10
ACTION
Accept
COMMENTS
Keep selected values for Line 2. Automatically insert another
line operation. This line will be 0.3375 inches long and will be
cut on an angle of 90 degrees with a Connect Radius of 0.250
inches. Fill in the Edit Operation portion of the screen exactly as
shown in Figure 8.
0006 LINE (CR)
Figure 8 - Third Line within the Profile cycle – Program Line #0006
PRESS
F10
ACTION
Accept
9-13
COMMENTS
Save values entered for Line 3. Automatically insert a fourth linear
operation into your profile. This line will be 0.8750 inches long, cut
at an angle of 180 degrees. Fill in the Edit Operation portion of the
screen exactly as shown in Figure 9.
5/18/11
T-Series Operator’s Manual
N0007
N0007 Line
Linear Type
End
Taper Angle
Taper Length
Connect Type
Connect Radius
Chamfer Distance
Tool Num/Offset
Finish Feedrate
Finish Spindle Speed
Cutter Comp
: Feedrate
0.7250
X:
Z:
-0.8750
:
180.0000
180.0000 ◦
:
0.8750
0.8750
: None
:
0.2500
:
0.0
0.0000
: T 0101
:
0.0050 F/R
:
600 CSS
: Right
Figure 9 - Fourth Line within the Profile cycle – Program Line #0007
PRESS
F8
ACTION
Graph
ESC
F10
Escape
Accept
COMMENTS
Displays a preview of the part up to this point. Your graph should
look like that shown in Figure 10.
Returns you to the Editing Menu
Keeps selected values for Line 4. Automatically inserts a fifth linear
operation into your profile. This line will be 0.1350 inches long, cut
at an angle of 90 degrees, with a 0007
blended
chamfer connector 0.1”
LINE
long. Fill in the Edit Operation portion of the screen exactly as
shown in Figure 11.
Figure 10 - Graph of Partial Profile
9-14
5/18/11
T-Series Operator’s Manual
N0008 Line
Linear Type
End
Taper Angle
Taper Length
Connect Type
Connect Radius
Chamfer Length
Tool Num/Offset
Finish Feedrate
Finish Spindle Speed
Cutter Comp
: Feedrate
0.9950
X:
Z:
-0.8750
:
90.0000 ◦
:
0.1350
: Bl Chamfer (Len)
0.2500
:
:
0.1000
: T 0101
:
0.0050 F/R
:
600 CSS
: Right
0008 LINE (WITH CHAMFER)
Figure 11 - Fifth Line within the Profile cycle – Program Line #0008
PRESS
F10
ACTION
Accept
COMMENTS
Keep selected values for Line 5. Automatically insert a sixth linear
operation into your profile. This line will be 0.8750 inches long and
will cut at an angle of 180 degrees with a connect Radius of 0.125
inches. Fill in the Edit Operation portion of the screen exactly as
shown in Figure 12.
X=0.9950”
Z=-1.7500”
0.1250” (CR)
180
0.875
0009 LINE
Figure 12 - Sixth Line within the Profile cycle – Program Line #0009
PRESS
F10
ACTION
Accept
9-15
COMMENTS
Keep selected values for Line 6. Automatically insert a seventh
linear operation into your profile. This line will be 0.2225 inches long
and will cut at an angle of 90 degrees with a connect radius of
0.015 inches at the corner. Fill in the Edit Operation portion of the
screen exactly as shown in Figure 13.
5/18/11
T-Series Operator’s Manual
X=1.4400”
Z=-1.7500”
0.1250” (CR)
0010 LINE
Figure 13 - Seventh Line within the Profile cycle – Program Line #0010
PRESS
F10
ACTION
Accept
COMMENTS
Keep selected values for Line 7. Inserts an eighth linear operation
into your profile. This line will be 0.3889 inches long and will cut at an
angle of 135 degrees, with a connect radius of 0.015 inches at the
corner. Fill in the Edit Operation portion of the screen exactly as
shown in Figure 14.
X=1.990”
Z=-2.025”
0.015” (CR)
0011 LINE
Figure 14 - Eighth Line within the Profile cycle – Program Line #0011
PRESS
F10
ACTION
Accept
9-16
COMMENTS
Keep selected values for Line 8. Inserts a ninth linear operation into
your profile. This line will be 0.625 inches long and will be cut at an
angle of 180 degrees. Fill in the Edit Operation portion of the screen
exactly as shown in Figure 15.
5/18/11
T-Series Operator’s Manual
0012 LINE
Figure 15 - Ninth Line Within the Profile cycle – Program Line #0120
PRESS
F8
ACTION
Graph
ESC
Escape
COMMENTS
Displays a preview of the part up to this point. The profile to this
point should look like that shown in Figure 16.
Returns you to the Editing Menu
Figure 16 - Partial Graph of Profile Through Program Line #0120
PRESS
F10
ACTION
Accept
9-17
COMMENTS
Keep selected values for Line 9. Automatically inserts a tenth linear
operation.
5/18/11
T-Series Operator’s Manual
Esc
F3
Escape/Cancel
Finish
Cancel tenth linear operation and return to profile edit menu.
Inserts a finishing pass to remove any excess material left from the
Rough Pass, and leave a smooth finish. Fill in the Edit Operation
portion of the screen exactly as shown in Figure 17.
● Note:
If the depth of cut for X and Z are 0 or equal to the Depth of Cut in line # 0030
(X=0.01inches, and Z=0.005 inches), the finish pass will be cut in one pass
0013 FINISH PASS
Figure 17 - Finish Pass Within the Profile cycle – Program Line #0013.
PRESS
F2
ACTION
Tool
F10
F10
Esc
↓
Accept
Accept
Escape
Down Arrow
D. Insert a Groove:
PRESS
ACTION
F3
Insert
F8
Groove
9-18
COMMENTS
Set the nose radius for Tool 2 = .0150, and the Nose Vector for Tool
2 = 3. Set the Spin Dir=CW, using the <space> bar to toggle thru
the choices available.
Sets the Tool Library for Tool #2.
Accepts Finish Pass values.
Exits the profile edit menu.
Cursor down so the next operation will be inserted after the end of
profile line.
COMMENTS
Insert a new operation after the end of the profile.
Creates an outside groove with a depth increment (X) of 0.05 inches
and a width increment (Z) of 0.025 inches, ending in a corner radius
of 0.030 inches. Fill in the Edit Operation portion of the screen
exactly as shown in Figure 18.
5/18/11
T-Series Operator’s Manual
0015 GROOVING
Figure 18 - Grooving Operation – Program Line #0015.
PRESS
F2
ACTION
Tool
F10
F8
Accept
Graph
COMMENTS
Set the nose radius for Tool 3 = .0070, and the Nose Vector for Tool
3 = 8. Set the Spin Dir=CW, using the <space> bar to toggle thru
the choices available. These same values can be set now for Tools
4 & 5, but be sure the cursor is back in the Tool 3 row before
pressing F10!
Sets the Tool Library for Tools #3, 4, & 5.
Displays a preview of the part up to this point. The part graph
should now look as shown in Figure 19.
Figure 19 - Graph of Grooving Operation – Program Line #0150
9-19
5/18/11
T-Series Operator’s Manual
PRESS
ESC
F10
ACTION
Escape
Accept
E. Add Threads:
PRESS
ACTION
F5
Thread
COMMENTS
Returns to the Editing Menu.
Accepts Grooving cycle.
COMMENTS
Places an external thread on the part with a compound angle of 60
degrees, 8 threads per inch with a thread lead of 0.125 inches. Fill
in the Edit Operation section of the screen as shown in Figure 20.
0016 THREADING
Figure 20 - Threading Operation – Program Line #0016.
PRESS
F10
ACTION
Accept
COMMENTS
Accepts values for the threading cycle.
F. Cut the Part From the Stock:
9-20
5/18/11
T-Series Operator’s Manual
PRESS
F9
ACTION
Cutoff
COMMENTS
Cuts off the part with a cutoff tool. Continuous cut Fill in the Edit
Operation section of the screen as shown in Figure 21.
0017 CUTOFF CYCLE
Figure 21 - Cutoff Cycle Removes the Machined Part from the Stock – Program Line #0170.
PRESS
F10
ACTION
Accept
G. Save and Post the Program:
PRESS
ACTION
ESC
Cancel
F8
Graph
ESC
F10
Cancel
Post
COMMENTS
Accepts values for cutoff cycle.
COMMENTS
Returns you to Intercon’s main menu.
Graphs the part one final time to be sure all steps were completed
correctly. The final graph should be as shown in Figure 22.
Returns you to the Intercon’s main menu.
Saves and posts job to control, creating G-codes for the program.
Figure 22 - Completed part
9-21
5/18/11
T-Series Operator’s Manual
9-22
5/18/11
T-Series Operator’s Manual
Chapter 10
CNC Program Codes
Code
E,F
N
O
P
Q
R
S
T
U
W
:
;
[]
Description
Feedrate or Thread Lead
Block Number
Program Number
Dwell Time, Subprogram Number, or General Parameter
Depth Parameter or General Parameter
Radius, Taper, Return Point, or General Parameter
Spindle Speed
Select Tool Number and Offsets
Incremental X Move
Incremental Z Move
Visible Comment
Internal Comment
Numerical Expression
The next three chapters contain a description of the CNC program codes and parameters supported by the T-Series
Control. The T-Series Control has some G codes and parameters that are modal, and some that are non-modal (one
shot). The G codes and parameters that are modal will stay in effect until a new G code or parameter is issued. One
shots are effective for the current line only.
For example, a movement command of G01, which is modal, will remain in effect until a different movement
command is issued, such as G00, G02, G03, etc.
Miscellaneous CNC Program Symbols
E, F - Feedrate or Thread Lead
In threading mode (G32, G76 and G92), E and F can specify thread lead (in units/rev). In other modes, only F can be
used to specify feedrate. Feedrate is either units/rev or units/min, depending on G98/G99 mode. The feedrate override
knob can be used to modify the programmed feedrate. The default feedrate is 3.0 units/minute.
Example:
G01 X1.0 Z-2 F0.1
; linear cut at X1 to Z-2 at 0.1 units/rev
N - Block Number
Block numbers are used to identify CNC program lines. Block numbers are optional, but can be used with the Search
Function (See Search option in Chapter 3) and make reading the NC files easier.
Example:
N1 G56 M26/Z
N2 G00 X0 Z0
T-Series Operator’s Manual
5/18/11
10-1
O - Program Number
The O program number allows you to identify your program with a certain number. However, if the specified program
number is 9100-9999, the G codes from the O number through the next M99 will be extracted (but not executed) and
placed in a separate subprogram/macro file named Oxxxx.cnc, where xxxx is the specified program number. This
separate file can later be called with M98 or G65.
Example:
O1521
N1 G56 M26/Z
N2 G00 X0 Z0
P - Parameter
P can correspond to Dwell Time, subprogram number, or a general parameter in canned cycles.
Examples:
G04 P1.32
G98 P9100 L1
G10 P73 R.1
;Pause execution for 1.32 seconds
;Call subprogram O9100.cnc
;Set parameter #73 (G73 retract) to .1 inches
Q - Parameter
Q is used as a depth parameter in canned cycles or as a general parameter in canned cycles.
Example:
G76 X.75 Z-1.5 P.1 Q.02 F.125 ;Q Sets depth of first cut at .02"
R - Radius, Taper, Return Point, Parameter
R can represent the radius, a taper amount, a return point, or a general parameter. R is similar to P.
Examples:
G10 P5 R.0625
G90 X1.0 Z-2.0 R.25 F.0115
;set nose radius of tool 5 = 0.0625
;tapered cut, from 0.5" diameter to 1.0"
;diameter
S - Spindle Speed Setting
Specifying a spindle speed causes the automatic spindle speed setting to be immediately updated. It does not cause the
spindle to start. In G97 mode (default), S specifies spindle speed in RPM. In G96 mode, S specifies surface speed in
feet/min or meters/min.
Example:
S1400 M3
;Starts the spindle CW at 1400 RPM
T - Select Tool and Offsets
Prompts the operator to insert the proper tool or change tools.
Examples:
T0100
T0101
T0201
;Prompt operator to load tool number 1, cancel offsets
;no tool change, but activate off set for tool 1
;prompt operator to load tool number 2, keep offsets from
;tool number 1
10-2
5/18/11
T-Series Operator’s Manual
U – Incremental X axis Move Command
To specify an incremental move on the X axis, use U in place of X in the command line. (See example below)
W – Incremental Z axis Move Command
To specify an incremental move on the Z axis, use W in place of Z in the command line. (See example below)
: - Visible Comment Identifier
The colon (:) is used to indicate the start of a comment line within a CNC program. The colon must be the first
character on the line.
Examples:
: Select work coordinate 3
G56
: Rapid to part zero
G00 X0 Z0
: Visible comments will be displayed on screen with the G-codes.
; - Internal Comment Identifier
The semicolon (;) is used to indicate the start of an internal comment within a CNC program line. All characters after
the semicolon are ignored when the program is run. Internal comments are used to document NC programs or
temporarily omit the remainder of a line.
Examples:
G56
G00
; select work coordinate 3
; G00 selected with no movement
T-Series Operator’s Manual
5/18/11
10-3
[ ] – Numerical Expression
The left bracket ‘[‘and right bracket ‘]’ are used to delimit a numerical expression. Numerical expressions can contain
floating-point numbers or user and system variables in combination with mathematical operators and functions. The
left parenthesis ‘(‘or bracket ‘[‘and right parenthesis ‘)’ or bracket ‘]’ can be used between the first left bracket and last
right bracket to force operator precedence or associativity. A bracketed numerical expression can be used anywhere a
number would be used. Comparison operators (‘eq’, ‘ne’, etc.) have built in rounding specified by parameter 144.
Without this rounding, ‘eq’ would usually return “false” when comparing two numbers calculated in different ways.
Comparison operators and logical operators (‘!’, ‘&&’, ‘||’) return 1.0 for “true” and 0.0 for “false”.
The mathematical operators and functions are:
+
*
/
^
mod or %
abs
sin
cos
tan
sqrt
#
Addition (or unary positive)j
Subtraction (or unary negative)
Multiplication
Division
Exponentiation
Modulo (remainder of devision)
Absolute value
Sine (degrees)
Cosine (degrees)
Tangent (degrees)
Square root
Variable access
eq or ==
ne or !=
ge or >=
gt or >
le or <=
lt or <
not or !
&&
||
and
xor
or
~
Equals
Not equals
Greater than or equals
Greater than
Less than or equals
Less than
Logical not
Logical and
Logical or
Bit-wise and
Bit-wise exclusive or
Bit-wise or
Bit-wise complement
Examples:
G91 X[13/64] Z[1+3/8]
; move the X axis 13/64 (0.2031) units
; and the Z axis 1 3/8 (1.375) units incrementally
X[SQRT[ABS[SIN[#101]-COS[#102]]]] ; Move X as a function of #101 and #102
User and System Variables
The ‘#’ character is used to reference a macro or a user or system variable. For variables that can be written, the ‘=’ is
used to assign to them. General purpose user variables are #100 to #149 and #29000 to #31999.
Index
1-3
4-6
7-9
10
11
12
13
14
15
16
17-18
19-21
22-24
25-27
28-30
31-33
Description
Macro arguments A-C
Macro arguments I-K (1st set)
Macro arguments D-F or 2nd set of I-K
3rd I (G is invalid)
Macro argument H or 3rd J
3rd K (L is invalid)
Macro argument M or 4th I
4th J (N is invalid)
4th K (O is invalid)
5th I (P is invalid)
Macro argument Q-R or 5th J-K
Macro arguments R-T or 6th set of I-K
Macro arguments U-W or 7th set of I-K
Macro arguments X-Z or 8th set of I-K
9th set of I-K
10th set of I-K
100 - 149
User variables
10-4
5/18/11
Returns
The floating point value if
defined by a G65 call, 0.0
otherwise.
These can be used as private,
local variables in any program
or subprogram. (See
examples.)
Floating-point value.
Initialized to 0.0 at start of job
processing
T-Series Operator’s Manual
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
Index
150 – 159
300-399
Description
Nonvolatile user variables
2400, 2401-2418
2500, 2501-2518
2600, 2601-2618
2700, 2701-2718
2800, 2801-2818
2900, 2901-2918
3000, 3001-3018
3100, 3101-3118
3200, 3201-3218
3901
3902
4001
4002
4003
4005
User string variables. These variables retain their
values until the CNC software is exited
Active WCS, WCS #1-18 CSR angles
Active WCS, WCS #1-18 Axis 1 values
Active WCS, WCS #1-18 Axis 2 values
Active WCS, WCS #1-18 Axis 3 values
Active WCS, WCS #1-18 Axis 4 values
Active WCS, WCS #1-18 Axis 5 values
Active WCS, WCS #1-18 Axis 6 values
Active WCS, WCS #1-18 Axis 7 values
Active WCS, WCS #1-18 Axis 8 values
Parts Cut (Part #)
Parts Required (Part Cnt)
Move mode
Constant surface speed mode
Positioning mode
Feedrate mode
4006
4014
4109
4119
4120
4121
4201
4202
5021-5028
5041-5048
9000-9399
10000
10001-10099
11000
11001-11099
12000
12001-12099
13000
13001-13099
14000
14001-14099
15000
15001-15099
16000
16001-16099
17000
17001-17099
18000
18001-18099
19000
19001-19099
20001-20008
20101-20108
20201-20208
20301-20308
20401-20408
Units of measure
WCS
Feedrate (F)
Spindle Speed (S)
Tool Number (“nn” in “Tnnoo”)
Current offset (“oo” in “Tnnoo”)
Job processing state
Search mode (0 = search mode off)
Machine Position (axis 1=5021, axis 2=5022, etc.)
Current Position (axis 1=5041, axis 2=5042, etc.)
Parameter values 0 – 399
Lathe: Tool X offset amount, current offset
Lathe: Tool X offset amount, offsets 01 - 99
Lathe: Tool Z offset amount, current offset
Lathe: Tool Z offset amount, offsets 01 - 99
Lathe: Tool nose radius, current offset
Lathe: Tool nose radius, offsets 01 - 99
Lathe: Tool nose vector, current offset
Lathe: Tool nose vector, offsets 01 - 99
Lathe: Tool coolant, current tool
Lathe: Tool coolant, offsets 01 - 99
Lathe: Tool spindle direction, current offset
Lathe: Tool spindle direction, offsets 01 - 99
Lathe: Tool location, current offset
Lathe: Tool location, offsets 01 - 99
Lathe: X wear adjustment, current offset
Lathe X wear adjustment, offsets 01 - 99
Lathe: Z wear adjustment, current offset
Lathe: Z wear adjustment, offsets 01 - 99
Lathe: nose radius wear adjustment, current offset
Lathe: nose radius wear adjustment, offsets 01 - 99
max_rate for axes 1-8
label for axes 1-8
slow_jog for axes 1-8
fast_jog for axes 1-8
screw_pitch for axes 1-8
T-Series Operator’s Manual
Returns
Floating-point value saved in
cnct.job file.
String Literal
R/W
R/W
R/W
Floating point value
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R
R
R
R
0.0 (rapid) or 1.0 (feed)
96.0 (on) 97.0 (off)
90.0 (abs) or 91.0 (inc)
98.0 (units per min) or
99.0 (units per rev)
20.0 (inches) or 21.0 (metric)
54.0-71.0 (WCS#1-18)
R
R
R
R
R
R
R
R
R
R
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
R/W
Floating point value
0 = normal, 1 = graph
0 = search mode off
Floating point value
See Chapter 14
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
1-9
1-9
7, 8, 9
7, 8, 9
3, 4, 5
3, 4, 5
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
Floating point value
5/18/11
R/W
R
R
R
R
R/W
10-5
Index
20501-20508
20601-20608
20701-20708
20801-20808
20901-20908
21001-21008
21101-21108
21201-21208
21301-21308
21401-21408
21501-21508
21601-21608
21701-21708
21801-21808
21901-21908
22001-22008
22101-22108
22201-22208
22301-22308
22401-22408
22501-22508
22601-22608
22701-22708
22801-22808
22901-22908
23001-23008
23101-23108
23201-23208
23301-23308
23401-23408
23501-23508
23601-23608
23701-23708
23801-23808
23901-23908
24001-24008
24101-24108
24301-24308
25000
25001
25002
25003
25004
25005
25006
25007
25008
25009
25010
25011
25012
25013
25014
25015
25016
Description
lash_comp for axes 1-8
counts_per_unit for axes 1-8
accel_time for axes 1-8
deadstart_velocity for axes 1-8
delta_vmax for axes 1-8
counts_per_turn for axes 1-8
minus_limit for axes 1-8
plus_limit for axes 1-8
minus_home for axes 1-8
plus_home for axes 1-8
reversed for axes 1-8
laser_comp for axes 1-8
proportional for axes 1-8
integration_limit for axes 1-8
kg for axes 1-8
integral for axes 1-8
kv1 for axes 1-8
derivative for axes 1-8
ka for axes 1-8
num_motor_poles for axes 1-8
drive_current for axes 1-8
drive_offset_angle for axes 1-8
pwm_kp for axes 1-8
pwm_ki for axes 1-8
pwm_kd for axes 1-8
abrupt_kp for axes 1-8
feed_forward_kp for axes 1-8
max_error (PID) for axes 1-8
min_error (PID) for axes 1-8
at_index_pulse for axes 1-8
travel_minus for axes 1-8
travel_plus for axes 1-8
axis_home_set for axes 1-8
abs_position (in encoder counts) for axes 1-8
PID_out for axes 1-8
reference set for axes 1-8
Axis reference value for axes 1-8
dsp positions for axes 1-8
DRO_display_units
default_units_of_measure
PLC_type
console_type
jog_panel_optional
min_spin_high
max_spin_high
home_at_powerup
screen_blank_time
Displayed / Calculated spindle speed. If parameter
178 =1 and spindle encoder is mounted.
current spindle position (in counts)
dsp_time (in seconds)
time (in seconds)
clear max/min PID errors
software type (Mill/Lathe)
feedrate override
spindle override
10-6
5/18/11
Returns
R/W
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R/W
R/W
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
R
T-Series Operator’s Manual
Index
Description
25017
OS
29000-31999
50001-51312
60001-61312
User variables. These variables retain their values
until the CNC software is exited.
PLC Inputs 1-1312
PLC Outputs 1-1312
70001-71024
80001-89999
90001-90064
91001-91064
92001-92064
93001-93256
94001-94256
95001-95256
96001-96044
97001-97022*
98001-98044
99001-99022
PLC Memory Bits 1-1024
Reserved
Timer 1-64 status bits
Reserved
Reserved
Stage 1-256 status bits
Fast Stage 1-256 status bits
Reserved
W1-W44 (32-bit signed integers)
DW1-DW22 (64-bit signed integers)
FW1-FW44 (32-bit floats)
DFW1-DFW22 (64-bit floats)
Returns
Windows/LINUX = 2;
other OS = 1.0
Floating point value
R/W
R
R/W
Jog Panel is on INP1057-1312
Jog Panel is on OUT10571312
R
R
R
R
R
R
R
R
R
R
R
R
R
R
* Since user or system variables are turned into (double) floating point values when referenced in an M- or
G-code program, the 64-bit integer values lose precision when they exceed 253 (9,007,199,254,740,992).
Examples:
#100 = #5041
G90 X[#5041+1+7/32]
#2501 = #5021
#2503 =[#2503+1/8]
;
;
;
;
set user variable #100 to the Z axis current position
move the Z axis 1 7/32 units (1.2188) incrementally
set WCS#1 Z value to the current Z position
add 1/8 units (.125) to the WCS#3 Z value
; Subroutine parameter and local variable access.
G1 Z#A X#B F#F
; move to the coordinates passed as parameters
#[Q] = #F * .10
; Assign local variable #Q to 10% of #F
#17 = #7 * .10
; Same statement as previous using number references.
#[C] = 0.05
; Reassign #C. (Value passed as parameter is lost.)
T-Series Operator’s Manual
5/18/11
10-7
Advanced Macro Statements
NOTICE
Branching and conditional execution are extremely powerful tools that, combined with
access to system variables, allow you to do many things that would otherwise be
impossible. Nevertheless, using branching and conditional execution can introduce
undesirable and even unpredictable behavior into your programs. Undesirable effects can
occur simply by graphing a program. The least of these undesirable effects could be
entering an endless loop, failing to draw anything, or wiping out all the information in your
tool library or WCS settings. It is your responsibility to make sure that undesirable things
do not happen in your programs. You must monitor the job processing and search modes in
your program, if necessary, and take appropriate action. Until you are confident of the
actions of your program, you should step through it one block at a time to confirm your
program logic.
GOTO - Branch Execution
To branch to another line within the same program or subprogram, use the statement
GOTO <expression>
Where <expression> is any expression that evaluates to a valid block number in the program. GOTO causes an
immediate branch to the specified destination. Program codes preceding a GOTO on the same line will be executed
normally. Any program codes following GOTO on the same line will cause an error.
If fast branching is disabled (parameter 145 = 0) then CNC11 searches forward in the program for the first matching
block number and resumes searching, if necessary from the top of the program. For this reason when fast branching is
disabled, backward branches take longer than forward branches and backward branch times depend on the total
program size. If the program is sufficiently large, use of the GOTO statement could introduce temporary pauses.
When fast branching is enabled (parameter 145 = 1) then CNC11 remembers the locations of block numbers as it finds
them during program execution. Backward branches always take place immediately. The first forward branch to a
block not yet encountered will take additional time as CNC11 searches forward for the block number; however,
subsequent forward branches to that block number will take place immediately. The trade-off for using fast branching
is that all line numbers at a given level of program or subprogram must be unique and programs will use more memory
(approximately 16kilobytes of memory for every 1000 block numbers in the program.)
IF THEN ELSE - Conditional Execution
Program symbols, G codes, M codes and GOTO commands may be executed conditionally using the IF statement.
The general form of the IF statement is:
IF <expression> THEN <execute if true> ELSE <execute if false>
Where <expression> is any valid expression, <execute if true> is one or more program codes to execute if
<expression> evaluates to “true” (non-zero) and <execute if false> is one or more program codes to execute if
<expression> evaluates to “false” (zero). All parts of the IF statement must appear on the same line. The “ELSE
<execute if false>” part of the statement is optional and may be omitted. The “THEN” may be omitted; however,
<expression> must be enclosed in brackets ([]). The IF statement may follow other program codes on the same line.
Compound conditionals are possible but they cannot be nested. The first THEN always pairs with the first IF. ELSE
always pairs with the first <expression> that evaluates to “false”. All program codes executed are executed as part of
the same block.
10-8
5/18/11
T-Series Operator’s Manual
Examples:
; Branch to N200 if machine position is okay, otherwise go to N300
N100 IF #5041 LE 5.0 THEN GOTO 200 ELSE GOTO 300
; Force subprogram parameter #D to be within range.
IF [#D LE 0.005] #[D] = 0.005
; Compound conditionals
IF [#A LE 0.0] GOTO 100 ELSE IF [#A LE 2.5] GOTO 200 ELSE GOTO 300
IF [#A GE 0.0] IF [#D/#A GE 0.0] #[C] = SQRT[#D/#A]
INPUT – Prompt Operator for Input
The INPUT macro prompts the operator for numeric input. The general form of the INPUT statement is:
INPUT “<prompt>” <variable>
Where <prompt> is the message prompt for the operator and <variable> is the variable in which to store the input.
CNC11 will display a dialog with the given prompt and space for the operator response. The operator may enter any
numeric expression (see above) including variables as a response. The operator must press CYCLE START or Alt-S
to dismiss the dialog. Pressing Esc will cancel the job.
CNC11 parses well ahead of the current execution to maximize throughput and efficiency. For this reason, an INPUT
macro may prompt the operator for input immediately even though the INPUT macro is located in the middle or near
the end of the job. (Use the “IF #6001” idiom to delay the prompt, if desired.) Parsing pauses while the dialog is
displayed. Any statements parsed prior to the INPUT macro will have been queued and will continue to execute in the
background while the prompt is displayed. Job processing will pause only if all queued statements have been executed
before the operator supplies a response.
INPUT macros will not graph. If you must graph the job, first set the input variable to a default value and use a
conditional to execute the INPUT only if the job is being run normally.
Use search mode cautiously with INPUT macros. To have search work properly, you may have to supply exactly the
same input during the search as you did during the last actual run.
Examples:
; Ask operator for pocket depth.
; Note: this will not graph.
INPUT “Enter pocket depth” #101
Store result in #101
; Allow job with INPUT statements to be graphed.
#101 = 0.5; Supply a default value for graphing
; Ask for operator input only if not graphing.
IF NOT #4201 THEN INPUT “Enter pocket depth” #101
T-Series Operator’s Manual
5/18/11
10-9
10-10
5/18/11
T-Series Operator’s Manual
CHAPTER 11
G Codes
G Code
G00
G01
G02
G03
G04
G10
G20
G21
G22
G23
G28
G29
G30
G32
G40
G41
G42
G50
G52
G53
G54
G55
G56
G57
G58
G59
G65
G70
G71
G72
G74
G75
G76
G80
G83
G84
G85
G90
G92
G94
G96
G97
G98
G99
*
*
*
*
*
*
*
Group
A
A
A
A
B
B
K
K
O
O
B
B
B
A
D
D
D
B
B
B
L
L
L
L
L
L
J
B
B
B
B
B
B
B
B
B
B
A
A
A
H
H
I
I
T-Series Operator’s Manual
Description
Rapid Positioning
Linear Interpolation
Circular or Helical Interpolation CW
Circular or Helical Interpolation CCW
Dwell
Parameter Setting
Select Inch Units
Select Metric Units
Work envelope on
Work envelope off
Return to Reference Point
Return from Reference Point
Return to Secondary Reference Point
Constant Lead Thread Cutting
Cutter Diameter Compensation Cancel
Cutter Diameter Compensation Left
Cutter Diameter Compensation Right
Coordinate System Setting, Max. Spindle Speed Setting
Offset Local Coordinate System
Rapid Position in Machine Coordinates
Select Work Coordinate System #1
Select Work Coordinate System #2
Select Work Coordinate System #3
Select Work Coordinate System #4
Select Work Coordinate System #5
Select Work Coordinate System #6
Call Macro
Finishing Cycle
Stock Removal in Turning
Stock Removal in Facing
End Face Peck Cutting
Outer/Inner Diameter Peck Cutting Cycle
Multi-Pass Threading Cycle
Cancel Canned Cycle
Deep Hole Drilling
Tapping
Boring Cycle
Outer/Inner Diameter Cutting Cycle
One-Pass Threading Cycle
End Face Cutting Cycle
Constant Surface Speed
Constant Surface Speed Cancel
Per Minute Feed
Per Revolution Feed
5/18/11
11-1
NOTES:
●All the default G Codes have been marked with the symbol " * ".
●A given line of a program may contain more than one G code.
●If several G codes from one group are used in the same line, only the G code specified last will remain active.
●G codes from group B are of "one shot" type (active only in the line in which they are specified). All other G
codes are modal (active until another G code of the same group is specified).
G00 - Rapid Positioning
G0 moves to the specified position at the maximum motor rate.
The coordinates may be either absolute positions or incremental
distances. G0 is modal and remains in effect until another
positioning mode (G1, G2, G3 etc.) is commanded. G0 is the
default-positioning mode.
Example:
G0 X0.0 Z0.0
This command moves both X and Z to the absolute coordinate 0.0 at maximum feedrate.
CAUTION
The feedrate override knob has no effect on G0 moves unless rapid override is
turned ON
G01 - Linear Interpolation
G1 moves to the specified position at the programmed feedrate. The
coordinates may be either absolute positions or incremental distances.
The movement will be along a straight line. G1 is modal and remains
in effect until another positioning mode (G0, G2, G3 etc.) is
commanded.
Example:
G01 X2 Z4 F10
G01 X6 Z3 F20
T-Series Operator’s Manual
5/18/11
11-2
G02 & G03 - Circular Interpolation
G2 moves in a clockwise* circular motion, and G3 moves in a
counterclockwise* circular motion. The X or Z position specified in the
G2 or G3 command is the end position of the arc, and may be an absolute
position (X, Z) or an incremental distance (U, W). G2 and G3 are modal
and remain in effect until another positioning mode (G0, G1, etc.) is
commanded.
Circular motion can be programmed in two different ways: specifying the
final point and the radius of the arc, or specifying the final point and the
parameters I and K (center point of the arc as incremental values from
the start position).
*The terms clockwise and counterclockwise can be somewhat confusing because they are relative directions which
change based on ones perspective. To help conceptualize the correct perspective, always program your part and set
up your tools as though the machine were a horizontal lathe with the tool post mounted in the rear and the head
stock to your left.
Rules of thumb:
1.
2.
3.
4.
5.
6.
7.
8.
All Convex OD Arcs which move towards a more negative Z position should be programmed as CCW.
All Concave OD Arcs which move towards a more negative Z position should be programmed as CW.
All Convex OD Arcs which move towards a more positive Z position should be programmed as CW.
All Concave OD Arcs which move towards a more positive Z position should be programmed as CCW.
All Convex ID Arcs which move towards a more negative Z position should be programmed as CCW.
All Concave ID Arcs which move towards a more negative Z position should be programmed as CW.
All Convex ID Arcs which move towards a more positive Z position should be programmed as CW.
All Concave ID Arcs which move towards a more positive Z position should be programmed as CCW.
METHOD 1: USING FINAL POINT AND RADIUS
The commands G2 and G3 will have the following structure:
G2 Xx Zz Rr
G3 Xx Zz Rr
where x and z will be the X and Z coordinates of the final
point of the arc, and r will be the radius.
Example:
G00 X2.0 Z1.0
;rapid to start
;position X2, Z1
G02 X4.0 Z2.0 R1 ;arc to X4 Z2 with
;radius of 1
T-Series Operator’s Manual
5/18/11
11-3
NOTE: A lathe is not usually used to cut an arc larger than 90 degrees. With the use of special tools, a lathe can
cut a 180-degree arc. This is the maximum value a lathe can cut an arc. Make sure the radius chosen follows the
cutting ability of the lathe.
METHOD 2: USING FINAL POINT AND PARAMETERS I & K
Another way to specify a circular operation is using
the parameters I and K instead of the radius R. The
parameters I and K are the incremental distances
from the start point to the center of the arc.
I = X center (radius) - X start (radius)
K = Z center - Z start
● NOTE: X coordinates are diameter values, but I
and R are always radius values.
Example:
G00 X2.0 Z1.0
;rapid to start
;pos. X2, Z0
G02 X4.0 Z2.0 K1 ;arc to X4 Z1
with radius 1
G04 - Dwell
G4 causes motion to stop for the specified time. The P parameter is used to specify the time in seconds to delay.
G4 causes the block to decelerate to a full stop.
The minimum delay is 0.01 seconds and the maximum is 327.67 seconds. The dwell time is performed after all
motion and M functions on the line. If the P parameter is not specified, X will be used instead. If neither P nor X is
specified, the default dwell time of 0.01 seconds will be used.
Example:
G0 X1 Z1
G4 P2.51
G0 X2 Z2
; rapid to X1 Z1
; pause for 2.51 seconds
; rapid to X2 Z2
T-Series Operator’s Manual
5/18/11
11-4
G10 - Parameter Setting
G10 allows you to set parameters for different program operations.
Examples:
G10 P5 Z-1.1
G10 P5 X-1.3
G10 P5 R.25
G10 P5 Q3
G10 P1073 R.05
;
;
;
;
;
Sets
Sets
Sets
Sets
Sets
tool #5
tool #5
tool #5
tool #5
machine
z offset to -1.1 in the Offset Library
x offset to -1.3 in the Offset Library
nose radius to .25 in the Offset Library
nose vector to 3 in the Offset Library
parameter 73 to 0.05
G20 - Select Inch Units
G20 selects inch units, affecting the interpretation of all subsequent dimensions and feedrates in the job file. G20
does not change the native machine units as set on the Control Configuration Menu.
G21 - Select Metric Units
G21 selects metric units, affecting the interpretation of all subsequent dimensions and feedrates in the job file. G21
does not change the native machine units, as set on the Control Configuration Menu.
G22/G23 – Work Envelope On/Off
G22 turns on programmable work envelope in machine coordinates. When the machine tries to move into the
forbidden area an “axis work envelope exceeded” message is displayed letting you know which line of the program
is at fault. The work envelope is set with the Z and X for the ‘+’ limit and I and J for the ‘-‘ limit. G22 is modal
and remains on until turned off by G23 or the end of the job. The limits entered in the Z, X and I, J parameters are
stored in the WCS menu under <F3> Work Envel.(see chapter 5).
G28 - Return to Reference Point
G28 moves to the first reference point, by way of an intermediate point. The location of the reference point, in
machine coordinates, may be set in the Work Coordinate System Configuration menu. The intermediate point is
specified in the local coordinate system, and may be at the current location (resulting in a move directly to the
reference point). If an intermediate point is specified, only those axes for which positions are specified will be
moved. If no axes are specified, all axes will be moved. The location of the intermediate point is stored for later
use with G29.
Examples:
G28 W0
; move Z axis directly to reference point
; (X doesn't move)
G28 U.5 W0
; move X +.5, then move BOTH axes to
; reference point
G28 X2 Z.1
; move both axes to (2,0.1), then to
; reference point
G28
; move all axes to the reference point
; (no intermediate point)
The G28 position is of great importance because it specifies the Tool Check position and the usual Tool Change
position. The G28 position is the machine coordinate position that the machine will move to when the <TOOL
CHECK> button is pressed. Also, the G28 position is the usual position at which tool changes occur during a job
run.
T-Series Operator’s Manual
5/18/11
11-5
G29 - Return from Reference Point
G29 moves all axes to the intermediate point stored in a preceding G28 or G30 command. It may be used to return
to the workpiece. If a position is specified, the machine will move to that position (in local coordinates) after
reaching the intermediate point. G29 may only be specified after G28 or G30, though there may be intervening
moves.
Examples:
G29
G29 X1 Z2
; move all axes back from reference point to
;intermediate point
; move all axes to intermediate point, then move to X1 Z2
G30 - Return to Secondary Reference Point
G30 moves to a specified return reference point, by way of an intermediate point. The P parameter may be used to
specify one of the 4 available Return Reference Points: The intermediate point is specified in the local coordinate
system, and may be at the current location (resulting in a move directly to the reference point). If an intermediate
point is specified, only those axes for which positions are specified will be moved. If no axes are specified, all axes
will be moved. The location of the intermediate point is stored for later use with G29.
The 4 available return reference points are defined in the Work Coordinate System Configuration menu. If you
issue G30 without a P parameter, it functions exactly like G28, except that by default it uses the second reference
return point.
The following table shows how to issue G-codes to utilize the 4 available Return Reference Points:
Return Reference Point
G-Code
Equivalent Alternate G-Code
G28
G30 P1
Return #1
G30
G30 P2
Return #2
G30 P3
Return #3
--G30 P4
Return #4
---
Examples:
G30 Z0
G30 P1
; move Z axis directly to second reference point
; move all axes to first reference point
● NOTE: G30 P1 is equivalent to G28.
G32 - Constant Lead Thread Cutting
G32 sets the constant lead thread cutting mode. During this
mode, both axes are locked to the spindle encoder count. Once
the encoder outputs a 1 turn signal, thread cutting is started at a
fixed point so that the tool path remains unchanged for repeated
thread cutting. Thread cutting follows the same tool path in
rough cutting through finish cutting.
● NOTE: When G32 is used, X and Z indicate the endpoint of
the cut and F indicates the lead.
Example:
G00 X1.5 Z0.0
; Step 1 - rapid move
G32 X1.5 Z-2.0 F0.125 ; Step 2 - straight
; thread cut of 2 inches, lead of .125
; or 8 threads per inch
G00 X1.7
; Step 3 - Clear X-axis
G00 z0.0
; Step 4 - Retract Z-axis
T-Series Operator’s Manual
5/18/11
11-6
G40, G41, G42 –Cutter Diameter Compensation
G41 and G42 in conjunction with the selected tool (T code) apply cutter compensation to the
programmed tool path. Cutter compensation is required whenever an angle or radius is being cut. G41
offsets the tool selected with the T code the amount of its nose radius, to the left of the workpiece,
relative to the direction of travel. G42 offsets the tool selected with the T code the amount of its nose
radius, to the right of the workpiece, relative to the direction of travel. G40 cancels G41 and G42.
Always program cutter compensation as though the machine were a horizontal lathe with the tool post
mounted in the rear and the head stock to your left.
Rules of Thumb:
1.
2.
3.
4.
All OD moves which move towards a more negative Z should use cutter comp right.
All OD moves which move towards a more positive Z should use cutter comp left.
All ID moves which move towards a more negative Z should use cutter comp left.
All ID moves which move towards a more positive Z should use cutter comp right.
Example:
G41 T03
; Tells the machine to compensate left the amount of the
; nose radius that corresponds to T03 in the Offset
; Library.
Imaginary Tool Nose
Tool nose compensation is necessary to prevent under-cutting (not cutting enough material) on diagonal lines and
arcs. Tool nose compensation does not affect horizontal and vertical lines because in those cases the actual tool
nose is at the same depth as the imaginary tool nose. When tool nose compensation is not used, it is the imaginary
tool nose that moves to the programmed position and not the cutter. Cutter compensation adjusts for the difference
in position by moving the actual tool nose to the programmed position.
Example with tool located on back side of material.
T-Series Operator’s Manual
5/18/11
11-7
Example with tool located on front side of material.
The direction of the imaginary tool nose is related to the nose vector or direction of the tool during cutting (see
Chapter 4). The following drawings show the possible imaginary tool nose directions. Imaginary Tool Nose
directions (tool located in back of material):
The tool nose compensation function (G41 or G42) should be in effect before the tool reaches the cutting start
point.
T-Series Operator’s Manual
5/18/11
11-8
G50 -Coordinate System Setting OR Maximum Spindle Speed for CSS mode
G50 has two functions depending on the supplied parameters:
● With axis parameters, G50 sets the current absolute position to the coordinates specified OR
● With the S parameter, G50 sets the maximum spindle speed when using constant surface speed (see G96 and
G97).
Examples:
G00 X5 Z-2
G50 X1 Z0
G50 S2500
;
;
;
;
;
moves to the specified location
sets the current position to the absolute position
specified.
limit spindle to 2500 rpm in G96 mode, no matter how
close X gets to 0.
G52 - Offset Local Coordinate System
G52 shifts the local coordinate system origin by a specified distance. Multiple G52 codes are not cumulative;
subsequent shifts replace earlier ones. The G52 shift may therefore be canceled by specifying a shift of zero. If
you are using multiple coordinate systems, the G52 shift amount will affect all coordinate systems.
Example:
G0 X0 Z0
M98 P9100
G52 Z4
G0 X0 Z0
M98 P9100
G52 Z0
;
;
;
;
;
;
move to origin
call subprogram
shift coordinate system 4 inches in Z
move to new origin
call subprogram again with new coordinates
restore unshifted coordinate system
G53 - Rapid Positioning in Machine Coordinates
G53 is a one-shot code that performs a rapid traverse using machine coordinates. It does not affect the current
movement mode (G00-G03) or coordinate system (G54-G59).
Example:
G53 X15 Z0
; move to 15,0 in machine coordinates
T-Series Operator’s Manual
5/18/11
11-9
G54 - G59 - Select Work Coordinate System
G54 through G59 select among the six regular work coordinate systems. After issuing the code, subsequent
absolute positions will be interpreted in the new coordinate system.
Example:
G54 G00 X0 Z0
G02 X1 Z-.5 R.5
G55 X1 Z1
; select first WCS, move to origin
; cut something...
; select second WCS, move to 1,1
Using Extended Work Coordinate Systems: There are actually total of 18 workpiece origins. The extra workpiece
origins are not accessible on the Work Coordinate Configuration menu; they can be set using Part Zero Menu. In a
G-code program, the 12 additional workpiece origins may be selected by issuing “G54 P1” through “G54 P12”
Regular WCS
WCS
G-Code
G54
WCS #1
G55
WCS #2
G56
WCS #3
G57
WCS #4
G58
WCS #5
G59
WCS #6
Extended Work Coordinate Systems
WCS
G-Code
WCS
G-Code
G54 P1
G54 P7
WCS #7
WCS #13
G54 P2
G54 P8
WCS #8
WCS #14
G54 P3
G54 P9
WCS #9
WCS #15
G54 P4
G54 P10
WCS #10
WCS #16
G54 P5
G54 P11
WCS #11
WCS #17
G54 P6
G54 P12
WCS #12
WCS #18
G65 - Call Macro
G65 calls a macro with user-specified values. A macro is a subprogram that executes a certain operation (e.g. linear
cut, threading, etc.) with values assigned to variable parameters within the operation.
Calling methods:
G65 Pxxxx Lrrrr Arguments
or
G65 "program.cnc" Lrrrr Arguments
where xxxx is the macro number (referring to file Oxxxx.cnc, 0000-9999 allowed, leading zeros required in
filename, capital O, lower-case .cnc), rrrr is the repeat value, "program.cnc" is the name of the macro file, and
Arguments is a list of variable identifiers and values. Arguments to macro calls are specified by using letters A-Z,
excluding G, L, N, O, and P.
Macros are written just like normal programs. However, macro programs may access their arguments by using #A,
#B, etc., or by using numbers: #1 for A, #2 for B, etc. (exceptions: #4-6 for I-K, #7-11 for D-H). Arguments I, J,
and K can be used more than once in a macro call, with the first set of values stored as #4-6, the second as #7-9,
etc., to a maximum of 10 sets.
Macros 9100 - 9999 may be embedded into a main program, using O91xx to designate the beginning of the macro
and M99 to end it. The CNC software will read the macro and generate a file O91xx.cnc, but will not execute the
macro. It will be executed when G65 is issued.
Example 1:
Main program:
G65 "TEST.cnc" A5 B3
Macro TEST.cnc:
G01 X#B Z-#A
This call will produce:
G01 X3 Z-5
T-Series Operator’s Manual
5/18/11
11-10
Example 2:
Main program:
G65 "TEST2.cnc" I3 J-5 K0.1 I2 J-2 I0 J0
Macro TEST2.cnc:
G01 X#4 Z#5 F#6
G01 X#7 Z#8
G01 X#10 Z#11
This call will produce:
G01 X3 Z-5 F0.1
G01 X2 Z-2
G01 X0 Z0
G70, G71, G72 - Stock Removal Cycles: General
Cleanout cycles remove material from a work piece, leaving a desired contour. The cycle works with the profile
you specify to generate the cleanout moves necessary. The G71 or G72 cleanout cycles can be used to generate
rough contours. After either the G71 or G72 contour cleanout cycles are used, a G70 finish cycle can be used to
produce a more smooth and accurate surface.
Position requirements before start of cycle:
● Outer Diameter Cleanout - the tool's X-axis starting position must be larger than any point on the specified
profile.
● Inner Diameter Cleanout - the tool's X-axis starting position must be smaller than any point on the specified
profile.
● The X's start position must take into account U finish allowance
Simulated jobs that violate position errors are displayed during backplot, but do not terminate. Jobs that violate
position errors are displayed in the operator's message window and are terminated.
If the profile's geometry begins with an arc, a rapid must precede the arc. The rapid actually does not take place.
The G0's position is only used to define the starting point of the arc.
If the profile's first segment is a rapid, the rough finish pass's first move will be a rapid.
Cycle Operation:
The cleanout cycle begins at the X-axis position prior to the start of the cycle. A rapid will be performed in the Zaxis to the starting Z-axis point of the profile if not already there. Once the cycle is finished, the tool is returned to
the start of the profile.
If U (W) and R-values are not specified in the G-code for the cycle, the values already stored in parameters 43, 44
will be used respectively.
The start block value P must be less than the end block value Q. The N end block cannot contain feedrate without a
move. The profile's start block must directly follow the clean out cycle G-codes. Several G-codes and M-codes are
not allowed in the profile.
These M codes are not allowed in the profile:
M2, M7, M8, M9, M10, M11, M26, M30, M50, M51, M91, M92, M102, M105, M106.
T-Series Operator’s Manual
5/18/11
11-11
These G codes are not allowed in the profile:
G7, G20-21, G28, G29, G30, G32, G50, G52, G53, G54-59, G70, G71, G72, G73,
G75, G76, G90, G92, G93, G94.
If cutter compensation is to be used; the G41 or G42 must be turned on prior to the G71/G72 cycle.
Finish allowance (U), depth of cut, and escape amounts are always treated as radius values.
G71 - Stock Removal in Turning
The G71 cycle removes stock in turning (see figure below). In the cycle, the tool starts at position 1 and cuts into
the material with a linear move. In another linear move, the tool cuts through position 2. The tool then pulls back
to position 3 and rapids back to position 1. This cutting cycle is repeated until the desired contour is achieved. The
cycle can perform both inner and outer diameter cleanouts.
Modal values, such as feedrates, in the profile do not take effect in the G71 cycle. Cutter compensation can be used
by the G71 cycle.
The G71 has two forms:
Parameter Setting:
G71 U_R_
U = depth of cut (radius amount); Parameter 43
R = escape amount (radius amount); Parameter 44
Cleanout with U and W:
G71 P_Q_U_W_F_S_T_L_
P = starting block number for profile
Q = ending block number for profile
U = finish allowance on X axis; see G70
W = finish allowance on Z axis; see G70
F = cutting feedrate (previous value if unspecified)
S = spindle or surface speed (previous value if unspecified)
T = tool number and/or offset (previous value if unspecified)
Example 1 -G71 Outer Diameter Cleanout:
G0 X4.5 Z0.4
; Positioning tool before clean out cycle
G71 U.1 R.2
G71 P1 Q8 U0.01 W0.005
N1 G0 X4
; Start block - start of profile definition
T-Series Operator’s Manual
5/18/11
11-12
N2
N3
N4
N5
N6
N7
G1
G1
G1
G1
G3
G1
Z0 F.01
; Second move of profile is Z move
X4 Z-1
X3 Z-3
X3 Z-4
X4 Z-4.5 I0 K-.5
Z-5
; End block - end of profile definition
The resulting contour is shown below:
Example 2 - G71 Inner Diameter Cleanout:
G0 X1 Z0.4
; Positioning
G71 U.1 R.2
G71 P1 Q8 U0.01 W0.005
N1 G0 X4
; Start block
N2 G1 Z0 F.01
; Second move
N3 G1 X4 Z-1
N4 G1 X3 Z-3
N5 G1 X3 Z-4
N6 G1 x4 Z-5
; End block -
tool before clean out cycle
- start of profile definition
of profile if Z move
end of profile definition
The resulting contour is shown below.
T-Series Operator’s Manual
5/18/11
11-13
G72 - Stock Removal in Facing
The G72 cycle removes stock in facing (see figure below). In the cycle, the tool starts at position 1. The tool cuts
downward, in the negative X direction, using a linear move. The tool is then pulled back in the positive Z direction
and rapids back in the positive X direction. The tool then moves to position 2 and proceeds to cut downward with a
linear move. The cycle is repeated until the desired contour is achieved. The cycle can perform both outer and
inner diameter cleanouts.
An escape move that would cause the tool to crash on the backside during a G72 cycle will not take place. Instead,
the tool will rapid back with no escape amount. Modal values, such as feedrates, in the profile do not take effect
during the G72 cycle. Cutter compensation can be used.
The G72 has two forms:
Parameter Setting:
G72 W_R_
W = depth of cut; parameter 43
R = escape amount; parameter 44
Clean out with U and W:
G72 P_Q_U_W_F_S_T_
P = starting block number for profile
Q = ending block number for profile
U = finishing allowance on X axis (radius)
W = finishing allowance on Z axis (radius)
F = cutting feederate (previous value if unspecified)
S = spindle or surface speed (previous value if unspecified)
T = tool number and/or offset (previous value if unspecified)
Examples 1 -G72 Outer Diameter Cleanout:
G0 X4.5 Z0.4
; Positioning tool before clean out cycle
G72 U.1 R.2
G72 P1 Q8 U0.01 W0.005
N1 G0 X4
; Start block - start of profile definition
T-Series Operator’s Manual
5/18/11
11-14
N1
N2
N3
N4
N5
N6
G1
G1
G1
G1
G3
G1
Z0 F.01
; Second move in profile is Z move
X4 Z-1
X3 Z-3
X3 Z-4
X4 Z-4.5 i0 k-.5
Z-5
; End block - end of profile definition
The resulting contour is shown below:
Example 2 - G72 Inner Diameter Cleanout:
G0 X1 Z0.4
; Positioning
G72 U.1 R.2
G72 P1 Q8 U0.01 W0.005
N1 G0 X4
; Start block
N2 G1 Z0 F.01
; Second move
N3 G1 X4 Z-1
N4 G1 X3 Z-3
N5 G1 X3 Z-4
N6 G1 x4 Z-5
; End block -
tool before cleanout cycle
- start of profile definition
in profile is Z move
end of profile definition
The resulting contour is shown below:
T-Series Operator’s Manual
5/18/11
11-15
G70 - Finishing Cycle
The G70 finishing cycle is used in conjunction with a G71 or G72 roughing cycle. The G70 cycle removes material
purposely left by the roughing cycle. A different feedrate and tool can be used to follow the exact contour of the
workpiece during the finishing cycle. Cutter compensation can be used with the finish pass. The type of
compensation used should match the cleanout cycles. The G41/G42 must appear before the G70 cycle is called.
The start and end block of the finish cycle do not need to match the G71/G72 profile. If the user picks block with in
the start and end block, the finish pass will only pass the tool over the picked block's surface.
Multiple finish pass cycles can be performed on a cleaned out contour. For each cycle, multiple passes can be
made. All modal values specified in the profile will take effect when the tool passes over the modal's corresponding
position. If more than one pass is made, the modal values are reset for each pass to their previous values before G70
was installed. G70 finish pass P and Q block values can only reference the previously executed cleanout profile.
The G70 cycle has two forms:
Finishing with no offset:
G70 P_Q_
P = starting block number for profile
Q = ending block number for profile
Finishing with U and W offsets:
G70 P_Q_U_W_
P = starting block number for profile
Q = ending block number for profile
U = finish allowance on X axis
W = finish allowance on Z axis
The cycle uses one or more passes along the profile. The number of passes is determined by the greater of:
G71/G72 allowance W
G70 allowance W
OR
G71/G72 allowance U
G70 allowance U
Examples of obtaining the desired number of finish passes:
Roughing cycle specification:
G71 U allowance = 0.02
G71 W allowance = 0.02
For 1 finish pass:
G70 U allowance = 0.02
or
G70 allowance = 0.0
G70 W allowance = 0.02
G70 allowance = 0.0
For 2 finishing passes:
G70 U allowance = 0.02
G70 W allowance = 0.01
For n finishing passes (each pass removes n amount of material)
G70 U allowance = G71 allowance U/n
G70 W allowance = G71 allowance W/n
Example: G71 Outer Diameter cutout with one finish pass:
G0 X1 Z6
; positioning of the tool before cleanout cycle
G71 U.1 R.2
G71 P1 Q6 U0.010 W0.005
N1 G0 X4
; start block - start of profile definition
N2 G1 Z-1 F.01
; Second move in profile is Z move
N3 G1 X4 Z-2
N4 G1 X3 Z-4
T-Series Operator’s Manual
5/18/11
11-16
N5 G1 X3 Z-5
N6 G3 X4 Z-5.5 I0 K-.5
N7 G1 Z-6
; end block - end of profile definition
G70 P1 Q6 U0.005 W0.005; finish pass
The resulting contour is shown below.
T-Series Operator’s Manual
5/18/11
11-17
G74 - End Face Peck Cutting Cycle
G74 sets the end face peck cutting cycle (chip breaking). If X remains constant at 0 and Z is the only moving axis,
then the peck cutting operation will be similar to the peck drilling operation on a mill. If X moves, grooves will be
cut with the Z-axis breaking the chips
The basic format of the end face peck cutting cycle is as follows:
G74 Rr1
G74 Xx Zz Pp Qq Rr Ff
Where:
r1:
escape/retract amount. This is a modal value and it is not changed until another value is
entered. This value can also be specified in parameter 44 (see Chapter 14).
x:
X value of the end point.
z:
Z value (total depth) of the end point.
p:
X-axis relief amount (radial). This value can be specified in parameter 45 (see Chapter 14).
q:
depth of cut. This value can be specified in parameter 43 (see Chapter 14).
r:
X-axis relief amount. This value can be specified in parameter 46 (see Chapter 14).
f:
feedrate.
● NOTE: In incremental mode X and Z are replaced by U and W, respectively. Also, even though R is used to
specify both ' r1' and ' r ', their functions are specified by the presence of X or U. When X or U is specified, ' r ' is
used.
T-Series Operator’s Manual
5/18/11
11-18
Example 2 (X>0):
G00 X1 Z0
; rapid move
G74 X1.5 Z-1.5 P0.05 Q0.1 R0.03 F.1
; peck cut groove to X1.5 to a Z depth of 1.5 at an increment
; of 0.1, moving in X at 0.05 increments with relief amount of
; 0.03 at the cutting bottom at a feedrate of 0.1.
Example 1 (at X0):
G00 X0 Z0
G74 R0.05
G74 Z-1.5 Q0.2 F0.1
; rapid move
; peck drilling escape/retract amount of 0.05
;(this is a modal value and is not changed
; until another value is entered)
; peck drill hole at X0 to a Z depth of 1.5 at
; an increment of 0.2, at a feedrate 0.1.
T-Series Operator’s Manual
5/18/11
11-19
G75 - Outside/Inside Diameter Peck Cutting Cycle
G75 selects the outer/inner diameter peck cutting cycle. The basic format of the outside/inside diameter peck
cutting cycle is as follows:
G75
G75
Where:
r1:
x:
z:
p:
q:
r:
f:
l
Rr1
Xx Zz
Pp
Qq
Rr
Ff Ll
retract amount. This is a modal value and it is not changed until
another value is entered. This value can also be specified in
Parameter 44.
X value (total depth) of the end point.
Z value of the end point.
Z-axis step amount. This value can also be specified in parameter 45.
depth of cut. This value can also be specified in parameter 43.
Z-axis relief amount. This value can also be specified in parameter 46.
feedrate.
Dwell at end X position
Example with Z step and Z relief amounts:
G00 X3 Z-3 ; rapid move
G75 R0.05
; retract amount of 0.05 (this value is modal and
; is not changed until another value is entered)
G75 X0.5 Z-5 P0.2 Q0.1 R0.05 F.01 L2
; peck cut inner diameter of 0.5 to a length of 2
; inches at an increment of 0.2, moving in x at
; 0.1 increments, relief amount of 0.05 at the
; bottom of cut at a feedrate of 0.01.
; dwell at inner diameter before pull out
T-Series Operator’s Manual
5/18/11
11-20
Example of Peck Cutting with no Z movement:
G00 X3 Z-3
: rapid move
G75 R0.05
; retract amount of 0.05 (this is a modal value
; and is not changed until another value is
; entered)
G75 X0.5 Q0.1 F0.01
; cut inner diameter of 1 at an increment of
; 0.1, feedrate of 0.01.
T-Series Operator’s Manual
5/18/11
11-21
G76 - Multi-Pass Threading Cycle
G76 sets the multi-pass threading cycle command. In this cycle, threading is performed in increments to a specified
depth.
The basic format for this cycle is as follows:
G76
G76
Where,
P:
Pmmrraa Qqmin
Xx Zz Rr Pp
Rqmax
Qq Ff
Q:
R:
mm:
rr :
aa :
qmin:
qmax:
finish count. Can be specified by parameter 50 (see Chapter 14).
chamfering amount. Can be specified by parameter 49 (see Chapter 14).
thread compound angle. Can be specified by parameter 51 (see Chapter 14).
minimum cutting depth. Can be specified by parameter 52 (see Chapter 14).
finish allowance. Can be specified by parameter 53 (see Chapter 14).
R:
P:
Q:
F:
r:
p:
q:
f:
taper radius amount. If 0, straight multi-pass threading will be performed.
thread height
cutting depth in first cut
thread lead (same as in G32)
Example:
G00 X4 Z3
; rapid move
G76 P011055 Q0.05 R0.001
; setting parameters
G76 X2 Z0 R0 P0.5 Q0.1 F0.1 ; multi-pass threading of
; 3 inches in length,
; thread height of 0.5 and
; minor diameter of 2 inches,
; lead of 0.1 and first cut
; depth of 0.1.
● NOTE: The first G76 line, without X and/or Z is optional. Without them, the values previously stored in the
parameters will be used.
T-Series Operator’s Manual
5/18/11
11-22
G80 – Canned Cycle Cancel
G80 is used to cancel a canned cycle once the operation has been performed.
G83 – Deep Hole Drilling
G83 is a deep hole drilling cycle. It periodically retracts the tool to the surface to clear accumulated chips, then
returns to resume drilling where it left off. The retract and return are performed at a rapid rate. Because there may
be chips in the bottom of the hole, the tool does not return all the way to the bottom at the rapid rate. It slows down
to federate a short distance above the bottom. This clearance distance is selected by setting parameter 83 with G10
(see example below).
Example:
G10 P83 R.05
G83 X0 R.1 Z-2 Q.5
T-Series Operator’s Manual
; set clearance to .05”
; drill 2” deep hole in 0.5” steps
5/18/11
11-23
G84 – Tap/Counter Tap
G84 performs both right-hand (Tap) and left-hand (Counter Tap) cycles. The tap direction, spindle speed, spindle
direction, feedrate and/or thread pitch should be set before the G84 is invoked. The tapping direction is set by
calling M29 with or without a P1 parameter (see M29 in Chapter 12). G84 defaults to right-hand Tap cycle if M29
P1 is not specified beforehand. The spindle should be started beforehand using M3 (Spindle CW) for the Tap
cycle, or using M4 (Spindle CCW) for the Counter Tap cycle.
For a floating tap head, the combination of the modal feedrate and spindle speed implicitly determines the
approximate thread lead or pitch. However, if Rigid Tapping is enabled, a Q may be used to explicitly set the
thread lead or pitch. However, because Q is not modal in the case of Rigid Tapping, you must specify Q on every
line at which Rigid Tapping is to occur.
The Tap/Counter Tap cycle might to cut a short distance beyond the programmed Z height as the spindle comes to a
stop before reversing. When tapping blind holes, be sure to specify a Z height slightly above the bottom of the hole
to prevent the tool from reaching bottom before the spindle stops. The exact distance you must allow will depend
on your machine and the diameter and pitch of the tapping tool.
WARNING
NOTICE
FEED HOLD is temporarily disabled during the tapping cycle, but it will be reenabled at the end of the cycle.
Pressing CYCLE CANCEL while the tap is in the hole will very probably break the tap or
strip the threads in the tap hole. However, do so if it is an emergency.
G85 – Boring Cycle
G85 is used to bore a hole so that a smooth finish may be acquired. The tool will feed into depth at the specified
federate and retract back out at the same federate.
G90 - Outside/Inside Diameter Cutting Cycle
G90 sets the outer/inner diameter cutting cycle command. These diameters can be specified along straight cuts or
diagonal/taper cuts.
Straight Cutting
The general form of the Straight Cutting Cycle is as follows:
G90 X_ Z_ P_ L_
In incremental programming form, the X and Z can be substituted with U and W. Note that X (or U) is affected
by the radius/diameter programming mode (see parameter 55 in Chapter 14). The optional parameter P specifies
the length of the return feed move (segment 5 in illustration above). This cycle behaves differently depending on
whether a non-zero P is specified or not. If P does not exist or is 0, then segments 1 and 4 will be rapid moves,
segments 2 and 3 will be feedrate moves, and segment 5 will be omitted. If P does exist and is non-zero, then
segment 4 will be a rapid move and all the other segments will be feedrate moves. The optional parameter L
specifies a dwell time between segments 2 and 3.
T-Series Operator’s Manual
5/18/11
11-24
Example:
G00 X2.5 Z-1.0
G90 X1.5 Z-4.0 F0.5 L1.5
; rapid to start point
; G90 cycle with 1.5 sec dwell at X1.5 Z-4.0
Taper Cutting
The general form of the Taper Cutting Cycle is as follows:
G90 X_ Z_ R_ P_ L_
This is actually the same as the Straight Cutting cycle (mentioned above) but with the addition of the R parameter.
Parameters P and L are optional. Taper is determined by offsetting the point between segments 1 and 2 on the X
coordinate by the incremental amount specified by the R parameter. Note that R is unaffected by the
radius/diameter programming mode, but X is (see parameter 55 in Chapter 14). All the other parameters have the
same meaning as those of the Straight Cutting cycle (mentioned above).
Example:
G00 X2.5 Z-1.0
G90 X1.5 Z-4.0 R-0.25 F0.5
; rapid to start point
; Tapered G90 cycle
The following table shows the relationship between the tool paths and the signs of U, W, and R during incremental
programming when performing taper cutting.
T-Series Operator’s Manual
5/18/11
11-25
G92 - Thread Cutting Cycle
G92 sets the thread cutting cycle command. This cycle can be specified for straight thread cutting or taper thread
cutting. In incremental programming, the signs of U and W will depend on the direction of the tool path when
approaching the workpiece. That is, if the cutter moves in the negative X direction, then the value of U will be
negative.
G92 is similar to G32 in that X and Z indicate the endpoint of the cut and F indicates the thread lead and X & Z are
slaved to the spindle. The chamfering amount, rr, which is selected by parameter 49 (see Chapter 14), is a multiplier
of the thread lead. That is, the chamfer distance is rr times the thread lead.
Straight Thread Cutting
In this cycle, the cutter moves to the diameter
indicated by X and threads in a straight line to
the depth or length indicated by Z. In the
example below, the cutter first rapids to the start
point located at X2.5Z-1, then rapids down to
X2 at the same Z, and then cuts with the
specified lead to Z-3. At Z-3, the cutter pulls out
of the part the amount of the chamfering
distance, then rapids back up to X2.5 and returns
to the start point.
Example:
G00 X2.5 Z-1.0
; Step 1
G92 X2.0 Z-3.0 F.1 ; Steps 2,3
; & 4
Taper Thread Cutting
In this cycle, the cutter threads diagonally to the
diameter and depth indicated by X and Z,
respectively. The value of R will dictate the
value of the starting diameters. A negative R will
make the ending diameter equal to X and the
starting diameter equal to X minus twice the
absolute value of R. A positive R will make the
ending diameter equal to X and the starting
diameter equal to X plus twice the value of R.
T-Series Operator’s Manual
5/18/11
11-26
In the example below, the cutter first rapids to the start point located at X3.5 Z-1, then rapids down to X2.5, the
inner diameter, at the same Z, and then cuts with the specified lead to Z-3. At Z-3 the value of the outer diameter is
2.5 and the cutter pulls out of the part the amount of the chamfering distance, then rapids back up to X2.5 and
returns to the start point.
Example:
G00 X3.5 Z-1.0
G92 X2.5 Z-3.0 R-0.25 F.1
Multiple thread leads
This is done by using the formula:
2nd – nth thread lead start point = previous thread lead start point + ((1/TPI) / # of leads)
Example:
We want to produce a triple lead thread with a thread lead of 10 threads per inch (TPI). The start point for the first
thread lead is 0.1000 from the face of the material being threaded.
Thread lead # 1 start point = 0.1000.
Thread lead # 2 start point = 0.1000 + ((1/10)/3) = 0.1333.
Thread lead # 3 start point = 0.1333 + ((1/10)/3) = 0.1666.
T-Series Operator’s Manual
5/18/11
11-27
G94 - End Face Turning
G94 sets the end face turning cycle command. This cycle can be specified for straight face turning or taper face
turning. In incremental programming, the signs of U and W will depend on the direction of the tool path when
approaching the work piece. That is, if the cutter moves in the negative X direction, then the value of U will be
negative. The L parameter can be set to allow the part to rotate at least one full revolution, at the end X position,
before the tool is moved back to the starting Z position.
Straight Face Turning
In this cycle, the cutter moves to the depth indicated by
Z and then cuts to the diameter indicated by X. In the
example below, the cutter first rapids to the start point
located at X2Z-1, then rapids to Z-1.25 at the same X,
and then cuts at the specified feedrate to X1. At X1, the
cutter dwells for .5 secs, then moves back to Z-1 at the
same feedrate and rapids back up to the start point.
Example:
G00 X2.0 Z-1.0
G94 X1.0 Z-1.25 F0.1 L.5
Taper Face Turning
In this cycle, the cutter cuts diagonally to the diameter
and depth indicated by X and Z, respectively. The value
of R will dictate the approach of the cutter to the
specified Z coordinate, that is, the value of R will
determine how much the cutter will stop short (positive
R) or pass (negative R) Z before cutting diagonally down
to the specified diameter.
In the example below the value of R is negative, thus,
the cutter first rapids to the start point located at X2Z-1,
then rapids to Z-1.5 at the same X, and then cuts
diagonally down to X1 at the specified feedrate. At X1,
the value of Z is -1.25, then the cutter moves back to Z-1
at the same feedrate and rapids back up to the start point.
Example:
G00 X2.0 Z-1.0
G94 X1.0 Z-1.25 R-0.25 F0.1
T-Series Operator’s Manual
5/18/11
11-28
The following table shows the relationship between the tool paths and the signs of U, W, and R during incremental
programming when performing taper face turning.
G96 & G97 - Constant Surface Speed Control & Cancel
G96 sets the mode for constant surface speed control in feet/min (sfm) or meters/min. S values are assumed as
surface speed. When CSS is active, the spindle speed changes as the X position changes, to maintain a constant
linear velocity at the tool tip. No matter how close X gets to X0, the spindle speed will not exceed the speed set
with G50 or the machine's maximum spindle speed, whichever is less. G97 cancels the constant surface speed
control.
G96 S800
G01 X1 Z-3 F0.1
G97 S1200
; sets constant surface speed to 800 feet/min
; cancels constant surface speed and sets
; spindle speed to 1200 rpm
G98 - Feed per minute
G98 sets the cutting feedrate mode in units/minute. There are no associated parameters.
G99 - Feed per revolution
G99 sets the cutting feedrate mode in units/rev. There are no associated parameters.
T-Series Operator’s Manual
5/18/11
11-29
T-Series Operator’s Manual
5/18/11
11-30
Chapter 12
M functions
M-functions are used to perform specialized actions in CNC programs. Most of the T-series Control M-functions
have default actions, but they can be customized with the use of macro files.
Certain restrictions apply to calling M functions:
● Only one M function per program line is permitted.
● M-functions are not allowed on the same line as a tool change (see T in Chapter 10).
Summary of M functions
M00 Stop For Operator
M01 Optional Stop for Operator
M02 Restart Program
M03 Spindle On Clockwise
M04 Spindle On Counterclockwise
M05 Spindle Stop
M07 Mist Coolant On
M08 Flood Coolant On
M09 Coolant Off
M10 Clamp On
M11 Clamp Off
M13 (macro) Cutoff *
M16 (macro) Chuck ID selection *
M18 (macro) Chuck OD selection *
M19 (macro) Spindle Orient *
M22 (macro) Extend part chute *
M23 (macro) Retract part chute *
M26 Set Axis Home
M29 Set Tap Mode for G84
M32 (macro) Tailstock Quill forward (out) *
M33 (macro) Tailstock Quill retract (in) *
M34 (macro) Part Catch forward *
M35 (macro) Part Catch retract *
M41,M42,M43 (macro) Select Spindle Gear Range *
M46 (macro) Door Open *
M47 (macro) Door Close *
M50 C Axis Disable
M51 C Axis Enable
M91 Move to Minus Home
M92 Move to Plus Home
M93 Release/Restore Motor Power
M94/M95 Output On/Off
M98 Call Subprogram
M99 Return from Macro or Subprogram
M100 Wait for PLC bit (Open, Off, Reset)
M101 Wait for PLC bit (Closed, On Set)
M102 Restart Program
M103 Programmed Action Timer
M104 Cancel Programmed Action Timer
M105 Move Minus to Switch
M106 Move Plus to Switch
M107 Output BCD Tool Number
M108 Enable Override Controls
M109 Disable Override Controls
M115,M116,M125,M126 Protected Move Probing Functions
M120 Open data file (overwrite existing file)
M121 Open data file (append to existing file)
M122 Record position(s) in data file
M123 Record value and/or comment in data file
M124 Record machine position(s) in data file
M127 Record Date and Time in a data file
M128 Move Axis by Encoder Counts
M150 Set Spindle Position to 0 on Next Index Pulse
M151 Unwind C axis
M200 Stop for Operator, Prompt for Action
M223 Write Formatted String to File
M224 Prompt for Operator Input Using Formatted String
M225 Display Formatted String for A Period of Time
M300 Fast Synchronous I/O update
M1000-M1015 Graphing Color for Feedrate movement
* M functions marked with “(macro)” actually have no standard default action, and could possibly be
unimplemented and therefore unavailable on your machine. Also, their stated function is only standard on certain
machines.
T-Series Operator’s Manual
5/18/11
12-1
Macro M functions (custom M functions)
Macro M functions are M functions that have been customized with a macro file. The T-Series CNC M functions
from 0 through 90 can be fully customized. No M-functions above 90 may be customized with macros. The
default action listed will be performed unless that M-function has been customized.
To create a macro for an M-function, a file must be created in the C:\cnct directory. The file's name must be
mfuncXX.mac where XX is the M-function number used to call the macro. M-functions 0-9 must use single digits
in the filename (e.g. use mfunc3.mac, not mfunc03.mac). The contents of the file may be any valid M and Gcodes.
The following is an example macro M-Function to turn on spindle with variable frequency drive and wait for "at
speed" response.
M94/1 ; request spindle start
M101/5005
; wait for up to speed signal
These lines would be placed in the file c:\cnct\mfunc3.mac. Each time the M-function is encountered in a program,
the macro file will be processed line by line.
● NOTE: Nesting of macro M-functions is allowed, but, recursive calls are not. If a macro M-function does call
itself, the default action of the function will be executed.
● NOTE: The M and G-codes within a macro M-function are not usually displayed on the screen as they are
executed, and are all treated as one operation in block mode. If you wish to see or step through macro M-functions
(e.g. for testing purposes), see Machine Parameter 10 in Chapter 14
● NOTE: The cnctch.mac file, which contains the G-code sequence for doing a customized tool change, is also
considered to be an M-function Macro so that its behavior can be modified by Machine Parameter 10.
12-2
5/18/11
T-Series Operator’s Manual
M00 - Stop For Operator
Motion stops and the operator is prompted to press the CYCLE START button to continue.
M01 - Optional Stop for Operator
M1 has no effect unless optional stops are turned on. When optional stops are on, M1 is identical to M0.
Default action:
M100/75
; if optional stops are turned on.
M02 - Restart Program
Restarts the program from the first line. The operator is prompted to press the CYCLE START button to continue.
M03 - Spindle On Clockwise
M3 requests the PLC to start the spindle in the clockwise direction.
Default action:
M95/2
M94/1
M04 - Spindle On Counterclockwise
M4 requests the PLC to start the spindle in the counterclockwise direction.
Default action:
M95/1
M94/2
M05 - Spindle Stop
M5 requests the PLC to stop the spindle.
Default action if the spindle had been spinning CW:
M95/2
M95/1
Default action if the spindle was OFF or was spinning CCW:
M95/1
M95/2
M07 - Mist Coolant On
M7 causes the PLC to start the mist coolant system.
Default action:
M95/3
M94/5
M08 - Flood Coolant On
M8 causes the PLC to start the flood coolant system.
Default action:
M95/5
M94/3
T-Series Operator’s Manual
5/18/11
12-3
M09 - Coolant Off
M9 causes the PLC to stop the coolant system.
Default action:
M95/3/5
M10 - Clamp On
M10 causes the PLC to activate the clamp.
Default action:
M94/4
M11 - Clamp Off
M11 causes the PLC to release the clamp.
Default action:
M95/4
M19 – Spindle Orient (Macro)
M19 has no default action, therefore a custom M19 macro must be defined for this feature to work. If defined, the
M19 macro sends a request to the PLC to rotate the spindle to its pre-set orient position.
M26 - Set Axis Home
M26 sets the machine home position for the specified axis to the current position (after the line's movement).
Example:
M92/X
M26/X
M91/Z
M26/Z
;
;
;
;
home X axis
set machine
home Z-axis
set machine
to plus home switch
home for X-axis there
to minus home switch
home for Z-axis there
M29- Set Tap Mode for G84
M29 sets the tap mode for G84; either right-hand or left-hand tapping. Right-hand tap mode is the initial default at
job start-up. If Left-hand tap mode is required, M29 and P1 need to be specified on the same line.
Tap Mode
CW ( Right-hand )
CCW ( Left-hand )
Command
M29
M29 P1
M41, M42, M43 – Select Spindle Gear Range (Macros)
M41, M42, and M43 have no default actions, and therefore custom macros must be defined for these M codes in
order to make this feature work. If defined, these macros notify the PLC of which spindle gear range is selected
according to the following table:
Macro M function
M41
M42
M43
12-4
Action
Select Low Gear Range
Select Medium-Low Gear Range
Select High Gear Range
5/18/11
T-Series Operator’s Manual
M50 – C Axis Disable
M50 is the command to disable the C axis and it is a locked software option. When the C axis is disabled, no axis
label will be present on the screen and the encoder information for the C axis is ignored. In order for the M50
command to work, the 3rd or 4th axis label must be set to ‘C’ with the associated parameter (93 for 3rd axis and 94
for 4th axis) set for C axis operation. In practical applications, the default behavior for the M50 command is usually
modified using a custom mfunc50.mac program.
Example mfunc50.mac:
M95/9
; Switch to speed mode
M50
; Perform the default actions for C axis disable
M51 – C Axis Enable
M51 is the command to enable the C axis and it is also locked as a software option.. When C axis is enabled, the C
axis label will be present on the DRO and encoder information for the C axis is used to determine the position of
the C axis. In order for the M51 command to work, the 3rd or 4th axis label must be set to ‘C’ with the associated
parameter (93 for 3rd axis and 94 for 4th axis) set for C axis operation. In practical applications, the default behavior
for the M51 command is modified using a custom mfunc51.mac program to ensure that the spindle has stopped
before the C axis is enabled.
Example mfunc51.mac:
G97
; Turn off CSS (constant surface speed)
M3 S0
; Turn off spindle
M101/9
; Wait for zero speed signal form inverter on INP9
M94/9
; Switch to torque mode
M51
; Perform the default actions for C axis enable
M151
; Unwind C-axis position
Note in the above examples for M50 and M51 where the M95/9 (turn off INP41) and M94/9 (turn on INP41)
commands are used, it is assumed that the plc program, conditioned upon the state of INP41, has been modified to
output the appropriate hardware signals required to switch between speed and torque mode.
M91 - Move to Minus Home
M91 moves to the minus home switch of the axis specified at the slow jog rate for that axis. After the minus home
switch is reached, the tool is moved back until the home switch resets. Then the next encoder index pulse is
reached.
Example:
M91/Z
G50 Z-10
; move the Z-axis to the minus home switch.
; sets Z minus home switch at -10
M92 - Move to Plus Home
M92 moves to the plus home switch of the axis specified at the slow jog rate for that axis. After the plus home
switch is reached, the tool is moved back until the home switch resets. Then the next encoder index pulse is
reached.
Example:
M92/X
G50 X+10
; moves the X-axis to the plus home switch.
; Sets X plus home switch at +10
T-Series Operator’s Manual
5/18/11
12-5
M93 – Release/Restore Motor Power
M93 releases or restores motor power for the axis specified. If no axis is specified, then all axes are released.
Example:
To release motor power:
M93/X
M93
; releases the X axis.
; releases the motors on all axes.
Example:
To restore power:
M93/X P1
M93 P1
; restore power to the X axis motor.
; restore power to the motors on all axes.
● NOTE: Any axis freed within a CNC program should not be used in that program afterwards. Incorrect
positioning may result.
M94/M95 - Output On/Off
There are 128 user definable system variable bits that can be used to communicate with the PLC. M94 and M95
are used to request those system variable bits to turn on or off respectively. Requests 1-128 are mapped to the PLC
as system variables SV_M94_M95_1 through SV_M94_M95_128 as shown in the following table:
On
M94/1
M94/2
M94/3
M94/4
.
.
.
M94/128
Off
PLC bit
M95/1
SV_M94_M95_1
M95/2
SV_M94_M95_2
M95/3
SV_M94_M95_3
M95/4
SV_M94_M95_4
.
.
.
.
.
.
M95/128 SV_M94_M95_128
To use M94 and M95 to control a function external to the servo control, such as an indexer, the input request must
be mapped to one of the PLC outputs in the PLC program. See M94/M95 function usage in the PLC section of the
service manual.
Example:
M94/5/6 ; turns on SV_M94_M95_5 and SV_M94_M95_6.
* NOTE: M94 and M95 will cause prior motion to decelerate to a stop before the requested bits are turned on or
off.
* NOTE: Requests 1-5, 15, and 16 are controlled by the default actions of M3, M4, M5, M6, M7, M8, M9, M10,
M11, and M39. To override or disable a bit used in one of these M codes, define a custom M-function.
12-6
5/18/11
T-Series Operator’s Manual
M98 - Call Subprogram
M98 calls a user-specified subprogram. A subprogram is a separate program that can be used to perform a certain
operation (e.g. a drilling pattern, contour, etc.) many times throughout a main program.
Calling methods:
M98 Pxxxx Lrrrr
or
M98 "program.cnc" Lrrrr
where xxxx is the subprogram number (referring to file Oxxxx.cnc, 0000-9999 allowed, leading 0's required in
filename, capital O, lowercase .cnc), rrrr is the repeat value, and "program.cnc" is the name of the subprogram file.
Subprograms are written just like normal programs, with one exception: an M99 should be at the end of the
subprogram. M99 transfers control back to the calling program.
Subprograms can call other subprograms (up to 20 nested levels of calling may be used), Macro M-functions, and
Macros. Macro M-functions and Macros can similarly call subprograms.
Subprograms 9100-9999 can also be embedded into a main program, using O9xxx to designate the beginning of the
subprogram and M99 to end it. CNC11 will read the subprogram and generate a file O9xxx.cnc. CNC11 will not
execute the subprogram until encounters M98 P9xxx.
● NOTE: An embedded subprogram definition must be placed before any calls to the subprogram.
M99 - Return from Macro or Subprogram
M99 designates the end of a subprogram or macro and transfers control back to the calling program when executed.
M99 may be specified on a line with other G-codes. M99 will be the last action executed on a line. If M99 is not
specified in a subprogram file, M99 is assumed at the end of the file:
Example:
G1 X3 M99 ;Move to X3 then return to calling program.
If M99 is encountered in the main job file, it will be interpreted as the end of the job. If M99 is encountered in an
M-function macro file, it will be interpreted as the end of any enclosing subprogram or macro or as the end of the
job.
T-Series Operator’s Manual
5/18/11
12-7
M100 - Wait for PLC bit (Open, Off, Reset)
M101 - Wait for PLC bit (Closed, On Set)
The M100/M101 commands wait for a PLC bit to reach a state as indicated in the table below.
Number
PLC bit
M100
M101
50001 – 51312 INP1 – INP1312
open
closed
60001 – 61312 OUT1 – OUT1312
off
on
70001 – 71024 MEM1 – MEM1024
reset
set
90001 – 90064 T1 – T64 status bits
reset (not expired) set (expired)
93001 – 93256 STG1 – STG256 status bits
reset (disabled)
set (enabled)
94001 – 94256 FSTG – FTSG256 status bits
reset (disabled)
set (enabled)
The number ranges 1-240 can be used to reference the first eighty INP, OUT, or MEM bits.
It is recommended that existing CNC10 programs and macros be converted to the new
ranges for use with CNC11.
1 – 80
INP1 – INP80
open
closed
81 – 160
OUT1 – OUT80
off
on
161 – 240
MEM1 – MEM80
reset
set
Example:
M101/50001 ; wait for INP1 to close
M100/60002 ; wait for OUT2 to turn off
M101/70123 ; wait for MEM123 to be set (1)
NOTE: The numbers assigned to the PLC bits (except 1-240) are the same as those that can be used when
referencing system variables in M- and G-code programs.
M102 - Restart Program
M102 performs any movement requested, and restarts the program from the first line. The operator is NOT
prompted to press the CYCLE START button to continue.
M103 - Programmed Action Timer
M103 starts a timer for the operations in a program. If M104 (stop timer) is not executed before the specified time
expires, the program will be canceled and the message "Programmed action timer expired" will be displayed. This
function is used to detect the failure of a device connected to the PLC and prevents further programmed action.
Example:
Activate a device and wait for a response. If no response within 4.5 seconds, cancel the program.
M94/12 ; turn on relay
M103/4.5
; start 4.5 second timer
M100/4 ; wait for input 4 to open
M104
; input 4 opened, cancel timer
● NOTE: The PLC program must detect the cancellation of the program and deactivate all programmed machine
functions.
12-8
5/18/11
T-Series Operator’s Manual
PLC Program for the above Example:
;PLC program
CNC_program_running is INP65
M12 is INP44
relay_out is OUT5
relay_out = M12 & CNC_program_running
;program running indicator
;M-function 12 indicator
;relay On/Off
;Relay On if M94/12 and the
;CNC program is active. Relay
;Off if M95/12 or the CNC
;program is terminated.
M104 - Cancel Programmed Action Timer
M104 stops the timer started by the last M103 executed.
M105 - Move Minus to Switch
M105 moves the requested axis in the minus direction at the current feedrate until the specified switch opens (if the
given P parameter is positive), or until the scecified switch closes (if P parameter is negative).
Example:
M105/X P5 F30
; move the X axis in minus direction at 30"/min until
; the switch on INP5 opens
; Sets X position to 10
; move the Z axis in minus direction until switch on INP6 closes
G92 X10
M105/Z P-6
M106 - Move Plus to Switch
M106 moves the requested axis in the plus direction at the current feedrate until the specified switch opens (if the
given P parameter is positive), or until the scecified switch closes (if P parameter is negative).
Example:
M106/Z P3 F30
; move the Z axis in the plus direction at 30"/min, until
; the switch on INP3 opens
; Sets Z position to 10
; move the X axis in the plus direction until the switch on INP3 closes
G92 X10
M106/X P-3
M107 - Output BCD Tool Number
M107 sends the current tool number to the automatic tool changer, via the PLC. The number is sent as BCD
(binary coded decimal). M107 does not set the tool changer strobe or look for an acknowledge from the changer.
Example:
M107
M94/16
M101/5
M95/16
M100/5
;
;
;
;
;
send
turn
wait
turn
wait
request for tool to changer
on tool changer strobe
for acknowledge on input 5
off strobe
for acknowledge to be removed
M108 - Enable Override Controls
M108 re-enables the feedrate override and/or spindle speed override controls if they have previously been disabled
with M109. A parameter of 1 indicates the feedrate override; a parameter of 2 indicates the spindle speed override.
Example:
M109/1/2
M108/1
M108/2
; disable feedrate and spindle speed overrides
; re-enable feedrate override
; re-enable spindle speed override
T-Series Operator’s Manual
5/18/11
12-9
M109 - Disable Override Controls
M109 disables the feedrate override and/or spindle speed override controls. M109 cannot be used in MDI mode.
Example:
M3 S500
M109/1/2
M108/1/2
; start spindle clockwise, 500 rpm
; disable feedrate and spindle speed overrides
; re-enable overrides
M115/M116/M125/M126 – Protected Move Probing Functions
The protected move probing functions provide the capability to program customized probing routines. The
structure for these commands is:
Mnnn
nnn
Axis
pos
p
f
L1
Q1
/Axis pos Pp Ff
is either 115, 116, 125, or 126.
is a valid axis label, i.e., X, Z, etc.
is an optional position
is a plc bit number, which can be negative.
is a feedrate (in units per minute.)
is an option for the M115/M116 commands that prevents an error if the probe does not detect a surface
is an option for M115/M116 that forces the DSP probe to move a “Recovery Distance” on retries
(Note: the Q1 option only applies for DSP Probes)
For M115 and M116 functions, the indicated axis will move to pos (if specified) until the corresponding plc bit p
state is 1, unless p is negative, in which case movement is until the plc bit state is 0. A p value of 1 to 80 (or -1 to 80) specifies plc bits INP1-INP80, 81 to 160 (or -80 to -160) specifies plc bits OUT1-OUT80, and 161 to 240 (or 161 to -240) specifies plc bits MEM1-MEM80. Warnings are generated in the CNC11 message window for
"Missing P value" and "Invalid P value."
If pos is not specified, M115 will move axis in the negative direction, and M116 will move axis in the positive
direction. Note that is pos is specified, then if does not matter whether M115 or M116 is used.
If pos is not specified, the movement is bounded by the settings in the software travel limits. In the absence of
software travel limits, movement is bounded by the maximum probing distance (Machine Parameter 16). In cases
where pos is specified, it is still bounded by the software travel limits.
If the bounded position is reached before the awaited plc bit state is found, a "Probe unable to detect surface" error
will be generated unless the L1 option is specified.
For M125 and M126 protected move functions, the behavior is identical to that of the M115 and M116 commands,
except in regards to the plc bit state. M125 and M126 will generate an "Unexpected probe contact" error message
if the specified plc bit state is triggered, again stopping any running job.
In summary, the M115 and M116 commands are to be used when one expects contact to be made and M125 and
M126 commands are to be used when one does not expect any contact to be made.
Example:
M115/X P-15 F20
M116/X P15 F5
12-10
; Move X minus at 20ipm waiting for contact on INP15
; Move X plus until no contact at 5 ipm
5/18/11
T-Series Operator’s Manual
M120 - Open data file (overwrite existing file)
This M function will open the requested data file for writing. If no drive or directory is specified with the file
name, then the file will be opened in the same directory as the CNC program. If the file cannot be successfully
opened, then an error will be returned, ultimately terminating the job. If a data file is already open when M120 is
called, that file will first be closed, then the new file opened.
Example:
M120 "probetst.dat"
M121 - Open data file (append to existing file)
This M function will open the requested file for writing at the end of the file. If no drive or directory is specified
with the file name, then the file will be opened in the same directory as the CNC program. If the file does not
already exist, it will be created. This is not an error. If the file cannot be successfully opened, then an error will be
returned, ultimately terminating the job. If a data file is already open when M121 is called, that file will first be
closed, then the new file opened.
Example:
M121 "c:\probetst.dat"
M122 - Record position(s) and optional comment in data file
This M function will write the current expected position value to the data file, in the usual format (i.e. axis label
before number, 4 decimal places in inch mode, 3 decimal places in millimeter mode. Any comment that appeared
on the line with M122 will be output after the position(s). With no axis arguments, M122 will write the positions of
all installed axes. With axis arguments, it will write the positions only of the requested axes. Positions will be
written in local (not machine) coordinates, in native machine units. If no data file has been opened with M120 or
M121 before M122 is called, then M122 will return an error and terminate the job. The parameter L1 may be used
to suppress the new line character normally outputted after the last position.
Examples (M function and sample output):
M122
->
X1.2345 Z-0.5678
M122 /Z ; at 10 ipm
->
Z-.4321 ; at 10 ipm
M122 /X/Z
->
X-1.0000 Z0.8732
M122 /X L1
->
X-1.5000
M122 /X
->
X-1.5000 X-2.0000
M123 - Record value and/or comment in data file
This M function will write the specified parameter value (if any) to the data file, followed by any comment that
appeared on the line with M123. If a P value is specified, M123 will output a numeric value (4 decimal places in
inches, 3 in millimeters). If no P value is specified, then M123 outputs the comment only. If neither a P value nor
a comment was specified, M123 does nothing. This is not an error. If no data file has been opened with M120 or
M121 before M123 is called, then M123 will return an error and terminate the job. The parameter L1 may be used
to suppress the new line character normally outputted after the last value. The R and Q parameters can be used to
specify the field width and precision, respectively.
T-Series Operator’s Manual
5/18/11
12-11
Examples (M function and sample output):
M123 P1.2345
->1.2345
M123 P#A ; first macro argument ->1.2345 first macro argument
M123 ; Probing X+ to surface
->Probing X+ to surface
M123
-><nothing>
M123 ;
-><nothing>
M123 ;; my comment
->; my comment
M123 Q0 P1.23
->1
M123 Q1 P1.23
->1.2
M123 R7 Q2 L1 P1.234
M123 R7 Q2
P98.765
->
1.23
98.77
M124 - Record machine position(s) and optional comment in data file
Identical to M122 above except that the m124 reports machine position instead of a local WCS position.
M127 - Record Date and Time in a data file
This M function is used to write the date, time, and year to the specified data file called out by the M120 or M121.
Examples (M function and sample output):
M121 “testdata.dat”
M127
If you opened testdata.dat you would see: Day of week, Month, day, time, and year.
(i.e. Wed Aug 29 11:56:57 2007)
M128 – Move Axis by Encoder Counts
M128 moves the requested axis by L which specifies an encoder count position or quantity. The L parameter is
subject to the current G90/G91 mode (absolute/incremental).
Example:
G91 M128/X L-5000
; move the X axis incrementally by -5000 counts
M150 – Set Spindle Position to 0 on Next Index Pulse
M150 will cause the spindle encoder position to be reset to 0 upon the next encounter of the spindle encoder’s
index pulse. M150 will not generate spindle movement. As a matter of fact, the spindle needs be be commanded to
move in order for M150 to work.
M151 – Unwind C axis
This M function will reset the C axis position to less than one revolution of the C axis (< 360 degrees).
Example (M51)
G97
; Turn off CSS (constant surface speed)
M3 S0
; Turn off spindle
M101/9
; Wait for zero speed signal form inverter on INP9
M94/9
; Switch to torque mode
M51
; Perform the default actions for C axis enable
M151
; Unwind C-axis position
Note in the above examples for M50 and M51 where the M95/9 (turn off INP41) and M94/9 (turn on INP41)
commands are used, it is assumed that the plc program, conditioned upon the state of INP41, has been modified to
output the appropriate hardware signals required to switch between speed and torque mode.
Warning: The spindle must be stopped before issuing the M151 or
unpredictable positions can result.
12-12
5/18/11
T-Series Operator’s Manual
Formatted String Commands- M200, M223, M224 & M225
The formatted string commands are provided to assist in custom screen and file I/O. A “formatted-string”
is similar to the C programming language “printf” command, with various restrictions. The basic form of
a formatted-string is a quoted string (comprised of a single line of up to 1024 characters) followed by a
(possibly empty) list of user and/or system variable expressions. The variable expression is a '#' character
followed by a number or bracketed expression. For example, given #100 = 88* (ASCII 'X'), #300 = “absolute”, and
#101 = 1.2345, this string:
“The %c* axis %s position is %f” #100 #300 #101 evaluates to “The X* axis absolute position is 1.234500”
The “%c”* is replaced by the ASCII character value of user variable #100, the “%s” is replaced by the string user
variable #300, and the “%f” is replaced by the value of user variable #101.
Type specifiers
The 's', 'c', and 'f' are type specifiers, with 's' specifying a string user variable, 'f' specifying a floating point user
variable, and 'c' specifying a single character substitution using the integer part of a floating point user variable.
There should be one user variable expression for every '%' character in the quoted string. It is also possible to
specify a field width by inserting a number between the '%' and the type specifier. Example:
%20s – specifies that the substituted string is displayed in a field 20 characters long, right justified and padded
with spaces on the left. Use “%-20s” for left justification.
The 'f' type can specify a precision such as:
•
“%.4f” - display number rounded at the fourth decimal place.
•
“%9.4f” - as above but in a field width nine characters wide.
•
“%+9.4f” - as above with a '+' output if variable is positive.
•
“%.0f” - display number rounded to integer
Special characters
The quoted string may contain up to “\n” which will be converted to a single newline character- up to seven
newlines can be used in a single formatted string- but it may not contain an embedded quote character '”' or
other printf-style escape sequences such as '\t', '\\', or '\”'. If a quote character is desired, use a %c type specifier
with a variable expression equal to 34.
User string variables #300-#399. These variables can be assigned a quoted string up to 80 characters in length
and are retained until the CNC software is exited. For example,
#300 = “What we have here is a failure to communicate”
*The above method of representing an axis label should be used only when writing to an external file or for display
in a message box. It is not valid if you are attempting to “build” a motion command in real-time from within the
currently running g code program. If your intent is to use a variable to represent an axis label for a real-time
command, you should instead use $ as the placeholder. The parser will replace a '$' character and the numerical
expression following it with the ASCII character equivalent to the numerical expression, provided that it evaluates
to the characters 'A' (65) through 'Z' (90). If the numerical expression is out-of-bounds, an “Invalid character” error
occurs. Ex:
Given #100 = 88, #101 = 1, #102 = 89, #103 = 2 and #104 = 10
G1 $[#100][#101] $[#102][#103] F[#104] evaluates to G1 X1 Y2 F10
T-Series Operator’s Manual
5/18/11
12-13
M200 – Stop for Operator, Prompt for Action
This M function is used to pause the currently running job and prompt the operator for action. If
M0_jogging is unlocked, or the control is in DEMO mode, jogging is enabled while waiting for the operator to
respond. If this option has not been enabled, the behavior will default to that of a standard M0. (jogging disabled)
The syntax is: M200 formatted-string [[user_var_expr] ...]
Example: (M function and sample output):
M200 “Please jog the %c and %c axes to the desired X0, Y0 position\nPress Cycle Start to continue” #100 #101
M223 – Write Formatted String to File
The M223 command writes a formatted-string to a file that was opened using the M120 or M121 commands. The
syntax is:
M223 formatted-string [[user_var_expr] ...]
Example: (M function and sample output):
M223 “; The measured diameter of the pocket = %.4f” #100
M224 – Prompt for Operator Input Using Formatted String
The M224 command displays a formatted-string and then accepts user input. The syntax is:
M224 lvalue_expr formatted-string [[user_var_expr] ...]
Where lvalue_expr is a user_var_expr that evaluates to a user variable that can be written. If lvalue_expr is a string
type (#300-#399) then the user input is assigned verbatim to the string. Otherwise, the user input is evaluated as any
other “bracketed” numerical expression.
Example: (M function and sample output):
M224 #300 “Please enter the direction that you wish to probe in the %c axis: (+ or -)” #100
M300 – Fast Synchronous I/O update
There are 32 user definable fast system integer variables that can be used to communicate with the PLC (similar to
M94 and M95), but without causing motion to decelerate to a stop* (unlike M94 and M95). The syntax is:
M300 /nn /vvv
where nn is 1-32 and vvv is a 32-bit signed integer value. The parameter nn (1-32) maps to system
variables SV_FSIO1 - SV_FSIO32. These commands work in conjunction with a PLC program that can
read the SV_FSIOx and act upon them.
Example:
M300 /21 /-1234 ; set SV_FSIO21 to integer value -1234
* NOTE: Motion will be decelerated to a stop if Smoothing is turned on (P220 = 1).
12-14
5/18/11
T-Series Operator’s Manual
M225 – Display Formatted String for A Period of Time
The M225 command displays a formatted-string for a specified period of time. The syntax is:
M225 time_expr formatted-string [user_var] ...
where time_expr is a user_var_expr that evaluates to a floating point variable specifying the number of seconds to
display the output, with a value of zero interpreted as indefinitely. The CYCLE_START key can be used to
immediately continue running without waiting for the time to expire.
Example: (M function and sample output):
M225 #100 “Warning, %s is not selected\nPlease select %s and press Cycle Start to continue” #300 #300
M1000-M1015 – Graphing Color for Feedrate movement
When a CNC program is graphed (F8 from the Main Screen), feedrate movements are normally plotted using the
color yellow. This color setting can be changed to another color as stated in the chart below.
M Code
Feedrate Graphing Color
M1000
black
M1001
Navy blue
M1002
green
M1003
teal
M1004
orange
M1005
blue
M1006
lime
M1007
aqua
M1008
maroon
M1009
purple
M1010
olive
M1011
gray
M1012
red
M1013
fuschia
M1014
yellow
M1015
white
Changing this feedrate graphing color can be used as a method highlighting or hiding parts of a graphed CNC
program, but will not affect the normal run of the program (when the CYCLE START button is pressed on the
Main Screen). The limitations to using these M codes are as follows: These M codes cannot be placed on the same
line as another M code, and also the rapid (G0) movement color cannot be changed.
T-Series Operator’s Manual
5/18/11
12-15
12-16
5/18/11
T-Series Operator’s Manual
Chapter 13
CNC Program Example
CNC Program
N010
N015
N020
N025
N030
N035
N040
N045
N050
N055
N060
N065
N070
N075
N080
N085
N090
N095
N100
N105
N110
N115
N120
N125
N130
N135
N140
G20
G50 S3000
G00 T0303
G97 S1777 M03
G00 X1.72 Z0.
G96 S800
X1.72
G99 G01 Z-1.955 F.01
X1.7901
X2.02 Z-2.0699
Z-2.215
X2.04
G00 Z0.
X1.42
G01 Z-1.955
X1.74
G00 Z0.
X1.12
G01 Z-1.955
X1.44
G00 Z0.
X.82
G01 Z-1.955
X1.14
G00 Z0.
X.52
G01 Z-1.955
T-Series Operator’s Manual
N145
N150
N155
N160
N165
N170
N175
N180
N185
N190
N195
N200
N205
N210
N215
N220
N225
N230
N235
N240
N245
N250
N255
N260
N265
N270
N275
5/18/11
X.84
G00 Z0.
X.52
G01 Z-1.955
X.54
G00 X2.1
G97 S3000
Z0.
X.5
G96 S1000
G01 Z-1.965 F.003
X1.7818
X2. Z-2.0741
Z-2.215
G28 T0300
M05
M00
G50 S3000
G00 T0404
G97 S1135 M03
G00 X2.02 Z-2.228
G96 S600
X2.02
G99 G01 X1.1932
G00 X2.02
Z-2.2392
G01 X1.2005
13-1
N280
N285
N290
N295
N300
N305
N310
N315
N320
N325
N330
N335
N340
N345
N350
N355
N360
N365
N370
N375
N380
N385
N390
N395
N400
N405
N410
N415
N420
N425
N430
N435
N440
N445
N450
N455
N460
N465
N470
N475
G00 X2.02
Z-2.2503
G01 X1.2078
G00 X2.02
Z-2.2615
G01 X1.2151
G00 X2.02
Z-2.2727
G01 X1.2224
G00 X2.02
Z-2.2838
G01 X1.2297
G00 X2.02
Z-2.295
G01 X1.237
G00 X2.02
Z-2.3062
G01 X1.2444
G00 X2.02
Z-2.3173
G01 X1.2517
G00 X2.02
Z-2.3285
G01 X1.259
G00 X2.02
Z-2.3396
G01 X1.2663
G00 X2.02
Z-2.3508
G01 X1.2736
G00 X2.02
Z-2.362
G01 X1.2809
G00 X2.02
Z-2.3731
G01 X1.2882
G00 X2.02
Z-2.3843
G01 X1.2956
G00 X2.02
13-2
N480
N485
N490
N495
N500
N505
N510
N515
N520
N525
N530
N535
N540
N545
N550
N555
N560
N565
N570
N575
N580
N585
N590
N595
N600
N605
N610
N615
N620
N625
N630
N635
N640
N645
N650
N655
N660
N665
N670
5/18/11
Z-2.3955
G01 X1.3029
G00 X2.02
Z-2.4066
G01 X1.3102
G00 X2.02
Z-2.4178
G01 X1.3175
G00 X2.02
Z-2.429
G01 X1.3248
G00 X2.02
Z-2.4401
G01 X1.3321
G00 X2.02
Z-2.4513
G01 X1.3394
G00 X2.02
Z-2.4625
G01 X1.3468
G00 X2.02
Z-2.4736
G01 X1.3541
G00 X2.02
Z-2.4848
G01 X1.3614
G00 X2.02
Z-2.496
G01 X1.3687
G00 X2.02
G97 S1910
Z-2.218
X2
G96 S1000
G01 X1.1656
X1.3497 Z-2.4991
G28 T0400
M05
M30
T-Series Operator’s Manual
Chapter 14
Configuration
(F3 from Setup)
General
The configuration option provides you with a means for modifying the machine and control configuration. The
majority of information in this section should not be changed without contacting your dealer.
WARNING
Some of the data, if corrupt or incorrect, could cause personal injury or machine
damage.
Password
When you press F3-Config from the Setup Menu, you may be prompted to enter a password. This level of security is
necessary so that users do not accidentally change vital parameters. The original default password is distributed in the
documentation provided to the owner of the machine when the control is installed. This password is changeable via
parameter 42.
If you know the password, type it and press ENTER. If the password you enter is incorrect, a message will appear
telling you the password was incorrect and the password prompt will reappear. Pressing ESC will remove the prompt.
If you don't know the password, simply press ENTER. You will be given access to the configuration options so that
you can view the information. However, you will not be able to change any of the data.
T Series Operators Manual
5/18/2011
14-1
Control Configuration
Pressing F1-Contrl from the configuration menu will display the Control Configuration menu in the edit window. The
Control Configuration menu provides you with a method of changing control dependent data. Each of the fields is
discussed in detail below.
If you wish to change a field, use the up and down arrow keys to move the cursor to the desired field. Type the new
value and press ENTER, or press SPACE to toggle. When you are done editing, press F10-Save to save any changes
you have made. If you wish to discard your changes and restore the previous values, press ESC.
DRO Display Units
This field controls the units of measure the DRO displays. The two options are ' Millimeters ' and ' Inches '. When this
field is highlighted by the cursor, "Press SPACE to change" appears at the bottom of the menu. This message is
explaining that pressing the SPACE key will toggle the value of this field between the two options.
The DRO display units do not have to be the same as the machine units of measure (explained below). This field is
provided for users of the G20 & G21 codes so that they may view the tool position in terms of job units (see Chapter
11).
Machine Units of Measure
This field controls which units of measure the machine uses for each job. The two options are ' Millimeters ' and
'Inches'. Press SPACE to toggle the field between the two options.
This field determines the default interpretation of job dimensions and feedrates. If ' Inches ' is selected, all feedrates
and dimensions will be interpreted as inches as well as any unit dependent parameters.
● NOTE: This field should rarely, if ever, be changed. If you wish to run a job in units other than the default machine
units, use the G20 & G21 codes.
T Series Operators Manual
5/18/2011
14-2
Maximum Spindle Speed (High Range)
This field sets the high range maximum spindle speed. All spindle speeds entered in a CNC program are output as
percentages of this maximum value. If your machine is equipped with a multi-range drive, the control will not exceed
the spindle speed set by this field while in high gear. See the Machine Parameters section for information on setting
the gear ratios for medium and low gear ranges. If your machine is not equipped with a multi-range drive, this field
determines the maximum spindle speed.
Minimum Spindle Speed (High Range)
This parameter is used to adjust the minimum spindle speed for the high range. This parameter allows the operator to
set the minimum value for spindle speed to a value other than 0. All changes in spindle speed are made in relationship
to this value, with this parameter as the minimum value. The values stored can range from 0 to 500000.0 RPM.
Machine Home at Power-up
This field controls how the machine will home at power-up. Set Machine Home at Power-up to Limit Switch if you
are homing off of switches or safe hard stops for all axes, and wish to use the switches or stops for homing. Set
Machine Home at Power-up to Ref Mark-HS if you are homing any axis to a fixed reference mark. In Ref Mark
homing, axes that contain a zero (0) for the plus or minus home switch in the Machine Configuration designate that
axis to have a Ref Mark home, while non-zero values specify Limit Switch homing. Set Machine Home at Power-up
to Jog if you need to manually move or jog the machine to its home position. See Chapter 1 for more information
about machine home.
PLC Type
This field tells the controller which PLC type is installed. This field is currently not used, and is for future expansion
to different PLC types. The best setting for this field is “Normal” for now.
Jog Panel Required
This field tells the controller whether a Jog Panel must be installed in order to run jobs. Also if set to “Yes” the control
requires you to press cycle start twice to start a program but if it’s set to “No” programs will start with one press of
CYCLE START.
Screen Blank Delay
This field determines the delay used for the screen blank function. Entering a non-zero value will specify the number
of minutes of idle time until the screen will go blank. The blanking function only works if no jobs are running. For
example, a value of 5 would blank the screen in 5 minutes if no actions were taken. When the screen is blank, pressing
any key will restore the screen. A value of zero will disable the blank function altogether.
Remote Drive & Directory
This field sets up the remapped default drive and directory for the F3-Remote key in the Load Job screen. This allows
you to conveniently load files from an attached computer via network (RJ-45 Ethernet) connection. The network drive
must be mapped in cnc.net.
User-Specified Paths
Operators can specify paths for INTERCON files and posted INTERCON files. These paths are specified in pathl.ini.
This file is automatically generated by CNC11 if it does not exist. The default pathl.ini file is:
INTERCON_PATH=c:\icn_lath\
ICN_POST_PATH=c:\cnct\ncfiles\
Path tag
INTERCON_PATH
ICN_POST_PATH
T Series Operators Manual
Purpose of path
Main directory containing *.lth files
Directory INTERCON places *.cnc files created when posting *.lth files.
5/18/2011
14-3
Machine Configuration
Pressing F2-Machine from the configuration menu will bring up the machine configuration menu, which provides you
with a method of changing machine dependent data.
If you wish to change a field, press F1-Jog or F2-Motor to select the Jog or Motor fields, use the arrow keys to move
the cursor and select the desired field. Type the new value and press ENTER or press SPACE to toggle. When you
are done editing, press F10-Save to save any changes you have made. If you wish to discard your changes and restore
the previous values, press ESC. Pressing ESC again will return you to the previous menu (Setup).
● NOTE: Although X appears on the first line of the DRO and Z appears on the second, their order is reversed on all
configuration menus. X is axis 2, and Z is axis 1.
● NOTE: Some of these values are set automatically by the Autotune option (See PID Configuration later in this
chapter).
F1 - Jog Parameters
This screen contains jog and feedrate information. See the figure below.
A description of each of these parameters is listed below.
● NOTE: Some of these values are set automatically by the Autotune option (See PID Configuration later in this
chapter).
Slow Jog: Determines the speed of motion on an axis when slow jog is selected and a jog button is pressed. The
slow jog rate cannot be set to a value greater than the maximum rate.
Fast Jog: Determines the speed of motion on an axis when fast jog is selected and a jog button is pressed. The fast
jog rate cannot be set to a value greater than the maximum rate.
Max Rate: Determines the maximum feedrate of each individual axis. The feedrate on each axis can never exceed
Max Rate, even if the feedrate override knob on the front panel is turned up above 100%. (See also the Machine
Parameters section for the "Multi-Axis Max Feedrate" parameter that limits the feedrate along move vectors, not
just each individual axis.)
T Series Operators Manual
5/18/2011
14-4
● NOTE: The maximum rate may be set to a smaller value if you wish to run your machine at a slower rate.
Deadstart: Determines the speed to which an axis decelerates before stopping or reversing direction. A low setting
will cause a large slowdown before reversals of direction, causing your machine to be more accurate. A high
setting will cause less slowdown before reversals, but this may cause your machine to "bang" and you may lose
accuracy. This parameter should not be changed.
Delta Vmax: The maximum instantaneous velocity change that will be commanded on a vector transition. This
parameter should not be changed.
Travel (-): The maximum distance the axis can travel in the minus direction from the home position. Set this
parameter to create a software limit that stops the axis before the fixture or tool collides with the machine.
Travel (+): The maximum distance the axis can travel in the plus direction from the home position. This parameter
is especially useful when using a part or fixture larger than the lathe bed. Set this parameter to create a software
limit that stops the axis before the fixture or tool collides with the machine.
F2 - Motor Parameters
This screen contains information about the motors, ballscrews, and switches installed on your machine.
WARNING
The Motor Parameters should not be changed without contacting
your dealer. Corrupt or incorrect values could cause damage to the
machine, personal injury, or both.
Special function indicators: These appear, if present, between the axis number and the label. ‘s’ – axis is the
spindle, ‘p$’ – axis is paired with axis ‘$’, ‘*’ – pairing conflict. See Machine Parameters for more information on
setting up special functions.
Label: The letter you want to use to identify the axis. The first two axes should always be Z and X. The unused
entries should be labeled N.
● NOTE: Although the 3rd through 8th axes are available in the lathe software, they may be used for special tool
changer and C axis applications. For C axis applications, the label must be set to C and the corresponding motor
parameter (93 or 94) must have the C axis bit on.
T Series Operators Manual
5/18/2011
14-5
Motor revs/inch OR Millimeters / motor rev: The number of revolutions of the motor that results in one inch of
movement (if the machine is set up in inches). OR the number of millimeters that the machine will move as a result
of one turn of the motor (if the machine is set up in millimeters).
Encoder counts/rev: The counts per revolution of the encoders on your servo motors.
Lash compensation: The uniform amount of backlash compensation to be applied along the whole length of the
axis. Backlash can be observed during axis direction reversals and is a normal occurrence due to looseness or wear
of moving parts in a machine. This parameter added to and works in conjunction with Screw Compensation (see
below). Consult your machine manual or T-Series Service Manual for instructions on measuring backlash.
● NOTE: It is required that the machine be rehomed after changing Lash Compensation.
Limits: The PLC input numbers corresponding to any limit switches that you may have on your machine. Your
installer should provide this information. If no limit switch is installed, this field should be set to 0.
Homes: The PLC input numbers of any Home Switches you may have. These are similar to the limit switches. If
your machine does not have home switches, this field should be set to the Limit Switch value. If no home or limit
switch is installed, this field should be set to 0. You may then use hard stops as homing points if you choose.
● NOTE: The Home Switch should never be physically located beyond the Limit Switch.
Direction reversed: Used to match the +/- reference of your machine to the control electronics. Toggle this value if
you actually move in the Z direction (reverse) when you jog Z+.
Screw Compensation: This value indicates whether mapping ballscrew compensation is enabled. Screw
Compensation is similar to Lash Compensation (see above), but has differing compensations depending on the
mapped locations along the axis. Screw Compensation is added to and works in conjunction with Lash
Compensation. For more information, contact your dealer. It is recommended that you enable ballscrew error
compensation at all times.
● NOTE: It is recommended that a rehoming of the machine be done after changing Screw Compensation.
F3 - Find Home
Press F3-Find Home to move an axis to its plus or minus home switch.
F4 - Set Home
Press F4-Set Home to set Machine Home for an axis at its current position. This is usually performed after Find
Home. This operation should not be used to set the part zero position. To set the part zero position, use the Part
Setup menu as described in Chapter 5.
F5 – M Comp
This menu lets you edit the ballscrew compensation tables.
NOTICE
The ballscrew compensation tables should not be changed without contacting your dealer.
Corrupt or incorrect values could adversely affect the accuracy of the positioning of your
machine.
T Series Operators Manual
5/18/2011
14-6
F7 – Scales
This menu lets you set up scale encoders for the purpose of applying scale encoder correction to one or more axes.
NOTICE
The Scale Settings should not be changed without contacting your dealer. Corrupt or
incorrect values could adversely affect the accuracy of the positioning of your machine.
Axis and Label are for informational purposes to indicate on which axis the scales will be applied. These values
cannot be modified on this screen.
Input is the scale encoder number based on the map shown on parameters 308-315. Numbers 1-6 are on the MPU11
and 7-14 are on Optic4 drives. If spare headers are available on the Optic4, they can be used for scale feedback.
Enabled Y enables the scale and N disables the scale.
Scale Counts/Unit is the number of counts of the scale per unit of measurement. This value should come directly
from the scale data sheet and should be entered in the control units. If the control is in inches, then the value should
be entered in inches.
Ratio is calculated as [(Motor Encoder Counts per Rev. * Motor Rev. per Unit) / Scale Counts per Unit] and cannot
be modified. It shows how close the counts/unit are between the motor encoder and scale encoder.
Deadband is the number of encoder counts away from the commanded position that the scale position can be before
compensating. Typically an integer multiple from 1 to 3 times the Ratio should be used.
Velocity is the number of motor encoder counts / interrupt at which the Scales should adjust the position. Typically
a value of 0.5 is a good starting value. To figure out a value to use based on a units/min. speed you need to convert
it. The equation is [units/min. * Motor Encoder Counts per Rev. * Rev. per unit * (1min/60 sec.) * (1sec./4000
int)].
Due to the nature of scale feedback it is inherently an oscillator and by adjusting the Deadband and Velocity that
oscillation can be kept to a minimum.
T Series Operators Manual
5/18/2011
14-7
Scale Indicator Changing the Input, Enabled, or Scale Counts/Unit fields will cause scale compensation to be
temporarily disabled. Scale compensation is also temporarily disabled during homing moves. Even though the
scale is enabled in the menu, scale compensation will be disabled until the axis is rehomed. When a scale is
configured for an axis, a scale indicator appears below the axis label on the DRO. It will have a green background
when the scale is enabled and a red background when the scale is disabled.
Machine Parameters
(F3 – Parms from Configuration)
This screen provides you with a method of changing various parameters that are used by the control. Altogether,
you have access to 500 parameters spread across 5 tables. Each table gives you access to 100 parameters at a time.
You can navigate between tables using the following keys: F7-Previous Table and F8-Next Table. The title at
the top tells you which table you are on. If you wish to change a field in the table, use the arrow keys to move the
cursor and select the desired field. A short description of the parameter will appear below the table. Type the new
value and press ENTER. When you are done editing the fields, press F10-Save to accept any changes you have
made and save them. Note that F10-Save is a single operation that will save all changes in every table that you
modified. Pressing ESC will discard all changes in every table that you modified and will return to the previous
menu [Setup].
● NOTE: Many machine parameters can also be set with the G10 G-code.
T Series Operators Manual
5/18/2011
14-8
Bit-mapped parameters
Certain control parameters are defined by bit-mapped values. In order to change these parameters you must understand
how bit mapping works. A bit-mapped parameter is stored as a number, representing a 16-bit value in the control. If a
certain bit needs to be turned on, that bit’s binary value must be added to the parameter value, if the bit needs turned
off, its binary value must be subtracted from the parameter value. The values for each of the 16 bits can be seen in the
table below.
Bit-Mapped Parameter Bits
15
14
13
12
11
10
9
8
7
6
5
4
3
2
1
0
Bit
Value 32768 16384 8192 4096 2048 1024
512
256
128
64
32
16
8
4
2
1
1
X
X
ON
X
0
X
ON
ON
X
To set bit-mapped parameters simply add together the bit values that you need to have enabled.
Examples:
Parameter
value
0
1
11 < 8+2+1
24 < 16+8
15
X
X
X
X
14
X
X
X
X
13
X
X
X
X
12
X
X
X
X
11
X
X
X
X
10
X
X
X
X
Bit number and settings
9
8
7
6
X
X
X
X
X
X
X
X
X
X
X
X
X
X
X
X
The following table shows the parameters that are currently defined:
Parameter Definition
0
E-Stop PLC Bit
1
Orientation of Jog keys and Graphics
2
G-Code Interpretation Control
3
Modal Tool and Length Offset Control
4
Remote File Loading Flag & Advanced File Ops
5
Suppress Machine Home Setup
6
Auto Tool Changer installed
7
Display colors
8
Available coolant system(s)
9
Display language
10
Macro M function control
11
Probe PLC Input
16
Probing Search Distance
19
MPG mode
20
Ambient temperature
21-24
Motor heating coefficients for axes 1,2,3,4
25-28
Motor cooling coefficients for axes 1,2,3,4
29
Warning temperature
30
Limit temperature
33
Spindle Motor Gear Ratio
34
Spindle Encoder Counts/Rev
35
Spindle Encoder Axis Number
36
Rigid Tapping Enable/Disable
37
Spindle Deceleration Time
38
Multi-Axis Max Feedrate
39
Feedrate Override Knob Limit
40
Basic Jog Increment
42
Password for Configuration Menus
43
G71/72 Depth of Cut
T Series Operators Manual
5/18/2011
5
X
X
X
X
4
X
X
X
ON
3
X
X
ON
ON
2
X
X
X
X
Default
0
0
0
0
0
0
0
0
2
0
0
0
10
0
72
Refer to text
Refer to text
150
180
1
8,000
4
0
10
0
200
0
0
0.01
14-9
Parameter
44
45
46
47
49
50
51
52
53
55
56
61
62
63
64
65-67
68
69
70
72
73
74
78
80
82
83
84
85
86
87-90
91-94
95-98
99
100
101
102
104
105
106
107
108
109
110
111
112
114
115
116
132-135
140
141
T Series Operators Manual
Definition
G71/72 Escape Amount
G74 X Axis Relief Amount
G75 Z Axis Relief Amount
G73 Repeat Count
Thread Chamfer Amount
G76 Finish Count
G76 Thread Angle
G76 Minimum Cutting Depth
G76 Finish Allowance
Radius Programming
Feedrate Override Display Properties
High Power Stall Timeout
High Power Stall PID Limit
High Power Idle PID Multiplier
4th/5th Axis Pairing
Spindle Gear Ratios
Minimum rigid tapping spindle speed
Duration for minimum spindle speed
Offset Library Inc/Decrement Amount
Data Recording M-Function Options
Peck Cutting Retract Amount
M-Function executed at tap hole depth
Display of spindle speed
Voltage Brake Applied Message Frequency
Spindle drift adjustment
Deep Hole Clearance Amount
M-Function executed at return to initial point of tapping cycle
“Door Open” Interlock PLC bit
Rapid/Linear vector rate limit
Autotune Ka Performance parameters for axes 1,2,3,4
Axis Properties for axes 1,2,3,4
Autotune Move Distance for axes 1,2,3,4
Cutter Diameter Compensation Look-ahead
Intercon comment generation
Intercon clearance amount
Intercon spindle coolant delay
Intercon modal line parameters
Intercon modal arc parameters
Intercon modal drilling cycle parameters
Intercon chamfer blend radius
Intercon polar display
Intercon modal display
MPU11 Velocity Blending
Intercon no spindle stop during tool change
Intercon no coolant stop during tool change
Intercon use G28 during tool change
Intercon help
Intercon G50 max spindle speed
Motor Heating Coefficients for axes 5,6,7,8
Message log priority level
Maximum message log lines
5/18/2011
Default
0
0
0
1
0
1
0
0.001
0.01
0
0
0
0
1.5
0
1
0
1.0
.001"/.02mm
0
0.05
4
0
0
0.0
0.05
3
0
0
48
0
2
2
0
0.1
3.0
0
0
0
0.01
0
0
0
0
0
0
0
0
Refer to text
1
1000
14-10
Parameter
142
143
144
145
146
147
Definition
Message log trim amount
DRO properties (load meters, 4/5 digits, DTG)
Comparison rounding
Advanced macro options (fast branching)
Feed hold threshold for feed rate override
Number of Status Messages to keep in Operator Message
Window
148
Miscellaneous Jogging Options
149
Spindle Speed/Surface Footage Threshold
150
Backplot Graphics display options
155
DSP Probe Installed
156-159
Autotune Move Distance for axes 5,6,7,8
163
Gang tooling
165
Acceleration/Deceleration Options
166-169
Axis Properties for axes 5,6,7,8
170-177
PLC parameters
178
PLC I/O configuration (PLC program specific)
179
Lube Pump Operation
180
File Transfer COM Port
181
File Transfer Baud Rate
182
File Transfer Data, Parity and Stop bit settings
183
File Transfer Flow Control Setting
184
File Transfer COM timeout
185
File Transfer Serial Port Option
187
Hard Stop Homing Power Limit
188-199
Aux key functions
200-207
OPTIC4 Tach Volts Per RPM
208-215
MPU Lash/Screw Comp Acceleration Coefficient
216
PC Based Lash Compensation on/off
217
PC Based Screw Compensation on/off
220-231
Smoothing Configuration of Feed Per Minute moves
236-239
Motor Cooling Coefficients for axes 5,6,7,8
252-255
Autotune Ka Performance parameters for axes 5,6,7,8
256
Autotune Enable / Disable
300-307
Drive assignment to Axes 1-8
308-315
Encoder assignment to Axes 1-8
316-323
Axis slaving parameter **Future feature, do not modify
324-331
Axis Boxcar size **Future feature, do not modify
332-335
Encoder error suppression
336-339
Motor torque estimation for velocity mode drives
340-347
Axis Boxcar ErrorSum range **Future feature, do not modify
348,351,354 MPG Encoder Input 1, 2, 3
349,352,355 MPG Detents per Revolution 1, 2, 3
350,353,356 MPG Encoder Counts per Revolution
357-364
Axis Drive Max RPM
399
AD1 arc chord tolerance adjustment
900-999
PLC program parameters
T Series Operators Manual
5/18/2011
Default
1000
0
0
0
0
10
0
0
0
2
0
0
0
0
0
0
0
19.2
801
0
10
0
0
0
0
0.125
0
0
Refer to text
0
0
0
Refer to text
Refer to text
0
0
0
Refer to text
0
15, 0, 0
100
400
0
.5
--
14-11
Parameter 0 – E-Stop PLC Bit
This parameter specifies the PLC bit to which the physical Emergency Stop switch is connected. It is mainly used for
ATC applications that use custom PLC messages.
PLC Type
RTK3
PLCIO2
DC3IO
Servo3IO
ESTOP Input on PLC
Input 11
Input 11
Input 11
Input 1
Parameter Value
11
11
11
1
Parameter 1 – Orientation of Jog Keys and Graphics
This parameter controls the orientation of the jog keys and graphics. The default value is 0. When the default value is
active, all graphical displays will depict Lathe Tooling mounted from the back.
Bit
0
1
2
3
Function Description
Flip X-axis on graphics displays?
Flip movement directions of X jog keys?
Exchange X axis and Z-axis jog keys?
Exchange X axis and Z axis on graphics displays?
Parameter Value
Yes = 1, No = 0
Yes = 2, No = 0
Yes = 4, No = 0
Yes = 8, No = 0
Parameter 2 – Dwell G-code Interpretation Control
This parameter is a bit field that controls optional interpretation of several G-codes. The following table shows the
functions performed by the value entered in this parameter: Currently, only bit 2 is relevant for lathe operations, and
all the other bits should be set to value = 0..
Bit
0
1
2
Function Description
(Not used for Lathe)
(Not used for Lathe)
Interpret dwell time (P) associated with G4 as milliseconds rather than
seconds
3 See M-series (Mill) manual for reference.
4 (Not used for Lathe)
5 See M-series (Mill) manual for reference.
Parameter 3 - Modal Tool and Length Offset Control
Bit Meaning
0 Tool and Length Offset numbers will be reset upon job completion
(and not remain modal and active between jobs).
1 Unused for Lathe. This bit should be set to 0.
2 Tool Length Offset Retention option. This option prevents the
current tool length offsets from being turned off when the user
enters the Tool Length Offset menu.
T Series Operators Manual
5/18/2011
Parameter Value
Set to 0
Set to 0
Yes = 4, No = 0
Recommended setting = 0
Set to 0
Recommended setting = 0
Parameter Value
Reset upon job completion = 1,
Remain modal between jobs = 0
Should always be = 0
Yes = 4, No = 0
14-12
Parameter 4 - Remote File Loading Flag & Advanced File Ops
This parameter controls the action of the Load Job Screen when CNC job files are selected from drive letters higher
than C. These drives (i.e. drives D, E, F, etc.) are presumed to be network drives or extra hard drives.
Value
0
1
Meaning
Job files are not copied or cached. They are run from whichever drives they reside on.
Job files are copied to the C drive (c:\cnct\ncfiles) when they are loaded. The local copy is used
when the job runs.
Turn on file caching. Job files are temporarily cached on the C drive. The cached copy is used
while the job is running. The cached copy is deleted when the next job is loaded or when
Parameter 4 changes to a 0 or 1.
Set the Advanced File load menu as default for loading files
2
4
File caching is useful for machines with both a flash card and a hard drive. By caching job files from the hard drive
on the flash card, the hard drive is not used while the job is running. As a result, the life of the hard drive is
extended and the flash card does not fill up with job files.
Parameter 5 - Suppress Machine Home Setup
This parameter controls machine homing upon startup of the control. The following table details the functions
controlled by this parameter:
Bit
0
1
2
Function Description
Suppress the requirement to set machine home before running jobs?
(Unused)
Disable stall detection when CNC11 first starts.
Parameter Value
Yes = 1, No = 0
---Yes = 4, No = 0
Bit 0 suppresses the requirement to set machine home before running. If bit 0 of parameter 5 is 0, machine home
must be set before jobs may be run. If bit 0 of parameter 5 is 1, machine home is not requested or required.
● NOTE: Parameter 5 Bit 0 is separate from the "Machine Home at Powerup" flag in the Control Configuration
Menu. Parameter 5 Bit 0 determines whether you must home the machine; the "Machine Home at Powerup" flag
determines how you will home the machine, if you must do so.
Parameter 6 - Automatic tool changer
This parameter tells the control whether you have an automatic tool changer installed on your machine. This field
affects the action of the T codes in your CNC programs. It also affects whether the ATC key is present in the Tool
Offset Setup.
Value Meaning
0
Auto Tool Changer NOT Installed
1
Auto Tool Changer Installed
Parameter 7 - Display colors
This parameter determines what combination of colors will be used for display. If you have a color display, set this
parameter to 0. If you have a monochrome display (especially a monochrome LCD panel) set this parameter to 1.
Parameter 8 - Installed coolant systems
This parameter is used by Intercon to determine what coolant systems are available on the machine. It should be set as
follows:
Value Meaning
1 Mist Coolant (M7) only
2 Both coolant systems
3 Flood Coolant (M8) only
T Series Operators Manual
5/18/2011
14-13
Parameter 9 - Display language
This parameter determines what language will be used for menus, prompts and error messages.
Value Meaning
0
English
1
Spanish
2
French
3
Traditional Chinese
4
Simplified Chinese
5
German
6
Swedish
7
Finnish
8
Portuguese
Parameter 10 - Macro M-function handling
This parameter is a 4-bit field that controls various aspects of M functions. The following table shows the functions
performed by the value entered in this parameter. The default value is 0.
Bit Function Description
Parameter Value
0 Display M & G codes in M function macros?
Yes = 1, No = 0
1 Step through M function macros in Block Mode?
Yes = 2, No = 0
2 Decelerate to stop on M105 and M106. With decel.set these moves take
Decel = 4,
longer and are slightly less accurate. With immediate stop these moves are Immediate Stop = 0
faster and more accurate; however the lack of controlled deceleration can
cause excessive machine vibration.
3 (not used on lathe)
set to 0
4 Decelerate to stop on M115,M116,M125,M126 probing moves. With
Decel = 16,
decel.set these moves take longer and are slightly less accurate. With
Immediate Stop = 0
immediate stop these moves are faster and more accurate; however the lack
of controlled deceleration can cause excessive machine vibration.
Parameter 11 – Probe PLC Input Number and Contact State
This parameter is used for the PLC input number that is used by the probe device on M115/M116/M125/M126
probing moves. Allowable range is a single value, +/- 1 to 240 and 50001 to 51312. A Positive number indicates
Closed on contact and a negative number indicates Open on contact.
NOTICE
Changing this parameter can cause damage to your probe device. You should contact your
Dealer or Local Tech Representative before any modifications are made.
Parameter 16 – Maximum Probing Distance
This is the maximum distance that the M115/M116/M125/M126 probing moves “search” for a surface in a given
direction if no travel limits have been entered. The default setting is 10 inches.
Parameter 19 - MPG modes
The MPG is a hand-held device that is used as an alternate way of jogging the machine. This parameter defines the
MPG’s mode of operation.
Bit
0
2
Function Description
Parameter Value
Ignore MPG encoder error
Yes = 1, No = 0
Enable Z axis MPG* -- This will allow the z- Yes = 4, No = 0
axis to be moved with the MPG while
running a job independent of the x and y axes
*PLC program interaction is needed for these features. The plc program is in direct control of MPG modes. Z-axis
MPG operation is not available with all controls.
T Series Operators Manual
5/18/2011
14-14
Parameters 20-30 (also 132-135, 236-239) - Motor Temperature Estimation
These parameters are used for motor temperature estimation. Parameters 20, 29 and 30 correspond respectively to
the ambient temperature of the shop, the overheating warning temperature, and the job cancellation temperature, all
in degrees Fahrenheit. Parameters 21-24 and 132-135 are the heating coefficients. Parameters 25-28 and 236-239
are the cooling coefficients.
SD
Drive
Parameters
21-24
132-135
25-28
236-239
20
29
30
Axes
1-4
5-8
1-4
5-8
N/A
N/A
N/A
Servo
Drive
Parameters
21-24
132-135
25-28
236-239
20
29
30
Suggested values for AC Brushless Motors and Drives
SD3, SD1 SD3, SD1
SD3, SD1
SD1 45A
SD1 45A
750 W
1,2 KW (finned heatsink) (finned heatsink) (finned heatsink)
motors
motors
1,2 KW motors
3 KW motors
4 KW motors
Values
Values
Values
Values
Values
0.23
0.5
0.23
0.23
0.23
0.23
0.5
0.23
0.23
0.23
12.0
9.0
12.0
12.0
14.5
12.0
9.0
12.0
12.0
14.5
72
72
72
72
72
150
150
150
150
150
180
180
180
180
180
Suggested values for DC Brush Motors and Drives
9A Drive, 12A Drive, 15A Drive, 15A Drive, 25A Drive,
17 in/lb
29 in/lb
29 in/lb
40 in/lb
40 in/lb
motors
motors
motors
motors
motors
Axes
Values
Values
Values
Values
Values
1-4
0.028
0.02
0.027
0.03
0.04
5-8
0.028
0.02
0.027
0.03
0.04
1-4
0.68
0.68
0.68
0.68
0.68
5-8
0.68
0.68
0.68
0.68
0.68
N/A
72
72
72
72
72
N/A
150
150
150
150
150
N/A
180
180
180
180
180
Parameter 33 - Spindle Motor Gear Ratio
NOTICE
The default value for this parameter is 1 and should not be changed unless you have
consulted your dealer or local Technical representative!!!
Sets the gear or belt ratio between the spindle motor and the chuck in high gear range. Should be greater than 1.0 if the
motor turns faster than the chuck and less than 1.0 if the chuck turns faster than the motor. Note: this value applies to
high range. The ratio between high range and lower ranges is established by the gear ratio parameters (65-67).
Parameter 34 - Spindle Encoder Counts/Rev
This parameter controls the counts/revolution for the spindle encoder. The spindle encoder is required for spindleslaved movements such as Threading, Feed-Per-Revolution moves, and Rigid Tapping, . If the encoder counts up when
running CW (M3), the value of this parameter must be positive. If the encoder counts up when running CCW (M4),
the value of this parameter must be negative.
Parameter 35 - Spindle Encoder Axis Number
Input from a spindle encoder is required for spindle-slaved movements such as Rigid Tapping, Threading, and Feed
per Revolution movement. This parameter specifies the axis number (1 through 8) to which the spindle encoder is
assigned. Encoder assignments are specified by parameters 308-315. For example, if you decide to configure the 5th
axis as the spindle, and the spindle’s encoder is the 1st MPU11 onboard input encoder, then Parameter 35 (this
parameter) should be set to 5, and Parameter 312 should be set to 1.
T Series Operators Manual
5/18/2011
14-15
Parameter 36 - Rigid Tapping Enable/Disable
This parameter is a bit field that enables or disables Rigid Tapping and its options.
Bit Function Description
0 Enable Rigid Tapping?
1 Suppress sending "Wait for Index Pulse" during Rigid
Tapping?
2 Allow Spindle Override during Rigid Tapping?
3 Use Spindle Off system variable bit?
(see note below)
Parameter Value
Yes = 1, No = 0
Yes = 2, No = 0
Yes = 4, No = 0
Yes = 8, No = 0
(see note below)
Note on Bit 3: This bit enables the spindle off system variable, for mpu11 systems. Most systems will not need to set
this bit. Mpu11 systems will not execute custom M5 macro commands during a rigid tap. Instead the software
determines which bit, M3 or M4, to turn off to stop the spindle. Alternatively, setting bit 3 will cause the software to
set the spindle off system variable bit, SV_PC_RIGID_TAP_SPINDLE_OFF. The plc program is then responsible for
monitoring that bit and performing all actions in order to turn off the spindle.
Parameter 37 - Spindle Deceleration Time
This parameter is used in conjunction with parameter 36 when rigid tapping is enabled. This sets the amount of time
required for the spindle to decelerate before it switches direction during a rigid tapping operation.
Parameter 38 - Multi-Axis Max Feedrate
This parameter is used to limit the feedrate along all feed-per-minute move vectors. This parameter can be used to
limit the speed of multi-axis moves on machines that may have enough power to move a single axis rapidly, but starve
out of power on 2 or 3 axis rapid moves. A zero in this parameter will disable this feature. Note that this feature has no
effect for movement commands handled by Smoothing (P220=1).
Parameter 39 - Feedrate Override Percentage Limit
This parameter is used for limiting the upper end of the Feedrate Override Knob percentage to a value from 100% to
200%. This parameter can be used to restrict the Feedrate Override Knob effect on machines with maximum rates
over 200 in/min. The Feedrate Override Knob percentage is normally allowed to go to 200%. However, on machines
with high cutting speeds, if the knob is turned up to 200%, it creates overshoots on corners. If this parameter for
example is set at 110, it will stop the Feedrate Override Knob from exceeding 110%, and thus cause the overshoots to
disappear.
Parameter 40 - Basic Jog Increment
This parameter holds the basic jog increment (0.0001" or 0.002mm by default). This value is used by the x1, x10 and
x100 jog keys (0.0001, 0.001 and 0.01 on older consoles).
Parameter 42 – Password for Configuration Menus
This parameter determines the password that the user must enter in order to gain supervisor access to the configuration
menus.
Value
Meaning
54.0
No password required for supervisor access; the user is not prompted for a password
ABCD.ABCD Password is 4 digits represented by “ABCD”
Any other number Password is “137”
Parameter 43 - G71/G72 Depth of Cut
The depth of each successive cut along the Z-axis (for G71) or X-axis (for G72). The minimum value is 0.0001"; the
maximum is 9999.9999"; the default is 0.01".
T Series Operators Manual
5/18/2011
14-16
Parameter 44 - G71/G72 Escape Amount
The distance the cutter will move away from the just-cut surface before going back to start the next pass. The
minimum value is 0; the maximum is 9999.9999"; the default is 0.
Parameter 45 - G74 X axis Relief Amount
Distance along the X axis that the cutter will move away from the surface before returning to the starting point at the
end of a pass. The minimum value is 0; the maximum is 9999.9999; the default is 0.
Parameter 46 - G75 Z axis Relief Amount
Distance along the Z axis that the cutter will move away from the surface before returning to the starting point at the
end of a pass. The minimum value is 0; the maximum is 9999.9999; the default is 0.
Parameter 47 - G73 Repeat Count
Number of passes to cut. The minimum value is 1; the maximum is 1000; the default is 1.
Parameter 49 - Thread Chamfer Amount
The length of the chamfer inserted at the end of threads cut with the G92 and G76 cycles, as a multiple of the thread
lead. A value of 1.0 inserts a one-thread chamfer. The minimum value is 0; the maximum is 100; the default is 0. See
Chapter 11 for more information on G92 and G76.
Parameter 50 - G76 Finish Count
Number of finish passes in the G76 cycle. All of the finish allowance is removed with the first finish pass; the
remaining passes are spring passes over the same path. The minimum value is 1; the maximum is 99; the default is 1.
See Chapter 11 for more information on G76.
Parameter 51 - G76 Thread Angle
Compound angle of the thread. The minimum value is 0; the maximum is 120; the default is 0. See Chapter 11 for
more information on G76.
Parameter 52 - G76 Minimum Cutting Depth
In the G76 cycle, each successive pass has a smaller depth increment. This parameter sets the minimum depth
increment. The minimum value is 0.0001"; the maximum is 999.9999"; the default is 0.0010". See Chapter 11 for
more information on G76.
Parameter 53 - G76 Finish Allowance
Finish allowance left after the depth passes, to be removed by the first finish pass. The minimum is 0.0001"; the
maximum is 9999.9999"; the default is 0.0100". See Chapter 11 for more information on G76.
Parameter 55 - Radius Programming
By default, all X-axis positions and X axis tool offsets are diameter values. The actual travel of the machine will be
half the requested distance. If parameter 55 is set to 1, X-axis positions and tool offsets will be interpreted as radius
values. In this case, the actual travel of the machine will be equal to the requested distance.
Parameter 56 – Feedrate Override Display Properties
This parameter is a 3-bit field that is used to define how the federate override is displayed in the status window.
Bit
0
1
2
Function
Not used
Display programmed rate not actual
Display a bar meter of percentage
T Series Operators Manual
5/18/2011
Parameter Value
Yes = 2; No = 0
Yes = 4; No = 0
14-17
Parameters 61-62 - Stall detection parameters
The T-Series control will detect and report several stall conditions. The low power stall occurs if the control has been
applying a specified minimum current for a specified time, and no encoder motion has been detected. This may
indicate a loose or severed encoder cable. A high power stall occurs if the control has been applying at least 90%
current for a specified time, and no motion greater than 0.0005" has been detected. This may indicate a physical
obstruction. Note that this feature will only work with torque mode drives and not velocity mode drives.
Parameter 61 is the time limit, in seconds, for a high power stall. The default is 0.5 seconds.
Parameter 62 is the PID output threshold for a high power stall. The default is 115.
Parameter 63 - High Power Idle PID Multiplier
This parameter holds the value of a constant used for motor temperature estimation when an axis is not moving and no
job is running but there is power going into the motor to maintain its position. The default value is 1.5. This
temperature estimation is intended to detect early if an axis is stopped against some abnormal resistance, such that it
will probably overheat later.
Parameter 64 – Fourth/Fifth Axis Pairing
This feature enables the 4th and 5th axes to be paired together or individually be run in a slaved state with any of the
other axes. This is intended to drive 2 screws on opposite sides of a table or gantry system. Set this parameter to 0
(default) to indicate that no other axis is paired with the 4th or 5th axis. In order to pair both the 4th and 5th axes on the
same system add the 4th axis value with the 5th axis value. Example: 4th axis paired with the Z-axis and 5th axis paired
with the 3rd axis a value of 49 would be entered into parameter 64. The axes are slaved upon power up but it is still
possible to move the paired (4th or 5th) axis independently if the axis is labeled.
* NOTE: You cannot run Autotune on paired axes.
Value Meaning
0
No Pairing (Default)
1
Pair 4th axis with Z Axis
2
Pair 4th axis with X Axis
3
Pair 4th axis with 3rd Axis
16
Pair 5th axis with Z Axis
32
Pair 5th axis with X Axis
48
Pair 5th axis with 3rd Axis
64
Pair 5th axis with 4th Axis
Parameters 65-67 - Spindle gear ratios
These parameters tell the control the gear ratios for a multi-range spindle drive. Up to four speed ranges are supported;
high range is the default. Parameters 65-67 specify the gear ratio for each lower range, relative to high range. For
example, if the machine is a lathe with a dual range spindle, and the spindle in low range turns 1/10 the speed it turns
in high range, then parameter 65 should be set to 0.1. Note that these values can be signed +/-. So, if switching from
high range to a lower range causes the spindle encoder to count in the opposite direction, then a negative value can be
used to compensate for this.
Parameter 65 is the low range gear ratio. The default is 1.
Parameter 66 is the medium-low range gear ratio. The default is 1.
Parameter 67 is the medium-high range gear ratio. The default is 1.
These parameters work in conjunction with the PLC program, which uses the states of INP63 and INP64 to signal to
the CNC software which range is in effect, according to the table below.
PLC INPUT
INP63
INP64
T Series Operators Manual
Spindle Range
High Range Medium High Range
0
1
0
0
5/18/2011
Medium Low Range
1
1
Low Range
0
1
14-18
Parameter 68 – Minimum Spindle Speed (Rigid Tapping Parameter)
This parameter holds the value that the spindle slows down to from the programmed spindle speed towards the end of
the tapping cycle. The lower the value, the more accurately the Z axis will land on target, but at the expense of
possibly stalling the spindle motor which in turn will cause Z to stop short. If this value is too large, the off target error
will increase. The suggested starting value is 640 rpm.
Parameter 69 – Duration for Minimum Spindle Speed Mode (Rigid Tapping Parameter)
This is the duration of time, in seconds, that the control will stay at minimum spindle speed. If the number is too small,
overshoot may occur. If the number is too large, the user waits longer for the hole to be tapped at the slow speed
specified by parameter 68. The suggested starting value is 1.25 seconds.
Parameter 70 - Offset Library Inc/Decrement Amount
Sets the increment and decrement amount used in the offset library.
Parameter 72 – Data M Function Options
The setting of this parameter affects the operation of the data M functions M122 and M123.
Bit
0
1
2
Function Description
Parameter Value
Suppress output of axis labels by M122?
Insert commas between positions/values with M122 and M123?
Suppress spaces between positions/values outputted by M122 and M123?
Yes = 1, No = 0
Yes = 2, No = 0
Yes = 4, No = 0
Parameter 73 - Peck Retract Amount
This parameter sets the peck retract amount associated with G74 and G75. The minimum value is 0; the maximum
value is 9999.9999"; the default value is 0.0500". See Chapter 11 for more information on G74 and G75.
Parameter 74 – M-function executed at tap depth (Canned Cycle Parameter)
This specifies the number of the M-function that is executed at the bottom of the Tap cycle (primarily used for
reversing the spindle in preparation for pulling out of the tap hole). This also specifies the number of the M-function
that is executed after the Counter Tap cycle is done (returned to the initial point). Both Tap and Counter Tap cycles
are performed by G84 (see G84 in Chapter 11).
Parameter 78 – Spindle Speed Display and Operations
Bit 0 specifies how the spindle speed is determined and displayed in the CNC11 status window. When set to 1.0, the
spindle speed is determined by reading the encoder feedback from the axis specified according to parameter 35.
Which has the number of encoder counts/revolution specified in parameter 34. When set to 0.0, the displayed speed is
not measured; the speed is calculated based upon the set speed, spindle override adjustment, and gear range. Bit 1
allows the control to slow the programmed feed rate if the spindle speed slows down. Bit 2 will make the control wait
until spindle at speed is at least the set percentage that is set in parameter 149.
Bit
0
1
2
Function
Display actual spindle speed
Slave feed rate to programmed spindle speed
Wait for spindle at speed
Value
Yes = 1, No = 0
Yes = 2, No = 0
Yes = 4, No = 0
Parameter 79 – Auto Brake Mode PLC Bit for Uniconsole-2
This parameter specifies which PLC bit signals the state of automatic brake mode when using the Uniconsole-2
console type. For other console types, it has no effect. This parameter can be changed to allow the Auto Brake mode
key to be located in different positions on the Uniconsole-2 jog panel.
T Series Operators Manual
5/18/2011
14-19
Parameter 80 – Voltage Brake Message Frequency
This parameter specifies the number of time the “450 Voltage brake applied message has to occur before we show it in
the message window and message log. A value of 0 or 1 will display the message for every instance that it occurs.
Parameter 82 – Spindle Drift Adjustment (Rigid Tapping Parameter)
This value is the number of degrees that the spindle will take to coast to a stop if it is cut off while it is spinning at the
spindle speed specified by parameter 68.
Parameter 83 – Deep Hole clearance amount (Canned Cycle Parameter)
Parameter 83 specifies the clearance amount used during a G83 deep hole drilling cycle.
Parameter 84 – M function executed at return to initial point of tapping cycle (Canned Cycle Parameter)
This specifies the number of the M-function that is executed after the Tap Cycle is done (returned to the initial point).
This also specifies the number of the M-function that is executed at the bottom of the Counter Tap cycle (to reverse the
spindle in preparation for pulling out of the countertap hole). Both Tap and Counter Tap cycles are performed by G84
(see G84 in Chapter 11).
Parameter 85 – “Door Open” Interlock PLC bit
This parameter provides a way for a system integrator to implement a safety interlock that limits rate of movement
when the doors are open. This parameter specifies the PLC bit number and PLC bit polarity that indicates the "door
open” condition. If the specified PLC bit is in the specified “door open” condition, then all rapids and non-Smoothing
feed-per-minute movement will be limited to the slow jog rate (as specified in the Jog Parameters menu in Machine
Configuration). Polarity of the “door open” condition is specified thuswise: a positive number indicates that the “door
open” condition occurs when the specified PLC bit is On, and a negative number indicates that the “door open”
condition occurs when the specified PLC bit is Off. Note that this parameter does not affect the spindle speed, and also
does not affect threading speeds nor feed-per-revolution moves. Furthermore, this feature has no effect on feed-perminute movement handled by Smoothing (P220=1). If this parameter is set to 0 (the default value), then this feature is
disabled, and no checking for a “door open” condition is done, and consequently all movement commands will run at
their normal programmed feedrates.
Parameter 86 – Rapid/Linear vector rate limit
This parameter controls the feature that imposes a limit on the number of rapid and/or feed-per-minute linear moves
allowed each second. If the value of this parameter is more than 0, Rapid and/or Linear moves will be combined to
prevent the aforementioned limit from being exceeded. This parameter is used for testing purposes and should be set
to 0 to disable this feature. Note that this feature has no effect for movement commands handled by Smoothing
(P220=1).
Parameters 87-90 (and also 252-255) - Autotune Ka Performance parameters
These parameters are used by autotune. Increasing the value will increase the Ka used by autotune which when used
will increase the PID used during acceleration. The default value is 0. The maximum value is 50 and the minimum
value is 0. Values for axes 1-4 are specified in parameters 87-90. Values for axes 4-8 are specified in parameters 252255.
T Series Operators Manual
5/18/2011
14-20
Parameters 91-94 (and also 166-169) – Axis Properties
These parameters may be used to set various axis properties. Properties for axes 1-4 are specified in parameters 91-94.
Properties for axes 4-8 are specified in parameters 166-169.
Bit
0
1
2
3
4
5
6
7
8
9
10
Function Description
Rotary/Linear Axis Selection
Rotary Display Mode
NOT USED ON LATHE
Suppress park function?
C Axis Selection
Linear Display of Rotary Axis
NOT USED ON LATHE
For C axis divide counts per rev by 360
NOT USED ON LATHE
Hide axis from DRO display
NOT USED ON LATHE
Parameter Value
Rotary Axis= 1, Linear Axis= 0
Wrap Around = 2, Show Rotations = 0
Recommended bit value is 0
Don’t Park = 8, Park = 0
C Axis = 16, Off = 0
Linear Display = 32, Default Rotary = 0
Recommended bit value is 0
Divide by 360 = 64, No Divide = 0
Recommended bit value is 0
Yes = 512, No = 0
Recommended bit value is 0
Bit 0: Turning this bit on will cause the DRO display for the affected axis to be displayed in degrees. Also this
information is used by Intercon to make rotary axis support available (by setting parameter 94 to 1, indicating that the
fourth axis is rotary). This bit is also used when performing inch/mm conversions: values for a rotary axis will not be
converted since they are assumed to be in degrees regardless of the system of linear units.
Bit 1: This bit has no effect unless Bit 0 (mentioned above) is turned on. When this bit is turned on, a “Wrap Around”
display is shown on the DRO. A “Wrap Around” Rotary Display is a display in degrees without the number of
rotations shown. If this bit is turned off, the number of rotations away from 0 degrees will be shown alongside the
degree display.
Bit 3: Setting this bit prevents <F1> (Park) in the Shutdown menu from parking this axis.
Bit 4: Setting this bit enables C axis control capability. The corresponding label field in the Machine Configuration
should also be set to a “C”.
Bit 5: This setting overrides only the DRO display options for an axis that has bit 0 set (including the Rotary Display
Mode – bit 1) so that the display does not reflect a degree symbol or any indication of the number of rotations, but
appears as a linear axis.
Bit 7: This setting will divide the counts per revolution being sent to the CPU by 360 to provide more precise
positioning for the C axis.
Bit 9: This setting will hide the affected axis from the DRO display. Note that this does not prevent such an axis from
being commanded to move.
Parameters 95-98 (and also 156-159) - Autotune Move Distance
These parameters hold the maximum distance that the control will move each axis in either direction from the starting
point when Autotune is executed. The default value for these parameters is 2.0 inches. Values for axes 1-4 are
specified in parameters 95-98. Values for axes 4-8 are specified in parameters 156-159.
Parameter 99 – Cutter Diameter Compensation Look-ahead
This parameter sets the default number of line or arc events for the G-code interpreter to scan ahead when cutter
diameter compensation (G41 or G42) is active. Values of 1 to 10 are allowed for this parameter.
Parameters 100-109, 111-116 – Intercon parameters
These parameters are some of the Intercon setup parameters. See Chapter 8 for more information about these
parameters. Changing values will change Intercon settings and may affect the output of the G-code program if it is reposted.
Parameter 110 – MPU11 Velocity Blending
This turns on/off the MPU11 feature which smooths the velocity transitions between adjacent vector moves. Note that
this feature has no effect for movement commands handled by Smoothing (P220=1).
T Series Operators Manual
5/18/2011
14-21
Parameters 132-135 – Motor Heating Coefficients for axes 5-8
See parameters 20-30 for more information.
Parameter 140 – Message log priority level
This parameter controls the messages that are written to the message log, which can be accessed through the F9 - Logs
function in the Utilities menu. See Chapter 15 for the list of numbered messages. Message logging can be disabled be
setting this parameter to –1. The recommended log level is 4.
Value Which numbered messages are logged
-1
None
1
Numbered messages 0-299 and 400-499 – The most serious faults.
4
Numbered messages 0-299 and 400 and higher – The most serious faults and medium severity errors.
9
All numbered messages.
Parameter 141 – Maximum message log lines
This parameter is the number of lines that will be kept in the message log. If this parameter is set to 10,000, for
example, the newest 10,000 messages will be retained. CNC11 will delete the oldest messages, trimming the log file
to the given number of lines at startup and periodically while CNC11 is in an idle state. Parameter 142 controls the
frequency of the log cleanup.
Parameter 142 – Message log trim amount
This parameter is the number of additional lines above the minimum that can be added to the log before it is reduced to
the minimum size. Setting this parameter to a lower value will cause the log file to be trimmed to its minimum size
more often. The higher the value, the less often the log will be trimmed. The speed of the disk drive and total size of
the log file at the time it is trimmed will determine how long the log cleanup takes. Under most circumstances, using
10,000 and 1,000 for parameters 141 and 142 will provide a reasonable and useful log size with no noticeable effects
on performance. If parameters 141 and 142 are set to excessively high values, the message "Trimming excess lines
from log file" will be presented. This message will appear at startup and very infrequently when CNC11 is idle.
Normal operation can proceed after the message disappears. If the delay is unacceptable, reduce the values of
parameters 141 and 142.
Parameter 143 – DRO Properties (load meters, 4/5 digits, Distance To Go)
This parameter controls the display of the axis load meters and 4/5 digits DRO precision.
Bit Function Description
Parameter Value
0 Enable Load Meters
Enable = 1, Disable = 0
1 Load Meter Outline
Enable = 2, Disable = 0
2 DRO 4/5 Digit Precision
5 digits = 4, 4 digits = 0
3 Mini DRO (Distance to Go) Enable = 8, Disable = 0
Add the values of the desired properties. For example, use a value of 3 to display load meters with outlines. The value
11 will display load meters, outlines and the mini-DRO. The axis load meters will be colored green for values that are
up to 70% of maximum power output, yellow for values between 70% and 90%, and red for values between 90% and
100%. The axis load meters appear below the DRO for each axis (see Chapter 1).
T Series Operators Manual
5/18/2011
14-22
Parameter 144 – Comparison Rounding
This parameter determines the built in rounding for the comparison operators (‘EQ’, ‘NE’, ‘LT’, ‘GT’, etc.) in
expressions. Rounding of comparison arguments is necessary due to extremely small errors that are part of every
floating-point calculation. The result of such errors is that two floating-point values are rarely exactly equal. The
value of parameter 144 represents the precision of comparison in places after the decimal point. If the parameter is set
to 9.0, for example, then comparison operators will declare two numbers that differ in value by less than 0.0000000005
as being equal. The value 0.0 is a special value that turns comparison rounding off. When comparison rounding is off,
it is up to the G code programmer to build the precision into conditional statements, for example “IF ABS[#A - #B] LT
0.00005 THEN GOTO 100”. When comparison rounding is off, the “EQ” usually returns “false”. If parameter 144 is
set to 9, the programmer can shorten the previous example to “IF #A EQ #B THEN GOTO 100”.
Parameter 145 – Advanced Macro Properties (Fast Branching)
This parameter turns fast branching on (1) and off (0). The other bits of this parameter are reserved for future use.
If fast branching is disabled, CNC11 searches forward in the program for the first matching block number and resumes
searching, if necessary, from the top of the program. For this reason, backward branches take longer than forward
branches and backward branch times depend on the total program size. If the program is sufficiently large, use of the
GOTO statement could introduce temporary pauses.
When fast branching is enabled, CNC11 remembers the locations of block numbers as it finds them during program
execution. Backward branches always take place immediately. The first forward branch to a block not yet
encountered will take additional time as CNC11 searches forward for the block number; however, subsequent forward
branches to that block number will take place immediately. The trade-off for using fast branching is that all line
numbers at a given level of program or subprogram must be unique and programs will use more memory
(approximately 16 kilobytes of memory for every 1000 block numbers in the program.)
Parameter 146 – Feed Hold Threshold for Feed Rate Override
This parameter sets the lowest value permitted as the feed rate override percentage before feed hold is engaged. Feed
hold will be released when the override percentage is greater than this value.
Parameter 147 – Number of Status Messages to keep in Operator Message Window
The Operator Message Window is the box of scrolling status messages that appears in the upper right corner of the
Main Screen. The number of remembered status messages can be adjusted by this parameter.
Parameter 148 – Miscellaneous Jogging Options
This parameter enables and/or disables certain optional modes of jogging.
Parameter Value
Bit Function Description
0 Unused
Should be set to 0
1 Prohibit Keyboard Jogging
Prohibit Keyboard Jogging = 2
Keyboard Jogging allowed = 0
Note: With this parameter set to zero, you need to set parameter 170 to enable keyboard jogging.
Parameter 149 – Spindle Speed/Surface Footage Threshold
This parameter defines the threshold at which linear motion will be permitted. It is specified as a percentage of the
programmed spindle speed. For example a value of 0.8 would inhibit linear motion until 80 percent of the
programmed spindle speed was reached. To enable this parameter a value of 4 must be added to parameter 78.
Parameter 150 – Backplot Graphics display options
This parameter controls the various options related to backplot graphics.
Bit
0
4
Function Description
Sets Run Time Graphics option default to
ON
Display Lash/Screw Compensation
T Series Operators Manual
5/18/2011
Parameter Value
Enable = 1, Disable = 0
Enable = 16, Disable = 0
14-23
Parameter 155 – Probe Device Type
This parameter specifies the type of probe being used.
Value
Meaning
0
Standard Mechanical probe
1
DSP probe
2
DP-7 probe
Parameters 156-159 – Autotune move distances for axes 5-8
See parameters 95 – 98 for more information.
Parameter 163 – Gang Tooling
This parameter enables the tool library to select front mount or back mount tool approach for gang tooling. If set to 1
you can measure both front mount and back mount tooling.
Parameters 165 – Acceleration/Deceleration Options
This is a bit field parameter which modifies certain details of axis acceleration and deceleration when an axis stops
moving, changes direction, or starts moving. The Jog Parameters screen in the Machine Configuration set the original
DeadStart values for each axis. This parameter allows you to modify these DeadStart settings under certain conditions.
Note that if both Bits 0 and 1 are turned on (value = 1+2 = 3), the effect is cumulative, i.e. the net effect will be that ½
DeadStart value will be used when a slave axis stops or starts up from a stop. Likewise, if both Bits 2 and 3 are turned
on, the effect will be cumulative also. Note that this feature has no effect for movement commands handled by
Smoothing (P220=1).
Bit
0
1
2
3
4
Function Description
Use ¼ DeadStart value for a slave axis that stops or starts from a
stop
Use 2 x DeadStart value for a slave axis that stops or starts from a
stop
Use ¼ DeadStart value for a slave axis that reverses
Use 2 x DeadStart value for a slave axis that reverses
Limit the feedrate along the path of G2 or G3 arc moves such that
the feedrate will be uniformly limited to the lesser of the maximum
rate of the 2 axes involved in the circular motion.
Parameter Value
Enable = 1, Disable = 0
Enable = 2, Disable = 0
Enable = 4, Disable = 0
Enable = 8, Disable = 0
Enable = 16, Disable = 0
Parameters 166-169 – Axis Properties for axes 5-8
See parameters 91-94 for more information.
Parameters 170-179 – PLC Parameters
These parameters are especially reserved as a space for data which is to be sent to the PLC. Parameters 177, 178, 179
have been standardized for specific applications. Parameter 177 is used for trouble shooting purposes only.
Parameters 170 – Enable Keyboard Jogging and set Feedrate over ride Control
This PLC parameter is used to enable keyboard jogging and determine whether jog panel or keyboard feedrate over
ride is used. To enable keyboard jogging set parameter 148 to zero and this parameter to a 1.
Bit
0
1
2
Function
Enables Keyboard jogging
Only looks at Feedrate over ride from Jog
panel
Only looks at Feedrate over ride from
keyboard
T Series Operators Manual
5/18/2011
Parameter Value
Enable = 1, Disable =
0
Enable = 2, Disable =
0
Enable = 4, Disable =
0
14-24
Parameter 178 – PLC I/O configuration
This parameter can be use to set switch types from NC to NO and some other options. Each Bit corresponds to a
different function. All values are to be added to the current setting. For example, if you need to switch low lube to
normally open add 1 to this parameter. NOTE: This parameter works only with specific PLC programs. The PLC
program installed in the control MAY NOT be mapped as indicated below. These parameters should only be changed
by a qualified factory technician. The example given below is intended for reference only:
Bit
0
1
Function
Lube Fault
Spindle Fault
Default state
Closed = OK
Closed = Fault
Opposite State
Add 1
Add 2
179 – Lube Pump Operation
This parameter can be configured to control a variety of lube pumps. The value is formatted as MMMSS, MMM for
minutes and SS for seconds. Below is a table of some examples.
Type of Pump
Mechanical/CAM
Electronic “lube
first”
Electronic “lube
last”
Direct Controlled
Pump
MM
M
0
S
S
0
16
0
0
0
0
1
5
16
30
Operation
179=0 Power is on when machine is running a job or in MDI
Mode
179=1600 Holds power on to the pump for 16 minutes of job or
MDI time
179=1600 Holds power on to the pump for 16 minutes of job or
MDI time
179=3015 Waits for 30 min of job or MDI time, then applies
power for 15 seconds.
Parameters 180 – File Transfer COM Port
This parameter specifies which COM port will be used for file transfer. Accepted values are 0 disabled and 1-4 for
COM1 – COM4. Setting this parameter to an accepted value other than 0 will provide a Download and an Upload
option in the drive list of the Advanced File Ops Menu.
Parameters 181 – File Transfer Baud Rate
This parameter sets the maximum file transfer rate for serial communication. The value of this parameter is in KBaud
and has a range of 1.2 to 115.2. The default is 19.2Kbaud. The longer the serial cable the lower the baud rate that can
be used for file transfer.
Parameters 182 – File Transfer Bit Parameters
This parameter sets the number of data bits, type of parity and the number of stop bits for the serial communication file
transfer. The default value is 801 for 8 data bits, no parity and 1 stop bit.
Digit
1’s
10’s
100’s
T Series Operators Manual
Function
Stop bits
Parity
Data bits
Value
1 or 2 stop bits accepted
0 = No Parity; 1 = Even Parity; 2 = Odd Parity
5 – 8 data bits accepted
5/18/2011
14-25
Parameters 183 – File Transfer Flow Control
The setting of this parameter determines the COM port file transfer flow control.
Value
0
1
2
Meaning
No Flow Control
Software (XON/XOFF) Flow Control
Hardware (CTS/RTS) Flow Control
Parameters 184 – File Transfer Timeout
This parameter is used to set the timeout time for downloads. When the Download option is selected you have to start
the download within the set amount of time or the download will time out. The default value of this parameter is 10
seconds, but can be set from 6 seconds to 600 seconds (10 minutes).
Parameters 185 – File Transfer Options
This is a 2 bit parameter to set file transfer options.
Bit
0
1
Function
Ignore CR on downloads
Translate NL (new line) to CR on upload.
Value
1= Yes; 0 = No
2= Yes; 0 = No
Parameters 187 – Hard Stop Homing
This parameter is used when homing off hard stops. The value set in this parameter determines the amount of current
sent to the motor while homing. Value range is 0-32000; typical value for a DC system is 16000. Note that this
feature does not work with velocity mode drives.
Parameters 188-199 – Aux Key Functions
These parameters are used to assign a function to aux keys 1-12 (i.e. P188 = Aux1 … P199 = Aux12). The following is
the list of possible functions that can be executed when an aux key is pressed.
Function
No Function
Input X Axis Position
Input Y Axis Position
Input Z Axis Position
Set Absolute Zero
Set Incremental Zero
One Shot - Drill
One Shot - Circular Pocket
One Shot - Rectangular Pocket
Parameter Value
0
1
2
3
4
5
6
7
8
Function
One Shot - Frame
One Shot - Face
Execute M Code file
Free Axes
Go to Power Feed Menu
XYZ Set Absolute Zero
One Shot - Drill Bolt Hole Circle
One Shot - Drill Array
Parameter Value
9
10
m11*
14
15
16
17
18
For example, if you wanted Aux4 to call up the “One Shot - Circular Pocket” , you would set parameter 191 to 7.
The Input Axis Position functions must be used with the Set ABS/INC Zero functions. After entering the desired value
at the input field provided by the Input Axis Position function, press an aux key assigned either the function Set ABS
Zero or Set INC Zero.
* m is the number of the M code to execute. For example, if the parameter value is set to 7211, the file mfunc72.mac
will be loaded and executed when the Aux key was pressed.
Custom overlays with the keys that represent these functions are available; contact your dealer for pricing.
T Series Operators Manual
5/18/2011
14-26
Parameters 200-207– OPTIC 4 Tach Volts Per 1000 RPM
These parameters control the digital Tach output on the Optic4 boards. They are used on drives like old Fanuc velocity
mode drives that require a tach input. The value put here is the volts/1000 RPM off of the motor.
Parameters 208-215 MPU-based Lash/Screw Compensation Acceleration Coefficient
These parameters control the speed of the Lash and/or Screw Compensation for axes 1-8. The lash will be taken up
with acceleration equal to the coefficient multiplied by the acceleration rate for the axis. A value of zero would
effectively disable MPU-based Lash and/or MPU-based Screw Compensation.
*NOTE: These coefficients are not used by PC-Based Lash nor PC-based Screw Compensation
Parameters 216 PC Based Lash Compensation on/off
This parameter controls which Lash Compensation Algorithm to use. The default value of 0 is recommended because
it allows lash compensation to occur during any kind of motion. If PC Based lash is used then only during an MDI or
programmed move (but not during jogging) will lash compensation be applied.
Function
Value
Use MPU-Based Lash Compensation
0
Use PC-Based Lash Compensation
1
*NOTE: Lash/Screw Compensation Acceleration Coefficients (parameters 208-215) are not used by PC-Based Lash
Compensation.
Parameters 217 PC Based Screw Compensation on/off
This parameter controls which Screw Compensation Algorithm to use. The default value of 0 is recommended because
it allows screw compensation to occur during any kind of motion. If PC-Based scew compensation is used then only
during an MDI or programmed move (but not during jogging) will screw compensation be applied.
Function
Value
Use MPU-Based Screw Compensation
0
Use PC-Based Screw Compensation
1
*NOTE: Lash/Screw Compensation Acceleration Coefficients (parameters 208-215) are not used by PC-Based Screw
Compensation.
Parameters 220-231 – Smoothing Configuration of Feed Per Minute moves
These parameters are used control the behavior of the Smoothing feature. In particular, parameter 220 turns
Smoothing on or off. Note that Smoothing only works for feed-per-minute moves.
Parameter
Description
Recommended values
220
Turn the Smoothing feature ON or OFF .
1 = Smoothing (set to 0 to use Exact
Stop mode)
221
NBpts: The number of points in the smoothing
5 to 10
filter. The higher this value, the more rounded
corners will become (see tolerance below)
222
STEP: Smoothing breaks up a G code program .001 inch / .025mm
into segments of this vector size. Use this rule
of thumb: Tolerance = (Nbpts*STEP)/2.
223
Umax: Sustained safe throughput rate going to
400
the CPU10/MPU11 card.
224
0 = All axes affect calculations during
Application of Centripetal Accel limiting:
This parameter allows you to specify which axis the Centripetal stage.
types affect the calculations done in the
-1 = Only linear axes affect
Centripetal stage of smoothing.
calculations during the Centripetal
stage. Rotary axes are excluded.
226
W: Feature Width over which the Min Angle is 10
determined.
T Series Operators Manual
5/18/2011
14-27
Parameter
227
228
229
230
231
Description
Min_Angle: Minimum angle to smooth in
degrees.
Settings of 95 to 100 degrees will come to a
near stop and produce sharp right angles. 60 to
85 will move continuously while rounding
angles.
S curve: Produces extra gentle stops, starts and
feedrate changes, but increases job run time and
may appear to pause at corners.
Backplot/Smoothing mode : This parameter is
not used on Lathe controls.
Curve Feedrate Multiplier: Reducing this
value below 1.0 will cause the machine to move
slower around curves and corners, minimizing
"bangs" and overshoots. Increasing this value
above 1.0 may allow you to run your machine
faster if the feedrates in arcs and corners are
still satisfactory.
Acceleration Multiplier: This parameter
allows you to adjust the overall acceleration /
deceleration rate as a means to reduce machine
vibration, and noise during starting, stopping
and feedrate changes. Reducing this value
below 1.0 will cause more gentle accelerations
and decelerations. Increasing this value above
1.0 will cause faster accelerations /
decelerations.
Recommended values
For Sharp corners
For rounded
95 to 100 degrees
corners
60 to 85
degrees
0 =Off completely
1 = On completely
Range 0.0 to 1.0
0
1.0 (default value)
0.1 to 5.0 (Depending on user's
preference for speed vs "bangs" and
overshoots)
1.0 (default value)
0.5 to 1.5 (Depending on user's
preference for quickness of
accelerations / decelerations)
Parameters 236-239 – Motor Cooling Coefficients for axes 5-8
See parameters 20-30 for more information.
Parameters 252-255 – Autotune Ka Performance parameters for axes 5-8
See parameters 87-90 for more information.
Parameters 256 – Autotune Enable / Disable
This parameter controls whether or not the Autotune feature can be accessed via the F5 Autotune key in the PID Menu.
Function
Enable Autotune feature, accessible via F5 in PID Menu
Prevent access to Autotune feature
Value
0
1
Autotune does not work with velocity mode drives and therefore this parameter should be set to 1 to prevent access to
Autotune on such machines with these drives.
T Series Operators Manual
5/18/2011
14-28
Parameter 300-307 – Drive assignment to Axes 1-8
These parameters control to what physical drive the commands for motion are sent. Parameter 300 assigns a physical
drive to axis 1, parameter 301 assigns a physical drive to axis 2, and so on. The values for these parameters can be set
to any value from 1-16 based on the table below. These parameters must be set before attempting to move motors.
Contact your dealer before changing these values.
Drive Number
Location
Description
1
Drive Bus Channel 1 Drive types are DC3IOB, DC1, ACSingle, and
2
Drive Bus Channel 2 OPTIC4.
3
Drive Bus Channel 3
4
Drive Bus Channel 4
5
Drive Bus Channel 5
6
Drive Bus Channel 6
7
Drive Bus Channel 7
8
Drive Bus Channel 8
9
GPIO4D Drive Out 1 Connected on the PLC fibers, the GPIO4D can
10
GPIO4D Drive Out 2 also be used with an Optic4 on the Drive fibers.
11
GPIO4D Drive Out 3
12
GPIO4D Drive Out 4
Legacy DC drives like the DC3IO are not
13
Legacy DC 1
compatible with the Drive Bus
14
Legacy DC 2
15
Legacy DC 3
16
Legacy DC 4
Future: Drive numbers may be expanded to support other drive types like the SD3 and SD1
Parameter 308-315 –Encoder assignment to Axes 1-8
These parameters control to which encoder the axis should look for feedback. Parameter 308 assigns an encoder to axis
1, parameter 309 assigns an encoder to axis 2, and so on. The values for these parameters can be set to any value from
1-15 based on the table below. These parameters must be set before attempting to move motors. Contact your
dealer before changing these values.
Encoder Number
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
Location
MPU11 onboard encoder 1
MPU11 onboard encoder 2
MPU11 onboard encoder 3
MPU11 onboard encoder 4
MPU11 onboard encoder 5
MPU11 onboard encoder 6
Drive Bus Channel encoder 1
Drive Bus Channel encoder 2
Drive Bus Channel encoder 3
Drive Bus Channel encoder 4
Drive Bus Channel encoder 5
Drive Bus Channel encoder 6
Drive Bus Channel encoder 7
Drive Bus Channel encoder 8
MPU11 onboard MPG encoder
T Series Operators Manual
5/18/2011
Description
Encoder inputs on the MPU11.
Every Drive Bus device takes up a
Drive Bus encoder even if there is no
encoder going to the drive. The
DC3IOB takes up three encoders.
MPG connector with no index pulse
14-29
Parameters 332-335 – Encoder error suppression
These parameters control suppression of various types of encoder errors on a per encoder basis. These parameters are
bitfields by encoder index, NOT axis index. The mpu11 has 15 encoder indexes. For example to disable encoder faults
for Encoder #5 on the mpu11, enter a 16 into the parameters 332 and 334.
Parameter
332
333
334
335
Function
Suppress encoder differential faults
Suppress encoder differential error messages
Suppress encoder quadrature faults
Suppress encoder quadrature error messages
Parameters 336-339 – Motor torque estimation for velocity mode drives
These parameters are intended to be used with velocity mode drives in order to faciliatate a more accurate display of
the axis load meter bars shown under each position in the main DRO display. If P336 = 0, then this feature is disabled
and the normal PID output is displayed by the axis load meter bars. This feature is enabled if P336 is non-zero.
Parameter
336
337
338
339
Symbol
G
Ga
Gs
Gd
Function
Overall gain setting (0 = disable Motor torque estimation)
Absolute error gain
Error sum gain
Delta error gain
Technical details:
The axis meter bar value (V) is then caluculated as: V = abs(100.0 * G * ((Ea*Ga + Es*Gs + Ed*Gd)) /
integration_limit), where Ea is the absolute error, Es is the error sum, and Ed is the delata error from the PID algorithm
and the integration_limit is from the “Limit” value set in the PID configuration menu. This value V is then bound to
the range 0-100.
Parameter 348, 351, and 354 – MPG/Handwheel Encoder Input 1, 2, and 3
The encoder input for the MPG or handwheel. (1-15) See the encoder chart above. Note: PLC program interaction is
needed to enable an MPG or handwheel.
Parameter 349, 352, and 355 – MPG/Handwheel Detents per Revolution 1, 2, and 3
This value is the number of clicks (detents) per revolution. It is the number of divisions or markings on the mpg or
handwheel. Moving the mpg or handwheel one detent or division will cause the motor to move one jog increment
(depending on the multiplier x1, x10, x100, etc). . Note: PLC program interaction is needed to enable an MPG or
handwheel.
Parameter 350, 353, and 356 –MPG/Handwheel Encoder Counts per Revolution 1, 2, and 3
This value is the number of counts generated per rotation of the mpg or handwheel. Note: PLC program interaction is
needed to enable an MPG or handwheel.
Parameters 357-364 – Axis Drive Max RPM for Axes 1-8
These parameters allow you to set the drive/motor max rate capability (in RPMs) for use by the PID algorithm for the
calculation of the axis KV1 contribution. This value is independent from the axis Max Rate setting in the Jog
Parameters menu, which is used by the control software. However, for those axes whose corresponding parameters are
set to 0 (the default) the the PID algorithm will use the axis Max Rate setting in the Jog Parameters for the calculation
of the axis KV1 contribution. These parameters are intended for 3rd party velocity mode drives that have a different
max rate setting than that of the control software.
T Series Operators Manual
5/18/2011
14-30
Parameters 392-394 – DP-7 parameters
These are parameters specific to the DP-7 probe and are used only if parameter 155 = 2.
Parameter Function
392
DP-7 Pullback Distance:
The distance the probe moves off of the surface after a probing move.
393
DP-7 Pullback Feedrate:
The feedrate for the pullback move.
394
DP-7 Measuring Feedrate:
The feedrate for the slow measuring move.
Parameters 399 – AD1 arc chord tolerance adjustment
This parameter adjusts the precision of AD1 arcs. When Smoothing is turned off (P220 = 0) arc moves (such as G2 and
G3) are generated as a string of many small linear moves that are used to closely approximate the programmed arc.
These small linear moves are called arc chords. These arc chords straddle each side of the theoretical true arc path, but
their distance (in encoder counts) from the path is limited by what value is set in this parameter. The default value is
.5, meaning that by default the arc chord never strays away from theoretical true arc by more than ½ encoder count.
Parameters 900-999 – PLC program parameters
These parameters are used as a way of communicating floating point values to a PLC program. The meanings of these
parameters depends on how a PLC program uses them and can vary from one machine to another. One suggested use
of these parameters is as a set of configuration values. The values of these parameters are saved upon modification
(via a menu or CNC job) and will be retain their values even after shutdown and restart of the control software.
All remaining parameters are reserved for further expansion.
T Series Operators Manual
5/18/2011
14-31
PID Menu
Pressing F4 - PID from the Configuration screen will bring up the PID Menu. The PID Menu provides qualified
technicians with a method of changing the PID dependent data to test and configure your machine.
WARNING
T Series Operators Manual
The PID Parameters should not be changed without contacting your dealer.
Corrupt or incorrect values could cause damage to the machine, personal injury,
or both.
5/18/2011
14-32
F1 - PID Config
This option displays the Oscilloscope tuning screen, and is intended for qualified technicians only. It allows
technicians to modify the PID values, and to see (in real time) the effects of those modifications. Altering the PID
values will cause DRAMATIC changes in the way the servo system operates, leading to possible machine damage.
DO NOT attempt to change these parameters without contacting your dealer.
The general idea is to reduce the Absolute Error (ErrAbs) and the Sum of Absolute Error (ErrSum), which are both
measured in encoder counts. Absolute Error tells you how far off position the machine is at any particular point in
time, and the Sum is used when tuning to make sure the overall error is being reduced.
WARNING
Improper PID
values can ruin
the machine,
cause personal
injury, and/or
destroy the motor
drives!!!
F1 – Edit
Program
Change the program that
will run when F2 is pressed
F2 – Run
Program
Causes the machine to run a
simple test program, while
collecting data
F3 – Ranges
Can be used to specify the
X and Y ranges for the
Oscilloscope view
F4 – Toggles &
Pan
Allows changes to how the
collected data is displayed,
and panning via the cursor
keys
F5 – Zoom In
Zooms in
F6 – Zoom Out
Zooms out
F7 – Zoom All
Fits all of the collected data
into the Oscilloscope view
F8 – Change
Axis
Tells the MPU11 to collect
data for a different axis
(displayed in the top left)
F9 – Save &
Apply
Saves any modifications
F10 – Save &
Exit
Saves any modifications
and exits the Oscilloscope
menu
Page Up –
Tweak +
Allows small modifications
(+1%) to the PID values
while the program is
running. Hold shift for a
larger (+10%) modification.
Page Down –
Tweak -
Allows small modifications
(-1%) to the PID values
while the program is
running. Hold shift for a
larger (-10%) modification.
F5 - Autotune
This option is used by qualified technicians to automatically determine values for Max Rate, Accel/decel time, and
Deadstart (See section Machine Configuration, earlier in this chapter) as well as the PID parameters for each installed
axis. The Autotune procedure will make a series of moves on each axis, traveling a limited distance (configured via
parameters 95-98 and 156-159) from the initial position in all directions to determine the friction and gravity of each
axis. The initial high-speed move will use half of this distance.
T Series Operators Manual
5/18/2011
14-33
● NOTE: You cannot run Autotune on paired axes. Do not run Autotune unless requested to do so by a qualified
technician.
F6 - Drag
This option is used by qualified technicians to determine whether your machine is binding anywhere along the axis
travel. Press F6-Drag to begin the drag test. Press F1 to select the axis you wish to check. Hit the CYCLE START
button. A text file drag_x.out, or drag_z.out file is generated and stored in the c:\cnct directory. If significant drag
occurs, a message will be displayed on-screen. Contact your dealer to correct the problem as soon as possible.
F7 - Laser
This option is used by qualified technicians to take automated laser measurements and create or adjust the ballscrew
compensation tables using accordingly. Do not attempt to run automatic laser compensation without first contacting
your dealer for details.
F8 - Drive
This menu will only appear on AC systems and only affects using SD or ACSingle drives. It is not for general viewing
and definitely not for modification by any unqualified individual. For more information about this menu option, refer
to the SD installation manual.
F9 - Plot
This option is used by qualified technicians to plot data.
Test
This menu only appears if the system has not yet been configured and initialized or if a new solid state disk has been
installed. For more information, please contact your dealer.
T Series Operators Manual
5/18/2011
14-34
Chapter 15
CNC Software Messages
CNC software startup errors and messages
Number Message
102
102 Error
initializing
CPU...cannot
continue.
103
Error sending setup
104
Error sending PID
setup
105
mpu.plc file read
error..cannot
continue
The PC clock
appears to be wrong
106
199
CNC started
Cause & Effect
Error while sending .hex file. Cannot
communicate with MPU11 or it is not
plugged in.
Action
Inspect MPU11 connection,
or fix missing or corrupted
hex file. Contact Dealer
Unable to send setup command to
MPU11. Cannot communicate with
MPU11 or it is not plugged in.
Unable to send PID setup command to
MPU11. Cannot communicate with
MPU11 or it is not plugged in.
Missing or error in mpu.plc.
Inspect MPU11 connection,
or fix missing or corrupted
hex file. Contact Dealer
Inspect MPU11 connection,
or fix missing or corrupted
hex file. Contact Dealer
Contact dealer
Install or recompile PLC
program.
The time on the PC internal clock is
earlier than the time recorded in a
previously stored file
CNC control software has started.
Messages issued upon exit from CNC software
Number Message
201
Exiting CNC due to a
known error
202
Exiting CNC due to a
math error
204
Exiting CNC...Normal
Exit
Autotune run
222
Cause & Effect
MPU11 not responding, or mpu11.hex,
mpu.plc is missing or damaged.
Action
Contact dealer
Check for possible software
corruption
A floating-point math error occurred.
Contact dealer
Possible corruption of cnc.tem, cncm.job, Delete corrupted files and
or cncm.wcs.
reboot software.
CNC control software is shuting down
normally.
added to log whenever autotune is run
Messages and Prompts in the Operator Status Window Status messages
Number Message
301
Stopped
302
Moving...
303
Paused...
304
MDI...
T-Series Operator’s Manual
Cause & Effect
No operations in progress
Motors are moving while a CNC program is
running
Motion is paused while a CNC program is
running (FEED HOLD)
CNC software running in MDI mode
5/18/11
Action
15-1
Number Message
305
Processing...
306
307
308
309
310
311
312
313
314
315
317
318
319
320
321
322
323
324
325
326
Error
327
328
329
330
331
332
15-2
Job finished
Operator abort: job
canceled
Waiting for input
#NN
Waiting for CYCLE
START button
Waiting for output
#NN
Waiting for memory
#NN
Waiting for PLC
operation (Mnn)
Waiting for dwell
time
Waiting for system
#NN
Searching...
Waiting for
automatic tool
change
Operator Abort
probing cancelled
Probing cycle
cancelled
Probe stuck
Stuck Probe Cleared
Stall: probing
cancelled
Stall: job cancelled
Limit: probing
cancelled
Limit: job cancelled
Fault: probing
cancelled
Message
Fault: job cancelled
Cutter comp error:
job cancelled
Invalid parameter:
job cancelled
Canned cycle error:
job cancelled
Threading error: job
cancelled
Search Failed
Cause & Effect
CNC software running in a mode other than
MDI
Normal end of CNC program
ESC or CYCLE CANCEL pressed. Job is
cancelled.
M100 or M101 executing. Program will
continue once specified input opens or closes.
M0, M1, M100/75, or Block Mode is executed.
M100 or M101 executing. Program will
continue once specified output opens or closes.
M100 or M101 executing. Program will
continue once specified memory bit changes to
the correct state.
PLC program not clearing PLC operation in
progress
G4 executing. Program waits for specified
dwell time then continues.
M100 or M101 executing. Program will
continue once specified PLC system variable
changes to the correct state.
Run/search in progress
cnctch.mac executing
Action
Press Cycle Start
Enter required
information.
ESC or CYCLE CANCEL pressed while
doing a probing move
probing cycle was cancelled
probe is stuck, or probe hit an object when it
wasn't expecting contact.
probe cleared after being stuck
probing was cancelled because of a stall
job was cancelled because of a stall
probing was cancelled because of a limit error
job was cancelled because of a limit error
probing was cancelled because of a fault
Cause & Effect
Action
job was cancelled because of a fault
job was cancelled because of a cutter comp
error
job was cancelled because of an invalid
parameter
job was cancelled because of a canned cycle
error
The programmed threading move will cause an
axis to exceed its maximum rate.
Run/Search was unable to find the requested Gcode line
5/18/11
T-Series Operator’s Manual
Number Message
334
Locating position to
resume job...
335
Emergency Stop
Released
336
Digitize cancelled
Cause & Effect
Run/Search is locating the job continuation
point in the program
Emergency Stop Button has been released
337
338
Digitize complete
Job Cancelled
339
Jogging...
340
Limit (#__) cleared
341
Probing Cycle
Finished
Waiting for motion to
stop
Waiting for stop
reason reset
342
343
344
345
346
Action
ESC or CYCLE CANCEL pressed during
digitizing
A digitizing routine ran to completion
ESC or CYCLE CANCEL pressed during job
run
An axis jog key is pressed and machine is
moving the corresponding axis
A previously tripped limit switch is now in the
“untripped” position
A probing cycle ran to completion
PC is waiting for the MPU11 to complete
motion
PC is waiting for the MPU11 to reset the stop
reason (as part of the PC/MPU11
communications handshake).
Feedrate modified
The effective feedrate has been lowered
due to spindle
because the spindle is spinning slower than the
threshold percentage of the commanded spindle
speed. (The threshold percentage is specified
in P149.)
Waiting for spindle to Job progress is paused until the actual spindle
get up to speed
speed reaches the threshold percentage of the
commanded spindle speed. (The threshold
percentage is specified in P149.)
Waiting for spindle
Job progress is paused until the spindle turns
direction
the commanded direction.
Abnormal stops (faults)
Abnormal stops are detected in the following order: PLC, servo drive, spindle drive, lube, ESTOP. This means that if
both the servo drive and the spindle drive have faulted, the servo drive fault message would appear.
Number Message
401
PLC failure
detected
404
Spindle drive
fault detected
Cause & Effect
MPU11 stopped with PLC failure
bit set. Job cancelled.
MPU11 stopped with spindle drive
fault bit set. Job cancelled.
405
Lubricant level
low
406
Emergency Stop
detected
limit (#1) tripped
MPU11 stopped with low lube fault
bit set. Current job will finish but
nothing will work after that.
MPU11 stopped with no fault bits
set. Job cancelled.
MPU11 stopped with limit switch
tripped. Job cancelled.
M103 time expired before M104
encountered. Job cancelled.
407
408
Programmed
action timer
expired
T-Series Operator’s Manual
5/18/11
Action
Check PLC fibers and PLC logic
power.
Check inverter for fault or reset spindle
contactor OCR, then cycle
EMERGENCY STOP
Add lube or check low lube switch
wiring then cycle EMERGENCY
STOP
Release Estop
Clear limit switch
Find out why timer expired before
specified action was completed.
15-3
Number Message
409
_ axis lag
410
15-4
_ axis position
error
Cause & Effect
Lag Distance (Allowable Following
Error) is detected on any axis for
more than 1.5 seconds. Where: Lag
Distance= Feedrate inch/min
--------------------------+ .0005 inch/int
240,000 ints/min
(Allowable Following Error)
All axis motion is stopped and the
CNC program is aborted. The
probable causes of this error are:
1. The machine is doing a very
heavy cut.
2. The maximum rates or the
acceleration values for the motors
are set too high.
3.The motors are undersized for the
application
A position error > .25 inches is
detected on any axis. All axis
motion is stopped, power to the
motors is released (all servo drive
commands cease) and the CNC
program is aborted.
The probable causes of this error
are:
1. The motor is wired up
backwards.
2. Noise is getting into the system
via the motor cables (the line
integrity has been violated).
3. An encoder error occurred.
5/18/11
Action
1. If the problem is occasional heavy
cuts, slowing down the cutting feedrate
can solve the problem.
2. If the problem only occurs on high
speed moves then either the maximum
speed or the acceleration is set too
high. Lower the values in the Motor
Setup screen or run Autotune again to
determine new values.
3. If there are persistent lag errors in
normal operations, this indicates that
the motors are too weak to handle the
required loads. Increase the gear ratios
or get more powerful motors.
1. Try to slow jog the motor and watch
the DRO position. If the position on
the DRO goes opposite the direction
indicated on the jog button, then the
motor is wired up backwards. Change
the motor wiring.
2. Check the motor cabling paying
particular attention to the ground
connections. Replace the cable if it is
damaged or repair the motor
connections.
3. Jog the motor awhile, at the
maximum rate, using the fast jog
buttons. (Check the fast jog rate in the
motor jog parameters screen to make
sure it is set equal to the maximum
motor rate.) If the motor seems to
jump around rather than accelerate and
decelerate smoothly then you are
probably fighting an encoder error.
Swap the motor with one from another
axis and see if the error follows the
motor. If it stays with the axis, replace
the MPU11. If it follows the motor,
replace the motor cable. If the problem
still persists, replace the motor and
encoder.
T-Series Operator’s Manual
Number Message
411
_ axis full power
without motion
Cause & Effect
90% Power (PID Output > 115) is
applied to any axis and no motion
>.0005 inches is detected, for more
than the time specified in parameter
61 (default .5 sec.). All axis motion
is stopped and the CNC program is
aborted.
The probable causes of this error
are:
1. One of the axes is against a
physical stop.
2. The servo drive has shutdown
due to a limit switch input.
412
_ axis encoder
differential error
417
Abnormal end of
job
Search Line or
Block not found
Search line in
embedded
subprogram
_ axis motor
overheating
An error condition was detected in
the differential signal levels for this
axis encoder. May indicate a loose
or severed encoder cable or a bad
encoder. This will stop all motion
and cancel the job.
Job ended without reason.
418
419
420
421
Motor(s) too hot:
job canceled
422
Check Jog Panel
cable
Check MPG
cable
428
T-Series Operator’s Manual
Action
1. If the axis has run into a physical
stop, use the slow jog mode to move
the axis away from the stop. Determine
and set software travel limits to stop
machine before in runs into the hard
stops.
2. If the axis is not on a physical stop,
check for a tripped limit switch. If it is
then the software is commanding a
move into the switch but the hardware
is shutting the move down. Go to the
motor setup screen and enter the limit
switch input number if applicable.
3. Make sure the switch input is not
unstable or noisy. If it is then replace
the switch. If the problem persists it
may be necessary to create separate
home and limit switch inputs.
Use slow jog to move opposite the
direction causing the error and clear all
limit switches. Jog toward the
direction causing the error, if no
motion occurs then a servo drive
failure is indicated.
Reconnect/replace encoder or encoder
cable.
Requested search input data not
found in loaded CNC file.
Requested search line is found, but
is part of an embedded/extracted
subprogram
CNC software estimates that a
motor has reached the warning
temperature (set in Parameter 29).
Motor is overheating or the
temperature file is corrupted. Job
will be cancelled.
CNC software estimates that one or
more motors have reached the limit
temperature (set in Parameter 30).
Will not be able to run until motor
cools down.
Jog panel failure or loose cable.
Reconnect jog panel cable.
MPG failure, loose cable, or was
turned off.
Reconnect MPG cable and turn axis
selector knob to an axis.
5/18/11
Type in correct data or load correct
job.
Use another line number
Contact dealer.
Determine what’s causing motor to
overheat or delete cnc.tem file and
reboot.
Contact dealer.
Determine what’s causing motor to
overheat or delete cnc.tem file and
reboot.
15-5
Number Message
434
_ idling too high:
Releasing power
435
436
_ axis runaway:
Check motor
wiring
Servo drive
shutdown
437
Servo power
removed
438
Spindle slave
position error
439
_ axis servo drive
data output error
441
_ axis
overvoltage
442
_ axis
undervoltage
15-6
Cause & Effect
Axis is not moving and no job is
running but axis has stopped against
some abnormal resistance. Power is
released to motors.
Motor was in a runaway fault
condition. Power to motor will
automatically be shut off.
This error message is produced by
hardware detection of a physical
error.
The servo drive hardware generates
this error message if it detects either
an overcurrent or overvoltage
condition. The particular hardware
condition is reflected on the servo
drive LED’s. Once the servo drive
detects this error condition it stops
all motion and removes power to
the motors. The hardware indicates
the presence of this condition to the
CNC software via the servo drive
fault input to the PLC.
Axis was moving more than 300
RPM while power was supposed to
be off.
1.) Motor may be wired backwards.
2.) May be a shorted servo drive.
3.) Axis motion is canceled but
motor continues to move due to
inertia, which is probably caused by
an unbalanced axis.
Power to motors is released.
The slaved axis moved too far in
the wrong direction during a
spindle-slaved move (such as in
rigid tapping, threading, and feedper-revolution moves). Job is
cancelled.
Logic power failure or lost of
communication from the drive to
the MPU11.
Input power has gone higher than
340VDC and will shutdown the
drive and removes power. The
motor brake will engage for 5
seconds in this condition.
Drive input power is less than 80
VDC.
5/18/11
Action
Run an autotune to adjust motor
settings.
Check motor wiring
On DC systems check status of the
servo drive LED’s and check fibers
4&5. If this message is displayed on an
AC system check P178 bit 4 is set.
Check motor wiring, servo drive, or
look at Kg value in PID and make sure
it’s not above +/- 5.
Check parameter 34 for wrong sign in
front of encoder counts.
Is logic LED on? Check fiber optic
cables to drive. For SD1 drives, make
sure bus cables are shielded and are as
short as possible. Power unit down
and check drive connections.
Check input voltage is below
340VDC. If not, incoming VAC needs
lowered.
Check supply voltage.
T-Series Operator’s Manual
Number Message
443
_ axis
commutation
encoder bad
Cause & Effect
Control detected invalid
commutation zone value.
444
_ axis
overtemperature
detected
_ axis overcurrent
detected
Drive overtemp sensor tripped. No
motor power.
446
_ axis servo drive
data input failure
Communication Checksum error.
No motor power.
447
_ axis (#) bad
index pulse
detected
_ axis(#) motor
wired backwards
Manual
movement
detected in
restricted area
Voltage brake
applied
Noise picked up by encoder cable
or misaligned encoder. No motor
power.
Detection for this error condition is
currently unimplemented.
Detection for this condition is
currently unimplemented.
451
Current brake
applied
Overcurrent spike was detected on
the drive.
452
PC Receive Data
Error
453
CPU Receive
Data Error
A fatal communication error
occurred between the MPU and PC.
The error was detected on the PC
side.
A fatal communication error
occurred between the MPU and PC.
The error was detected on the
MPU11 side
445
448
449
450
T-Series Operator’s Manual
Overcurrent detected on an axis.
No motor power.
Overvoltage condition was
detected. Electronic braking was
applied by offloading excess
voltage to dropping resistors.
5/18/11
Action
Perform a motor Move Sync in the
Drive menu. A Zero (0) or Seven (7)
is an invalid zone. Check for:
a.) Wiring problem in the encoder
cable or motor end cap (broken
encoder wires).
b.) Encoder cable shield connected at
motor end, when it shouldn’t be.
c.) Bad encoder.
d.) Motor power cable shields not
connected.
e.) Drive not grounded properly.
The drive is being run at over capacity
or the cooling fan is either not
functioning or its air flow is blocked.
Try to jog the axis. The drive will
reset the current limit and try to move
the motor. If the error comes back,
check for a short in the motor output.
Check fiber optic cables. Verify
continuity between drive chassis,
ground strip and Earth ground.
Remove noise or align the encoder.
This error condition should not appear.
But if it does, contact your dealer.
This condition should not appear.
Usually this error condition is
innocuous even if this message occurs
every once in a while in a job.
However, if this message occurs in a
continuous stream, contact your dealer.
Usually this error condition is
innocuous even if this message occurs
every once in a while in a job.
However, if this message occurs too
often, it may mean you need a higher
current drive. But, if this message
appears in a continuous stream,
something is seriously wrong, and you
should hit E-Stop to cut power to the
drive and then contact your dealer.
Restart the software to clear the error.
If this error occurs often there may be
an issue with the network
configuration or the Ethernet cable.
Restart the software to clear the error.
If this error occurs often there may be
an issue with the network
configuration or the Ethernet cable.
15-7
Number Message
454
axis scale
encoder
differential error
455
axis encoder
quadrature error
456
axis scale
encoder
quadrature error
457
Unable to find
home
461
Spindle axis is
not set
Cause & Effect
An error condition was detected in
the differential signal levels for this
axis scale encoder. May indicate a
loose or severed encoder cable or a
bad encoder. This will stop all
motion and cancel the job.
The axis encoder skipped a
transition state on its countup/count-down sequence. May
indicate a bad encoder or a loose or
severed encoder cable. This will
stop all motion and cancel the job.
The scale encoder skipped a
transition state on its countup/count-down sequence. May
indicate a bad encoder or a loose or
severed encoder cable. This will
stop all motion and cancel the job.
A commanded move was seeking
either an index pulse or a hard stop,
but neither was found.
An operation aborted because the
spindle axis parameter (P35) has an
incorrect value.
Action
Reconnect/replace scale encoder or
scale encoder cable.
Reconnect/replace encoder or encoder
cable.
Reconnect/replace scale encoder or
scale encoder cable.
Reconnect/replace encoder or encoder
cable if move was seeking an index
pulse. Check that hard stop was not
broken off nor overrun.
Contact dealer.
CNC syntax errors
Number Message
501
Invalid character on
line NNNNN
502
Invalid G code on line
NNNNN
503
Invalid M function on
line NNNNN
504
Invalid parameter on
line NNNNN
505
Invalid value on line
NNNNN
506
Only 1 M code per line
15-8
507
No closing quote
508
509
Macro nesting too
deep
Option not available
510
Too many macro arg’s
511
Missing parameter
Cause & Effect
Invalid character on CNC line. Job
cancelled.
Invalid G code encountered on CNC line.
Job cancelled.
Invalid M function encountered on CNC
line. Job cancelled.
Invalid or missing number after letter. Job
cancelled.
Value out of range (T, H, D). Job
cancelled.
More than one M code appears on the line.
Job cancelled.
The closing quotation mark (“) is missing.
Job cancelled.
Macro nesting limit exceeded on attempt to
invoke a subroutine. Job cancelled.
Attempt to access a locked software option.
Job cancelled.
Too many arguments were given in a G65
macro. Job cancelled.
A parameter is required or expected but not
found. Job cancelled.
5/18/11
Action
Remove character from
program.
Correct invalid G-code.
Correct invalid M-code.
Correct program.
Correct program.
Move 2nd M-code to
next line.
Add quotation.
Create a second
program.
Contact Dealer.
Correct number of
arguments.
Correct program.
T-Series Operator’s Manual
Number Message
513
Expected “=”
514
Empty expression
515
518
Syntax error in
expression
Unmatched bracket
(parenthesis)
Evaluation stack
overflow
Undefined variable
519
Too many variables
520
Invalid variable name
521
522
Divide by zero
Domain error
523
Invalid value in
assignment
Variable is read-only
516
517
524
525
526
Missing P value
M22x Missing initial
variable
527
M22x initial variable
parse error
M225 String variable
not allowed
528
Cause & Effect
Error in expression to left of “=”, missing
“=”, or orphaned parameter. Job cancelled.
The expression contains no operands. Job
cancelled.
Illegal character in number, variable or
function. Job cancelled.
Brackets or parentheses are paired
improperly or misplaced. Job cancelled.
Brackets or parentheses are nested too
deeply. Job cancelled.
The variable name does not exist. Job
cancelled.
The space allotted for user-defined
variables has been exceeded. Job
cancelled.
The variable name contains an illegal
character. Job cancelled.
Attempt to divide by zero. Job cancelled.
Imaginary number would result (square
root of a negative number). Job cancelled.
Attempt to assign an illegal value to a
system variable. Job cancelled.
Attempt to assign a value to a read-only
system variable. Job cancelled.
P parameter is expected but is missing
M224 or M225 was not immediate
followed by a #variable reference.
M224 or M225 was immediate followed
by an invalid #variable reference.
M225 was immediately followed by a
string #variable (which is invalid). Only
numeric variables are allowed here.
The #variable specified after the M225 was
not valid, or not readable due to a machine
error.
The #variable specified after the M224 was
read-only, or not writeable due to a
machine error.
The beginning of the quoted (“) format
string was not found or was in the wrong
place on the G-code line.
The format string did not end with a quote
(”)
529
M225 invalid variable
530
M224 invalid variable
531
M22x missing initial
quote
532
M22x missing end
quote
533
M22x embedded quote The format string contained a quote (“) in
not allowed
the middle of it.
534
M22x character limit
exceeded
M22x invalid format
string
535
T-Series Operator’s Manual
The format string was too long
The format string contained invalid format
codes
5/18/11
Action
Correct equation.
Correct expression.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
See Chapter 13 for
syntax of M224 or
M225
Correct program.
Correct program.
Correct program.
Correct program.
See Chapter 13 for
syntax of M200, M223,
M224 or M225
See Chapter 13 for
syntax of M200, M223,
M224 or M225
See Chapter 13 for
syntax of M200, M223,
M224 or M225
Correct program.
Correct program.
15-9
Number Message
536
M22x missing format
specifier
537
M22x Missing
Argument
538
M22x argument parse
error
539
M22x variable type
mismatch
540
M22x variable cannot
be read
542
543
544
M22x character limit
exceeded
Missing L parameter
Too many axes
545
Value out of range
547
Move by counts not
allowed
548
String too long
Cause & Effect
The format code was missing the its
specifier
A format code was specified in the format
string, but its corresponding #variable
argument was missing
A format code was specified in the format
string, but its corresponding #variable
argument had a syntax error
A string format code was specified in the
format string, but its corresponding
#variable argument was numeric OR a
numeric format code was specified in the
format string, but its corresponding
#variable argument was a string
A format code was specified in the format
string, but its corresponding #variable
argument was invalid or there was a
machine error when accessing it.
The resultant formatted string after all the
format codes were processed was too long.
L code was missing
More than 1 axis was specified with M128,
OR the Simultaneous Contouring feature is
not enabled. Without the Simultaneous
Contouring feature, a maximum of 3 axes
are allowed per G-code line.
Parse error occurred because value was out
of range
Cutter comp (G41/G42) was on when
M128 was specified
A quoted string was too long (usually a file
name was longer than its allowed limit).
Action
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Correct program.
Specify fewer axes on
the G-code line OR
Contact Dealer for
information about
obtaining the
Simultaneous
Contouring feature.
Correct the value
Issue G40 (Cutter comp
off) before issuing
M128
Shorten the file name.
Cutter compensation errors
Number Message
601
Error: no compensation
in MDI
603
605
606
607
15-10
Arc as first uncomp.
move on line NNNNN
Canned cycle not
allowed on line
NNNNN
G53 not allowed on line
NNNNN
Set home not allowed
on line NNNNN
Cause & Effect
G41 or G42 entered in MDI. MDI is not
canceled, but cutter compensation does
NOT go into effect. Remainder of line
processed.
Arc specified as first move after end of
compensation (G40). Job cancelled.
Canned cycle attempted during
compensation. Job cancelled.
G53 attempted during compensation.
Job cancelled.
M26 attempted during compensation.
Job cancelled.
5/18/11
Action
Do not use G41 or G42 in
MDI.
First move after G40 must
be a linear move.
Do not use cutter comp.
with canned cycles.
Do not use M26 with
cutter comp.
T-Series Operator’s Manual
Number Message
608
Ref. point move not
allowed on line
NNNNN
Cause & Effect
G28, G29, or G30 attempted during
compensation. Job cancelled.
Action
Do not use return points
with cutter comp.
Parameter setting errors
Number Message
701
G10 error: no R-value
on line NNNNN
702
G10 error: invalid D on
line NNNNN
703
G10 error: invalid H on
line NNNNN
704
G10 error: invalid P on
line NNNNN
705
G10 error: No D, H, or
P on line NNNNN
Cause & Effect
G10 used with no R-value. Job cancelled.
Action
Input an R-value.
Job cancelled (D0 cannot be set; it is
always zero).
G10 H0 Rxx specified. Job canceled (H0
cannot be set; it is always zero).
G10 used with unknown P value. Job
cancelled.
G10 used without D, H, or P to assign
value. Job cancelled.
Change D to a valid
value.
Change H to a valid
value.
Change P to a valid
value.
Add appropriate D, H,
or P value.
Canned cycle errors
Number Message
801
Error: No R point on line
NNNNN
802
Error: Q = 0 on line
NNNNN
803
Error: No Z point on line
NNNNN
804
Error: Ggg invalid on
line NNNNN (gg = 76,
86, 87, 88)
805
Error: No Q value on line
NNNNN
806
Error: No P value on line
NNNNN
Cause & Effect
No R-value specified. Job cancelled.
Action
Add an R-point.
Q value of 0 specified (Q used for G73
and G83 only). Job cancelled.
No Z value specified for canned cycle. Job
cancelled.
Unimplemented canned cycle requested.
Job cancelled.
Insert a Q non-zero
value.
Add a Z-value.
Q value not specified for G73 or G83. Job
cancelled.
P value (dwell time) not specified for G82
or G89. Job cancelled.
Insert a Q-value.
Change to a valid Gcode.
Add a P-value.
Miscellaneous errors
Number Message
901
Ref. point invalid on
line NNNNN
902
No prior G28 or G30
on line NNNNN
903
Warning: No
coordinates for G50 on
line NNNNN
905
Warning: 0 radius arc
on line NNNNN
906
Warning: unknown arc
on line NNNNN
T-Series Operator’s Manual
Cause & Effect
G30 with invalid P value (must be 1 or 2).
Job cancelled.
G29 with no preceding G28 or G30.
Action
Change P-value to a 1
or 2.
Add a G29 or G30.
G50 with no axis coordinates to set.
Remainder of line processed; job continues.
Add coordinates.
Arc move was specified with a zero radius.
Specify a radius.
Move is done as a linear move; job continues.
Position of arc move could not be determined Correct program.
from parameters. Move is done as a linear
move; job continues.
5/18/11
15-11
Number Message
907
_ axis travel exceeded
on line NNNNN
909
Program too long: job
canceled
910
No subroutines in MDI
911
Illegal recursion
913
Could not open file
filename.ext
914
Tool library invalid for
Tnn
915
DSP window retry sN
fN rN
916
Unexpected probe
contact
Invalid tilt lookup table
917
918
Probe unable to detect
surface
919
DSP window failed
maximum retries
Unable to clear
obstacle
Unable to determine
corner
Out of memory
File read error
920
921
922
924
925
926
927
928
929
15-12
Error reading job file
Failed to locate job
continuation position
Too many subprogram
calls
Error Loading Log
Configuration file…
Using defaults
Log Level set to __
Cause & Effect
Software travel limit would be exceeded by
the requested move. Job cancelled.
Attempt to run a job over 1MB in length,
without the unlimited program size option.
Job cancelled.
Specified O9100 - O9999 in MDI, which
would begin an embedded subprogram. MDI
cancelled.
Attempt to execute a subprogram or macro
that calls itself, either directly or indirectly.
Job cancelled.
Attempt to call a subprogram or macro, but
the subprogram file does not exist. Job
cancelled.
Enhanced ATC is enabled and the tool library
does not have a valid bin number assigned.
Job cancelled.
DSP window checking failed, move will be
repeated unless the maximum retries have
been reached, s = number of successes, f =
number of failures, r = number of times the
maximum retry value has been reached
probed tripped when a cycle did not expected
contact
The tilt lookup table file (tilt.tab) has an
invalid format or if it is not found
Probe travelled maximum distance without
contact,dsp window checking failed,or probe
repeatability failed.
DSP probe reached the maximum retry limit
without a successful window
Probing cycle failed to clear an obstacle
Probing cycle failed to find corner (inside
and outside corner)
problem allocating memory
Problem reading the job file, this error occurs
if the file was opened successfully but there
was an error while reading the file.
same as above at a different place in the code
Job continuation from the Run Menu failed.
Action
Check program, part
zero or tool offset.
Contact Dealer or
break up program.
Call correct
subprogram.
Make sure file name is
correct and is in the
ncfiles directory.
Put tool in valid bin.
Do a Run/Search
Nesting level of subprograms is too high. I.e.
a subprogram calls another subprogram
which calls another subprogram, which calls
another subprogram, etc…
There was an error while loading the log
configuration file. Default settings will be
used.
The logging level parameter (P140) has been
changed.
5/18/11
T-Series Operator’s Manual
Number Message
930
Log Level
Configuration file not
found… Creating new
configuration.
931
Using MPU based
Backlash
Compensation...
932
Error during Tool
Check
933
Log file initialized
934
Warning: Excess
precision truncated
935
_ axis (#) scale
disabled
936
_ axis (#) scale enabled
944
945
946
947
MPU requested resend
PC requested resend
PC resending
PC received data out of
order
PC packet error
948
Cause & Effect
The log level configuration file was not
found. A default file will be created.
This is a notification that backlash
compensation will be handled by the MPU,
and not on the PC.
A general error condition occurred when the
Tool Check key was pressed.
There was an error in trimming the log file,
or the log file did not exist, so a new log file
has been created.
A CNC program is using axis positioning
precision greater than what is displayed, and
therefore the actual commanded positions are
truncated. This happens when the
Simultaneous Contouring feature was not
enabled. This feature must be enabled for the
extra precision to be acknowledged.
A scale is enabled for this axis but
compensation was disabled. Scale
compensation is disabled at initial power up,
configuration changes, and during homing
moves.
A scale is enabled for this axis and
compensation was enabled. This happens
after homing the axis.
The MPU requested a resend
The PC requested a resend
The PC is resending
The PC needed to reorder data received from
the MPU
The PC received bad data from the MPU and
will try to recover by requesting a resend.
Action
Not Applicable
Contact Dealer for
information about
obtaining the
Simultaneous
Contouring feature.
Home the machine.
Not Applicable
Status Message
Status Message
Status Message
Status Message
Status Message
Configuration Modification messages
Number
111
444
555
556
777
999
Message
___modified: __ -> __
__ modified: __ -> __
__ modified: __ -> __
Axis __ converted: __ -> __
__ modified: __ -> __
Parm #__ modified: __ -> __
T-Series Operator’s Manual
Cause & Effect
An axis configuration parameter was modified.
A servo drive configuration parameter was modified.
A PID configuration parameter was modified.
A PID configuration parameter was converted.
An axis configuration parameter was modified.
A machine parameter was modified.
5/18/11
15-13
15-14
5/18/11
T-Series Operator’s Manual