advertisement
MILLPWR
G2
ACU-RITE
®
User’s Manual
ii
Controls of the MILLPWR
G2
Keys on console
Motion control keys
Key Function
GO
key (e.g. run a program).
STOP
key (duel function: press once to pause, press twice to stop a program).
Data Entry keys
Key Function
CANCEL
key cancels operation, i.e. form.
CLEAR
key clears selections, i.e. values in a field, a program step.
USE
key completes operation, i.e. data entered in a form.
ENTER
key completes selection, i.e. values entered in a field.
Function keys
Key Function
ABS/INCR
key toggles between Absolute or Incremental positioning.
DRO/PGM
key toggles between the DRO display or Program mode display.
VIEW
key opens menu for setting part graphic display parameters, i.e. type, orientation.
INFO
key opens on-screen manual.
MM
key toggles between INCH or MM mode.
SETUP
key opens configuration menu.
Numerical keys
Key Function
ZERO
key.
Axis Keys
Key
Soft Keys
Key
ONE
key.
TWO
key.
THREE
key.
FOUR
key.
FIVE
key.
SIX
key.
SEVEN
key.
EIGHT
key.
NINE
key.
DECIMAL
key.
PLUS / MINUS
key.
Function
AXIS
keys open the datum, or preset form.
Function
SOFT KEYS
performs the function directly above it.
Move Table and Navigation keys
Key Function
LEFT
ARROW key will move the table or display cursor depending on the function selected.
RIGHT
ARROW key will move the table or display cursor depending on the function selected.
UP
ARROW key will move the table or display cursor depending on the function selected.
DOWN
ARROW key will move the table or display cursor depending on the function selected.
Calculator Function keys
Key Function
CALC
key opens the calculator.
PLUS
key.
Milling Function keys
Key Function
TOOL
key opens the SET TOOL
Dialogue.
RECT
key opens the Rectangle milling popup menu.
CIRCLE
key opens the Circle milling popup menu.
HOLES
key opens the Hole pattern popup menu.
POS
key opens the POSITION / DRILL data input dialogue.
LINE
key opens the MILL LINE data input dialogue.
ARC
key opens the MILL ARC data input dialogue.
BLEND
key opens the BLEND \
CHAMFER data input dialogue.
BLANK
key opens the user defined milling function data input form.
MINUS
key.
MULTIPLIER
key
DIVIDE
key.
Peripherals Supported:
USB memory devices; e.g. a memory stick.
Networking, USB pointing devices; e.g. a mouse, USB keyboard.
Potentiometer for feed rate override
Feed rate override
ACU-RITE MILLPWR
G2
iii
iv
Manual Information
Message symbols
Attention!
This symbol indicates that there is one or more of the following risks when using the described function
Danger to work piece
Danger to fixtures
Danger to tool
Danger to machine
Danger to operators
Damage!
This symbol indicates that there is risk of MILLPWR
G2 damage, or electrical shock if instructions are not adhered to.
Different from machine to machine!
This symbol indicates that instructions may apply differently from one type of machine to another type of machine.
Refer to another Manual!
This symbol indicates that information required is located elsewhere (i.e. Machines Owner Manual).
Advice!
This symbol indicates that an Advice tip is being provided.
Important, and/or additional information about the function described.
ACU-RITE MILLPWR
G2
v
Fonts Used in this manual
Reference to the: Console HARD KEYS.
Reference to the: Display Screen Soft Keys.
Reference to the: Display Screen DIALOGUES.
Reference to the: Display Screen FIELDS.
Changes (errors)
HEIDENHAIN CORPORATION is continuously striving to improve.
Please help HEIDENHAIN CORPORATION by sending your request to the following e-mail address: [email protected]
Visit www.ACU-RITE.com for latest version of this manual.
Model, Software and Features
This manual describes functions and features provided by
MILLPWR
G2
as of the following NC software number.
Console model
ACU-RITE MILLPWR
G2
Software
NC software number
751005-01
The machine tool builder may not allow some of the functions described in this manual, therefore they may not be among the features provided by the MILLPWR
G2
on your machine tool.
The machine tool builder representative can assist with becoming familiar with the features of the machine.
Many machine manufacturers, as well as HEIDENHAIN Corp., offer programming courses for the MILLPWR
G2
. We recommend these courses as an effective way of improving your programming skill and sharing information and ideas with other MILLPWR
G2
users.
Intended place of operation
The MILLPWR
G2
is intended for use primarily in industrially-zoned areas. Refer to the respective installation manual for additional information.
vi
MILLPWR
G2
Access Code
Access Code
Attention!
The parameter access code is 8891
Access to Machine Parameter Operations
The access code must be entered before the installation setup parameters can be accessed or changed.
Press the SETUP key to enter the Job Setup dialogue.
Press the Config Data soft key, and enter the access code in the yellow message bar.
Attention!
To prevent setup parameters from being changed, remove this page from the manual after initial system setup.
Retain this information in a safe place for future use.
ACU-RITE MILLPWR
G2
vii
viii
Table of Contents
Controls of the MILLPWR
G2
Manual Information
MILLPWR
G2
Access Code
1.1 MILLPWR
G2
1.2 Operating in 2 Axes and 3 Axes Modes
ACU-RITE MILLPWR
G2
ix
1.3 Console
1.4 Operating Mode Screens
1.5 Accessories
2.1 Conventions
x
2.2 Manual Machine Positioning
3.1 DRO Manual Data Input
3.2 Calculator
4.1 Tool Table
ACU-RITE MILLPWR
G2
xi
4.2 Tool Data
Teaching Tool Length Offsets in the Tool Table ............................................... 48
5.1 Programming Introduction
5.2 Program Mode Functions
5.3 Creating programs overview
xii
6.1 Conversational Programming
G2
Program ....................................................................... 85
6.2 Folders
(MPT) Program ............................................................ 93
ACU-RITE MILLPWR
G2
xiii
Starting or Stopping a G-code Program ........................................................... 96
Additional G-code Conventions for MILLPWR
............................................ 104
7.1 Demonstration Program
Tool Change for the Rectangular Pocket ........................................................ 120
Programming the Rectangular Pocket ............................................................ 121
xiv
8.1 Milling and Drilling
Changing to a Tool of unknown length in DRO mode .................................... 129
Changing to a Tool of unknown length in a program ...................................... 131
8.2 Additional Milling Functions
Tool Path Description for Custom Pocket, and Islands................................... 163
ACU-RITE MILLPWR
G2
xv
9.1 Setup
10.1 Updating System Software
11.1 MILLPWR Off-Line Software
xvi
Introduction
2
1.1 MILLPWR
G2
The ACU-RITE MILLPWR
G2
control is a workshop-oriented contouring control that enables you to program conventional machining operations right at the machine in an easy-to-use conversational programming language. It is designed for milling and drilling machine tools, with up to 3 axes.
MILLPWR
G2
was developed to satisfy the wants and needs of tool and die makers and other machinists where manual and automated operation are both useful and needed. MILLPWR
G2
will enable you to maximize your throughput by significantly reducing set-up time, scrap, and other non-productive operations, thereby increasing your efficiency, productivity and profitability.
The MILLPWR
G2
has many powerful features that will improve your productivity. The screen layout is clearly arranged in such a way that the functions are easy to access, fast and user friendly.
MILLPWR
G2
is a closed-looped system with positioning feedback provided by ACU-RITE precision glass scales (1µm/0.00005" resolution). MILLPWR
G2
also includes Position-Trac™, an advanced, unique feature that enables you to easily, quickly and accurately re-establish work piece zero after shutting down, or power loss.
ACU-RITE conversational, and G-code format
The ACU-RITE conversational programming format is a method of writing programs; g-code (ISO) programming can be used, and run, but can not be edited. Preview graphics in the editor illustrate the individual machining steps for programming the contour as well as the corresponding tool path generated. A production drawing does not need to be dimensioned for NC programming, the MILLPWR
G2
can be programmed using the dimensions directly from the production drawing. The programming format is the same as used in previous
MILLPWR products. Always verify old programs before machining with MILLPWR
G2
.
1 Introduction
Powering Up
The MILLPWR
G2
console does not disconnect the power supply to the spindle motor. It can only be disconnected by turning off the main power supply.
Turn the power switch On [1], (to the I position) on the MILLPWR
G2 console which is located on the back of the unit.
Follow the builder’s instructions to turn off the machine.
The start up screen with 3 soft keys will be displayed; Shut Down,
Find Home
, and Cancel. After pressing either the Find Home, or
Cancel
soft key, the default DRO screen will be displayed.
It is strongly recommended that the MILLPWR
G2 performs the Find Home feature at start up, prior to any other action taken.
If a program was loaded when the MILLPWR
G2
was shut down, that same program will be reloaded when the unit is powered up again.
If the MILLPWR
G2
did not perform the Find Home feature at start up, press the Datum soft key from the default DRO screen to display the Home soft key. Press the Home soft key then the Find Home soft key will be displayed.
ACU-RITE MILLPWR
G2
3
E-STOP and Shutdown
The E-STOP is used for emergency program shut down by turning off the servo motors. It does not shut down the spindle motor. The spindle motor must always be manually stopped using the spindle switch to stop the motor, and the cutting tool.
When the E-STOP button is pressed, the servo motors are stopped, and the quill can be raised.
When the STOP key is pressed once, the servo motors pause, but are still active. All axes are locked, and can not be moved.
The program can now either continue by pressing the
GO
key, or stopped by pressing the STOP key a second time.
If the STOP key is pressed a second time canceling the program, the spindle motor must be stopped, and the tool raised before moving any of the remaining axes.
Shutting down the MILLPWR
G2
system is done by using the Shutdown soft key.
Press the Shutdown soft key to shut down the
MILLPWR
G2
system. This soft key is available in both
DRO
and PGM mode.
Confirm the shut down by pressing the Yes soft key.
Press the No soft key to cancel and exit the shut down procedure.
Always shutdown the MILLPWR
G2
before turning power off to the machine. Refer to the builder's instructions for for additional information on turning power off.
4
1 Introduction
Emergency Stop (E-STOP)
Press E-STOP to take all axes servos offline. This ends all machine movement, and allows the quill to be raised to move the tool out of the way.
To reset the E-STOP, turn the rotary switch clockwise in the direction of the arrows. The switch pops outward, and is reset.
Resetting E-STOP does not reactivate the servos.
Activating/Resetting the Servos
For safety reasons, the mill powers up with the servomotors disengaged. While the servos are disengaged the mill axes cannot move under servo power. The axes can be manually positioned if necessary.
Reset the servos as follows:
If a limit switch disengaged the servos, manually reposition the machine inside its normal range of travel.
If a miscount occurs, press the Find Home soft key to reset the servos and return all axes to their home position.
ACU-RITE MILLPWR
G2
5
Find Home
You should find home before a program is run, or immediately after startup.
During start up, the Find Home soft key is provided on the start up screen soft key area.
If the find home step is not performed at initial start up, it can be initiated at any time during operation. Press the Datum soft key, then press the Home soft key, and then press the Find Home soft key.
A 3 axes system will move the table and quill. They will automatically move a few inches along the Z, Y, and then X to find home. If a W axis exists (i.e. coupling knee to quill) then the control will prompt you to move the W manually to home it.
A 2 axes system will move the table. The table will automatically move a few inches along the Y, and then X to find home. Then the control will prompt you to move the Z quill manually to home it. If a
W axis exists (i.e. coupling knee to quill) then the control will prompt you to move the W manually also to home it.
Before finding home with a 2 axes system, the quill must be fully raised first.
When finding home, the MILLPWR
G2
will use (on machines equipped with ACU-RITE glass scales), the Position-Trac™ distance-encrypted reference mark line pattern. This line pattern allows MILLPWR
G2
to accurately find home and re-establish workpiece zero from any position.
Finding home applies to the X, Y, Z, and W axes.
Position-Trac will accurately re-establish workpiece zero after power loss, or shut down. After home has been found, the tool’s position
(relative to the most recent datum set) will be displayed.
Not finding home before moving the table will risk exceeding the table's travel limits, and possible damage to the machine, and the MILLPWR
G2
system.
Programs will not be allowed to run if the homing process does not complete successfully.
6
1 Introduction
Disengage Z Axis feature
MILLPWR
G2
provides the flexibility to switch between 2 axes and
3 axes operation.
Disengaging the Z axis drive:
Leave the Z BEGIN field blank when programming a step, or a one time milling operation.
Raise the quill, then loosen the quick release knob [1] on the front of the the Z axis drive system.
When a program step, or milling operation is then performed, the operator is prompted to manually position the quill.
Re-engaging the Z axis drive
Raise the quill handle to seat the ball screw into the nut block (e.g. this would be similar to hitting a dead stop).
Tighten the quick release knob [1].
ACU-RITE MILLPWR
G2
7
Writing Programs
Overview
The MILLPWR
G2
allows many features to be used without having to write a program. For operations that repeat, or complex machining it is best to write a program. Before writing a program, determine the work-holding device and the location of Part Zero (the point to which all movement is referenced). Since absolute positions are defined from Part Zero, try to select a location that directly corresponds to dimensions provided on the part print, such as the lower left corner of the work. Then you can develop a program. The following is a general approach to programming:
First, select the unit of measurement (Inch/MM) using the MM key.
This will place the DRO in the required unit of measure, and all dialogues will use the selection. If the selection is changed after data has been entered, the MILLPWR
G2 will convert the data to the new unit of measure.
The first step in a program selects the tool that is to be used. It’s size can be entered in either Inch or MM regardless of the unit of measure selected in the DRO. The Tool dialogue provides fields for data input for the tool position. This is a tool change position, a location away from the work area where the axes can return for safe tool changing. TOOL POSITION will use the unit of measure that has been selected for the DRO.
The remaining steps in the program describe the required moves, single cycles, and Tool changes to complete the machining.
The next to the last step in the program returns the axes to the Tool change position and ends the program.
After writing a program, verify it. Run it to troubleshoot for errors.
Verify that all programmed moves are safe, and accurate to the part print dimensions.
Setup the work piece into the intended holding device.
First run the program in Single-Step Mode to verify that both the program and the setting of Tool Offsets are correct. Single-Step
Mode allows you to run the program step-by-step. Make any necessary corrections. Once verified, the program can be run in
Auto Mode.
When the finished program is ready for production, back it up on a
USB memory device.
If there is an interruption to the power supply, the program is not lost. The program is periodically saved. Verify that the most recent steps (prior to the power failure) are in the program. The fixture zero location is also remembered.
8
1 Introduction
1.2 Operating in 2 Axes and 3 Axes
Modes
Overview
The MILLPWR
G2
is capable of running a 2 axes machine (manual Z) or a 3 axes machine with the Z being switched to manual as needed. This
User's Manual covers 2 axes and 3 axes operation. This section provides some general guidelines. In 2 axes mode, all Z moves must be made manually.
When running a program, the system will pause and provide a prompt whenever a Z move is required.
The incremental DRO display will show the distance to the Z axis target position.
Press the ABS/INCR key to toggle between absolute and incremental display modes.
In incremental mode, a bar graph is displayed below each axis position. A small blue indicator moves toward the center of the bar as the incremental position approaches 0. When at 0, the blue indicator will be centered.
After moving the Z axis to the programmed position, press the GO key to continue running the program.
Program Steps in 2 Axis Mode
When running a program step in 2 axis mode, not all information in the program step is used. Values may be programmed for Z Pass, Z Peck, and Tool Retract, but they will not be used when running in 2 axis mode.
When prompted to set Z, the incremental display will show the distance to the Z end depth.
After drilling to depth, raise the quill and press the GO key to continue running the program.
For pocket steps, raise the quill and press GO when prompted.
If an additional pass is needed for a step, press STOP to end the program and run the step again.
It may also be necessary to repeat a set of steps for each pass in a program.
ACU-RITE MILLPWR
G2
9
Selecting 2 Axis Mode on 3 Axis Systems
To run a program in 2 axis mode, disengage the quill assembly before pressing the GO key.
A prompt will appear indicating that the quill is disengaged.
If this is intentional, press GO and the program will run in 2 axis mode.
To program a specific step to run in 2 axis mode:
Select POSITION for the Z operation type (drill steps).
For pockets, clear the Z begin depth field.
When the step is run, the Z axis servo motor will be turned off to allow manual movement.
Table.
10
1 Introduction
1.3 Console
Operating Console
The ACU-RITE MILLPWR
G2
Console has a 12.1-inch Flat-Panel Color
Screen Display. The following list of items are located on the front panel.
See "DRO display screen" on page 21 for mapping information of the
start up screen.
See "Console Keypad" on page 20 for a full description of the console
keypad layout. The individual keys are fully described on page ii of the inside front cover.
The following features are located on the front panel of the console:
1
Color flat panel screen display.
2
Emergency “E” Stop
3
Soft keys
4
Power On indicator light / Error indicator light
5
Potentiometer for feed rate override
6
Go, Pause/Stop, Navigation keys, and Move Table keys
7
Axis keys
8
Console keypad
9
USB Port
See "Calculator" on page 18 for a full description of the calculator
keypad.
Rear Panel
The ACU-RITE MILLPWR
G2
DRO rear panel has the following list of items located on the panel.
1
Power switch
2
Power connector
3
Servo Power connector
4
Earth (ground) terminal
5
Ethernet port
6
USB port
7
KT 130 Edge Finder
8
Pendant (Remote switch)
9
RS-232-C connector
10 Auxiliary Machine Interface (AMI); for future expansion.
11 Servo connector (X, Y, and Z)
12 Grounding Edger Finder
13 Encoder Inputs (W and Z axis)
ACU-RITE MILLPWR
G2
11
Screen Navigation
The MILLPWR
G2
display layout changes between DRO Mode and
PGM
(Program) Mode by pressing the DRO/PGM key. The following illustrates the differences between the two screen modes.
DRO Mode display
In general, the display changes as different functions are activated.
Soft keys in the lower display area change per the function selected.
Soft keys perform their associated function by pressing the key directly below it. Basic procedures and features remain the same regardless of which mode is selected. For a complete description of
the display areas see "DRO Screen" on page 31.
1
Status Bar display for Servo Motor Status, Feed rate, Tool,
Datum, Scale, Skew, (Inch/MM), Estimated Time, Part Clock,
Parts (run), Job Clock, and Time of Day. See "Status Bar Display" on page 32.
2
Axes Display (current position).
3
Operator Intervention Message line (OIM).
4
Soft keys display area.
5
Dialogue box display area for milling functions.
PGM Mode display
When PGM mode is selected, the display changes from DRO mode to display program functions and graphics. Soft keys change to programming functions. All soft keys are run by pressing the
corresponding hard key located directly below it. See "Status Bar
Display" on page 32 for complete descriptions.
1
Status Bar display for Servo Motor Status, Estimated Time, Tool,
Datum, Scale, Skew, (Inch/MM).
See "Status Bar Display" on page 32.
2
Display window of graph simulation.
3
Operator Intervention Message (OIM).
4
Soft keys display area.
5
Program name.
6
Program steps.
12
1 Introduction
Dialogues, and Drop Down Menus
This manual provides complete information where specific examples of actions are being explained.
As a general overview of the dialogues provided by the MILLPWR
G2
, several fields are likely to be provided for input. To navigate a dialogue, use the ARROW keys to select the desired field. After entering the data into a field, press either the ENTER key, or the UP or DOWN ARROW keys to move to the next field. Exiting a field with one of these key methods will retain the entered data in that field.
When the required data has been entered, press the USE key to accept the data entered for use in that specific function.
Most dialogues contain Drop Down menus. Specific milling functions may require additional information. The choices available are provided in a drop down menu. In most cases, they are also provided as soft keys. The choices can be selected from either location.
Operator Prompts
For actions that require immediate input to continue the operation an operator prompt will be displayed by the MILLPWR
G2
in the message bar. The required data can be entered with the numerical keypad, and in some instances using the alphanumeric on screen keyboard.
Cursor
The MILLPWR
G2
uses a highlighted cursor to mark a field for selection or editing. In some instances, the cursor will default to a field without highlighting the field. Use the ARROWS keys to move the cursor. The UP, and DOWN ARROWS move the cursor through the fields available. The
RIGHT
ARROW will open a field that contains more choices, or subfolders in the folder tree. The LEFT ARROW will close the menu, or subfolders.
The cursor will also change from a highlighted bar to a text cursor when a field selected is having data entered.
ACU-RITE MILLPWR
G2
13
General Operating Guidelines
General operating guidelines for the MILLPWR
G2
.
Additional operation soft keys are located in the soft key area along with task selection, and dialogue. The soft keys change in relation to the task being performed.
Selection of a particular soft key that requires additional information may open a popup menu [1].
A soft key may open a dialogue menu that requires input necessary to continue with the operation selected.
The status bar in the top of the display is constant, and reflects only what has been selected for the current program.
Use the Context Sensitive Help (INFO key) feature when assistance is desired. This is an intuitive feature that aids the user by going directly to the section in the manual in relation to the feature, or key that has been selected to obtain assistance with.
14
1 Introduction
Operating Modes
The MILLPWR
G2
has two main operating modes: DRO, and PGM
(Program). These are accessed from the front panel hard key. This is a toggle key.
DRO
mode shows the current position of each axis relative to current datum. In DRO mode, manual machining, and Single Cycles can be performed. Tool selection, units, along with most setup features can be accessed.
Program mode PGM, displays the list of program steps and part-view graphics. New programs can be created as well as editing existing programs.
Programs, new or existing, can be saved, deleted, or copied using program functions.
A USB pointing device e.g. mouse, trackball, etc. may also be used.
If a pointing device is being used, the action of clicking on a soft key button is the same as pressing the corresponding soft key. A USB keyboard can also be used for data entry and cursor control.
ACU-RITE MILLPWR
G2
15
Popup Menus
Within the soft keys, additional features may be available in program mode. A soft key that has a down arrow in the lower right hand corner indicates that additional soft keys are available for that feature.
As an example, pressing the Program Steps soft key (in PGM mode) opens another set of soft keys available for this function. Then you will notice an up arrow on most of the soft keys. This indicates a popup menu will open when that key is pressed.
Soft keys for PGM provide access to edit existing programs, or create a new program. Sub menus provide dialogue for machining operations such as milling a line, an arc, engraving, drilling and creating pockets.
Pressing the required operation step soft key will open a popup menu to further define the machining operation required.
A selection for a popup can occur in one of two ways:
Use the shortcut number to the left of the feature; for example, pressing 9 on the numeric keypad will select the Circle Ring dialogue.
Or use the Up and Down arrow keys to highlight the feature to be used, then press ENTER.
When the type of machining operation has been selected, the corresponding dialogue opens so that the required data can be entered.
A dialogue in DRO mode will retain the previous data entered making it possible to re-run the previous operation without having to re-enter all the data.
At anytime when entering data into a dialogue the calculator can be accessed by pressing the CALC key.
Soft keys for CALC provide access to additional math functions such as trig functions.
When a dialogue is activated, it is not possible to change to another dialogue. The current dialogue must be exited by pressing USE to save the data in the dialogue or pressing
CANCEL
to discard the data.
16
1 Introduction
Keyboard
An on screen QWERTY keyboard will automatically popup when you enter a field that requires text information input.
The keyboard becomes visible (popup) when text, and numerical information is required for an action (e.g. saving a program, or entering text for engraving).
Use the ARROW keys for navigation of the cursor to go to the desired character and press ENTER to select the character.
When the information has been entered using the keyboard, press the Save soft key. The keyboard will disappear from the screen. The keyboard will also be removed from the screen when the CANCEL key is pressed.
When using a USB keyboard, the on screen keyboard can be disabled by pressing the Keyboard soft key. The on screen keyboard will remain disabled untill it is enabled by pressing the Keyboard soft key again. When the console goes through a power cycle, the key board will retain its setting prior to the power cycle.
Special Characters
The keyboard also provides a “Special Characters” display which is accessed by the “(#*\!...” key.
Arrow over to the “(#*\!...” key to highlight the key, and press the the ENTER key.
Navigational Soft keys
The following navigational soft keys are always available on the keyboard.
The “Up Arrow” key switches the keyboard from upper to lower case letter mode, or from lower to upper case letter mode depending on the current keyboard mode.
The “Abc” key switches the keyboard from the special character key mode to the alpha numeric key mode.
The “(#*\!...” key switches the keyboard from the alpha numeric key mode to the special character key mode.
ACU-RITE MILLPWR
G2
17
Editing Keys
The following keys are available for editing text on the keyboard.
The Copy key will copy the highlighted text in the text field.
The Paste key will paste to the text field text that was previously highlighted, and copied.
The Clear key will remove all text in the text field.
The back space key will delete text in the text field one character at a time.
Calculator
Numeric Keypad
The numeric keypad on the front of the console resembles a standard calculator with keys for numbers 0 through 9, four math function symbols (+, -, x, and ÷), a decimal point, and a positive/negative sign
(+/-).
The calculator is accessible from nearly any screen or field. Press the CALC key to access the “stand-alone” calculator. The math function soft keys are displayed in the soft key area. Calculations can be entered directly into a highlighted field.
Using the calculator in an entry field in a dialogue requires the operator to press the ENTER key to run the calculation.
To move to the next field using the ENTER key requires the operator to press ENTER a second time.
Anytime data is entered into an entry field in a dialogue and the value is changed using the +/- key, the operator is required to press the ENTER key to use the value change.
Moving to the next field using the ENTER key requires the operator to press ENTER a second time.
18
1 Introduction
Context Sensitive Help
The MILLPWR
G2
uses an intuitive method to aid the user when assistance is required. When assistance is needed with a feature, the
User Manual can be displayed directly at the point which describes the feature.
To use this help, in this example, the console is in PGM mode, and a
Linear Engraving cycle is being programed. It is desired to see descriptions of the cycle parameters, and the cycle itself. The following steps describe the actions needed to take.
Using Context Sensitive Help
Press the INFO key to open the on screen User
Manual.
This will display a new window containing the section in the User
Manual, opened directly to the description of the desired feature.
This is the active window when Context Sensitive Help is activated.
To activate the Contents View on the left side of the display, press the Contents View soft key. This allows the user to see all available topics from the User Manual. The Forward and Back soft keys will navigate the users previous history. The Previous Topic and
Next Topic
soft keys will select the previous and next topic in the manual contents (shown in the Contents View on the left hand side).
These soft keys allow the user to select other sections of the User
Manual while in Context Sensitive Help. Using these keys will navigate the User Manual even if the Contents View is hidden.
The following describes the action, and use of the soft keys:
The Back soft key navigates one page back per key press to a previous page that was viewed from the history. History is not cleared when the Help Screen is exited.
The Forward soft key navigates one page forward per key press from the viewed pages in history.
The Previous Topic soft key navigates one Topic up in the contents window per key press.
The Next Topic soft key navigates one Topic Down in the contents window per key press.
The Contents View soft key is a toggle key to show/ hide the contents view on the left hand side of the display.
To close, press the Exit soft key.
ACU-RITE MILLPWR
G2
19
Console Keypad
The following keys are located on the console keypad. There is also a quick reference guide located at the beginning of this manual on page ii of the inside front cover.
1
Axis keys, use to select the required axis.
2
Numeric keys, use to enter numeric data.
3
CANCEL
key, use to cancel current action.
4
CLEAR
key, use to clear selections such as values entered in a field.
5
ARROW
keys, use to navigate around the screen, and highlight dialogue fields. Also used to move the table axes.
6
STOP
key, use to pause, or stop a program that is running, or a machine operation.
7
GO
key, use to start, or resume a program.
8
USE
key, use to complete an operation, i.e. data values entered in a dialogue.
9
ENTER
key, use to activate selections, and entries.
10 +/- key, use to toggle key for “Plus/Minus” data entry.
11 CALC key, opens the fully functional calculator.
12 Function keys, select appropriate key for quick access to the
function and data entry.
13 Milling function keys. Selection of appropriate key provides direct
access to the milling function dialogue.
20
1 Introduction
1.4 Operating Mode Screens
Display navigation
The DRO mode is the default start up mode, and PGM mode can be selected from the front panel key after start up. A condensed description of these has been provided here on how to navigate, and become familiar with the information that is being provided.
Complete descriptions, and details of these are provided later in this
manual, see "DRO Screen" on page 31.
DRO display screen
The MILLPWR
G2
display screen provides the information required to monitor the machine, it’s movement, programming, and more.
The default screen, or home screen, displays two main windows, and soft keys in the soft key display area. When the console is first turned
on, the unit defaults to this screen. See "Screen Navigation" on page
The DRO screen displays information per the current operation. DRO mode allows the use of the milling function keys, or can be used as a
DRO in manual machining operations.
The system Shutdown soft key is located here as well as in PGM mode.
ACU-RITE MILLPWR
G2
21
Program Display Screen
From the DRO mode, press the DRO/PGM key, and the display changes to program mode showing the currently selected or loaded program.
When Programing a job, the display activates a graphic view of the program. While the program is running, the operation that is being performed is graphically shown as well. The VIEW key provides features to configure the graphic area.
For more information, see "Program Function Screen" on page 55.
1.5 Accessories
Electronic Edge Finder
The Electronic Edge Finder KT 3D enables the ability to teach positions, find the center point of a circle, or locate datum (work piece zero) by touching off on the part. Advantage of an electronic edge finder is that it instantly senses when contact is made with the point
(even if the axis over traveled).
22
1 Introduction
Machining
Fundamentals
2.1 Conventions
Axis Conventions
Count Direction
When programming a part using MILLPWR
G2
, table movement and tool movement are determined by the use of positive or negative numbers. MILLPWR
G2
has been factory set with the following positive and negative count directions for the X, Y and Z-axes:
X axis
The table will move to the left and the tool will move to the right for a positive count direction.
Y axis
The table will move toward you while the tool moves away from you for a positive count direction.
Z axis
The quill will move up (away from the table surface) for a positive count direction.
Cartesian Coordinates
A cartesian coordinate is a position that can be measured from the
X- and Y-axes.
Polar Coordinates
A polar coordinate is a position that is defined by an angle and a radius.
24
2 Machining Fundamentals
Absolute and incremental work piece positions
Absolute work piece positions
Absolute coordinates are position coordinates that are referenced to the datum of the coordinate system (origin). Each position on the work piece is uniquely defined by its absolute coordinates.
Example 1: Holes dimensioned in absolute coordinates
Hole 1
X = 10 mm
Y = 10 mm
Hole 2
X = 30 mm
Y = 20 mm
Hole 3
X = 50 mm
Y = 30 mm
Incremental work piece positions
Incremental coordinates are referenced to a previous step within the program, which serves as the relative (imaginary) datum. When you write a part program in incremental coordinates, you thus program the tool to move by the distance between the previous and the subsequent nominal positions. Incremental coordinates are therefore also referred to as chain dimensions.
Example 2: Holes dimensioned in incremental coordinates
Absolute coordinates of hole 4
X = 10 mm
Y = 10 mm
Hole 5, with respect to 4
X = 20 mm
Y = 10 mm
Hole 6, with respect to 5
X = 20 mm
Y = 10 mm
ACU-RITE MILLPWR
G2
25
Setting the datum
Overview
Datum is the workpiece zero or absolute zero, and is a point of reference that the MILLPWR
G2
bases all of the part's coordinates from.
A datum must be established for every job. Datum's location may be indicated on the print; or the operator may establish a datum that allows most of the part's dimensions be entered directly using the least amount of calculations.
When establishing datum, it may be easiest to locate a known point on each axis, such as the corner of the part, or a location on a vise or fixture.
Datum can be set at a point on the top surface, a position beneath the surface, or at a point where there's no material present (such as in the center of a circular part). Touching off the edge of a work piece using
a tool, or an edge finder can be used when establishing a datum. See
"Steps to Establish the datum" on page 80.
26
2 Machining Fundamentals
2.2 Manual Machine Positioning
Move Table
Non Cutting Mode
You can make or change jog moves when in DRO mode with the servos on.
Jog Mode Description
Rapid
Default rapid speed for continuous jogs. Use arrow keys. Actual speed determined at machine setup, and can be over ridden using the potentiometer.
Jog: 0.1
Jog: 0.01
Conventional Jog increment set at 0.100”.
Conventional Jog increment set at 0.010”.
Jog: 0.001
Conventional Jog increment set at 0.001”.
In mm units the jog increment is 20 microns, 200 microns and 2000 microns respectively.
Changing the Mode
Jog move modes are performed at the currently active feedrate. The active Jog is selected by pressing the appropriate soft key, then pressing the appropriate ARROW key to move the table in the direction required. The up and down arrows move the table in the Y axis. The left and right arrows move the table in the X axis. Use the soft keys
Move Z Up or Move Z Down to move the Z axis in the desired direction.
Incremental Moves
In DRO Mode, Press the MOVE TABLE soft key.
Then select the soft key Jog increment required. Then press the arrow keys (for X and Y) or the soft keys for Z. One jog increment is moved per arrow key press.
Continuous Moves
To manually position the machine using continuous movement, press the Move Table soft key. Make sure none of the incremental
Jog keys are highlighted.
Press the appropriate ARROW key (or soft key) to move the table in the direction required for the axis move. The table will move at the currently active jogging speed. The table will move until the arrow key is released.
ACU-RITE MILLPWR
G2
27
Preset Moves
To access the PRESET dialogue in the MILLPWR
G2
, take the following steps:
Press the DRO/PGM key on the front panel to place the
MILLPWR
G2
in DRO mode.
Press the ABS/INCR key on the front panel to place the
MILLPWR
G2
to INCR.
Press the Preset soft key to open the PRESET dialogue.
Press the X=0 soft key to zero the X axis.
Press the Y=0 soft key to zero the Y axis.
Press the Z=0 soft key to zero the Z axis.
With the values entered for X, Y, or Z, press the USE key to move the table or quill.
Press the CANCEL key at any time to cancel and exit the
PRESET dialogue.
Adjusting the Feedrate
The Feedrate Override rotary switch can be used to override the currently active feedrate or rapid rate for machine moves. The switch provides a range of 0% to 150%. Setting the switch to 100% will allow the actual feedrate or rapid rate currently active to be used.
The machine builder determines the default rapid rate and maximum feedrate at setup. If the MILLPWR
G2
is shut down, the configuration file reloads these default rates at the next power up.
28
2 Machining Fundamentals
DRO Mode and
Calculator
3.1 DRO Manual Data Input
Overview
The MILLPWR
G2
is in either DRO mode or PGM mode. DRO mode allows data input for short one step machining operations. Manual operation, single step operation, and single commands can be entered. DRO mode
also allows the running of programs; See "DRO Operations" on page
The following describes the concepts, and formats used with the
MILLPWR
G2
which are being introduced in this chapter.
DRO Screen
Status Bar Display
Move Table
Milling Functions
Zeroing an Axis
Teach Position
Electronic Edge Finder
Skewing
Milling Function Keys
DRO Operations
DRO Mill Cycles
Calculator
30
3 DRO Mode and Calculator
DRO Screen
The DRO screen displays information per the current operation. The
DRO
mode allows the use of the milling function hard keys, or can be used as a DRO in manual machining operations.
viewed on the display in DRO mode.
When the console is first turned on, the soft keys Shut Down, Find
Home
, and Cancel are displayed.
Press the Find Home soft key.
After pressing either the Find Home, or Cancel soft key, the default
DRO screen will be displayed.
If the MILLPWR
G2
did not perform the Find Home feature at start up, press the Datum soft key from the default DRO screen to display the Home soft key. Press the Home soft key then the Find Home soft key will be displayed.
1
Status Bar displays the servo motor status Stop/Run/Pause, feedrate override, current Tool (blank if none is selected), Datum,
Scale, Skew, unit of measure selected (Inch/MM), Estimated
Time, Part Clock, Parts (run), Job Clock, and Time of Day.
See "Status Bar Display" on page 32
2
Display current position of each axis, and relative to the current datum.
3
Operator Intervention Message line (OIM) that provides prompts, and messages to the operator.
4
Soft keys display. The soft keys change per the function that has been selected. Each are activated by the associated hard key that is directly below it. When a soft key appears as being pressed, it is activated. If the key is not pressed in, it is not currently active.
Active soft key text changes to yellow text.
5
This window displays program steps if a program is loaded. If no program is loaded, then this window is blank. When a function has been selected (e.g. Pocket), its dialogue box is displayed in this window.
ACU-RITE MILLPWR
G2
31
Status Bar Display
Status Bar
Display
Program
State
Feed
Tool
Description
This field indicates the program state: Stop when program is not running, Run when program is running, or Pause when program is paused for operator.
This field indicates the current feedrate of the table or quill.
In DRO mode, this field indicates the current tool selection. In PGM mode, this field indicates the programmed tool for the highlighted step.
This field indicates the active Datum number.
This field indicates the active Scale factor.
Datum
Scale
Skew
Units
This field indicates the active Skew angle.
This field indicates the active display units. All dimensions are displayed in these units (inch or mm). The current feedrate is displayed in these units (inch or mm per minute).
Estimated
Time
This field indicates the estimated machining time for the active program. This time assumes the program runs at 100% of the programmed feeds. It does not include the time necessary to perform manual operations such as changing a tool.
Part Clock
This field shows the cumulative running time of the current program. The timer is reset when a program is loaded.
Parts
Time of
Day
This field shows the number of times the current program was run to create a part.
Job Clock
This field shows the total elapsed time for the current job. This timer is started and stopped by the operator.
This field shows the current time.
32
3 DRO Mode and Calculator
Move Table
The Move Table soft key when pressed will turn on the servo motors.
Pressing it again will turn the servo motors off.
The desired feed rate can be set, or it can be left at 100% for rapid
feed rate. See "Adjusting the Feedrate" on page 28.
To move the table in increments, first select the soft key increment wanted (e.g. 0.001, or 0.01, or 0.1).
A 3 axes system allows the Z axis to be moved by selecting the soft keys Move Z Up, or Move Z Down.
A 2 axes system requires the Z axis to be moved manually.
A 3 axes system allows the X, Y, (and Z) axis can be moved simultaneously by pressing the desired direction ARROW hard keys at the same time.
A 2 axes system allows the X, and Y axis to be moved simultaneously by pressing the desired direction ARROW hard keys at the same time.
Always fold in the table crank handles before moving the table using the servos.
The axis move one increment per key press when using step increment. The axis moves continuously until released when using continuous jog.
Milling Function
One Step Milling function may also be referred to as Single Cycle milling functions. Most milling functions can be used as one time machining operations as well as for programming. The BLEND key does not support single operation. Each milling function will either open its own dialogue or allow selection of choices from a soft key popup.
These milling function keys are described in more detail later in this chapter.
ACU-RITE MILLPWR
G2
33
Zeroing an Axis
Pressing the Zero X, Zero Y, or Zero Z soft keys will zero the incremental position for those axes.
A datum must be set to establish the point from which all absolute dimensions are based.
Teach Position
Whenever X, Y or Z coordinates are being entered, the Teach Position soft key will appear, enabling MILLPWR
G2 use the current coordinate(s). MILLPWR
to be in teach mode and to
G2
will base each coordinate on the current absolute position, and enter that position into the field that is highlighted.
While programming, the MILLPWR
G2
can switch between the DRO and PGM screens without losing the program that is either being created, or being edited.
To teach the MILLPWR
G2
a coordinate (while programming a milling function e.g. Rectangle Pocket):
Use the arrow keys to highlight the X, Y, or Z axis fields.
Move your tool, indicator, or electronic edge finder to the position you want to teach.
Press the Teach Position soft key to enter that location then press the ENTER key.
The numeric keypad, and calculator functions can be used to adjust the number.
Repeat the steps for each axis and each location that will be used to teach the MILLPWR
G2
.
Press USE to accept the dialogue or press CANCEL to cancel the dialogue.
34
3 DRO Mode and Calculator
Electronic Edge Finder
A HEIDENHAIN Electronic Edge Finder enables you to teach positions, find the center point of a circle, skew a part or locate datum
(also referred to as workpiece zero) by simply touching off on the part.
The advantage of an electronic edge finder is that it instantly senses when you’ve made contact with the point even when you over-travel.
MILLPWR
G2
lets you define the diameter and unit of measure for an electronic edge finder. Once this information has been entered,
MILLPWR
G2
will automatically compensate for the radius of the tip of the electronic edge finder when performing any of the operations mentioned above.
To teach a coordinate with the edge finder, highlight the appropriate field then slowly move the table (1in/min) until the electronic edge finder touches the workpiece. When the electronic edge finder touches the part’s surface, the coordinate will appear in the field. The electronic edge finder is active whenever an entry field is highlighted.
ACU-RITE MILLPWR
G2
35
Skewing
The skew function automatically compensates for the offset angle of the part when it is not perfectly parallel with either the X or Y axis.
Press the DRO/PGM key to place the MILLPWR
G2
in
DRO mode.
Press the ABS/INCR key to place the MILLPWR
G2
in
ABS mode.
Press the Datum soft key to open the SET DATUM dialogue.
Enter the Datum Number in the DATUM NUMBER field.
Enter the Skew Angle in the SKEW ANGLE field.
Press the CANCEL key at any time to cancel and exit the
SET DATUM dialogue.
Each datum has its own skew angle. When a new datum is selected, that datum’s skew angle will be used.
To compensate for the skewed part, touch off on two or more points along one axis, either X or Y. Use an electronic edge finder or a mechanical indicator. At each point selected, press the Teach
Position
soft key to enter the data.
Always choose a line that you want to make parallel with the table’s X or Y axis, do not enter coordinates along a curve, along two different lines or along a line that’s positioned at a true 45 degree angle.
MILLPWR
G2
will calculate the skew angle based upon a straight line between the points you’ve entered.
If you’re working with a part that has a rough edge, it’s best to enter multiple points along the straightest edge so that MILLPWR
G2
can more accurately calculate the skew angle.
The skew feature does not work with G-code programs.
Remove any skew angle prior to running a G-code program.
36
3 DRO Mode and Calculator
Milling Function Keys
The following describes in general, the milling function keys.
Most milling functions can be used as one time machining operations.
The BLEND key does not support single operation.
Hard Key Function
TOOL
opens the SET TOOL dialogue where information regarding the tool can be entered.
RECT
opens the popup menu above the Rectangle soft key. Choose the type of rectangle milling that is to be done by selecting it from the popup menu. The required dialogue will open for that choice.
CIRCLE
opens the Circle popup menu above the
Circle
soft key. Choose the type of circle milling that is to be done by selecting it from the popup menu. The required dialogue will open for that choice.
HOLES
opens the popup menu above the Hole
Pattern
soft key. Choose the type of hole drilling that is to be done by selecting it from the popup menu. The dialogue where information can be entered to drill a row, frame array, or a bolt circle pattern will open.
POS
opens the POSITION / DRILL dialogue where information can be entered to move the table to a position in the X & Y direction.
LINE
opens the MILL LINE dialogue where information can be entered to mill a line.
ARC
opens the MILL ARC dialogue where information can be entered to mill an arc.
BLEND
opens the BLEND dialogue while in PGM mode where information can be entered to mill an arc, blending two surfaces together. Also used for chamfer.
ACU-RITE MILLPWR
G2
37
DRO Operations
The following explains a few of the machining operations that are available. This example is providing an overview to the operator of the
MILLPWR
G2
capabilities.
The RECT, or CIRCLE keys as an example access popup menus to further refine the type of milling to be completed. Selecting the type of milling operation required will open the dialogue for that type of milling operation.
An operation is run by pressing the USE key. The CANCEL key can be pressed at anytime to cancel an operation.
Rectangle milling
Press the RECT key on the front panel. The soft key is displayed, and a popup menu appears on the display listing the type of rectangles available for milling.
Rectangle milling example
(e.g. pocket, frame, face, or slot)
Select Pocket from the popup menu.
The popup menu disappears, and the RETANGLE POCKET dialogue is displayed.
Enter the data to mill the pocket.
An operation is run by pressing the GO key. While running a graphic representation can be seen by pressing the VIEW key. The STOP key can be pressed at anytime to pause, or stop an operation.
38
3 DRO Mode and Calculator
Circle milling
Press the CIRCLE key on the front panel. The soft key
CIRCLE
is displayed, and a popup menu appears on the display listing the type of circles available for milling.
Circle milling example
(e.g. pocket, frame, ring, or helix)
Select Pocket from the popup menu.
The popup menu disappears, and the CIRCLE POCKET dialogue is displayed.
Enter the data to mill the pocket.
Press GO to run the circle pocket.
ACU-RITE MILLPWR
G2
39
DRO Mill Cycles
The one step milling function are grouped in Four categories as shown in these groups.
Drill Cycles
Position
Row of Holes
Rectangular Frame
Rectangular Array
Bolt Circle
Rectangular Pocket Cycles
Frame
Slot
Face
Circular Pocket Cycles
Frame
Ring
Helix
Other one step milling features
Mill Line
Mill Arc
When a Milling Function key is selected for a single step operation, either a popup menu is displayed, or the available soft keys for that function are provided and its dialogue is opened. When a popup menu appears, further selection is required, then the dialogue is displayed.
The DRO screen is also displayed, showing the current axes location.
The RECT, CIRCLE, and HOLES keys, when selected, display a popup menu. These three keys provide additional selections to further specify the type of machining required.
Press the milling function hard key that is to be performed in DRO mode.
40
3 DRO Mode and Calculator
3.2 Calculator
Accessing the calculator
The built in calculator can be used for simple arithmetic, or other math functions. The calculator can be accessed at any time, during most operations.
To access the calculator press the CALC key, and select the calculator function to be used.
The following calculator soft keys are available:
Soft key Description
Sin
Trigonometric Sine function
Cos
Trigonometric Cosine function
Tan
Trigonometric Tangent function
Open Parenthesis (
Used as one of a pair to enclose a sum, or other expression.
Close Parenthesis )
Used as one of a pair to enclose a sum, or other expression.
Square
Number multiplied by itself
Square Root
Square root of a number
More Cmds
(see next soft key display area)
ACU-RITE MILLPWR
G2
41
More Commands, second menu.
Soft key Description
ArcSin
Inverse function of Sine
ArcCos
Inverse function of Cosine
ArcTan
Inverse function of Tangent
To exit the calculator press the CALC key a second time or press CANCEL.
Press the CLEAR key to clear the entry field.
Using the calculator to insert data
The calculator can be used in the numeric field of dialogues.
Example, Milling a circle pocket:
The radius of a circle is required in the data input field, and the part drawing provides a diameter dimension.
The diameter dimension can be entered into the dialogue field.
Make sure CALC has been pressed to activate the calculator.
Then press the Divide by key. The ( ÷ ) divide by symbol will appear in the field showing the calculation step.
Then press the 2 key. This will also appear in the field as part of the calculation steps.
Then press the ENTER key, and the result will be entered into the dialogue field.
Trig Functions
When calculating the Sine, Cosine, or Tangent of an angle, enter the angle first (in decimal degrees), then press the function soft key.
42
3 DRO Mode and Calculator
Tool Table
4.1 Tool Table
Overview
When the MILLPWR
G2
runs a program step that activates a tool, it only activates the diameter, and length values on that row of the Tool
Table. The tool number, or tool type are not activated in dialogues that have these fields. The tool type must be entered in the dialogue.
Tool Table values are automatically converted to their inch or millimeter equivalents when the MILLPWR
G2
mode is changed. All typed values must match the current unit mode of the MILLPWR
G2
.
Define and store up to 99 tools on the tool table. Type of data stored on the Tool Table is information specific to each tool. Diameter, and length offset are the only values used from the Tool Table.
The Tool Table can only be used with G-code programs.
Tool Compensation Required Data
You usually program the coordinates of path contours as they are dimensioned on the work piece drawing. To allow the MILLPWR
G2
to calculate the tool center path, e.g. the tool compensation, you must also enter the diameter of each tool you are using.
Tool data can be entered either directly in the part program or separately in the Tool Table. In the Tool Table, you can also enter additional data for the specific tool. The MILLPWR
G2
will consider all the data entered for the tool when running the part program.
44
4 Tool Table
Tool numbers / Tool names
Each tool is identified by a number between 0 and 99. The tool name is its tool number.
The tool number 0 is automatically defined as the zero tool (empty spindle) with the length L=0 and the diameter D=0.
Sign for the length difference
Δ
L
If the tool is longer than the T1 tool:
Δ
L > 0 (+).
If the tool is shorter than the T1 tool:
Δ
L < 0 (–).
The tool length offset can be entered as a known value, or use the
Teach
soft key. The MILLPWR
G2
can determine the offset automatically.
The tool length offset may be entered as a known value, or the
MILLPWR
MILLPWR
G2
G2
may determine the offset automatically. To have the
determine a tool’s length offset involves touching the tip of each tool to the part’s Z0 surface, and pressing the Teach soft key.
This provides information to the MILLPWR
G2
to determine the tool length offset for each tool.
Tool Diameter “D”.
Enter the tool diameter ”D” directly.
The Tool Table should not have any tool length for a tool that is not repeatable.
Locating the Tool Table
The Tool Table is accessed from the DRO setup screen.
To activate the tool table, press the SETUP key.
Then press the Tool Table soft key.
ACU-RITE MILLPWR
G2
45
Tool Table
Editing the tool table
When the tool table is open, a new tool can be added, or an existing tool can be edited by changing the existing information for that tool.
It is necessary to first select the unit of measurement before entering values into the tool table.
To enter a new tool, a blank numbered row will need to be selected.
Using the ARROW keys, highlight the next available blank row number.
Highlight the Diameter field, and using the numeric keypad, enter the tool diameter.
Press the ENTER key.
Arrow over to the next field and enter the tool Length if it is to be used.
Press the ENTER key.
Arrow over to the Type field and press the ENTER key. The Type is only for informational purpose.
From the drop down menu, arrow down to select the description of the tool that is being added (e.g. flat end mill).
Press the ENTER key.
Continue to add additional tools as necessary.
When all tools have been added, press the Exit soft key, or USE key to save changes to the tool table.
Press the Teach soft key. The MILLPWR
G2
calculates the tool length offset for the selected tool putting the data to the length column.
Additional data can be input such as Diameter Wear,
Length Wear and Plunge Angle. These fields are not required to use the tool selected. See the Tool Table
Structure on the following page.
46
4 Tool Table
Editing an existing tool
To edit an existing tool is similar to adding a new tool using the same dialogues.
Highlight the desired field of the tool to be changed.
Type in the new value, then press the ENTER key.
When all changes have been made, press the Exit soft key, or USE key to save changes to the tool table.
Only add the tool diameter and length if it is repeatable each time it is selected.
When running G-code programming, the tool length for each tool in the program is provided from the tool table. As an example, T1 M6 prompts the operator to load tool 1 into the spindle. The tool length and diameter offset are retrieved for tool #1 in the tool table, and used to adjust the tool path and Z axis position. This is repeated for each tool used.
Tool Table Structure
Tool table: Standard tool data
Abbr.
Tool
Inputs
Number by which the tool is called in the program (e.g. tool 2 = T2).
Diameter
Length
Type
Compensation value for the tool diameter D.
Compensation value for tool length L.
D. Wear
Tool type: A popup menu appears where you can select the type of tool being used.
Tool diameter wear value.
(Only used in G code programs)
L. Wear
Plunge Angle
Tool length wear value.
(Only used in G code programs)
Angle of plunge cut.
(Only used in G code programs)
ACU-RITE MILLPWR
G2
47
4.2 Tool Data
Tool-Length Offsets
Tool-length offset is the distance from Z0 Machine Home to the tip of the tool at the part Z0 (the surface of the work).
Tool-length offsets allow each tool used in the part program to be referenced to the part surface. In an idle state, the MILLPWR
G2
does not have a tool-length offset active. Therefore, Tool #0 (T0) is active.
When T0 is active, all Z dimensions are in reference to the Z Home position. When you program T1, all Z dimensions become referenced to the surface on which the tool-length offset of Tool #1 was activated.
For machines that do not have a Z axis automatic homing feature, you must set the Z0 position of the Z axis. Usually, it is the fully retracted
(Up) position of the quill or machine head. Tool-Length Offsets are referenced to this position.
Because tools differ in length, Z0 axis (Part Zero) is not set the same way as X0 or Y0. The tool-length offset is the distance from the tip of the tool to the top of the part. Enter a length offset for each tool in the
Tool Table.
With tool-length offsets active, the Z axis position display reads 0.00 when the active tool moves to Part Zero. Tool-length offsets simplify programming.
Teaching Tool Length Offsets in the Tool Table
The Tool Length Offset data is placed in the “Length” column in the
Tool Table.
Activate the Tool Table by pressing the SETUP key from
DRO
mode.
Then press the Tool Table soft key.
Select the tool number that is to be edited.
Use the arrow keys to highlight the “Length” column field.
With the tool in the spindle, move the tool down until it touches the top surface of the work piece. This is referred to as “Part Zero”.
Press the Teach soft key. The MILLPWR
G2
calculates the tool length offset for the selected tool putting the data in the length column.
48
4 Tool Table
Diameter Offset in Tool Table
When you activate a tool, you automatically activate the length offset and diameter values recorded on the Tool Table (DRO mode only activates a tool when GO is pressed). When a tool is activated, the length offset is applied immediately to provide an accurate Z axis position display.
The active diameter value is important when you program compensated moves and use cycles with built-in tool compensation.
If tool diameter is correct, compensated moves and cycles are performed accurately.
Enter tool-length offsets and tool diameter values on the numbered lines of the Tool Table. The numbered lines on the Tool Table identify the tool number (T-Code) that activates those values.
On machines equipped with collet-type tool holders, it is impractical to use the Tool Table to store tool-length offsets. You can set tool-length offset at tool change. Tool Table diameters are still required for compensated moves and when using cycles that have built-in compensation.
ACU-RITE MILLPWR
G2
49
Tool Radius Offset
Tool radius offset is available with the MILLPWR
G2
. The tool center moves in the working plane along the programmed path or to the programmed coordinates. When programming a part profile, the path of the tool is a half of a diameter away from the depth of the cut.
Offset the tool to the right-hand or left-hand of the cutting edge.
“Right” or “Left” refers to the side of the cutting edge to which the tool offsets. Program tool offset as Right or Left according to the desired cutting edge.
Moving without radius offset
The tool center moves in the working plane along the programmed path or to the programmed coordinates. Program tool offset as Center when no radius offset is needed.
Applications: Drilling and boring, pre-positioning.
50
4 Tool Table
Machining with radius offset
The tool center moves along the contour at a distance equal to the radius. “Right” or “left” are to be understood as based on the direction of tool movement along the work piece contour as viewed from behind a moving tool.
ACU-RITE MILLPWR
G2
51
Radius offset: Machining corners
Outside corners:
A programmed path around the outside corners on a transitional arc should have the feed rate at the outside corners reduced to relieve machining stress. Typical for any great changes of direction.
Inside corners:
The operator must program the MILLPWR
G2
for the intersection of the tool center paths at inside corners. From this point it then starts the next contour element. This prevents damage to the work piece.
The permissible tool radius, therefore, is limited by the geometry of the programmed contour.
Danger of collision!
To prevent the tool from damaging the contour, be careful not to program the starting or end position for machining inside corners at a corner of the contour.
52
4 Tool Table
Program Overview
5.1 Programming Introduction
Program Display mode
If the console has the Calculator active while in DRO mode, exit from
Calc by pressing the Calc key, returning the MILLPWR
G2
to DRO mode.
Program Functions can not be accessed when the
Calculator is active in DRO mode.
From DRO mode, press the DRO/PGM key, and the display changes to PGM mode. If a program is loaded, it will be displayed, otherwise the display screen will be blank.
The program display provides soft keys for program selection, creating, editing, and running functions. The Clear Program soft key will exit out of a current loaded program. The system Shutdown soft key is provided on the PGM mode display the same as it is on the DRO mode display. The Program Functions soft key provides access to program management features.
Display area
Programming functions, graphics, and soft keys are provided in the display area. Each soft key is activated by pressing the corresponding hard key located directly below it.
1
Status Bar displays the servo motor status Stop/Run/Pause,
Time, loaded Tool (blank if none is selected), Datum, Scale, Skew, and unit of measure selected (inch/mm).
2
Graphic display window of the current loaded program. If a program is loaded, a graphical simulation is shown.
3
Operator Intervention Message (OIM) provides prompts, and messages to the operator.
4
Soft keys display area. The soft keys change per the function that is selected. They are activated by the associated hard key that is directly below it. When a soft key appears as being pressed in, it is activated and its text is yellow. When a soft key is grayed out, it is not available for the current program function.
5
The name of the current loaded program is displayed above the program steps display.
6
The program display window displays the program steps of the current loaded program.
54
5 Program Overview
Program Function Screen
The Program Function screen displays several windows, and soft keys which are defined in the contents of this chapter. The display area window is briefly described in the following table. The Program
Functions
soft key provides access to Network or USB memory devices by pressing the Folder View soft key. The features of this soft key are explained on the following page.
Press the Program Functions soft key to access programs stored in the Console, on a Network, USB memory devices, or to create a new program.
The Program Functions screen displays all programs that are stored in a selected folder. The default storage folder for the console is v:\user\.
General Information and the programming steps of the highlighted program are displayed in the lower left window [3], for a quick access review. If a program has ran in its entirety (without errors), graphic preview [2] is also displayed.
1
Available soft keys.
2
Program graphic preview.
3
Program steps preview.
4
Current folder selected.
5
Constant status bar.
6
List of all the programs stored in the current location (or folder).
Folder View
The Folder View soft key includes additional access to the user. The
Folders Tree [9] is displayed which allows the user to access different folders, and narrow a search to selected program types.
Access to Network or USB memory devices is available in the Folders
Tree.
The Folder View soft key stays active until it is pressed again.
7
Displays the current program loaded.
8
Shows the type of programs being displayed (e.g. MILLPWR
G2
, or G-Code programs to be displayed; or DXF files.
9
The Folders Tree can be used when connected to a network, USB memory devices, or folder management.
The MILLPWR
G2
can save programs to a USB device, or to network drive (e. g. a PC) as well as to the MILLPWR
G2
User folder.
The internal memory of the MILLPWR
G2
is organized into a folder structure. The default folder is the User folder.
Programs can be stored in the User folder. Additional folders can be created to better organize programs.
Features in Program Functions allow for navigation of all folders, USB memory devices and network folders.
To return to the Program Display Mode:
ACU-RITE MILLPWR
G2
55
From Folder View, press the Folder View soft key to exit back to the Program Functions display.
Press the Exit soft key to exit back to Program Mode.
Program Drawing View
While a program is running (or being created), individual steps being performed are graphically shown as they are being ran or created.
Pressing the VIEW hard key displays different soft keys for viewing choices of the program. The VIEW key acts as a toggle switch, pressing it again will remove the view soft keys and return to the previous display. Pressing CANCEL or USE will also exit the view soft keys.
To activate the bottom menu soft keys for viewing choices, press the VIEW key. The view soft keys are
Soft keys that have a small arrow in the upper left hand corner indicates that a popup menu is available when the key is selected for additional choices.
To return to the previous display, press the VIEW key again, or the USE key.
If the CANCEL key is pressed, it will exit out of the view mode, and return to the previous display, but will not cancel out any view changes made.
56
5 Program Overview
Program Screen Display
When programming a machining step, the display changes according to the machining step selected. Once a machining step has been selected using the Program Steps soft key, the display will appear as shown here. The program steps display windows are described in the following table.
1
Current program steps.
2
Dialogue for a new milling step (e.g. CIRCLE POCKET)
3
Dialogue field graphic assistant. Graphic changes per input field illustrating information required.
4
Soft keys.
5
Program name. If an asterisk appears at the end of the name, it is indicating that the program has not been saved since its last edit.
Soft keys that have a small arrow in the lower right hand corner indicates that additional soft keys are available when the key is selected. Soft keys that have up arrow in the top left hand corner indicates that a popup menu is available when selected.
ACU-RITE MILLPWR
G2
57
Program Mode Soft Keys
When the DRO/PGM key is selected from DRO mode, the MILLPWR
G2 screen changes to PGM mode, and the program default screen is displayed.
When the MILLPWR
G2 is set to program mode, types of milling functions specific to the hard key selected become available as soft keys.
Keys Function
Program Functions
opens additional soft keys to
Load, Save, Clear, or Copy a program along with several other functions listed on the following page.
Step Functions
opens additional soft keys for modifying the program steps (e.g. reverse path, delete steps, ect.).
Program Steps
opens additional soft keys for programming, or modifying an existing program by adding addition milling functions (e.g. add a pocket, mill a circle, etc.).
Clear Program
will unload the current program when the Yes soft key is selected. The program is not saved. If any changes were made, they are lost.
Shutdown
will shut down the MILLPWR
G2
system.
Only then can power be turned off.
Save/Discard
opens a popup menu which provides the choice to either save the changes made to the program, or discard the changes by returning the program to its original state.
Run Options
opens additional soft keys for running a program (e.g. dry run, graphics only, etc.).
Once Clear Program is used the program cannot be recovered.
58
5 Program Overview
Program Functions
Program Functions soft keys
The Program Functions soft key provides access to the following soft keys for saving, clearing, or loading an existing program to either edit or run.
Soft key Function
The Load soft key will load the selected program. If a program is currently loaded, a prompt will be displayed asking for confirmation to clear the loaded program. If a program is currently loaded, it must be saved prior to pressing this key.
The Save soft key will save the currently loaded program, or the program can be saved under a new program name.
The Program Type soft key opens a popup Menu providing the choices which type of programs to display in the folder listing; MILLPWR
G2
programs,
G-code programs, DXF drawings, All programs or All files.
The Function soft key opens a popup Menu providing the choices to Cut, Copy, Paste, Merge,
Rename, or Delete any program that is listed in the folder. It does not need to be the currently loaded program.
The Select soft key allows the operator to select one or more programs from the current folder, or select all the programs. Select the Clear option to un-select the current selected program(s). This allows features within the Function soft key to be done on the selected group of programs.
The Change Window soft key toggles the cursor between the folder list, folder tree (if displayed) and program list.
The Folder View soft key opens the folder tree to access all folders, and sub folders. Use the Change
Window
soft key to navigate to the available windows.
Press the Exit soft key to return to the Program
Function screen.
ACU-RITE MILLPWR
G2
59
Pressing the Select soft key feature opens a popup menu that provides these three choices:
The Select feature will select one or more programs. Highlight each program to be selected, and choose Select for each program highlighted.
The Select All feature will select all programs in the folder.
The Clear feature will un-select one or more programs that have been highlighted. Clear does not delete a program, it will only un-select it.
Having a program, or programs selected, use the Function soft key to continue on taking the appropriate action required.
The Function soft key provides several choices that can be executed for the action taken after using the
Select
soft key feature:
The selected program(s) can be Cut from the current folder, then moved to another folder using the Paste feature.
In the same fashion, using the Copy feature, the selected program(s) can be copied to the same folder, or to a different folder using the Paste feature.
Use the Merge feature to paste the contents from the selected program to the currently loaded program at the current cursor location. This feature is only available for MILLPWR
G2
(.MPT) programs. Once this function is executed, it will exit the program functions, and return to program view.
Use the Rename feature to rename the selected program. Only one program at a time can be selected to use this feature.
60
5 Program Overview
Choosing the Delete feature will delete one or more programs selected. The message bar will be displayed showing the first selected program asking for confirmation to delete it. Four soft keys are displayed for deleting options.
Yes
will delete the current program displayed in the message bar.
Cancel
will cancel out of the current operation. Cancel will not restore any prior deletions that had been made.
All
will delete all the selected programs by automatically answering yes to confirm deletion of each program.
No
will cancel the deletion of the current program in the message bar.
Any program that is deleted can not be recovered.
Located in the upper right folder display area are two soft keys
Forward (+), Backward (-). These keys can be accessed directly
when using a mouse. Direct console access is accomplished by using the Plus, and Minus keys on the console keypad. The keys are used to facilitate navigation among folders in the console, network and USB memory devices.
Pressing the Minus key always takes you back to the previous folder location. Pressing the Plus key takes you to the next folder in the history. Plus is only available if Minus has been used.
The MILLPWR
G2 will save 20 history steps. The 21st history step will replace the 1st history step.
Edits to a program that have not been saved are lost.
ACU-RITE MILLPWR
G2
61
View hard key
Once a program is opened, the first step is to select how the part should be displayed in the graphics window. Pressing the VIEW key displays different soft keys for graphic viewing options of the program.
Pressing the View key again, or pressing the CANCEL key will turn the
view key display off. See "Program Drawing View" on page 56.
The VIEW key provides access to the following soft keys for selecting how the part should be viewed.
Keys Function
The Block Form (3D solid) opens a dialogue so that the operator can specify the block size shown in the graphic display area. MILLPWR
G2
normally calculates this but the user can adjust the values if necessary.
The arrow keys are used to adjust the view. The
Adjust View
opens a popup menu to select either
Zoom, Pan, or Rotate to have adjusted with the arrow keys.
Change View
opens a popup menu where either 2D
Line, 3D Line, or 3D solid view of the graphic display can be selected. The default is 2D line view.
Show Grid
toggles on, or off the grid display. This is only active in 2D Line view. The grid size can be
adjusted in Job Setup; see page 175.
Show Step Numbers
displays the program step number that is creating a particular tool path. These are best displayed with the Line View feature. This is a toggle key that turns the numbers on or off.
Show Toolpaths
displays the complete path the tool moves in each program step. This is a toggle key that turns the toolpaths view ON or OFF.
Show Contour
is available with 2D Line and shows the program geometry with a white line. When the
Show Step Numbers
is also selected, labels are added to the path showing which step was used to create that portion of the path.
Reset Graphics
restores the default zoom, pan, and rotate settings.
62
5 Program Overview
Step Functions soft keys
The Step Functions soft key provides access to the following soft keys for assistance with programing steps, and modifying or arranging the programs steps.
Soft key Function
The Explode soft key will explode a program step e.g. such as a bolt circle converting it from a radius and number of holes equally spaced to individual
coordinates for each hole. See "Explode" on page
158 for additional information.
The Reverse Step soft key will reverse the tool path of the selected step so that it will be followed in the reverse order.
The Reverse Path soft key will reverse the tool path selected of all the steps so that it will be followed in the reverse order.
The purpose of the Shift Steps feature is to transpose a range of steps from one location to another on the actual work piece within a program.
The Change Steps soft key opens a dialogue that will allow the operator to select a range of steps that can be modified for the Z axis, Offset, and Feed Rate.
The Delete Steps soft key opens a dialogue that will allow the operator to select a range of steps, or a step to be deleted.
The Copy / Move Steps soft key opens a dialogue that will allow the operator to select a range of steps to either be copied, or moved else where in the program.
ACU-RITE MILLPWR
G2
63
Program Steps soft keys
The Program Steps soft key accesses the soft keys listed in the table below. Each soft key (except for the Tool key) provides additional selections on a popup menu. This allows to further define the milling action to be programmed.
Soft key Function
The Tool soft key opens a tool dialogue to enter the size and type of tool to be used for the following step(s).
The Position/Milling soft key opens a popup menu to further define the milling operation e.g. Position/
Drill, Line, Arc, Blend (Round), and Blend (Chamfer).
The Custom Pocket soft key opens a popup menu to further define the milling operation e.g. Custom
Pocket, Island, and Contour.
The Hole Pattern soft key opens a popup menu to further define the milling operation e.g. Row of
Holes, Rectangle Frame, Rectangle Array, and Bolt
Circle.
The Rectangle soft key opens a popup menu to further define the type of milling operation e.g.
Pocket, Frame, Face, and Slot.
The Circle soft key opens a popup menu to further define a milling operation e.g. Pocket, Frame, Ring, and Helix.
The Repeat, Rotate ... soft key opens a popup menu to further define a milling operation e.g.
Repeat, Rotate, or Mirror
The Other Steps soft key opens a popup menu to further define the type of milling operation e.g. Engrave Line, Engrave Arc, Comment, Auxiliary
Function, Dwell, or Reference Point.
64
5 Program Overview
Clear Program soft key
This soft key provides a quick method to clear the current loaded program. It does not provide an option to save before exiting. Its function is meant to quickly clear a program (e.g. once it has been run and is no longer needed), so that a new program can be loaded, or a blank program is available, or return to DRO mode without having a program loaded. If the program has been edited the operator is asked to confirm the Clear operation. Save program changes before using
Clear. All changes are lost and cannot be recovered.
Press the Clear Program soft key to close the program.
Save/Discard soft key
Save/Discard
soft key opens a popup menu which provides the choice to either save the changes made to a program, or discard the changes by returning the program to its original state.
Press the Save/Discard soft key and select from the popup menu to either save the program, or discard the changes made to the program.
ACU-RITE MILLPWR
G2
65
Run Options soft keys
The Run Options soft key allows the program to be run and tested with various options for a program. These options allow the operator to test a program without actually cutting material. The Run Options must be set before you start to run the program.
Soft key Function
The Single Step soft key will move the machine one step at a time.
The Dry Run soft key will run the program’s tool path at the speed defined in Job Setup. No material should be placed within the tool path for this function. Dry Run is intended to provide a quick verification of the machine movements in the program.
The Graphics Only soft key will run through the program drawing the tool movement on the display only. Graphics Only is intended to provide a quick verification of the tool path in the display; no machine movement will occur.
The Optional Stop soft key will allow the program to be stopped at different locations to allow for verification of particular program steps selected has the operator. If a program has an optional stop (i.e.:
M01 in a G-code program), the system will only stop at this block when Optional Stop is enabled. If it is disabled, it will be skipped. The Optional Stop is an
M01 in a G-code program.
The Exit soft key will exit the Run Options function and return to the previous display.
66
5 Program Overview
Program Saving
When you create programs with the MILLPWR within MILLPWR
G2
G2
, they can be saved
's User folder, on a USB device, or a network location.
MILLPWR
G2
will retain a program in memory so it is not lost in the case of a power failure.
Programs can be organized in MILLPWR
G2
, on a USB device, or a network location; or in personalized folders that the operator can create.
Saving a Program
A new blank program can be saved prior to having any program steps added, a newly created set of program steps can be saved as a new program, or an existing program can either be saved as a new program by replacing the current name, or save the existing program.
To save the current active program, select the Save soft key. The keyboard will popup with the Save key highlighted. Press the ENTER key. A prompt will ask to overwrite the existing program. Press the Yes softkey.
The keyboard will automatically be displayed with the current program
name highlighted in the keyboard display window (see "Keyboard" on page 17).
The Save/Discard key is also available to quickly save a program, or discard any changes made since the last time it was saved.
Press the Save/Create soft key to save the program with its current name, or enter a new name for the current program to create a new program.
A name can not be longer than 60 alphanumeric characters. The MILLPWR
G2
displays program names as they were entered. No two programs can have the same name.
The program’s graphic preview is updated whenever the program is saved. In order for the new graphic preview to be created correctly, the program must not have any errors. The operator must allow the program graphics to finish drawing the program before pressing any keys.
ACU-RITE MILLPWR
G2
67
5.2 Program Mode Functions
Program Type Filter
In PGM mode, press the Program Functions soft key to display the
Folder View
, and Program Type soft keys. Program type aids with locating programs by type, and reduces the number of programs that are displayed.
To select what type of programs to show, press the Program Type soft key, and select which program type(s) to display using the ARROW keys.
USB Access
As soon as the USB memory device is inserted, its contents will be displayed in the Folder Contents window. From here the operator can modify, copy, delete, etc. any of the programs, or folders on the
USB device.
In PGM mode, the operator can access a USB memory device by inserting the USB device into a USB port of the MILLPWR
G2
.
From DRO mode, press the DRO/PGM to enter PGM mode.
Press the Program Functions soft key.
Press the Folder View soft key.
The display will now show the USB device in the Folder Contents window, and when selected, will show its content in the upper right window.
It is recommended to copy programs from the USB device to the user folder and use the program from the
MILLPWR
G2
.
Prior to removing the USB memory device, check that the activity indicator light on the USB drive is not active or blinking. This will ensure that all commanded disk operations have completed, and that it is now safe to remove the drive.
68
5 Program Overview
5.3 Creating programs overview
New Part Program
The following briefly describes how a new program is created. See
"Fundamentals for Creating a Program" on page 75 for more complete
information.
Press the DRO/PGM key from DRO mode to enter PGM mode.
A new program can be created from an existing program, or create a completely new program.
To create a new program from an existing program:
Press the Program Functions soft key.
Select an existing program that will be used to create the new program, and press the Load soft key.
Press the Program Functions soft key.
Press the Save soft key. Press the Keyboard soft key to display the keyboard if the keyboard is not automatically displayed. Type in the name of the new program and select Save.
The new program is now loaded, and can be modified as required.
To create a new (blank) program:
When a program is currently loaded, press the Clear
Program
soft key in the PGM mode display to clear the loaded program from memory, and to create a new program.
Press the Save soft key. Press the Keyboard soft key to display the keyboard if the keyboard is not automatically displayed. Type in the name of the new program and select Save.
ACU-RITE MILLPWR
G2
69
70
5 Program Overview
Programming
6.1 Conversational Programming
Programming Considerations
“From” and “To” points
Lines and arcs are defined by their FROM point (the point where they begin) and TO point (the point where they end).
Depth of Cut
When programming the depth of cut, MILLPWR
G2
will prompt for the
BEGIN and END locations for the Z axis.
The location that is entered into the Z BEGIN field tells MILLPWR
G2 where the quill is to begin cutting at the programmed feed rate. The
END location defines the depth of the cut.
Always be sure that the BEGIN location is above the surface of the workpiece.
Pass
PASS refers to the number of cuts or the distance (depth) of each cut that are used to machine an area to its END depth. The operator selects which is to be required in this field from Job Setup. In the JOB
SETUP dialogue, DISTANCE or NUMBER of CYCLES must be
selected. Which selection is chosen will appear on all dialogues where it is required. The number of passes can be controlled by entering a value in the PASS field (where ever it is available).
PASS is ignored on 2 axes systems. The operator must set the depth of cut for each pass, and repeat the operation
until the full depth has been reached (see "Machining Your
Leaving the field blank programs the MILLPWR
G2
to make the cut in the number of passes it decides is necessary.
No pass will exceed the diameter of the active tool
72
6 Programming
Tool Offset
MILLPWR
G2 will calculate the actual tool path when using left and right offsets. Program the dimensions of the part as identified by the part drawing.
Program a line, arc, frame, etc. using the “Tool Offset” field to tell
MILLPWR
G2
which side of the line the tool is to be on. See "Tool
To determine which offset to use: If the tool needs to be on the left side of the line, use a LEFT offset. If the tool needs to be on the right side of the line, use a RIGHT offset.
When using a CENTER offset, the programmed dimensions are for the center of the tool. For some milling functions, like frame and arc,
INSIDE and OUTSIDE offsets are available to make it easier to define the tool offset.
Datum Selection
If the datum isn't defined on your print, then determine the datum based upon where most of the dimensions originate.
Pick a point which will let you enter most of the dimensions directly, with fewest calculations.
Establishing a datum requires that the Z retract position be provided
(the position the quill returns to between program steps).
By setting a retract position, you can ensure that the tool you are using does not make contact with your workpiece when the quill moves from one position to the next.
Establish a retract position for the Z axis each time the console is powered, otherwise the MILLPWR
G2
will use the quill’s previous retract position.
A two axes system also requires the Z depth, and Z retract position. The operator will be prompted to manually move to a depth, or retract position.
ACU-RITE MILLPWR
G2
73
Absolute vs. Incremental Dimensions
MILLPWR
G2
allows both absolute and incremental dimensions to be entered. A dimension measured from the point you defined as datum is an absolute dimension. A dimension measured from any other point
is an incremental dimension. See "Absolute and incremental work piece positions" on page 25.
The dimension moves of 8, then 8 again are incremental moves.
The dimension moves of 8, then 16 are absolute moves.
Continuous Milling
When you program a continuous contour of lines and/or arcs the contour will cut without stopping if there is no programmed stop.
MILLPWR
G2
will automatically recognize continuous contours as you're programming. There are no special key presses or other functions to learn.
For lines and arcs to be continuous, they must:
Be consecutive steps in a program.
Have the same depth.
Be cut with the same tool.
Be cut using the same tool offset.
Share a common “From” or “To” point (one step must end at the point where the next one begins).
If one step follows another, then MILLPWR
G2
assumes that they are to be connected (see steps 003 through 006). The single line bracket indicates the steps that will be machined with continuous milling.
MILLPWR
G2
automatically fills in the FROM point, DEPTH, and TOOL
OFFSET from the previous step. The TO point must be filled in, and then press the USE key.
Different feed rates within each step of a continuous contour are allowed, and can be used.
74
6 Programming
Fundamentals for Creating a Program
In DRO mode press the DRO/PGM key to enter program mode.
Programs are created by developing a list of milling steps to be performed. As steps are added to the list, each will immediately be drawn on the screen so that it can be displayed graphically, showing the part machining in progress.
MillPwr G2 allows a maximum of 9999 program steps.
Entering milling steps
Before any programming steps are entered, a tool must first be
selected and entered. See "Editing the tool table" on page 46.
The milling function keys are among the eight yellow keys located in the upper right corner of the console. The function you select will appear in the program listing and will enable you to enter the data and add the step into the program.
Additional milling functions are available in PGM mode, and are accessed by pressing the Program Steps soft key. Program Steps soft keys are also displayed when RECT, CIRCLE, or the HOLES keys are pressed in PGM mode.
To enter a milling step, press the appropriate milling function (e.g.
LINE
). Some keys will open a popup menu with the soft key to further define the type of milling step that is to be performed.
After entering the data for the program step, press the
USE
key to add the step to the program.
Press the CANCEL key at anytime to exit the milling step dialogue and not add it to the program.
ACU-RITE MILLPWR
G2
75
Adding/Inserting milling steps
A new program step number automatically appears following the last step entered, and the new step is highlighted.
If the cursor was moved for any reason, use the arrow keys to highlight the new step, then select the milling function to be added.
To insert a step between two existing steps, position the cursor to the step below where the new step is to be placed.
Press the desired milling function key, and it will be inserted above the highlighted program step.
Additional milling functions are available by pressing the Program
Steps
soft key. The soft keys change, displaying several Milling function soft keys. Each soft key when selected will have a popup menu for further selection to refine the type of milling operation to be entered. For example, the Circle soft key will display choices for the type of circle to be milled; a Pocket, Frame, Ring, or a Helix.
Editing or Deleting a milling step
To edit a program step, use the arrow keys to highlight the step to be changed and press the USE or ENTER key, or just enter a step number using the numeric keypad.
A Goto program line number popup dialogue is immediately displayed. The total number of lines in the program are shown in the
Line Count: field.
Enter the desired line number and press ENTER.
Press ENTER or USE again to to edit the program step.
After making the appropriate changes, press the USE key to accept the changes and place the step back into the program. Or press
CANCEL
to discard any changes to the step.
To delete a step, highlight the step to be deleted, then press the
CLEAR
key.
VIEW
key
If you need to see the machined part in more or less graphic detail, press the VIEW key. This enables you to
access the viewing soft keys that are available. See
"View hard key" on page 62 for a complete description
of these soft keys.
76
6 Programming
Program Errors
When an error is detected in a program, the step with the error is highlighted in the program listing with a red " x " symbol. Edit the program step to correct the error.
Additional information about the error is added to the error log. See
After correcting the errors, remember to delete them from the error log. A quick method for deleting all errors in the log is to press the “0” on the numeric keypad.
If there is more than one error in the program, only the first step with an error will be highlighted. After correcting the first error, the next error will be highlighted.
Program Edited
When a saved program is loaded, only the name and extention is displayed.
If the saved program is then edited, the program name will show an asterisk at the end of the name.
This tells the operator that the program has changed, but has not been saved.
Saving the program will remove the asterisk, or exit the program without saving the changes.
When a program that has been edited, but not saved, then it will revert back to the last saved version when closed. The program will not display an asterisk the next time it is loaded.
ACU-RITE MILLPWR
G2
77
Running a Program
Skewing a Part
For some machining operations it is more convenient to use the Skew feature rather than indicating in the work piece.
With MILLPWR
G2
, it may save time setting up a job by skewing the part. The Skew feature automatically compensates for the offset angle of the part by touching off one straight edge with an electronic edge finder or a mechanical indicator.
To skew a part touch off on two or more points along one axis, either
X or Y. Touch off and use the teach position feature.
Do not enter coordinates along a curve, two different lines, or along a line that’s positioned at a 45 degree angle.
MILLPWR
G2
will calculate the skew angle based upon a straight line between the points that have been entered.
A work piece that has a rough edge should have multiple points entered along the straightest edge to more accurately calculate the skew angle.
78
6 Programming
Using an electronic edge finder:
Press the Datum softkey to open the DATUM dialogue. Highlight the
Angle field.
Touch off on two or more points along any single straight edge of your part. You’ll notice that the POINTS and ANGLE fields change as you enter points.
Press USE to accept all of the points and return to the DRO screen.
Press CANCEL to return to the DRO screen without accepting any points or affecting your previous skew angle.
The Clear Angle soft key will reset the number of POINTS and the
SKEW ANGLE to zero.
Using Teach Position:
Move the table so that a mechanical indicator rests against any straight edge on the part. Press the Teach Position soft key to enter your coordinate.You’ll notice that the POINTS change.
Now move the table so that the mechanical indicator touches another point on the same straight edge. Press the Teach Position soft key.
You’ll notice that the POINTS and ANGLE fields change.
Repeat this process for any additional points.
Press USE to accept all of the points and return to the DRO screen.
Press CANCEL to return to the previous screen without affecting your previous skew angle.
Establishing a Datum
Overview
Datum is the workpiece zero or absolute zero, and is a point of reference that the MILLPWR
G2
bases all of the part's coordinates from.
A datum must be established for every job. Datum's location may be indicated on the print; or the operator may establish a datum that allows most of the part's dimensions be entered directly using the least amount of calculations.
When establishing datum, it may be easiest to locate a known point on each axis, such as the corner of the part, or a location on a vise or fixture.
Datum can be set at a point on the top surface, a position beneath the surface, or at a point where there's no material present (such as in the center of a circular part). The following example will illustrate touching off the edge of a work piece using a tool, but an edge finder can also be used in place of the tool. Either item will accomplish the same result.
ACU-RITE MILLPWR
G2
79
Steps to Establish the datum
Where and how you establish the datum will vary from job to job. The following step, by step process is a common method of establishing a datum. Being familiar with the basics, the same principles will apply for other parts, making adjustments to the procedure as needed when setting the datum.
From the DRO mode, press the Datum soft key.
In the datum number field, enter a number for the datum to be defined. Since this will be the first datum being defined, use the number 1.
Insert a tool into the spindle (e.g. such as the tool for the first cut).
When Tool information is listed in the Status Bar at the top of the screen, it is ignored by the MILLPWR
G2
when establishing a datum. The information for the tool that is actually being used to establish the datum must be used.
This example will establish the datum on the corner where the left, front and top surfaces of the part intersect. This will be accomplished by “touching” each face with the tool that will make the first cut to the part.
Using the calculator in an entry field in a dialogue requires the operator to press the ENTER key to perform the calculation. To move to the next field using the ENTER key requires the operator to press ENTER a second time.
In the SET DATUM dialogue the X, Y and Z fields are always active, displaying the machine position relative to the selected datum.
Open the SET DATUM dialogue to view the machines position relative to any defined datum number by entering the number in the
DATUM NUMBER field. Then press ENTER, or ARROW DOWN. This provides the operator with a constant quick reference for the datum selected.
Viewing other datum numbers does not change the selected datum displayed in the Status Bar. To change to another defined datum, press the USE key.
When a new datum number is defined, or another number is selected, and the USE key is not pressed, all information entered is discarded, and the current active datum number is retained.
80
6 Programming
X Axis Datum:
Lower the tip of the tool so that it falls below the top surface of the part.
Move the table along the X axis, slowly spinning the tool by hand as you go. When the tool contacts the part, stop the table.
Using the numerical keypad, enter the radius of the tool (the distance from the center of the tool to the edge of your part) into the
X: field. Be sure to specify if it’s a negative value.
In this example, the value will be specified as a negative value, because the tool's center is on the negative side of our datum (refer to Axis Conventions).
Press the +/- key.
Enter the radius value.
Press the ENTER key to enter the data and move to the next field.
Y Axis Datum
Lower the tip of the tool so that it falls below the top surface of the part as done with the X axis.
Move the table along the Y axis, slowly spinning the tool by hand as you go. When the tool contacts the part, stop the table.
Using the numerical keypad, enter the radius of the tool (the distance from the center of the tool to the edge of your part) into the
Y: field.
Press the +/- key to change the data to a negative value.
Enter the radius value.
Press the ENTER key to enter the data and move to the next field.
Z Axis Datum
Position the tool so that its tip touches the top surface of the part.
Press the Z = 0 soft key.
Press the ENTER key. With the data entered, the cursor will highlight the next field.
ACU-RITE MILLPWR
G2
81
Retract Z
Now either enter the Z axis retract position (the position that the quill should return to between steps) which is the location above the top surface of your part.
Or press the CLEAR key to clear the value. If no value is set, the quill will retract to the upper travel limit between steps.
Press the ENTER or USE Key to save the datum location and return to
DRO
mode.
Datum and the Z axis retract position have now been established.
Each datum has its own retract position. When a new datum is selected, that datum’s retract position will be used.
Using an electronic edge finder
When the SET DATUM dialogue is first opened, the DATUM
NUMBER field is highlighted. Enter a new datum number, or select a number that is to be modified.
When a DATUM field is selected (X, Y or Z), the Probe softkey is enabled. This allows the operator to set the datum using an electronic edge finder.
When the probe key is selected, the electronic edge finder is automatically selected. The radius of the tip must first be entered into the Job Setup dialogue.
82
6 Programming
Select the datum field that is to be set (X, Y or Z axes), then press the Probe soft key.
The datum is set for the axis that was last used when the edge finder was triggered. If moving the X axis when the edge finder is triggered, the X datum will be set and the X datum field will be set to 0.0000.
With the Probe soft key activated, select the type of probing to be performed by pressing the appropriate softkey: Edge, Centerline, or
Circle Center
.
Keys Function
Edge
sets the datum with a single trigger of the edge finder. The system will prompt to "Move to edge".
Using any axis, start movement until the edge finder is triggered. Once triggered, the system will exit the probing mode and set the moving axis' datum.
Centerline
sets the datum with 2 triggers of the edge finder and will use the center point as the axis' datum. The axis that is used for the first trigger must be used for the second. For example, if the first trigger occurred using the X axis, the X axis must be used for the second trigger.
Circle Center
sets the datum using 3 points of a circle. This operation will only work with the X and
Y axis and any of the triggers can be accomplished by moving either of these axes. This function will set the datum for both X and Y.
ACU-RITE MILLPWR
G2
83
Test the Datum Setting
It's recommended to test the datum setting before beginning a program.
To confirm the datum setting use the Pos key.
To quickly move to the datum for X and Y, press the Pos key.
With the Z axis at its retract position, enter 0.0000 for the go to position for both the X and Y (leave the Z field blank). Press the GO key.
The table will move to the datum position X 0.0000, Y 0.0000.
Lower the tool until it touches the part.
Visually check the tool's position. The lower left corner of the part should be positioned directly beneath the center point of the tool.
The readout screen should be at 0.0000, confirming the datum is accurate and programming can now begin.
The value of 0.0000 in the Z axis display may vary slightly depending on how the tool tip contacts the top surface of the part on the corner edge.
84
6 Programming
Testing a MILLPWR
G2
Program
Before machining a part, test the program for things like correct tool path, count direction, feed rate, and sequence of operations.
MILLPWR
G2
provides several run-time choices to assist doing this.
Always verify a program when it was loaded, or edited.
Whenever a program is about to run, check that the handles are recessed.
Keys
From the PGM screen, press Run Options to display the following soft keys:
Function
Single Step
runs through the program one step at a time. Some steps will run as a single group such as a contour, or custom pocket.
Dry Run
runs through the program at the defined dry run feedrate instead of programmed feeds. This option is useful to more quickly test the tool path motion. The dry run feedrate is set in the JOB
SETUP dialogue.
Graphics Only
runs through the program graphically.
The table and quill do not move. This option is useful to test the tool path without risk of damage to tool or workpiece.
The Optional Stop soft key will allow the program to be stopped at different locations to allow for verification of particular program steps selected by the operator. If a G-code program has an M01
(optional stop) in it, the system will only stop at this block when Optional Stop is enabled. If it is disabled, it will be skipped.
ACU-RITE MILLPWR
G2
85
Press any soft key to activate the option; press it again to deactivate it.
Before pressing the GO key to begin the Single Step, Dry
Run
features, check that the tool will not touch the workpiece when the quill begins to move. To avoid interference, do one or more of the following:
• Lower the knee
• Remove the tool or workpiece
• Reestablish datum away from the part.
Single Step
Normally, a continuous contour will be machined without stopping.
With Single Step activated, MILLPWR
G2
will stop after each step.
This enables a check of the tool position of the Z axis relative to the part and ensure that the tool path and other program details are correct. Press the GO key to begin, and after each step finishes.
Dry Run
With Dry Run activated, MILLPWR
G2
will run the entire program at high speed without stopping. Visually follow the position of the tool relative to the part and ensure that the tool path and other program details are correct. The dry run speed is defined in Job Setup. Press the GO key to begin.
Graphics Only
With this activated, the table and quill will not move. The graphics screen will show how the part will be cut. Press the GO key to begin.
Note: Dry Run and Graphics Only can be used to quickly verify your program.
86
6 Programming
Machining Your Part
Before running a program step, check the Status bar (located along the top of the MILLPWR
MILLPWR
G2
G2
screen) to ensure that the tool identified by
matches the tool in the spindle. If there’s no tool identified, or if it’s incorrect, start with a SET TOOL step that accurately identifies the tool that is to be used.
To move quickly to a step, use the up/down ARROW keys to highlight the required step, or just enter a step number using the numeric keypad.
A Goto program line number popup dialogue is immediately displayed. The total number of lines in the program are shown in the
Line Count: field.
Enter the desired line number and press ENTER.
Press ENTER or USE again to to edit the program step.
After highlighting the step to begin with, press the GO key. An Operator
Intervention Message may ask to confirm that the tool is correct.
Confirm that the correct tool is being used, then press the GO key again to begin milling.
If the tool is positioned above the Z axis retract position before running a program, the table will rapidly move to position, and then the quill will rapidly move to the retract position. If the tool is below the retract position, the quill will move first.
A 2 axes system requires that the quill be raised manually before pressing GO.
Once the quill has reached its retract position, it will rapidly move to the BEGIN depth then move at the programmed feed rate to the End depth.
The remote STOP/GO switch acts as a pause switch if the table is moving, and as a GO switch if the machine is paused or stopped.
If the travel limit for the Z axis is set below the established retract position, a travel limit fault will occur and the program will stop.
ACU-RITE MILLPWR
G2
87
MILLPWR
G2
will automatically pause at points that require action to be taken (e.g., change tools). After each task has been completed, press the GO key.
A 2 axes system requires the Z axis to be moved manually into position.
If the STOP key is pressed once while cutting, the tool will pause in its cutting path and an Operator Intervention Message will appear. Press
GO
to resume machining, or STOP again to end the program.
If machining is started from the middle of a program,
MILLPWR
G2
will determine which tool should be used, and will prompt the operator to mount the tool if it is not mounted.
Potentiometer for Feedrate Override
Feedrate Override are controlled with the potentiometer which will change the feed rate by a certain percentage with the knob rotation.
The feed rate percentage will be displayed in the status bar at the top of the screen. A feed rate percentage of 100% means that actual feed rates will run at 100% of the programmed feed rates. If the feed rate percentage is 50%, actual feed rates will run at half of the programmed feed rates.
Adjustment of the feed rate with the potentiometer can be done at any time, even while the table or quill is moving.
88
6 Programming
Manually Positioning the Quill
Programs that do not include a BEGIN depth will require the operator to manually position the Z axis during machining. The same is true when the Z axis has been disengaged during setup.
If an END depth is programmed, when it is time to manually position the Z axis, a preset value will be displayed in the Z axis display. The
DRO screen will appear, along with the prompts shown.
When multiple passes are required, in this example the complete program can be run for each pass. It may also be necessary to repeat a set of steps for each pass in a program (e.g. milling a pocket).
An example of an Operator Intervention Message (OIM) similar to the one shown to the right will appear.
Manually move the Z axis incrementally until 0.0000 is displayed for the Z axis.
ACU-RITE MILLPWR
G2
89
6.2 Folders
Folder Functions
The soft keys available are described in the previous chapter, see
"Program Functions soft keys" on page 59.
MILLPWR
G2
offers several versatile features for loading, saving, deleting, and backing up programs. Programs can be organized by creating folders. Folders can be quickly selected, created, make a backup copy, or if necessary, deleted.
Folders
Organize programs by saving them in folders. Folders may be used to group programs by job, operator, date, customer, or any other method preferred. Creating folders can only be done in PGM mode.
Creating a Folder
First decide where to place the folder. It can be placed on V:\User which is the MILLPWR
G2
folder in the console, on a USB device, on a network, or within sub-folders that have already been created. Use the following steps to create any type of folder, top level or sub level folders.
When the Folder View soft key is activated, it remains active until it is pressed again to deactivate folder view.
Press the Program Functions soft key, then press the Folder View soft key.
Press the Change Window soft key to select the Folder Tree window.
Navigate through the folders to place the cursor where the new folder is to be created by using the ARROW keys.
To expand a folder use the RIGHT ARROW key. To collapse an expanded folder, use the LEFT ARROW key.
Highlight the folder where the new sub-folder is to be placed, and press the Create Folder soft key.
90
6 Programming
Naming a new folder
Using the on screen Keyboard, enter the name of the new folder. If the keyboard is not automatically displayed, press the Keyboard soft key.
Once the new folder’s name has been entered, press the Save/
Create
soft key to create the new folder.
Deleting a Folder
MILLPWR
MILLPWR
G2
will delete folders that contain programs, or files.
G2
will prompt the operator that there are files within the folder, and ask for confirmation if they are to be deleted.
Press the PROGRAM FUNCTIONS soft key, then press the Folder View soft key.
Press the Change Window soft key to select the Folder Tree window.
Navigate through the folders, and place the cursor where the folder is to be deleted.
Press the Function soft key, and select Delete from the popup menu.
Press the Yes soft key to erase the folder, and all files in the folder, or the No soft key to cancel.
Once a folder is deleted it cannot be recovered.
Saving a Program
When creating programs with the MILLPWR within MILLPWR
G2
G2
, they can be saved
's User folder, on a USB device, or to a network location. A graphic view of the program is displayed in the Preview
Window if it has been run successfully.
Programs can be organized in MILLPWR
G2
, on a USB device, or a network location; or in personalized folders that the operator can create.
To save the current program for the first time:
Press the Program Functions soft key.
Press the Save/Create soft key.
The keyboard should automatically be displayed with the cursor in the
Program Name field (see "Keyboard" on page 17).
ACU-RITE MILLPWR
G2
91
Naming a Program
Before you can save a program, MILLPWR
G2
requires it to be named.
Enter the program name using the ARROW keys to navigate the keyboard. Highlight the key to be used (e.g. letter, or number), then press the ENTER key to add the selection into the Program Name: Field.
Continue in the same manner until the name is complete.
To add numbers to your program name, press any of the number keys on the numerical keypad, or from the keyboard display.
Press the Save/Create soft key. MILLPWR
G2
will store the program in the folder that had been previously selected.
A message will alert you if the program was not saved properly, or if the name that you’ve chosen already exists.
Back up MILLPWR
G2 programs regularly to avoid accidental loss
(e.g. USB device, or to a network location).
Deleting a Program
Press the Change Window soft key to select the Folder Contents window.
Highlight the desired program.
Press the Function soft key, and select Delete from the popup menu.
Press the Yes soft key to erase the program, or the No soft key to cancel.
Once a program is deleted it cannot be recovered.
92
6 Programming
Loading a MILLPWR
G2
(MPT) Program
The Load soft key allows you to open programs in the folder listing.
The steps below explain how to load a program from MILLPWR
G2
User folder, a USB device, or from a network location.
Program extensions:
MILLPWR
G2
programs have a .mpt extension.
G-code programs have a .G or .NC extension.
DXF files must have a .DXF extension.
If a program is loaded, save the open program, it does not have to be cleared.
From the PGM screen, press the Program Functions soft key.
When a program is not located in the current folder, select the location of the MILLPWR
G2
program using the Folder View soft key, and Change Window soft key as needed.
Verify that MILLPWR Programs is selected in the Program Type popup menu. Only MILLPWR
G2
programs stored in the selected
folder will be displayed, see "Program Type Filter" on page 68.
Using the ARROW keys for navigation in the display window, highlight the MILLPWR
G2
program to load.
Press the Load soft key, and verify that the desired program is now loaded.
When loading a program from a network, or a USB memory device, first select the device from the Folders Tree, then follow the same procedure as would be done from the MILLPWR
G2
User folder.
Use Folder View for locating folders, and programs to load.
It is recommended that all programs be copied to the local
MILLPWR
G2
User folder for usage.
ACU-RITE MILLPWR
G2
93
Importing a DXF drawing
Save any running programs. Locate the folder containing the DXF drawing.
If a program is loaded, save the open program, it does not have to be cleared.
From the PGM screen, press the Program Functions soft key.
When a DXF drawing is not located in the current folder, select the location of the DXF drawing using the Folder View soft key, and
Change Window
soft key as needed.
Verify that DXF Drawing is selected in the Program Type popup menu. Only DXF drawings stored in the selected folder will be
displayed, see "Program Type Filter" on page 68.
Using the ARROW keys for navigation in the display window, highlight the DXF drawing to load.
Press the Load soft key, and verify that the desired program is now loaded.
MILLPWR
G2
will assign default values for any information that’s missing from the DXF drawing (e.g. tool offset, feed rate, etc.). The required SET TOOL steps must be added.
MILLPWR
G2
will then arrange the steps in a logical order based on common end points, and create a tool path. The program will then appear on the display.
Test the program before machining to ensure that the program steps and tool path do what is expected. The program can be edited and steps rearranged as needed.
94
6 Programming
G-code Programs
MILLPWR
G2 has the ability to read and run G-code programs, however those programs can not be edited. It is important to fully test the
G-code program before machining a part.
Loading a G-code Program
A G-code program can be loaded into MILLPWR manner as MILLPWR
G2
G2
in the same
programs. Once loaded, MILLPWR
G2
will indicate with an " x " the first error regardless of the cursor location. An error message also appears in the message line indicating that the line contains invalid code. The invalid code can be removed editing the program outside of the MILLPWR
G2
.
The Load soft key opens programs that have already been saved. Use the following steps to load a G-code program from MILLPWR
G2
User folder, a USB device, or from a network location.
If a program is loaded, save the open program, it does not have to be cleared.
When a G-code program is not located in the current folder, select the location of the G-code program using the Folder View soft key, and Change Window soft key as needed.
Verify that G-code Programs is selected in the Program Type popup menu. Only G-code programs stored in the selected folder will be
displayed, see "Program Type Filter" on page 68.
Using the ARROW keys for navigation in the display window, highlight the G-code program to load.
Press the Load soft key, and verify that the desired program is now loaded.
When loading a program from a network, or a USB memory device, first select the device from the directory tree and follow the same procedure as would be done from the MILLPWR
G2
User folder.
G-code programs are “run only”, and cannot be edited. All editing should be done outside of the MILLPWR
G2
.
ACU-RITE MILLPWR
G2
95
Running a G-Code Program
MILLPWR
G2
has the ability to read and run G-code programs, however those programs can not be edited by the MILLPWR
G2
. It is important to create and proof the G-code program before attempting to machine a part.
Verify the program in the CAD/CAM system that generated the program. MILLPWR
G2
will draw the program when Loaded. Finally, lower the knee and dry run the program to verify that the tool path, feeds and speeds are correct.
Using the Tool Table
Each "T" block refers to the corresponding number in the Tool Table.
For example, T1 will cause MILLPWR
G2
to retrieve the tool length offset from tool 1 of the Tool Table. MILLPWR
G2 spindle by this amount. T2 will cause MILLPWR
will then offset the
G2
to retrieve the tool
length offset from tool 2 of the Tool Table, etc. See chapter "4.1 Tool
Table" on page 44 for a complete description about using the Tool
Table.
It is very important not to have any tool length offsets in the Tool Table if the tooling is not repeatable. The user will need to set the Z datum after mounting the new tool. This is done before pressing GO to continue running the program.
Failure to maintain the Tool Table can cause unpredictable results.
Verifying tool length offsets prior to program execution is strongly recommended.
Starting or Stopping a G-code Program
Always start the program from a place in the program where the feed rate, X, Y, and Z axes position are known, such as a tool step. Alternate starting points can be programmed by placing the proper code in the desired locations.
Pressing the GO button will cause MILLPWR
G2
to begin executing the
G-code program. Always insure the program step highlighted is an appropriate starting point.
When a program is running, pressing the STOP button or the remote pendant will cause the program and all axis motion to pause. Pressing the remote pendant switch again or the GO button will cause the program to resume. Pressing the STOP button a second time will halt the program execution.
96
6 Programming
G17
†
G18
†
G19
†
G20
†
G21
†
G-code and M-Code Definitions
G-code
The following is a list of supported, and unsupported G-codes.
† Represents supported G-codes.
G-code Listing
Comment G-code
G0
†
Description
Linear Interpolation (Rapid)
G1
†
G2
†
G3
†
Linear Interpolation (Feed)
Circular Interpolation (CW)
Circular Interpolation (CCW)
These commands generate table/quill motion. The motion command applies to current and subsequent blocks containing at least one X, Y, or
Z coordinate. The default motion command is a linear move at feed (G1).
G4
† Dwell
This command causes the system to pause for the specified period of time. The period of time is determined by the P address (in milliseconds) or X address (in seconds). T Address also specifies the time in seconds.
XY Plane Selection
XZ Plane Selection
YZ Plane Selection
Set Program Units (INCH)
Set Program Units (MM)
These commands set the plane in which arcs are executed. The setting applies to current and subsequent blocks. The default is G17 (XY).
These commands set the unit of measure. The setting applies to current and subsequent blocks. The default is G20 (INCH).
ACU-RITE MILLPWR
G2
97
G-code
G28
G30
G44
G49
G54
G55
G40
†
G41
†
G42
†
G43
G56
G57
G58
G59
Description
Return to Home Reference
Cancel Cutter Compensation
Cutter Compensation (Left)
Cutter Compensation (Right)
Tool Length Offset (+)
Tool Length Offset (-)
Cancel Tool Length
Comment
MILLPWR
G2
does not have a method for establishing a "home" position.
If one or more coordinates are specified in the block, the table/quill will rapid to that location. Program execution will continue with the next program block.
MILLPWR
G2
supports automatic cutter compensation. Enable cutter compensation using G41 (left) or G42 (right). Disable compensation using G40 (center).
MILLPWR
G2
does not support tool length offsetting. The offset is retrieved from MILLPWR
G2
’s tool library when a tool change is executed. These commands are ignored.
MILLPWR
G2
does not support presettable work coordinate systems.
G54 through G59 are ignored. Selecting a coordinate system is possible, but setting it (G10 or G92) will generate a run-time error
Work Coordinate System
98
6 Programming
G-code
G61
†
G64
†
G70
†
G71
†
G80
†
G81
G82
G83
G85
†
†
†
†
Description
Set "stop" Path Mode
Set "continuous" Path Mode
Set Program Units (INCH)
Set Program Units (MM)
Cancel Motion Mode
Basic Drill Cycle
Counterbore Drill Cycle
Peck Drill Cycle
Boring Bidirectional Cycle
Comment
These commands set the path mode. The setting applies to current and subsequent blocks. The default is G64 (continuous).
These commands set the unit of measure. The setting applies to current and subsequent blocks. The default is G70 (INCH).
This command cancels the current modal drilling cycle. The modal drilling cycles are described below (G80 series).
Basic drilling cycle is generally used for center drilling or hole drilling that does not require a pecking motion. It feeds from the begin depth (R) to the specified hole depth (Z) at a given feedrate (F), then rapids to the retract height (P).
G81 Z(zDepth) R(zBegin) P(zRetract) F(feedrate)
Required: Z, R
Counterbore drill cycle generally used for counterboring. It feeds from the begin depth to Z depth, dwells for specified time, then rapids to the retract point.
G82 Z(zDepth) R(zBegin) P(zRetract) D(dwell) F(feedrate)
Required: Z, R, and D
The peck drilling cycle is generally used for peck drilling relatively shallow holes. It feeds from the begin depth to the first peck depth
(calculated so that all pecks are equal and do not exceed the maximum peck distance programmed in I word). Then rapid retracts to begin depth
(to clear chip), rapids down to previous depth less .02", and continues this loop until it reaches the final hole depth. It then rapids to the retract point.
G83 Z(zDepth) R(zBegin) P(zRetract) I(zPeck) F(feedrate)
Required: Z, R, and I
Boring Bidirectional is a boring cycle, generally used to make a pass in each direction on a bore or to tap with a self-reversing tapping head. It feeds from the begin depth to Z depth, and then feeds back to the retract height.
G85 Z(zDepth) R(zBegin) P(zRetract) D(dwell) F(feedrate)
Required: Z(zDepth) R(zBegin)
ACU-RITE MILLPWR
G2
99
G-code
G87
G89
G90
G*
†
†
†
G91
†
G120
†
Description
Chip Break Cycle
Flat Bottom Boring Cycle
Set Offset Mode (ABS)
Set Offset Mode (INC)
Block Form
Comment
This is the chip-breaker peck-drilling cycle, generally used to :
Peck-drill medium to deep holes. The cycle feeds from the begin depth to the first peck depth in Z, rapid retracts the chip-break increment (W), feeds to the next calculated peck depth (initial peck less J), and continues this sequence until it reaches a U depth, or until final hole depth is reached. The peck distance is never more than I or less than K.
This cycle enables optimum drilling conditions for holes. For maximum efficiency in deep hole drilling, set parameters to accommodate the material and tool types used. Generally, the deeper the hole, the smaller the peck distance (J). This prevents the binding of chips, tool, and workpiece. Set U to retract the drill completely at set depth intervals.
G87 Z(zDepth) K(minPeck) R(zBegin) J(peckDecr) I(firstPeck) P(zRetract)
U(retractDepth) W(chipBreakInc) F(feedrate)
Required: Z(zDepth) K(minPeck) R(zBegin) J(peckDecr)
This boring cycle generally used to program a pass in each direction with a dwell at the bottom. The tool feeds from the begin depth to Z depth, dwells for specified time, then feeds to the retract (P) dimension.
G89 Z(zDepth) R(zBegin) P(zRetract) D(dwell) F(feedrate)
Required: Z(zDepth) R(zBegin) D(dwell) I(firstPeck)
These commands set the mode for interpreting coordinates. In ABS mode, coordinates are relative to MILLPWR
G2
’s datum. In INC mode, coordinates are relative to the tool’s position after completing the previous move. The setting applies to current and subsequent blocks.
The default is G90 (ABS)
The BlockForm command is used to define a window in relation to the part zero. This is used by the Draw function to present a solid model of the raw stock. Block Form can be placed anywhere within the program and must be accompanied by all of the parameters.
G120 X(xMax) Y(yMax) Z(zMax) I(xMin) J(yMin) K(zMin)
All other G codes not listed will generate a run-time error.
100
6 Programming
M-Code Definition
The following is a list of available M-Codes. Be advised that many
M-codes are machine dependant, and often machine manufacturers will add, and/or remove some M-Codes.
† Represents supported M-codes.
M-Code List
Description M-Code
M*
†
Comment
All other M codes not listed will generate a run-time error.
M0
† Program Stop
M1
† Optional Program Stop
This command pauses the program. Press GO to resume.
This command pauses the program if the Optional Stop run option is selected. Press GO to resume.
M2
† Program End
This command stops the program after completing of the block. The cursor moves to the beginning of the program. The current settings are reset to default values.
M3
†
M4
†
M5
†
M6
M7
M8
M9
†
†
M30
†
Spindle On (CW)
Spindle On (CCW)
Spindle Off
If spindle control hardware is present, the spindle is turned on or off automatically. If the hardware is not present, the operator is prompted to turn the spindle on or off and/or to set the speed.
Tool Change
M6 is not necessary. A tool change occurs when the Tool Selection command is processed.
Coolant On (Mist)
Coolant On (Flood)
If the AMI hardware is present, the coolant is turned on or off automatically. If the hardware is not present, the operator is prompted to turn the coolant on (mist), on (flood), or off.
Coolant Off
Program End w/ Pallet Shuttle
MILLPWR
G2
does not support control of a pallet changer. This code has the same effect as M2.
ACU-RITE MILLPWR
G2
101
M-Code
M48
M49
M60
Description
Enable Speed/Feed Override
Comment
It is not possible to disable feed rate override on MILLPWR
G2
. These commands are ignored.
Disable Speed/Feed Override
Program Stop w/ Pallet Shuttle
MILLPWR
G2
does not support control of a pallet changer. This code has the same effect as M0.
102
6 Programming
X
†
Y
†
Z
†
K
†
N
†
O
†
I
†
J
†
Other
Addresses
F
†
S
T
†
†
Description Comment
Set Feed Rate
X Axis Coordinate
Y Axis Coordinate
Z Axis Coordinate
The feed rate uses the current program units in effect (ipm or mmpm).
The setting applies to current and subsequent blocks. The default is determined from MILLPWR
G2
's configuration setup.
Arc center coordinate parallel to X axis
Arc center coordinate parallel to Y axis
Arc center coordinate parallel to Z axis
These are the arc center coordinates for G2 and G3 arcs. They are assumed to be programmed in incremental from the current tool position.
Line Number
Program Number
Spindle Speed
Tool Selection
Line numbering is optional and for readability only. MILLPWR
G2
does not make use of this information.
Used at the beginning of a program.
The spindle speed is set to the specified speed (rpm). If the spindle is currently off (M5), it will not be turned on unless accompanied by a spindle direction block (M3 or M4). The setting applies to current and subsequent spindle direction blocks. The default is 0 rpm.
This command is used to select the active tool. The tool is specified by tool number or by its diameter. If the diameter is not specified, it is retrieved from the tool table.
The program pauses at a tool command and prompts the user to complete the tool change. Press GO to resume.
T(toolNumber) D(toolDiameter) L(toolLength)
The coordinates represent the destination for the G0, G1, G2, or G3 command currently in effect. They use the current units (G20/21 or G70/
71) and offset mode (G90 or G91).
ACU-RITE MILLPWR
G2
103
Additional G-code Conventions for MILLPWR
G2
The following lists some of the expectations and limitations of programs ran in MILLPWR
G2
.
Blocks may contain multiple commands and are executed with the following precedence:
Messages
Tool Change
Spindle Control
Coolant Control
Dwell
Motion
Stop
Operator comments should be enclosed in parentheses.
An operator comment with “MSG” appearing within the text is considered a message. The text following “MSG” (up to 60 characters) is displayed to the operator at run-time. Program execution pauses until the operator acknowledges the message by pressing GO. Format is MSG (Operator message) or MSG ("Operator
message").
Parametric programming (use of variables or algebraic operations) is not supported.
Program delimiters (“%”) are ignored. Text following the delimiter is ignored.
White space is ignored between parameters but not within a numeric value or message.
If a coolant command (M7, M8 and M9) appears in the block, the
Operator Intervention Message is displayed regardless of the current coolant setting. If AMI hardware is present, the block will execute without the need for any operator intervention or acknowledgement.
Tool length off set is read from MILLPWR
G2
‘s tool library.
For example: In a G-code file, T1 will use the tool length offset from
Tool #1 in the tool library. T2 will use tool length offset from tool library tool #2, etc.
The skew feature does not work with G-code programs. Remove any skew angle prior to running a G-code program.
104
6 Programming
Backing Up a Program
To back up a program is similar to saving a program. A backup program can be saved to another location (e.g. memory device, or on a network), or to the same program location. If it is saved to the same program location, then it can be with the same name plus an indication in the name that it is a backup copy. The MILLPWR
G2
Copy and Paste functions do this automatically, and is further explained below.
In the same manner, this can also apply to backing up a G-code program.
It is also possible to select all programs in a folder and be saved as a backup to the same folder.
Copy and Paste programs
Press the Program Functions soft key.
Press the Change Window soft key to select the Folder
Tree. Repeat to select the Folder Contents window.
ACU-RITE MILLPWR
G2
105
Use the arrow keys to highlight the program to be copied, then press the Select soft key.
A popup menu will open where either the highlighted program can be selected, or all programs in the folder can be selected. Highlight
Select, or Select All, then press the ENTER key.
If the program that was selected is not the correct one, select the
Clear feature, and press ENTER. The program is un selected, and another program can now be selected.
Press the Function soft key and select Copy from the popup menu, then press the ENTER key.
Press the Function soft key again, and select Paste from the popup menu, then press the ENTER key.
A copy of the selected program has now been copied to the same folder and was named with a suffix of “Copy”. Another folder location could have been chosen before Paste to copy the program to the new location.
If a program is copied multiple times using the Paste function, each pasted program copy would then have sequential numbering
(e.g. Copy, Copy (2), Copy (3), and so on).
Program Errors
When an error is detected in a program, the step with the error is highlighted in the program listing with a red " x " symbol. Edit the program step to correct the error.
Additional information about the error is added to the error log. See
After correcting the errors, remember to delete them from the error log. A quick method for deleting all errors in the log is to press the “0” key.
If there is more than one error in the program, only the first step with an error will be highlighted. After correcting the first error, the next error will be highlighted.
106
6 Programming
Demonstration
Program
7.1 Demonstration Program
Overview
The following steps and key stroke sequences will guide you through creating a demonstration program based upon information from the part drawing shown.
All dimensions are in inches.
This will help introduce you to MILLPWR
G2
and familiarize you with how it operates.
Selecting Datum
Although there is no clear "zero point" identified on this print, use the center of the bolt hole pattern as datum. There are advantages to using this location:
It is the center of the bolt hole pattern
It is the center of the large arc, making it easy to calculate the arc's start and end points.
The pocket is dimensioned from this point, and nearly all of the dimensions on the print originate from this point.
This print could also be programmed using another point such as the upper left corner, for example as datum.
The datum will be ready to set just before running a program.
108
7 Demonstration Program
Begin Programming
From the DRO mode, begin by pressing the DRO/PGM key to enter the PGM mode.
If a program is loaded, save the open program, it does not have to be cleared. This is example is done in INCH mode. Make sure INCH is selected.
Selecting A Tool
The first step for this program is to choose the tool that will be used to begin the machining. For this step, a 1/4” diameter FLAT END MILL will be used.
Press the TOOL key to access the SET TOOL Dialogue.
In the SET TOOL dialogue enter 0.25 in the SIZE / DIAMETER field.
Press ENTER twice or ARROW Down to highlight the TOOL TYPE field.
With the TOOL TYPE field highlighted, press either the right ARROW key, or press the Tool Types soft key to open the TOOL TYPE drop down menu.
ARROW
down to highlight the FLAT END MILL.
Press the ENTER key to select the tool type.
In most dialogues, there is a drop down menu and a soft key available for choosing a selection. This program example will refer to the use of the soft keys when available.
ARROW
down to highlight the SPINDLE field.
Select Forward by pressing the Forward soft key
ARROW
down to highlight the SPEED field and enter 1300 using the numeric keypad.
ARROW
down to highlight the TOOL POSITION field.
Enter -5.00 in the X TO field.
Enter 0.00 in the Y TO field.
Enter 1.00 in the Z TO field.
Press the USE key.
The programming of the part can now begin.
Refer to chapter 8 "Selecting A Tool" on page 127 for more information
about Tool Position.
ACU-RITE MILLPWR
G2
109
Programming a line
For this example, the part will begin at the upper left hand corner, and cut in a clockwise (CW) direction.
Press the LINE key. The cursor will default to the
FROM: X1 field in the MILL LINE dialogue.
Using the numerical keypad, enter the following information:
In the FROM: X1 field enter -3, and press the ARROW Down key.
In this case, pressing the ENTER key twice is required to move the cursor down to the next field because a negative number was entered. The arrow key accomplishes the same result with one press of the key.
In the FROM: Y1 field enter 1.5, and press the ARROW Down key.
In the TO: X2 field enter 0, and ARROW Down.
In the TO: Y2 field enter 1.5, and ARROW Down.
In the Z: BEGIN field enter .02, and ARROW Down.
In the Z: END field enter -.25, and ARROW Down.
ARROW
Down to the OFFSET: field and press the Left soft key.
Notice that the ANGLE and TOOL specifications were filled in automatically. The tool specifications were taken from the information entered in Step 001.
To cut around the outside of the contour in a clockwise direction, a left offset is used. MILLPWR
G2
has been factory set with a feed rate of 10 inches per minute, and is used for this operation.
Press the USE key.
The line is now displayed on the Program (PGM) screen and in the graphics area.
Next, the arc will be added to the program.
If it is preferred to see the complete material work piece size for program verification, press the VIEW key, then press the Block Form soft key. In the BLOCK FORM dialogue enter the overall blank size for the part, or cutting piece. MILLPWR
G2
will calculate the block form as the program is entered.
110
7 Demonstration Program
Programming an Arc
Press the ARC key. The cursor defaults to the TO: X1 field in the MILL ARC dialogue.
MILLPWR
G2
assumes that the program is continuing from the last step, so it automatically fills in the FROM: X1, and Y1 fields, the
Z: fields, TOOL: fields, FEED: fields, and the OFFSET field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter 0, and ARROW Down.
In the TO: Y2 field enter -1.5, and ARROW Down.
In the RADIUS: MINOR field enter 1.5 and ARROW Down.
In the DIRECTION: field, press the CW soft key.
Since this arc will be starting at the top and moving out, and around to the bottom, the arc will be machined in a clockwise direction.
Press the USE key.
Saving the program:
At this point, enough information has been entered that the program can be saved and given a name.
Press the Save / Discard soft key.
Select Save from the popup menu.
Enter the program name in the popup keyboard using the ARROW
keys. Name the program DemonstrationProgram.MPT. See
"Saving a Program" on page 91 in the previous chapter for more
information.
Press the Save / Create soft key.
Next, the lower horizontal line will be programmed.
ACU-RITE MILLPWR
G2
111
Programming the connecting Line
Step 001 is now highlighted. ARROW Down to the last blank step number (004) to highlight that step.
The next step to program is the line that starts at the bottom of the arc.
Press the LINE key.
Again, MILLPWR
G2
assumes that the program is continuing from the last step. So it has automatically filled in the FROM: X1, and Y1 fields, the Z: fields, TOOL: fields, FEED: fields, and the OFFSET field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter -3.0, and ARROW Down.
In the TO: Y2 field enter -1.5, and ARROW Down.
Press the USE key.
Now that the upper edge, arc, and lower line have been created, the following steps will close the contour.
First the lower vertical line will be added.
112
7 Demonstration Program
Programming the lower vertical Line
Next, the line that starts vertical from the bottom line at the end of the arc will be entered.
Press the LINE key.
Again, MILLPWR
G2
assumes that the program is continuing from the last step. So it has automatically filled in the FROM: X1, and Y1 fields, the Z: fields, TOOL: fields, FEED: fields, and the OFFSET field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter -3.0, and ARROW Down.
In the TO: Y2 field enter -.838, and ARROW Down.
Press the USE key.
Next, the lower angled line will be added.
ACU-RITE MILLPWR
G2
113
Programming the lower angle Line
Next, the line that angles in to the part from the lower vertical line will be added.
Press the LINE key.
MILLPWR
G2
has again assumed that it will continue from where it left off, and all fields are filled in except for the TO: fields. The cursor is also located here, in the first field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter .75.
Now press the ABS/INCR key.
The INC field next to the X2 field has opened. Press the X1 soft key.
X1 is displayed in this field next to the X2 field.
ARROW
Down once to the Y2 field.
In the TO: Y2 field enter 0.00.
If the X1 soft key had not been pressed, then INCR would not have been used, and MILLPWR
G2
would assume that
ABS is to be continued.
Press the USE key.
Next, the upper angle line will be added to the program.
114
7 Demonstration Program
Programming the upper angle Line
The upper line that angles away from the part will now be added.
Press the LINE key.
With MILLPWR
G2
assuming that it is continuing from where it was left off, all fields are filled in except for the TO: fields. Which is also where the cursor is located in the first TO: field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter -3.0, and ARROW Down.
In the TO: Y2 field enter .838.
Press the USE key.
Although changes are not lost if a power cycle occurs, you may wish to save your program periodically while creating it, or you may want to discard the most recent changes made since the last save.
Press the Save / Discard soft key.
Select Save from the popup menu to save the program, or select discard to delete the most recent changes since the last save.
Next, a blend will be added to the two angled lines.
ACU-RITE MILLPWR
G2
115
Programming a Blend
In this step, a BLEND will be inserted between program steps 6 and 7.
ARROW
up one step to highlight program step 7.
Press the BLEND key.
In the TYPE field be sure that Blend is selected.
Program Step 7 has now moved to program Step 8, and the BLEND program step is now Step 7.
Also notice that the continuous line in the program steps between steps 6 and 8 is now broken. This indicates that these steps will be blended.
ARROW
down to the RADIUS: field, and enter .25.
Leave the CONTOUR field set at the default setting of OPEN.
Press the USE key.
The two angled lines are now blended with a .25 radius, and the line in the programming steps is now continuous from Step 2 through
Step 8.
The blend step could have been added prior to adding the next line in the program step, but it would not have been displayed until the connecting line was added.
Press the down ARROW key to Step 9 (last step in the program) to continue with the program.
The following step will close the contour of the part.
116
7 Demonstration Program
Closing the contour
The contour of the part will now be closed, and all milling steps entered will be one continuous machining operation.
Press the LINE key.
As MILLPWR
G2
assumes that you are continuing from where it was left off, all fields are filled in except for the TO: fields. Which is also where the cursor is located in the first TO: field.
Using the numerical keypad, enter the following information:
In the TO: X2 field enter -3.0, and ARROW Down.
In the TO: Y2 field enter 1.5.
Press the USE key.
The contour of the part is now complete. You may notice that the tool path shows a double radius where the tool started, and then ended.
This is because the program is dimensioning the center of the tool.
The continuous line along the program steps has now changed to a closed rectangle. This represents that the contour is now closed. This happens when the TO point of the last step is the same as the FROM point of the first step.
ACU-RITE MILLPWR
G2
117
Tool Change for the Bolt hole Pattern
Begin first by changing the tool.
Press the TOOL key. The tool form will open with the cursor in the SIZE: DIAMETER field.
Enter 0.25 in the SIZE: DIAMETER field using the numeric keypad.
Press ARROW Down to highlight the TOOL TYPE field (the LENGTH field will be left blank).
In the TOOL TYPE field, press the Tool Types soft key to open the
TOOL TYPE drop down menu.
ARROW
down to highlight the DRILL.
Press the ENTER key to select the tool.
ARROW
down to highlight the SPINDLE field.
Press the Forward soft key.
ARROW
down to enter the selection, and move to the RPM field.
Enter 1300 (e.g. example) using the numeric keypad, and ARROW down to the REQUIRE CHANGE field.
Press the Yes soft key.
Press the USE key.
A new tool has now been added to the program, and the previous tool will need to be changed when running the program. The program, when running, will stop at this point, and request the tool change before continuing.
118
7 Demonstration Program
Programming the Bolt circle
Press the HOLES key.
A popup menu will appear for selecting the type of hole pattern to be used.
Select the Bolt Circle selection. The BOLT CIRCLE input dialogue will be displayed.
In the CENTER X field enter 0.00, and Y field enter 0.00. For this program it is also the CENTER location for the Bolt Circle (which is also where datum X 0 and Y0 was set).
ARROW
down to highlight the Z: END field, and press the CLEAR key to delete the default data in the field that may be present.
Enter a value of -.40 in the Z: END field.
ARROW
down to highlight the PECK field, and enter 6 for the
NUMBER.
ARROW
down to highlight the RADIUS field. Press the CLEAR key to delete any default data in the field, then enter 0.75.
ARROW
down to highlight the DIRECTION field, and press the CW
(Clockwise) soft key.
ARROW
down to highlight the HOLES field, and enter 5.
Press the USE key.
In this example, the starting and ending angles were not changed. As a result, the first hole is placed at zero degrees. If you were to look at the face of a clock, zero degrees will be at 3 o’clock. Without a specified ending angle MILLPWR
G2
spaces the number of holes entered evenly around a full circle. If a counter-clockwise direction was applied to the hole pattern, the second hole of our five hole pattern will be between 12 o’clock and 1 o’clock. The holes continue around the circle as shown below.
ACU-RITE MILLPWR
G2
119
Tool Change for the Rectangular Pocket
Begin by changing the tool.
Press the TOOL key.
In the SET TOOL dialogue enter 0.125 in the SIZE: DIAMETER field.
ARROW
Down to highlight the TOOL TYPE field.
With the TOOL TYPE field highlighted, press the Tool Types soft key to open the TOOL TYPE drop down menu.
ARROW
down to highlight the FLAT END MILL.
Press the ENTER key to select the tool.
ARROW
down to highlight the SPINDLE field.
Select Forward by pressing the Forward soft key
ARROW
down to highlight the RPM field and enter 1300 using the numeric keypad.
ARROW
down to highlight the REQUIRE CHANGE field and press the Yes softkey.
Press the USE key.
A new tool has now been added to the program, and a tool change will be required when running the program.
The program, when running, will stop at this point, and request the tool change before continuing.
The rectangular pocket, which is the final feature, can now be programmed.
120
7 Demonstration Program
Programming the Rectangular Pocket
Press the RECT key.
A popup menu will appear for selecting the type of rectangle to be milled.
Highlight Pocket and press the ENTER key. The RECTANGLE
POCKET dialogue will be displayed. The cursor will default to the
first field (X1).
In the 1st CORNER: X1 field enter -2.0.
In the 1st CORNER: Y1 field enter -1.0.
ARROW
down to SIZE: X field and enter 0.5
ARROW
down to SIZE: Y field and enter 2.0.
The 2nd CORNER fields will automatically fill in based on the data from the 1st CORNER: fields, and the SIZE: fields.
The Z: begin field, and Z: End field inserts the same information that was entered for the BOLT CIRCLE dialogue information.
ARROW
down to highlight the Z: BEGIN field and enter .100.
ARROW
down to highlight the Z: END field and enter -.25.
ARROW
down to highlight the Z: PASS field, and enter 4 for the
NUMBER.
ARROW
down to the CORNER BLEND RADIUS: field, and enter 0.125.
ARROW
down to highlight the DIRECTION field, and select CW
(Clock Wise) by pressing the CW soft key.
Press the USE key.
The demonstration program is now complete.
Save the program, replacing the existing program.
ACU-RITE MILLPWR
G2
121
Testing the Program
Whenever a new program has been created, it should always be tested first.
Graphics only
The following steps will run the program graphically only, and there will be no table movement.
Press the Run Options soft key.
Press the Graphics Only soft key.
Use the arrow up key to highlight step 001 of the program.
Press the Exit soft key.
Press the GO soft key (there will be no table movement). The part machining steps will be shown in the display graphics.
Dry Run with table movement
The complete program will be run, and the cutting of the part will be displayed graphically as the program steps are being performed.
The following steps will run the program graphically, and the table will move.
Before you press the GO key to begin the dry run, ensure that the tool will not touch the workpiece when the quill begins to move. To avoid tool interference, do one or more of the following:
- Lower the knee
- Remove the tool or workpiece
- Reestablish datum away from the part
122
7 Demonstration Program
Press the Run Options soft key.
Press the Graphics Only soft key to display the machining steps. Displaying the graphics is not required, but can be of assistance when executing the dry run feature.
Press the Dry Run soft key.
Use the arrow up key to highlight step 001 of the program.
Press the Exit soft key.
Press the GO soft key (the table will move).
Running the Program
The first step in running a new program is to establish datum.
Remember to chose the center of the bolt circle as datum.
Place the workpiece into a vise.
Place the first tool of the program into the spindle.
From the DRO screen, press the Move Table soft key. Using the arrows, and soft keys, position the workpiece under the tool where the center of the bolt circle’s datum is to be.
After the table has been properly positioned, press the Exit soft key to return to the DRO screen.
Touch the tool to the top surface of your workpiece.
Press the Datum soft key.
Press the X = 0, Y = 0 and Z = 0 soft keys to establish the current tool position as datum.
Press the DOWN ARROW key.
Set the Z retract position 1” above the workpiece.
Press the USE key.
ACU-RITE MILLPWR
G2
123
Tool Changes
Whenever you encounter a SET TOOL step, MILLPWR
G2
will display the DRO screen and let you know which tool to load. If no tool diameter was programmed in the Tool Step, a prompt will be displayed to provide one.
Use the Move Table soft key and ARROW keys to move the workpiece away from the tool.
Insert the required tool into the spindle.
Using the Move Table soft key, position the surface of a known depth on the workpiece under the tool.
Press the Datum soft key.
Position your tool so that it touches a known surface, then enter that position into the Z axis.
Press the USE key.
Raise the tool and press the GO key to continue the program.
Clearing the Program
Press the DRO/PGM key to return to the Program mode.
Press the Clear Program soft key.
Press the Yes soft key to confirm exiting the program.
The program is cleared from the screen, and at any time another program can be loaded or a new program written.
If a program is loaded, and saved, it does not have to be cleared to open a new program.
If for some reason a program can not be cleared with the
Clear Program
soft key, there is an alternate method.
Cycle the power to the console. While at the home (DRO mode) screen, prior to finding home, press and hold the
CLEAR
key for 5 seconds.
Follow the instructions to clear the current program.
124
7 Demonstration Program
Milling and Drilling
8.1 Milling and Drilling
Overview
Most of the program steps described in this section can be performed as one-step milling functions from the DRO screen or be included as steps in a program. Many of the dialogues are similar in the way that the data is entered. Much of the information in this chapter should be familiar after performing the demonstration program in Chapter 7.
SET TOOL defines the tool and should appear as the first step in a program. A SET TOOL step is required anywhere a tool change is required. MILLPWR
G2
will apply the latest tool setting to the program
steps that follow. See "Selecting A Tool" on page 109 as the following
information is very similar.
Warning: Spindle speeds used in this manual are for
example only. A spindle speed is totally dependant on many factors (i.e. material, if coolant is used, tool diameter, etc.). The speeds listed are not meant to be a recommendation.
For complete information regarding a 2 Axes system Refer to
Chapter 1, "Operating in 2 Axes and 3 Axes Modes" on page 9.
126
8 Milling and Drilling
Selecting A Tool
The first step for a program is to choose the tool that will be used to begin the machining. For this example, a 1/4” diameter FLAT END
MILL will be used as an example.
Press the DRO/PGM key to enter PGM mode.
Press the Program Steps soft key.
Press the Tool soft key to open the SET TOOL
Dialogue.
In the SET TOOL dialogue the cursor defaults to the SIZE:
DIAMETER field. Enter 0.25 in the SIZE / DIAMETER field.
Select the unit of measure using the Inch or MM soft keys if a change is required.
ARROW
DOWN to highlight the TOOL TYPE field. The LENGTH: field will be left blank.
Though in most cases, pressing the ENTER key will enter the data into the field, and place the cursor into the next field, the ARROW keys will be used in these steps for navigation, and entering data.
With the TOOL TYPE field highlighted, press the Tool Types soft key to open the TOOL TYPE drop down menu.
ARROW
DOWN to highlight the FLAT END MILL.
Press the ENTER key to select the tool.
In most dialogues that contain a drop down menu, there are soft keys available for choosing a selection. These examples will refer to the use of the soft keys when available.
ACU-RITE MILLPWR
G2
127
ARROW
DOWN to highlight the SPINDLE: field.
Press the Forward soft key
ARROW
DOWN to the SPEED: field (RPM) and enter the speed required
(e.g. 1300) using the numeric keypad.
ARROW
DOWN to tool position and enter the location where it is best to make a tool change away from the part and fixtures.
MILLPWR
G2
moves to the TOOL POSITION before prompting the user for a tool change, making it unnecessary to program a POSITION/DRILL step before a tool change.
ARROW
DOWN to the REQUIRED CHANGE field and select YES, or NO.
MILLPWR
G2
prompts the user to change the tool if the
SET TOOL step has a different tool than the one currently mounted (as indicated in the status bar). If the REQUIRE
CHANGE field is set to YES, then MILLPWR
G2
will always pause and prompt the user for a tool change (even if the
SET TOOL matches the currently mounted tool).
Press the USE key.
The programming of a part can now begin.
Tool length offsets are discussed on the following pages.
If the TOOL TABLE is used to enter a tool, MILLPWR
G2 will fill in the DIAMETER, and LENGTH fields in PGM mode only.
128
8 Milling and Drilling
Repeatable Tool Length Offsets
Programming a Tool
When a program is using the Tool Length function, there are two requirements that must be followed to ensure that the tip of all additional tools is actually where MILLPWR
G2
has calculated it to be.
All tools used must have a fixed, repeatable length.
The surface that the tool touches off on must be a repeatable surface and used for all tools added to the program.
This also applies to all tools added to the Tool Table.
Setting the Datum using an electronic edge finder is for illustration only, and is not a requirement.
Press the Datum soft key.
Touch the first tool to the top surface that will be used to set all other tools.
Press the Z = 0 soft key.
The Z axis Datum is now set to 0.00.
All tools entered into the tool table will have length offsets relative to the first tool Datum. All tools entered after the first tool, whether into the tool table or into a program should have their length set using the
Teach Tool Length
soft key.
Once you have identified the tools you will be using, you can program the Tool Length Offsets into the SET TOOL steps.
When all tools have been added to a program with their tool length offset programmed, MILLPWR
G2
will retain the offset information between each tool and the Datum.
If a program that is using tool offsets requires a change from where the initial first tool datum was set, MILLPWR
G2
will reset the offset information for the remaining tools.
When setting a the Datum, consideration of the height of the new location can avoid possible tool collision with the part when running the program. If necessary, reset the Z Retract height.
Tools, and their offsets can be used from the Tool Table, and inserted into a program. The Datum for the program can be set at a new location as mentioned above. MILLPWR
G2
will reset the offset information for the remaining tools to the new location. Their offset will stay relevant to the new Datum.
After the tool information is established in the program, later you can edit the values as needed to adjust for accuracy and wear.
Changing to a Tool of unknown length in DRO mode
If you are in the DRO mode and need to set a new tool, do the following:
Place the tool in the spindle.
From the DRO mode, press the TOOL key.
Enter the tool diameter, delete any data in the LENGTH field.
ACU-RITE MILLPWR
G2
129
Enter the necessary data in the remaining fields where applicable.
Press the GO key.
An Operator intervention message will appear asking you to “use” the selected tool.
Press the GO key to confirm that you have installed the tool.
At this point, your program’s tool length offsets are not valid. Follow the steps below to reestablish the Z axis datum and tool length offsets for your program.
Position the tool over the surface where the Datum was established for the other tools.
Touch the tip of the tool to the top surface.
Press the Teach Tool Length soft key.
MILLPWR
G2
will now add this tool to the known tool offsets, and the program’s tool length offsets are now valid.
This tool length offset is only valid while the tool is mounted. Once this tool is removed, these steps must be repeated to re-establish the tool length when it is used again.
130
8 Milling and Drilling
Changing to a Tool of unknown length in a program
When running a program, it is possible to switch between tools of known length, to using a tool that has a non-repeatable length.
When the tool which has a non-repeatable length is mounted, it’s length will be established in the same manner as above in DRO mode.
Place the tool in the spindle.
In the SET TOOL Dialogue, enter the necessary data in the fields where applicable, but delete any data in the LENGTH field.
Press the USE key.
At this point, your program’s tool length offsets are no longer valid. perform the following steps to reestablish the Z axis datum and tool length offsets for the program.
Position the tool over the surface where the Datum was established for the other tools.
Touch the tip of the tool to the top surface.
Press the Teach Tool Length soft key.
MILLPWR
G2
will now add this tool to the known tool offsets, and the program’s tool length offsets are now valid.
This tool length offset is only valid while the tool is mounted. Once this tool is removed, these steps must be repeated re-establish the tool length when it is used again.
By resetting Datum during a tool step within the program, all of the tool offsets in the program become valid again.
ACU-RITE MILLPWR
G2
131
Position / Drill
The Position / Drill function will move the table to specific position based upon the X and Y axes coordinates entered.
From the PGM screen, press the Pos key to access the
POSITION / DRILL Dialogue.
In the POINT field enter the X and Y axes coordinates.
In the Z field enter the BEGIN and END depths.
Enter either the number of pecks or the distance between each peck (also know as Chip Break). If the option wanted is not displayed, go to Job Setup and select the other.
Select the job option to be used: DRILL, BORE, or POSITION using the soft keys, or from the drop down menu.
DRILL: Basic drilling cycle is generally used for center drilling or hole.
BORE: Generally used to make a pass in each direction on a bore or to tap with a self-reversing tapping head. It feeds from the begin depth to Z depth, and then feeds back to the retract height.
POSITION: Data can be entered to move the table to a position in the X & Y direction. Z moves are done manually.
Enter the Z axis feed rate. The default FEED IPM rate provided must be adjusted according to the current machining operation. This field will automatically use the last entered feed rate in the program
If you want the tool to retract enter either the number of retracts or the distance between each retract.
Enter the length of time (in seconds) the tool should dwell (pause) after it has retracted out of the part.
Enter the length of time (in seconds) the tool should dwell at the end depth before the final retract.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running the program or one-step milling function.
132
8 Milling and Drilling
Line
Lines are defined by their “From” point (the point where they begin) and “To” point (the point where they end).
There are two ways you can program a line:
With four coordinates (X1, Y1, X2, Y2).
With three of the coordinates above (X1, X2, Y2 or X1, Y1, X2, etc.) and an angle.
Choose a method based upon the information available from your print.
Entering Data:
From the PGM screen, press the LINE key to access the
MILL LINE Dialogue.
Enter the beginning X and/or Y axes coordinates into the FROM field.
Enter the ending X and/or Y axes coordinates into the TO field.
Enter the BEGIN and END depths for the Z axis.
Enter the Z axis feed rate. The default FEED ... IPM rate provided must be adjusted according to the current machining operation. This field will automatically use the last entered feed rate in the program.
If one of the X- or Y-axes fields above was left blank, enter an angle.
Highlight the Offset field and press the LEFT, CENTER, or RIGHT soft key.
Enter the table’s feed rate. The default feed rate is what was entered into JOB SETUP dialogue.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running the program.
ACU-RITE MILLPWR
G2
133
Arc
An arc can be defined several ways:
With a From point, To point and a radius
With a From point, To point and a center point
With a From, To and a 3rd point along the arc
With a start point to an end point for a sweep angle
Choose a method based upon the information available from part drawing. While programming, keep in mind that the arc's sweep angle is measured from the X axis.
Entering Data:
From the PGM screen, press the ARC key to access the
ARC Dialogue.
Enter the beginning coordinates for the X axis (X1) and Y axis (Y1) in the FROM field.
Enter the ending coordinates for the X axis (X2) and Y axis (Y2) in the
TO field.
Enter the begin and end depths for the Z axis.
Enter the Z axis feed rate.
Enter the arc's radius, then press either the Major Arc or Minor Arc soft key. (A Major Arc has a sweep angle greater than 180 degrees; a Minor Arc’s sweep angle is less than 180 degrees.)
Select the cutting direction. Press the CW soft key for a clockwise direction or the CCW soft key for a counter-clockwise direction.
ARROW
down and highlight the OFFSET field. Using the soft keys, select the tool offset— Left, Center, Right, Inside or Outside.
Enter the table’s FEED IPM.
134
8 Milling and Drilling
If you need to enter a center coordinate, 3 rd
point and/or sweep angle press the More soft key:
CENTER field:
Enter the center coordinate’s position for the X and Y axes.
3 rd
POINT field:
Enter your 3 rd
coordinate’s position for the X axis (X3) and Y axis
(Y3).
SWEEP ANGLE field:
Enter the sweep angle.
Information that appears in blue has been calculated. If any of these values are already displayed in blue, then MILLPWR
G2
has enough data for the arc and has calculated the rest.
Press the USE key.
Note: If the tool size and type listed in the Tool field are incorrect, change the tool settings before running the program.
Blend/Chamfer
A blend is an arc that connects two lines, two arcs or a line and an arc.
Provide the radius for the blend. The tangent points will then be calculated.
The two steps to be blended can, but don't have to, intersect or touch.
If they don't come into contact with each other, check that the radius is large enough to connect them.
It's also possible to close a contour (e.g., a triangle) using the blend feature by inserting a blend step immediately after the last step in the contour.
Enter the blend's radius, press the Close Contour soft key, and
MILLPWR
G2
will blend the last step with the first step.
ACU-RITE MILLPWR
G2
135
Blend
Highlight a step within your program where you want to place a blend.
The blend step can be added prior to adding the connecting line in the program step, or between two connecting lines. When placed before the connecting line is added, it will not be displayed until the connecting line is placed in the program.
From the PGM screen, press the BLEND key to access the BLEND Dialogue.
Confirm that Blend is selected in the soft key.
Check that the steps listed in the FROM and TO fields are the steps to be blended. If they're incorrect, press the CANCEL key and highlight the appropriate step.
Enter the blend's radius.
Press the Close Contour soft key to blend the end of a contour with the beginning. The step numbers in the TO and FROM fields will automatically change.
Press either the Normal Arc or Inverted Arc soft key. A normal arc curves outward; an inverted arc curves inward.
Enter the table’s feed rate.
Press the USE key.
Chamfer
A Chamfer is done in the same way, but with less steps. In the SIZE field enter the length of the chamfer.
A chamfer is a bevel or line that’s inserted between two lines to relieve sharp angles or corners on a part. A chamfer can be inserted between two intersecting lines whose steps are adjacent in the program step.
A chamfer can also close a contour (e.g., a triangle) by inserting the chamfer step immediately after the last step in the contour.
136
8 Milling and Drilling
From the PGM screen, locate the lines where the chamfer is to be inserted between.
Highlight the second line.
Press the BLEND key.
Press the Chamfer soft key after the dialogue opens.
MILLPWR
G2
will automatically fill in the FROM and TO fields in
STEPS for you.
Enter the distance from the common point of both lines. LENGTH is the distance from the end points at which the chamfer will be inserted.
Press the Open Contour soft key to chamfer the end of a contour with the beginning.
Press the USE key.
ACU-RITE MILLPWR
G2
137
Rectangular Milling Functions
MILLPWR
G2
offers several rectangular milling functions that let you
Rectangle Pocket
A pocket is a cavity or area on the part where material is removed when you machine. You can program a rectangular pocket two ways:
Using the coordinates of two diagonal corners.
Using the coordinates of one corner and the size of the pocket. The
X and Y size can be positive or negative dimensions which allows the 1st corner to be any of the corners of the pocket.
From the PGM screen, press the RECT key to access the
RECT
popup Menu.
Select Pocket from the popup Menu.
Entering Data
Enter the 1st CORNER X1 and Y1 axes coordinates.
Now enter either the SIZE of the pocket or the 2nd CORNER coordinates.
Either data entry will automatically fill in the fields for the other option.
To enter the SIZE, enter the length of the pocket along the X and Y axes.
Or enter the X and Y axes coordinates for the 2nd CORNER. The 2nd corner must be located diagonally from the 1st corner.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate.
Add a corner blend radius to the corners of the rectangular pocket.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
138
8 Milling and Drilling
ARROW
down or press the More soft key and enter the table’s feed rate.
If you need to program a corner blend radius, tilt angle and/or finish cut:
You can tilt a rectangular pocket by identifying a tilt angle. Highlight the ANGLE field and enter an angle measured from the X axis.
Finish
Finish allows you to leave some excess material that will be removed during the finish cut reducing tool marks. The finish cut will automatically arc on and arc off.
Enter the amount of material to be removed during the finish cut in the CUT field.
Enter the FEED rate for the finish cut.
Select the finish cut’s DIRECTION. Press the CW soft key for a clockwise direction or the CCW soft key for a counter-clockwise direction.
Enter a stepover percentage (what percent of the tools diameter is to pass over the previous cut).
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
Tool Path Description:
Machining of the rectangle pocket begins at its center.
The tool plunges at the Z feed rate.
The pocket is milled from the center out.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts slightly (0.01" or 2 mm) between Z passes.
A finish allowance is optional. If specified, this amount is left on the bottom and sides of the pocket to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped. Finish direction applies only to the side finish.
ACU-RITE MILLPWR
G2
139
Rectangle Frame
When you program a rectangular frame, you define it by its first corner, and its size or diagonal corner. You can program a frame in one of two ways:
Using the coordinates of two diagonal corners.
Using the coordinates of one corner and the size of the pocket.
To program a rectangular frame:
From the PGM screen, press the RECT key to access the
RECT
popup Menu.
Select Frame from the popup Menu.
Entering Data:
Enter the 1st CORNER X1 and Y1 axes coordinates.
Now enter either the SIZE of the pocket or the 2nd CORNER coordinates.
Either data entry will automatically fill in the fields for the for the other option.
To enter the SIZE, enter the length of the pocket along the X and Y axes.
Or enter the X and Y axes coordinates for the 2nd CORNER. The 2nd corner must be located diagonally from the 1st corner.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the frame to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate.
140
8 Milling and Drilling
Add a corner blend radius to the corners of the rectangular frame.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
ARROW
DOWN or press the More soft key and select the TOOL OFFSET.
ARROW
DOWN or press the More soft key and enter the table’s feed rate.
You can tilt a rectangular frame by identifying a tilt angle. Highlight the ANGLE field and enter an angle measured from the X axis.
Finish:
Finish allows you to leave some excess material that will be removed during the finish cut reducing tool marks. The finish cut will automatically arc on and arc off.
Enter the amount of material to be removed during the finish cut in the CUT field.
Enter the FEED rate for the finish cut.
Select the finish cut’s DIRECTION. Press the CW soft key for a clockwise direction or the CCW soft key for a counter-clockwise direction.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
Tool Path Description:
Machining of the frame begins at the center of the line forming the top of the rectangle.
The tool plunges at the Z feed rate.
The frame is milled in the direction programmed (CW or CCW)
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The side finish allowance is optional and is only applicable to frames with a tool offset. If specified, this amount is left on the side of the frame to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped.
ACU-RITE MILLPWR
G2
141
Rectangle Face
The “Rectangle Face” step provides a quick way to face off your workpiece. Simply enter the coordinates from one corner and either the size of the area to be faced off or the coordinates for a diagonal corner. MILLPWR
G2
will position your table at the lower left end of the area you've programmed.
You can program a rectangle face in one of two ways:
Using the coordinates of two diagonal corners.
Using the coordinates of one corner and the size of the pocket.
To program a rectangular face:
From the PGM screen, press the RECT key to access the
RECT
popup Menu.
Select Face from the popup Menu.
Entering Data:
Enter the 1st CORNER X1 and Y1 axes coordinates.
Now enter either the SIZE of the pocket or the 2nd CORNER coordinates.
Either data entry will automatically fill in the fields for the for the other option.
To enter the SIZE, enter the length of the pocket along the X and Y axes.
Or enter the X and Y axes coordinates for the 2nd CORNER. The 2nd corner must be located diagonally from the 1st corner.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate.
ARROW
down or press the More soft key.
You can tilt the face by identifying a tilt angle. Highlight the ANGLE field and enter an angle measured from the X axis.
Enter a stepover percentage (how much the tool to is to overlap on each pass) for the FINISH pass.
142
8 Milling and Drilling
Tool Path Description:
Machining of the face begins near the first corner.
The tool plunges at the Z feed rate.
The tool makes back and forth passes in the XY plane along the defined length of the face. Tool motion extends beyond the ends of the rectangle by an amount equal to the tool radius.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts to the active datum's retract position between Z passes.
ACU-RITE MILLPWR
G2
143
Rectangle Slot
You can program a slot two ways:
By entering the center point of each arc and the slot's width
By entering the center point of one arc, the length and width of the slot, and an angle.
Choose a method based upon the information available from your print.
To program a slot:
From the PGM screen, press the RECT key to access the
RECT
popup Menu.
Select Slot from the popup Menu.
Entering Data:
Enter the 1st ARC CENTER X1 and Y1 axes coordinates.
Now enter the size of the pocket in the 2nd ARC CENTER fields X2 and Y2 axes coordinates.
Enter the BEGIN and END depths for Z. If this information was entered on a previous program step, it will automatically be displayed. If necessary, adjust the data for this program step.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
Enter the SLOT WIDTH. The slot length will automatically be calculated.
ARROW
DOWN or press the More soft key and enter the table’s feed rate.
144
8 Milling and Drilling
The TOOL fields will automatically be filled in with the current tool loaded. If a different tool is to be used, enter a SET TOOL step prior to this program step.
You can tilt a rectangular slot by identifying a tilt angle. Highlight the
ANGLE field and enter an angle measured from the X axis.
The FINISH fields will assume the same as the previous finish fields in the program if it exists. Otherwise this data must be added if necessary to include it. Leave it blank if it is not required.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
Enter a stepover percentage (how much the tool to is to overlap on each pass).
Press the USE key.
Tool Path Description:
Machining of the slot begins at its first center location.
The tool plunges at the Z feed rate.
The slot is milled from the center out.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts slightly (0.01" or 2 mm) between Z passes.
A finish allowance is optional. If specified, this amount is left on the bottom and sides of the pocket to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped.
Finish direction applies only to the side finishes.
ACU-RITE MILLPWR
G2
145
Circular Milling Functions
MILLPWR
G2
offers several circular milling functions that let you
program pockets, frames, ring, and helix. Refer to Chapter 1,
"Operating in 2 Axes and 3 Axes Modes" on page 9 for information
regarding 2 Axes Systems.
Circle Pocket
A pocket is a cavity or area on your part where material is removed when you machine. You can program a circular pocket by indicating the center point and radius.
To program a circular pocket:
From the PGM screen, press the CIRCLE key to access the Circle popup Menu.
Select Pocket from the popup Menu.
Entering Data:
Enter the X and Y axes coordinates for the center of the pocket.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the radius.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
The TOOL fields will automatically be filled in with the current tool loaded.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed.
146
8 Milling and Drilling
ARROW
DOWN or press the More soft key.
The FINISH fields will assume the same as the previous finish fields in the program if it exists. Otherwise this data must be added if required, or leave it blank if not required.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
Enter a stepover percentage (how much the tool to is to overlap on each pass). The last stepover percentage used previously in the program will be displayed
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
Tool Path Description:
Machining of the ring begins near the inner radius and works outward.
The tool plunges at the Z feed rate.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts to the active datum's retract position between Z passes.
A finish allowance is optional. If specified, this amount is left on the bottom and sides of the pocket to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped. Finish direction applies only to the side finishes. To match cutting convention the outer radius is machined in the opposite direction of the inner radius.
ACU-RITE MILLPWR
G2
147
Circle Frame
A frame is a cavity or area on your part where material is removed when you machine. You can program a circular frame by indicating the center point and radius.
To program a circle frame:
From the PGM screen, press the CIRCLE key to access the Circle popup Menu.
Select Frame from the popup Menu.
Entering Data:
Enter the X and Y axes coordinates for the center of the frame.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the frame to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed.
Enter the radius.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
The TOOL fields will automatically be filled in with the current tool loaded.
Select the OFFSET from the drop down menu, or the soft keys Left,
Center
, Right, Inside, Outside.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed.
148
8 Milling and Drilling
ARROW
DOWN or press the More soft key.
The FINISH and FEED fields will assume the same as the previous finish fields in the program if it exists. Otherwise this data must be added if required, or leave it blank if not required.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
Tool Path Description:
Machining of the frame begins at the top of the circle.
The tool plunges at the Z feed rate.
The frame is milled in the directions programmed (CW or CCW)
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The side finish allowance is optional and is only applicable to frames with a tool offset. If specified, this amount is left on the side of the frame to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped.
ACU-RITE MILLPWR
G2
149
Circle Ring
A ring is a circular pocket with a circular island in the center. A ring is determined by its center point, outside radius (radius of the pocket) and inside radius (radius of the island).
The direction of the cut on the inside radius will determine whether you are climb cutting or conventional cutting. MILLPWR
G2
will reverse the tool direction on the outside radius so that the cutting direction stays the same.
From the PGM screen, press the CIRCLE key to access the Circle popup Menu.
Select Ring from the popup Menu.
Entering Data
Enter the X and Y axes coordinates for the center of the ring using the ARROW DOWN key to enter the data, and move to the next field.
Enter the BEGIN and END depths for Z.
Enter either the number of passes or the distance between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. Which choice is shown in the dialogue was selected in Job Setup.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed.
In the RADIUS field enter the OUTSIDE radius, then enter the
INSIDE radius.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
The TOOL fields will automatically be filled in with the current tool loaded.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed. Select RAPID for a dry run without a tool by using the Rapid soft key, or select from the drop down menu.
150
8 Milling and Drilling
ARROW
DOWN or press the More soft key.
The FINISH and FEED fields will assume the same as the previous finish fields in the program if it exists. Otherwise this data must be added if required, or leave it blank if not required.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
Tool Path Description:
Machining of the ring begins near the inner radius and works outward.
The tool plunges at the Z feed rate.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts to the active datum's retract position between Z passes.
A finish allowance is optional. If specified, this amount is left on the bottom and sides of the pocket to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped. Finish direction applies only to the side finishes. To match cutting convention the outer radius is machined in the opposite direction of the inner radius.
ACU-RITE MILLPWR
G2
151
Circle Helix
The circle helix can only be performed with a 3 axes system.
A helix is defined by one of two ways:
By the radius, depth and pitch
By the radius, depth and number of revolutions
To program a helix:
From the PGM screen, press the CIRCLE key to access the CIRCLE popup Menu.
Select Helix from the popup Menu.
Entering Data
In the CENTER field enter the X and Y axes coordinates for the center of the helix using the ARROW DOWN key to enter the data, and move to the next field.
Enter the BEGIN and END depths for Z.
In the RADIUS field enter the radius.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
The PITCH field will automatically be filled in (optional to change).
The TOOL field will default to the current tool selected.
In the OFFSET field select INSIDE for a external helix, or OUTSIDE for an internal helix.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed. Select RAPID for a dry run without a tool by using the Rapid soft key, or select from the drop down menu.
ARROW
DOWN or press the More soft key.
START ANGLE (optional). Enter the angle where the helix begins
(3 o’clock position is 0 degrees; 12 o’clock position is 90 degrees).
In the PITCH field enter the number of revolutions.
Press the USE key.
If the tool size and type listed in the TOOL field are incorrect, change the tool settings before running your program.
152
8 Milling and Drilling
Hole Patterns
MILLPWR
G2
includes several built-in routines that let you program hole patterns quickly and easily. The following hole patterns are described here:
Row of Holes
Rectangle Frame
Rectangle Array
Bolt Circle
Row of Holes
A row of holes, can be programmed two ways:
By entering the coordinates of the first and last hole
By entering the coordinates of the first hole, the spacing between each hole and the row’s angle
The “From” point refers to the center of the first hole, while the “To” point is the center of the last hole. Any additional holes will be spaced equally between these two.
You’ll also be prompted for peck and tool retract values. “Peck” lets you break chips and reduce chip buildup during drilling operations.
“Tool Retract” allows you to program MILLPWR
G2
to raise the tool at regular intervals.
To program a row of holes:
MILLPWR
G2
includes several built-in routines that let you program hole patterns quickly and easily
From the PGM screen, press the HOLES key to access the HOLES popup Menu.
ACU-RITE MILLPWR
G2
153
Entering data:
Select the Row of Holes from the popup Menu.
In the FROM field, enter the X and Y axes coordinates for the center of the first hole and ARROW DOWN to the next field.
Now either: Enter the X and Y axes coordinates for the center of the last hole in the TO field; or perform the following step instead.
ARROW
DOWN and enter the distance between each hole (from center point to center point) in the HOLE SPACING field, then enter the angle of the row of holes.
ARROW DOWN
, enter the Z fields, BEGIN, END, and PECK data.
Select the type of machining to be done: DRILL, BORE, or
POSITION. Either pick from the drop down menu, or the soft keys.
Enter the Z axis FEED rate. The last feed rate used previously in the program will be displayed. RAPID is also available, select by using the Rapid soft key, or select from the drop down menu.
ARROW
DOWN or press the More soft key.
Additional information can be entered for tool retract, and tool dwell.
The TOOL field enters the current tool selected as reference information. To use a different tool, that tool has to be entered as the current tool.
Press the USE key.
154
8 Milling and Drilling
Hole Frame and Array
HOLE FRAME and HOLE ARRAY patterns require the same information, but their patterns differ slightly. Hole frames limit holes to the outside edge of a rectangular shape, while hole arrays allow holes along the outside edge and throughout the center.
Hole Frames and Hole Arrays can be defined three ways:
By the position of the 1st Corner, size, and the number of holes.
By the position of the 1st Corner, position of the 2nd (diagonal)
Corner, and number of holes.
By the position of the 1st Corner, hole spacing, and number of holes
Choose the method that’s easiest for you based upon the information from your print.
You’ll also be prompted for Peck and Tool Retract values. Peck lets you break chips and reduce chip buildup during drilling operations. Tool
Retract allows you to program MILLPWR
G2
to raise the tool at regular intervals.
ACU-RITE MILLPWR
G2
155
Entering data:
From the PGM screen, press the HOLES key to access the HOLES popup Menu.
Select the Rectangle Array from the popup Menu.
Enter the 1st CORNER X1 and Y1 axes coordinates.
Now enter either the SIZE of the array or the 2 nd
CORNER coordinates.
Either data entry will automatically fill in the fields for the for the other option.
To enter the SIZE, enter the length of the array along the X and Y axes.
Or enter the X and Y axes coordinates for the 2 nd
CORNER. The 2 corner must be located diagonally from the 1 st
CORNER. This nd information may be calculated automatically based on the option to put the data in the dialogue.
Enter the BEGIN and END depths for Z. Enter the PECK distance
(depth).
Select the type of machining to be done: DRILL, BORE, or
POSITION. Either pick from the drop down menu, or the soft keys.
Enter the Z axis FEED rate.
ARROW
DOWN, and enter the number of holes in the X field, then the number of holes in the Y field.
ARROW
DOWN or press the More soft key.
The HOLE SPACING field information may be calculated automatically based on the option to put the data in the dialogue. If this is the data to be entered, enter the X and Y fields.
Enter the hole pattern angle in the ANGLE field, default is 0.00 (X axis).
The TOOL RETRACT, and TOOL fields are optional.
The TOOL field enters the current tool selected as reference information. To use a different tool, that tool has to be entered as the current tool.
Press the USE key.
156
8 Milling and Drilling
Bolt Circle Patterns
A Bolthole Circle pattern is defined by its center point, radius and number of holes. You can program partial bolthole patterns by pressing the More soft key and entering a start angle and an end angle.
Entering Data
From the PGM screen, press the HOLES key to access the HOLES popup Menu.
Select the Bolt Circle from the popup Menu.
Enter the CENTER X and Y axes coordinates.
Enter the BEGIN and END depths for Z. Also enter the PECK distance (depth).
Select the type of machining to be done: DRILL, BORE, or
POSITION. Either pick from the drop down menu, or the soft keys.
Enter the Z axis FEED rate.
ARROW
DOWN, and enter the required data in the RADIUS field.
For DIRECTION, press either the CW soft key for a clockwise cutting direction or the CCW soft key for a counter-clockwise cutting direction.
In the HOLES field enter the number of holes required in the bolt circle.
Enter the hole pattern angle in the ANGLE field, default is 0.00 (X axis).
In the start angle field enter the angle of the first hole in relationship to 0.00 (X axis).
ARROW
DOWN or press the More soft key.
The TOOL RETRACT, and TOOL DWELL fields are optional.
The TOOL field enters the current tool selected as reference information. To use a different tool, that tool has to be entered as the current tool.
Press the USE key.
ACU-RITE MILLPWR
G2
157
8.2 Additional Milling Functions
Step Functions soft key
Additional functions are available from the PGM screen by pressing the
Step Functions
soft key.
Explode
When in PGM mode there are certain functions that can be exploded. Pressing the Explode soft key will explode a program step into several, more detailed steps. You can explode the following functions:
All HOLES functions, Row, Frame, Array and Bolt Circle
Repeat
, Mirror and Rotate
During the explode operation, the program list populates as it is being exploded. A message will be displayed “Exploding the selected step”.
A Cancel soft key becomes available during the explode operation.
When this key is pressed, the explode operation stops, and the program returns to it original state. No other options are available during the explode operation.
Example:
A Bolt Circle with eight holes has been programmed.
Edit the program by first highlighting the BOLT CIRCLE step.
Press the Step Functions soft key.
Press the Explode soft key.
MILLPWR
G2
will explode the “Bolt Circle” step into eight steps (002 thru 009).
The step that was exploded is now replaced with the individual lines, arcs or positions that made up the step.
Highlight the step that represents the hole that will be edited and press the ENTER key, or press the CLEAR key to delete it.
158
8 Milling and Drilling
Reverse Step
The reverse step feature instantly switches the FROM and TO points and TOOL OFFSET.
To reverse a milling function:
From the PGM screen, use the arrow keys to highlight the step that you want to reverse.
Press the Step Functions soft key.
Press the Reverse Step soft key.
Reverse Path
With the reverse path option, you can reverse any continuous tool path. This will especially come in handy when you're working with
DXF files. As you import DXF files, MILLPWR
G2
will sort and then group the steps into a logical order, creating continuous paths. In some cases, the paths may need to be reversed after they've been imported so that your tool's offset, direction and beginning and end points satisfy your machining requirements.
As you become more familiar with this feature, you'll find other creative ways to use it to your advantage. For instance, you can save time as you're cutting a part by using a heavy cutting tool and a conventional cut for a rough first pass. On the second pass, switch to a finish cutter, then copy and reverse the path for a climb cut on the finish pass.
To reverse a continuous tool path:
From PGM mode, highlight any step within the continuous tool path that you want to reverse.
Press the Step Functions soft key.
Press the Reverse Path soft key. The original steps are replaced with steps in the reverse order.
ACU-RITE MILLPWR
G2
159
Change Steps
The Change Steps feature gives you the ability to change or edit the depth, offset and feed rate of several steps simultaneously.
You can use this feature from anywhere within your program and does not require the specific step to be highlighted.
To Change Steps:
From the PGM screen, press the Step Functions soft key.
Press the Change Steps soft key.
Enter the first and last step numbers that you would like to change in the STEP RANGE field.
Use the arrow keys to select each field that you want to change and enter the new data.
Press the USE key.
Highlight the changed steps in the program sequence, then press the
ENTER
key. Each step should include the new settings.
Shift Steps
The purpose of the Shift Steps feature is to transpose a range of steps from one location to another on the actual work piece.
This feature can be used from anywhere within the program, and does not require the specific step(s) to be highlighted.
To Shift Steps:
From the PGM screen press the Step Functions soft key, then the Shift Steps soft key.
Enter the first and last step numbers to be transposed.
Enter in each axis field the distance to shift per axis. Leaving a field empty will result in no shift per that axis.
Press the USE key to apply the shift to the selected steps.
Highlight the changed steps in the program sequence, then press the
ENTER
key. Each step should show the new axis coordinates.
160
8 Milling and Drilling
Delete Steps
MILLPWR
G2
provides options for deleting steps in two ways: using the Delete Steps soft key or using the CLEAR key.
When deleting single steps, highlight the step, then press the CLEAR key.
When deleting a range of steps, the Delete Steps feature is usually the best option.
To delete a group of steps from a program:
From the PGM screen, press the Step Functions soft key.
Press the Delete Steps soft key.
In the STEP RANGE field, enter the first and last step numbers to be deleted.
Press the USE key.
Copy/Move Steps
Copy/Move operations make it easy for you to duplicate or rearrange steps within your program. You'll find the MOVE feature especially useful for editing steps generated from a DXF file.
After you press the Copy/Move Steps soft key, you'll be asked to enter a step range, then either copy or move the steps and select a location where to copy or move the steps (i.e. Paste Location).
Press the Move soft key to relocate the steps. Press the Copy soft key to create an identical copy of the steps you've chosen (the original steps will remain in place). After you press the USE key, the new steps will be inserted into your program.
To copy or move steps:
From the PGM screen, highlight a step where you would like to add or insert the step(s) that you want to move or copy. If you are already in
Copy/Move Steps then press Paste Location and scroll in the program where you want to move or copy the steps.
Press the Step Functions soft key.
Enter the first and last step numbers that you would like to move or copy.
Press the Copy/move Steps soft key.
Press either the Move Or Copy soft key. Make sure the desired location is selected in the program or, use Paste Location to select where to move or copy the steps.
Press the USE key.
ACU-RITE MILLPWR
G2
161
Custom Pockets
A custom pocket step must immediately follow a closed contour.
You can create a custom pocket from any closed contour. A closed contour is any shape consisting of lines, arcs, and/or blends (or chamfer), where the last step ends at the same point where the first step begins. MILLPWR
G2
will indicate a closed contour with double lines to the right of the applicable steps in the program list.
The Custom Pocket step must be placed immediately following the last step of the closed contour. MILLPWR
G2
will automatically fill in the step range for you. You’ll still need to fill in the “Entry Point,” and set the feed rate for the custom pocket.
If a finish cut is specified, the system will mill the central portion of the pocket first, leaving the finish amount on the bottom and side. It will then mill the bottom pass followed by the side pass.
Custom Pocket
Create a closed contour.
Position the cursor immediately below the closed tool path contour.
Press the Program Steps soft key.
Press the Custom Pocket soft key and select Custom Pocket.
MILLPWR
G2
will automatically fill in the step range for you.
Enter the X and Y axes coordinates for the START POINT.
Enter the Z the number of passes OR the DISTANCE between each pass. PASS refers to the cuts that are used to machine the pocket to its End depth. What is shown on the dialogue is what was selected in JOB SETUP.
Enter the feed rate for the Z axis.
Enter the table’s feed rate.
In the FINISH field enter the amount of material to be removed during the finish CUT.
Enter the feed rate for the finish cut.
For DIRECTION, press either the CW soft key for clockwise or the CCW soft key for a counter-clockwise direction.
Enter the stepover percentage (how much you want your tool to overlap on each pass).
Press the USE key.
The system will determine the best location to start feeding into the part. Depending on the shape of the pocket and island contours, the pocket may be split into more than one region. The system will machine each region separately.
162
8 Milling and Drilling
Island
An island is a raised area (e.g. a boss) within a custom pocket that remains after material has been removed from around all of its sides.
Though islands are easy to program, they must be placed correctly within the program sequence. Steps for the island's continuous tool path must appear first, followed by the Island step. Steps for the custom pocket's continuous tool path must appear next, followed by the Custom Pocket step. You may program more than one island within the Custom Pocket.
To program an island:
Program a closed contour for the island.
From the PGM screen, place the cursor below the last step of the island’s closed contour.
Press the Program Steps soft key.
Press the Custom Pocket soft key.
Select Island in the popup Menu.
Check that the first and last steps listed in the step range match the first and last steps for the island’s continuous tool path. If they’re correct, press the USE key; if they’re not, press the CANCEL key and check that the closed contour for the island is correct and/or the correct step has been highlighted.
Tool Path Description for Custom Pocket, and Islands
Machining of the custom pocket begins at a location based on pocket geometry. The software automatically determines this location.
The tool ramps into the material at the Z feed rate.
The XY step size is determined by the system and will not exceed the specified percentage of the tool diameter.
The percentage must be 50% or less. This is required to make sure that all material is removed.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts to the active datum's retract position between Z passes.
A finish allowance is optional but recommended. If specified, this amount is left on the bottom and sides of the pocket and islands to be removed on the finish pass.
When the finish feed is 0, the finish pass will be skipped. The tool retracts to the active datum's retract height and the specified
"staging" position between rough, bottom finish, and side finish operations.
ACU-RITE MILLPWR
G2
163
Contour
The Contour step enables you to approach and/or depart from your part on a straight line or with an arc.
The contour step must immediately follow the contour steps.
Contours can only be associated with lines, arcs, blends and chamfers. By adding contours before and/or after a continuous tool path, you'll avoid starts and stops striking against the workpiece edge.
With an arc approach/departure, the tool will take a rounded turn as it nears or exits the workpiece.
With a straight approach/departure, the tool path is extended away from the workpiece.
The step range can include one or more steps. If you're planning to add a contour to an individual step, the first and last steps in the range will be the same.
Because the approach and departure fields are independent of each other, you may select one or both for the step range you've chosen.
Select None as the type for whichever option you don't want.
To program a contour:
From the PGM screen, highlight the step below the last step in the continuous contour.
Press the Program Steps soft key.
Press the Custom Pocket soft key.
Select Contour from the popup menu.
FIRST and LAST in the STEP RANGE field will be filled in.
If you wish to program an approach, select the Straight or Arc soft key, or use the drop down menu as your approach type. Otherwise, press the None soft key.
Enter how far from the part you want the approach to begin in the
DISTANCE field.
To program a departure, select the Straight or Arc soft key, or use the drop down menu as your approach type. Otherwise, press the
None
soft key.
164
8 Milling and Drilling
Enter how far from the part you want your tool to travel in the
DISTANCE field.
If you would like to program a FINISH CUT, enter the amount of material to be removed during the finish cut.
Enter the FEED RATE.
Press the USE key.
Tool Path Description:
The tool path follows the profile of the contour steps.
The Z step size is determined by the system and will not exceed the specified distance or number of passes.
The tool retracts to the active datum's retract position between Z passes.
Approach and departure moves are optional. For LINE, the tool approaches/departs with a linear move tangent to the first or last step of the contour.
For ARC, the tool approaches/departs with a tangential arc to a location away from the contour.
A finish allowance is optional. If specified, this amount of material is left on the side of the contour to be removed on the finish pass.
When finish feed is 0, the finish pass will be skipped.
ACU-RITE MILLPWR
G2
165
Repeat, Rotate, ...
The Repeat, Rotate, ... soft key provides milling functions available with the MILLPWR
G2
product.
Repeat
Using this step you can repeat sections of programs with any combination of X, Y or Z offsets.
To program a repeat:
From the PGM screen, press the Program Steps soft key.
Press the Repeat, Rotate, ... soft key.
Enter the number of the FIRST step and the LAST step in the STEP
RANGE that you want to repeat.
Enter the OFFSET for the X, Y and/or Z axis. The offset is the distance between repeats.
Enter the number of times you want to REPEAT the original steps.
Press the USE key.
The steps being repeated must precede the REPEAT step.
The number of repeats must be 1 or more.
Rotate
With ROTATE, you can rotate sections of programs.
The steps rotated must precede the ROTATE step.
To program a ROTATE:
From the PGM screen, press the Program Steps soft key.
Press the Repeat, Rotate, ... soft key.
Enter the first and last steps in the STEP RANGE that you would like to rotate.
Enter the X and Y axes coordinates for the CENTER point of rotation.
Enter the Z offset.
Enter the angle for each rotation in the ANGLE field.
Enter the number of times required to rotate the original steps.
Press the USE key.
166
8 Milling and Drilling
Mirror
The steps being mirrored must precede the Mirror step.
With Mirror you can create a mirror image of an entire program or a section of a program.
To program a MIRROR:
From the PGM screen, press the Program Steps soft key.
Press the Mirror soft key.
Enter the first and last steps in the STEP RANGE that you would like to mirror.
Enter the X and Y axes coordinates which define the line across which the step range is mirrored.
Enter the Z offset.
Press the USE key.
Other Steps
Other Steps
soft key provides additional milling functions available with the MILLPWR
G2
product.
From the PGM screen, press the Program Steps soft key, then press the Other Steps soft key to display the popup Menu.
With MILLPWR
G2
, you have the ability to engrave letters, numbers and symbols, along a straight line or on an arc. Choose from a simple, stick or stencil font. The character height, font and modifier settings you select will define your engraving’s appearance.
The tool diameter being used establishes the spacing between letters.
ACU-RITE MILLPWR
G2
167
Engrave Line
All ASCII characters within the range of x032 - x126 are allowed, which includes Uppercase, Lowercase, Numbers, and Punctuation.
From the PGM screen, press the Program Steps soft key.
Then press the Other Steps soft key.
In the popup menu select Engrave Line.
With the cursor in the TEXT input field, press the Alphanumeric
Keyboard
soft key, and insert the desired text.
Enter the X and Y axes coordinates for the point at the lower left corner of the engraving.
Enter the character height.
Enter the tilt angle if there is to one.
Enter the begin and end depths for the Z axis.
Enter the Z axis feed rate.
Select the font required from 3 choices, SIMPLE, STENCIL, or
STICK, soft keys, or the drop down menu.
Select the MODIFIER as either the NORMAL or MIRRORED soft key. Normal is readable from left to right; Mirrored will make the engraving appear backwards.
Enter the table’s feed rate.
Press the USE key.
168
8 Milling and Drilling
Engrave Arc
All ASCII characters within the range of x032 - x126 are allowed, which includes Uppercase, Lowercase, Numbers, and Punctuation.
From the PGM screen, press the Program Steps soft key.
Then press the Other Steps soft key.
In the popup menu select Engrave Arc.
Highlight the TEXT input field, press the Alphanumeric Keyboard soft key, and insert the desired text.
Enter the X and Y axes coordinates for the TEXT CENTER from the center of the engraving.
Enter the CHARACTER HEIGHT.
Enter the RADIUS that the text will follow, and select Arc Up, or Arc
Down
(e.g. Arc Down is shown in the example).
Enter the begin and end depths for the Z axis.
Enter the Z axis feed rate.
Select the font required from 3 choices, SIMPLE, STENCIL, or
STICK, soft keys, or the drop down menu.
Select the MODIFIER as either the NORMAL or MIRRORED soft key. Normal is readable from left to right; Mirrored will make the engraving appear backwards.
Press the USE key.
ACU-RITE MILLPWR
G2
169
Comment Step
With MILLPWR
G2
, you have the ability to insert messages anywhere within a program. These messages can be displayed during machining
(at run-time) or as Operator Intervention Messages (OIM). These messages become operational steps within the program and communicate pertinent information like "ROTATE PART" or "ACTIVATE
COOLANT".
For comments that don't require an operator intervention, select NO when asked if you want the comment displayed at run-time, and
MILLPWR
G2
will skip over them during machining. You can always retrieve the message by highlighting the comment step in your program steps list and pressing ENTER.
To program a comment step:
From the PGM screen, place the cursor below the last step where the comment is needed.
Press the Program Steps soft key.
Press the Other Steps soft key.
Select Comment in the popup Menu.
Enter your message. You may include up to 60 characters, mixing numbers, letters, spaces and symbols if needed. Press the
Alphanumeric Keyboard
soft key to chose alphabet characters. See
"Keyboard" on page 17 for using the keyboard.
Highlight DISPLAY AT RUN-TIME. Press the Yes soft key to display the message during machining or the No soft key if you don't want the message displayed.
Press the USE key.
170
8 Milling and Drilling
Dwell
This is where the time is set for the machine to pause it’s movement, and stay in its current position for a programmed amount of time measured in seconds.
From PGM screen, press the Program Steps soft key, then press the
Other Steps
soft key.
Select Dwell in the popup Menu.
Enter the Dwell time in seconds, tenth of seconds can also be entered.
Press the USE key.
A Dwell of 0 will cause the program to Pause until the operator presses GO.
Reference Point
Reference points are commonly used to identify center points, tangent points and other part features. They can even be used as the basis for incremental moves.
As you program, note that placing a reference point in a continuous tool path will break the path. Otherwise, reference points do not affect your program's performance in any way in fact, MILLPWR
G2
will skip over them altogether when you run a program.
To program a reference point:
From the PGM screen, press the Program Steps soft key, then press the Other Steps soft key.
Press the Reference Point in the popup Menu.
Enter your reference point’s position for X, Y and Z.
Press the USE key.
ACU-RITE MILLPWR
G2
171
172
8 Milling and Drilling
Setup
9.1 Setup
Overview
The MILLPWR
G2 has a set of parameters that can be setup as default values. Some of these values can be over-ridden per the program step dialogue, while others remain in affect until changed in the setup dialogue.
Setup
Press the SETUP key to access the setup parameters.
The setup parameters are grouped into two categories: Job Setup and Installation Setup (e.g.
Config Data).
Job Setup
parameters can be changed to accommodate specific machining requirements for each job.
Installation Setup parameters are established during the initial installation and typically are not changed. The installation setup parameters are protected by a passcode. These parameters are described within the Technical Manual.
Tool Table
Press the Tool Table soft key to access the Tool
Table.
The Tool Table is briefly discussed in this chapter. In the table, up to
99 tools can be entered and used in any program that would required
that tool. See chapter 4.1 Tool Table on page 44 for a complete
description about using the Tool Table.
Error Log
Press the Error Log soft key to access the Error Log display.
The Error Log records all errors, and is retained by the MILLPWR
G2 until it is deleted. An error in the log can be highlighted, and an explanation of the error can be displayed by pressing the Info soft key.
The Error Log entries may also be deleted from the DRO or PGM screen by pressing the 0 numeric key.
174
9 Setup
Job Setup
Three soft keys: Job Setup, Tool Table, and Error Log are used to setup the MILLPWR
G2
for operation, programing, and DRO mode.
Job Setup
Press the Job Setup soft key to access the Job setup parameters.
In the JOB SETUP dialogue there are four parameters that can be set which the MILLPWR
G2
will default to when not overridden by another setting.
SCALING: Typically most jobs are scaled at 1 to 1 (full scale).
Occasionally a job may be scaled down to as an example 1/2 scale.
In such a case, before programming the job, the scale factor should be changed here so that it becomes the default scale factor for the program.
FEED RATE: This is a Default setting that the MILLPWR
G2
will use as well. Though this setting can change per job, and material used.
The MILLPWR
G2
will use this as the default in a program unless it is changed (e.g. by a step that is in the program), then that new feed rate will be used until changed again.
DISPLAY: For Peck\Pass, the setting can either be in Distance, or
Number Of Cycles. The selected option will be the default for the dialogues and can only be changed here in Job Setup.
JOB CLOCK - PARTS COUNTER: For setting the parts counter and stopping or starting the Job Clock. The Job Clock will provide an estimate of time to machine the part, provide a stop watch, parts counter, and overall Job time.
PROBING: When a probe is used, the probe tip radius is entered here. This value will be used in dialogues where applicable.
DISPLAY GRID: When viewing a part graphic, a grid can be turned on as an overlay to the part graphic. The grid spacing is set using this field, and is relative to the actual part size.
TRAVEL LIMITS: The X, Y, and Z travel limits are set in the TRAVEL
LIMITS fields for each axis. Travel limits can be set at any location that does not exceed the actual travel of the machine.
ACU-RITE MILLPWR
G2
175
Scale Factor
Scale factor is a multiplier that lets you expand or shrink the print’s dimensions without performing complex calculations, or affecting the proportion of your part. Enter the number that the dimensions should be multiplied by, then run the program normally. MILLPWR
G2
will adjust the programmed dimensions (but not the tool size) automatically.
There is no limit, or restrictions when using a scale factor.
The MILLPWR
G2
scale default setting is 1.0000. A value greater than
1.0000 will increase the part’s dimensions; a value less than 1.0000 will reduce them. This is saved to the configuration block and will be remembered until it is changed to a new setting.
MILLPWR
G2
will display the current scale factor in the status bar at the top of the display screen.
To change the scale factor
In Job Setup, highlight the SCALING field, and enter the multiplication factor.
Press the USE key.
Feed Rate
The parameters set here will be used as the default by MILLPWR
G2 and will only change if it is modified in any of the milling functions dialogue.
Highlight the Default field, and specify the inches per minute. Also select the unit of measure, Inch or MM by pressing the appropriate soft key.
Next, highlight the Dry Run field, and enter the inches per minute that is required. The default is 80 IPM.
Display: Peck\Pass
Enter either the Number of Cycles or the Distance between each cut.
This applies to the Z axis depth of cut. This setting acts a little different depending on what function has been selected.
When drilling a hole, the Number of Cycles refers to the number of times the drill retracts to clear the debris from the hole. If Distance is used in stead, it would mean how deep the drill plunges before it retracts.
Similarly, if milling, and using a flat end mill, Distance will mean the depth of each pass. Number of Cycles will mean how many times the end mill make a pass, cutting material away each time.
176
9 Setup
Job Clock - Parts Counter
The parts counter appears on the status bar when in DRO mode, or running a program. This is useful to track how many times the current program has run and therefore how many parts have been completed.
Here, setting the parts counter, stopping or starting the Job Clock are setup. The Job Clock will provide an estimate of time to machine the part, provide a stop watch, parts counter, and overall Job time.
Preset a starting count by entering the value in the Parts field.
Press the Set Count soft key to set the counter to the field value.
Press the Reset Count soft key to set the Parts field to 0.
The parts counter resets to 0 when a new program is loaded.
The Job Clock is also displayed on the status bar, and operates like a stop watch. It is started, or stopped by the user from the JOB SETUP dialogue.
The Pause Clock soft key will pause the Job Clock temporarily.
The Resume Clock soft key will resume the Job Clock after it has been paused.
The Reset Clock soft key will stop, and reset the Job Clock to 0.00.
There is no MILLPWR
G2 requirement for these features. They are provided to the operator for job assistance, and informational purposes.
Probing
When using a probe, the radius of the tip of the probe is used for establishing the location of an edge of a work piece. The value of the probes radius will be used in all applicable dialogues when the probe is the selected tool.
Select the PROBING Radius field.
Enter the tip radius of the probe.
Press the USE key to enter the data.
ACU-RITE MILLPWR
G2
177
Display Grid
When in PGM mode, and a program is selected, the graphic view of the part is displayed. A grid overlay can be added to the display. The grid spacing is defined in this field. The grid spacing is relative to the actual size of the part, and not the display size.
For an example; if the part size is 3.0 x 3.0 inches, and the selected grid spacing is .5”, then the grid shown would have 5 horizontal, and
5 vertical lines displayed. If the part size is 6.0 x 6.0 inches, then there would be 11 horizontal, and 11 vertical lines displayed.
Select the DISPLAY GRID Spacing field.
Enter the spacing preferred (e.g. .50”).
Press the USE key to enter the data.
Travel Limits
Find Home must be established before travel limits can be set.
Travel limits define how far the table is allowed to move along the X and Y axes, and how far up and down the Z axis quill can be moved.
When a value is set to zero, then no limit stop is set for that axis.
If a limit setting has been set incorrectly, the operator will be able to exit, and continue. Pressing the USE key will cause a warning to be displayed in the Operator Intervention Message display that the limits were set incorrectly. The limit setting in that axis will return to zero, and the settings must be re-defined.
The error message must first be cleared from the error log before returning to the Job Setup dialogue.
When using the Move Table soft key (Jog Mode), all travel limits are removed. Caution must be taken not to exceed the actual table travel limits. Damage to the system, or to the machine could occur.
178
9 Setup
To set the X axis Travel Limits:
Select the TRAVEL LIMITS X Axis field.
Move the table by pressing the Move Table soft key, then use the right and left ARROW keys, or manually move the table with the hand wheel.
Move the table to the left to locate the right side table travel limit stop.
With the table in the required location, press the Set Right softkey.
Move the table to the right to locate the left table travel limit stop is to be set, and press the Set Left softkey.
The X axis travel field will now update to show the maximum allowable travel distance between the left and right table travel limit stops.
Press the Exit soft key to exit Move Table, and accept the X Axes limit stop locations, and return to the dialogue.
The next field can not be accessed unless the Exit soft key, or
CANCEL
key is pressed. Each axes must be set individually in order to return to the dialogue form.
To set the Y axis Travel Limits:
ARROW
down to the TRAVEL LIMITS Y Axis field.
Move the table by pressing the Move Table soft key, then use the UP
ARROW
key to move the table towards the column. The DOWN ARROW key is used to move the table away from the column. The table can also be manually moved with the hand wheel.
Move the table towards the column to where the Inside table travel limit stop is to be set.
With the table in the required location, press the Set Inside softkey.
Move the table out to where the Outside table travel limit stop is to be located.
With the table in the required location, press the Set Outside softkey.
The Y axis travel field will now update to show the maximum allowable travel distance between the Inside and Outside table travel limit stops.
Press the Exit soft key to exit Move Table, and accept the Y Axes limit stop locations, and return to the dialogue.
ACU-RITE MILLPWR
G2
179
To set the Z axis Travel Limits:
ARROW
down to the TRAVEL LIMITS Z Axis field.
Move the quill by pressing the Move Table soft key, then use the
Move Z Up
and Move Z down soft keys. The axis can also be manually moved with the hand lever, or wheel.
Move the quill up to where the top of the quill travel limit stop is to be set with the Move Z Up soft key, or done manually. With the quill set in the required location, press the Set Top softkey.
Move the quill down to where the bottom travel limit stop is to be set using the Move Z Down soft key, or done manually. With the quill set in the required location, press the Set Bottom softkey.
The Z axis travel field will now update to show the maximum allowable travel distance between the upper and lower limit stops.
Press the Exit soft key to exit Move Table, and accept the Z Axes limit stop locations.
Press the USE key to accept all the settings in Job Setup.
If a power cycle occurs while in the Job Setup dialogue, all travel limits set will be lost.
180
9 Setup
Tool Table
MILLPWR
G2
contains a tool table that can store the diameter, length, unit of measure, and tool type for up to 99 tools. MILLPWR
G2
only requires that you provide the tool's diameter; however, it may be helpful to the operator if additional information is provided so that each tool is easier to identify from the tool list. Chapter 4 provides complete
information regarding the tool table. See "Tool Table" on page 44
Set up the tool table so that the tools used most often appear first.
From SETUP, press the Tool Table soft key.
Error Log
MILLPWR
G2
includes a built-in error log that will record system error messages. If an error is detected, MILLPWR
G2
will automatically record the date, along with a brief description of the error.
If an error is present that prevents running of another program the front panel indicator light will flash.
Press the Info soft key to display additional information on the highlighted error which will open in its own display window. The additional information includes Cause and suggested correction
Action.
Press the Detail soft key to display the detailed information available on the source of the error. This will also open in its own display window.
Press the Delete soft key to clear the highlighted message.
Pressing the Delete All soft key will clear all messages. Pressing the Delete All soft key will also exit the Error Log dialogue.
Pressing the Delete soft key will only exit the dialogue if there was only one error message.
To exit the Error Log, press the Exit soft key.
A quick method for deleting all errors in the log is to press the “0” on the numeric keypad.
ACU-RITE MILLPWR
G2
181
Service Files
Occasionally, it may be necessary to provide files that document problems. These are known as service files.
The service files can be generated by pressing the Log Files soft key and then pressing the Service Files soft key (accept the default name and press the OK soft key).
The services files take a few seconds to generate. Once generated they can be found in V:\ with the name service1.zip.
Use features in Program Functions to copy the service file (i.e.: service1.zip) and e-mail it if ever asked to do so.
Multiple service files can be re-generated. The most recent one is always service1.zip; second most recent one service2.zip; etc.
After copying the service files delete them so they do not occupy program storage space.
182
9 Setup
Software Update
10.1 Updating System Software
Software Update
HEIDENHAIN Corporation recommends making a backup of the control with the included USB Recovery Drive (684138-xx) before updating the NC software. Please refer to the manual included with the drive for the backup procedure.
Use a blank USB memory stick (1 GB or larger) to update the software.
Do not use any memory stick with a smaller storage capacity.
The software installation files are required for updating the software.
The files will automatically be recognized by the installation program of the control and must be contained in a folder named “install” on the
USB memory device with typical files called setup.zip, and setup.ini.
Procedure for updating the software
Shut down the control software using the normal method of pressing the Shutdown soft key and then confirming the shutdown by pressing Yes.
Wait for the screen message which indicates that it is safe to switch off power, or restart.
Insert the USB memory device containing the folder named “install” on the USB memory device.
Press ENTER to restart the system.
After starting, the MILLPWR
G2
Software Update screen will appear with a confirmation box. If necessary, use the UP/DOWN ARROW keys to select the language (e.g. English) and press ENTER.
A confirmation box will appear. If necessary, use the LEFT or RIGHT
ARROW
keys to select Yes, then press ENTER.
The software update will now be done automatically, taking approximately 10 - 20 minutes.
When the update is complete, it will prompt you to remove the USB drive and restart. At this time, remove the USB drive and press
ENTER
to restart.
After the system has restarted, it will start up normally to the control software.
If any issues are encountered, please either refer to the technical manual or contact your service representative for assistance.
If the USB memory stick used for installation is not removed, then the prompt to install the software will continue to appear on subsequent power cycles.
184
10 Software Update
Off-Line Software
11.1 MILLPWR Off-Line Software
Off-Line Simulator
The off-line software provides a convenient way to write part programs and simulate machine behavior using a standard Windows based computer. Features and functionality are virtually identical to that of the MILLPWR
G2
control itself.
System Requirements
Platform: IBM compatible PC.
Operating System: All 32-bit and 64-bit editions of ** Windows
Vista
®
, and Windows
®
7 are supported.
Available Drive Space: 2GB or higher.
Memory: 1GB or higher.
Display Resolution: 1024x768 (XGA) or higher required. 1440 x 900
(WXGA+) recommended.
Peripherals: Keyboard and pointing device.
**Microsoft
®
and Windows
®
are registered trademarks of Microsoft
Corporation in the United States and/or other countries.
186
11 Off-Line Software
Installation
The software is installed in the usual manner by launching the setup program, selecting an installation destination, and choosing the desired features to be installed. Using the default setting for a
"Complete" feature installation is highly recommended to ensure proper functionality. On some systems, you may be required to restart the computer after installation before the application will display properly.
Operation
The off-line software can be started by using either the "MILLPWR
G2
Off-Line" shortcut created on your desktop during installation or from the Start menu. Once the software is running, it is operated in the same manner as the machine itself. Similarly, it should be shut down using the same sequence of selecting Shutdown and confirming
Shutdown at the prompt. If for some reason the software becomes unresponsive, a force quit can be done using the "ShutDown
MILLPWR
G2
" shortcut created on your desktop during installation or from the Start menu. Normal shutdown procedure should be used unless the force quit method is absolutely required.
Programs created in the off-line software can be copied to the CNC, and (with the correct setup) run on your machine.
ACU-RITE MILLPWR
G2
187
On Screen Keypad
The MILLPWR
G2
Off-Line software includes an on-screen keypad application. This can be used to simulate the hard keys that are normally available on the machine console. Pressing the buttons on the keypad application will activate the same operation that would occur when pressing the corresponding buttons on the machine console.
The keypad application will automatically start and shutdown when the MILLPWR
G2
software is started and shutdown. If necessary, the keypad application can be manually shutdown by clicking the red "X" button in the top right corner of the keypad window. Likewise, if necessary, the keypad application can be manually started using the
"Launch Keypad" shortcut located in the Windows® Start Menu, under
All Programs - ACU-RITE - MillPWR Off-Line.
Keyboard Shortcuts
The keys on the MILLPWR
G2
keypad can be simulated using the key combinations described below. These can be used when the on-screen keypad is closed or when the PC keyboard is connected to a MILLPWR
G2
console
Keys Shortcut
Alt + T (Tool)
Alt + R (Rectangle)
Alt + C (Circle)
Alt + H (Holes)
Alt + P (Position)
Alt + L (Line)
Alt + A (Arc)
Alt + B (Blend/Chamfer)
188
11 Off-Line Software
Keys
<USER>
Shortcut
Alt + I (Absolute/Incremental)
Alt + D (DRO/Program mode)
Alt + V (Display View)
Alt + U (User ID)
Alt + N (On screen User Manual)
Alt + F (Inch/MM)
Alt + Enter (Configuration menu)
Alt + K (Calculator)
F12 (Plus/Minus Toggle)
F12 (Plus/Minus Toggle)
Esc (Cancel)
Del (Clear)
Alt + Enter (Use)
Enter (Enter)
Alt + J (Press once: Pause / Press Twice: Stop)
Alt + S (Go)
ACU-RITE MILLPWR
G2
189
Soft keys Shortcut
7
8
5
6
3
4
1
2
F1
F2
F3
F4
F5
F6
F7
F8
Numeric, and arrow keys:
The arrow keys on a standard PC keyboard will simulate the console arrow keys, and the number keys will simulate the console number keys (using number lock). When number lock is turned off, the arrow keys on the number keys (2, 4, 8, 6) will simulate the console arrow keys.
Updating
It is not necessary to un-install the software before installing updates.
Running the new setup program will update the existing installation to the newer version. Although your created part programs will remain intact, it is always recommended to make a backup of your programs and/or configurations before updating the software installation.
190
11 Off-Line Software
A
Absolute work piece positions 25
Activating/Resetting the Servos 5
Advanced Functions
C
Change Window
D
E
F
G
I
Incremental work piece positions 25
J
K
M
N
O
P
Program Steps in 2 Axis Mode 9
R
S
Setup
Soft keys
Calculator
ACU-RITE MILLPWR
G2
191
View
T
U
W
Z
192
HEIDENHAIN CORPORATION
333 East State Parkway
Schaumburg, IL 60173-5337 USA
+1 (847) 490-1191
+1 (847) 490-3931
E-Mail: [email protected]
www.heidenhain.com
1034384-20 Ver 00 9/2013
advertisement
* Your assessment is very important for improving the workof artificial intelligence, which forms the content of this project