Programming. ACU-RITE MILLPWRG2
The ACU-RITE MILLPWRG2 is a shop-floor, conversational programming control designed for milling and drilling machine tools, with up to 3 axes. It is designed to satisfy the wants and needs of tool and die makers and other machinists where manual and automated operation are both useful and needed. It enables you to easily, quickly and accurately re-establish workpiece zero after shutting down, or power loss.
Advertisement
Advertisement
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
Advertisement
Key Features
- Conversational Programming
- G-code Format
- Position-Trac™
- Intuitive Screen Layout
- Closed-looped System with Precision Scales
- USB Memory Devices Supported
- Networking, USB pointing devices Supported
- Tool Table with Tool Length Compensation
- Program Preview Graphics
- Milling and Drilling Functions