Acu-Rite Control System MILLPWRG2 User Manual

							ACU-RITE MILLPWRG2 121
6.2 Folders
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 93.
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. 
						

							1226 Programming
6.2 Folders
G-code programs
G-code editing capabilities
G-code programs have basic editing capabilities. The value of an 
existing g-code address can be changed.
There are no soft keys available for editing, all navigation is done using 
the ARROW keys. Use UP and DOWN ARROW keys to move the cursor to the 
line that needs to be edited. And press ENTER to edit the line.
Use the LEFT and RIGHT ARROW keys to move from address value to 
address value within the line. Enter the new value for an address. The 
UP and DOWN ARROW keys do not function in this mode.
Only the value of an address when highlighted can be changed. The 
CANCEL key will cancel any edits made. The ENTER key and the LEFT or 
RIGHT ARROW key accepts changes made to an address, and then 
moves to the next address. The USE key accepts the changes to the 
line and allows use of UP and DOWN ARROW keys.
The values of the following addresses can be edited: F, I, J, K, L, M, 
N ,  O , P ,   S ,  T ,  X ,  Y ,  a n d  Z .   S e e  G-code and M-Code definitions starting 
on page 125.
A highlighted line can be removed by pressing the CLEAR key.
The MILLPWR
G2 will calculate the block form of the G-code program. 
The values for the block form can be viewed using the Block Form soft 
key. The block form can be edited and even inserted into the program 
by using the soft key Insert G120. Once inserted in the program 
(G120), the block form in the program is used. Remove the line 
containing the G120 to revert back to the calculated  block form. 
						

							ACU-RITE MILLPWRG2 123
6.2 Folders
Loading a G-code program
MILLPWRG2 has the ability to read and run G-code programs.  Basic 
editing is also possible. It is important to fully test the G-code program 
before machining a part.
A G-code program can be loaded into MILLPWR
G2 in the same 
manner as MILLPWRG2 programs. Once loaded, MILLPWRG2 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 by 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 93.
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.
Running a G-code program
MILLPWR
G2 has the ability to read and run G-code programs. 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. 
						

							1246 Programming
6.2 Folders
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. MILLPWRG2 will then offset the 
spindle by this amount. T2 will cause MILLPWRG2 to retrieve the tool 
length offset from tool 2 of the Tool Table, etc.  See chapter 4.1 Tool 
Table on page 68 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. 
						

							ACU-RITE MILLPWRG2 125
6.2 Folders
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 
G-codeDescriptionComment
G0 † Linear Interpolation (Rapid)
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). G1 † Linear Interpolation (Feed)
G2 † Circular Interpolation (CW)
G3 † Circular Interpolation (CCW)
G4 †DwellThis 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.
G17 † XY Plane Selection
These commands set the plane in which arcs are executed.  The setting 
applies to current and subsequent blocks.  The default is G17 (XY). G18 † XZ Plane Selection
G19 † YZ Plane Selection
G20 † Set Program Units (INCH)
Same functions as G70 and G71. These commands set the unit of 
measure.  The setting applies to current and subsequent blocks.  The 
default is G20 (INCH).
G21 † Set Program Units (MM) 
						

							1266 Programming
6.2 Folders
G-codeDescriptionComment
G28
Return to Home ReferenceMILLPWR
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. G30
G40 † Cancel Cutter Compensation MILLPWR
G2 supports automatic cutter compensation.  Enable cutter 
compensation using G41 (left) or G42 (right).  Disable compensation 
using G40 (center).
G41 † Cutter Compensation (Left)
G42 † Cutter Compensation (Right)
G43Tool Length Offset (+) MILLPWR
G2 does not support tool length offsetting. The offset is 
retrieved from MILLPWRG2’s tool library when a tool change is 
executed. These commands are ignored.
G44Tool Length Offset (-)
G49Cancel Tool Length 
G54
Work Coordinate SystemMILLPWR
G2 does not support presettable work coordinate systems. 
G54 through G59 are ignored.
G55
G56
G57
G58
G59 
						

							ACU-RITE MILLPWRG2 127
6.2 Folders
G-codeDescriptionComment
G61 † Set “stop” Path Mode
These commands set the path mode.  The setting applies to current and 
subsequent blocks.  The default is G64 (continuous).
G64 † Set “continuous” Path Mode
G70 † Set Program Units (INCH)
Same functions as G20 and G21. These commands set the unit of 
measure.  The setting applies to current and subsequent blocks.  The 
default is G70 (INCH). 
G71 † Set Program Units (MM)
G80 † Cancel Motion ModeThis command cancels the current modal drilling cycle. The modal 
drilling cycles are described below (G80 series).
G81 † Basic Drill CycleBasic 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
G82 † Counterbore Drill CycleCounterbore 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
G83 † Peck Drill CycleThe 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
G85 † Boring Bidirectional CycleBoring 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) 
						

							1286 Programming
6.2 Folders
G-codeDescriptionComment
G87 † Chip Break CycleThis 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 address 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)
G89 † Flat Bottom Boring CycleThis 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)
G90 † Set Offset Mode (ABS) 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) G91 † Set Offset Mode (INC)
G120 †Block Form 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 addresses.
G120 X(xMax) Y(yMax) Z(zMax) I(xMin) J(yMin) K(zMin)
G*All other G codes not listed will generate a run-time error. 
						

							ACU-RITE MILLPWRG2 129
6.2 Folders
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 
M-CodeDescriptionComment
M* † All other M codes not listed will generate a run-time error.
M0 † Program Stop This command pauses the program.  Press GO to resume.
M1 † Optional Program StopThis command pauses the program if the Optional Stop run option is 
selected.  Press GO to resume.
M2 † Program EndThis 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 † Spindle On (CW)
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. M4 † Spindle On (CCW)
M5 †Spindle Off
M6Tool ChangeM6 is not necessary.  A tool change occurs when the Tool Selection 
command is processed.
M7 † Coolant On (Mist)
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. M8 † Coolant On (Flood)
M9 † Coolant Off
M30Program End w/ Pallet ShuttleMILLPWR
G2 does not support control of a pallet changer.  This code has 
the same effect as M2. 
						

							1306 Programming
6.2 Folders
M-CodeDescriptionComment
M48Enable Speed/Feed Override It is not possible to disable feed rate override on MILLPWR
G2.  These 
commands are ignored.
M49Disable Speed/Feed Override
M60Program Stop w/ Pallet ShuttleMILLPWR
G2 does not support control of a pallet changer.  This code has 
the same effect as M0.