Acu-Rite Control System MILLPWRG2 User Manual

							ACU-RITE MILLPWRG2 161
8.1 Milling and Drilling
Position/Milling
MILLPWRG2 offers several Position / Milling functions that let you 
program a Line, Arc, Blend (Arc), Blend (Chamfer), and Contour that 
can be accessed directly using the Position/Milling soft key popup 
menu.
Position / Drill
The Position / Drill function will move the table to specific position  
based upon the X and Y axes coordinates entered.
Press the Position / Milling soft key.
From the PGM screen, press the Pos key to access the Position / 
Drill dialogue.
Or press the Program Steps soft key, then press the Position / 
Milling soft key, and select Position / Drill from the popup 
menu.
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. 
						

							1628 Milling and Drilling
8.1 Milling and Drilling
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.
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.
Or press the Program Steps soft key, then press the Position / 
Milling soft key, and select Line from the popup menu.
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 or one-step milling function.
If the tool size and type listed in the Tool field are 
incorrect, change the tool settings before running the 
program. 
						

							ACU-RITE MILLPWRG2 163
8.1 Milling and Drilling
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 arcs sweep angle 
is measured from the X axis.
Entering data:
From the PGM screen, press the ARC key to access the Arc dialogue.
Or press the Program Steps soft key, then press the Position / 
Milling soft key, and select Arc from the popup menu.
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 arcs 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. 
						

							1648 Milling and Drilling
8.1 Milling and Drilling
If you need to enter a center coordinate, 3rd 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 Pointfield:
Enter your 3rd 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. 
The arc is tangent to the adjacent steps. 
An inverted blend is also an arc that connects two lines, two arcs, or a 
line and arc. They are perpendicular to the adjacent steps.
The two steps to be blended can, but dont have to, intersect or touch. 
If they dont come into contact with each other, check that the radius 
is large enough to connect them.
Its 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 blends radius, press the Close Contour soft key, and 
MILLPWR
G2 will blend the last step with the first step. 
						

							ACU-RITE MILLPWRG2 165
8.1 Milling and Drilling
Blend
Highlight a step within your program where you want to place a 
blend.
From the PGM screen, press the BLEND key to access the Blend 
dialogue.
Or press the Program Steps soft key, then press the Position / 
Milling soft key, and select Blend (Arc) from the popup menu.
Select the blend type. A blend is tangent to the two steps. An 
inverted blend is perpendicular to the two steps.
Check that the steps listed in the From and To fields are the steps 
to be blended. If theyre incorrect, press the CANCEL key and 
highlight the appropriate step.
Enter the blends 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 the USE key.
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.
Confirm that Blend is selected in the soft key. 
						

							1668 Milling and Drilling
8.1 Milling and Drilling
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.
From the PGM screen, locate the lines where the chamfer is to be 
inserted between.
Highlight the second line.
Press the BLEND key.
Or press the Program Steps soft key, then press the Position / 
Milling soft key, and select Blend (Chamfer) from the popup menu.
Press the Chamfer soft key after the dialogue opens.
Check that the steps listed in the From and To fields are the steps 
to be blended. If theyre incorrect, press the CANCEL key and 
highlight the appropriate step.
For Length 1, enter the distance from the common point to the From 
line. 
For Length 2, enter the distance from the common point to the To 
line. 
Press the Closed soft key to chamfer the end of a contour with the 
beginning
Press the USE key. 
						

							ACU-RITE MILLPWRG2 167
8.1 Milling and Drilling
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, youll 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 youre 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 youve chosen. 
Select None as the type for whichever option you dont 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 Position / Milling 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.
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.
Select either Forward or Reverse for the direction of the finish pass.  
With Forward selected, the finish pass is made in the same direction 
as previous passes.  With Reverse selected, the finish pass is made 
in the opposite direction.
Press the USE key. 
						

							1688 Milling and Drilling
8.1 Milling and Drilling
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 datums 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 MILLPWRG2 169
8.1 Milling and Drilling
Rectangular milling functions
MILLPWRG2 offers several rectangular milling functions that let you 
program pockets, frames, faces and slots. For 2 axes systems, Refer 
to Chapter 1, Operating in 2 Axes and 3 Axes Modes on page 31.
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 three 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.
Using the coordinates of the center and the size 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 or a chamfer 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.
ARROW DOWN or press the More soft key and enter the table’s feed rate.
If programming by center and size, enter the Center X and Y axes 
coordinates.
You can tilt a rectangular pocket by identifying a tilt angle. Highlight 
the Angle field and enter an angle measured from the X axis. 
						

							1708 Milling and Drilling
8.1 Milling and Drilling
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 ramps or 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 pocket is machined at the feed rate programmed in the 
rectangle pocket step.  When the tool makes a cut greater than the 
step over such as the initial cut down the center of the pocket, the 
full cut override is applied to the feed.  The full cut override only 
applies to the rough pass.  The finish pass runs entirely at the 
programmed finish feed.
The Z step size is determined by the system and will not exceed the 
specified distance or number of passes.  
The tool retracts slightly (0.1 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 to both the bottom and side finishes.