Milling and Drilling. 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
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
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