boxford 190 VMC Programming Manual
Programming Manual
Boxford 190 VMC
CNC Milling
Machine Tool
Boxford
Boxford Ltd.,
Wheatley, Halifax, West Yorkshire,
England, HX3 5AF.
(Registered Office)
Telephone: 01422 358311
Fax: 01422 355924
E-Mail: info@boxford.co.uk
Web: www.boxford.co.uk
Boxford 190 VMC Contents
Contents
1 Introduction
2 Running the Demonstration Program
3 Axes and Tooling
3.1 Fitting Tooling
3.2 Axes, Datums and Offsets
3.3 Tool Storage
3.4 Tool Data Library and Catalogue
3.5 Setting Up
3.6 Datum Shift
4 Main Front End Menu
5 CAD
5.1 Cad Window
5.2 Drawing Aids
5.3 Drawing Tools
5.4 Editing Objects
5.5 Area Filling
5.6 Machining Considerations
6 CAM Processor
6.1 Settings
6. 2 CAM Processor Error Messages
7 File Imports
7.1 Drawing File Import
7.2 G&M Code Program Import
8 Administration Mode
8.1 Access & Password Setting
8.2 Tool Library
8.3 Material Cutting Data
8.4 Park Position and Units
8.5 CAM Processor Default Settings
8.6 Language Settings
9 Cutter Path CAM Programming
9.1 Functions
9.2 Information Required
9.3 Drawing a Component
9.4 Example
9.5 Defining Straight Line Moves
9.6 Defining Arcs
9.7 Pockets and PCD Drilling
9.7.1 Rectangular Pockets
9.7.2 Circular Pockets
9.7.3 Slots
9.7.4 PCD Drilling
9.7.5 Dish Milling
9.8 Cutter Radius Compensation
9. 9 Tool Changing
9.10 Processing a Cutter Path
9.11 Editing a CAM Program
ContentsBoxford 190 VMC
10 Manual Data Input CNC Programming
10.1 Operations and Programming Sheets
10.2 Absolute and Incremental Co-ordinates
10.3 Speeds and Feeds
10.4 Program Format
10.5 Preparatory Functions (G Codes)
10.6 Miscellaneous Functions (M Codes)
10.7 Programming a Tool Change
10.8 Inputting a New Program
10.8.1 Information required
10.8.2 Tabulated Format
10.8.3 ZOOM Facility
10.8.4 Compact Format
10.9 Saving a Program
10.10 Examining an Existing Program
10.10.1 PROGRAM Display
10.10.2 ZOOM and VIEW Facility
Boxford 190 VMC Contents
10.10.3 Simulation of Machining
10.11 Editing a Program
10.11.1 New Programs
10.11.2 Existing Programs
10.11.3 MENU Editing Options
10.11.4 Changing the Initial Tool
10.12 Continuing a Program
11 CNC and CAM Machining
11.1 Initial Checks
11.2 Manufacture
11.3 Options During Machining
12 Manual Machining
13 Robotic Interfacing
CNC Tutorials and Exercises
Tutorial 1: X and Y Co-ordinate Calculation -
Absolute and Incremental Co-ordinates
Exercise 1: Calculation of Co-ordinates
Tutorial 2: Linear Interpolation
Exercise 2: Linear Interpolation - Absolute Co-ordinates
Tutorial 3: Canned Cycles - Hole Drilling and Pocket Milling
Exercise 3: Canned Cycles - Programming a Tool Change
Tutorial 4: Circular Interpolation - Clockwise and Counter-clockwise
Exercise 4: Circular Interpolation
Tutorial 5: Combining Operations and Tool Changing
Exercise 5: Combining Operations
ContentsBoxford 190 VMC
Tutorial 6: Subroutines
Exercise 6: Subroutines
Tutorial 7: Mirror Images
Exercise 7: Mirror Images
Tutorial 8: Further Canned Cycles - Pitch Circle Drilling and Dish Milling
Exercise 8: Use of Canned Cycles - Pitch Circle Drilling and Dish Milling
Tutorial 9: Subroutines, Mirror Images and Circular Interpolation
Exercise 9: Subroutines and Mirror Images
Tutorial 10: Datum Shift and Jump to Line
Exercise 10: Datu m Shift and Jump to Line
Operations Sheet
Programming Sheet
1 Introduction
This manual gives guidance in using the 190VMC CAD/CAM software to create ISO
G& M code programs for milled components.
The 190VMC CAD/CAM software includes a demonstration program (called
190VMC), and a number of tutorial programs.
It is suggested the manual is used as follows:
1. Refer to section 2 and run the demonstration. This will provide rapid familiarisation
with the operation of the software and the machining process.
2. Study Section 3 to become proficient in setting up the tooling.
3. Refer to sections 4, 5 and 6 to demonstrate the ease of operation of the integrated CAD
and CAM processor package.
4. Refer to Section 7 to become familiar with the conventions for importing drawing files
from third party CAD packages and G & M programs from CAM packages.
5. Refer to Section 8 for details of the functions available to administrators (tutors) of the
CAD/CAM system.
6. Refer to section 9 for computer assisted cutter path generation.
7. Use section 10 for detailed instruction in CNC programming.
Tutorial 2 is used as an example to demonstrate the stages of programming and
software operation.
8. Use the Tutorials and Exercises in the order in which they appear, to progress from
basic programming skills to proficiency in the more advanced features of CNC
programming.
9. When programs have been written and verified, refer to section 6 as required, to
machine components.
Boxford 190 VMC
2 Running the Demonstration Program
2 Running the Demonstration
Program
The demonstration program contains examples of linear and circular interpolation,
rectangular and circular pocket milling and pitch circle drilling, and a finished component
can be machined from the billet supplied with the machine. Run the program as follows
to provide a tutorial in programming and machining.
Setting Up the Machine
Check Tool Settings
1. Set up the tooling and billet as follows:
6mm slot drill fitted in cutter holder, secured in spindle.
3mm slot drill ready for the programmed toolchange.
Billet: plastic, length 75.00 mm, width 60.00mm, height 10.00mm, securely fitted in vice.
2. Run the software and check that the Simulation and Manufacture software is correctly
configured by selecting CONFIG from the main menu. (Refer to Section 5 - Installation
in the Installation and User manual, and Section 3 - Axes and Tooling).
3. From the main menu, select MACHINE and then Tools to display the Tool Data Library.
Check the setting of the reference tool, and the second tool, which should be as follows:
No. Type Pos Description Diameter Length Offset
1 2 1 Slot drill 6.00 7.50 0.00
2 2 2 Slot drill 3.00 7.50 0.00
If the settings are incorrect, refer to Section 3 - Axes and Tooling, 3.5 - Setting Up.
4. Turn off the display.
The screen shows: Main Menu
2 Running the Demonstration ProgramBoxford 190 VMC
5. Select PROGRAM
The screen shows:
6. Select PROGRAM
The screen shows the Catalogue Display. View the catalogue to identify the demonstration
program, which is called VMC 190.
Boxford 190 VMC
2 Running the Demonstration Program
7. Select VMC 190
The screen shows the Program Display with a 2D view of the component.
2 Running the Demonstration ProgramBoxford 190 VMC
View the Component
8. Select
VIEW
to produce a 3D view of the component. After a pause the display will
show the 3D view:
Manipulate the 3D view as follows:
Using a Mouse:
Click on the control buttons -
Rotate
clockwise
Increase
size
Decrease
size
Rotate
anticlockwise
Restore
original view
Boxford 190 VMC
2 Running the Demonstration Program
Show the Program
Details
Using the Keyboard:
Rotate
clockwise
Increase
size
Decrease
size
Rotate
anticlockwise
HOME
Restore
original view
Note:
The time taken for the display to respond will depend on the speed of the PC and whether a co-processor
is fitted.
9. Select
INFO
to show the program details:
10. Turn off the program details display. (Click off the display window or press Return).
2 Running the Demonstration ProgramBoxford 190 VMC
11. Select
MENU
and then Display:Display the Program
Scroll the display to examine the program:
Using a Mouse:
Click on the buttons
page
down
Using the Keyboard:
Press or to scroll 1 line
Page
Press or to scroll 1 page
12. Turn off the program display.
➔
up
1 line
down
1 lineuppage
up
➔
Page
down
Boxford 190 VMC
2 Running the Demonstration Program
Zoom the Display
The ZOOM facility enables a rectangular area of the workpiece to be isolated and viewed
in greater detail for editing purposes. Full use of the facility is explained in Section 10 -
Manual Data Input CNC Programming, 10.8.3 - ZOOM Facility.
The following steps provide a brief demonstrations, returning to the display of the
complete workpiece.
13. Select
ZOOM
. The screen displays a 2D view of the workpiece with a menu bar at the
top, and sliders and arrow buttons arranged horizontally and vertically.
Explore the use of the REDUCE and ENLARGE options, and the sliders and arrow
buttons, to define a section of the workpiece with the rectangular selecting frame.
(RESET restores the frame to its original size).
14. Select
ACCEPT
. After a pause the screen shows the program EDIT display with a 3D
view of the selected area of the workpiece.
15. Select
ZOOM
, then Unzoom to restore the 3D view of the complete workpiece.
2 Running the Demonstration ProgramBoxford 190 VMC
Simulate Machining
- 2D
16. Select
MENU
, then 2D Simulate:
Repeatedly click the mouse button or press Return to move through the program line-by-
line. The simulation shows the tool movement and metal removed as each line of the
program is executed.
To move forward through the program to a specific line, select
MENU
to Line. Type the required line number when prompted, and press Return.
tool
depth
display
, and then Go
To produce a 3D view of the workpiece, select
MENU
and then Solid View. To return
to the 2D view, click the mouse button or press Return.
To run the simulation automatically, select
MENU
and then Fast Mode; the program
will be run in a continuous sequence. To return to line-by-line simulation, select
MENU
and then Step Mode.
To end the simulation before the end of the program, click on the 'off' button or press
ESC
.
At the end of the program the screen returns to the program display.
Boxford 190 VMC
2 Running the Demonstration Program
Simulate Machining
- 3D
Machine the
Component
17. Select
Select
MENU
MENU
, then 3D Simulate:
, and demonstrate the use of the options available as for the 2D
simulation, until the screen again shows the program display.
Refer to Section 11 - CNC and CAM Machining.
Boxford 190 VMC
Axes and Tooling
3 Axes and Tooling
3.1 Fitting Tooling (Figure 3.1)
The cutting tool fits directly into a tool holder and is secured in position by a single
Allen screw.
The tool holder in turn fits into the machine spindle taper and is orientated by two dogs
which engage with the tool holder flange.
The tool holder pull stud is then drawn upwards by the spindle drawbar thus securing
the tool holder.
The drawbar can be manually operated by a lever on the side of the spindle or an
automatic tool changing device can be specified if required.
3.2 Axes, Datums and Offsets (Figure 3.1)
Axes
Datum Position
Figure 3.1 shows the movement of the tool in the X, Y and Z axes, in relation to the
billet. (In the X and Y axes the billet moves in relation to the tool, but for simplicity
and to conform with standard programming practice, it is the movement of the tool
in relation to the billet which must be considered).
On new machines, all Datum positions and Tool Offsets are set at the factory when tooling and clamping
is ordered with the machine.
The offsets of all required tools are set in relation to the machine Z datum.
Before any Tool Offsets can be set, the Machine Z Datum has to be defined.
From the machines Home Position, the Machine Z Datum is the measured distance from
the underside of the of the spindle head to the machine table top as shown in the diagram overleaf.
The X and Y Datum is the distance from the spindle centreline to a fixed point on the machine
table where the same corner of every workpiece locates to. (on a standard Vice, this is the imaginary
intersection of the vice rear jaw and the left hand end stop - a point where the Left Hand
corner of a workpiece locates to).
The datum position can be set to reference from Back Left, Back Right, Front Right
and Front Left corners of the workpiece (see section 3.5 - point 15 onwards for further
details).
Boxford 190 VMC Axes and Tooling
Drawbar lever
3.1
DRAWING
Tool X,Y datum
Spindle
Tool holder
Cutting tool
Tool X,Y datum
+Y
Billet
Rectangular
billet
+X
+
Z
X
+
Drawing datum
Tool X,Y datum
Workholding vice
+Y
Circular
billet
-
+
Y
-
-
+X
Figure 3.1 Axes and Tool Datum
Drawing datum
Boxford 190 VMC Axes and Tooling
3.2
Drawing Datum
Offsets
Dimensions on drawings are measured from the drawing datum. For convenience this
can be placed at the bottom left-hand corner of the billet and given X and Y co-
ordinates of zero. When a component is manufactured, the difference between the Y
co-ordinates of the tool and drawing datums is entered and the software compensates
for this difference.
The 190 software also allows the use of circular billets. For these, the X and Y datum
is usually at the bottom left hand corner of a square enclosing the billet.
Each tools offset is the distance from the Underside of the Spindle Head to the
tool end (bottom).
Underside of Head
Tool Z Offset
Machine Z Datum
Total Height of
Workpiece & Clamp
Machine Table Top
Boxford 190 VMC Axes and Tooling
Tool rack
(basic 190VMC)
Spindle
3.2
Auto tool changer
Figure 3.2 Tool Storage
Carousel
To pressure gauge
Boxford 190 VMC
3.3 Tool Storage (Figure 3.2)
3.3
Axes and Tooling
Tool Rack
(Figure 3.2)
Auto Tool Changer
(Figure 3.2)
Manual Operation
On the basic 190 VMC a tool rack is provided, as shown in Figure 3.2, to facilitate
storage of up to 5 tool holders and associated cutting tools.
It is advisable to store the tools in the same order as they will be called for in the
machining program.
Automatic tool changing equipment is supplied as an optional extra .
A carousel facilitates storage of up to 5 tool holders and associated cutting tools. Each
tool holder must be loaded into the correct carousel station so as to correspond with
the machining program prior to cycle start, i.e.:
Tool No.1 = Station No.1
Tool No.2 = Station No.2
The machine cycle start cannot be activated until the carousel has been indexed to Tool
No. 1, the reference tool station.
The auto tool changer is a pneumatic device requiring a compressed air supply of 80
lbf/in2.
Ensure therefore that the system pressure gauge reads 80 lbf/in2 prior to operating the
auto tool changer controls.
Pressing the Tool Change button on the main control panel will direct the auto tool
changer to remove the tool holder currently in the spindle, place it in the correct
carousel station, index the carousel to the next station, secure the next tool holder into
the spindle and retract.
Note:
When using the Tool Change button ensure that the spindle is at least 5mm below the upper Z+
limit of its travel.
Programming the Auto Tool
Changer
The CNC code for a tool change is the same as for a standard machine. Using the M
code M06 you must define the tool type e.g. type 2 (a slot drill), the diameter of the
tool and the station number 1 5 in the carousel, for example:
M06 I2 J6 F4
Where I = a slot drill
J = diameter of 6mm
F = station No. 4.
On completion of the part-program the machine will automatically change back to tool
1 allowing batch quantities to be machined.
Boxford 190 VMC
3.4
Axes and Tooling
3.4 Tool Data Library and Catalogue
The 190 software provides a Tool Data Library which enables details of tooling and
offsets to be entered and a tool catalogue from which tools can be selected for inclusion
in the library. The library is set up by means of a tooling menu.
Before attempting to set up the tooling for the first time, view the library, the tooling
menu and the catalogue to become familiar with the details, as follows:
1. Switch on the PC, run the 190 Software.
2. From the main menu, select MACHINE and then Tools.
Tool Data Library
Details of selected tool are highlighted.
When the display first appears, the initial
tool is highlighted. Other tools can be
selected as shown below.
The screen shows the Tool Data Library, (Figure 3.3). Practice selecting tools using
the mouse and keyboard.
3412
1. Tool number used by CNC program to select
required tool
2. Tool type (selected from tool catalogue)
3. Tool station (carousel)
4. Tool description (selected from tool carousel)
567
5. Scroll buttons
6. Tool offset
7. Tool flute length
To select a tool:
Using a mouse
Click on the scroll buttons (6) to highlight the required tool.
Using the keyboard
Press ➔ or ➔ to highlight the required tool.
Figure 3.3 Tool Data Library
Boxford 190 VMC Axes and Tooling
3.4
Tooling Menu
Tool Catalogue
3. Select MENU to display the tooling menu:
The use of these options for setting and editing the Tool Data Library is detailed later
in this section.
Note:
After setting up or editing the library, always select Save Tool data.
4. From the tooling menu, select Display Tools.
The screen shows the tool catalogue, (Figure 3.4).
Turn off the tool catalogue display to reveal the Tool Data Library.
Figure 3.4 Tool Catalogue
Boxford 190 VMC Axes and Tooling
Spindle Carousel Direction
of rotation
Fit reference
tool here
3.5
3.5 Setting Up
Note:
A billet of the appropriate size will be required for this procedure. In order to run the demonstration
program, a 5mm slot drill and a 5mm end mill are required. To run the program, set up the slot drill
as the initial tool and the end mill as the second tool in the following procedure. If you want to fit a
different initial tool or second tool, substitute the tool details as appropriate.
Fit Initial Tool
Fit the billet into the workholder, then fit the tooling as detailed below:
1. Basic 190 VMC with Tool Rack
Fit the 5mm slot drill into the tool holder and secure the tool
holder into the spindle by operating the drawbar lever (Figure 3.1).
If the spindle is too close to the work holding vice to allow the tool to be fitted then
use the manual controls to move the spindle up until sufficiently clear. (See Section 12
- Manual Machining).
2. 190 VMC with Auto Tool Changer
Fit the 5mm slot drill into the tool holder and secure the tool holder into the carousel
as shown in Figure 3.5.
Ensure that the spindle is in the correct Z+ position to facilitate auto tool changing.
Press the TOOL CHANGE button on the control panel.
The carousel will then traverse left to the spindle position, perform the actions of
removing a tool holder from the spindle, index to the reference tool, load and secure
the reference tool into the spindle, and retract.
The reference tool is now fitted in the spindle.
Figure 3.5 190 VMC with Auto Tool Changer - Reference Tool Position
Boxford 190 VMC Axes and Tooling
3.5
Configure Software
Set Initial Tool Offset
3. Check that the POWER ON RESET button on the machine control panel is lit.
4. Run the 190 Software. From the main menu select CONFIG and then Program.
5. Set the required values and turn off the display.
The screen shows:
6. Select YES
7. Select CONFIG and then Hardware. Make the required settings, turn off the display,
and save the settings.
The screen shows the Main Menu.
8. From the main menu, select MACHINE and then Tools to display the Tool Data
Library. The settings for the 5mm slot drill will be highlighted, for example:
Check the tool details (excluding the offset). If they are correct, continue at step 10 to
set the offset.
9. To edit the tool details, select
The screen shows the tool editing display, with the first item (Tool type) highlighted,
(Figure 3.6).
Edit the display to show the correct settings.
MENU
and then Edit tool.
Boxford 190 VMC Axes and Tooling
QUIT
OK
3.5
1
2
3
1 To check tool type, press Escape or select
Display tools to view tool catalogue.
2 Diameter of slot drill is 5.00mm
3 Offset for reference tool is zero.
To edit tool details:
Type required number in highlighted box
Press Return to highlight next box
When last box is highlighted, press Return: highlight will disappear
Press Return or click on
Figure 3.6 Tool Editing Display
, then select
to turn off display
MENU
and
Boxford 190 VMC Axes and Tooling
3.5
10. Select
If the touch-on point is to be the top of the billet, enter the height of the billet. If the
touch-on point is to be the base of the workholder, enter zero.
11. If the Software detects the machine is in Manual Mode, the user is prompted to
Cancel Manual Mode
The window below is shown.
MENU
, and then Set Tool Offset. The screen shows:
1. The machine RESET button is pressed.
2. a. The Z+ and Z- keys are pressed simultaneously (this axis must reach
home position before step b. can be started.
b. The X+ and X- keys are pressed simultaneously.
c. The Y+ and Y- keys are pressed simultaneously
2. ALTERNATIVELY, the F1 function key on the PC keyboard can be
pressed. This automatically performs steps a, b and c.
Boxford 190 VMC Axes and Tooling
12. When the axes reach the home position, the screen shows:
On the machine control panel, select Manual mode. Using the axis control buttons,
touch the point of the tool on to the top of the billet.
3.5
Set Additional
Tool Offsets
13. When the tool is in the correct position, select
again shows the Tool Data Library.
If additional tool offsets are to be set, continue at step 14. If not, continue at step 15
to set the machine datum position.
14. To set the offset of the next tool, fit or index the tool and repeat the procedure from
step 8.
Note:
For setting the offsets of the second and any subsequent tools, it will not be necessary to enter the height
of the billet or to home the axes (steps 10 and 11).
When the offsets of all the required tools have been set, either select
then Save Tool Data, or click the 'off' button of the Tool Data Library display. If the
'off' button is clicked, the screen shows the message:
Click on
or press Return to save the offsets.
YES
or press Return. The screen
EOB
MENU
and
Boxford 190 VMC Axes and Tooling
3.5
Set Machine
Datum Position
Note
It is only necessary to set the datum position if the workholder position is changed or the Datum
position (back, front, left, right) is changed
15. There are now a number of additional Datum Position options.
Datum Position - Select CONFIG and then Hardware.
The window below is shown.
With the DATUM POSITION option highlighted, the options can be accessed
and selected using ALTER.
The datum position is:- a point on the machine table where the same corner of every workpiece
locates to.
e.g. On a VMC machine fitted with a standard Vice, the workpiece BACK face locates
to the fixed rear vice jaw and the workpiece LEFT face locates to the vice end stop
- hence the setting would be BACK LEFT
The Datum Position is selected and the settings saved.
From the main menu, select MACHINE and then Datum Position.
Boxford 190 VMC Axes and Tooling
3.5
16. Select
SETUP
. The screen shows the Enter a Tool display:
17. Select a tool for which the offset has been set, (for example tool no. 1), and
select
ACCEPT
or press Return.
If the Software detects the machine is in Manual Mode, the user is prompted to
Cancel Manual Mode
The window below is shown.
1. The machine RESET button is pressed.
2. a. The Z+ and Z- keys are pressed simultaneously (this axis must reach
home position before step b. can be started.
b. The X+ and X- keys are pressed simultaneously.
c. The Y+ and Y- keys are pressed simultaneously
2. ALTERNATIVELY, the F1 function key on the PC keyboard can be
pressed. This automatically performs steps a, b and c.
Boxford 190 VMC Axes and Tooling
3.5
18. When the axes reach the home position, the screen shows:
Measure the dimension (from the underside of the spindle head to the machine table
top), and enter the value. (This establishes the Z axis datum).
19. Select
OK
or press Return twice. The screen shows:
Note:
The Face of the billet to touch on will depend on the Datum Position setting in the Hardware
configuration - see point 15
On the machine control panel, press MAN to select Manual mode. Use the axis control
buttons to touch the side of the tool on to the left face of the billet. (This establishes
the X axis datum; the software compensates for the radius of the tool).
20. When the tool is in the correct position, select
ENTER
or press Return. The message
on the display now prompts you to touch on to the rear face of the workpiece with the
selected tool.
Using the axis control buttons, follow the instructions to establish the Y datum in the
same way as for the X datum.
Loading...