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: [phone] Fax: [phone] E-Mail: [e-mail] Web: www.boxford.co.uk

Boxford 190 VMC

Contents

Contents

1 Introduction

2 Running the Demonstration Program

3Axes and Tooling

3.1Fitting Tooling

3.2Axes, Datums and Offsets

3.3Tool Storage

3.4Tool Data Library and Catalogue

3.5Setting Up

3.6Datum Shift

4 Main Front End Menu

5CAD

5.1Cad Window

5.2Drawing Aids

5.3Drawing Tools

5.4Editing Objects

5.5Area Filling

5.6Machining Considerations

6CAM Processor

6.1Settings

6.2CAM Processor Error Messages

7File Imports

7.1Drawing File Import

7.2G&M Code Program Import

8Administration Mode

8.1Access & Password Setting

8.2Tool Library

8.3Material Cutting Data

8.4Park Position and Units

8.5CAM Processor Default Settings

8.6Language Settings

Boxford 190 VMC

Contents

9Cutter Path CAM Programming

9.1Functions

9.2Information Required

9.3Drawing a Component

9.4Example

9.5Defining Straight Line Moves

9.6Defining Arcs

9.7Pockets and PCD Drilling

9.7.1Rectangular Pockets

9.7.2Circular Pockets

9.7.3Slots

9.7.4PCD Drilling

9.7.5Dish Milling

9.8Cutter Radius Compensation

9.9ToolChanging

9.10Processing a Cutter Path

9.11Editing a CAM Program

10Manual Data Input CNC Programming

10.1Operations and Programming Sheets

10.2Absolute and Incremental Co-ordinates

10.3Speeds and Feeds

10.4Program Format

10.5Preparatory Functions (G Codes)

10.6Miscellaneous Functions (M Codes)

10.7Programming a Tool Change

10.8Inputting a New Program

10.8.1Information required

10.8.2Tabulated Format

10.8.3ZOOM Facility

10.8.4Compact Format

10.9Saving a Program

10.10Examining an Existing Program

10.10.1PROGRAM Display

10.10.2ZOOM and VIEW Facility

Boxford 190 VMC

Contents

10.10.3Simulation of Machining

10.11Editing a Program

10.11.1New Programs

10.11.2Existing Programs

10.11.3MENU Editing Options

10.11.4Changing the Initial Tool

10.12Continuing a Program

11CNC and CAM Machining

11.1Initial Checks

11.2Manufacture

11.3Options During Machining

12Manual Machining

13Robotic Interfacing

Boxford 190 VMC

Contents

CNC Tutorials and Exercises

Tutorial 1: X and Y Co-ordinate Calculation -

Absolute and Incremental Co-ordinates

Exercise1: CalculationofCo-ordinates

Tutorial 2: LinearInterpolation

Exercise2: Linear Interpolation - Absolute Co-ordinates

Tutorial 3: Canned Cycles - Hole Drilling and Pocket Milling

Exercise3: Canned Cycles - Programming a Tool Change

Tutorial 4: CircularInterpolation-ClockwiseandCounter-clockwise

Exercise4: CircularInterpolation

Tutorial 5: Combining Operations and Tool Changing

Exercise5: Combining Operations

Tutorial 6: Subroutines

Exercise6: Subroutines

Tutorial 7: Mirror Images

Exercise7: Mirror Images

Tutorial 8: Further Canned Cycles - Pitch Circle Drilling and Dish Milling

Exercise8: Use of Canned Cycles - Pitch Circle Drilling and Dish Milling

Tutorial 9: Subroutines, Mirror Images and Circular Interpolation

Exercise9: Subroutines and Mirror Images

Tutorial 10: Datum Shift and Jump to Line

Exercise10: Datum Shift and Jump to Line

OperationsSheet

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.

2 Running the Demonstration Program

Boxford 190 VMC

2Running the Demonstration Program

The demonstration program contains examples of linear and circular interpolation, rectangularandcircularpocketmillingandpitchcircledrilling,andafinishedcomponent 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 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 configuredbyselecting CONFIGfromthemainmenu.(RefertoSection5-Installation in the Installation and User manual, and Section 3 - Axes and Tooling).

Check Tool Settings 3. Fromthemainmenu,selectMACHINEandthenToolstodisplaytheToolDataLibrary. 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

Boxford 190 VMC

2 Running the Demonstration Program

5.SelectPROGRAM

The screen shows:

6.SelectPROGRAM

ThescreenshowstheCatalogueDisplay.Viewthecataloguetoidentifythedemonstration program, which is called VMC 190.

2 Running the Demonstration Program

Boxford 190 VMC

7.SelectVMC190

The screen shows the Program Display with a 2D view of the component.

Boxford 190 VMC

2 Running the Demonstration Program

View the Component	8. Select VIEW toproducea3Dviewofthecomponent.Afterapausethedisplaywill
	show the 3D view:

Manipulate the 3D view as follows:

UsingaMouse:

Click on the control buttons -

	Increase
	size
Rotate		Rotate
clockwise		anticlockwise
	Decrease	Restore
	size
		original view

2 Running the Demonstration Program

Boxford 190 VMC

Show the Program

Details

UsingtheKeyboard:

Increase

size

Rotate

Rotate

clockwise

anticlockwise

Decrease

size

Restore

HOME

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).

Boxford 190 VMC

2 Running the Demonstration Program

Display the Program

11. Select MENU and then Display:

Scroll the display to examine the program:

UsingaMouse:

Click on the buttons

page	1 line	1 line	page
down	down	up	up

UsingtheKeyboard:

Press

or

to scroll 1 line

	Press	Page	or	Page	to scroll 1 page
		up		down

12.Turn off the program display.

2 Running the Demonstration Program

Boxford 190 VMC

Zoom the Display	TheZOOMfacilityenablesarectangularareaoftheworkpiecetobeisolatedandviewed
	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
	completeworkpiece.
13.	Select	ZOOM .Thescreendisplaysa2Dviewoftheworkpiecewithamenubaratthe
	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 .AfterapausethescreenshowstheprogramEDITdisplaywitha3D
	view of the selected area of the workpiece.
15.	Select	ZOOM , then Unzoom to restore the 3D view of the complete workpiece.

Boxford 190 VMC

2 Running the Demonstration Program

SimulateMachining	16. Select MENU , then 2D Simulate:
- 2D

tool depth display

RepeatedlyclickthemousebuttonorpressReturntomovethroughtheprogramline-by- line. The simulation shows the tool movement and metal removed as each line of the program is executed.

Tomoveforwardthroughtheprogramtoaspecificline,select MENU ,andthenGo to Line. Type the required line number when prompted, and press Return.

Toproducea3Dviewoftheworkpiece,select MENU andthenSolidView.Toreturn to the 2D view, click the mouse button or press Return.

Torunthesimulationautomatically,select MENU andthenFastMode;theprogram 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.

2 Running the Demonstration Program

Boxford 190 VMC

SimulateMachining	17. Select MENU , then 3D Simulate:
- 3D

	Select MENU , and demonstrate the use of the options available as for the 2D
	simulation, until the screen again shows the program display.
Machinethe	Refer to Section 11 - CNC and CAM Machining.
Component

Boxford 190 VMC

Axes and Tooling

3 Axes and Tooling

3.1 Fitting Tooling (Figure 3.1)

Axes

Datum Position

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)

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

3.1 Axes and Tooling

				Drawbar lever
					DRAWING
				Spindle	Tool X,Y datum
				Tool holder
				Cutting tool
				Billet	+Y
					Rectangular
					billet
Tool X,Y datum	+				+X
	Z			+
	-	-	X		Drawing datum
	+
	Y -				Tool X,Y datum
				Workholding vice	+Y
					Circular
					billet
					+X
					Drawing datum

Figure 3.1 Axes and Tool Datum

Boxford 190 VMC

3.2 Axes and Tooling

Drawing Datum	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.
Offsets	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

3.2 Axes and Tooling

	Auto tool changer
Tool rack
(basic 190VMC)
Spindle
	Carousel
	To pressure gauge
Figure 3.2	Tool Storage

Boxford 190 VMC

3.3 Axes and Tooling

3.3 Tool Storage (Figure 3.2)

Tool Rack (Figure 3.2)

Auto Tool Changer (Figure 3.2)

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.
Manual Operation	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	The CNC code for a tool change is the same as for a standard machine. Using the M
Changer	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	The screen shows the Tool Data Library, (Figure 3.3). Practice selecting tools using
	the mouse and keyboard.
	1	2	3	4	7	5	6

Details of selected tool are highlighted.

When the display first appears, the initial tool is highlighted. Other tools can be selected as shown below.

1.	Tool number used by CNC program to select	5.	Scroll buttons
	required tool	6.	Tool offset
2.	Tool type (selected from tool catalogue)	7.	Tool flute length

3.Tool station (carousel)

4.Tool description (selected from tool carousel)

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

3.4 Axes and Tooling

Tooling Menu

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.

Tool Catalogue 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

3.5Axes and Tooling

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.
		Spindle	Carousel	Direction
				of rotation

Fit reference tool here

Figure 3.5 190 VMC with Auto Tool Changer - Reference Tool Position

Boxford 190 VMC

3.5 Axes and Tooling

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 MENU and then Edit tool.

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.

Boxford 190 VMC	3.5Axes and Tooling

1

2

3

1	To check tool type, press Escape or select	QUIT , then select MENU and
	Display tools to view tool catalogue.
2	Diameter of slot drill is 5.00mm

3Offset 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 OK to turn off display

Figure 3.6 Tool Editing Display

Boxford 190 VMC

3.5Axes and Tooling

10. Select MENU , and then Set Tool Offset. The screen shows:

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.

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

3.5Axes and Tooling

12.When the axes reach the home position, the screen shows:

Set Additional

Tool Offsets

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.

13. When the tool is in the correct position, select EOB or press Return. The screen 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 MENU and 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 YES or press Return to save the offsets.

Boxford 190 VMC

3.5 Axes and Tooling

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

3.5 Axes and Tooling

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

3.5 Axes and Tooling

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.