Copyright: Copyright © 2000 - Denford Limited - Version 1.0
Citation: Copyright © 2000 - Denford Limited - VR CNC Turning for Windows software helpfile - Version 1.1 - No part of this helpfile may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose, without the express written permission of Denford Limited.


Block Skip
Options Toolbar: [Block Skip] button.

Click this button to active the block skip option.  The current setting of the option is displayed in the main program status bar.

When a forward slash character, / , is followed by a block number (at the beginning of a block) and the block skip option is active, the block will be ignored in memory operation.

When the block skip option is inactive, then the blocks indicated by the / characters will be considered as valid.

For example,

N3Ø  X4Ø ;

/ N4Ø  Z5Ø ;

/ N5Ø  X7Ø ;

/ N6Ø  Z9Ø ;

N7Ø .....

If the block skip option is active, then blocks indicated by the / character are ignored.  In the above example, block numbers N40, N50, and N60 will be ignored when block skip is active.

Note:  A / character must be specified at the start of the block.  If it is placed elsewhere in the block, the information from the / character to the ; character (the end of block mark) will be ignored, whilst the information before the / character will be effective.


Cascade
"Windows|Cascade"

Select this option to display any open windows in a cascading pattern, one on top of another (shown above).  This option is applied to any windows open in the VR CNC Turning software.  The window that is currently active in the VR CNC Turning software will be placed as the prime (visible) viewing window.

Any windows open in the VR CNC Turning software will be listed under the "Cascade" and "Tile" options, as shown in the example below.  The currently active window is always highlighted by a tick mark.  To move focus to a different window, click on the window title required.  This is particularly useful for switching between windows when viewing in "Cascade" mode.


Co-ordinate Based System
CNC Theory: The Co-ordinate Based Grid System

Precise points are plotted on the CNC machine using the positions of the X and Z axes.

These X and Z values relate to a two dimensional grid, as shown in the example below.

The zero point of this grid is called the datum.


Co-ordinate System Display Modes
CNC Theory: Co-ordinate System Display Modes

The CNC machine can plot co-ordinate movements using two different modes:

Machine Co-ordinates:  Any co-ordinate values plotted relate to the fixed machine datum.  The co-ordinate display always shows the true position of the machine.  The machine datum position is set by your CNC machine manufacturer and can never be moved, since it defines the physical movement capability of the machine.

When running in Machine Co-ordinates Mode, the Machine Datum (Home position) is displayed with the position X=0, Z=0.

Workpiece Co-ordinates:  Any co-ordinate values plotted relate to the programmed workpiece datum.  The co-ordinate display shows the position of the machine when any offsets are being used.  The workpiece datum is set by the operator as the location where we want any machining to begin.  Offsets temporarily shift the entire co-ordinate based grid system of the machine, as shown below.

When running in Workpiece Co-ordinates Mode or 'Program' coordinates, the Billet/Workpiece Datum is displayed with the position X=0, Z=0.


Computer Specifications

The following are MINIMUM and RECOMMENDED computer specifications for running the VR CNC Turning software:

MINIMUM Specification

Pentium 120MHz.

24Mb RAM.

Colour Monitor running at 800 x 600 resolution with 16bit (High Colour) graphics.

100% Microsoft compatible Mouse.

1 free serial port.

1 free Parallel port.

Windows 95 Operating System.

10Mb Free hard disk space.

RECOMMENDED Specification

Pentium 166MHz MMX.

32 Mb RAM.

Colour Monitor running at 1024 x 768 resolution with 16bit (High Colour) graphics.

100% Microsoft compatible Mouse.

2 free serial ports.

1 free parallel port.

Windows 98 Operating System.

10Mb Free hard disk space.

Frequently Asked Questions

Q.  Will the software run on Windows NT / Windows200 ?

A.  Yes, but there may still be issues arising from different service pack releases.

Q.  Do I need a special graphics card for VR?
A.  No, but the Virtual Reality CNC Machine Worlds operates better with a 'Hardware Accelerated' graphics card.

Q.  Can I user my Desk Top Tutor with the new software?
A.  Special overlays have been developed to allow the Desktop Tutor to drive the software.	However, you will still to use a mouse and keyboard for some features.

Q.  Can I upgrade my existing machine tool to run with the new software?

A.  Yes, providing that your existing machine is controlled by a EuroStep, SmartStep or DenStep controller running at 16 MHz.  Contact our Customer Services Dept. with your machines Serial Number to find out if your machine can be upgraded.  If this is the case then you just require a chip change in the machines controller plus the software upgrade.  Price yet to be confirmed.  Remember that the Computer Specification quoted above still applies and you may need to upgrade your machines PC too.


Configure Utilities
"Utilities | Configure Utilities..."

The "Configure Utilities" window (shown above) is used to setup shortcuts to other "Windows" programs.  In the example above, we have added shortcuts to the Denford TurnCAM Designer program (for design and generation of simple CNC files) and Windows Paint (to view any bitmaps we save when using the VR CNC Turning software).  When a program is highlighted, use the blue up and down arrow buttons to arrange the order of the list that appears in the "Utilities" menu (see the last screenshot on this page).  Use the [Add] button to specify a new program (see below).  Use the [Edit] button to change any properties on the highlighted program.  Use the [Delete] button to remove a highlighted program from the "Utilities" menu.

The "Utilities Properties" window (shown above) is used to specify any new programs.  Words entered in the "Title" dialogue box will appear in the lists in both the "Configure Utilities" window and the "Utilities" menu.  Use the [...] button opposite the "Program:" dialogue box to specify the new program executable file.  Use the [...] button opposite the "Working dir:" dialogue box to specify the working directory for the new program.  Use the "Parameters" dialogue box to set any specific actions for the new program.

Click the [OK] button to add the new program to both the "Configure Utilities" window and the "Utilities" menu

When the "Utilities" menu is selected, any programs added into the "Configure Utilities" window will appear in the dropdown list.  Highlight and click the title of the required program to start it.


Context Sensitive G and M code Help

To obtain context sensitive help on an individual G or M code within the CNC file, position the "Editor" window cursor in the middle of the text for the code required, highlighted red in the above screenshot.

Click the [Ctrl + F1] keys to display the appropriate menu topic from the CNC Milling Programming helpfile, as shown above.

Note - The CNC Milling Programming helpfile is always displayed on top of the VR CNC Turning software.


Context Sensitive Menu Help

To obtain context sensitive help on a menu in the VR CNC Turning software, click the required menu title to display its dropdown list of options, highlighted red in the above screenshot.

Click the [F1] key to display the appropriate menu topic from the VR CNC Turning helpfile, as shown above.


Context Sensitive Window Help

To obtain context sensitive help on a window in the VR CNC Turning software, click the required window so it becomes active, highlighted red in the above screenshot.

Click the [F1] key to display the appropriate menu topic from the VR CNC Turning helpfile, as shown above.


Conventions used in this Helpfile

Mouse Usage

When asked to click on a menu tile or object, click the LEFT mouse button ONCE.  When asked to right click on a menu tile or object, click the RIGHT mouse button ONCE.  When asked to double click on an object, click the LEFT mouse button TWICE.

"Quotation Marks"

Quotation marks are used to specify any software menu, title and window selections, e.g. click the "File" menu would mean click the left mouse button once, when the cursor is positioned over the File menu label.

When a sequence of menu commands are requested, the menu and option names are separated by a vertical line, for example - Click "File | Open" would mean open the File menu, then click on the Open option.

Bold Text

Bold Text is used to show any characters, or text, that must be entered, e.g. type file1 would mean type the word file1 into the appropriate text entry box.

[Square Brackets]

Square brackets are used to show any on-screen software button selections, e.g. Click the [OK] button would mean click the left button of the mouse once, when the cursor is directly pointing over the button labeled OK.

[Bold Square Brackets]

Bold square brackets containing text show individual keys to press on your qwerty keyboard, e.g. press [Enter] would mean press the Enter key.

If a number of  keys must be pressed in sequence they are shown with plus signs outside any square brackets, e.g. press [Alt] + [Enter] would mean press the Alt key first followed by the Enter key second.

If a number of keys must be pressed simultaneously they are shown with plus signs inside any square brackets, e.g. press [Alt + Enter] would mean press both the Alt key and Enter key together, at the same time.

Screenshots

Please note that any screenshots are used for explanation purposes only.

Any numbers, wording, window or button positions may be different for the configuration of the VR CNC Turning software you are using.

Language

Please note that this helpfile is written in European English.

Updates

We take great pride in the accuracy of information given in this helpfile, but due to nature of software developments, be aware that software specifications and features of this product can change without notice.  No liability can be accepted by Denford Limited for loss, damage or injury caused by any errors in, or omissions from, the information supplied in this helpfile.

Denford VR CNC Turning Helpfile - version 1.0

Any comments regarding this helpfile should be referred to the following e-mail address:

mailto:customer_services@denford.co.uk

Any updates to this helpfile will be posted in the 'Downloads' section of the Denford website:

http://www.denford.co.uk


Cycle Expansion
"Setup | Cycle Expansion"

This feature expands program cycles, such as repeat drilling operations, to show full the code enclosed in the program cycle in question.  The expanded code is shown line by line in a dialogue box at the base of the "Editor" window.

The screen above shows an example CNC file running an expanded program cycle operation.


Default Billet Size
"Setup | Default Billet Size..."

Select this option to define the size of the billet used in the 2D Simulation, 3D Simulation and Virtual Reality windows.

Enter values for each of the two parameters (outlined below) in the appropriate dialogue boxes.  Note - the numerical values entered must match the units of measurement currently in use by the software (see the menu option Setup | Units).  Click the [OK] button to set the default billet size parameters.

"Z Size" defines the length of the billet.

"X Size" defines the diameter of the billet.


Default Tooling Library

The following list contains the tool profiles available in the "Tooling Library" window, upon initial installation of the VR CNC Turning software.

(All values shown as Metric but would be displayed in Inches if you were in Imperial units - see Setting the Units of Measurement )

Roughing Tool

Tip Size=12

Length=60

Width Diameter=12

Grooving Tool

Tip Size=6

Length=60

Width Diameter=12

Internal Thread

Tip Size=9

Length=60

Width Diameter=12

Boring Bar

Tip Size=12

Length=60

Width Diameter=12

Center Drill

Tip Size=10

Length=80

Width Diameter=19

External Thread

Tip Size=12

Length=60

Width Diameter=12

Finishing Tool

Tip Size=12

Length=60

Width Diameter=12

Drill

Tip Size=15

Length=80

Width Diameter=12

Parting Off Tool

Tip Size=4

Length=60

Width Diameter=12

Pusher

Length=60

Width Diameter=12

TipIndex=18


Editor | Hi-light
"Editor | Hi-light | {choose from list of address letters}"

The "Hi-Light" option is used to visually display certain address codes.  Address codes are the single letters that make up CNC file words, for example address G in the CNC file words G1, G2, G3 etc.

Click on the address letter required and the words associated with that address letter will be highlighted in colour against the remainder of the CNC file.  In the example above, the address letter G has been selected.

To clear the Hi-Lights from the CNC file, select menu:  "Editor | Show Normal".  The example above shows the normal display for the 'Editor' window.


Example CNC file Stucture

Composition of a CNC file

A CNC file, or Part Program, is a list of coded instructions which describes how the designed component, or part, will be manufactured.

These coded instructions are called data - a series of letters and numbers.  The part program includes all the geometrical and technological data to perform the required machine functions and movements to manufacture the part.

The part program can be further broken down into separate lines of data, each line describing a particular set of machining operations.  These lines, which run in sequence, are called blocks.

A block of data contains words, sometimes called codes.  Each word refers to a specific cutting/movement command or machine function.  The programming language recognised by the CNC, the machine controller, is an I.S.O. code, which includes the G and M code groups.

Each program word is composed from a letter, called the address, along with a number.

Part Program Example

[BILLET X25 Z55

O0001

G21

G99

M06 T0101

G97 S1500 M03

G00 X25 Z0

G01 X-1 F.05

G00 X25 Z2

G71 U1.5 R.25

G71 P1 Q2 U1.0 W.1 F.07

N1 G00 X0

G01 Z0

G03 X17 Z-8.5 R8.5

G01 Z-13.5

X20 Z-14.36

Z-28.5

X24 Z-46.5

X26

N2 G00 X26 Z2

G70 P1 Q2

G28 U0 W0

M06 T0303

G97 S350 M03

G00 X20.5 Z-10

G76 P050060 Q035 R.05

G76 X18.00 Z-26.5 P1000 Q070 F1.5

G28 U0 W0

M30

Block example:  N2 G00 X26 Z2

Word example:  G03

Address example:  G


Glossary

ABSOLUTE:  In absolute programming, zero is the point from which all other dimensions are described.

ARC:  A portion of a circle.

AUTOMATIC CYCLE:  A mode of control operation that continuously runs a cycle or stored program until a program stop or end of program word is read by the controller.

AUXILIARY FUNCTION:  The function of the CNC machine (ie, F, S, T, M codes etc.), other than co-ordinate based commands.

AXIS (AXES):  The planes of movement for the cutting tool, usually referred to as X (horizontal left and right, parallel to the front edge of the table), Y (horizontal forward and backwards, parallel to the side edge of the table) and Z (directly vertical).  Combinations of all 3 allow precise co-ordinates to be described.

BILLET:  The actual material being machined, sometimes referred to as the "workpiece".

BLOCK:  A collection of program words that collectively describe a machining operation.  A single program line in the CNC file.

CHARACTER:  A number, letter or symbol as entered into a CNC program.

CIRCULAR INTERPOLATION:  G-code term for a programmed arc movement.

COMMAND:  A signal (or group of signals) instructing one step / operation to be carried out.

CO-ORDINATES:  Positions or relationships of points or planes.  Co-ordinates are usually described using three numbers referring to the (X,Y,Z) axes, e.g. the co-ordinate (23,35,45) means X axis = +23 units, Y axis = +35 units and Z axis = +45 units.

CNC:  Computer Numerical Control.

CNC FILE:  The sequence of commands describing the manufacture of a part on a CNC machine, written using G and M codes, also called the CNC program.

CUTTER SPEED:  The velocity of the cutting edge of the tool relative to the workpiece.  With circular tools, the cutting speed is related to the tool when new (maximum cutting diameter).  Usually the effect of feedrate is ignored.

CYCLE:  A sequence of events or commands.

DATUM:  The point (co-ordinate) from which a series of measurements are taken.

DESKTOP TUTOR:  The input control keypad for the machine.  Keypad overlays are interchangeable according to the type of controller required.

DIRECTORY:  An area of a disk containing the names and locations of the files it currently holds.

DISK:  A computer information storage device, examples, C: (drive) is usually the computers hard (internal) disk and A: (drive) is usually the floppy (portable 3.5" diskette) disk.

DRIVE:  The controller unit for a disk system.

DRY RUN:  An operation used to test how a CNC program will function without driving the machine itself.

DWELL:  A programmed time delay.

EDIT:  The mode used for altering the content of a CNC program via the Desktop Tutor or qwerty keyboard.

END OF BLOCK SIGNAL:  The symbol or indicator ( ; )that defines the end of a block of data.  The pc equivalent of the return key.

G-CODE:  The programming language understood by the machine controller.

FEEDRATE:  The rate, in mm/min or in/min at which the cutting tool is advanced into the workpiece.  For milling and drilling, the feedrate applies to the reference point on the end of the axis of the tool.

FILE:  An arrangement of instructions or information, usually referring to work or control settings.

FORMAT:  The pattern or way that data is organised.

FNC:  FANUC Miller file, extension ".fnc".  Contains G and M codes describing the machine and cutting operations.

G CODE:  A preparatory code function in a CNC program that determines the control mode.

HARDWARE:  Equipment such as the machine tool, the controller, or the computer.

HOME:  Operation to send the axes of the CNC machine to their extreme limits of movement.  Defines the machine datum, also called the home position.

INCREMENTAL:  Incremental programming uses co-ordinate movements that are related from the previous programmed position.  Signs are used to indicate the direction of movement.

INPUT:  The transfer of external information (data) into a control system.

INTERFACE:  The medium through which the control/computer directs the machine tool.

M CODE:  A miscellaneous code function in a CNC program used to indicate an auxiliary function (ie, coolant on, tool change etc.).

MACHINE CODE:  The code obeyed by a computer or microprocessor system with no need for further translation.

MACHINE DATUM:  A fixed zero reference point, used to define the co-ordinate based grid system of the CNC machine..  All machining co-ordinates originate from this point.

MDI:  Manual Data Input is the method used for inserting data into the control system (ie, Desktop Tutor, qwerty keyboard etc.).

MODAL:  Modal codes entered into the controller by a CNC program are retained until changed by a code from the same modal group or cancelled.

NC:  Numerical control.

OFFSET:  Combination of two types of file, the workpiece offset and the tool offset.  Used to describe the workpiece datum, a zero reference used on the CNC machine to ensure machining occurs in the correct place on the billet.  Offsets shift the entire co-ordinate based grid system of the CNC machine.

PART DATUM:  Used as a zero reference point in a CNC file.  All machining co-ordinates originate from this point.

PC:  Personal computer.

PRJ:  Denford CNC Project file, extension ".prj".  Project files contain global information about user defined settings in the VR CNC Turning software, such as toolpost set-up, tooling library, offsets, toolbar and window positions etc.

PROGRAM:  A systematic arrangements of instructions or information to suit a piece of equipment.

SPINDLE SPEED:  The rate of rotation (velocity) of the machine head / cutting tool, measured in RPM.

SOFTWARE:  Programs, tool lists, sequence of  instructions etc.....

TECHNICAL AUTHOR:  The personnel responsible for bringing you this documentation. Click the title for their contact details . . .

TOOL OFFSET:  When machining, allowances must be made for the size of tools being used, since they all differ in length.  The tool offset is the amount the Z value must be moved (or offset), so that all the different cutting tool tips used line up with each other, so they can all be used by one CNC file.

TOOLPOST:  The holder for the various cutting tools.  ATCs (Automatic Tool Changers) are mounted above the spindle centreline, whilst manual toolposts are mounted below it.

TRAVERSE:  Movement of the cutting tool through the 3 machine axes between cutting settings.

TXT:  Standard Windows text only file, extension ".txt".

WORK (WORKPIECE):  The actual material being milled. Quite often, this work is also secured onto a sub-table.  The work is sometimes referred to as the a 'billet'.

WORKPIECE DATUM:  Used as a zero reference point on the real billet.  All machining co-ordinates originate from this point, when offset files are used.

WORD:  A combination of a letter address and digits, used in a CNC program (ie, G42, M04 etc.).

XNC:   Denford Compiled CNC file, extension ".xnc".  A compiled file is a FANUC Miller file that is formatted to allow 3D elements such as the 3D Viewer to run as quickly as possible.  XNC files can also be used to drive an attached CNC machine when run through the VR CNC Turning software.

Z TOOL OFFSET:  See Tool Offset


Homing the Machine
CNC Theory: Homing the CNC Machine

Immediately after being switched on, all three axes of the CNC machine must be homed.

When you home the CNC machine, all both axes will move to the furthest positions available on their slides.

On a back turret / slant bed lathe this will mean the turret will move back (away from you) and to the right.

On a standard front turret machine (eg, Microturn) this will mean movement towards and to the right.

These movements are always positive because all movements into or toward the billet are negative.

Homing the CNC machine defines:

The co-ordinate based system used for plotting any programmed movements - this gives us a working envelope for the cnc machine (explained further in a later section).

The machine datum - the zero reference point for the CNC machine (explained further in a later section).


Machine Datum
CNC Theory: The Machine Datum

The usual symbol for machine datums or points of reference is:

The machine datum, or home position, is the zero reference point of the CNC machine.  It's the point from which all co-ordinates we load or program are calculated.  If there are no offsets loaded and we begin to run a CNC program, the machine datum is the location where any machining will begin.

The position of the machine datum is set by your CNC machine manufacturer and can never be moved, since it defines the physical movement capability of the machine.

If we place a tool in the machine head, then home both axes, we can describe the machine datum as being the edge of the cutting tool tip.  The position of the machine datum, when using machine co-ordinates, will be X=0 and Z=0.


Machine Working Envelope
CNC Theory: The CNC Machine Working Envelope

The diagram below shows the home position of the CNC machine.

The purple shaded block represents the maximum working envelope of the machine, effectively the full length of movement in each of the axes.  In other words, most tool tips can effectively be positioned within this purple block.

Note: As you can see, it may be possible to crash the tool into the chuck so use the VR machine and 2D or 3D simulations first to be sure that your programs will not do anything unexpected !


Miller Tooling DataBase Files
A Turning Tooling DataBase File (.TTD) is a collection of data describing a selection of tool profiles.


Miller Tooling File
A Tooling File Turning (.TFT) is a file which holds the current Tool offsets and which tools are present in the machines turret.


Modal and Non-modal G codes.

Modal (retained) G codes.

A modal G code, once programmed into a block, will affect any subsequent blocks of the program without having to be restated.

Additionally, modal G codes are further split into groups according to their task and function. A modal G code will remain active until another G code from the same group is programmed into a block, or it is cancelled.

For example,

G01 and G00 are modal G codes from group 1:

G01	X _ _ _ _ ;

Y _ _ _ _ ;

X _ _ _ _ ;

G00	Z _ _ _ _ ;

The machine controller has the ability to interpret a maximum of four G codes in one single block of data.  However, these G codes must be from separate modal groups.  When two or more G codes from the same group are specified in the same block, the CNC will only make the last stated G code from that modal group effective.

Non-modal (one-shot) G codes.

A non-modal G code must be programmed into every block when it is required.  It is only effective in the block in which it is specified.


Modify | Add Padding Token
"Modify | Add Padding Token"

Select this option to add a specified number of spaces between program words.

The screen above shows an example CNC file.  If you want to add spaces to only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, as shown above, the edit will be applied to the whole of the CNC file.

In the "Request" window dialogue box enter the number of spaces required between each program word, then click the [OK] button.  In the example above, 4 spaces have been specified.

As shown above, 4 spaces have been placed between each of the program words.


Modify | Alter Feed Rates...Page 1 of 2
"Modify | Alter Feed Rates..." Page 1 of 2

The "Alter Feed Rates..." option allows global changes to be applied across the range of feed rate values in the currently loaded CNC file.  Feed Rate values are denoted using the address letter "F".  This can be achieved by percentage, using the "Alter all feed rates by %" panel (described on this page) or by specified increments, using the "Alter feed rates at Beta" panel (described on the next page).

Editing Feed Rate by Percentage

The screen above shows an example CNC file.  If you want to edit only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, the edit will be applied to the whole of the CNC file.

To change the feedrates shown in the CNC file by percentage, click the circle marker so a bullet is shown next to the "Alter all feed rates by %" panel (the options in the lower panel will become greyed out).  Enter the percentage increase or decrease required.  In the example above, an increase of 150% is specified.  Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each feed rate change.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any feed rates found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted feed rate should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Alter Feed Rates...Page 2 of 2
"Modify | Alter Feed Rates..." Page 2 of 2

Editing Feed Rate by Percentage

The screen above shows an example CNC file.

To change the feedrates shown in the CNC file by specified increments, click the circle marker so a bullet is shown next to the "Alter all feed rates at Beta" panel (the options in the upper panel will become greyed out).

Enter the shift value in the "Shift [+/-]" dialogue box.  Use the up arrow to set feed rate increases or the down arrow to set feed rate decreases.  The values of any identified feed rates will be shifted by the amount of units specified.  In the example above any identified feed rates will shift up by 15 units.

Enter the beta value in the "Beta Value" dialogue box.  This is the marker value from which all feed rates to be changed are identified from.  In the example above a beta value of 100 is specified.

The three lower checkboxes are used to indicate which feed rate values should be changed.  Place a tick mark in each checkbox to apply the indicated option.  When the "Change Values Above Beta" checkbox is selected, any feed rate values above the beta value are marked for change.  When the "Change Values Below Beta" checkbox is selected, any feed rate values below the beta value are marked for change.  When the "Change Values At Beta" checkbox is selected, any feed rate values matching the beta value are marked for change.  In the example above only the "Change Values Below Beta" checkbox is selected.  Since the "Beta Value" is set at 100, this means only feed rates below 100 will be marked for changing.  If changed they will be increased by 15 units (set in the "Shift [+/-]" dialogue box).

Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each feed rate change identified.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any feed rates found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted feed rate should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Alter Speeds...Page 1 of 2
"Modify | Alter Speeds..." Page 1 of 2

The "Alter Speeds..." option allows global changes to be applied across the range of spindle speed values in the currently loaded CNC file.  Spindle speed values are denoted using the address letter "S".  This can be achieved by percentage, using the "Alter all spindle speeds by %" panel (described on this page) or by specified increments, using the "Alter spindle speeds at Beta" panel (described on the next page).

Editing Spindle Speed by Percentage

The screen above shows an example CNC file.  If you want to edit only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, the edit will be applied to the whole of the CNC file.

To change the spindle speeds shown in the CNC file by percentage, click the circle marker so a bullet is shown next to the "Alter all spindle speeds by %" panel (the options in the lower panel will become greyed out).  Enter the percentage increase or decrease required.  In the example above, an increase of 150% is specified.  Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each feed rate change.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any spindle speeds found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted spindle speed should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Alter Speeds...Page 2 of 2
"Modify | Alter Speeds..." Page 2 of 2

Editing Spindle Speed by Percentage

The screen above shows an example CNC file.

To change the spindle speeds shown in the CNC file by specified increments, click the circle marker so a bullet is shown next to the "Alter all spindle speeds at Beta" panel (the options in the upper panel will become greyed out).

Enter the shift value in the "Shift [+/-]" dialogue box.  Use the up arrow to set spindle speed increases or the down arrow to set spindle speed decreases.  The values of any identified spindle speeds will be shifted by the amount of units specified.  In the example above any identified spindle speeds will shift up by 150 units.

Enter a spindle speed value in the "Beta Value" dialogue box.  This is the marker value from which all spindle speeds to be changed are identified from.  In the example above a beta value of 1200 is specified.

The three lower checkboxes are used to indicate which spindle speed values should be changed.  Place a tick mark in each checkbox to apply the indicated option.  When the "Change Values Above Beta" checkbox is selected, any spindle speed values above the beta value are marked for change.  When the "Change Values Below Beta" checkbox is selected, any spindle speed values below the beta value are marked for change.  When the "Change Values At Beta" checkbox is selected, any spindle speed values matching the beta value are marked for change.  In the example above only the "Change Values Above Beta" checkbox is selected.  Since the "Beta Value" is set at 1200, this means only spindle speeds above 1200 will be marked for changing.  If changed they will be increased by 150 units (set in the "Shift [+/-]" dialogue box).

Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each spindle speed change identified.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any spindle speeds found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted spindle speed should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Alter X Values...Page 1 of 2
"Modify | Alter X Values..." Page 1 of 2

The "Alter X Values..." option allows global changes to be applied across the range of X Value co-ordinate values in the currently loaded CNC file.  X Value co-ordinates are denoted using the address letter "X".  This can be achieved by percentage, using the "Alter all X values by %" panel (described on this page) or by specified increments, using the "Alter X values at Beta" panel (described on the next page).

Editing X values by Percentage

The screen above shows an example CNC file.  If you want to edit only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, the edit will be applied to the whole of the CNC file.

To change the X values shown in the CNC file by percentage, click the circle marker so a bullet is shown next to the "Alter all X values by %" panel (the options in the lower panel will become greyed out).  Enter the percentage increase or decrease required.  In the example above, an increase of 150% is specified.  Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each X value change.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any X values found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted X value should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Alter X Values...Page 2 of 2
"Modify | Alter X Values..." Page 2 of 2

Editing X values by Percentage

The screen above shows an example CNC file.

To change the X values shown in the CNC file by specified increments, click the circle marker so a bullet is shown next to the "Alter all X values at Beta" panel (the options in the upper panel will become greyed out).

Enter the shift value in the "Shift [+/-]" dialogue box.  Use the up arrow to set X value increases or the down arrow to set X value decreases.  Any identified X values will be shifted by the amount of units specified.  In the example above any identified values will shift up by 15 units.

Enter an X value in the "Beta Value" dialogue box.  This is the marker value from which all X values to be changed are identified from.  In the example above a beta value of 35 is specified.

The three lower checkboxes are used to indicate which X values should be changed.  Place a tick mark in each checkbox to apply the indicated option.  When the "Change Values Above Beta" checkbox is selected, any X values above the beta value are marked for change.  When the "Change Values Below Beta" checkbox is selected, any X values below the beta value are marked for change.  When the "Change Values At Beta" checkbox is selected, any X values matching the beta value are marked for change.  In the example above only the "Change Values Above Beta" checkbox is selected.  Since the "Beta Value" is set at 35, this means only X values above 35 will be marked for changing.  If changed they will be increased by 15 units (set in the "Shift [+/-]" dialogue box).

Click the "Confirm Changes?" checkbox to show a tick mark - this will effect a confirmation prompt before each X value change identified.

Click the [OK] button to start the search.  The search will proceed from the cursor position downwards in the CNC file.  Any X values found are highlighted, as shown above.

The "Confirm" window will prompt whether the changes to the highlighted X value should be applied, as shown above.

When the operation is complete all changes are indicated by bold coloured text, as shown above.


Modify | Append Line End Token
"Modify | Append Line End Token"

Select this option to add line end formatting to program lines.  The standard format for denoting the end of a program line is the semi-colon character ;

The screen above shows an example CNC file.  If you want to add line end tokens to only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, as shown above, the edit will be applied to the whole of the CNC file.

In the "Request" window dialogue box enter the character/s to be used for denoting the end of program lines, then click the [OK] button.  In the example above, the semi-colon character ; has been specified.

As shown above, end of line characters have been applied to the CNC file.


Modify | Change to LowerCase
"Modify | Change to LowerCase"

Select this option to change any highlighted characters in the "Editor" window to lowercase.  If no characters are highlighted, the option is applied to all characters in the "Editor" window, as shown below.


Modify | Change to UpperCase
"Modify | Change to UpperCase"

Select this option to change any highlighted characters in the "Editor" window to CAPITALS.  If no characters are highlighted, the option is applied to all characters in the "Editor" window, as shown below.


Modify | Line Numbering...
"Modify | Line Numbering..."

Select this option to add or remove program line numbers to or from the beginning of each program line.

The screen above shows an example CNC file without program line numbers.

In the "Line Numbering" window enter the number for first line of the program in the "Start Number" dialogue box.  In the example above, 1 has been specified.

The "Numbering Increment" dialogue box is used to set the numerical gap between each program line number.  In the example above, 10 has been specified, so the program line numbers will follow the sequence 1, 11, 21, 31, 41, 51 etc.

The "Minimum number length" dialogue box is used to set the amount of characters used to display each program line number.  In the example above, 3 has been specified, so the program line numbers will follow the sequence 001, 011, 021, 041, 051 etc.

The "Numbering Token" dialogue box is used to add an address character to start of each program line number.  The standard numbering token used is N.  In the example above, the program line numbers will follow the sequence N 001, N 011, N 021, N 041, N 051 etc.

Click the [OK] button to apply program line numbering settings to the CNC file.

The screen above shows the example CNC file with program line numbers applied.

To remove program line numbers from a CNC file, place a tick mark in the "Remove Numbering" checkbox, then click the [OK] button.


Modify | Remove Line End Token
"Modify | Remove Line End Token"

Select this option to remove line end formatting from program lines.

The screen above shows an example CNC file.  If you want to remove line end tokens from only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, as shown above, the edit will be applied to the whole of the CNC file.

In the "Request" window dialogue box enter the character/s used for denoting the end of program lines, then click the [OK] button to remove them.  In the example above, the semi-colon character ; has been specified.

As shown above, end of line characters have been removed from the CNC file.


Modify | Remove Padding Token
"Modify | Remove Padding Token"

Select this option to remove a specified number of spaces between program words.

The screen above shows an example CNC file.  If you want to remove spaces from only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, as shown above, the edit will be applied to the whole of the CNC file.

In the "Request!" window dialogue box enter the number of spaces to be removed between each program word, then click the [OK] button.  In the example above, 4 spaces have been specified.

As shown above, 4 spaces have been removed between each of the program words.


Preferences | Background Colour...
"Preferences | Background Colour..."

The "Background Colour..." option is used to specify a colour for the background of the "Editor" window.  White is the default background colour.

To select a new colour, click one of the coloured squares in the "Basic colors" area.  To apply this new colour to the background, click the [OK] button.

The [Define Custom Colors] button will display a mixing palette, allowing colours to be mixed visually or specified by their RGB values.  Colours created in the mixing palette are saved in the "Custom colors" area, where they can be applied to the background.

Above: "Editor" window will background colour applied.  The text background colour is white by default.  To change this to the same colour as the "Editor" window background, use "Preferences | Display Options...".  Set the "Text Background" to the same colour used in the "Editor" window background, then select "Preferences | Colour Format Text".


Preferences | Colour Format Text
"Preferences | Colour Format Text"

The "Colour FormatText" option will format the CNC file, allowing groups of program words to be highlighted by colour and/or style, as shown above.  The colour and style of each program word highlighted can be edited using "Preferences | Display Options...".


Preferences | Display Options...
"Preferences | Display Options..."

The "Display Options..." option opens the "Colour Preferences" window.  This window allows colour and style changes to be edited for each program address letter shown in the lefthand panel.  Click on the address letter required, then edit the settings for text and background colour, together with letter style.  Click the [OK] button to close the window.

Use "Preferences | Save Format..." to save the current settings of this option before closing the VR CNC Turning software.

To apply any colour and style changes, use "Preferences | Colour Format Text".


Preferences | Font...
"Preferences | Font..."

The "Font..." option is used to change the name and format of typeface used for the CNC file text in the "Editor" window.  Options are set using the various dropdown boxes, checkboxes and scrolling panels.  Note - the "Sample" panel will show how the typeface will display before being applied.

When the [OK] button is clicked the font and styles selected will be applied to the CNC file, as shown above.


Preferences | Format Using...
"Preferences | Format Using..."

The "Format Using..." option is used to load a collection of option settings for the windows available in the "Preferences" menu.  This allows the "Editor" window to be formatted in varying styles on demand.  Format files are saved using the file extension ".ncf".

Note - when format files are opened you have the option to set them to read only, to prevent further editing.  Place a tick mark in the "Open as read-only" checkbox to apply this option.


Preferences | Save Format...
"Preferences | Save Format..."

The "Save Format" option is used to save the current status of all option settings that appear in the "Preferences" menu.  In addition the status of the following option settings from the Modify menu are also saved: UpperCase/LowerCase setting, Padding Token setting, Line End Token setting and Line Number setting.

This allows the "Editor" window to be formatted in varying styles on demand.  Format files are saved using the file extension ".ncf".


Real CNC Machine Configuration
Software Configuration with a 'real' CNC Machine

Accessing the "Machine Properties Editor" window

Use the "Machine Properties Editor" window to view or configure the software for use with a 'real' CNC machine.  Configuring any values in the "Machine Properties Editor" window will affect the behaviour and operational characteristics of both CNC machines viewed using the Virtual Reality windows an any 'real' CNC machines connected to your computer.

To display the "Machine Properties Editor" window, select the "Setup" menu and click on the "Setup Machine Parameters" option.

On requesting the "Machine Properties Editor" window, a password window will be displayed.  If the password is entered correctly, parameters can be edited as required.  If the password is entered incorrectly, parameters can only be read and not edited.

Important !

The fields in the "Machine Properties Editor" window should only be edited by your CNC machine Technician or Supervisor.  Please refer to the separate parameter helpfile distributed on the VR CNC Turning CD-ROM for further information.  Updated parameter helpfiles can be downloaded from the Denford website:  http://www.denford.com/

Using the "Machine Properties Editor" window

CNC Machine Selection:  The CNC machine for control by the software is highlighted in red, shown as Mirac in the example below.

To select a different CNC machine, click the RIGHT mouse button on the name of the CNC machine required, then highlight and click the "Set As Active Machine" option from the pop-up list.

RS232 Communications:  Select the (RS232) "Communications" option on the selected CNC machine to display the "Communications" dialogue boxes as shown below.

The Baud rate (the speed at which data is sent and received) should be set to 19200.

Enter the serial port number in the "Com Port" dialogue box - this is usually '1' or '2' but on some computers your serial ports may be defined as '3' or '4'.

Stop bits can be 1 or 2. 2 stop bits can sometimes solve problems with on-board serial controllers.

Note that any edited parameter settings are automatically saved to the appropriate CNC machine INI file on the fly.  There is no undo or cancel command available in the "Machine Properties Editor" window.


Real CNC Machine Connections
Hardware Connections with a 'real' CNC Machine

Data is sent and received between your computer and your CNC machine using an RS232 lead.

One end of the RS232 lead fits into the serial (COM) port of the computer running the VR Milling Windows software.  Computer serial ports are the small plugs, each containing two rows of 5 and 4 pins, usually positioned on the back panel of your computer.

The opposite end of the RS232 lead fits into the serial (COM) port on your CNC machine control box.


Real CNC Machine Powerup
Power-up Procedure with a 'real' CNC Machine

Ensure the RS232 lead is fitted securely between the computer and the CNC machine.

Switch on the CNC machine.

Power up the computer and start the VR CNC Turning software.

To start the CNC Machine attached to the computer, click the [Machine] button (shown below) from the "Machine Control" toolbar.


Real CNC Machine Troubleshooting
Troubleshooting with a 'real' CNC Machine

If the software is unable to connect to the CNC machine, a warning window will be displayed, as shown below.

It is also possible that the application will 'freeze' with the hour glass spinning. If this is the case the press [CTRL+ALT+DELETE] and teminate the VR turning task. You can run the software again and re-configure your Com port as detailed below.

Click the [OK] button to clear the window.

Rectify the connection problem before attempting to reconnect.  The most common problems encountered include:

1) The CNC machine was not switched on before a connection was attempted.  The CNC machine must be switched on before clicking the [Machine] button from the "Machine Control" toolbar.

2) The connections at both ends of the RS232 lead between the computer and the CNC machine are insecure.

3) The correct serial port number is not specified in the "Machine Properties Editor" window.  Select the "Setup" menu and click on the "Setup Machine Parameters" option to display the "Machine Properties Editor" window.  A password may be required to access the window.  Select the (RS232) "Communications" option on the selected CNC machine to display the "Communications" dialogue boxes as shown below.

4) If the new Mint file has been automatically download but the machine will not then connect:

Close VR Turning

Switch the machine off at the isolator for around 5 seconds

Switch machine back on and wait at least 10 seconds (The mint file does take some time to run initially)

Now run VR turning again and try to re-connect.

Enter the serial port number in the "Com Port" dialogue box.  Click the [OK] button to confirm any changes.

4) The correct CNC machine type is not specified in the "Machine Properties Editor" window.  Select the "Setup" menu and click on the "Setup Machine Parameters" option to display the "Machine Properties Editor" window.  A password may be required to access the window.  The selected CNC machine is highlighted in red, shown as Mirac in the example below.

To select a different CNC machine, click the right mouse button on the name of the CNC machine required, then highlight and click the "Set As Active Machine" option from the pop-up list.  Click the [OK] button to confirm any changes.

5) The serial ports on the computer or CNC machine control box are faulty.


Save as Bitmap (3D)
"3D Simulation | Capture as Bitmap"

This option allows you to save a windows bitmap file (*.BMP) to disk.

Once this capture window is available, you can reset your 3D view point witihin the 3D simulation window and hit  "re-capture" to capture the image again. So, you can adjust your 3D settings until you get the perfect picture, then save the output as any size bitmap for editing or printing later.

An automatic text box is created at the top left corner of the bitmap, showing the name of the CNC file which was used to create the part.

This window is re-sizeable, so you can exand it to see how good or bad the resolution is. If you require better resolution, increase the bitmap output size under Options in the 3D Simulate menubar and simply "re-capture" the image.

Note: These images can take up a lot of hard disk space. eg:

320 x 240 = 301,000 bytes (0.3 Mb)

640 x 480 = 1,200,000 bytes (1.2 Mb)

800 x 600 = 1,876,000 bytes (1.8Mb)

1024 X 768 = 3,073,000 bytes (3.073 Mb)

Once you are happy with your image, click "Save As" to bring up the save dialog and save your picture as anything you like.


Search | Check Syntax
"Search | Check Syntax"

The "Check Syntax" option is a verification procedure used to find any illegal entries in the code, without having to run the CNC file.

Any lines in the CNC file containing errors are automatically highlighted.  In the example above, program line N660 is highlighted because it contains an error (the Gh5k entry should infact have read G3).  When an error is discovered, establish the nature of the error, then re-edit the code.  Use the G and M code helpfile to find out more about specific G and M code structure and format.  Run the "Check Syntax" option until no further errors are reported.

Note that when there are no errors in the code, the cursor will just return to the start of the CNC file.


Search | Find...
"Search | Find..."

The "Find..." option is used to search through the CNC file for specific characters and words.

Enter the character or words in the "Find what:" dialogue box.  The word G98 has been entered in the example above.  Press the [Find Next] button to begin the search.

Searches are made in directions, either up or down the CNC file text, according to the setting in the "Find" window.  Click in the circle markers to switch the option between "Up" or "Down" - a bullet is used to show which option is selected.  The position of the cursor in the CNC file is always used as the starting position for any searches.

Additionally, the "Match whole word only" and "Match case" options can help to narrow down the search.  Placing a tick mark in the corresponding checkbox will apply each option.  "Match whole word only" searches through the CNC file and reports results when it finds spaces either side of the word entered.  "Match case" searches through the CNC file and reports results when it finds a copy of the word exactly matching the positions of any CAPITALS and lowercase characters entered.

As characters or words are found, they are highlighted in the CNC file text, as shown above.  Keep clicking the [Find Next] button until the search is complete.


Search | Goto Line Number
"Search | Goto Line Number"

The "Goto Line Number" option is used to move to a specific line of the CNC file. Note - this is the text line number in the editor and NOT the program line number (address N).

If the CNC file uses program line numbers use Search | Find... to move to a known area of code.

Enter the text line number required by clicking the up and down arrow buttons.  Press the [OK] button to search for the text line number requested.

The text line number requested will be highlighted in the CNC file, as shown above.


Setup Graphics...
"2D Simulation | Options..."

This option is used to display the "2D Simulation Setup" window, shown above, used to configure the graphics shown in the "2D Simulation" window.

Checkboxes are used to show when the various options in this window are active.  When a tick mark is visible, the associated option is active.  To add or remove a tick mark in a checkbox, click the left mouse button on the required checkbox.

The top section allows you to configure the tool path colors and whether or not they are shown. To change color just click on the colored box associated with the movement type. eg, If you wished to show circular motion as blue, in the example above you would click the orange box next to Circular Movement Colour and choose blue from the colour picker window.

The bottom section allows configuration of the window and billet color. Again if you wished to make the 2D window background color black, you would click on the color box next to Background Colour and select black from the colour picker. (you get the idea).

Click the [OK] button to save any changes or the [Cancel] button to discard any changes made to the options in the "2D Simulation Setup" window.


Setup Machine Parameters...
"Setup | Setup Machine Parameters..."

The "Machine Properties Editor" window allows the comprehensive range of settings for each CNC machine to be viewed or edited.  Configuring any values in the "Machine Properties Editor" window will affect the behaviour and operational characteristics of both CNC machines viewed using the Virtual Reality windows an any real CNC machines connected to your computer.

Important !

The fields in this option should only be edited by your CNC machine Technician or Supervisor.  Please refer to the separate parameter helpfile distributed on the VR CNC Turning CD-ROM for further information.  Updated parameter helpfiles can be downloaded from the Denford website:  http://www.denford.com/

Password Features

On requesting the "Machine Properties Editor" window, a "Password" window will be displayed, as shown above.  Enter the password in the dialogue box, then click the [OK] button to open the "Machine Properties Editor" window.  The default password supplied is denny.

If the password is entered correctly, parameters can be edited as required.

If the password is entered incorrectly, parameters can only be read and not edited.

To change the password, click the [Change Password] button in the bottom righthand corner of the "Machine Properties Editor" window.  The "Change Password" window will be displayed, as shown above.  Enter the old password in the top dialogue box.  Enter the new password in the middle and bottom dialogue boxes.  Click the [OK] button to change the password.

General Layout

The lefthand panel displays the list of available CNC machines and their parameters.  On first opening the "Machine Properties Editor" window, the active machine (shown by the red tick) is always displayed with its parameters directory expanded.  This is shown as the Mirac in the example screenshot above.

The righthand panel displays the options and dialogue boxes associated with the highlighted parameter, chosen from the list of parameters in the lefthand panel.  The "Machine Capability" section is displayed in the example screenshot above.

Expanding and Collapsing the Lists

Click on the [+] squares to expand a list or the [-] squares to collapse an open list, displayed in the lefthand panel of the "Machine Properties Editor" window.  To highlight a CNC machine or parameter, click on its title - the options associated with the highlighted CNC machine or parameter will be displayed in the righthand panel of the "Machine Properties Editor" window.

Updates

Updated parameter setting lists and editing helpfiles can be downloaded from the Denford website:  http://www.denford.com/


Software in Use
VR CNC Turning for Windows in Use

The diagram below shows how all the different elements of the software work together, from CNC file source through to a software or hardware outcome.


Standard Menus


Stuff about the Authors
Contact the Personnel responsible for this documentation

Feedback is always welcome. Comments regarding this helpfile should be addressed to the following personnel:

USA and Canada only:

Coree Kilo-Price - Tecnical Editor for Denford Inc. - USA (email: ckilo@denford.com)

UK and the rest of the world:

Andrew Teal - Systems Engineer for Denford Limited - UK (email: ateal@denford.co.uk)

Matthew Clayton - Technical author for Denford Limited - UK (email: mclayton@denford.co.uk)


Technical Support

Denford Limited provides unlimited Technical Support on this software.

Technical Support is only available to registered users. If your software was not registered with Denford Limited at the point of sale, e-mail or fax your registration details to Denford Limited, or your authorised Denford shipping agent as soon as possible.

When you request Technical Support, please be at your computer, with your computer and software documentation to hand. To minimise delay, please be prepared to provide the following information:

- Dongle Serial Number.

- Registered user's name / company name.

- Software name and version number (found in the "Help | About" menu).

- The wording of any error messages that appear on your computer screen.

- A list of the steps that were taken to lead up to the problem.

UK Contact Details:

Denford Limited,

Birds Royd, Brighouse, West Yorkshire, HD6 1NB, UK.

Telephone: 01484 712264

Fax: 01484 722160

ISDN: 01484401157:01484401161

E-mail: mailto:service@denford.co.uk

Technical Support: Monday to Friday 8.30am - 4.30pm GMT

http://www.denford.co.uk

For USA please contact:

Denford Inc.

815 West Liberty Street, Medina, Ohio 44256, USA.

Telephone: 330 7253497

Fax: 330 7253297

E-mail: mailto:service@denford.com

Technical Support: Monday to Friday 8.30am - 4.30pm Eastern

http://www.denford.com


The 2D Simulation Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Note:  This menu is only available when the "2D Simulation" window is active.

Options:  Select this option to display the "2D Simulation Setup" window, used to configure the graphics shown in the "2D Simulation" window such as billet color, tool path color.

Click here for more about "Options..."

Auto Save Bitmap?:  Select this option to automatically save the contents of the "2D Simulation" window, as a bitmap image, after the CNC file has been fully executed.  The 2D bitmap image will be saved using the same filename and location as the CNC file but with the file extension ".BM2".  A tick mark will be displayed when the option is active.

Use Offsets:  Select this option to choose between executing the CNC file using either any programmed X and Y offsets or no offsets whatsoever.  A tick mark will be displayed when any programmed X and Y offsets will be used.

Click here for more about "Use X,Y Offsets"

Related Topics:

The Outputs Toolbar

The 2D Simulation Window


The 2D Simulation Window Page 1 of 3

To display the "2D Simulation" window, click the [2D Simulation] button (shown below) from the "Outputs" toolbar.

General Layout

The "2D Simulation" window displays the output from the CNC file on a plan view of the billet.

Displaying the "2D Simulation" window using the X,Z Offsets

To display the "2D Simulation" window using the current X,Z Offsets, select the "Use Offsets" option on the "2D Simulation" menu, so a tick mark is shown next to the title.

The status bar at the top of this window displays and updates X and Z co-ordinates.

In the example shown below, the simulation offset being used is denoted by the black datum crosshairs, in the centre and on the right of the billet image.

To set the position of the datum, either enter offsets into the X Z edit boxes, or click on the black datum symbol and move it to the position you require.

Displaying the "2D Simulation" window without using the X,Y Offsets

To display the "2D Simulation" window without using any X,Z Offsets, select the "Use Offsets" option on the "2D Simulation" menu, so a tick mark is not shown next to the title.

The X and Z datum is always the default position of X on centre Z on the right hand face of the billet.


The 2D Simulation Window Page 2 of 3

The "2D Simulation" measuring cursor

To display the "2D Simulation" measuring cursor, click the LEFT mouse button in the crosshair icon (highlighted in red below). Now, wherever you move your mouse cursor - you get a constant position update shown in the yellow box. (X 18.704 Z-24.630 in the screenshot)

Zoom In:  Click this option to increase the size of the 2D simulation image.

Zoom Out:  Select this option to reduce the size of the 2D simulation image.


The 2D Simulation Window Page 3 of 3

Activating SourceTrack technology

This unique feature allows you to 'back track' into your program from any move made in the 2D simulation window:

To do this, simply move your mouse around the linears and arcs shown in the 2D window. When you are near the end or beginning point of these lines, the line will highlight and go thicker. In the screen shot below, the mouse pointer is highlighted in red and you can see that the arc move has been highlighted in purple and by going thicker.

Click the LEFT mouse button over the selected element and the SourceTrack info box will appear. This shows more data than you really need to know, but can be a great way to debug CNC programs - especially complex ones.

Clicking the [Edit Source] button will highlight the line of the CNC file in which the element appears.

Note:  The "Line Number" refers to the text line number in the "Editor" window and not the program line number.(N address).

Using SourceTrack in reverse

This method of finding out what part of your program was used to create a 2D element can also be used the other way round - you can select any line in your CNC program editor, and tell it to show you which element was created in the 2D simulation window.

Simply right click on the line in the editor and select "Show 2D draw element "

In this screenshot the line shown by the red arrow has been highlighted as the move created by " G00 X25 Z2 "


The 3D Simulation Window Page 1 of 3

To display the "3D Simulation" window, click the [3D Simulation] button (shown below) from the "Outputs" toolbar.

General Layout

The "3D Simulation" window displays the output from the CNC file on a 3 dimensional view of the billet.:

Zooming and panning around the 3D window

The mouse is the only way to alter the viewpoint of the billet - as follows:

Zoom In: Hold down the RIGHT mouse button and move mouse upwards

Zoom Out: Hold down the RIGHT mouse button and move mouse downwards

Pan Left: Hold down the RIGHT mouse button and move mouse to the left

Pan Right: Hold down the RIGHT mouse button and move mouse to the right

Rotate around the X axis: Hold down the LEFT mouse button and move mouse to the left or right

Rotate around the Z axis: Hold down the LEFT mouse button and move mouse up or down

Raise Viewpoint : Hold down the MIDDLE mouse button and move mouse down

Lower Viewpoint : Hold down the MIDDLE mouse button and move mouse up

(if you do not have a MIDDLE mouse button, then hold down [Shift] on the keyboard and use the RIGHT mouse button)

Displaying the "3D Simulation" window using the X,Y Offsets

Click here for more about "Running a 3D simulation with offsets"

Displaying the "3D Simulation" window without using the X,Y Offsets

To display the "3D Simulation" window without using any X,Y Offsets, select the "Use X,Y Offsets" option on the  "3D Simulation" menu, so a tick mark is not shown next to the title.


The 3D Simulation Window Page 2 of 3

Slicing the billet to view internal cuts

In order to easily view interal cuts on the lathe, the 3D billet can be 'cut' or 'sliced' to let you see inside as shown below:

To alter the cutting angle, select the "Angle" button, then hold down the RIGHT mouse button and move the mouse UP or DOWN to change the angle:

Note: if the "Angle" button is pressed, you will still be able to Zoom and Pan the billet, but not rotate. Simply press the button again to turn angle selection off.


The 3D Simulation Window Page 3 of 3

Measuring your finished Part

Once you have run a CNC program through, and the 3D billet model has been created, it is possible to measure diameters, lengths and angles of your part.

In this screenshot, the "Measure" button is pressed and an information box appears to its' right.

The Button has also been un-docked so that it can be positioned in a more suitable place.

Measuring probes also appear on the model, indicating which point on the surface you are 'measuring'.

Information box details

X: The current diameter as determined by the point of the measuring probes.

Z: The current Z dimension in relation to the front datum point.

L: The length of the item that is highlighted in a paler colour.

A: The angle of the item that is highlighted in a paler colour.

In the above example you can see that the probes are measuring the end diameter of the long tapered cut. Its diameter is 24mm; it ends 46.5mm from the front face of the billet (ie, Z datum point); the length of the taper (as highlighted) is 18.111mm and the angle of the taper is 6.34 degrees. (Where 0 degrees is parallel to the Z axis)

Moving the probes to a different part of the model

Press and hold the LEFT mouse button and move the mouse left or right.

Note: if the "Measure" button is pressed, you will still be able to Zoom and Pan the billet, but not rotate. Simply press the button again to turn Measure feature off.


The 3D Viewer Menu

Click the menu title to display the dropdown list. Click the highlighted option to select it.

Note:  This menu is only available when the "3D Simulation" window is active.

Options: Brings up the 3D simulation setup window - allows the configuration of 3D billet color / materials, toolpath colors, Bitmap output size and general color customisation

Show Original Size: Resets the zoom and pan position to their defaults. (Does not reset the billets current shape)

Capture as Bitmap:  Select this option to allow a windows type .BMP file to be created. You are given a preview of the output before saving so you can re-adjust the 3D viewpoint. The size, in pixels, of this bitmap can be configured under Options.

Click here for more about "Capture as Bitmap"

Auto Save Bitmap?:  Select this option to automatically save the contents of the "3D Simulation" window, as a bitmap image, after the CNC file has been fully executed.  The 3D bitmap image will be saved using the same filename and location as the CNC file but with the file extension ".bm3".  A tick mark will be displayed when the option is active. The size in pixels of this bitmap can be configured under Options.

Use Offsets:  Select this option to choose between executing the CNC file using either any programmed X and Z offsets or no offsets whatsoever.  A tick mark will be displayed when any programmed X and Z offsets will be used and the X Z offset edit boxes will appear/disappear from the 3D Simulation window.

Click here for more about "Running a 3D simulation with offsets"

Related Topics:

The Outputs Toolbar

The 3D Simulation Window


The Denford Virtual Reality Window Page 1 of 3

Part 1: Starting the Virtual reality CNC Machine

Before starting the Virtual reality CNC Machine:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

To start the Virtual Reality CNC Machine, click the [VR Machine] button, shown above, from the "Options" toolbar.

The "Denford Virtual Reality" window will open.  This window is used for viewing the 3D model of the VR CNC machine.  Any tools present in the "Machine Tooling" window (the Turret) will also be loaded, when applicable.

The "Control Panel" window will also open.  This window is used for controlling the movements of the VR CNC machine.

General Layout

The "Denford Virtual Reality" window is used to display a three dimensional representation of the CNC machine.  This VR CNC machine is driven and responds in exactly the same way as its real-life counterpart, making the VR Machine Mode ideal for offline CNC training.  In the example below, a Denford Triac VMC CNC Milling Machine is being controlled through virtual reality.

The "Denford Virtual Reality" window, shown above, is split into three basic areas:

The Viewbar (circled red) is the area of the window where preset viewpoints can be applied and the virtual reality world configured.

The Main Viewing Area, the largest area of the window, is where the objects and devices in the virtual worlds can be seen.

The Movebar (circled yellow) is the area of the window containing the controls for moving around the virtual world.

Related Topics:

The Machine Control Toolbar


The Denford Virtual Reality Window Page 2 of 3

The Viewbar

The viewbar is the area of the window where any of the preset viewpoints can be applied and the virtual reality world configured.

There are usually 6 available viewpoints:

Button [1]:  Looking at full machine.

Button [2]:  Looking at guard remove switch. (Some VR machines have a magic switch which will make the enclosure guarding disappear so you get a clear view of the insides of the machine).

Button [3]:  Looking at chuck and billet.

Button [4]:  Close up of turret.

Button [5]:  Close up of job.

Button [6]:  Overall view of machine.

Viewpoints are particularly useful for navigating quickly, or regaining position when lost in the virtual world.  To select a viewpoint, click on the number button of the viewpoint required.  Hovering the mouse cursor over a viewpoint number button will display a pop-up description of the assigned view, as shown above.

Virtual Reality World Configuration

Clicking the [Setup] button will display the virtual reality configuration menu, shown above.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Select Device:  Select this option to display the "3D Control Setup" window, used for enabling and disabling devices (such as mouse control or sound effects) and configuring the viewing screen display options.  For more detailed help using this window, press the [?] button on the "3D Control Setup" window titlebar or press the [F1] key to display context sensitive help.

Setup Proportional Device:  Select this option to display the "Proportional Control Setup" window, used for configuring multiaxis movement devices such as a Spacemouse or joystick.  For more detailed help using this window, press the [?] button on the "3D Control Setup" window titlebar or press the [F1] key to display context sensitive help.

Reset Proportional Device:  Changes all variables associated with the selected proportional device back to their default values.

Related Topics:

The Machine Control Toolbar


The Denford Virtual Reality Window Page 3 of 3

Part 3: Moving around the Virtual Reality World

The movebar tools allow you to freely 'fly' around the virtual world, using your mouse.  Try to think of the display in the Main Viewing Area as being the view from a floating camera head, which you can control using the three movement icons.  Each icon is used to control a different type of movement in the virtual world.

Using the Movebar to move around the Virtual Reality world

You can change the position of your viewpoint using the icons in the Movebar.

  :  Moves the viewpoint in the vertical plane.

  :  Moves the viewpoint in the horizontal plane, forwards, backwards and turning.

  :  Tilts the viewpoint up and down.

Click and hold the left mouse button on one of the three movement icons, then drag the mouse.  As you drag the mouse the icon indicates the direction you are moving, and the viewpoint moves in the corresponding direction.  The further you move the cursor from the icon, the faster you will move.  Release the mouse button to stop the movement.

Interactive Objects

Some objects on the VR CNC machines are interactive:

Right click on the guard handle to open the machine guard.

Left or right click on the Chuck to open/close the jaws.

Related Topics:

The Machine Control Toolbar


The Edit Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

The following options are used when editing text characters in the "Editor" window.

Undo:  Select this option to undo the last command performed in the "Editor" window.

Redo:  Select this option to repeat the last command performed in the "Editor" window.

Cut:  Select this option to cut any highlighted text from the "Editor" window to the Windows clipboard.  To select areas of text in the "Editor" window, click and drag over the required characters to highlight them.  Computer keyboard shortcut: [CTRL + X]

Copy:  Select this option to place any text held in the Windows clipboard to the current "Editor" window cursor position.  To select areas of text in the "Editor" window, click and drag over the required characters to highlight them.  Computer keyboard shortcut: [CTRL + C]

Paste:  Select this option to place any text held in the Windows clipboard to the current "Editor" window cursor position.  Computer keyboard shortcut: [CTRL + P]

Select All:  Select this option to highlight all the text in the "Editor" window.

Related Topics:

The Editor Window


The Editor Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options and display any secondary menus.  Click the highlighted option to select it.

Hi-Light:  Select this option to display a secondary menu that allows certain address characters in your CNC file to be hi-lighted.  Note - only one address character can be hi-lighted at any one time.

Click here for more about "Hi-Light".

G:  G code - Preparatory function.

M:  M code - Miscellaneous function.

T:  Tooling management.

F:  Feed rates.

S:  Spindle speeds.

X:  Absolute/incremental distance travelled by the slide tool in the X axis direction.

Y:  Absolute/incremental distance travelled by the slide tool in the Y axis direction.

Z:  Absolute/incremental distance travelled by the slide tool in the Z axis direction.

I:  Distance command (used in conjunction with J) to identify arc centre co-ordinates.

J:  Distance command (used in conjunction with I) to identify arc centre co-ordinates.

Show Normal:  Select this option to remove any hi-lights applied to your CNC file.

Edit: This brings up the usual editing functions like cut, copy and pasting of text.

Preferences: Allows the editor window to be configured to your favourite fonts and colors.

Modify: Allows you to modify certain values (eg, all feedrates increase by 50%), add line numbering etc . .

Search: Allows the CNC program to be searched via text match or to a specific line number, also gives the option of syntax checking a program.

Printer Setup...:  Select this option to configure the type of printer you wish to use for printing out any CNC files.

Print...:  Select this option to print the contents of the "Editor!" window.

Related Topics:

The Editor Window


The Editor Window Page 1 of 3

General Layout

The "Editor" window is used for viewing and editing the text content of the CNC file.  The Editor is also the main window used when CNC files are entered in MDI (Manual Data Input) mode.

The titlebar of the "Editor" window displays the name and location of the currently loaded CNC file, circled yellow in the example above.

The editor text display panel shows the content of the CNC file,listed line by line from the top to bottom.

The statusbar of the "Editor" window displays the editor panel line and column numbers relating to the position of the cursor.  In the example above, the cursor (highlighted green) is at column position 9, on text line 6 (circled red).

Note:  Do not confuse the editor text line number with the CNC file (N address) number.


The Editor Window Page 2 of 3

Editing text in the CNC File

Sections of the CNC file can be changed by using the "Editor " window as a simple word processor.

Positioning the "Editor" window cursor

The "Editor" window cursor is a flashing vertical black line, shown circled red in the above screenshot.  This cursor shows where characters can currently be inserted, removed or highlighted.  To remove characters directly behind the "Editor" window cursor, press the [Delete] key.  To create a new CNC file line, press the [Enter/Return] key.

The mouse positioning cursor is a vertical black line with bars at its top and bottom, shown circled yellow in the above screenshot.  This cursor is used to move the "Editor" window cursor to new positions in the CNC file.

To reposition the cursor in the "Editor" window:

Position the mouse positioning cursor in the required area, then click the left mouse button to move.

Use the four computer [Cursor] arrow keys to move the "Editor" window cursor to the required position.

Use the [Page Up] key to move to the top of the CNC file.

Use the [Page Down] key to move to the bottom of the CNC file.

Use the [Home] key to move to the beginning of the current CNC file line.

Use the [End] key to move to the end of the current CNC file line.

Selecting and editing areas of text

To select areas of text in the "Editor" window, position the "Editor" window cursor (the vertical black line) at the start or end of the text required, then click and hold down the left mouse button.  Drag over the required characters to highlight them, as shown above.  To select all the text in the "Editor" window use the "Select All" option from the "Edit" menu.

The highlighted characters can be edited using the following commands:

Select the "Cut" option from the "Edit" menu to cut any highlighted text from the "Editor" window to the Windows clipboard.  Computer keyboard shortcut: [CTRL + X]

Select the "Copy" option from the "Edit" menu to copy any highlighted text from the "Editor" window to the Windows clipboard.  Computer keyboard shortcut: [CTRL + C]

Select the "Paste" option from the "Edit" menu to place any text held in the Windows clipboard to the current "Editor" window cursor position.  Computer keyboard shortcut: [CTRL + P]

Select the "Undo" option from the "Edit" menu to undo the last command performed in the "Editor" window.

Select the "Redo" option from the "Edit" menu to repeat the last command performed in the "Editor" window.

Related Topics:

The Editor Menu (colour hilighting areas of text)

The Edit Menu (manipulation of text)


The Editor Window Page 3 of 3

Formatting editor text between CAPITALS and lowercase

Select the "Change to UpperCase" option from the "Modify" menu to change any highlighted characters in the "Editor" window to CAPITALS, as shown above left.

Select the "Change to LowerCase" option from the "Modify" menu to change any highlighted characters in the "Editor" window to lowercase, as shown above right.

Adding spaces between CNC program words

Select the "Add Padding Token" option from the "Modify" menu to add a specified number of spaces between program words.  In the example above, the left screen shows no additional padding, whilst the right screenshot shows a padding of 3 spaces.

Select the "Remove Padding Token" option from the "Modify" menu to remove a specified number of spaces between program words.

Adding Line End Formatting

Select the "Append Line End Token" option from the "Modify" menu to add line end formatting to program lines.  In the example above, the left screen shows no line end formatting, whilst the right screenshot uses the ; character as the line end token.

Select the "Remove Line End Token" option from the "Modify" menu to remove line end formatting from program lines.

Adding Line Numbers to CNC program lines

Select the "Line Numbering..." option from the "Modify" menu to add or remove program line numbers to or from the beginning of each program line.  In the example above, the left screen shows no program line numbering, whilst the right screenshot shows program numbers signified by the N address letter.

Related Topics:

The Modify Menu


The File Control Toolbar

File Control buttons, listed from left to right:

[Play]:  Click this button to start running the CNC file currently loaded in the "Editor" window.  If no output option for the CNC file is selected you will be prompted to select one before the CNC file is executed.  The CNC file will start playing from the cursor position in the "Editor" window.

[Pause]:  Click this button to pause the playing of a CNC file.  To restart the CNC file from the paused line,click the [Play] button again.

[Stop]:  Click this button to stop the playing of a CNC file.

[Rewind to Start]:  Click this button to move the cursor position in the "Editor" window back to the start of the CNC file.

Note: Buttons are greyed out when unavailable.


The File Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options and display any secondary menus.  Click the highlighted option to select it.

New:  Select this option to create a New File in the "Editor" window.

Open:  Select this option to open a file.  Files that can be opened include FANUC Lathe files (.fnl), Denford Compiled CNC files (.xnc).

ReOpen:  Select this option to display a secondary menu of recently opened files.  Highlight and click on the chosen file to load it into the software.

Save:  Select this option to save any changes made to a previously saved file.

Save As:  Select this option to save a file in a specific directory and folder with a user defined filename.  Files can be saved as either a FANUC lathe file (.fnl), Text Only file (.txt) or Any file of your choice.

Save Project:  Select this option to save a Turning Project File (.prj).

Source:  Select this option to display a secondary menu allowing configuration of the CNC file display.

File:  Select this option to display the CNC file in the "File Input" window.  The CNC File is displayed a single line at a time.  When the CNC File is run, the window will update, showing the appropriate program line being executed.  Using the "File Input" window will not allow any editing of the code.

Editor:  Select this option to display the CNC file in the "Editor" window.  The CNC file is displayed in full.  Lines of code can be manually edited, through using the window in the same way as a word processor.

Compiled:  Select this option to display the CNC file in the "Compiled Input" window.  The CNC file is compiled into a format that allows faster processing of any 3D elements used in the VR CNC Turning software.

Exit:  Click this option to close down the VR CNC Turning software.


The Help Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Contents:  Select this option to display the contents page for VR CNC Turning for Windows software helpfile.  This helpfile contains VR CNC Turning tutorials, detailed information about the various features of the VR CNC Turning software, troubleshooting guides and a guide to CNC Theory.

Context sensitive help is also available:

Menu:  To obtain context sensitive help on a software menu, click the menu title to display its dropdown list of options, then press the [F1] key.

Click here for more about Context Sensitive Menu Help

Window:  To obtain context sensitive help on a software window, press the [F1] key when the required window is active.

Click here for more about Context Sensitive Window Help

CNC Programming:  Select this option to display the contents page for the CNC Milling Programming helpfile.  This helpfile contains detailed information about individual G and M codes and structure of CNC files.

Context sensitive help is also available:

G and M codes:  To obtain context sensitive help on an individual G or M code, position the "Editor" window cursor in the middle of the text for the code required, then press the [Ctrl + F1] keys.

Click here for more about Context Sensitive G and M code Help

About...:  Select this option to display information about the VR CNC Turning software, including the version number.


The Machine Control Toolbar

Machine Control buttons, listed from left to right:

[VR Machine]:  Click this button to begin controlling a CNC machine in a Denford Virtual Reality world.

[Machine]:  Click this button to begin controlling a real CNC machine connected to the computer.


The Machine Mode Window Page 1 of 6
The Machine Mode Window (Control Panel) Page 1 of 6

Tip: Press [CTRL+D] for real machine debug I/O window.

General Layout

The "Machine Mode" window is displayed when either the VR Machines or 'real' CNC Machines are active.

To start the VR Machine, click the [VR Machine] button (shown below) from the "Machine Control" toolbar.

To start a 'real' CNC Machine attached to the computer, click the [Machine] button (shown below) from the "Machine Control" toolbar.

The "Machine Mode" window is used for controlling the movements of both the Virtual Reality machine and any 'real' CNC machine attached to the computer.

The "Machine Mode" window contains four tabs, shown highlighted by the yellow box in the above screenshot:

Mdi: Manual Data Input mode. Lets you type small CNC programs that you can run as if you were in automatic single step.

Jog:  Jog Mode, used for manually moving the machine within its co-ordinate envelope.

Home:  Home Mode, used for configuring the machine, before it can be fully used.  This finds the Machine Datum and limits of co-ordinate movement.

Auto:  Auto Mode, used for controlling the machine with a CNC file.

Note:  The "MDI", "Jog" and "Auto" tabs will not be displayed until the machine has been configured by homing both axes.

The statusbar, highlighted by the red box in the above screenshot, is positioned at the bottom of the "Position Display" window.  It displays the following information, listed from top to bottom:

The last programmed Feedrate setting:  Denoted by "Feed:" and a numerical value.  When the [Units] of Measurement are set to "Inch" the feedrate is measured using inches per minute.  When the [Units] of Measurement are set to "Metric" the feedrate is measured using millimetres per minute. If feedrate mode is per revolution, then the description changes accordingly.eg, 'Feed: 0.05mm/rev'.

The last programmed Spindle Speed setting:  Denoted by "Speed:" and a numerical value.  The spindle speed is measured using revolutions per minute or Metres per minute for Constant Surface Speed (feet per minute if units are Imperial).

The last programmed Tool Change:  Denoted by "Tool:" and the number of the tool.

The last programmed Tool Offset:  Denoted by "Offset:" and the number of the tool.

Note: The initial tool offset value is "None". Be sure to activate any offset required - before setting up your workpiece offsets.


The Machine Mode Window Page 2 of 6
The Machine Mode Window (Control Panel) Page 2 of 6

Home Mode

Note:  The numerical figures depicted on screenshots will differ according to the CNC machine and offsets being used on your computer system.

The "Home" tab is used for configuring the machine before it can be fully used.  This defines the Machine Datum, used as a zero reference for describing all co-ordinate positions and defines the limits of co-ordinate movement for the machine.

Click here for more about the Theory behind Homing the Machine and the Machine Datum

Note:  The "Jog" and "Auto" tabs will not be displayed until the machine has been configured by homing all of the three axes.

To configure the machine X axis only, click the [X Axis ONLY] button.  The X machine slide will move until it has found its limits of co-ordinate movement.

To configure the machine Z axis only, click the [Z Axis ONLY] button.  The Z machine slide will move until it has found its limits of co-ordinate movement.

To configure both axes together, click the [All Axes] button.  All machine slides will move until the limits of co-ordinate movement have been found.

Co-ordinate System Display Mode

The [Co ordinates] button is used to switch between the two systems used for displaying the co-ordinate positions.  The far right panel on the statusbar, at the bottom of the "Machine Mode" window, displays the current setting for this button.  When the [Units] of Measurement are set to "Inch" the co-ordinates are displayed using inches.  When the [Units] of Measurement are set to "Metric" the co-ordinates are displayed using millimetres.

Click here for more about the Theory behind Co-ordinate System Display Modes

Work Piece Co-ordinates System :  This system displays the co-ordinate position relative to the moveable workpiece datum.  When the Co-ordinate System Display Mode is set to Work Piece or Program display, the button graphic shows the X,Z symbol with a picture of the work piece (billet). The display panel shows the text "Program".

Machine Co-ordinates System:  This system displays the co-ordinate position relative to the fixed machine datum.  When the Co-ordinate System Display Mode is set to Machine, the button graphic shows the X, Z symbol with a picture of the chuck and turning tool.  The display panel shows the text "Machine".

Both Co-ordinates System:  This system displays both Machine values and Program as above. There is also a display of the 'distance to go' for each axis. When running a CNC program in automatic, this display shows how far the current move has got to go until it is complete.  The programmed and actual spindle speed is also shown. (Actual being the accurate chuck speed read from the machines encoder)


The Machine Mode Window Page 3 of 6
The Machine Mode Window  (Control Panel) Page 3 of 6

Jog Mode

The "Jog" tab is used for manually moving the machine within its co-ordinate envelope.

The "Jog" tab is used for manually moving the machine within its co-ordinate working envelope.

Jog Control Modes

The "Jog" panel displays the 2 rotary controls for changing feed and speed values.

The axes can be jogged, or moved, using two different methods, outlined below - Continuous or Step.

To change the jog control value, click and hold down the left mouse button on the rotary knob, then drag the knob around in a circular motion to the new position.

When the [Units] of Measurement are set to "Inch" the rate of movement is measured using inches per minute.  When the [Units] of Measurement are set to "Metric" the rate of movement is measured using millimetres per minute.

Jog Continuous:  In jog continuous mode, the selected machine axis will move at the indicated speed when one of the machine axis movement keys are pressed and held down.  The selected machine axis will continue to move until the key is released.  The slider bar can be moved to set jog speeds between 0 and 1000 units.  When Jog Continuous is active, the [Jog] button graphic will be displayed as shown below. (Indicating the current jog speed as 1050mm per minute)

Jog Step:  In jog step mode, the selected machine axis will move one indicated increment, each time the selected axis movement key is pressed.  The slider bar can be moved to set jog increments of 0.01, 0.05, 0.1, 0.5, 1, 2 and 5 mm.  When Jog Step is active, the [Jog] button graphic will be displayed as shown below. (Currently set to 0.5mm step value). Feedrate for the step movement will be at whatever feedrate was last selected.

Jog Control Keys

The Keys used for Jogging can be configured for each different machine, but are usually set to the CURSOR arrow keys where arrow left would be Z minus, arrow right Z plus, arrow up X plus etc ...

Losing Jog Mode

For safety reasons, the software has been written so the using the cursor keys on the keyboard will not accidentally Jog the real machine. So, if another window such as the Editor is selected, then Jog mode is disabled even though you are still technically in Jog mode. The green background on the Jog tab indicates whether you are in Jog mode or not:

 means Jog mode active

 means Jog mode inactive

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


The Machine Mode Window Page 4 of 6
The Machine Mode Window (Control Panel) Page 4 of 6

Jog Mode cont'd.

Spindle Speed Control

The "Spindle" panel displays the [Spindle] button, a vertical slider bar and the numerical spindle speed value.  To change the spindle speed value, click and hold down the left mouse button on the slider bar, then drag the slider bar up or down to the new position.  The spindle speed setting is also displayed in the "Machine Mode" window statusbar, using the "S" address letter.  The spindle speed is measured using revolutions per minute.

To start the spindle manually, click the [M Codes] button, then highlight and click the "M3 Spindle Forward" option.

When the spindle is running, it can be switched off by clicking the [X] button, shown below, or by clicking the [M Codes] button, then highlighting and clicking the "M5 Spindle Stop" option.

Alter the speed by typing the exact speed into the box, or rotate the speed control knob with your mouse.

M Codes

Click the [M Codes] button to display the list of M codes, shown below.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.  For detailed information regarding M code Programming, click "Help | CNC Programming" to display the "Denford CNC Programming for Milling Machines" helpfile.

Coolant Control

Click the [Coolant] button to manually switch the coolant pump (when fitted to the machine) on and off.

Coolant Off:  When the coolant pump is not running, the graphic below is displayed on the button:

Coolant On:  When the coolant pump is running, the graphic below is displayed on the button:


The Machine Mode Window Page 5 of 6
The Machine Mode Window (Control Panel) Page 5 of 6

Auto Mode

Adjusting the feedrate or spindle speed can be done by moving the Potentiometers (where fitted) on a real machine, or by click the large up/down buttons as shown above.

Feed override is available from 0 to 150%

Speed override is available from 50 to 120%

The "Auto" tab is used for controlling the VR CNC machine when running a CNC file.

To start the CNC file, ensure the "Editor" window cursor is positioned at the start of the CNC file.  Click the triangular [Play] button from the "File Control" toolbar, shown above.

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


The Machine Mode Window Page 6 of 6
The Machine Mode Window (Control Panel) Page 6 of 6

MDI Mode

The MDI mode lets you enter small CNC programs and run them one block at a time.

Select MDI, type your commands into the white box as shown above.

Use the standard file controls to start and stop your program. Each line will be executed one at a time, so you will need to press START (Highligthed in red) each time the previous block completes.

Pressing reset/rewind will clear the MDI window of all your commands.

The example above, would firstly rapid to a position near the workpiece, then start the spindle at 1000RPM. This would then be an ideal position for you to go into Jog mode and 'touch on' your workpiece for setting your offsets.


The Machine Tooling Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options and display any secondary menus.  Click the highlighted option to select it.

Note:  This menu is only available when the "Machine Tooling" window is active.

New:  Select this option to start a new collection of data describing the tool profiles present in the lathes' turret.

Open:  Select this option to open a previously saved tooling file (.TFT ) which includes the tool offsets and which tools are in the turret.

Save: Saves the current tooling layout as a .tft file under its original filename

Save As: Saves the current tooling layout as a new .tft filename

Related Topics:

The Options Toolbar

The Machine Tooling Window

The Tooling Library Window


The Machine Tooling Window Page 1 of 3
The Machine Tooling Window 1 of 2

Part 1: Displaying the "Tooling" window

The "Machine Tooling" window allows different types of tool profile from the "Tooling Library" to be added to the numbered pockets in the Automatic Tool Changer carousel.

These tool numbers are used by any CNC files in the 2D or 3D Simulation windows and on the Virtual Reality CNC machines and real CNC machines.

To display the "Machine Tooling" window, click the [Tooling] button, shown above, from the "Options" toolbar.

General Layout

Each coloured number refers to a pocket on the Tool Changer (ie, Turret).  A greyed out number indicates that the pocket is empty. When a tool is transferred from the "Tooling Library" window to the carousel, the colour allocated to that tool from the "Tooling Library" window is also transferred.  These colours are applied to the different pocket numbers as they become filled.

A depressed number button indicates the tool data that is now been viewed and that which would be changed to if the'Change Tool' button was pressed. In the example above, tool number 3 - external threading tool is currently shown.

The Change Tool button causes the machine to the start tool change sequence (eg, Turret rotation) and is active under the following conditions:

1. VR or Real machine is connected and running

2. Control panel mode is Auto

3. The tool required is not already the currently active tool

The data panel in the centre of the window shows some of the tools' details. To see all the details click the small button marked >>.

To close the "Machine Tooling" window, click the [Tooling] button, from the "Options" toolbar.

Related Topics:

The Options Toolbar

The Machine Tooling Menu

The Tooling Library Window

The Tooling Library Menu


The Machine Tooling Window Page 2 of 3
The Machine Tooling Window 2 of 2

Part 2: Transferring Tools into the "Tooling" window

Tool profiles are transferred from the "Tooling Library" window into the "Machine Tooling" window, where they become available for use with any CNC files.

Deleting Tools from the "Tooling" window

Right click on the tool station that you wish to remove then select "Remove":

Click the right mouse button on the carousel pocket number of the tool you want to remove.  Highlight and click the "Remove Tool" option on the pop-up menu, then highlight and click on the title of the tool you want to add.  The selected tool will then be added to the specified carousel pocket number.

Adding Tools into the "Tooling" window

Click the right mouse button on the empty carousel pocket number in the "Tooling" window.  Highlight and click the "Insert Tool" option on the pop-up menu, then highlight and click on the title of the tool you want to add. Only tools that have not already been used from the tool library, will be available.

Drag and Dropping Tools into the "Tooling" window

In the "Tooling Library" window, click and hold down the left mouse button on the title of the tool you want to add to the turret (carousel).  Whilst continuing to hold down the left mouse button, drag the tool across and into the "Tooling" window.  Position the cursor over the required empty turret number and release the left mouse button.  The selected tool will then be added to the specified turret pocket number.

Related Topics:

The Options Toolbar

The Machine Tooling Menu

The Tooling Library Window

The Tooling Library Menu


The Main VR CNC Milling Program Status bar
The Main VR CNC Turning Program Status bar

The main VR CNC Turning status bar is displayed in the bottom left corner of the main program window.

Information is displayed along two rows.

Upper row (boxed information listed from left to right):

1) Offsets: (name of the currently loaded workpiece offset ).

2) File: (name and location of the currently loaded CNC file).

Lower row (boxed information listed from left to right):

1) Units of Measurement, defined by "Metric" (Metric - millimetre units) or "Inch" (Imperial - inch units).

2) Editor Play Mode, defined by "Continuous" (CNC file plays from start to finish) or "Single Step" (CNC file plays one line at a time).

3) Block Skip Mode, defined by "Block Skip OFF" (CNC file lines beginning with a / character are included) or "Block Skip ON" (CNC file lines beginning with a / character are excluded)

4) Radius or Diameter programming mode - see Radius/Diameter programming for an explanation


The Modify Menu

Alter Feed Rates...:  Select this option to apply global changes across the range of feed rate values in the CNC file.

Click here for more about "Alter Feed Rates..."

Alter Speeds...:  Select this option to to apply global changes across the range of spindle speed values in the CNC file.

Click here for more about "Alter Speeds..."

Alter X Values...:  Select this option to to apply global changes across the range of X co-ordinate values in the CNC file.

Click here for more about "Alter X Values..."

Change to UpperCase:  Select this option to change any highlighted characters in the "Editor" window to CAPITALS.

Click here for more about "Change to UpperCase"

Change to LowerCase:  Select this option to change any highlighted characters in the "Editor" window to lowercase.

Click here for more about "Change to LowerCase"

Add Padding Token:  Select this option to add a specified number of spaces between program words.

Click here for more about "Add Padding Token"

Remove Padding Token:  Select this option to remove a specified number of spaces between program words.

Click here for more about "Remove Padding Token"

Append Line End Token:  Select this option to add line end formatting to program lines.

Click here for more about "Append Line End Token"

Remove Line End Token:  Select this option to remove line end formatting from program lines.

Click her for more about "Remove Line End Token"

Line Numbering...:  Select this option to add or remove program line numbers to or from the beginning of each program line.

Click here for more about "Line Numbering..."


The Options Toolbar

Outputs buttons, listed from left to right:

[Units]:  Click this button to switch the units of measurement between Metric (millimetres) and Imperial (Inch).  The current setting of the option is displayed in the main program status bar.  This option can also be configured using the "Setup | Units" menu option.

[Offsets]:  Click this button to display the "Work Piece Offsets" window, used to configure any tool offsets to be used with the CNC file.

[Tooling]:  Click this button to display the "Machine Tooling" window, allowing different types of tool from the "Tooling Library" to be added to the numbered slots in the ATC (Automatic Tool Changer) carousel.

[Tool Library]:  Click this button to display the "Tooling Library" window, allowing configuration of all the various pieces of data that relate to the individual types of tool that can be used with the CNC machine.

[Block Skip]:  Click this button to active the block skip option.  The current setting of the option is displayed in the main program status bar.  When active, any blocks are ignored by the control when a forward slash character, / , is placed in front of the block.

Click here for more about Block Skip

[Continuous] / [Single Step]:  Click this button to switch between "Continuous" or "Step" modes, defining the methods used for running any CNC file.  The current setting of the option is displayed in the main program status bar.  This option can also be configured using the "Setup | Execute Mode" menu option.

[Continuous]:

When the CNC file is started, all program lines will be executed until the program is paused, stopped, an error is encountered or the end of the program is reached.

[Step]:

When the CNC file is started, the program will only run the line on which the "Editor" window cursor is placed.  The [Enter] key on the computer keyboard must be pressed to execute the next program line.


The Outputs Toolbar

Outputs buttons, listed from left to right:

[2D Simulation]:  Click this button to display the output from the CNC file on a plan view of the billet, when the [Play] button is clicked on the "File Control" toolbar.

[3D Simulation]:  Click this button to display the output from the CNC file on a 3 dimensional view of the billet, when the [Play] button is clicked on the "File Control" toolbar.

[Compiled]:  Click this button to save the output from the CNC program as as a Denford Compiled file (.XNC), when the [Play] button is clicked on the "File Control" toolbar.

[Post Output]:  Click this button to save the output from the CNC program as as a Denford Post Processor file (.GNC), when the [Play] button is clicked on the "File Control" toolbar.


The Preferences Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Background Colour...:  Select this option to change the colour of the "Editor" window background.

Click here for more about "Background Colour..."

Display Options...:  Select this option to configure the colour and style used to highlight each program word when applying "Colour Format Text".

Click here for more about "Display Options..."

Colour Format Text:  Select this option to apply a format to the CNC file, allowing groups of program words to be highlighted by colour and/or style.

Click here for more about "Colour Format Text"

Font...:  Select this option to change the name and format of typeface used in the "Editor" window.

Click here for more about "Font... "

Format Using...:  Select this option to load a collection of editor format settings.

Click here for more about "Format Using..."

Save Format...:  Select this option to save the current collection of editor format settings.

Click here for more about "Save Format..."


The Search Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options and display any secondary menus.  Click the highlighted option to select it.

Find...:  Select this option to search through the CNC file for specific characters and words.

Click here for more about "Find..."

Goto Line Number:  Select this option to move to a specific line number in the CNC file.

Click here for more about "Goto Line Number"

Check Syntax:  Select this option to check for illegal entries in the CNC file.

Click here for more about "Check Syntax"


The Setup Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options and display any secondary menus.  Click the highlighted option to select it.

Units:  Select this option to set the software to read "Metric! or "Inch" units of measurement, in line with the format used in the CNC file.  A bullet marker is displayed next to the title of the selected option.

Metric:  Metric units - millimetres.

Inch:  Imperial units - inches.

Execute Mode:  Select this option to switch between "Continuous" or "Step" modes, defining the methods used for running any CNC file.

Continuous:  When the CNC file is started, all program lines will be executed until the program is paused, stopped, an error is encountered or the end of the program is reached.

Step:  When the CNC file is started, the program will only run the line on which the "Editor" window cursor is placed.  The [Enter] key on the computer keyboard must be pressed to execute the next program line.

Select Language:  Select this option to change the type of language used for the software menus, toolbars and windows, from the language options available.

Machine Parameters...:  Select this option to open the "Machine Properties Editor" window, allowing a comprehensive range of settings for each CNC machine to be viewed or edited.

Click here for more about "Setup Machine Parameters..."

Default Billet Size...:  Select this option to define the size of the billet used in the "2D Simulation", "3D Simulation" and "Denford Virtual Reality" windows.

Click here for more on "Default Billet Size..."

ToolBars:  Select this option to open the "ToolBar Setup" window.  This window allows the settings for each toolbar button to be configured and may be password protected.  Note - the fields in this option should only be edited by your CNC machine Technician or Supervisor.  Please refer to the separate helpfile distributed on the VR CNC Turning CD-ROM for further information.

View Cycle Expansion  Select this option to switch the "Cycle Expansion" feature on or off.  When the feature is selected a tick mark is displayed next to the title. Expands program cycles to show full code at the base of the "Editor" window, when the CNC file is run.

Click here for more about "Cycle Expansion"

Related Topics:

Toolbar Defaults


The Tooling Library Menu

Click the menu title to display the dropdown list. Click the highlighted option to select it.

Note:  This menu is only available when the "Tooling Library" window is active.

Import:  Select this option to display the "Open" window, allowing a Turning Tooling DataBase File (.TTD) to be imported.

Export:  Select this option to display the "Save As" window, allowing the current Turning Tooling DataBase File (.TTD) to be exported.

Related Topics:

The Options Toolbar

The Machine Tooling Window

The Tooling Library Window


The Tooling Library Window Page 1 of 3
The Tooling Library Window Page 1 of 2

To display the "Tooling Library" window, click the [Tool Library] button (shown below) from the "Options" toolbar.

The Tooling Library contains the list of tool profiles available for use in the Automatic Tool Changer (when fitted) and in the machine head.

General Layout

To highlight a tool profile, click on its title.  A graphic will be displayed in the left panel, relating to the type of tool selected.  Highlighted tool profiles are shown using white title text on a blue background.

Click here for a list of the default Tooling Library profiles available

To close the "Tooling Library" window, click the [Tool Library] button, from the "Options" toolbar.

Related Topics:

The Options Toolbar

The Tooling Library Menu

The Machine Tooling Window

The Machine Tooling Menu


The Tooling Library Window Page 2 of 3
The Tooling Library Window Page 2 of 2

Within the tool library, it is possible to change any of the parameters for each tool available (Simulation colour, tip size, angle etc . .)

You can also add or delete tools.

In the screenshot above, the tool called "Roughing Tool" has been changed into a Drill type tool. Click on the drop down menu under 'ToolType' to change to type of tool.

To alter data such as shank length simply click the small up/down arrows on the right of the edit box you wish to change. Alternatively, click inside the box and enter a new value

You will notice that this tool is previewed in the bottom left hand corner of the display.

It is currently pointing in the wrong direction. To remedy this, alter the Tool Orientation and Tip Orientation values by clicking on their drop down menus:

Tool definitions can be added, deleted or copied by right clicking in the tool list :

Note:  Any data changes made will also be applied to tools currently available in the machines Tooling window (ie, in the turret).

Related Topics:

The Options Toolbar

The Tooling Library Menu

The Machine Tooling Window

The Machine Tooling Menu


The Utilities Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Configure Utilities...:  Select this option to display the "Configure Utilities" window, used to setup shortcuts to other programs using the MS Windows Operating System.

Click here for more about "Configure Utilities..."


The Windows Menu

Click the menu title to display the dropdown list.  Move the cursor down the list to highlight the options.  Click the highlighted option to select it.

Cascade:  Select this option to display any open windows in a cascading pattern, one on top of another.

Click here for more about "Cascade"

Tile:  Select this option to display any open windows in a tiled pattern, one next to another.

Click here for more about "Tile"

??? Window name: Any sub windows such as the editor, 2D and 3D simulations can be selected or highlighted by checking the name at the bottom of this menu bar.


The Work Piece Offsets Window Page 1 of 5
The Work Piece Offsets Window Page 1 of 3

To display the "Work Piece Offsets" window, click the [Offsets] button (shown below) from the "Options" toolbar.

Click here for more about the Theory of Offsets

General Layout

The "Work Piece Offsets" window is used for configuring the workpiece offset values.

Note - Workpiece Offset files are global.  All tool profiles use the values contained in the loaded Workpiece Offset file.

These offset files are used on the 'real' CNC machine and the VR CNC machine.  They are used to set the position of the workpiece datum.  The 2D and 3D Simulation windows use seperately defined offsets which can be set relative to the front and centre of the billet shape.

The List of Offsets

The large white panel on the left of the "Work Piece Offsets" window displays the list of available machine and simulation offsets. To highlight an offset, click on its title.  Highlighted offsets are shown using white title text on a blue background.  In the example above, the "Offset 3" has been highlighted.

Modifiying the list of Offsets

RIGHT click on any offset title to bring up the menu shown above. Here you can copy, paste, delete or edit that offset.

"Make Current" will activate that offset so that your CNC program will take these values into account. Note the red rick mark that appears next to the currently active offset title.

Related Topics:

The Theory of Offsets

Coordinate system display types


The Work Piece Offsets Window Page 2 of 5
The Work Piece Offsets Window Page 2 of 3

Working with the list of Machine Offsets

Machine Offset files are used on the 'real' CNC machine and the VR CNC machine.  They can also be set to be used on the 2D and 3D Simulation windows.

Note - Workpiece Offset files are global.  All tool profiles use the values contained in the loaded Workpiece Offset file.

The screenshot above shows the automatic datum buttons (highlighted in RED) which become available when you are connected to a VR or Real machine.

Pressing X or Z auto-datum button will bring up the menu 'X offset' or 'Z offset'.

In the screenshot above, the yellow highlight shows the current billet size as programmed (80mm). When 'Include Diameter' is selected, then this value is taken into account when you press OK to set your workpiece offset. In this example, pressing OK will enter a number into the X value for offset 1 which cause the current Program position readout to read X 80.000

So, the current position of the current tool is now set to X 80.000

If the "Use origin only" option was selected, then the readout would be X 0.000

Related Topics:

The Theory of Offsets

Coordinate system display types


The Work Piece Offsets Window Page 3 of 5
The Work Piece Offsets Window Page 3 of 3

Working with the list of Machine Offsets cont'd.

The screenshot above shows the automatic datum button for Z axis (highlighted in RED) which becomes available when you are connected to a VR or Real machine.

Pressing Z auto-datum button will bring up the window 'Z offset'.

In the screenshot above, the yellow highlight shows the clearance setting (10mm). This value is taken into account when you press OK to set your workpiece offset. In this example, pressing OK will enter a number into the Z value for offset 1 which cause the current Program position readout to read Z 10.

So, the current position of the current tool is now set to Z 10.000

If the clearance value was 0, then the Program readout would be Z 0.000

Procedure for setting workpiece offsets on a VR or real machine

1. Call up your first tool, and check that its tool offset is also active.

2. Jog the tool to a position that you know the dimensions of, in relation to you workpiece.

This may be by touching the workpiece, or touching a 'slip' which you know the size of.

3. Call up the workpiece offset window, click the X or Z datum buttons. Enter the size that you know the tool is touching.

4. Confirm your setting by looking at the program display type in the machine control panel. It should now read the size that you know the tool is touching. For, example if you have turned a billet down to 23.567mm and the tool is still in line with this diameter, then when you set your X offset the Program readout should say X 23.567

Related Topics:

What are offsets?

Coordinate system display types


Tile
"Windows|Tile"

Select this option to display any open windows in a tiled pattern, one above the other (shown above).  This option is applied to any windows open in the VR CNC Turning software.  The windows are tiled in a configuration suitable for the overall size of the VR CNC Turning software window and the number of internal windows open.


Tutorial: Configuring Tool Offsets for use with the VR CNC Machine Part 1
Configuring Offsets with a VR CNC Machine

Part 1: What are Offsets?

When we write a CNC program, all co-ordinates used for describing the shape of the part are stated relative to a zero reference, called the part datum.

In the sample CNC files used with this tutorial, the part datum is positioned in the centre and the at end face imaginary billet.

The CNC machine also has a zero reference, called the machine datum.  If no offsets are loaded, our CNC file will use this position as the start location for any machining co-ordinates.

Offsets are used to establish the location of the workpiece datum on the real billet.  The workpiece datum is the position where we want any physical machining co-ordinates to be taken from.  Using the Offsets facility, we can temporarily shift the entire co-ordinate based grid system of the CNC machine.  We must move the two dimensional grid, so the position of the workpiece datum registers as zero, rather than the position of the machine datum.

Offsets are very important because without them, the CNC machine will not know where to begin cutting on the billet.  Offsets must always be configured before manufacturing our part.  However, once you configure and save an offset file, the same file may be used over and over again, as long as the following holds true:

- The same cutting tools are used.

- The billet size does not change.

- The fixture that holds the billet does not move position on the machine table.

Click here for more detailed information about Offsets

The Process of Configuring Offsets

In order to establish the workpiece datum, so it is in the same position for all the tool profiles we want to use, two types of offset file must be configured:

1) The Workpiece Offset File - This file allows global values to be set for the X and Z co-ordinates, ie, workpiece offset values are used by every tool, irrespective of tool size.  The X and Z offsets need only be set once, since their values are common to all tool profiles.

2) The X and Z Tool Offset Files - Since all tool profiles differ in relative position to each other, each tool profile has its own individual X and Z tool offset file.  These values will be different for each tool.  They compensate for the differences in length, so various tools can be used together on with single CNC file.

The X and Z position of the workpiece datum is defined by the value entered into the X or Z dialogue boxes of the workpiece offsets window:-

The X and Z position of the Tool offset datum is defined by the value entered into the X or Z dialogue boxes of the tooling offsets window:-

Different tool offsets can be defined for the same tool. For example programming T0101 M6 will change the tool in the machine to station 1 and activate tool offset number 1. Programming T0106 M6 will change the tool in the machine to station 1 and activate tool offset number 6. Usually, however, the tool offset number matches the actual tool number.

Configuring the Tool Offsets for the Sample CNC file on a VR CNC Machine

If you are running through the tutorials using the sample CNC files,  the procedure for setting workpiece datum and tool offsets for tool 1 and tool 3 is as follows:

1. Set the X and Z tool offset values for tool offset 1 to 0.000  (in the above screen shot they are currently X-20.00 Z 0.8)

2. Select tool 1 on the machine by clicking "Change Tool !" (Remember you must be in Auto mode for this to work)

3. Make sure tool 1 offset 1 is selected on the control panel

4. Jog the tool to the billets' front face and touch the outer diameter:

5. Select workpiece offsets and select Datums so X reads 25.000 and Z reads 0.000.  The workpiece offset is now set and tool 1s' tool offset is X0.000 Z0.000 ie, zero. In this way, we have made tool 1 our 'master' tool and all other tool offset dimensions are relative to this.

6. Select tool 3 on the machine by clicking "Change Tool !" (Remember you must be in Auto mode for this to work)

7. Jog this tool to the billets' front face and touch the outer diameter:

6. Select the tool offsets window this time and set the datums for both X and Z tool offsets. (Remember to select "Include Diameter" so that X reads 25.000 - the billets diameter). You will notice that the tool offsets values for offset 3 will read somewhere between +/- 5mm - that is the difference in position/size between the tips of tool 1 and tool 3.

7. The machine is now ready to run the example program !

Recap - When we configure the offsets, we are temporarily shifting the entire co-ordinate based grid system of the CNC machine, so its zero co-ordinate aligns with our workpiece datum.


Tutorial: Configuring Tool Offsets with a real CNC Machine Part 1
Configuring offsets on a real CNC Machine

Part 1: What are Offsets?

When we write a CNC program, all co-ordinates used for describing the shape of the part are stated relative to a zero reference, called the part datum.

In the sample CNC files used with this tutorial, the part datum is positioned in the centre and the at end face imaginary billet.

The CNC machine also has a zero reference, called the machine datum.  If no offsets are loaded, our CNC file will use this position as the start location for any machining co-ordinates.

Offsets are used to establish the location of the workpiece datum on the real billet.  The workpiece datum is the position where we want any physical machining co-ordinates to be taken from.  Using the Offsets facility, we can temporarily shift the entire co-ordinate based grid system of the CNC machine.  We must move the two dimensional grid, so the position of the workpiece datum registers as zero, rather than the position of the machine datum.

Offsets are very important because without them, the CNC machine will not know where to begin cutting on the billet.  Offsets must always be configured before manufacturing our part.  However, once you configure and save an offset file, the same file may be used over and over again, as long as the following holds true:

- The same cutting tools are used.

- The billet size does not change.

- The fixture that holds the billet does not move position on the machine table.

Click here for more detailed information about Offsets

The Process of Configuring Offsets

In order to establish the workpiece datum, so it is in the same position for all the tool profiles we want to use, two types of offset file must be configured:

1) The Workpiece Offset File - This file allows global values to be set for the X and Z co-ordinates, ie, workpiece offset values are used by every tool, irrespective of tool size.  The X and Z offsets need only be set once, since their values are common to all tool profiles.

2) The X and Z Tool Offset Files - Since all tool profiles differ in relative position to each other, each tool profile has its own individual X and Z tool offset file.  These values will be different for each tool.  They compensate for the differences in length, so various tools can be used together on with single CNC file.

The X and Z position of the workpiece datum is defined by the value entered into the X or Z dialogue boxes of the workpiece offsets window:-

The X and Z position of the Tool offset datum is defined by the value entered into the X or Z dialogue boxes of the tooling offsets window:-

Different tool offsets can be defined for the same tool. For example programming T0101 M6 will change the tool in the machine to station 1 and activate tool offset number 1. Programming T0106 M6 will change the tool in the machine to station 1 and activate tool offset number 6. Usually, however, the tool offset number matches the actual tool number.

Configuring the Tool Offsets for the Sample CNC file on a VR CNC Machine

If you are running through the tutorials using the sample CNC files,  the procedure for setting workpiece datum and tool offsets for tool 1 and tool 3 is as follows:

1. Set the X and Z tool offset values for tool offset 1 to 0.000  (in the above screen shot they are currently X-20.00 Z 0.8)

2. Select tool 1 on the machine by clicking "Change Tool !" (Remember you must be in Auto mode for this to work)

3. Make sure tool 1 offset 1 is selected on the control panel

4. Jog the tool to the billets' front face and touch the outer diameter:

On the real machine you would take a facing then turning cut in order to accurately set the tools' position. ie:

Turn a small amount off the diameter of the billet.

Keep the X axis in the position used to take the cut.

Measure the cut diameter and use this value when setting the tool offset.

(as an example, you may have measured a cut of 23.567mm diameter)

Then, face off a small amount off the end of the billet.

Keep the Z axis in the position used to take the cut.

Now, you can set the Z axis offset to exactly zero, knowing that your tool must be touching the face of the billet.

5. Select workpiece offsets and select Datums so X reads 25.000 and Z reads 0.000.  The workpiece offset is now set and tool 1s' tool offset is X0.000 Z0.000 ie, zero. In this way, we have made tool 1 our 'master' tool and all other tool offset dimensions are relative to this.

6. Select tool 3 on the machine by clicking "Change Tool !" (Remember you must be in Auto mode for this to work)

7. Jog this tool to the billets' front face and touch the outer diameter:

6. Select the tool offsets window this time and set the datums for both X and Z tool offsets. (Remember to select "Include Diameter" so that X reads 25.000 - the billets diameter). You will notice that the tool offsets values for offset 3 will read somewhere between +/- 5mm - that is the difference in position/size between the tips of tool 1 and tool 3.

7. The machine is now ready to run the example program !

Recap - When we configure the offsets, we are temporarily shifting the entire co-ordinate based grid system of the CNC machine, so its zero co-ordinate aligns with our workpiece datum.


Tutorial: Connecting to the real CNC Machine Part 1
Connecting to a real CNC Machine

Data is sent and received between your computer and your CNC machine using an RS232 lead.

One end of the RS232 lead fits into the serial (COM) port of the computer running the VR Milling Windows software.  Computer serial ports are the small plugs, each containing two rows of 5 and 4 pins, usually positioned on the back panel of your computer.

The opposite end of the RS232 lead fits into the serial (COM) port on your CNC machine control box.


Tutorial: Context Sensitive Help Part 1
Context Sensitive Help

What is Context Sensitive Help?

At the press of a key, context sensitive help automatically guides you to the appropriate sections of helpfiles, whenever you need help with various parts of the software.  Context sensitive help is available for the following items:

Menu:  To obtain context sensitive help on a software menu, click the menu title to display its dropdown list of options, then press the [F1] key.

Click here for more about Context Sensitive Menu Help

Window:  To obtain context sensitive help on a software window, press the [F1] key when the required window is active.

Click here for more about Context Sensitive Window Help

G and M codes:  To obtain context sensitive help on an individual G or M code, position the "Editor" window cursor in the middle of the text for the code required, then press the [Ctrl] + [F1] keys.

Click here for more about Context Sensitive G and M code Help

Available Helpfiles

The VR CNC Turning software contains two separate helpfiles, both available from the "Help" menu title.

VR CNC Turning:  The VR CNC Turning for Windows software helpfile (the helpfile currently being viewed).  This helpfile contains VR CNC Turning tutorials, detailed information about the various features of the VR CNC Turning software, troubleshooting guides and a guide to CNC Theory.

CNC Programming:  The CNC Milling Programming helpfile.  This helpfile contains detailed information about individual G and M codes and structure of CNC files.


Tutorial: Creating a New CNC file Part 1
Creating a New CNC file

Part 1: Creating a New CNC file

Click "File | New" to create a new CNC file, as shown below.

The blank "Editor" window will be displayed, as shown below.

The "Editor" window behaves in a similar way to a simple word processor, such as Windows Notepad.


Tutorial: Creating a New CNC file Part 2
Creating a New CNC file

Part 2: Entering Data into the "Editor" window

Click the mouse inside the "Editor" window, then begin typing in the text from your CNC file.

Your CNC file describes the program of commands and movements used to manufacture the part, hence CNC files are often referred to as Part Programs.

If you intend running through the entire series of tutorials, we suggest you use the sample CNC files...

Click here to view the a sample CNC files used in this tutorial

As text characters are typed, they will appear on the appropriate line of the "Editor" window, as shown below.

When each line of text is completed, press the [Enter/Return] key to create a new program line.

CNC Programming Basics

CNC files are constructed using G and M codes.

Each line of G and M codes is called a block, for example, 'G91 G28 X0 Y0 Z0', from the part program shown above.

Each block is created from different program words, for example, 'G91' is one word from the part program shown above.

Each program word is constructed from a letter, called the address, and a number.  The address letter, together with its number describes the type of code used.

For more information about using G and M codes, click "Help | CNC Programming" to display the CNC Programming helpfile, containing sections on part program structure and illustrated descriptions explaining the use of each G and M code.


Tutorial: Editing a CNC file Part 1
Editing a CNC file

Part 1: Positioning the "Editor" window cursor

The "Editor" window cursor is a flashing vertical black line, shown circled red in the above screenshot.  This cursor shows where characters can currently be inserted, removed or highlighted.  To remove characters directly behind the "Editor" window cursor, press the [Delete] key.  To create a new CNC file line, press the [Enter/Return] key.

The mouse positioning cursor is a vertical black line with bars at its top and bottom, shown circled yellow in the above screenshot.  This cursor is used to move the "Editor" window cursor to new positions in the CNC file.

To reposition the cursor in the "Editor" window:

Position the mouse positioning cursor in the required area, then click the left mouse button to move.

Use the four computer [Cursor] arrow keys to move the "Editor" window cursor to the required position.

Use the [Page Up] key to move to the top of the CNC file.

Use the [Page Down] key to move to the bottom of the CNC file.

Use the [Home] key to move to the beginning of the current CNC file line.

Use the [End] key to move to the end of the current CNC file line.


Tutorial: Editing a CNC file Part 2
Editing a CNC file

Part 2: Selecting and editing areas of text

To select areas of text in the "Editor" window, position the "Editor" window cursor (the vertical black line) at the start or end of the text required, then click and hold down the left mouse button.  Drag over the required characters to highlight them, as shown above.

To select all the text in the "Editor" window, click "Edit | Select All".

The highlighted characters can be edited using the following commands:

Select the "Cut" option from the "Edit" menu to cut any highlighted text from the "Editor" window to the Windows clipboard.  Computer keyboard shortcut: [CTRL + X]

Select the "Copy" option from the "Edit" menu to copy any highlighted text from the "Editor" window to the Windows clipboard.  Computer keyboard shortcut: [CTRL + C]

Select the "Paste" option from the "Edit" menu to place any text held in the Windows clipboard to the current "Editor" window cursor position.  Computer keyboard shortcut: [CTRL + P]

Select the "Undo" option from the "Edit" menu to undo the last command performed in the "Editor" window.

Select the  "Redo" option from the "Edit" menu to repeat the last command performed in the "Editor" window.


Tutorial: Example CNC file Part 1
Sample CNC file - Metric version

The CNC file shown below is used throughout this series of tutorials:

Below: 3d simulation of the metric (millimetres) sample CNC file.

Billet: Brass or Steel

Part Datum Position: Centre line of part and opposite the chuck end.

Dimensions: X (Diameter) 25mm,  Z (Length) 55mm

Tools required:

Tool 1 : General Roughing/Finishing Turning tool.

Tool 3 : Threading tool.

Metric (millimetres) sample CNC file with no formatting:

This program is written in Diameter programming - be sure that your software is configured for diameter programming - for more information see Radius Diameter programming

Check that the units of measurement are set to "Metric".  The units of measurement are configured using the [Units] button on the "Options" toolbar.

Copy and paste the CNC file listed below into a new (blank) "Editor" window.

Save the CNC file as "Dalek.fnc".

! Warning ! Do not renumber this program as block N1 is used to define the start of the profile.

[BILLET X25 Z55

O0001

G21

G99

M06 T0101

G97 S1500 M03

G00 X25 Z0

G01 X-1 F.05

G00 X25 Z2

G71 U1.5 R.25

G71 P1 Q2 U1.0 W.1 F.07

N1 G00 X0

G01 Z0

G03 X17 Z-8.5 R8.5

G01 Z-13.5

X20 Z-14.36

Z-28.5

X24 Z-46.5

X26

N2 G00 X26 Z2

G70 P1 Q2

G28 U0 W0

M06 T0303

G97 S350 M03

G00 X20.5 Z-10

G76 P050060 Q035 R.05

G76 X18.00 Z-26.5 P1000 Q070 F1.5

G28 U0 W0

M30


Tutorial: Example CNC file Part 2
Sample CNC file - Metric version

Explanation of metric (millimetres) sample CNC file:

[BILLET X25 Z55

^ Sets the size of the billet to be displayed in 2D 3D and VR windows

O0001

^ Says that this is program 0001

G21

^ All relavant numbers are interpreted as metric values

G99

^ Sets the feed type to mm per revolution of the spindle (So, spindle must be running for any feedrate moves to occur)

M06 T0101

^ Calls up Tool 1, offset 1 - M06 will send the machine command to spin the turret where available

G97 S1500 M03

^ G97 says that the next spindle speed will be in Revs Per Minute (RPM)

^ S1500 sets the current spindle to 1500 RPM and M03 starts the spindle clockwise

G00 X25 Z0

^ Do a rapid (Max feed), two axis move to the position X25 Z0 (The top right corner of the billet)

G01 X-1 F.05

^ Take a feed cut down the face of the billet to X-1 with a feed of 0.5 mm per revolution of the spindle

G00 X25 Z2

^ Rapid move to X25 Z2

G71 U1.5 R.25

G71 P1 Q2 U1.0 W.1 F.07

^ Defines the cutting parameters for the stock removal cycle (see Programming help for more details)

^ Then does stock removal using profile/shape between in blocks N1 and N2 (P1 Q2)

N1 G00 X0

^ Start of profile definition - block number N1

G01 Z0

G03 X17 Z-8.5 R8.5

G01 Z-13.5

X20 Z-14.36

Z-28.5

X24 Z-46.5

X26

N2 G00 X26 Z2

^ end of profile definition - block number N2

G70 P1 Q2

^ Now run a finishing pass over the profile defined between block N1 and N2 (P1 Q2)

G28 U0 W0

^ Send X and Z axes back to home position (machine datum point)

M06 T0303

^ Calls up Tool 3, offset 3 - M06 will send the machine command to spin the turret where available

G97 S350 M03

^ G97 says that the next spindle speed will be in Revs Per Minute (RPM)

^ S350 sets the current spindle to 350 RPM and M03 starts the spindle clockwise

G00 X20.5 Z-10

^ Rapid move to X20.5 Z-10

G76 P050060 Q035 R.05

G76 X18.00 Z-26.5 P1000 Q070 F1.5

^ Definition of the multi-pass threading cycle. See programming manual/help for full details

G28 U0 W0

^ Return to machine home position

M30

^ Finish the program, stops the spindle and rewinds back to the beginning.


Tutorial: Formatting a CNC file Part 1
Formatting a CNC file

Part 1: Adding Program Line Numbering

To add program line numbers to your finished CNC file, click "Modify|Line Numbering..." to display the "Line Numbering" window.

! Warning ! Some programs will not work as expected if you renumber them because of stock removal profile definition

Enter the number you want to use as first line of the program in the "Start Number" dialogue box.  In the example above, 1 has been specified.

The "Numbering Increment" dialogue box is used to set the numerical gap between each program line number.  In the example above, 10 has been specified, so the program line numbers will follow the sequence 1, 11, 21, 31, 41, 51 etc.

The "Minimum number length" dialogue box is used to set the amount of characters used to display each program line number.  In the example above, 3 has been specified, so the program line numbers will follow the sequence 001, 011, 021, 041, 051 etc.

The "Numbering Token" dialogue box is used to add an address character to start of each program line number.  The standard numbering token used is N.  In the example above, the program line numbers will follow the sequence N 001, N 011, N 021, N 041, N 051 etc.

Click the [OK] button to apply program line numbering settings to the CNC file.

An example of a modified CNC file is shown below.

Before modifications:

After modifications (add program line numbering):


Tutorial: Formatting a CNC file Part 2
Formatting a CNC file

Part 2: Adding End of Block symbols

To add end of block symbols to your finished CNC file, click "Modify | Append Line End Token..." to display the "Request" window.

If you want to add end of block symbols to only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, end of block symbols will be applied to the whole of the CNC file.

In the "Request" window dialogue box enter the character/s to be used for denoting the end of program lines, then click the [OK] button.  The standard symbol used when CNC programming is the [semi-colon] character ;.

An example of a modified CNC file is shown below.

Before modifications:

After modifications (add ; symbol):


Tutorial: Formatting a CNC file Part 3
Formatting a CNC file

Part 3: Adding Program Line Spacing

To add padding spaces between program words in your finished CNC file, click "Modify | Add Padding Token..." to display the "Request" window.

If you want to add padding spaces to only part of the CNC file, drag across the required program lines to highlight them.  If no program lines are highlighted, padding spaces will be applied to the whole of the CNC file.

In the "Request" window dialogue box enter the number of spaces required between each program word, then click the [OK] button.  In the example above, 2 spaces have been specified.

An example of a modified CNC file is shown below.

Before modifications:

After modifications (add 2 padding spaces):


Tutorial: Homing a real CNC Machine (Home Mode) Part 1
Homing a real CNC Machine

Part 1: Home Mode

When a CNC machine is first started, the "Machine Mode" window will be displayed with only the "Home" tab active, as shown above.

The "Home" tab is used for configuring the machine before it can be fully used.  This defines the Machine Datum, used as a zero reference for describing other co-ordinate positions and defines the limits of co-ordinate movement for the machine.

Note:  The "MDI" "Jog" and  "Auto" tabs will not be displayed until the machine has been configured by homing both axes.

Homing the CNC Machine Axes

To configure the machine X axis only, click the [X Axis] button.  The X machine slide will move until it has found its limits of co-ordinate movement. Usually this would be upwards on a slant bed lathe.

To configure the machine Z axis only, click the [Z Axis] button.  The Z machine slide will move until it has found its limits of co-ordinate movement. Usually this would be to the right .

To configure both axes together, click the [Both] button.  All machine slides will move until the limits of co-ordinate movement have been found.

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Homing a real CNC Machine (Home Mode) Part 2
Homing a real CNC Machine

Part 2: Co-ordinate System Display Mode

The [Co ordinates] button (highlighted red in both the screenshots below) is used to switch between the two systems for displaying the co-ordinates positions.

The far right panel on the statusbar (highlighted yellow in both the screenshots below) displays the current setting for this button.

When the [Units] of Measurement are set to "Inch" the co-ordinates are displayed using inches.

When the [Units] of Measurement are set to "Metric" the co-ordinates are displayed using millimetres.

Work Piece Co-ordinates Display System

The Work Piece Co-ordinates system displays the co-ordinate position values relative to the moveable workpiece datum.

Machine Co-ordinates Display System

The Machine Co-ordinates system displays the co-ordinate position values relative to the fixed machine datum.moveable

Click here for more about the Co-ordinates Display System Modes

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Homing the VR CNC Machine (Home Mode) Part 1
Homing a VR CNC Machine

Part 1: Home Mode

When a VR CNC machine is first started, the "Machine Mode" window will be displayed with only the "Home" tab active, as shown above.

The "Home" tab is used for configuring the machine before it can be fully used.  This defines the Machine Datum, used as a zero reference for describing other co-ordinate positions and defines the limits of co-ordinate movement for the machine.

Note:  The "MDI" "Jog" and  "Auto" tabs will not be displayed until the machine has been configured by homing both axes.

Homing the CNC Machine Axes

To configure the machine X axis only, click the [X Axis] button.  The X machine slide will move until it has found its limits of co-ordinate movement. Usually this would be upwards on a slant bed lathe.

To configure the machine Z axis only, click the [Z Axis] button.  The Z machine slide will move until it has found its limits of co-ordinate movement. Usually this would be to the right .

To configure both axes together, click the [Both] button.  All machine slides will move until the limits of co-ordinate movement have been found.

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Homing the VR CNC Machine (Home Mode) Part 2
Homing a VR CNC Machine

Part 2: Co-ordinate System Display Mode

The [Co ordinates] button (highlighted red in both the screenshots below) is used to switch between the two systems for displaying the co-ordinates positions.

The far right panel on the statusbar (highlighted yellow in both the screenshots below) displays the current setting for this button.

When the [Units] of Measurement are set to "Inch" the co-ordinates are displayed using inches.

When the [Units] of Measurement are set to "Metric" the co-ordinates are displayed using millimetres.

Work Piece Co-ordinates Display System

The Work Piece Co-ordinates system displays the co-ordinate position values relative to the moveable workpiece datum.

Machine Co-ordinates Display System

The Machine Co-ordinates system displays the co-ordinate position values relative to the fixed machine datum.moveable

Click here for more about the Co-ordinates Display System Modes

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: How to use the Tutorials Part 1
How to use the Tutorials

The tutorials section is designed as a full course, helping you to start using all the different features in the VR CNC Turning software.

The tutorials are divided into six sections:

1: Tutorials Introduction

2: Working with CNC files

3: Using Tool Profiles

4: Running Simulations

5: Using a Virtual Reality CNC Machine

6: Using a real CNC Machine

There are two courses to follow.  If you are new to using the VR CNC Turning software, we recommend that you follow one of the courses from start to finish.  Each full course should take around 1 hour to complete.

Virtual Reality Course:  This course is designed for users intending to use the software offline, ie, with a Virtual reality CNC machine. Follow tutorials 1, 2, 3, 4 and 5.

Real CNC Machine Course:  This course is designed for users intending to use the software online, ie, with a real CNC machine. Follow tutorials 1, 2, 3, 4 and 6.


Tutorial: Loading a CNC file Part 1
Loading a CNC file

Part 1: Loading a CNC file

To load a previously saved CNC file, click "File | Open".

Select the directory used for storing the CNC file, using the "Look in:" panel.

Click on the name of the file required - its name will appear in the "File name:" dialogue box.

2D or 3D Graphic bitmaps of the CNC file are also displayed in the righthand panel, when previously saved, as shown above.

Click the preview icon (highlighted above in red)  to see a larger preview of the bitmap

Click the [Open] button to load the CNC file into the "Editor" window.


Tutorial: Loading a CNC file Part 2
Loading a CNC file

Part 2: Fast Loading of a known CNC file

The "ReOpen" option can be used to gain fast access to known CNC files.

Click "File | ReOpen | choice of filename", to reopen the required CNC file, as shown above.


Tutorial: Moving the Axes on a real CNC Machine (Jog Mode) Part 1
Moving the Axes on a real CNC Machine

Part 1: Jog Mode

The "Jog" tab is used for manually moving the machine within its co-ordinate working envelope.

Jog Control Modes

The "Jog" panel displays the 2 rotary controls for changing feed and speed values.

The axes can be jogged, or moved, using two different methods, outlined below - Continuous or Step.

To change the jog control value, click and hold down the left mouse button on the rotary knob, then drag the knob around in a circular motion to the new position.

When the [Units] of Measurement are set to "Inch" the rate of movement is measured using inches per minute.  When the [Units] of Measurement are set to "Metric" the rate of movement is measured using millimetres per minute.

Jog Continuous:  In jog continuous mode, the selected machine axis will move at the indicated speed when one of the machine axis movement keys are pressed and held down.  The selected machine axis will continue to move until the key is released.  The slider bar can be moved to set jog speeds between 0 and 1000 units.  When Jog Continuous is active, the [Jog] button graphic will be displayed as shown below. (Indicating the current jog speed as 1050mm per minute)

Jog Step:  In jog step mode, the selected machine axis will move one indicated increment, each time the selected axis movement key is pressed.  The slider bar can be moved to set jog increments of 0.01, 0.05, 0.1, 0.5, 1, 2 and 5 mm.  When Jog Step is active, the [Jog] button graphic will be displayed as shown below. (Currently set to 0.5mm step value). Feedrate for the step movement will be at whatever feedrate was last selected.

Jog Control Keys

The Keys used for Jogging can be configured for each different machine, but are usually set to the CURSOR arrow keys where arrow left would be Z minus, arrow right Z plus, arrow up X plus etc ...

Losing Jog Mode

For safety reasons, the software has been written so the using the cursor keys on the keyboard will not accidentally Jog the real machine. So, if another window such as the Editor is selected, then Jog mode is disabled even though you are still technically in Jog mode. The green background on the Jog tab indicates whether you are in Jog mode or not:

 means Jog mode active

 means Jog mode inactive

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Moving the Axes on a real CNC Machine (Jog Mode) Part 2
Moving the Axes on a real CNC Machine

Selecting M Codes

M codes are used for miscellaneous functions, such as switching the spindle on / off and opening / closing the VR CNC machine guard.

Click the [M Codes] button to display the list of M codes, shown above.

Or select "Manual  M code entry" and enter an mcode number into the dialog box that appears.

Move the cursor down the list to highlight the options.  Click the highlighted option to select it.  For detailed information regarding M code Programming, click "Help | CNC Programming" to display the "Denford CNC Programming for Milling Machines" helpfile.


Tutorial: Moving the Axes on the VR CNC Machine (Jog Mode) Part 1
Moving the Axes on a VR CNC Machine

Part 1: Jog Mode

The "Jog" tab is used for manually moving the machine within its co-ordinate working envelope.

Jog Control Modes

The "Jog" panel displays the 2 rotary controls for changing feed and speed values.

The axes can be jogged, or moved, using two different methods, outlined below - Continuous or Step.

To change the jog control value, click and hold down the left mouse button on the rotary knob, then drag the knob around in a circular motion to the new position.

When the [Units] of Measurement are set to "Inch" the rate of movement is measured using inches per minute.  When the [Units] of Measurement are set to "Metric" the rate of movement is measured using millimetres per minute.

Jog Continuous:  In jog continuous mode, the selected machine axis will move at the indicated speed when one of the machine axis movement keys are pressed and held down.  The selected machine axis will continue to move until the key is released.  The slider bar can be moved to set jog speeds between 0 and 1000 units.  When Jog Continuous is active, the [Jog] button graphic will be displayed as shown below. (Indicating the current jog speed as 1050mm per minute)

Jog Step:  In jog step mode, the selected machine axis will move one indicated increment, each time the selected axis movement key is pressed.  The slider bar can be moved to set jog increments of 0.01, 0.05, 0.1, 0.5, 1, 2 and 5 mm.  When Jog Step is active, the [Jog] button graphic will be displayed as shown below. (Currently set to 0.5mm step value). Feedrate for the step movement will be at whatever feedrate was last selected.

Jog Control Keys

The Keys used for Jogging can be configured for each different machine, but are usually set to the CURSOR arrow keys where arrow left would be Z minus, arrow right Z plus, arrow up X plus etc ...

Losing Jog Mode

For safety reasons, the software has been written so the using the cursor keys on the keyboard will not accidentally Jog the real machine. So, if another window such as the Editor is selected, then Jog mode is disabled even though you are still technically in Jog mode. The green background on the Jog tab indicates whether you are in Jog mode or not:

 means Jog mode active

 means Jog mode inactive

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Moving the Axes on the VR CNC Machine (Jog Mode) Part 2
Moving the Axes on a VR CNC Machine

Selecting M Codes

M codes are used for miscellaneous functions, such as switching the spindle on / off and opening / closing the VR CNC machine guard.

Click the [M Codes] button to display the list of M codes, shown above.

Or select "Manual  M code entry" and enter an mcode number into the dialog box that appears.

Move the cursor down the list to highlight the options.  Click the highlighted option to select it.  For detailed information regarding M code Programming, click "Help | CNC Programming" to display the "Denford CNC Programming for Milling Machines" helpfile.


Tutorial: Running a 2D Simulation of a CNC file Part 1
Running a 2D Simulation of a CNC file

Part 1: Displaying the "2D Simulation" window

To display the "2D Simulation" window, click the [2D Simulation] button, shown above, from the "Outputs" toolbar.

Checking 'Auto Save Bitmap' will cause a *.BM2 file to be created every time a program runs through the 2D window.

This file is a bitmap file with the same name as your CNC file which is used for previewing files in the File open dialog.

To close the "2D Simulation" window, click the [2D Simulation] button, shown above, from the "Outputs" toolbar.


Tutorial: Running a 2D Simulation of a CNC file Part 2
Running a 2D Simulation of a CNC file

Part 2: Running a 2D Simulation

Before running the 2D simulation:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

To run the CNC file, ensure the "Editor" window cursor is positioned at the start of the CNC file.

Click the triangular [Play] button from the "File Control" toolbar, shown above.


Tutorial: Running a 2D Simulation with a simulated Tool Offset Part 1
Running a 2D Simulation with a simulated Offset

Part 1: Displaying the "2D Simulation" window using X, Y Offsets

Check that the required "Simulation Offset" is highlighted and configured in the "Tool Offsets" window, as described in the Simulating Offsets tutorial section.

To display the "2D Simulation" window, click the [2D Simulation] button, shown above, from the "Outputs" toolbar.

Note: This menu will only appear when the 2D window is selected (highlighted)

Click the "Use Offsets" option on the "2D Simulate" menu, so a tick mark is shown next to the title, as shown above.

This will display the 2D simulation offset values highlighted in red below.

The position of the workpiece datum is shown by the black and white circular datum symbol:

In the example shown below, the workpiece datum is shifted 15mm positive in the Z axis

To close the "2D Simulation" window, click the [2D Simulation] button, shown above, from the "Outputs" toolbar.


Tutorial: Running a 3D Simulation of a CNC file Part 1
Running a 3D Simulation of a CNC file

Part 1: Displaying the "3D Simulation" window

To display the "3D Simulation" window, click the [3D Simulation] button, shown above, from the "Outputs" toolbar.

Click the "Use X,Y Offsets" option on the "3D Viewer" menu, so a tick mark is shown next to the title, as shown above.  This will display the 3D simulation and allow the changing of simulated offsets.

The "3D Simulation" window will show a fullsize view of the billet, as shown below:

The datum point is shown as centre of piece on the right hand side. Altering the X or Z edit boxes will move this position.

NB, machine offsets are not affected by these values.

To close the "3D Simulation" window, click the [3D Simulation] button, shown above, from the "Outputs" toolbar.


Tutorial: Running a 3D Simulation of a CNC file Part 2
Running a 3D Simulation of a CNC file

Part 2: Running a 3D Simulation

Before running the 3D simulation:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

To run the CNC file, ensure the "Editor" window cursor is positioned at the start of the CNC file.

Click the triangular [Play] button from the "File Control" toolbar, shown above.


Tutorial: Running a 3D Simulation with a simulated Tool Offset Part 1
Running a 3D Simulation with a simulated Offset

Part 1: Displaying the "3D Simulation" window using X, Y Offsets

To display the "3D Simulation" window, click the [3D Simulation] button, shown above, from the "Outputs" toolbar.

Note: This menu will only appear when the 3D window is selected (highlighted)

Click the "Use Offsets" option on the "3D Simulate" menu, so a tick mark is shown next to the title, as shown above.

This will display the 2D simulation offset values highlighted in red below.

The position of the workpiece datum is shown by the clear and white circular datum symbol:

In the example shown below, the workpiece datum is shifted 10mm positive in the Z axis and 0mm in the X axis

To close the "3D Simulation" window, click the [3D Simulation] button, shown above, from the "Outputs" toolbar.


Tutorial: Running a 3D Simulation with a simulated Tool Offset Part 3
Running a 3D Simulation with a simulated Offset

Part 2:  Displaying the "3D Simulation" window using X, Y Offsets

Before running the 3D simulation:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

To run the CNC file:

Ensure the "Editor" window cursor is positioned at the start of the first line of the CNC file.

If you do not wish the real or VR machine to move, then make sure machine is not in Auto mode

Click the triangular [Play] button from the "File Control" toolbar, shown above.

The "3D Simulation" window will show the billet being cut, using the configured simulation offset, as shown below.

In this example the shape was cut 10mm away from the front face of the billet (Z+10)


Tutorial: Running a CNC file on a real CNC Machine (Auto Mode) Part 1
Running a CNC file on a real CNC Machine

Auto Mode

Adjusting the feedrate or spindle speed can be done by moving the Potentiometers (where fitted) on a real machine, or by click the large up/down buttons as shown above.

Feed override is available from 0 to 150%

Speed override is available from 50 to 120%

The "Auto" tab is used for controlling the VR CNC machine when running a CNC file.

To start the CNC file, ensure the "Editor" window cursor is positioned at the start of the CNC file.  Click the triangular [Play] button from the "File Control" toolbar, shown above.

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Running a CNC file on the VR CNC Machine (Auto Mode) Part 1
Running a CNC file on a VR CNC Machine

Auto Mode

Adjusting the feedrate or spindle speed can be done by moving the Potentiometers (where fitted) on a real machine, or by click the large up/down buttons as shown above.

Feed override is available from 0 to 150%

Speed override is available from 50 to 120%

The "Auto" tab is used for controlling the VR CNC machine when running a CNC file.

To start the CNC file, ensure the "Editor" window cursor is positioned at the start of the CNC file.  Click the triangular [Play] button from the "File Control" toolbar, shown above.

Note:  The numerical figures depicted on any screenshots will differ according to the CNC machine type, the units of measurement setting for the VR CNC Turning software and any offsets being used on your computer system.


Tutorial: Sample CNC file no formatting
Sample CNC files

Metric (millimetres) sample CNC file with no formatting:

Check that the units of measurement are set to "Metric".  The units of measurement are configured using the [Units] button on the "Options" toolbar.

Copy and paste the CNC file listed below into a new (blank) "Editor" window.

Save the CNC file as "Dalek.fnl".

[BILLET X25 Z55

O0001

G21

G99

M06 T0101

G97 S1500 M03

G00 X25 Z0

G01 X-1 F.05

G00 X25 Z2

G71 U1.5 R.25

G71 P1 Q2 U1.0 W.1 F.07

N1 G00 X0

G01 Z0

G03 X17 Z-8.5 R8.5

G01 Z-13.5

X20 Z-14.36

Z-28.5

X24 Z-46.5

X26

N2 G00 X26 Z2

G70 P1 Q2

G28 U0 W0

M06 T0303

G97 S350 M03

G00 X20.5 Z-10

G76 P050060 Q035 R.05

G76 X18.00 Z-26.5 P1000 Q070 F1.5

G28 U0 W0

M30

M06 T0303

G97 S1200 M03

G00 X26 Z-49.5

G01 X-1.0 F.06

G00 X26

G28 U0 W0

M05

M30


Tutorial: Saving a CNC file Part 1
Saving a CNC file

To save your CNC file, click "File|Save As".

Select the directory used for storing your CNC files, using the "Save in:" panel.

Enter the filename in the "File name:" dialogue box, using the file extension ".fnc", as shown above, then click the [Save] button.


Tutorial: Setting the Units of Measurement Page 1
Setting the Units of Measurement

The units of measurement used by the VR CNC Turning software must be set to match the units of measurement used by your CNC file and any tool profiles used.

For example, if you set the VR CNC Turning software to run in Metric Mode, you must use a metric compatible CNC file and metric tooling.

Click the [Units] button (shown above) from the "Options" toolbar, to change the units of measurement mode between:

"Metric" Mode:  Metric - millimetre units.

"Inch" Mode:  Imperial - inch units.

The current setting of the option is displayed in the main program status bar, positioned in the bottom left corner of the main program window.  The first information box on the upper line of this status bar (highlighted red in the screenshot above) indicates the units of measurement currently in use.

The units of measurement can also be configured using the "Setup | Units" menu option.


Tutorial: Simulating Tool Offsets Part 1
Simulating Offsets

Part 1: What are Offsets?

When we write a CNC program, all co-ordinates used for describing the shape of the part are stated relative to a zero reference, called the part datum.

The part datum should be positioned in a convenient location with respect to the actual size of the billet you intend to use, as shown below.  This position will need to be identified later on the real billet.

In the sample CNC files used with this tutorial, the part datum is positioned in the top lefthand corner of the imaginary billet.

The CNC machine also has a zero reference, called the machine datum.  If no offsets are loaded, our CNC file will use this position as the start location for any machining co-ordinates.

Offsets are used to establish the location of the workpiece datum on the real billet.  The workpiece datum is the position where we want any physical machining co-ordinates to be taken from.  Using the Offsets facility, we can temporarily shift the entire co-ordinate based grid system of the CNC machine.  We must move the three dimensional grid, so the position of the workpiece datum registers as zero, rather than the position of the machine datum.

Note that the workpiece datum must be positioned on the real billet in the same place as the part datum datum was positioned with respect to the imaginary billet.  If these datums do not align, the part will be machined in the wrong place on the real billet.

Offsets are very important because without them, the CNC machine will not know where to begin cutting on the billet.  Offsets must always be configured before manufacturing our part.  However, once you configure and save an offset file, the same file may be used over and over again, as long as the following holds true:

- The same cutting tools are used.

- The billet size does not change.

- The fixture that holds the billet does not move position on the machine table.

Click here for more detailed information about Offsets


Tutorial: Starting the real CNC Machine Part 1
Starting a real CNC Machine

Part 1: Power-up Procedure

1) Ensure the RS232 lead is fitted securely between the computer and the CNC machine.

2) Switch on the CNC machine.

3) Power up the computer and start the VR CNC Turning software.

3) Before starting the real CNC Machine:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

Check that any tools present in a real Automatic Tool Changer, when fitted, match the exact position numbers of the tools configured in the software Automatic Tool Changer from the "Machine Tooling" window.

5) To start the real CNC Machine, click the [Machine] button, shown below, from the "Options" toolbar.

The "Machine Mode" window will open.  This window is used for controlling the movements of the real CNC machine using exactly the same principles as for the VR CNC machine described in the previous tutorial section.

For more information about how to configure your machine connection see Connecting to a real CNC Machine


Tutorial: Starting the real CNC Machine Part 2
Starting the real CNC Machine

Part 2: Using the sample CNC files with a real CNC Machine

Billet: Brass or Steel

Dimensions: X (Diameter) 25mm,  Z (Length) 55mm

Part Datum Position: Centre line of part and opposite the chuck end.

Tools required:

Tool 1 : General Roughing/Finishing Turning tool.

Tool 3 : Threading tool.

Put the billet into the chuck and tighten the jaws securely.


Tutorial: Starting to use a Virtual Reality CNC Machine Part 1
Starting to use a Virtual Reality CNC Machine

Part 1: Starting the Virtual reality CNC Machine

Before starting the Virtual reality CNC Machine:

Check that the units of measurement set for the VR CNC Turning software matches the units used in both the CNC file and any tooling profiles.  The units of measurement setting for the VR CNC Turning software is configured using the [Units] button on the "Options" toolbar.

Check that the tool numbers and tool profiles used in the "Machine Tooling" window match those used by your CNC file.

To start the Virtual Reality CNC Machine, click the [VR Machine] button, shown above, from the "Options" toolbar.

The "Denford Virtual Reality" window will open.  This window is used for viewing the 3D model of the VR CNC machine.  Any tools present in the "Machine Tooling" window (the Turret) will also be loaded, when applicable.

The "Control Panel" window will also open.  This window is used for controlling the movements of the VR CNC machine.

General Layout

The "Denford Virtual Reality" window is used to display a three dimensional representation of the CNC machine.  This VR CNC machine is driven and responds in exactly the same way as its real-life counterpart, making the VR Machine Mode ideal for offline CNC training.  In the example below, a Denford Triac VMC CNC Milling Machine is being controlled through virtual reality.

The "Denford Virtual Reality" window, shown above, is split into three basic areas:

The Viewbar (circled red) is the area of the window where preset viewpoints can be applied and the virtual reality world configured.

The Main Viewing Area, the largest area of the window, is where the objects and devices in the virtual worlds can be seen.

The Movebar (circled yellow) is the area of the window containing the controls for moving around the virtual world.


Tutorial: Starting to use a Virtual Reality CNC Machine Part 2
Starting to use a Virtual Reality CNC Machine

Part 2: Moving around the Virtual Reality World

The movebar tools allow you to freely 'fly' around the virtual world, using your mouse.  Try to think of the display in the Main Viewing Area as being the view from a floating camera head, which you can control using the three movement icons.  Each icon is used to control a different type of movement in the virtual world.

Using the Movebar to move around the Virtual Reality world

You can change the position of your viewpoint using the icons in the Movebar.

  :  Moves the viewpoint in the vertical plane.

  :  Moves the viewpoint in the horizontal plane, forwards, backwards and turning.

  :  Tilts the viewpoint up and down.

Click and hold the left mouse button on one of the three movement icons, then drag the mouse.  As you drag the mouse the icon indicates the direction you are moving, and the viewpoint moves in the corresponding direction.  The further you move the cursor from the icon, the faster you will move.  Release the mouse button to stop the movement.

Interactive Objects

Some objects on the VR CNC machines are interactive:

Right click on the guard handle to open the machine guard.

Left or right click on the Chuck to open/close the jaws.


Tutorial: Starting to use a Virtual Reality CNC Machine Part 3
Starting to use a Virtual Reality CNC Machine

Part 3: Using the Predefined Viewpoints

The viewbar is the area of the window where any of the preset viewpoints can be applied and the virtual reality world configured.

There are usually 6 available viewpoints:

Button [1]:  Looking at full machine.

Button [2]:  Looking at guard remove switch. (Some VR machines have a magic switch which will make the enclosure guarding disappear so you get a clear view of the insides of the machine).

Button [3]:  Looking at chuck and billet.

Button [4]:  Close up of turret.

Button [5]:  Close up of job.

Button [6]:  Overall view of machine.


Tutorial: Using Menubars and Toolbars Part 1
Using Menubars and Toolbars

Part 1: Toolbars

The various toolbars in the software can be repositioned to form different screen layouts, as required.

Note - Only toolbars can be docked and undocked.  Any windows appearing through use of the toolbar buttons can only be displayed in the main software window.

If you are unsure about the function of any toolbar button, hover your mouse cursor over the button to display a pop-up hint caption.

Docked Toolbar Example:

A docked toolbar can be positioned anywhere on the main software window docking bars.  Docking bars are provided on the top, lefthand and bottom grey border edges of the main software window.  To move a docked toolbar click and hold your left mouse button on the two grey lines at the end of the toolbar, circled red in the screenshot above.  Drag the toolbar to the new position and release the mouse button.  To undock a toolbar, drag it off the window docking bar into the main software window, then release the mouse button.

Undocked Toolbar Example:

An undocked toolbar can be positioned anywhere in the main software window.  To move an undocked toolbar click and hold your left mouse button on the toolbar titlebar, circled red in the screenshot above.  Drag the toolbar to the new position and release the mouse button.  To dock a toolbar drag and position it over one of the grey border edges of the main software window.


Tutorial: Using Menubars and Toolbars Part 3
Using Menubars and Toolbars

Part 2: Menubars

The VR CNC Turning software menubar, circled red in the screenshot above, is located under the main software title.  It contains text captions identifying each individual menu.

To display the options available in each menu, click the menu text title to display its dropdown list, as shown above, then move the mouse cursor down the list to highlight the options.  Click the highlighted option to select it or display its sub-menu, when available.

Context Sensitive Menus

The menus available will change according to the windows that are active in the software.

When the software is first started, the following menus are available:

File, Editor, Setup, Utilities, Windows, Help.

Additional Menus become available on selection of various software options:

Machine Tooling on selection of the [Tooling] button.

Tooling Library on selection of the [Tool Library] button.

2D Simulation on selection of the [2D Simulation] button.

3D Viewer on selection of the [3D Simulation] button.


Tutorial: Using the Automatic Tool Changer Carousel Part 1
Using the Tooling window 1 of 2

Part 1: Displaying the "Tooling" window

The "Machine Tooling" window allows different types of tool profile from the "Tooling Library" to be added to the numbered pockets in the Automatic Tool Changer carousel.

These tool numbers are used by any CNC files in the 2D or 3D Simulation windows and on the Virtual Reality CNC machines and real CNC machines.

To display the "Machine Tooling" window, click the [Tooling] button, shown above, from the "Options" toolbar.

General Layout

Each coloured number refers to a pocket on the Tool Changer (ie, Turret).  A greyed out number indicates that the pocket is empty. When a tool is transferred from the "Tooling Library" window to the carousel, the colour allocated to that tool from the "Tooling Library" window is also transferred.  These colours are applied to the different pocket numbers as they become filled.

A depressed number button indicates the tool data that is now been viewed and that which would be changed to if the'Change Tool' button was pressed. In the example above, tool number 3 - external threading tool is currently shown.

The Change Tool button causes the machine to the start tool change sequence (eg, Turret rotation) and is active under the following conditions:

1. VR or Real machine is connected and running

2. Control panel mode is Auto

3. The tool required is not already the currently active tool

The data panel in the centre of the window shows some of the tools' details. To see all the details click the small button marked >>.

To close the "Machine Tooling" window, click the [Tooling] button, from the "Options" toolbar.


Tutorial: Using the Automatic Tool Changer Carousel Part 2
Using the Tooling window 2 of 2

Part 2: Transferring Tools into the "Tooling" window

Tool profiles are transferred from the "Tooling Library" window into the "Machine Tooling" window, where they become available for use with any CNC files.

Deleting Tools from the "Tooling" window

Right click on the tool station that you wish to remove then select "Remove":

Click the right mouse button on the carousel pocket number of the tool you want to remove.  Highlight and click the "Remove Tool" option on the pop-up menu, then highlight and click on the title of the tool you want to add.  The selected tool will then be added to the specified carousel pocket number.

Adding Tools into the "Tooling" window

Click the right mouse button on the empty carousel pocket number in the "Tooling" window.  Highlight and click the "Insert Tool" option on the pop-up menu, then highlight and click on the title of the tool you want to add. Only tools that have not already been used from the tool library, will be available.

Drag and Dropping Tools into the "Tooling" window

In the "Tooling Library" window, click and hold down the left mouse button on the title of the tool you want to add to the carousel.  Whilst continuing to hold down the left mouse button, drag the tool across and into the "Tooling" window.  Position the cursor over the required empty turret number and release the left mouse button.  The selected tool will then be added to the specified carousel pocket number.


Tutorial: Using the Tool Library Part 1
Using the Tool Library	 1 of 2

Part 1: Displaying the "Tooling Library" window

The Tooling Library contains the list of tool profiles available for use in the Automatic Tool Changer (when fitted) and in the machine head.

To display the "Tooling Library" window, click the [Tool Library] button, shown above, from the "Options" toolbar.

General Layout

To highlight a tool profile, click on its title.  A graphic will be displayed in the left panel, relating to the type of tool selected.  Highlighted tool profiles are shown using white title text on a blue background.

Click here for a list of the default Tooling Library profiles available

To close the "Tooling Library" window, click the [Tool Library] button, from the "Options" toolbar.


Tutorial: Using the Tool Library Part 2
Using the Tool Library 2 of 2

Part 2: Viewing and Editing Tool Profile Data

Within the tool library, it is possible to change any of the parameters for each tool available (Simulation colour, tip size, angle etc . .)

You can also add or delete tools.

In the screenshot above, the tool called "Roughing Tool" has been changed into a Drill type tool. Click on the drop down menu under 'ToolType' to change to type of tool.

To alter data such as shank length simply click the small up/down arrows on the right of the edit box you wish to change. Alternatively, click inside the box and enter a new value

You will notice that this tool is previewed in the bottom left hand corner of the display.

It is currently pointing in the wrong direction. To remedy this, alter the Tool Orientation and Tip Orientation values by clicking on their drop down menus:

Tool definitions can be added, deleted or copied by right clicking in the tool list :

Note:  Any data changes made will also be applied to tools currently available in the machines Tooling window (ie, in the turret).


Use X,Y Offsets (2D)
"2D Simulation | Use Offsets"

This option is used to select whether any programmed X and Z offsets should be taken into account when displaying the 2D image.

When the "Use Offsets" option is active, the X and Z edit boxes will appear in the 2D simulation window (ringed in red). Use thes values to shift the default position of the billets datum. In the screenshot above, the datum has been moved 10mm away from the front of the billet in the Z axis.


Using the Menubars

The VR CNC Turning software menubar (circled red in the screenshot below) is located under the main software title.  It contains text captions identifying each individual menu.

To display the options available in each menu, click the menu text title to display its dropdown list (as shown below), then move the mouse cursor down the list to highlight the options.  Click the highlighted option to select it or display its sub-menu, when available.

The menus available will change according to the windows that are active in the software and which window is currently selected.

Additional Menus become available on selection of various software options:

Machine Tooling  on selection of the [Tooling] button.

Tooling Library  on selection of the [Tool Library] button.

2D Simulation  on selection of the [2D Simulation] button.

3D Viewer  on selection of the [3D Simulation] button.

Note: To make options appear on the main menubar, simply click on the window to select it and menubar options for that window will appear:

Note: The 3D simulation in this screenshot is selected - the top bar is blue, if it wasn't selected / highlighted then this bar would be greyed out.


Using the Toolbars

The various toolbars in the software can be repositioned to form different screen layouts, as required.

Docked Toolbar Example.

A docked toolbar can be positioned anywhere on the main software window docking bars.  Docking bars are provided on the top, lefthand and bottom grey border edges of the main software window.  To move a docked toolbar click and hold your left mouse button on the two grey lines at the end of the toolbar (circled red in the screenshot above).  Drag the toolbar to the new position and release the mouse button.  To undock a toolbar, drag it off the window docking bar into the main software window, then release the mouse button.

Undocked Toolbar Example.

An undocked toolbar can be positioned anywhere in the main software window.  To move an undocked toolbar click and hold your left mouse button on the toolbar titlebar (circled red in the screenshot above).  Drag the toolbar to the new position and release the mouse button.  To dock a toolbar drag and position it over one of the grey border edges of the main software window.

Note - Only toolbars can be docked and undocked.  Any windows appearing through use of the toolbar buttons can only be displayed in the main software window.

If you are unsure about the function of any toolbar button, hover your mouse cursor over the button to display a pop-up hint caption.


Using the Toolbars 2
Using the Toolbars

Toolbar buttons can be displayed in three different ways, according to the settings specified in the "Setup | Toolbars" menu:

Large format toolbar buttons (graphics and text), as shown below.

Small format toolbar buttons (graphics only), as shown below.

Small format toolbar buttons (text only), as shown below.

To alter how toolbars look, simply RIGHT click on the any button on the toolbar and select your option:

Undocked toolbars can be configured in horizontal and vertical positions, using the same method as resizing any program windows.  Click and hold down the left mouse button on the corner of a toolbar, then drag the ghosted image of the toolbar to the required position and release the left mouse button, as shown below.


block
A block is a single program line in the CNC file.


fnc
FNL:  FANUC Lathe file, extension '.fnl'.  Contains G and M codes describing the machine and cutting operations.


prj
TPR:  Denford CNC Turning Project file, extension '.tpr'.  Project files contain global information about user defined settings in the VR CNC Turning software, such as toolpost set-up, tooling library, offsets and program file etc.


txt
TXT:  Standard Windows text only file, extension '.txt'.


xnc
XNC:   Denford Compiled CNC file, extension '.xnc'.  A compiled file is a FANUC lathe file that is formatted to allow 3D elements such as the 3D Viewer to run as quickly as possible.  XNC files can also be used to drive an attached CNC machine when run through the VR CNC Turning software.


3D simulation setup
The 3D simulation setup window

This option is used to display the "3D Simulation Setup" window, shown above, used to configure the graphics shown in the "3D Simulation" window.

Checkboxes are used to show when the various options in this window are active.  When a tick mark is visible, the associated option is active.  To add or remove a tick mark in a checkbox, click the left mouse button on the required checkbox.

The top section allows you to configure the tool path colors and whether or not they are shown. To change color just click on the colored box associated with the movement type. eg, If you wished to show circular motion as blue, in the example above you would click the orange box next to Circular Movement Colour and choose blue from the colour picker window.

Move history is the number of moves (tool path lines) remembered and kept on the display. Note that arcs are drawn as small segments so one arc move may require a minumum history of 30.

Contouring points are small white ticks which will appear at the intersections between moves. They show that on a real machine that move would be contoured (ie, a smooth change from one move to the other will take place without pausing). Contouring is dependant upon machine parameters Feed -> Max Contour Feed and Max Contour angle. See Software Configuration

The middle section allows configuration of the window and billet color. Again if you wished to make the 3D window background color black, you would click on the color box next to Background Colour and select black from the colour picker. You can also select from a range of materials or plastic colours for your billet. Click either the Material type or the Plastic colour boxes to get a range of selections. Note, only one tick box can be selected as you must choose a material OR a plastic type colour.

The bottom section lets you specify the size, in pixels, of the .BM3 preview file which is automatically created every time a CNC program is run. It also specifies the size of any windows .BMP file which you can save with the Capture as Bitmap option under the 3D simulate menubar.

! Do not set the normal bitmap size too high as you will be creating large files every time you run a CNC program - if  Auto Save Bitmap is checked !

Click the [OK] button to save any changes or the [Cancel] button to discard any changes made to the options in the "3D Simulation Setup" window.


The 3D Simulation Window Page 4 of 4
The 3D Simulation Window Page 3 of 3

Measuring your finished Part

Once you have run a CNC program through, and the 3D billet model has been created, it is possible to measure diameters, lengths and angles of your part.

In this screenshot, the "Measure" button is pressed and an information box appears to its' right.

The Button has also been un-docked so that it can be positioned in a more suitable place.

Measuring probes also appear on the model, indicating which point on the surface you are 'measuring'.

Information box details

X: The current diameter as determined by the point of the measuring probes.

Z: The current Z dimension in relation to the front datum point.

L: The length of the item that is highlighted in a paler colour.

A: The angle of the item that is highlighted in a paler colour.

In the above example you can see that the probes are measuring the end diameter of the long tapered cut. Its diameter is 24mm; it ends 46.5mm from the front face of the billet (ie, Z datum point); the length of the taper (as highlighted) is 18.111mm and the angle of the taper is 6.34 degrees. (Where 0 degrees is parallel to the Z axis)

Moving the probes to a different part of the model

Press and hold the LEFT mouse button and move the mouse left or right.

Note: if the "Measure" button is pressed, you will still be able to Zoom and Pan the billet, but not rotate. Simply press the button again to turn Measure feature off.


Coordinate system display types
Co-ordinate System Display Types

The [Co ordinates] button is used to switch between the two systems used for displaying the co-ordinate positions.  The far right panel on the statusbar, at the bottom of the "Machine Mode" window, displays the current setting for this button.  When the [Units] of Measurement are set to "Inch" the co-ordinates are displayed using inches.  When the [Units] of Measurement are set to "Metric" the co-ordinates are displayed using millimetres.

Click here for more about the Theory behind Co-ordinate System Display Modes

Work Piece Co-ordinates System :  This system displays the co-ordinate position relative to the moveable workpiece datum.  When the Co-ordinate System Display Mode is set to Work Piece or Program display, the button graphic shows the X,Z symbol with a picture of the work piece (billet). The display panel shows the text "Program".

Machine Co-ordinates System:  This system displays the co-ordinate position relative to the fixed machine datum.  When the Co-ordinate System Display Mode is set to Machine, the button graphic shows the X, Z symbol with a picture of the chuck and turning tool.  The display panel shows the text "Machine".

Both Co-ordinates System:  This system displays both Machine values and Program as above. There is also a display of the 'distance to go' for each axis. When running a CNC program in automatic, this display shows how far the current move has got to go until it is complete.  The programmed and actual spindle speed is also shown. (Actual being the accurate chuck speed read from the machines encoder)


Use X,Y Offsets (3D)
This option is used to select whether any programmed X and Z offsets should be taken into account when displaying the 3D image.

When the "Use Offsets" option is active, the X and Z edit boxes will appear in the 3D simulation window (ringed in red). Use these values to shift the default position of the billets datum. In the screenshot above, the datum has been moved 10mm away from the front of the billet in the Z axis.


What is VR CNC Turning for Windows
What is VR CNC Turning for Windows?

VR CNC Turning is a Windows based software package allowing full editing and control of CNC files, either offline (away from the CNC machine) or online (controlling the operation of a CNC machine).

Information is accessed and displayed using an interface similar to other popular software applications.  The familiar dropdown menus, toolbars and software display windows can be configured to suit the level and requirements of each user.  Since the software supports full offline facilities, it allows many tasks such as setting tool offsets, to be carried out away from the CNC machine itself.  Options such as these allow groups of students to work simultaneously whilst helping to free valuable CNC machine resources.  The same interface is used online, allowing students to produce their designs without having to learn any new CNC machine control software.

Features available in the VR CNC Turning software package include:

Full CNC file editing.

2 Dimensional graphical simulation of CNC files.

3 Dimensional graphical simulation of CNC files.

Comprehensive Tooling features.

Full offline control of a CNC machine using Virtual Reality.

Full online control of a CNC machine.

Context sensitive online help, including help with G and M code Programming and CNC file structure.

Copyright © 2000 - Denford Limited - VR CNC Milling for Windows software helpfile - Version 1.1 - No part of this helpfile may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose, without the express written permission of Denford Limited.


What is Radius or Diameter Programming
CNC Theory: What is Radius or Diameter Programming?

The VR CNC Turning software is configurable for either radius programming or diameter programming.

To check what your current mode is look at the status bar on the bottom of the window:

This mode is configured via "Setup" - "Machine Parameters" and can differ per each machine configuration.

The software must be restarted if you re-configure this setting.

Diameter Programming means that all X values programmed are relative to the overall diameter of the billet.

This is the most common form of programming for a lathe because it is easier to understand whereabouts the tool is and what size you are cutting to.

This means that if your billet was 30mm diameter and you programmed X25 Z0 then X25 Z-100 you would turn your billet size down to 25mm diameter.

Radius Programming means that all X values programmed are relative to the radius of the part.

Radius programming is less common but can be used to make program creation easier if your dimensioned drawings show only the profile of the turned part - showing all dimensions as radius values.

Therefore, if you tried to turn your 30mm billet at a value of  X25, you would not cut the material at all. (X25 in radius programming

would mean cutting a diameter of 50mm !)

This diagram shows the difference between radius and diameter programming in a lathe:


Types of Offsets
CNC Theory: Types of Offset

1) Workpiece Offsets

A workpiece offsets file contains three values relating to any co-ordinate shift required along the direction of the X, Y and Z axes.

Without any workpiece offsets file loaded, the zero co-ordinate of the CNC machine is the location of the machine datum.

Workpiece offsets are used to temporarily shift the entire co-ordinate based grid system of the machine, setting a new location for the zero co-ordinate of the CNC machine.

Any values entered into a workpiece offsets file are global, ie, they are used by all tool profiles, irrespective of their different lengths.

2) Tool Offsets

Tool Length Offsets apply only to the particular tool you are currently using.

They allow a variety of tool profiles to be used together on the same CNC program, by offsetting their differences in position against a common fixed reference point. This common point is usually tool 1 which has X=0 Z=0 offset value.In this way, all other tools are described as the difference in position between tool 1 and the other tools.

When tool offsets are used, their values are combined with currently loaded workpiece offset, to calculate the X, Z co-ordinate describing the location of the workpiece datum.


What are Offsets?
CNC Therory: What are Offsets? Part 1

When we write a CNC program, all co-ordinates used for describing the shape of the part are stated relative to a zero reference, called the part datum.

The part datum should be positioned in a convenient location with respect to the actual size of the billet you intend to use, as shown below.  This position will need to be identified later on the real billet.

We recommend that the Z co-ordinate of the part datum is set to the front face of the part (opposite the chuck) and the X co-ordinate for each different tool is on the centre line of the chuck / billet.

In doing so, any negative Z values programmed will indicate that the tool is cutting into the billet, any positive Z values programmed will indicate that the tool is clear from the billet. Any X values then programmed would either signify the diameter or the radius of the cutting path.

However, the part datum can be positioned anywhere.  It could be positioned in one of the corners of a part design drawing or with the chuck face being Z zero. In most CAD/CAM software packages it may be set automatically when the CNC program is generated.

The CNC machine also has a zero reference, called the machine datum.  If no offsets are loaded, our CNC program will use this position as the start location for any machining co-ordinates. This position is usually the same as the Home position.

WorkPiece offsets define roughly where the billet datum is.

Tool offsets define where this datum is exactly, for each tool that we are using.

For example,

Tool 1 could be used to turn and face the part. We could then measure the part and set the Workpiece offsets for X and Z. Doing this would mean that the Tool offset for Tool 1 would not require setting and their values should be zero. Then we could select Tool 3 and touch onto the billet to find the datum position for this tool and only need to set the Tool offset values. Normally each tool in a turret would not have greatly varying offsets, however the tool offset value for an internal tool such as a drill will vary considerably to a standard external roughing tool.

It is important to note that the physical position of the machine datum does not move, since it is permanently fixed.  Remember, it's the co-ordinate based grid system of the CNC machine that temporarily moves, giving the illusion that the machine datum itself has moved.

Note that the workpiece datum must be positioned on the real billet in the same place as the part datum datum was positioned with respect to the imaginary billet in 2D or 3D simulations.

What are Offsets? Part 2 >>


What are Offsets? part2
CNC Therory: What are Offsets? Part 2

The concept of Home postion, Workpiece offsets and Tool offsets is shown below:

However, the part datum can be positioned anywhere.  It could be positioned in one of the corners of a part design drawing or with the chuck face being Z zero. In most CAD/CAM software packages it may be set automatically when the CNC program is generated.

The CNC machine also has a zero reference, called the machine datum.  If no offsets are loaded, our CNC program will use this position as the start location for any machining co-ordinates. This position is usually the same as the Home position.

WorkPiece offsets define roughly where the billet datum is.

Tool offsets define where this datum is exactly, for each tool that we are using.

For example,

Tool 1 could be used to turn and face the part. We could then measure the part and set the Workpiece offsets for X and Z. Doing this would mean that the Tool offset for Tool 1 would not require setting and their values should be zero. Then we could select Tool 3 and touch onto the billet to find the datum position for this tool and only need to set the Tool offset values. Normally each tool in a turret would not have greatly varying offsets, however the tool offset value for an internal tool such as a drill will vary considerably to a standard external roughing tool.

It is important to note that the physical position of the machine datum does not move, since it is permanently fixed.  Remember, it's the co-ordinate based grid system of the CNC machine that temporarily moves, giving the illusion that the machine datum itself has moved.

Note that the workpiece datum must be positioned on the real billet in the same place as the part datum datum was positioned with respect to the imaginary billet in 2D or 3D simulations.


Tool offsets window
The Tool Offsets Window

Also See Machine Tooling Window

Working with the list of Tool Offsets

The screenshot above shows the automatic datum buttons (highlighted in RED) which become available when you are connected to a VR or Real machine.

Pressing X or Z auto-datum button will bring up the menu 'X offset' or 'Z offset'.

In the screenshot above, the yellow highlight shows the current billet size as programmed (80mm). When 'Include Diameter' is selected, then this value is taken into account when you press OK to set your workpiece offset. In this example, pressing OK will enter a number into the X value for offset 1 which cause the current Program position readout to read X 80.000

So, the current position of the current tool is now set to X 80.000

If the "Use origin only" option was selected, then the readout would be X 0.000

Remember, that any tool can have any tool offset associated with it. So, Tool 1 could use offsets 1, 2, 3 ,4 etc.. To activate an offset for with a different number to the tool number, click on the offsets value box, change it and then click another box. You will then be asked if you want to 'activate offset ?? for tool ??'.

Note: Setting Tool offsets will take into account the currently active Workpiece offset - be sure to set you workpiece offsets first.

Related Topics:

The Theory of Offsets

Coordinate system display types

Workpiece offset setting