Override control knobs for feed rate/spindle speed
100
1
50
50
S %
0
100
1
50
50
F %
0
Mode of operation
Manual Operation
Decimal point
Change arithmetic sign
Confirm entry and resume dialog
End block
Clear numerical entry or TNC error message
Abort dialog, delete program section
Programming aids
MOD functions
HELP function
Moving the cursor, going directly to blocks, cycles and
parameter functions
Move highlight
Move highlight, skip dialog question
Select blocks and cycles directly
Positioning with Manual Data Input (MDI)
Program Run/Test Run
Programming and Editing
TNC Models, Software and
Features
This manual describes functions and features provided by
the TNCs with the following NC software numbers.
TNC ModelNC Software No.
TNC 310286 140-xx
TNC 310 M286 160-xx
The machine tool builder adapts the useable features of the
TNC to his machine by setting machine parameters. Some
of the functions described in this manual may not be
among the features provided by the TNC on your machine
tool.
TNC functions that may not be available on your machine
include:
■ Probing function for the 3-D touch probe
■ Rigid tapping cycle
■ Boring cycle
■ Back boring cycle
Please contact your machine tool builder to become familiar
with the individual implementation of the control on your
machine.
Many machine manufacturers, as well as HEIDENHAIN,
offer programming courses for the TNCs. We recommend
these courses as an effective way of improving your
programming skill and sharing information and ideas with
other TNC users.
Contents
Location of use
The TNC complies with the limits for a Class A device in
accordance with the specifications in EN 55022, and is
intended for use primarily in industrially-zoned areas.
IHEIDENHAIN TNC 310
Contents
Introduction
1
Manual Operation and Setup
Positioning with Manual Data Input (MDI)
Programming: Fundamentals, File
Management, Programming Aids
Programming: Tools
Programming: Programming Contours
Programming: Miscellaneous Functions
Programming: Cycles
Programming: Subprograms and
Program Section Repeats
Programming: Q Parameters
Test Run and Program Run
3-D Touch Probes
2
Contents
3
4
5
6
7
8
9
10
11
12
MOD Functions
Tables and Overviews
13
14
IIIHEIDENHAIN TNC 310
1 INTRODUCTION.....1
1.1 The TNC 310.....2
1.2 Visual Display Unit and Keyboard.....3
Contents
1.3 Modes of Operation.....4
1.4 Status Displays.....7
1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels.....11
2 MANUAL OPERATION AND SETUP.....13
2.1 Switch-On.....14
2.2 Moving the Machine Axes.....15
2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M.....18
2.4 Datum Setting (Without a 3-D Touch Probe).....19
3 POSITIONING WITH MANUAL DATA INPUT (MDI).....21
3.1 Programming and Executing Simple Positioning Blocks .....22
4 PROGRAMMING: FUNDAMENTALS OF NC, FILE MANAGEMENT, PROGRAMMING AIDS.....25
4.1 Fundamentals of NC.....26
4.2 File management.....31
4.3 Creating and Writing Programs.....34
4.4 Interactive Programming Graphics.....39
4.5 HELP function.....41
5 PROGRAMMING: TOOLS.....43
5.1 Entering Tool-Related Data.....44
5.2 Tool Data.....45
5.3 Tool Compensation.....51
IV
Contents
6 PROGRAMMING: PROGRAMMING CONTOURS.....55
6.1 Overview of Tool Movements.....56
6.2 Fundamentals of Path Functions.....57
6.3 Contour Approach and Departure.....60
Overview: Types of paths for contour approach and departure.....60
Important positions for approach and departure.....60
Approaching on a straight line with tangential connection: APPR LT.....62
Approaching on a straight line perpendicular to the first contour point: APPR LN.....62
Approaching on a circular arc with tangential connection: APPR CT.....63
Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT.....64
Departing tangentially on a straight line: DEP LT.....65
Departing on a straight line perpendicular to the last contour point: DEP LN.....65
Departing tangentially on a circular arc: DEP CT.....66
Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT.....67
6.4 Path Contours — Cartesian Coordinates.....68
Overview of path functions.....68
Straight line L.....69
Inserting a chamfer CHF between two straight lines.....69
Circle center CC.....70
Circular path C around circle center CC.....71
Circular path CR with defined radius.....72
Circular path CT with tangential connection.....73
Corner Rounding RND.....74
Example: Linear movements and chamfers with Cartesian coordinates.....75
Example: Circular movements with Cartesian coordinates.....76
Example: Full circle with Cartesian coordinates.....77
6.5 Path Contours—Polar Coordinates.....78
Polar coordinate origin: Pole CC.....78
Straight line LP.....79
Circular path CP around pole CC.....79
Circular path CTP with tangential connection.....80
Helical interpolation.....81
Example: Linear movement with polar coordinates .....83
Example: Helix .....84
Contents
VHEIDENHAIN TNC 310
7 PROGRAMMING: MISCELLANEOUS FUNCTIONS.....85
7.1 Entering Miscellaneous Functions M and STOP.....86
7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant.....87
Contents
7.3 Miscellaneous Functions for Coordinate Data.....87
7.4 Miscellaneous Functions for Contouring Behavior.....89
7.5 Miscellaneous Function for Rotary Axes.....92
8 PROGRAMMING: CYCLES.....93
8.1 General Overview of Cycles.....94
8.2 Drilling Cycles.....96
PECKING (Cycle 1).....96
DRILLING (Cycle 200).....98
REAMING (Cycle 201).....99
BORING (Cycle 202).....100
UNIVERSAL DRILLING (Cycle 203).....101
BACK BORING (Cycle 204).....103
TAPPING with a floating tap holder (Cycle 2).....105
RIGID TAPPING (Cycle 17).....106
Example: Drilling cycles.....107
Example: Drilling cycles .....108
8.3 Cycles for Milling Pockets, Studs and Slots.....109
POCKET MILLING (Cycle 4).....110
POCKET FINISHING (Cycle 212).....111
STUD FINISHING (Cycle 213).....113
CIRCULAR POCKET MILLING (Cycle 5).....114
CIRCULAR POCKET FINISHING (Cycle 214).....116
CIRCULAR STUD FINISHING (Cycle 215) .....117
SLOT MILLING (Cycle 3).....119
SLOT with reciprocating plunge-cut (Cycle 210).....120
CIRCULAR SLOT with reciprocating plunge-cut (Cycle 211) .....122
Example: Milling pockets, studs and slots.....124
VI
Contents
8.4 Cycles for Machining Hole Patterns.....126
CIRCULAR PATTERN (Cycle 220).....127
LINEAR PATTERN (Cycle 221) .....128
Example: Circular hole patterns.....130
8.5 Cycles for multipass milling.....132
MULTIPASS MILLING (Cycle 230).....132
RULED SURFACE (Cycle 231).....134
Example: Multipass milling.....136
8.6 Coordinate Transformation Cycles .....137
DATUM SHIFT (Cycle 7).....138
DATUM SHIFT with datum tables (Cycle 7).....138
MIRROR IMAGE (Cycle 8).....140
ROTATION (Cycle 10).....141
SCALING FACTOR (Cycle 11) .....142
Example: Coordinate transformation cycles.....143
8.7 Special Cycles .....145
DWELL TIME (Cycle 9) .....145
PROGRAM CALL (Cycle 12).....145
ORIENTED SPINDLE STOP (Cycle 13) .....146
Contents
9 PROGRAMMING: SUBPROGRAMS AND PROGRAM SECTION REPEATS.....147
9.1 Labeling Subprograms and Program Section Repeats.....148
9.2 Subprograms.....148
9.3 Program Section Repeats.....149
9.4 Nesting.....151
Subprogram within a subprogram .....151
Repeating program section repeats.....152
Repeating a subprogram.....153
Example: Milling a contour in several infeeds .....154
Example: Groups of holes .....155
Example: Groups of holes with several tools .....156
VIIHEIDENHAIN TNC 310
10 PROGRAMMING: Q PARAMETERS.....159
10.1 Principle and Overview.....160
10.2 Part Families — Q Parameters in Place of Numerical Values.....161
Contents
10.3 Describing Contours through Mathematical Operations.....162
10.4 Trigonometric Functions .....164
10.5 If-Then Decisions with Q Parameters .....165
10.6 Checking and Changing Q Parameters .....166
10.7 Additional Functions .....167
10.8 Entering Formulas Directly.....173
10.9 Preassigned Q Parameters.....176
10.10 Programming Examples.....178
Example: Ellipse.....178
Example: Concave cylinder machined with spherical cutter .....180
Example: Convex sphere machined with end mill .....182
12.1 Touch Probe Cycles in the Manual Operation Mode.....202
Calibrating a touch trigger probe.....203
Compensating workpiece misalignment.....204
12.2 Setting the Datum with a 3-D Touch Probe.....205
12.3 Measuring Workpieces with a 3-D Touch Probe.....208
VIII
Contents
13 MOD FUNCTIONS.....211
13.1 Selecting, Changing and Exiting the MOD Functions.....212
13.2 System Information.....212
13.3 Entering the Code Number.....213
13.4 Setting the Data Interface.....213
13.5 Machine-Specific User Parameters.....216
13.6 Position Display Types.....216
13.7 Unit of Measurement.....216
13.8 Axis Traverse Limits .....217
13.9 Running the HELP File.....218
14 TABLES AND OVERVIEWS.....219
14.1 General User Parameters.....220
Input possibilities for machine parameters.....220
Selecting general user parameters.....220
External data transfer.....221
3-D Touch Probes.....222
TNC displays, TNC editor.....222
Machining and program run.....224
Electronic handwheels.....225
14.2 Pin Layout and Connecting Cable for the Data Interface.....226
RS-232-C/V.24 Interface .....226
14.3 Technical Information.....227
TNC features.....227
Programmable functions.....228
TNC Specifications.....228
14.4 TNC Error Messages.....229
TNC error messages during programming.....229
TNC error messages during test run and program run.....229
14.5 Exchanging the Buffer Battery.....232
Contents
IXHEIDENHAIN TNC 310
Introduction
1
1.1The TNC 310
HEIDENHAIN TNC controls are shop-floor programmable
contouring controls for milling, drilling and boring machines.
You can program conventional milling, drilling and boring operations
right at the machine with the easily understandable interactive
conversational guidance. The TNC 310 can control up to 4 axes.
Instead of the fourth axis, you can also change the angular position
of the spindle under program control.
1.1 The TNC 310
Keyboard and screen layout are clearly arranged in a such way that
the functions are fast and easy to use.
Programming: HEIDENHAIN conversational format
HEIDENHAIN conversational programming is an especially easy
method of writing programs. Interactive graphics illustrate the
individual machining steps for programming the contour. Workpiece
machining can be graphically simulated during test run.
You can enter a program while the control is running another.
Compatibility
The TNC can execute all part programs that were written on
HEIDENHAIN controls TNC 150 B and later.
In addition, the TNC can also run programs with functions that
cannot be programmed directly on the TNC 310 itself, such as:
■ FK free contour programming
■ Contour cycles
■ ISO programs
■ Program call with PGM CALL
2
1 Introduction
1.2Visual Display Unit and Keyboard
Visual display unit
The figure at right shows the keys and controls on the VDU:
Setting the screen layout
Soft key selector keys
Switching the soft-key rows
Header
When the TNC is on, the selected operating mode is shown in
the screen header. Dialog prompts and TNC messages also
appear here (unless the TNC is showing only graphics).
Soft keys
In the right margin the TNC indicates additional functions in a softkey row. You can select these functions by pressing the keys
immediately beside them
are rectangular boxes indicating the number of soft-key rows.
These rows can be called with the
box representing the active soft-key row is filled in.
Screen layout
You select the screen layout yourself: In the PROGRAMMING AND
EDITING mode of operation, for example, you can have the TNC
show program blocks in the left window while the right window
displays programming graphics. You could also display help
graphics for cycle definition in the right window instead, or display
only program blocks in one large window. The available screen
windows depend on the selected operating mode.
. Directly beneath the soft-key row
outside right and left. The
1.2 Visual Display Unit and Keyboard
To change the screen layout:
Press the SPLIT SCREEN key: The soft-key row
shows the available layout options.
<
Select the desired screen layout.
3HEIDENHAIN TNC 310
Keyboard
The figure at right shows the keys of the keyboard grouped
according to their functions:
MOD function,
HELP function
Numerical input
Dialog buttons
Arrow keys and GOTO jump command
Modes of Operation
Machine control buttons
Override control knobs for feed rate/spindle speed
1.3 Modes of Operation
The functions of the individual keys are described in the foldout of
the front cover. The exact functioning of the machine control
buttons, e.g. NC START, is described in more detail in your Machine
Manual.
1.3Modes of Operation
The TNC offers the following modes of operation for the various
functions and working steps that you need to machine a workpiece:
Manual Operation and Electronic Handwheel
The Manual Operation mode is required for setting up the machine
tool. In this operating mode, you can position the machine axes
manually or by increments. Datums can be set by the usual
scratching method or by using the TS 220 triggering touch probe.
The TNC also supports the manual traverse of the machine axes
using a HR electronic handwheel.
Soft keys for selecting the screen layout
Screen windowsSoft key
Positions
Left: positions, right: general
program information
The operating mode Positioning with Manual Data Input is
particularly convenient for simple machining operations or prepositioning of the tool. You can write the a short program in
HEIDENHAIN conversational programming and execute it
immediately. You can also call TNC cycles. The program is stored in
the file $MDI. In the operating mode Positioning with MDI, the
additional status displays can also be activated.
Soft keys for selecting the screen layout
Screen windowsSoft key
Program
Left: program blocks, right: general
program information
Left: program blocks, right: positions and
Coordinates
Left: program blocks, right: tool
tools
Left: program blocks, right: coordinate
transformations
Left: program blocks, right: help graphics for
cycle programming (2nd soft-key level)
Programming and Editing
In this mode of operation you can write your part programs. The
various cycles help you with programming and add necessary
information. If desired, you can have the programming graphics
show the individual steps.
Soft keys for selecting the screen layout
1.3 Modes of Operation
Screen windowsSoft key
Program
Left: program blocks, right: help graphics for
cycle programming
Left: program blocks, right: programming graphics
Interactive Programming Graphics
5HEIDENHAIN TNC 310
Test run
In the Test Run mode of operation, the TNC checks programs and
program sections for errors, such as geometrical incompatibilities,
missing or incorrect data within the program or violations of the
work space. This simulation is supported graphically in different
display modes. Use a soft key to activate the test run in the Program Run operating mode.
Soft keys for selecting the screen layout
Screen windowsSoft key
Program
n Test run graphics
1.3 Modes of Operation
Left: program blocks, right: general
program information
Left: program blocks, right: positions and
Coordinates
Left: program blocks, right: tool
tools
Left: program blocks, right: coordinate
transformations
6
1 Introduction
Program Run/Single Block and
Program Run/Full Sequence
In the Program Run, Full Sequence mode of operation the TNC
executes a part program continuously to its end or to a manual or
programmed stop. You can resume program run after an
interruption.
In the Program Run, Single Block mode of operation you execute
each block separately by pressing the NC START button.
Soft keys for selecting the screen layout
Screen windowsSoft key
Program
Left: program blocks, right: general
program information
Left: program blocks, right: positions and
Coordinates
Left: program blocks, right: tool
tools
Left: program blocks, right: coordinate
transformations
1.4 Status Displays
1.4Status Displays
“General” status display
The status display informs you of the current state of the machine
tool. It is displayed automatically in all modes of operation:
In the operating modes Manual Operation and Electronic
Handwheel and Positioning with MDI the status display appears in
the large window
.
7HEIDENHAIN TNC 310
Information in the status display
TheMeaning
ACTL.Actual or nominal coordinates of the current position
X Y ZMachine axes
S F M Spindle speed S, feed rate F and active M functions
1.4 Status Displays
ROTAxes are moving
Program run started
Axis locked
plain
Additional status displays
The additional status displays contain detailed information on the
program run. They can be called in all operating modes, except in
the Manual Operation mode.
To switch on the additional status display:
Call the soft-key row for screen layout.
<
Select the layout option for the additional status
display, e.g. positions and coordinates.
You can also choose between the following additional status
displays:
81 Introduction
General program information
Name of main program / Active block number
Program called via Cycle 12
Active machining cycle
Circle center CC (pole)
Dwell time counter
Number of the active subprogram or active program section
repeats/
Counter for current program section repeat
(5/3: 5 repetitions programmed, 3 remaining to be run)
Operating time
Positions and coordinates
Name of main program / Active block number
Position display
Type of position display, e.g. distance-to-go
Angle of a basic rotation
1.4 Status Displays
9HEIDENHAIN TNC 310
Information on tools
T: Tool number
Tool axis
Tool length and radius
Oversizes (delta values) from TOOL CALL block
1.4 Status Displays
Coordinate transformations
Name of main program / Active block number
Active datum shift (Cycle 7)
Active rotation angle (Cycle 10)
Mirrored axes (Cycle 8)
Active scaling factor (Cycle 11)
For further information, refer to section 8.6 “Coordinate Transformation Cycles.”
10
1 Introduction
1.5Accessories: HEIDENHAIN 3-D
Touch Probes and Electronic
Handwheels
3-D Touch Probes
With the various HEIDENHAIN 3-D touch probe systems you can:
■ Automatically align workpieces
■ Quickly and precisely set datums
TS 220 touch trigger probe
This touch probe is particularly effective for automatic workpiece
alignment, datum setting and workpiece measurement. The TS 220
transmits the triggering signals to the TNC via cable.
Principle of operation: HEIDENHAIN triggering touch probes feature
a wear resisting optical switch that generates an electrical signal as
soon as the stylus is deflected. This signal is transmitted to the
TNC, which stores the current position of the stylus as an actual
value.
HR electronic handwheels
Electronic handwheels facilitate moving the axis slides precisely by
hand. A wide range of traverses per handwheel revolution is
available. Apart from the HR 130 and HR 150 integral handwheels,
HEIDENHAIN also offers the HR 410 portable handwheel.
1.5 Accessories: HEIDENHAIN 3-D Touch Probe and Electronic Handwheels
11HEIDENHAIN TNC 310
2
Manual Operation and Setup
2.1Switch-On
Switch-on and traversing the reference points can vary
depending on the individual machine tool. Your machine
manual provides more detailed information.
ú Switch on the power supply for control and machine.
2.1 Switch-On
The TNC automatically initiates the following dialog
Memory test
<
The TNC memory is automatically checked.
Power interrupted
<
TNC message that the power was interrupted
— clear the message.
TRANSLATE PLC program
<
The PLC program of the TNC is automatically compiled.
Relay Ext. DC Voltage Missing
<
Switch on the control voltage.
The TNC checks the functioning of the
EMERGENCY STOP circuit.
Traverse Reference Points
<
Cross the reference points in any sequence:
Press and hold the machine axis direction
button for each axis until the reference point has
been traversed, or
Cross the reference points with several axes at
the same time: Use soft keys to select the axes
(axes are then shown highlighted on the
screen), and then press the NC START button.
The TNC is now ready for operation in the
Manual Operation mode.
14
2 Manual Operation and Setup
2.2Moving the Machine Axes
Traversing the machine axes with the axis direction keys
is a machine-dependent function. Refer to your machine
tool manual.
Traverse the axis with the axis direction keys
Select the Manual Operation mode.
<
Press the axis direction button and hold it as
long as you wish the axis to move.
...or move the axis continuously:
and Press and hold the axis direction button, then
press the NC START button: The axis continues
to move after you release the keys.
2.2 Moving the Machine Axes
Press the NC STOP key to stop the axis.
You can move several axes at a time with these two methods.
15HEIDENHAIN TNC 310
Traversing with the HR 410 electronic handwheel
The portable HR 410 handwheel is equipped with two permissive
buttons. The permissive buttons are located below the star grip.
You can only move the machine axes when an permissive button is
depressed (machine-dependent function).
The HR 410 handwheel features the following operating elements:
EMERGENCY STOP
Handwheel
Permissive buttons
Axis address keys
Actual-position-capture key
Keys for defining the feed rate (slow, medium, fast; the feed rates
are set by the machine tool builder)
Direction in which the TNC moves the selected axis
2.2 Moving the Machine Axes
Machine function
(set by the machine tool builder)
The red indicators show the axis and feed rate you have selected.
To move an axis:
Select the Manual Operation mode.
<
Activate handwheel, set soft key to ON
<
Press the permissive button.
<
Select the axis on the handwheel
<
Select the feed rate.
<
orMove the active axis in the positive or negative
direction.
16
2 Manual Operation and Setup
16
X
Z
8
8
8
Incremental jog positioning
With incremental jog positioning you can move a machine axis by a
preset distance each time you press the corresponding axis
direction button.
Select the Manual Operation mode.
<
Select incremental jog positioning, set the soft
key to ON
JOG INCREMENT?
<
Enter the jog increment in millimeters
(here, 8 mm).
Select the jog increment via soft key (select 2nd
or 3rd soft-key row)
<
Press the axis direction button to position as
often as desired
2.2 Moving the Machine Axes
17HEIDENHAIN TNC 310
2.3Spindle Speed S, Feed Rate F and
Miscellaneous Functions M
In the Manual Operation mode, enter the spindle speed S and the
miscellaneous function M using soft keys. The miscellaneous
functions are described in Chapter 7 ”Programming: Miscellaneous
Functions.” The feed rate is defined in a machine parameter and can
be changed only with the override knobs (see next page).
Entering values
Example: Entering the spindle speed S
To enter the spindle speed, press the S soft key.
SPINDLE SPEED S=
<
1000Enter the desired spindle speed,
and confirm with the NC START button
The spindle speed S with the entered rpm is started with a
miscellaneous function.
Proceed in the same way to enter the miscellaneous functions M.
Changing the spindle speed and feed rate
With the override knobs you can vary the spindle speed S and feed
rate F from 0% to 150% of the set value.
The knob for spindle speed override is effective only on
machines with an infinitely variable spindle drive.
The machine tool builder determines which
miscellaneous functions M are available on your TNC and
what effects they have.
2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M
182 Manual Operation and Setup
2.4Datum Setting
(Without a 3-D Touch Probe)
You fix a datum by setting the TNC position display to the
coordinates of a known position on the workpiece.
Preparation
ú Clamp and align the workpiece.
ú Insert the zero tool with known radius into the spindle.
ú Ensure that the TNC is showing the actual position values.
Y
Z
X
Y
X
Datum setting
Fragile workpiece? If the workpiece surface must not be scratched,
you can lay a metal shim of know thickness
tool axis datum value that is larger than the desired datum by the
d
.
value
Select the Manual Operation mode.
<
Move the tool slowly until it touches the
workpiece surface.
<
Select the function for setting the datum
<
Select the axis.
DATUM SET Z=
<
Zero tool in spindle axis: Set the display to a
known workpiece position (here, 0) or enter the
d
thickness
the tool radius.
of the shim. In the tool axis, offset
d
on it. Then enter a
2.4 Setting the Datum
Repeat the process for the remaining axes.
If you are using a preset tool, set the display of the tool axis to the
length L of the tool or enter the sum Z=L+d.
19HEIDENHAIN TNC 310
3
Positioning with Manual Data
Input (MDI)
3.1Programming and Executing Simple Positioning Blocks
The operating mode Positioning with Manual Data Input is
particularly convenient for simple machining operations or prepositioning of the tool. You can write the a short program in
HEIDENHAIN conversational programming and execute it
immediately. You can also call TNC cycles. The program is stored in
the file $MDI. In the operating mode Positioning with MDI, the
additional status displays can also be activated.
Select the Positioning with MDI mode of
operation. Program the file $MDI as you wish.
To start program run, press the machine START
button.
Limitations:
The following functions are not available:
- Tool radius compensation
- Programming graphics
- Programmable probing functions
- Subprograms, program section repeats
- Path functions CT, CR, RND and CHF
- Cycle 12 PGM CALL
Z
Y
Example 1
A hole with a depth of 20 mm is to be drilled into a single
workpiece. After clamping and aligning the workpiece and setting
the datum, you can program and execute the drilling operation in a
few lines.
3.1 Programming and Executing Simple Positioning Blocks
First you pre-position the tool in L blocks (straight-line blocks) to the
hole center coordinates at a setup clearance of 5 mm above the
workpiece surface. Then drill the hole with Cycle 1 PECKING.
0 BEGIN PGM $MDI MM
1 TOOL DEF 1 L+0 R+5
2 TOOL CALL 1 Z S2000
3 L Z+200 R0 FMAX
4 L X+50 Y+50 R0 FMAX M3
22
50
50
Define tool: zero tool, radius 5
Call tool: tool axis Z
Spindle speed 2000 rpm
Retract tool (FMAX = rapid traverse)
Pos. tool aboveholeatFMAX , spindle On
3 Positioning with Manual Data Input (MDI)
X
5 L Z+5 F2000
6 CYCL DEF 1.0 PECKING
7 CYCL DEF 1.1 SET UP 5
8 CYCL DEF 1.2 DEPTH -20
9 CYCL DEF 1.3 PECKG 10
10 CYCL DEF 1.4 DWELL 0.5
11 CYCL DEF 1.5 F250
12 CYCL CALL
13 L Z+200 R0 FMAX M2
14 END PGM $MDI MM
The straight-line function is described in section 6.4 “Path Contours
— Cartesian Coordinates,” the PECKING cycle in section 8.3 “Dril-
ling Cycles.”
Position tool to 5 mm above hole
Define PECKING cycle:
Setup clearance of the tool above the hole
Total hole depth (Algebraic sign=working direction)
Depth of each infeed before retraction
Dwell time in seconds at the hole bottom
Feed rate for pecking
Call PECKING cycle
Retract tool
End of program
3.1 Programming and Executing Simple Positioning Blocks
23HEIDENHAIN TNC 310
Protecting and erasing programs in $MDI
The $MDI file is generally intended for short programs that are only
needed temporarily. Nevertheless, you can store a program, if
necessary, by proceeding as described below:
Select operating mode: Programming
and Editing
<
Call up the file manager: PGM NAME soft key
<
Move the highlight to the $MDI file.
<
Select „Copy file“: Press the COPY soft key
Target file =
<
1225Enter the name under which you want to save
the current contents of the $MDI file.
<
Copy the file.
<
Exit the file manager: END key
Erasing the contents of the $MDI file is done in a similar way:
Instead of copying the contents, however, you erase them with the
DELETE soft key. The next time you select the operating mode
Positioning with MDI, the TNC will display an empty $MDI file.
3.1 Programming and Executing Simple Positioning Blocks
For further information, refer to section 4.2 “File Management.”
243 Positioning with Manual Data Input (MDI)
4
Programming:
Fundamentals of NC,
File Management,
Programming Aids
4.1Fundamentals of NC
Position encoders and reference marks
The machine axes are equipped with position encoders that
register the positions of the machine table or tool. When a machine
axis moves, the corresponding position encoder generates an
electrical signal. The TNC evaluates this signal and calculates the
precise actual position of the machine axis.
If there is an interruption of power, the calculated position will no
longer correspond to the actual position of the machine slide. The
CNC can re-establish this relationship with the aid of reference
marks when power is returned. The scales of the position encoders
contain one or more reference marks that transmit a signal to the
TNC when they are crossed over. From the signal the TNC identifies
4.1 Fundamentals of NC
that position as the machine-axis reference point and can reestablish the assignment of displayed positions to machine axis
positions.
Linear encoders are generally used for linear axes. Rotary tables
and tilt axes have angle encoders. If the position encoders feature
distance-coded reference marks, you only need to move each axis a
maximum of 20 mm (0.8 in.) for linear encoders, and 20° for angle
encoders, to re-establish the assignment of the displayed positions
to machine axis positions.
Z
Y
X
X
MP
X (Z,Y)
26
4 Programming: Fundamentals of NC, File Management, Programming Aids
Reference system
A reference system is required to define positions in a plane or in
space. The position data are always referenced to a predetermined
point and are described through coordinates.
The Cartesian coordinate system (a rectangular coordinate system)
is based on three coordinate axes X, Y and Z. The axes are mutually
perpendicular and intersect at one point called the datum. A
coordinate identifies the distance from the datum in one of these
directions. A position in a plane is thus described through two
coordinates, and a position in space through three coordinates.
Coordinates that are referenced to the datum are referred
to as absolute coordinates. Relative coordinates are referenced to
any other known position (datum) you define within the coordinate
system. Relative coordinate values are also referred to as
incremental coordinate values.
Reference systems on milling machines
When using a milling machine, you orient tool movements to the
Cartesian coordinate system. The illustration at right shows how
the Cartesian coordinate system describes the machine axes. The
figure at right illustrates the “right-hand rule” for remembering the
three axis directions: the middle finger is pointing in the positive
direction of the tool axis from the workpiece toward the tool (the Z
axis), the thumb is pointing in the positive X direction, and the index
finger in the positive Y direction.
The TNC 310 can control up to 4 axes. The axes U, V and W are
secondary linear axes parallel to the main axes X, Y and Z,
respectively. Rotary axes are designated as A, B and C. The
illustration shows the assignment of secondary axes and rotary
axes to the main axes.
+Y
Z
Y
X
4.1 Fundamentals of NC
+Z
+Y
+X
+Z
+X
V+
Z
Y
W+
C+
B+
A+
X
U+
27HEIDENHAIN TNC 310
Polar coordinates
If the production drawing is dimensioned in Cartesian coordinates,
you also write the part program using Cartesian coordinates.
For parts containing circular arcs or angles it is often simpler to give
the dimensions in polar coordinates.
While the Cartesian coordinates X, Y and Z are three-dimensional
and can describe points in space, polar coordinates are twodimensional and describe points in a plane. Polar coordinates have
their datum at a circle center (CC), or pole. A position in a plane can
be clearly defined by the
■ Polar Radius, the distance from the circle center CC to the
position, and the
■ Polar Angle, the size of the angle between the reference axis and
the line that connects the circle center CC with the position.
4.1 Fundamentals of NC
See figure at lower right.
Definition of pole and angle reference axis
The pole is set by entering two Cartesian coordinates in one of the
three planes. These coordinates also set the reference axis for the
polar angle PA.
Coordinates of the pole (plane) Reference axis of the angle
XY+X
YZ+Y
ZX+Z
10
Z
Y
PR
PA
2
PA
3
PR
CC
PA
PR
1
0°
X
30
Y
Z
Y
X
Z
Y
28
X
X
4 Programming: Fundamentals of NC, File Management, Programming Aids
Absolute and relative workpiece positions
Absolute workpiece positions
Absolute coordinates are position coordinates that are referenced
to the datum of the coordinate system (origin). Each position on the
workpiece is uniquely defined by its absolute coordinates.
Example 1: Holes dimensioned in absolute coordinates
Hole
X=10 mmX=30 mmX=50 mm
Y=10 mmY=20 mmY=30 mm
Hole Hole
30
20
10
Y
3
2
1
Relative workpiece positions
Relative coordinates are referenced to the last programmed
nominal position of the tool, which serves as the relative (imaginary)
datum. When you write a part program in incremental coordinates,
you thus program the tool to move by the distance between the
previous and the subsequent nominal positions. Incremental
coordinates are therefore also referred to as chain dimensions.
To program a position in incremental coordinates, enter the prefix
“I”(soft key) before the axis.
Example 2: Holes dimensioned with relative coordinates
Absolute coordinates of hole
:
X= 10 mm
Y= 10 mm
referenced to hole Hole referenced to hole
Hole
IX= 20 mmIX= 20 mm
IY= 10 mmIY= 10 mm
Absolute and incremental polar coordinates
Absolute polar coordinates always refer to the pole and the
reference axis.
Incremental polar coordinates always refer to the last programmed
nominal position of the tool.
10
1010
3010
50
4.1 Fundamentals of NC
Y
6
5
4
X
20
10
20
Y
X
10
PR
+IPA
+IPR
PR
+IPA
30
CC
PA
PR
0°
X
29HEIDENHAIN TNC 310
Selecting the datum
A production drawing identifies a certain form element of the
workpiece, usually a corner, as the absolute datum. Before setting
the datum, you align the workpiece with the machine axes and
move the tool in each axis to a known position relative to the
workpiece. You then set the TNC display to either zero or a
predetermined position value. This establishes the reference
system for the workpiece, which will be used for the TNC display
and your part program.
If the production drawing is dimensioned in relative coordinates,
simply use the coordinate transformation cycles. For further
information, refer to section 8.6 “Coordinate Transformation
Cycles.”
If the production drawing is not dimensioned for NC, set the datum
4.1 Fundamentals of NC
at a position or corner on the workpiece, which is the most suitable
for deducing the dimensions of the remaining workpiece positions.
The fastest, easiest and most accurate way of setting the datum is
by using a 3-D touch probe from HEIDENHAIN. For further
information, refer to section 12.2 “Setting the Datum with a 3-D
Touch Probe.”
Example
The workpiece drawing at right illustrates the holes
are dimensioned to an absolute datum with the coordinates X=0
Y=0. The holes
absolute coordinates X=450 Y=750. By using the DATUM SHIFT
cycle you can shift the datum temporarily to the position X=450,
Y=750 and program the holes
calculations.
to are referenced to a relative datum with the
to without any further
to , which
750
320
Z
Y
X
Y
150
0
7
6
-150
0,1
5
±
300
1
3
0
2
4
30
325
450900
950
4 Programming: Fundamentals of NC, File Management, Programming Aids
X
4.2File management
Files and file management
When you write a part program on the TNC, you must first enter a
file name. The TNC then stores the program as a file with the same
name. You can also store tables as files.
File names
The name of a file can have up to 8 characters. When you store
programs and tables as files, the TNC adds an extension to the file
name, separated by a point. This extension identifies the file type
(see table at right).
35720.H
File nameFile type
Files in the TNCType
Programs
in HEIDENHAIN conversational format .H
4.2 File Management
Table for
Tools.T
The TNC can manage up to 64 files. Their total size, however, must
not exceed 128 MB.
Working with the file manager
This section informs you about the meaning of the individual
screen information, and describes how to select files. If you are not
yet familiar with the TNC file manager, we recommend that you
read this section completely and test the individual functions on
your TNC.
Calling the file manager
Press the PGM NAME soft key:
the TNC displays the file management window
The window shows all of the files that are stored in the TNC. Each
file is shown with additional information that is illustrated in the
table on the next page.
Table for
Datums.D
display.Meaning
FILE NAMEName with up to 8 characters
and file type Number following
the name:
File size in bytes
StatusProperties of the file:
M Program is in a
Program Run mode of
operation.
P File is protected against
editing and erasure
(Protected)
31HEIDENHAIN TNC 310
Selecting a file
Calling the file manager
<
Use the arrow keys to move the highlight to the desired file:
Move the highlight up or down.
Deleting a file
ú Move the highlight to the file you want to delete.
ú To select the erasing function,
press the DELETE soft key.
The TNC inquires whether you
really intend to erase the file.
ú To confirm erasure: Press the YES
soft key. Abort with the NO soft key
if you do not wish to erase the
directory
Enter the first or more numbers of the file you wish to select and
4.2 File Management
then press the GOTO key: The highlight moves to the first file that
matches these numbers.
<
The selected file is opened in the operating
mode from which you have the called file
manager: Press ENT.
Copying a file
ú Move the highlight to the file you wish to copy.
ú Press the COPY soft key to select the copying
function.
ú Enter the name of the destination file and confirm your entry with
the ENT key: The TNC copies the file. The original file is retained.
Renaming a file
ú Move the highlight to the file you wish to rename.
ú Select the renaming function.
ú Enter the new file name; the file type cannot be
changed.
ú To execute renaming, press the ENT key.
Protecting a file/Canceling file
protection
ú Move the highlight to the file you want to protect.
ú To enable file protection, press the
PROTECT/UNPROTECT soft key.
The file now has status P.
You also need to enter the code number 86357.
To cancel file protection, enter the code number
86357.
32
4 Programming: Fundamentals of NC, File Management, Programming Aids
Read in/read out files
ú To read in or read out files: Press the ENT soft key.
The TNC provides the following functions:
Functions for reading in/reading out filesSoft key
Read in all files
Only read in selected files; To accept a file suggested
by the TNC, press the YES soft key;
Press the NO soft key if you do not want to accept it.
Read in the selected file: Enter the file name
Read out the selected file: Move the highlight
to the desired file and confirm with ENT
Read out all of the files in the TNC memory
Display the file directories of the external unit
on your TNC screen
4.2 File Management
33HEIDENHAIN TNC 310
4.3Creating and Writing Programs
Organization of an NC program in HEIDENHAIN
conversational format.
A part program consists of a series of program blocks. The figure at
right illustrates the elements of a block.
The TNC numbers the blocks in ascending sequence.
The first block of a program is identified by “BEGIN PGM,” the
program name and the active unit of measure.
The subsequent blocks contain information on:
■ The blank form:
■ tool definitions and tool calls,
■ Feed rates and spindle speeds as well as
■ Path contours, cycles and other functions
The last block of a program is identified by “END PGM,” the pro-
gram name and the active unit of measure.
4.3 Creating and Writing Programs
Defining the blank form — BLK FORM
Immediately after initiating a new program, you define a cuboid
workpiece blank. This definition is needed for the TNC’s graphic
simulation feature. The sides of the workpiece blank lie parallel to
the X, Y and Z axes and can be up to 30 000 mm long. The blank
form is defined by two of its corner points:
■ MIN point: the smallest X, Y and Z coordinates of the blank form,
entered as absolute values.
■ MAX point: the largest X, Y and Z coordinates of the blank form,
entered as absolute or incremental values.
Block:
10 L X+10 Y+5 R0 F100 M3
Path functionWords
Block number
Z
Y
MAX
X
34
The TNC can display the graphic only if the short side of
the BLK FORM is longer than 1/64 of the long side.
4 Programming: Fundamentals of NC, File Management, Programming Aids
MIN
Creating a new part program
You always enter a part program in the Programming and Editing
mode of operation.
Program initiation in an example:
Select the Programming and Editing mode of
operation.
<
Call up the file manager: Press the PGM NAME
soft key
File name =
<
3056 Enter the new program number and confirm
your entry with the ENT key.
File name = 3056.H
<
Select the default setting for unit of
measurement (mm): Press the ENT key, or
Switch to inches: Press the MM/INCH soft key
and confirm with ENT.
4.3 Creating and Writing Programs
35HEIDENHAIN TNC 310
Define the blank
Open the dialog for blank definition: Press the
BLK FORM soft key
Working spindle axis X/Y/Z ?
<
Enter the spindle axis.
Def BLK FORM: Min corner?
<
0Enter in sequence the X, Y and Z coordinates of
the MIN point.
0
-40
Def BLK FORM: Max-corner?
4.3 Creating and Writing Programs
<
100Enter in sequence the X, Y and Z coordinates of
the MAX point.
100
0
The program blocks window shows the following BLK FORM
definition
0 BEGIN PGM 3056 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 END PGM 3056 MM
The TNC automatically generates the block numbers as well as the
BEGIN and END blocks.
36
4 Programming: Fundamentals of NC, File Management, Programming Aids
Program begin, name, unit of measure
Tool axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure
Programming tool movements in conversational
format
To program a block, initiate the dialog by pressing a soft key. In the
screen headline, the TNC then asks you for all the information
necessary to program the desired function.
Example of a dialog
Initiate the dialog.
Coordinates ?
<
10Enter the target coordinate for the X axis.
<
5 Enter the target coordinate for the Y axis,
and go to the next question with ENT.
Radius comp. RL/RR/no comp. ?
<
Enter “No radius compensation” and go to the
next question with ENT.
Feed rate ?F=
<
100Enter a feed rate of 100 mm/min for this path
contour; go to the next question with ENT.
Miscellaneous function M ?
<
3Enter the miscellaneous function M3 “spindle
ON”; pressing the ENT key will terminate this
dialog.
Functions during the dialogKey
Ignore the dialog question
End the dialog immediately
Abort the dialog and erase the block
4.3 Creating and Writing Programs
The program blocks window will display the following line:
3 L X+10 Y+5 R0 F100 M3
37HEIDENHAIN TNC 310
Editing program lines
While you are creating or editing a part program, you can select any
desired line in the program or individual words in a block with the
arrow keys (see table at top right).
Selecting blocks or wordsSoft keys/keys
Move from one block to the next
Scrolling through the program
ú Press the GOTO key
ú Enter the block number and confirm with ENT, and the TNC will
go to the indicated block, or
ú Press one of the superimposed soft keys to scroll to another page
(see table at top right.)
Looking for the same words in different blocks
To select a word in a block, press the arrow keys
repeatedly until the highlight is on the desired
word.
4.3 Creating and Writing Programs
Select a block with the arrow keys.
The word that is highlighted in the new block is the same as the
one you selected previously.
Inserting blocks at any desired location
ú Select the block after which you want to insert a new block and
initiate the dialog.
Inserting the previously edited (deleted) block at any location
ú Select the block after which you want to insert the block you have
just edited (deleted.)
ú If you wish to insert a block you have stored in the buffer memory,
press the soft key INSERT NC BLOCK
Select individual words in a
block
Go to the previous page
Go to the next page
Jump to beginning
of program
Jump to beginning
End
Erasing blocks and wordsKey
Set the value of the selected word to
zero
Erase an incorrect number
Clear a (non-blinking) error message
Delete the selected word
Delete the selected block (cycle)
Editing and inserting words
ú Select a word in a block and overwrite it with the new one. The
plain-language dialog is available while the word is highlighted.
ú To accept the change, press the END key.
If you want to insert a word, press the horizontal arrow keys
repeatedly until the desired dialog appears. You can then enter the
desired value.
38
4 Programming: Fundamentals of NC, File Management, Programming Aids
Delete the program sections:
First select the last block of the
program section to be erased, then
erase with the DEL key.
4.4Interactive Programming Graphics
While you are writing the part program, you can have the TNC
generate a graphic illustration of the programmed contour.
To generate/not generate graphics during programming:
ú To switch the screen layout to displaying program blocks to the
left and graphics to the right, press the SPLIT SCREEN key and
PGM + GRAPHICS soft key.
ú Set the AUTO DRAW soft key to ON. While you are
entering the program lines, the TNC generates
each path contour you program in the graphics
window in the right screen half.
If you do not wish to have graphics generated during programming,
set the AUTO DRAW soft key to OFF.
AUTO DRAW ON does not simulate program section repeats.
To generate a graphic for an existing program:
ú Use the arrow keys to select the block up to which you want the
graphic to be generated, or press GOTO and enter the desired
block number.
ú To generate graphics, press the RESET + START
soft key.
Additional functions are listed in the table at right.
To erase the graphic:
ú Shift the soft-key row (see figure at right)
ú Delete graphic: Press CLEAR GRAPHIC soft key
FunctionsSoft key
Generate interactive graphics
blockwise
Generate a complete graphic
or complete it after
RESET + START
Interrupt interactive graphics
This soft key only appears while the
TNC generates the interactive graphics
4.4 Interactive Programming Graphics
39HEIDENHAIN TNC 310
Magnifying or reducing a detail
You can select the graphics display by selecting a detail with the
frame overlay. You can now magnify or reduce the selected detail.
ú Select the soft-key row for detail magnification/reduction
(last row, see figure at right)
The following functions are available:
FunctionSoft key
Reduce the frame overlay — press and
hold the soft key to reduce the detail
Enlarge the frame overlay — press and
hold the soft key to magnify the detail
Move the frame overlay to the left:
Press and hold the soft key. Move the
frame overlay to the right:
Press and hold the arrow to the right soft key
4.4 Interactive Programming Graphics
With the WINDOW BLK FORM soft key, you can restore the original
section.
ú Confirm the selected section with the WINDOW
DETAIL soft key
40
4 Programming: Fundamentals of NC, File Management, Programming Aids
4.5HELP function
Certain TNC programming functions are explained in more detail in
the HELP function. You can select a HELP topic using the soft keys
.
Select the HELP function
ú Press the HELP key
ú Select a topic: Press one of the available soft keys
Help topics / FunctionsSoft key
M functions
Cycle parameters
HELP that is entered by the machine manufacturers
(optional, not executable)
Go to previous page
Go to next page
Go to beginning of file
Go to end of file
Select search functions; Enter a number,
Begin search with ENT key
The HELP provided by the machine manufacturer can
only be displayed and not executed.
4.5 HELP Function
End the HELP function
Press the END key.
41HEIDENHAIN TNC 310
Programming:
Tools
5
5.1Entering Tool-Related Data
Feed rate F
The feed rate is the speed (in millimeters per minute or inches per
minute) at which the tool center moves. The maximum feed rates
can be different for the individual axes and are set in machine
parameters.
Input
You can enter the feed rate in every positioning block. For further
information refer to section 6.2 “Fundamentals of Path Contours.”
Rapid traverse
If you wish to program rapid traverse, enter FMAX. To enter FMAX,
press the ENT key or the FMAX soft key as soon as the dialog
question “Feed rate F = ?” appears on the TNC screen.
Duration of effect
A feed rate entered as a numerical value remains in effect until a
5.1 Entering Tool-Related Data
block with a different feed rate is reached. F MAX is only effective in
the block in which it is programmed. After the block with F MAX is
executed, the feed rate will return to the last feed rate entered as a
numerical value.
Changing during program run
You can adjust the feed rate during program run with the feed-rate
override knob.
Spindle speed S
The spindle speed S is entered in revolutions per minute (rpm) in a
TOOL CALL block.
Z
S
S
Y
F
X
Programmed change
In the part program, you can change the spindle speed in a TOOL
CALL block by entering the spindle speed only:
ú To program a tool call, press the
TOOL CALL soft key (3rd soft-key row)
ú Ignore the dialog question for „Tool number ?“ with
the right arrow key
ú Ignore the dialog question for „Working spindle axis
X/Y/Z ?“ with the right arrow key
ú Enter the new spindle speed for the dialog
question “Spindle speed S= ?”.
Changing during program run
You can adjust the spindle speed during program run with the
spindle-speed override knob.
44
5 Programming: Tools
5.2Tool Data
You usually program the coordinates of path contours as they are
dimensioned in the workpiece drawing. To allow the TNC to
calculate the tool center path — i.e. the tool compensation — you
must also enter the length and radius of each tool you are using.
Tool data can be entered either directly in the part program with
TOOL DEF or (and) separately in tool tables. The TNC will consider
all of the data entered when executing the part program.
Tool number
Each tool is identified by a number between 0 and 254.
The tool number 0 is automatically defined as the zero tool with the
length L=0 and the radius R=0. In tool tables, tool 0 should also be
defined with L=0 and R=0.
Tool length L
There are two ways to determine the tool length L:
1 The length L is the difference between the length of the tool and
that of a zero tool L
For the algebraic sign:
■ The tool is longer than the zero toolL>L
■ The tool is shorter than the zero tool:L<L
To determine the length:
ú Move the zero tool to the reference position in the tool axis
(e.g. workpiece surface with Z=0).
ú Set the datum in the tool axis to 0 (datum setting).
ú Insert the desired tool.
ú Move the tool to the same reference position as the zero tool.
ú The TNC displays the difference between the current tool and the
zero tool.
ú Enter the value in the TOOL DEF block or in the tool table by
pressing the „ACTUAL POSITION“ key
2 If you determine the length L with a tool presetter, this value can
be entered directly in the TOOL DEF block without further
calculations.
.
0
0
0
Z
L
0
5.2 Tool Data
X
45HEIDENHAIN TNC 310
Tool radius R
You can enter the tool radius R directly.
Delta values for lengths and radii
Delta values are offsets in the length and radius of a tool.
A positive delta value describes a tool oversize (DR>0), a negative
5.2 Tool Data
delta value describes a tool undersize (DR<0). Enter the delta
values when you are programming with TOOL CALL.
Input range: You can enter a delta value with up to ± 99.999 mm.
R
L
DR<0
R
Entering tool data into the program
The number, length and radius of a specific tool is defined in the
TOOL DEF block of the part program.
ú To select tool definition, press the TOOL DEF key.
ú Enter the Tool number: Each tool is uniquely
identified by its number. When the tool table is
active, enter tool numbers greater than 99
(dependent on MP7260)
ú Enter the tool length: Enter the compensation
value for the tool length.
ú Enter the Tool radius.
During the dialog, you can take the values for length and
radius directly from the position display with the soft
keys „CUR.POS X, CUR.POS Y or CUR.POS Z“.
Resulting NC block:
4 TOOL DEF 5 L+10 R+5
DR>0
DL<0
DL>0
46
5 Programming: Tools
Entering tool data in tables
You can define and store up to 254 tools and their tool data in the
tool table (the maximum number of tools in the table can be set in
machine parameter 7260).
Tool table: Available input data
Abbr.Input
TNumber by which the tool is called in the program
LValue for tool length compensation L
RCompensation value for the tool radius R
Editing the tool table
The tool table has the name TOOL.T is automatically active in a
program run operating mode.
To open the tool table TOOL.T:
ú Select any machine operating mode.
ú To select the tool table, press the TOOL TABLE soft
key.
ú Set the EDIT soft key to ON.
ú Select the Programming and Editing mode of operation.
ú Calls the file manager.
ú Move the highlight to TOOL.T. Confirm with the
ENT key.
Dialog
–
Tool length?
Tool radius?
5.2 Tool Data
When you have opened the tool table, you can edit the tool data by
moving the cursor to the desired position in the table with the
arrow keys (see figure at center right). You can overwrite the stored
values, or enter new values at any position. The available editing
functions are illustrated in the table on the next page.
If you edit the tool table parallel to tool change the TNC
does not interrupt the program run. However, the
changed data does not become effective until the next
tool call.
To leave the tool table:
ú Finish editing the tool table: Press the END key.
ú Call the file manager and select a file of a different type, e.g. a
part program.
47HEIDENHAIN TNC 310
Editing functions for tool tablesSoft key
Take the value from the position
display
Select previous page in table
(2nd soft-key row)
5.2 Tool Data
Select next page in table
(2nd soft-key row)
Move the highlight one column to
the left
Move the highlight one column to
the right
Delete incorrect numerical value,
re-establish preset value
Re-establish the last value stored
Move the highlight back to beginning of line
48
5 Programming: Tools
Calling tool data
A TOOL CALL block in the part program is defined with the
following data:
ú Select the tool call function with the TOOL CALL
key
ú Tool number: Enter the number of the tool. The
tool must already be defined in a TOOL DEF block
or in the tool table.
ú Working spindle axis X/Y/Z: Enter the tool axis.
ú Spindle speed S
ú Tool length oversize: Enter the delta value for the
tool length.
ú Tool radius oversize: Enter the delta value for the
tool radius.
Example:
Call tool number 5 in the tool axis Z with a spindle speed 2500 rpm.
The tool length is to be programmed with an oversize of 0.2 mm,
the tool radius with an undersize of 1 mm.
20 TOOL CALL 5 Z S2500 DL+0.2 DR-1
The character D preceding L and R designates delta values.
Tool change
The tool change function can vary depending on the
individual machine tool. Refer to your machine tool
manual.
5.2 Tool Data
Tool change position
A tool change position must be approachable without collision. With
the miscellaneous functions M91 and M92, you can enter machinereferenced (rather than workpiece-referenced) coordinates for the
tool change position. If TOOL CALL 0 is programmed before the
first tool call, the TNC moves the tool spindle in the tool axis to a
position that is independent of the tool length.
Manual tool change
To change the tool manually, stop the spindle and move the tool to
the tool change position:
ú Move to the tool change position under program control.
ú Interrupt program run (see section 11.3 “Program Run”).
ú Change the tool.
ú Resume the program run (see section 11.3 “Program Run”).
49HEIDENHAIN TNC 310
Pocket table for tool changer
The TOOLP.TCH (TOOL Pocket)table must be programmed to enable
automatic tool change.
To select the pocket table:
ú In the Programming and Editing mode,
5.2 Tool Data
ú In a machine operating mode
ú Calls the file manager.
ú Move the highlight to TOOLP.TCH. Confirm with the
ENT key.
ú To select the tool table, press the TOOL TABLE soft
key.
ú To select the pocket table,
press the POCKET TABLE soft key
ú Set the EDIT soft key to ON
Editing functions for pocket tableSoft key
Select previous page in table
(2nd soft-key row)
When you have opened the pocket table, you can edit the tool data
by moving the cursor to the desired position in the table with the
arrow keys (see figure at upper right). You can overwrite the stored
values, or enter new values at any position.
You may not use a tool number twice in the pocket table. If you do
so the TNC will output an error message when you exit the table.
You can enter the following information on a tool into a pocket table
Abbr.Input
PPocket number of the tool in the tool magazine
TTool number
STSpecial tool with large radius requiring more than one
pocket (ST: If your special tool takes up pockets in front
of and behind its actual pocket, these additional
pockets need to be locked (status L).
FFixed tool number.
The tool is always returned to the same pocket.
LLocked pocket
PLCInformation on this tool pocket that is to be
sent to the PLC
Select next page in table
(2nd soft-key row)
Move the highlight one column to
the left
Move the highlight one column to
the right
Reset pocket table
Dialog
–
Tool number?
Special tool ?
Fixed pocket?
Locked pocket?
PLC status?
50
5 Programming: Tools
5.3Tool Compensation
The TNC adjusts the spindle path in the tool axis by the
compensation value for the tool length. In the working plane, it
compensates the tool radius.
If you are writing the part program directly on the TNC, the tool
radius compensation is effective only in the working plane.
Tool length compensation
Length compensation becomes effective automatically as soon as a
tool is called and the tool axis moves. To cancel length
compensation call a tool with the length L=0.
If you cancel a positive length compensation with TOOL
CALL 0, the distance between tool and workpiece will
be reduced.
After TOOL CALL, the path of the tool in the tool axis, as
entered in the part program, is adjusted by the difference
between the length of the previous tool and that of the
new one.
For tool length compensation, the TNC takes the delta values from
the TOOL CALL block into account:
Compensation value = L + DL
Lis the tool length L from the TOOL DEF block or tool
table
DL
TOOL CALL
is the oversize for length DL in the TOOL CALL block
(not taken into account by the position display)
TOOL CALL
where
5.3 Tool Compensation
Tool radius compensation
The NC block for programming a tool movement contains:
■ RL or RR for compensation in the tool radius
■ R+ or R– for radius compensation in single-axis movements
■ R0 if no radius compensation is required
Radius compensation becomes effective as soon as a tool is called
and is moved in the working plane with RL or RR. To cancel radius
compensation, program a positioning block with R0.
51HEIDENHAIN TNC 310
For tool radius compensation, the TNC takes the delta values from
the TOOL CALL block into account:
Compensation value = R + DR
TOOL CALL,
where
Ris the tool radius R from the TOOL DEF block or tool
table
DR
TOOL CALL
is the oversize for radius DR in the TOOL CALL block
(not taken into account by the position display)
Tool movements without radius compensation: R0
The tool center moves in the working plane to the programmed
path or coordinates.
Applications: Drilling and boring, pre-positioning
(see figure at center right)
5.3 Tool Compensation
Tool movements with radius compensation: RR and RL
RR The tool moves to the right of the programmed contour
RL The tool moves to the left of the programmed contour
The tool center moves along the contour at a distance equal to the
radius. “Right” or “left” are to be understood as based on the
direction of tool movement along the workpiece contour (see
illustrations on the next page).
Between two program blocks with different radius
compensations (RR and RL) you must program at least
one block without radius compensation (that is, with R0).
Radius compensation does not come into effect until the
end of the block in which it is first programmed.
Whenever radius compensation is activated with RR/RL
or canceled with R0, the TNC positions the tool
perpendicular to the programmed starting or end
position. Position the tool at a sufficient distance from
the first or last contour point to prevent the possibility of
damaging the contour.
RL
R0
R
R
Z
Y
X
Y
X
52
5 Programming: Tools
Entering radius compensation
When you program a path contour, the following dialog question is
displayed after entry of the coordinates:
Radius comp.: RL/RR/no comp. ?
<
To select tool movement to the left of the
contour, press the RL soft key, or
To select tool movement to the right of the
contour, press the RR soft key, or
Y
RL
To select tool movement without radius
compensation or to cancel radius
compensation, press the ENT key or the R0 soft
key.
To terminate the dialog, press the END key.
X
5.3 Tool Compensation
Y
RR
X
53HEIDENHAIN TNC 310
Radius compensation: Machining corners
Outside corners
If you program radius compensation, the TNC moves the tool in a
transitional arc around corners. The tool “rolls around” the corner
point. If necessary, the TNC reduces the feed rate at outside
corners to reduce machine stress, for example at very great
changes of direction.
Inside corners
The TNC calculates the intersection of the tool center paths at
inside corners under radius compensation. From this point it then
starts the next contour element. This prevents damage to the
workpiece. The permissible tool radius, therefore, is limited by the
geometry of the programmed contour.
5.3 Tool Compensation
To prevent the tool from damaging the contour, be
careful not to program the starting or end position for
machining inside corners at a corner of the contour.
Machining corners without radius compensation
If you program the tool movement without radius compensation,
you can change the tool path and feed rate at workpiece corners
with the miscellaneous function M90. See ”7.4 Miscellaneous
Functions for Contouring Behavior.”
RL
RLRL
54
5 Programming: Tools
6
Programming:
Programming Contours
6.1Overview of Tool Movements
Path functions
A workpiece contour is usually composed of several contour
elements such as straight lines and circular arcs. With the path
functions, you can program the tool movements for straight lines
and circular arcs.
Miscellaneous functions M
With the TNC’s miscellaneous functions you can affect
■ Program run, e.g., a program interruption
■ Machine functions, such as switching spindle rotation and coolant
supply on and off
■ Contouring behavior of the tool
Subprograms and program section repeats
6.1 Overview of Tool Movements
If a machining sequence occurs several times in a program, you can
save time and reduce the chance of programming errors by
entering the sequence once and then defining it as a subprogram
or program section repeat. If you wish to execute a specific program section only under certain conditions, you also define this
machining sequence as a subprogram. In addition, you can have a
part program call a separate program for execution.
How subprograms and program section repeats are used in
programming is described in Chapter 9.
L
L
CC
L
C
Y
80
60
40
CC
R40
56
11510
X
6 Programming: Programming Contours
6.2Fundamentals of Path Functions
Programming tool movements for workpiece
machining
You create a part program by programming the path functions for
the individual contour elements in sequence. You usually do this by
entering the coordinates of the end points of the contourelements given in the production drawing. The TNC calculates the
actual path of the tool from these coordinates, and from the tool
data and radius compensation.
The TNC moves all axes programmed in a single block
simultaneously.
Movement parallel to the machine axes
The program block contains only one coordinate. The TNC thus
moves the tool parallel to the programmed axis.
Depending on the individual machine tool, the part program is
executed by movement of either the tool or the machine table on
which the workpiece is clamped. Nevertheless, you always program path contours as if the tool moves and the workpiece remains
stationary.
Example:
L X+100
LPath function for “straight line”X+100Coordinate of the end point
The tool retains the Y and Z coordinates and moves to the position
X=100. See figure at upper right.
Movement in the main planes
The program block contains two coordinates. The TNC thus moves
the tool in the programmed plane.
Example:
L X+70 Y+50
The tool retains the Z coordinate and moves in the XY plane to the
position X=70, Y=50. See figure at center right.
50
Z
Y
X
100
Z
6.2 Fundamentals of Path Functions
Y
X
70
Z
Three-dimensional movement
The program block contains three coordinates. The TNC thus moves
the tool in space to the programmed position.
Example:
L X+80 Y+0 Z-10
See figure at lower right.
Y
-10
X
80
57HEIDENHAIN TNC 310
Circles and circular arcs
The TNC moves two axes simultaneously in a circular path relative
to the workpiece. You can define a circular movement by entering
the circle center CC.
When you program a circle, the TNC assigns it to one of the main
planes. This plane is defined automatically when you set the
spindle axis during a tool call:
Spindle axisMain plane
ZXY
YZX
XYZ
Direction of rotation DR for circular movements
When a circular path has no tangential transition to another contour
element, enter the direction of rotation DR:
Clockwise direction of rotation: DR–
Counterclockwise direction of rotation: DR+
Radius compensation
Radius compensation must be programmed before the block
containing the coordinates for the first contour element. You cannot
6.2 Fundamentals of Path Functions
begin radius compensation in a circle block. It must be activated
beforehand in a straight-line block.
Pre-positioning
Before running a part program, always pre-position the tool to
prevent the possibility of damaging it or the workpiece.
Y
Y
Y
C
C
X
CC
X
CC
X
Z
DR+
Y
DR–
CC
CC
X
58
6 Programming: Programming Contours
Creating the program blocks with the path function keys
Use the path function keys to open a conversational dialog. The
TNC asks you successively for all the necessary information and
inserts the program block into the part program.
You may not program controlled and non-controlled axes
in the same block.
Example — programming a straight line:
Initiate the programming dialog (here, for a
straight line).
Coordinates ?
<
10Enter the coordinates of the straight-line end
point.
5
Transfer the coordinates of the selected axis:
Press ACTUAL POSITION soft key (second softkey row)
6.2 Fundamentals of Path Functions
Radius comp.: RL/RR/NOcomp. ?
<
Select the radius compensation (here, press the
RL soft key — the tool moves to the left of the
programmed contour).
Feed rateF=
<
100Enter the feed rate (here, 100 mm/min), and
confirm your entry with ENT.
Miscellaneous function M ?
<
3Enter a miscellaneous function (here, M3), and
terminate the dialog with ENT.
The part program now contains the following line:
L X+10 Y+5 RL F100 M3
59HEIDENHAIN TNC 310
6.3Contour Approach and Departure
Overview: Types of paths for contour approach and
departure
The functions for contour approach and departure are activated with
the APPR/DEP key. You can then select the following contour forms
using soft keys.
Function Soft keys:Approach Departure
Straight line with tangential connection
Straight line perpendicular to a contour point
Circular arc with tangential connection
Circular arc with tangential connection to
the contour. Approach and departure to an
auxiliary point outside of the contour on a
tangentially connecting line.
6.3 Contour Approach and Departure
Approaching and departing a helix
The tool approaches and departs a helix on its extension by moving
in a circular arc that connects tangentially to the contour. You
program helix approach and departure with the APPR CT and DEP
CT functions.
Important positions for approach and departure
■ Starting point P
You program this position in the block before the APPR block. P
lies outside the contour and is approached without radius
compensation (R0).
■ Auxiliary point P
Some of the paths for approach and departure go through an
auxiliary point P
APPR or DEP block.
■ First contour point P
You program the first contour point PA in the APPR block. The last
contour point P
■ If the APPR block also contains a Z axis coordinate, the TNC will
first move the tool to P
the entered depth in the tool axis.
■ End point P
The position PN lies outside of the contour and results from your
input in the DEP block. If the DEP block also contains a Z axis
coordinate, the TNC will first move the tool to P
plane, and then move it to the entered depth in the tool axis.
60
S
H
that the TNC calculates from your input in the
H
and last contour point P
A
can be programmed with any path function.
E
in the working plane, and then move it to
H
N
E
in the working
H
S
RL
P
A
P
RL
H
P
R0
S
RL
RL
P
R0
N
P
RL
E
6 Programming: Programming Contours
You can enter the position data in absolute or incremental
coordinates and in Cartesian or polar coordinates.
The TNC does not check whether the programmed contour will be
damaged when moving from the actual position to the auxiliary
point P
. Use the test graphics to simulate approach and departure
H
before executing the part program.
When approaching the contour, allow sufficient distance between
the starting point P
and the first contour point PA to assure that the
S
TNC will reach the programmed feed rate for machining.
The TNC moves the tool from the actual position to the auxiliary
point P
at the feed rate that was last programmed.
H
Radius compensation
For the TNC to interpret an APPR block as an approach block you
must program a change in compensation from R0 to RL/RR. The
TNC automatically cancels the radius compensation in a DEP block.
If you wish to program a contour element with the DEP block (no
change in compensation), then you need to program the active
radius compensation again (2nd soft-key row, if the F element is
highlighted).
If no change in compensation is programmed in an APPR or in a
DEP block, the TNC makes the contour connection as follows:
FunctionContour connection
APPR LTTangential connection to the following
Contour element
APPR LNPerpendicular connection to the following
Contour element
APPR CTwithout angle of traverse/without radius:
Tangentially connecting circular arc between the
preceding and the following contour element.
without angle of traverse/with radius:
Tangentially connecting circular arc with programmed
radius to the following contour element
with angle of traverse/without radius:
Tangentially connecting circular are with angle of
traverse to the following contour element
with angle of traverse/with radius:
Tangentially connecting circular arc with connecting
line and angle of traverse to the following contour
element
Tangentially connecting circular arc
between the preceding and the
following Contour element
without angle of traverse/with
radius:
Tangentially connecting circular arc
with programmed radius to the
preceding contour element
with angle of traverse/without
radius:
Tangentially connecting circular arc
with angle of traverse to the
preceding contour element
with angle of traverse/with radius:
Tangentially connecting circular arc
with connecting line and angle of
traverse to the preceding contour
element
DEP LCTTangent with tangentially
connecting circular arc to the
preceding contour element
6.3 Contour Approach and Departure
61HEIDENHAIN TNC 310
Approaching on a straight line
with tangential connection: APPR LT
The tool moves on a straight line from the starting point PS to an
auxiliary point P
on a straight line that connects tangentially to the contour. The
auxiliary point P
distance LEN.
ú Use any path function to approach the starting point P
Example NC blocks
7 L X+40 Y+10 R0 FMAX M3
8 APPR LT X+20 Y+20 Z-10 LEN15 RR F100
9 L X+35 Y+35
6.3 Contour Approach and Departure
10 L ...
. It then moves from PHto the first contour point P
H
is separated from the first contour point PA by the
H
ú Initiate the dialog with the APPR/DEP key and APPR
LT soft key:
ú Coordinates of the first contour point P
ú LEN: Distance from the auxiliary point P
first contour point P
ú Radius compensation for machining
A
Approaching on a straight line perpendicular to the
first contour point: APPR LN
The tool moves on a straight line from the starting point PS to an
auxiliary point P
on a straight line perpendicular to the first contour element. The
auxiliary point P
distance LEN plus the tool radius.
ú Use any path function to approach the starting point P
ú Initiate the dialog with the APPR/DEP key and APPR LN soft key:
. It then moves from PHto the first contour point P
H
is separated from the first contour point PA by the
H
ú Coordinates of the first contour point P
ú Length: Distance from the auxiliary point P
first contour point P
A
Always enter LEN as a positive value!
ú Radius compensation RR/RL for machining
.
S
A
to the
H
.
S
A
to the
h
Y
35
A
20
10
P
RR
15
H
P
RR
A
20
Approach PS without radius compensation
PA with radius comp. RR
End point of the first contour element
Next contour element
Y
35
P
RR
RR
15
H
20
A
P
A
20
10
RR
10
RR
35
P
S
R0
X
40
P
S
R0
X
40
Example NC blocks
7 L X+40 Y+10 R0 FMAX M3
8 APPR LN X+10 Y+20 Z-10 LEN+15 RR F100
9 L X+20 Y+35
10 L ...
62
Approach PS without radius compensation
PA with radius comp. RR, distance PH to PA: LEN=15
End point of the first contour element
Next contour element
6 Programming: Programming Contours
Approaching on a circular arc
with tangential connection: APPR CT
The tool moves on a straight line from the starting point PS to an
auxiliary point P
following a circular arc that is tangential to the first contour
element.
The arc from P
center angle CCA. The direction of rotation of the circular arc is
automatically derived from the tool path for the first contour
element.
ú Use any path function to approach the starting point P
ú Initiate the dialog with the APPR/DEP key and APPR CT soft key:
Example NC blocks
7 L X+40 Y+10 R0 FMAX M3
8 APPR CT X+10 Y+20 Z-10 CCA180 R+10 RR F100
9 L X+20 Y+35
10 L ...
. It then moves from PH to the first contour point P
H
to PA is determined through the radius R and the
H
.
S
ú Coordinates of the first contour point P
ú Center angle CCA of the arc
■ CCA can be entered only as a positive value.
■ Maximum input value 360°
ú Radius R of the circular arc
■ If the tool should approach the workpiece in the
A
direction defined by the radius compensation:
Enter R as a positive value.
■ If the tool should approach the workpiece opposite
to the radius compensation:
Enter R as a negative value.
ú Radius compensation RR/RL for machining
Y
35
CCA=
180°
RR
P
20
A
P
20
10
A
RR
R10
Approach PS without radius compensation
PA with radius comp. RR, Radius R=10
End point of the first contour element
Next contour element
RR
P
S
R0
H
X
4010
6.3 Contour Approach and Departure
63HEIDENHAIN TNC 310
Approaching on a circular arc with tangential
connection from a straight line to the contour:
APPR LCT
The tool moves on a straight line from the starting point PS to an
auxiliary point P
on a circular arc.
The arc is connected tangentially both to the line P
to the first contour element. Once these lines are known, the radius
then suffices to completely define the tool path.
ú Use any path function to approach the starting point P
ú Initiate the dialog with the APPR/DEP key and APPR LCT soft key:
. It then moves from PH to the first contour point P
H
– PH as well as
S
ú Coordinates of the first contour point P
ú Radius R of the arc
Always enter R as a positive value.
ú Radius compensation for machining
Y
35
RR
A
20
10
.
S
A
Approach PS without radius compensation
PA with radius compensation RR, radius R=10
End point of the first contour element
Next contour element
P
RR
A
R10
20
P
RR
H
P
S
R0
X
4010
64
6 Programming: Programming Contours
Departing tangentially on a straight line: DEP LT
The tool moves on a straight line from the last contour point PE to
the end point P
element. P
ú Program the last contour element with the end point P
radius compensation.
ú Initiate the dialog with the APPR/DEP key and DEP LT soft key:
Example NC blocks
23 L Y+20 RR F100
24 DEP LT LEN12.5 R0 F100
25 L Z+100 FMAX M2
. The line lies in the extension of the last contour
N
is separated from PE by the distance LEN.
N
ú LEN: Enter the distance from the last contour
element P
to the end point PN.
E
and
E
Y
RR
20
12.5
P
RR
P
R0
E
N
X
Last contour element: PE with radius compensation
Depart contour by LEN = 12.5 mm
Retract in Z, return to block 1, end program
Departing on a straight line perpendicular to the
last contour point: DEP LN
The tool moves on a straight line from the last contour point PE to
the end point P
last contour point P
plus the tool radius.
ú Program the last contour element with the end point P
radius compensation.
ú Initiate the dialog with the APPR/DEP key and DEP LN soft key:
Example NC blocks
23 L Y+20 RR F100
24 DEP LN LEN+20 F100
25 L Z+100 FMAX M2
. The line departs on a perpendicular path from the
N
. PN is separated from PE by the distance LEN
E
and
E
ú LEN: Enter the distance from the last contour
element P
to the end point PN.
E
Important: Always enter LEN as a positive value!
Y
RR
P
N
20
R0
20
P
RR
E
X
Last contour element: PE with radius compensation
Depart perpendicular to contour by LEN = 20 mm
Retract in Z, return to block 1, end program
6.3 Contour Approach and Departure
65HEIDENHAIN TNC 310
Departing tangentially on a circular arc: DEP CT
The tool moves on a circular arc from the last contour point PE to
the end point P
contour element.
ú Program the last contour element with the end point P
radius compensation.
ú Initiate the dialog with the APPR/DEP key and DEP CT soft key:
Example NC blocks
23 L Y+20 RR F100
24 DEP CT CCA 180 R+8 F100
6.3 Contour Approach and Departure
25 L Z+100 FMAX M2
. The arc is tangentially connected to the last
N
ú Center angle CCA of the arc
ú Radius R of the circular arc
■ If the tool should depart the workpiece in the
direction of the radius compensation (i.e. to the
right with RR or to the left with RL):
Enter R as a positive value.
■ If the tool should depart the workpiece on the
direction opposite to the radius compensation:
Enter R as a negative value.
and
E
Y
RR
P
N
20
R0
R8
180°
P
RR
E
X
Last contour element: PE with radius compensation
Center angle=180°, arc radius=10 mm
Retract in Z, return to block 1, end program
66
6 Programming: Programming Contours
Departing on a circular arc tangentially connecting
the contour and a straight line: DEP LCT
The tool moves on a circular arc from the last contour point PE to an
auxiliary point P
straight line. The arc is tangentially connected both to the last
contour element and to the line from P
known, the radius R then suffices to completely define the tool
path.
ú Program the last contour element with the end point P
radius compensation.
ú Initiate the dialog with the APPR/DEP key and DEP LCT soft key:
Example NC blocks
23 L Y+20 RR F100
24 DEP LCT X+10 Y+12 R8 F100
25 L Z+100 FMAX M2
. It then moves from PH to the end point PN on a
H
to PN. Once these lines are
H
E
ú Enter the coordinates of the end point P
ú Radius R of the arc
.
N
Always enter R as a positive value
and
Y
RR
20
R8
12
10
P
R0
P
H
N
R0
Last contour element: PE with radius compensation
Coordinates PN, arc radius = 10 mm
Retract in Z, return to block 1, end program
P
RR
E
X
6.3 Contour Approach and Departure
67HEIDENHAIN TNC 310
6.4Path Contours — Cartesian
Coordinates
Overview of path functions
Function Contour function soft key
Line L
CHamFer
Circle Center
Circle
Circle by Radius
Circle Tangential
Circle Tangential
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
Corner RouNDing
Tool movement
Straight line
Chamfer between two straight lines
No tool movement
Circular arc around a circle
center CC to an arc end point
Circular arc with a certain radius
Circular arc with tangential connection
to the preceding contour element
Circular arc with tangential connection
to the preceding and subsequent
contour elements
Required input
Coordinates of the straight-line
end point
Chamfer side length
Coordinates of the circle center or
pole
Coordinates of the arc end point,
direction of rotation
Coordinates of the arc end point,
arc radius, direction of rotation
Coordinates of the arc end point
Rounding-off radius R
68
6 Programming: Programming Contours
Straight line L
The tool moves on a straight line from its current position to the line
end point. The starting point is the end point of the preceding block.
Y
40
ú Enter the coordinates of the end point.
Further entries, if necessary:
ú Radius compensation RL/RR/R0
ú Feed rate F
ú Miscellaneous function M
Example NC blocks
7 L X+10 Y+40 RL F200 M3
8 L IX+20 IY-15
9 L X+60 IY-10
Inserting a chamfer CHF between two straight lines
The chamfer enables you to cut off corners at the intersection of
two straight lines.
■ The blocks before and after the CHF block must be in the same
working plane.
■ The radius compensation before and after the chamfer block must
be the same.
■ An inside chamfer must be large enough to accommodate the
current tool.
ú Chamfer side length: Enter the length of the
chamfer
Further entries, if necessary:
ú Feed rate F (only effective in CHF block)
15
10
10
20
X
60
Y
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
X
Example NC blocks
7 L X+0 Y+30 RL F300 M3
8 L X+40 IY+5
9 CHF 12
10 L IX+5 Y+0
You cannot start a contour with a CHF block
A chamfer is possible only in the working plane.
If you have not programmed a feed rate in the CHF block,
the TNC will move at the last programmed feed rate.
A feed rate programmed in the CHF block is effective
only in that block. After the CHF block, the previous feed
rate becomes effective again.
The corner point is cut off by the chamfer and is not part
of the contour.
30
Y
5
12
40
12
5
X
69HEIDENHAIN TNC 310
Circle center CC
You can define a circle center CC for circles that are programmed
with the C soft key (circular path C). This is done in the following
ways:
■ Entering the Cartesian coordinates of the circle center
■ Using the circle center defined in an earlier block
■ Capturing the coordinates with the
„ACTUAL POSITION“ soft key
ú Select circle functions: Press the „CIRCLE“ soft key
(2nd soft-key row)
ú Coordinates CC: Enter the circle center coordinates
If you want to use the last programmed position,
do not enter any coordinates.
Example NC blocks
5 CC X+25 Y+25
or
10 L X+25 Y+25
11 CC
The program blocks 10 and 11 do not refer to the illustration.
Duration of effect
The circle center definition remains in effect until a new circle
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
center is programmed.
Z
Y
CC
Y
CC
X
CC
X
Entering the circle center CC incrementally
If you enter the circle center with incremental coordinates, you
have programmed it relative to the last programmed position of the
tool.
The only effect of CC is to define a position as circle
center: The tool does not move to this position.
The circle center is also the pole for polar coordinates.
70
6 Programming: Programming Contours
Circular path C around circle center CC
Before programming a circular path C, you must first enter the
circle center CC. The last programmed tool position before the C
block is used as the circle starting point.
ú Move the tool to the circle starting point.
ú Select circle functions: Press the „CIRCLE“ soft key
(2nd soft-key row)
ú Enter the coordinates of the circle center.
ú Enter the coordinates of the arc end point
ú Direction of rotation DR
Further entries, if necessary:
ú Feed rate F
ú Miscellaneous function M
Y
E
CC
S
X
Example NC blocks
5 CC X+25 Y+25
6 L X+45 Y+25 RR F200 M3
7 C X+45 Y+25 DR+
Full circle
Enter the same point you used as the starting point for the end
point in a C block.
The starting and end points of the arc must lie on the
circle.
Input tolerance: up to 0.016 mm.
25
Y
CC
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
25
45
X
71HEIDENHAIN TNC 310
Circular path CR with defined radius
The tool moves on a circular path with the radius R.
ú Select circle functions: Press the „CIRCLE“ soft key
(2nd soft-key row)
ú Enter the coordinates of the arc end point.
ú Radius R
Note: The algebraic sign determines the size of the
arc.
ú Direction of rotation DR
Note: The algebraic sign determines whether the
arc is concave or convex.
Further entries, if necessary:
ú Feed rate F
ú Miscellaneous function M
Y
E1=S
R
2
S1=E
CC
2
X
Full circle
For a full circle, program two CR blocks in succession:
The end point of the first semicircle is the starting point of the
second. The end point of the second semicircle is the starting point
of the first. See figure at upper right.
Central angle CCA and arc radius R
The starting and end points on the contour can be connected with
four arcs of the same radius:
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
Smaller arc: CCA<180°
Enter the radius with a positive sign R>0
Larger arc: CCA>180°
Enter the radius with a negative sign R<0
The direction of rotation determines whether the arc is curving
outward (convex) or curving inward (concave):
Convex: Direction of rotation DR– (with radius compensation RL)
Concave: Direction of rotation DR+ (with radius compensation RL)
The distance from the starting and end points of the arc
diameter cannot be greater than the diameter of the arc.
The maximum possible radius is 30 m.
Circular path CT with tangential connection
The tool moves on an arc that starts at a tangent with the previously
programmed contour element.
A transition between two contour elements is called “tangential”
when there is no kink or corner at the intersection between the two
contours — the transition is smooth.
The contour element to which the tangential arc connects must be
programmed immediately before the CT block. This requires at
least two positioning blocks.
ú Select circle functions: Press the „CIRCLE“ soft key
(2nd soft-key row)
ú Enter the coordinates of the arc end point.
Further entries, if necessary:
ú Feed rate F
ú Miscellaneous function M
Example NC blocks
7 L X+0 Y+25 RL F300 M3
8 L X+25 Y+30
9 CT X+45 Y+20
10 L Y+0
30
25
Y
20
25
45
X
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
A tangential arc is a two-dimensional operation: the
coordinates in the CT block and in the contour element
preceding it must be in the same plane of the arc.
73HEIDENHAIN TNC 310
Corner Rounding RND
The RND function is used for rounding off corners.
The tool moves on an arc that is tangentially connected to both the
preceding and subsequent contour elements.
The rounding arc must be large enough to accommodate the tool.
ú Rounding-off radius: Enter the radius of the arc.
ú Feed rate for rounding the corner.
Example NC blocks
5 L X+10 Y+40 RL F300 M3
6 L X+40 Y+25
7 RND R5 F100
8 L X+10 Y+5
In the preceding and subsequent contour elements,
both coordinates must lie in the plane of the rounding
arc.
The corner point is cut off by the rounding arc and is not
part of the contour.
A feed rate programmed in the RND block is effective
only in that block. After the RND block, the previous feed
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
rate becomes effective again.
You can also use an RND block for a tangential contour
approach if you do not want to use an APPR function.
40
Y
R5
5
25
X
10
40
74
6 Programming: Programming Contours
Example: Linear movements and chamfers with Cartesian coordinates
Example: Linear movements and chamfers with Cartesian coordinates
0 BEGIN PGM 10 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+10
4 TOOL CALL 1 Z S4000
5 L Z+250 R0 F MAX
6 L X-20 Y-10 R0 F MAX
7 L Z-5 R0 F1000 M3
8 L X+5 Y+5 RL F300
9 RND R2
10 L Y+95
11 L X+95
12 CHF 10
13 L Y+5
14 CHF 20
15 L X+5
16 RND R2
17 L X-20 R0 F1000
18 L Z+250 R0 F MAX M2
19 END PGM 10 MM
Y
95
5
5
Define blank form for graphic workpiece simulation
Define tool in the program
Call tool in the spindle axis and with the spindle speed S
Retract tool in the spindle axis at rapid traverse FMAX
Pre-position the tool
Move to working depth at feed rate F = 1000 mm/min
Approach the contour at point 1
Tangential approach to circle with R=2 mm
Move to point 2
Point 3: first straight line for corner 3
Program chamfer with length 10 mm
Point 4: 2nd straight line for corner 3, 1st straight line for corner 4
Program chamfer with length 20 mm
Move to last contour point 1, second straight line for corner 4
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program
20
10
10
20
X
95
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
75HEIDENHAIN TNC 310
Example: Circular movements with Cartesian coordinates
Example: Circular movements with Cartesian coordinates
Y
0 BEGIN PGM 20 MM
6.4 Path Contours — Cartesian Coordinates
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+10
4 TOOL CALL 1 Z S4000
5 L Z+250 R0 F MAX
6 L X-20 Y-20 R0 F MAX
7 L Z-5 R0 F1000 M3
8 L X+5 Y+5 RL F300
9 RND R2
10 L Y+85
11 RND R10 F150
12 L X+30
13 CR X+70 Y+95 R+30 DR14 L X+95
15 L Y+40
16 CT X+40 Y+5
17 L X+5
18 RND R2
19 L X-20 Y-20 R0 F1000
20 L Z+250 R0 F MAX M2
21 END PGM 20 MM
95
85
40
5
Define blank form for graphic workpiece simulation
Define tool in the program
Call tool in the spindle axis and with the spindle speed S
Retract tool in the spindle axis at rapid traverse FMAX
Pre-position the tool
Move to working depth at feed rate F = 1000 mm/min
Approach the contour at point 1
Tangential approach to circle with R=2 mm
Point 2: first straight line for corner 2
Insert radius with R = 10 mm, feed rate: 150 mm/min
Move to point 3: Starting point of the arc with CR
Move to point 4: End point of the arc with CR, radius 30 mm
Move to point 5
Move to point 6
Move to point 7: End point of the arc, radius with tangential
connection to point 6, TNC automatically calculates the radius
Move to last contour point 1
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program
R10
5
R30
403070
95
X
76
6 Programming: Programming Contours
Example: Full circle with Cartesian coordinates
Example: Full circle with Cartesian coordinates
Y
0 BEGIN PGM 30 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+12.5
4 TOOL CALL 1 Z S3150
5 CC X+50 Y+50
6 L Z+250 R0 F MAX
7 L X-40 Y+50 R0 F MAX
8 L Z-5 R0 F1000 M3
9 L X+0 Y+50 RL F300
10 RND R2
11 C X+0 DR12 RND R2
13 L X-40 Y+50 R0 F1000
14 L Z+250 R0 F MAX M2
15 END PGM 30 MM
50
Define the workpiece blank
Define the tool
tool call
Define the circle center
Retract the tool
Pre-position the tool
Move to working depth
Approach starting point of circle
Tangential approach to circle with R=2 mm
Move to the circle end point (= circle starting point)
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program
CC
50
X
6.4 Path Contours — Cartesian Coordinates
6.4 Path Contours — Cartesian Coordinates
77HEIDENHAIN TNC 310
6.5Path Contours—
Polar Coordinates
With polar coordinates you can define a position in terms of its
angle PA and its distance PR relative to a previously defined pole
CC. See section ”4.1 Fundamentals of NC.”
Polar coordinates are useful with:
■ Positions on circular arcs
■ Workpiece drawing dimensions in degrees, e.g. bolt hole circles
Circular path around circle center/pole
CC to arc end point
Circular path with tangential
connection to the preceding contour
element
Combination of a circular and a linear
movement
Polar coordinate origin: Pole CC
You can define the pole CC anywhere in the part program before
blocks containing polar coordinates. Enter the pole in Cartesian
coordinates as a circle center in a CC block.
ú Select circle functions: Press the „CIRCLE“ soft key
ú Coordinates CC: Enter Cartesian coordinates for
the pole, or:
If you want to use the last programmed position,
do not enter any coordinates.
Polar radius, polar angle of the
straight-line end point
Polar angle of the arc end point,
direction of rotation
Polar radius, polar angle of the arc
end point
Polar radius, polar angle of the arc
end point, coordinate of the end
point in the tool axis
Y
Y
C
C
CC
78
X
X
CC
6 Programming: Programming Contours
Straight line LP
The tool moves in a straight line from its current position to the
straight-line end point. The starting point is the end point of the
preceding block.
ú Select straight line function: Press the L soft key
ú Select entry of polar coordinates: Press the P soft
key (2nd soft-key row). Polar coordinates-radius PR:
Enter the distance from the pole CC to the straightline end point.
ú Polar-coordinates angle PA: Angular position of the
straight-line end point between –360° and +360°
The sign of PA depends on the angle reference
axis:
Angle from angle reference axis to PR is
counterclockwise: PA>0
Angle from angle reference axis to PR is clockwise:
PA<0
The polar coordinate radius PR is also the radius of the arc. It is
defined by the distance from the starting point to the pole CC. The
last programmed tool position before the CP block is the starting
point of the arc.
ú Select circle functions: Press the „CIRCLE“ soft key
ú Select circular path C: Press the C soft key
ú Select entry of polar coordinates: Press the P soft
key (2nd soft-key row).
ú Polar coordinates angle PA: Angular position of the
12 CC X+40 Y+35
13 L X+0 Y+35 RL F250 M3
14 LP PR+25 PA+120
15 CTP PR+30 PA+30
16 L Y+0
The pole CC is not the center of the contour arc!
35
CC
R25
40
R30
30°
X
80
6 Programming: Programming Contours
Helical interpolation
A helix is a combination of a circular movement in a main plane and
a linear movement perpendicular to this plane.
A helix is programmed only in polar coordinates.
Application
■ Large-diameter internal and external threads
■ Lubrication grooves
Calculating the helix
To program a helix, you must enter the total angle through which
the tool is to move on the helix in incremental dimensions, and the
total height of the helix.
For calculating a helix that is to be cut in a upward direction, you
need the following data:
Z
Y
CC
X
Thread revolutions n
Total height h
Incremental
total angle IPA
Starting coordinate Z
Shape of the helix
The table below illustrates in which way the shape of the helix is
determined by the work direction, direction of rotation and radius
compensation.
Internal thread Work direction Direction Radius compensation
Thread revolutions + thread overrun at
the start and end of the thread
Thread pitch P x thread revolutions n
Thread revolutions x 360° + angle for
beginning of thread + angle for thread
overrun
Thread pitch P x (thread revolutions +
thread overrun at start of thread)
6.5 Path Contours — Polar Coordinates
6.5 Path Contours — Polar Coordinates
81HEIDENHAIN TNC 310
Programming a helix
6.5 Path Contours — Polar Coordinates
Always enter the same algebraic sign for the direction of
rotation DR and the incremental total angle IPA. The tool
may otherwise move in a wrong path and damage the
contour.
For the total angle IPA, you can enter a value from
–5400° to +5400°. If the thread has of more than 15
revolutions, program the helix in a program section
repeat (see section 9.2 ”Program Section Repeats”).
ú Select circle functions: Press the „CIRCLE“ soft key
ú Select circular path C: Press the C soft key
ú Select entry of polar coordinates: Press the P soft
key (2nd soft-key row).
ú Polar coordinates angle: Enter the total angle of
tool traverse along the helix in incremental
dimensions. After entering the angle, identify the
tool axis using a soft key.
ú Enter the coordinate for the height of the helix in
incremental dimensions.
ú Direction of rotation DR
Clockwise helix: DR–
Counterclockwise helix: DR+
ú Radius compensation RL/RR/R0
Enter the radius compensation according to the
table above.
0 BEGIN PGM 40 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+7.5
4 TOOL CALL 1 Z S4000
5 CC X+50 Y+50
6 L Z+250 R0 F MAX
7 LP PR+60 PA+180 R0 F MAX
8 L Z-5 R0 F1000 M3
9 LP PR+45 PA+180 RL F250
10 RND R1
11 LP PA+120
12 LP PA+60
13 LP PA+0
14 LP PA-60
15 LP PA-120
16 LP PA+180
17 RND R1
18 LP PR+60 PA+180 R0 F1000
19 L Z+250 R0 F MAX M2
20 END PGM 40 MM
5
50
Define the workpiece blank
Define the tool
tool call
Define the datum for polar coordinates
Retract the tool
Pre-position the tool
Move to working depth
Approach the contour at point 1
Tangential approach to circle with R=1 mm
Move to point 2
Move to point 3
Move to point 4
Move to point 5
Move to point 6
Move to point 1
Tangential departure from circle with R=1 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program
0 BEGIN PGM 50 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+5
4 TOOL CALL 1 Z S1400
5 L Z+250 R0 F MAX
6 L X+50 Y+50 R0 F MAX
7 CC
8 L Z-12.75 R0 F1000 M3
9 LP PR+32 PA-180 RL F100
10 RND R2
11 CP IPA+3240 IZ+13,5 DR+ F200
12 RND R2
13 L X+50 Y+50 R0 F MAX
14 L Z+250 R0 F MAX M2
15 END PGM 50 MM
50
Define the workpiece blank
Define the tool
tool call
Retract the tool
Pre-position the tool
Transfer the last programmed position as the pole
Move to working depth
Approach contour
Tangential approach to circle with R=2 mm
Helical interpolation
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program
Identify beginning of program section repeat
Enter the thread pitch as an incremental IZ dimension
Program the number of repeats (thread revolutions)
6 Programming: Programming Contours
7
Programming:
Miscellaneous functions
7.1Entering Miscellaneous Functions
M and STOP
With the TNC's miscellaneous functions - also called M functions you can affect:
■ Program run, e.g., a program interruption
■ Machine functions, such as switching spindle rotation and coolant
supply on and off
■ Contouring behavior of the tool
The machine tool builder may add some M functions
that are not described in this User's Manual. Your
machine manual provides more detailed information.
M functions are always entered at the end of a positioning block.
The TNC then displays the following dialog question:
Miscellaneous function M ?
Only enter the number of the M function in the programming
dialog.
In the MANUAL OPERATION operating mode, the M functions are
entered with the M soft key.
Please note that some F functions become effective at the start of
a positioning block, and others at the end.
M functions come into effect in the block in which they are called.
Unless the M function is only effective blockwise, it is canceled in a
subsequent block or at the end of the program. Some M functions
are effective only in the block in which they are called.
7.1 Entering Miscellaneous Functions M and STOP
Entering an M function in a STOP block
If you program a STOP block, the program run or test run is
interrupted at the block, for example for tool inspection. You can
also enter an M function in a STOP block:
ú To program an interruption of program run,
press the STOP key.
ú Enter miscellaneous function M
Example NC block
87 STOP M6
86
7 Programming: Miscellaneous functions
7.2Miscellaneous Functions for Program Run Control, Spindle and
Coolant
MEffect
M00Stop program run
Spindle STOP
Coolant OFF
M01Stop program run
M02Stop program run
Spindle STOP
Coolant OFF
Go to block 1
Clear the status display (dependent
on machine parameter 7300)
M03Spindle ON clockwise
M04Spindle ON counterclockwise
M05Spindle STOP
M06Tool change
Spindle STOP
Program run stop (dependent on
machine parameter 7440)
M08Coolant ON
M09Coolant OFF
M13Spindle ON clockwise
On the scale, a reference mark indicates the position of the scale
reference point.
Machine datum
The machine datum is required for the following tasks:
■ Defining the limits of traverse (software limit switches)
■ Moving to machine-referenced positions (such as tool change
positions)
■ Setting the workpiece datum
X
MP
X (Z,Y)
7.2 Miscellaneous functions for Program Run Control, Spindle and Coolant;
87HEIDENHAIN TNC 310
The distance in each axis from the scale reference point to the
machine datum is defined by the machine tool builder in a machine
parameter.
Standard behavior
The TNC references coordinates to the workpiece datum (see
“Datum setting”).
Behavior with M91 — Machine datum
If you want the coordinates in a positioning block to be referenced
to the machine datum, end the block with M91.
The coordinate values on the TNC screen are referenced to the
machine datum. Switch the display of coordinates in the status
display to REF (see section 1.4 “Status Displays”).
Behavior with M92 — Additional machine datum
In addition to the machine datum, the machine tool
builder can also define an additional machine-based
position as a reference point.
For each axis, the machine tool builder defines the
distance between the machine datum and this additional
machine datum. Refer to the machine manual for more
information.
If you want the coordinates in a positioning block to be based on
the additional machine datum, end the block with M92.
Radius compensation remains the same in blocks that
are programmed with M91 or M92. The tool length,
however, is not compensated.
7.3 Miscellaneous Functions for Coordinate Data
Effect
M91 and M92 are effective only in the blocks in which they are
programmed with M91 or M92.
M91 and M92 become effective at the start of block.
Workpiece datum
The figure at right shows coordinate systems with the machine
datum and workpiece datum.
Z
Z
Y
Y
X
X
M
88
7 Programming: Miscellaneous functions
Loading...
+ hidden pages
You need points to download manuals.
1 point = 1 manual.
You can buy points or you can get point for every manual you upload.