HEIDENHAIN TNC 407 User Manual

Download

Controls on the TNC 407, TNC 415 B and TNC 425

Controls on the visual display unit

Toggle display between machining and programming modes

GRAPHICS TEXT SPLIT SCREEN

Switch-over key for displaying graphics only, program blocks only, or both program blocks and graphics

Soft keys for selecting function in screen

Shift keys for soft keys

Brightness, Contrast

Typewriter keyboard for entering letters and symbols

G F S T M

File names/

YW E T

comments

ISO programs

Machine operating modes

MANUAL OPERATION

EL. HANDWHEEL

POSITIONING WITH MDI

Programming path movements

APPR

DEP

CHF

RND

Approach/depart contour

Straight line

Circle center/pole for polar coordinates

Circle with center point

Circle with radius

Tangential circle

Chamfer

Corner rounding

Tool functions

TOOL

DEF

TOOL CALL

Enter or call tool length and radius

Activate tool radius compensation

Cycles, subprograms and program section repeats

CYCL

DEF

LBL SET

CALL

LBL

CALL

Define and call cycles

Enter and call labels for subprogramming and program section repeats

PROGRAM RUN/SINGLE BLOCK

PROGRAM RUN/FULL SEQUENCE

Programming modes

PROGRAMMING AND EDITING

TEST RUN

Program/file management

PGM

NAME

PGM

CALL

EXT

MOD

Select programs and files

Delete programs and files

Enter program call in a program

Activate external data transfer

Select miscellaneous functions

Moving the cursor and for going directly to blocks, cycles and parameter functions

Move cursor (highlight)

GOTO

Go directly to blocks, cycles and parameter functions

Override control knobs Feed rate Spindle speed

100

STOP

TOUCH PROBE

Enter program stop in a program

Enter touch probe functions in a program

Coordinate axes and numbers, editing

Select coordinate axes or

...

enter them into program

Numbers

Decimal point

Arithmetic sign

Polar coordinates

Incremental dimensions

Q parameters for part families or in mathematical functions

Capture actual position

ENT

END

ENT

Skip dialog questions, delete words

Confirm entry and resume dialog

End block

S %

DEL

F %

Clear numerical entry or TNC message

Abort dialog; delete program sections

TNC Guideline:

From workpiece drawing to program-controlled machining

Step Task TNC Section in

operating mode manual

Preparation

1 Select tools —— ——

2 Set workpiece datum for

coordinate system —— ——

3 Determine spindle speeds

and feed rates —— 12.4

4 Switch on machine —— 1.3

5 Cross over reference marks

6 Clamp workpiece —— ——

7 Set datum /

Reset position display...

7a ... with

7b ... without

8 Enter part program or download 5 to 8

9 Test part program for errors 3.1

10 Test run: Run program block by

11 If necessary: Optimize part

3D Touch Probe or 9.2

3D Touch Probe or 2.3

Entering and testing part programs

over external data interface

block without tool 3.2

program 5 to 8

or 1.3, 2.1

EXT

or or 10

Machining the workpiece

12 Insert tool and run

part program 3.2

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

The TNCs are shop-floor programmable contouring controls for boring machines, milling machines and machining centers with up to 5 axes. It also features oriented spindle stop.

In the TNC, one operating mode for machine movement (machining modes) and one for programming or program testing (programming modes) are always simultaneously active.

The TNC 425

This control features digital control of machine axis speed. The TNC 425 provides high geometrical accuracy, even with complex workpiece surfaces and at high speeds.

The TNC 415 B

The TNC 415 B uses an analog method of speed control in the drive amplifier. All the programming and machining functions of the TNC 425 are also available on the TNC 415 B.

The TNC 407

The TNC 407 uses an analog method of speed control in the drive amplifier. Most programming and machining functions of the TNC 425 are also available on the TNC 407, with the following exceptions:

• Graphics during program run

• Tilting the machining plane

• Three-dimensional radius compensation

• Linear movement in more than three axes

Technical differences between TNCs

TNC 425 TNC 415 B TNC 407

Speed control Digital Analog Analog Block processing time 4 ms 4 ms 24 ms Control loop cycle time:

Position controller 3 ms 2 ms 6 ms Control loop cycle time:

Speed controller 0,6 ms 0.6 ms --Program memory 256 K byte 256 K byte 128 K byte Input resolution 0.1 µm 0.1 µm 1 µm

TNC 425/TNC 415 B/TNC 4071-2

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

Visual display unit and keyboard

The 14-inch color screen displays all the information necessary for effective use of the TNCs’ capabilities. Immediately below the screen are soft keys (keys whose functions are identified on screen) to simplify and improve flexibility of programming.

The keys are arranged on the keyboard in groups according to function: This makes it easier to create programs and to use the TNC’s functions.

Programming

The TNCs are programmed right at the machine with interactive, conversational guidance. If a production drawing is not specially dimensioned for NC, the HEIDENHAIN FK free contour programming makes the necessary calculations automatically. The TNCs can also be programmed in ISO format or in DNC mode.

The TNC function for sectioning programs provides a clearer view of long programs. You can use this function to subdivide a specific program into structural points. The individual structural points are then displayed in the right window of the screen and enable you to recognize the structure of the program at a glance.

Graphics

Interactive graphics show you the contour that you are programming. Workpiece machining can be graphically simulated both during (only TNC 415 B and TNC 425) or before actual machining. Various display modes are available.

Compatibility

The TNCs can execute all part programs that were written on HEIDENHAIN controls TNC 150 B and later.

TNC 425/TNC 415 B/TNC 407 1-3

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

Keyboard

The keys on the TNC keyboard are marked with symbols and abbreviations that make them easy to remember. They are grouped according to the following functions:

Typewriter-style keyboard for entering file names, comments and other texts, as well as programming in ISO format

Numerical input and axis selection

Program and file management

Machine operating modes

The functions of the individual keys are described in the fold-out of the front cover.

Machine panel buttons, e.g.

for your machine tool. In this manual they are shown in gray.

(NC start), are describe in the manual

Programming modes

Dialog initiation

Arrow keys and GOTO jump command

TNC 425/TNC 415 B/TNC 4071-4

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

Visual display unit

Soft keys with context-specific functions, and two shift keys for additional soft-key rows

Brightness control

Contrast control

Switchover between the active programming and machining modes

GRAPHICS TEXT SPLIT SCREEN

SPLIT SCREEN key for switching screen layout (see page 1-6)

Headline

The two selected TNC modes are written in the screen headline: the machining mode to the left and the programming mode to the right. The currently active mode is displayed in the larger box, where the dialog prompts and TNC messages also appear.

Soft keys

The soft keys select functions which are described in the fields immediately above them. The shift keys to the right and left call additional softkey functions. Colored lines above the soft-key row indicate the number of available rows. The line representing the active row is highlighted.

TNC 425/TNC 415 B/TNC 407 1-5

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

Screen layout

You can select the type of display on the TNC screen by pressing the SPLIT SCREEN key and one of the soft keys listed below. Depending on the active mode of operation, you can select:

Mode of operation Screen layout Soft key

MANUAL Display positions only ELECTRONIC HANDWHEEL

POSITIONING WITH MANUAL DATA INPUT Display program blocks only

PROGRAM RUN / FULL SEQUENCE, Display program blocks only PROGRAM RUN / SINGLE BLOCK, TEST RUN

Display positions in the left and STATUS in the right screen window

Display program blocks in the left and STATUS in the right screens window

Display program blocks in the left and program structure in the right screen window

Display program blocks in the left and STATUS in the right screen window

Display program blocks in the left and graphics in the right screen window

Display graphics only

PROGRAMMING AND EDITING Display program blocks only

Display program blocks in the left and program structure in the right screen window

Display program blocks in the left and programming graphics in the right screen window

TNC 425/TNC 415 B/TNC 4071-6

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

Screen layout of modesScreen layout of modes

Screen layout of modes

Screen layout of modesScreen layout of modes

PROGRAMMING AND EDITING

Machining mode

Programming mode is active

Text of the selected program

TEST RUN:

Machining mode

Display of structural points

Soft-key row

Programming mode is active

Text of the selected program

TNC 425/TNC 415 B/TNC 407 1-7

Graphics (or additional status display, or program structure)

Soft-key row

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

MANUAL OPERATION and ELECTRONIC HANDWHEEL modes:

• Coordinates

• Selected axis

• ❊, if TNC is in

operation

• Status display, e.g. feed rate F, miscellaneous function M, Symbols for basic rotation and/or tilted working plane

A machining mode is selected

Programming mode

Additional status display

Soft-key row

PROGRAM RUN / FULL SEQUENCE, PROGRAM RUN / SINGLE BLOCK

A machining mode is selected

Text of the selected program

Status display

Programming mode

Graphics (or additional status display, or program structure)

Soft-key row

TNC 425/TNC 415 B/TNC 4071-8

1 Introduction

1.1 The TNC 425, TNC 415 B and TNC 407

TNC Accessories

3D touch probes

The TNC provides the following features when used in conjunction with a 3D touch probe (see Chapter 9):

• Electronic workpiece locating (compensation of workpiece misalignment)

• Datum setting

• Workpiece measurement during program run

• Digitizing 3D surfaces (option)

• Tool measurement with the TT 110 touch probe

Fig. 1.6: HEIDENHAIN 3D touch probes TS 511 and TS 120

Floppy disk unit

With the HEIDENHAIN FE 401 floppy disk unit you can store programs and tables on diskette. It is also a means of transferring programs which were created on a personal computer.

With the FE 401 you can transfer programs that were written on a PC to the TNC. Very large programs that exceed the storage capacity of the TNC can be “drip fed” block-by-block: The machine executes the transferred blocks and erases them immediately, freeing memory for more blocks from the FE.

Electronic handwheel

Electronic handwheels give you manual control of the axis slides. Similar to a conventional machine tool, the machine slide moves in direct relation to the rotation of the handwheel. A wide range of traverses per handwheel revolution is available.

Portable handwheels such as the HR 330 are connected via cable to the TNC. Integral handwheels such as the HR 130 are built into the machine control panel. An adapter permits connection of up to three handwheels.

Your machine manufacturer can tell you more about the handwheel configuration of your machine.

Fig. 1.7: HEIDENHAIN FE 401 floppy disk unit

Fig. 1.8: The HR 330 electronic handwheel

TNC 425/TNC 415 B/TNC 407 1-9

1 Introduction

1.2 Fundamentals of Numerical Control (NC)

Introduction

This chapter covers the following points:

• What is NC?

• The part program

• Conversational programming

• Reference system

• Cartesian coordinate system

• Additional axes

• Polar coordinates

• Setting a pole at a circle center (CC)

• Datum setting

• Absolute workpiece positions

• Incremental workpiece positions

• Programming tool movements

• Position encoders

• Reference marks

What is NC?

NC stands for “Numerical Control,” that is, control of a machine tool by means of numbers. Modern controls such as the TNC have a built-in computer for this purpose and are therefore called CNC (Computerized Numerical Control).

The part program

The part program is a complete list of instructions for machining a part. It contains, for example, the target position of a tool movement, the path function—how the tool should move toward the target position— and the feed rate. Information on the radius and length of the tool, spindle speed and tool axis must also be given in the program.

Conversational programming

Conversational programming is an especially easy method of writing and editing part programs. From the very beginning, the TNCs from HEIDENHAIN were developed specifically for shop-floor programming by the machinist. This is why they are called TNC, or “Touch Numerical Controls.”

You begin programming each machining step by simply pressing a key. The control then asks for all the information that it needs to execute the step. It points out programming errors that it recognizes.

In addition to conversational programming, you can also program the TNC in ISO format or transfer programs from a central host computer for DNC operation.

TNC 425/TNC 415 B/TNC 4071-10

1 Introduction

0° 90°90°

0°

30°

60°

Greenwich

1.2 Fundamentals of NC

Reference system

In order to define positions one needs a reference system. For example, positions on the earth's surface can be defined absolutely by their geographic coordinates of longitude and latitude. The word from the Latin word for "that which is arranged." The network of longitude and latitude lines around the globe constitutes an absolute reference system—in contrast to the relative definition of a position that is referenced to a known location.

coordinate

comes

Cartesian coordinate system

On a TNC-controlled milling machine, workpieces are normally machined according to a workpiece-based Cartesian coordinate system (a rectangular coordinate system named after the French mathematician and philosopher Renatus Cartesius, who lived from 1596 to 1650). The Cartesian coordinate system is based on three coordinate axes X, Y and Z which are parallel to the machine guideways.

The figure to the 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.

Fig. 1.9: The geographic coordinate system

is an absolute reference system

Fig. 1.10: Designations and directions of the

axes on a milling machine

TNC 425/TNC 415 B/TNC 407 1-11

1 Introduction

1.2 Fundamentals of NC

Additional axes

The TNCs (except TNC 407) can control the machine in more than three axis. The axes U, V and W are secondary linear axes parallel to the main axes X, Y and Z, respectively (see illustration). Rotary axes possible. They are designated as A, B and C.

are also

W+

C+

B+

V+

A+

Polar coordinates

The Cartesian coordinate system is especially useful for parts whose dimensions are mutually perpendicular. For parts containing circular arcs or angles it is often simpler to give the dimensions in polar coordinates. While Cartesian coordinates are three-dimensional and can describe points in space, polar coordinates are two dimensional and describe points in a plane. Polar coordinates have their datum at a circle center (CC), or pole, from which a position is measured in terms of its distance from that pole and the angle of its position in relation to the pole.

You could think of polar coordinates as the result of a measurement using a scale whose zero point is fixed at the datum and which you can rotate to different angles in the plane around the pole.

The positions in this plane are defined by

U+

Fig. 1.11: Direction and designation of

additional axes

Fig. 1.12: Identifying positions on a circular arc with polar coordinates

0°

• the Polar Radius (PR) which is the distance

from the circle center CC to the position, and the

• Polar Angle (PA) which is the size of the

angle between the reference axis and the scale.

TNC 425/TNC 415 B/TNC 4071-12

1 Introduction

1.2 Fundamentals of NC

Setting a pole at a circle center (CC)

The pole is set by entering two Cartesian coordinates. These coordinates also set the reference axis for the polar angle (PA).

Coordinates of the pole Reference axis of the angle

X Y +X Y Z +Y Z X +Z

0°

Fig. 1.13: Polar coordinates and their associated reference axes

Setting the datum

The workpiece drawing identifies a certain prominent point on the workpiece (usually a corner) as the absolute datum and perhaps one or more other points as relative datums. The process of datum setting establishes these points as the origin of the absolute or relative coordinate systems: The workpiece, which is aligned with the machine axes, is moved to a certain position relative to the tool and the display is set either to zero or to another appropriate position value (e.g. to compensate the tool radius).

0°

Fig. 1.14: The workpiece datum serves as

the origin of the Cartesian coordinate system

TNC 425/TNC 415 B/TNC 407 1-13

1 Introduction

1.2 Fundamentals of NC

Example:

Drawings with several relative datums (according to ISO 129 or DIN 406, Part 11; Figure 171)

1225

750

320

125

250

216,5

250

-250

-125

-216,5

125 0

-125

-216,5

-250

150 0

-150

300±0,1

325

450

700

900

950

Example:

Coordinates of the point ➀ :

X = 10 mm Y = 5 mm Z = 0 mm

The datum of the Cartesian coordinate system is located 10 mm away from point ➀ on the X axis and 5 mm on the Y axis.

The 3D Touch Probe System from HEIDENHAIN is an especially convenient and efficient way to find and set datums.

Fig. 1.16: Point ➀ defines the coordinate

system.

TNC 425/TNC 415 B/TNC 4071-14

1 Introduction

Z=15mm

X=20mm

Y=10mm

Z=–15mm

X=10mm

Y=10mm

1.2 Fundamentals of NC

Absolute workpiece positions

Each position on the workpiece is clearly defined by its absolute coordinates.

Example:Example:

Example: Absolute coordinates of the position ➀:

Example:Example:

X = 20 mm Y = 10 mm Z = 15 mm

If you are drilling or milling a workpiece according to a workpiece drawing with absolute coordinates, you are moving the tool to the coordinates.

Incremental workpiece positions

A position can be referenced to the previous nominal position: i.e. the relative datum is always the last programmed position. Such coordinates are referred to as incremental coordinates (increment = “growth”), or also incremental or chain dimensions (since the positions are defined as a chain of dimensions). Incremental coordinates are designated with the prefix I.

Example: Incremental coordinates of the position ➂

referenced to position ➁

Absolute coordinates of the position ➁:

X = 10 mm Y = 5 mm Z = 20 mm

Incremental coordinates of the position ➂:

IX = 10 mm IY = 10 mm IZ = –15 mm

If you are drilling or milling a workpiece according to a workpiece drawing with incremental coordinates, you are moving the tool by the coordinates.

An incremental position definition is therefore a specifically relative definition. This is also the case when a position is defined by the distance-to-go to the target position (here the relative datum is located at the target position). The distance-to-go has a negative sign if the target position lies in the negative axis direction from the actual position.

The polar coordinate system can also express both types of dimensions:

• Absolute polar coordinates

always refer to the

pole (CC) and the reference axis.

• Incremental polar coordinates always refer to the last programmed nominal position of the tool.

Fig. 1.17: Definition of position ➀ through

Fig. 1.18: Definition of positions ➁ and ➂

+IPR

+IPA +IPA

absolute coordinates

through incremental coordinates

0°

TNC 425/TNC 415 B/TNC 407 1-15

Fig. 1.19: Incremental dimensions in polar coordinates (designated

with an "I")

1 Introduction

1.2 Fundamentals of NC

Example: Workpiece drawing with coordinate dimensioning

(according to ISO 129 or DIN 406, Part 11; Figure 179)

2.1

2.2

2.3

3.4

3.5

3.6

3.7 3

3.8

3.9

3.10 Y2

2 1.3

3.3

3.11

3.2

3.1

3.12

1.21.1

Dimensions in mm

Coordinate Origin Pos. X1 X2 Y1 Y2 r

1100 – 1 1,1 325 320 Ø 120 H7 1 1,2 900 320 Ø 120 H7 1 1,3 950 750 Ø 200 H7 1 2 450 750 Ø 200 H7 1 3 700 1225 Ø 400 H8 2 2,1 –300 150 Ø 50 H11 2 2,2 –300 0 Ø 50 H11 2 2,3 –300 –150 Ø 50 H11 3 3,1 250 0° Ø 26 3 3,2 250 30° Ø 26 3 3,3 250 60° Ø 26 3 3,4 250 90° Ø 26 3 3,5 250 120° Ø 26 3 3,6 250 150° Ø 26 3 3,7 250 180° Ø 26 3 3,8 250 210° Ø 26 3 3,9 250 240° Ø 26 3 3,10 250 270° Ø 26 3 3,11 250 300° Ø 26 3 3,12 250 330° Ø 26

Coordinates

ϕϕ

ϕ d

ϕϕ

TNC 425/TNC 415 B/TNC 4071-16

1 Introduction

1.2 Fundamentals of NC

Programming tool movements

During workpiece machining, an axis position is changed either by moving the tool or by moving the machine table on which the workpiece is fixed.

You always program as if the tool is moving and the workpiece is stationary.

If the machine table moves, the axis is designated on the machine operating panel with a prime mark (e.g. X’, Y’). Whether an axis designation has a prime mark or not, the programmed direction of axis movement is always the direction of tool movement relative to the workpiece.

Position encoders

The position encoders – linear encoders for linear axes, angle encoders for rotary axes – convert the movement of the machine axes into electrical signals. The control evaluates these signals and constantly calculates the actual position of the machine axes.

If there is an interruption in power, the calculated position will no longer correspond to the actual position. When power is returned, the TNC can re-establish this relationship.

Reference marks

The scales of the position encoders contain one or more reference marks. When a reference mark is passed over, it generates a signal which identifies that position as the machine axis reference point. With the aid of this reference mark the TNC can re-establish the assignment of displayed positions to machine axis positions.

If the position encoders feature distance-coded reference marks, each axis need only move a maximum of 20 mm (0.8 in.) for linear encoders, and 20° for angle encoders.

Fig. 1.21: On this machine the tool moves in

the Y and Z axes; the workpiece moves in the positive X' axis.

Fig. 1.22: Linear position encoder, here for

the X axis

Fig. 1.23: Linear scales: above with

distance-coded-reference marks, below with one reference mark

TNC 425/TNC 415 B/TNC 407 1-17

1 Introduction

1.3 Switch-on

The switching on and traversing of reference marks are machine tool dependent functions. See your machine tool manual.

Switch on the TNC and machine tool. The TNC automatically initiates the following dialog:

MEMORY TEST

The TNC memory is automatically checked.

POWER INTERRUPTED

TRANSLATE PLC PROGRAM

The PLC program of the TNC is automatically translated.

RELAY EXT. DC VOLTAGE MISSING

MANUAL OPERATION

TRAVERSE REFERENCE POINTS

The TNC is now ready for operation in the MANUAL OPERATION mode.

TNC message indicating that the power was interrupted. Clear the message.

Switch on the control voltage. The TNC checks the function of the EMERGENCY OFF button.

Move the axes in the displayed sequence across the reference marks: For each axis press the START key. Or

Cross the reference points in any direction: Press and hold the machine axis direction button for each axis until the reference point has been traversed.

The reference marks need only be traversed if the machine axes are to be moved. If you intend only to write, edit or test programs, you can select the PROGRAMMING AND EDITING or TEST RUN modes of operation immediately after switching on the control voltage. The reference marks can then be traversed later by pressing the PASS OVER REFERENCE soft key in the MANUAL OPERATION mode.

The reference point of a tilted coordinate system can be traversed by pressing the machine axis direction buttons. The "tilting the working plane" function (see page 2-11) must be active in the manual operating mode. The TNC then interpolates the corresponding axes. The NC START key has no function and if it is pressed the TNC will respond with an ERROR message. Make sure that the angular values entered in the menu correspond with the actual angle of the tilted axis.

TNC 425/TNC 415 B/TNC 4071-18

1 Introduction

1.4 Graphics and Status Displays

In the PROGRAMMING AND EDITING mode of operation the programmed macro is displayed as a two-dimensional graphic. During free contour programming (FK) the programming graphic is interactive.

In the program run (except on TNC 407) and test run operating modes, the TNC provides the following three display modes:

• Plan view

• Projection in three planes

• 3D view

The display mode is selectable via soft key.

On the TNC 415 B and TNC 425, workpiece machining can also be graphically simulated in real time.

The TNC graphic depicts the workpiece as if it is being machined by a cylindrical end mill. If tool tables are used, a spherical cutter can also be depicted (see page 4-10).

The graphics window does not show the workpiece if

• the current program has no valid blank form definition

• no program is selected

With the machine parameters MP7315 to MP7317 a graphic is generated even if no tool axis is defined or moved.

The graphics cannot show rotary axis movements (error message).

Graphics during program run

A graphical representation of a running program is not possible if the microprocessor of the TNC is already occupied with complicated machining tasks or if large areas are being machined.

Example:

Stepover milling of the entire blank form with a large tool.

The TNC interrupts the graphics and displays the text “ERROR” in the graphics window. The machining process is continued, however.

TNC 425/TNC 415 B/TNC 407 1-19

1 Introduction

1.4 Graphics and Status Displays

Plan view

The depth of the workpiece surface is displayed according to the principle “the deeper, the darker.”

Use the soft keys to select the number of depth levels that can be displayed.

• TEST RUN mode: 16 or 32 levels

• PROGRAM RUN modes: 16 or 32 levels

Plan view is the fastest of the three graphic display modes.

Fig. 1.24: TNC graphics, plan view

Switch over soft keys.

Show 16 or 32 shades of depth.

TNC 425/TNC 415 B/TNC 4071-20

1 Introduction

1.4 Graphics and Status Displays

Projection in 3 planes

Similar to a workpiece drawing, the part is displayed with a plan view and two sectional planes. A symbol to the lower left indicates whether the display is in first angle or third angle projection according to ISO 6433 (selectable via MP

7310).

Details can be isolated in this display mode for magnification (see page 1–24).

Shifting planes

The sectional planes can be shifted as desired. The positions of the sectional planes are visible during shifting.

Fig. 1.25: TNC graphics, projection in three planes

Fig. 1.26: Shifting sectional planes

Shift the soft-key row.

Shift the vertical sectional plane to the right or left.

Shift the horizontal sectional plane upwards or downwards.

TNC 425/TNC 415 B/TNC 407 1-21

1 Introduction

1.4 Graphics and Status Displays

Cursor position during projection in 3 planes

The TNC shows the coordinates of the cursor position at the bottom of the graphics window. Only the coordinates of the working plane are shown.

This function is activated with machine parameter MP7310.

Cursor position during detail magnification

During detail magnification, the TNC displays the coordinates of the axis that is currently being moved.

The coordinates describe the area determined for magnification. To the left of the slash is the smallest coordinate of the detail in the current axis, to the right is the largest.

Fig. 1.27: The coordinates of the cursor position are

displayed to the lower left of the graphic

3D view

The workpiece is displayed in three dimensions, and can be rotated around the vertical axis.

The shape of the workpiece blank can be depicted by a frame overlay at the beginning of the graphic simulation.

In the TEST RUN mode of operation you can isolate details for magnification.

Fig. 1.28: TNC graphics, 3D view

TNC 425/TNC 415 B/TNC 4071-22

1 Introduction

1.4 Graphics and Status Displays

To rotate the 3D view:

Shift the soft-key row.

Rotate the workpiece in 27° steps around the vertical axis.

The current angular attitude of the display is indicated at the lower left of the graphic.

To switch the frame overlay display on/off:

Show or omit the frame overlay of the workpiece blank form.

Fig. 1.29: Rotated 3D view

TNC 425/TNC 415 B/TNC 407 1-23

1 Introduction

1.4 Graphics and Status Displays

Magnifying details

You can magnify details in the TEST RUN mode of operation in the

• projection in three planes, and

• 3D view

display modes, provided that the graphical simulation is stopped. A detail magnification is always effective in all three display modes.

To select detail magnification:

Fig. 1.30: Magnifying a detail of a projection in three planes

Shift the soft-key row.

Select the left/right workpiece surface.

Select the front/back workpiece surface.

Select the top/bottom workpiece surface.

Shift sectional plane to reduce/magnify the blank form.

If desired

Select the isolated detail.

Restart the test run or program run.

If a graphic display is magnified, this is indicated with MAGN at the lower right of the graphics window. If the detail in not magnified with TRANSFER DETAIL, you can make a test run of the shifted sectional planes.

If the workpiece blank cannot be further enlarged or reduced, the TNC displays an error message in the graphics window. The error message disappears when the workpiece blank is enlarged or reduced.

TNC 425/TNC 415 B/TNC 4071-24

1 Introduction

1.4 Graphics and Status Displays

Repeating graphic simulation

A part program can be graphically simulated as often as desired, either with the complete workpiece blank or with a detail of it.

Function Soft key

• Restore workpiece blank as it was last shown

• Show the complete BLK FORM as it appeared before a detail was magnified via TRANSFER DETAIL

The WINDOW BLK FORM soft key will return the blank form to its original shape and size, even if a detail has been isolated and not yet magnified with TRANSFER DETAIL.

Measuring the machining time

At the lower right of the graphics window the TNC shows the calculated machining time in

hours: minutes: seconds

(maximum 99 : 59 : 59)

• Program run: The clock counts and displays the time from program start to program end. The timer stops whenever machining is interrupted.

• Test run: The clock shows the time which the TNC calculates for the duration of tool movements.

To activate the stopwatch function:

Fig. 1.31: The calculated machining time is shown at the

lower right of the workpiece graphic

Press the shift keys until the soft-key row with the stopwatch functions appears.

The soft keys available to the left of the stopwatch functions depend on the selected display mode.

TNC 425/TNC 415 B/TNC 407 1-25

1 Introduction

1.4 Graphics and Status Displays

Stopwatch functions Soft key

Store displayed time

Show the sum of the stored time and the displayed time

Clear displayed time

Status displays

During a program run mode of operation the status display contains the current coordinates and the following information:

• Type of position display (ACTL, NOML, ...)

• Number of the current tool T

• Tool axis

• Spindle speed S

• Feed rate F

• Active M functions

• “Control in operation” symbol: ❊

• “Axis is locked” symbol:

• Axis can be moved with the handwheel:

• Axes are moving in a tilted working plane:

• Axes are moving under a basic rotation:

Additional status displays

The additional status displays contain further information on the program run.

To select additional status displays:

Fig. 1.32: Status display in a program run mode of operation

Set the STATUS soft key to ON.

Shift the soft-key row.

TNC 425/TNC 415 B/TNC 4071-26

1 Introduction

1.4 Graphics and Status Displays

Additional status display Soft key

General program information

Positions and coordinates

Tool information

Coordinate transformations

Tool measurement

General program information

Positions and coordinates

Name of main program

Active programs

Cycle definition

Dwell time counter

Machining time

Circle center CC (pole)

Type of position display

Coordinates of the axes

Tilt angle of the working plane

Display of a basic rotation

TNC 425/TNC 415 B/TNC 407 1-27

1 Introduction

1.4 Graphics and Status Displays

Tool information

T: Tool name and number RT: Name and number of a replacement tool

Tool axis

Tool length and radii

Oversizes (delta values)

Tool life, maximum tool life and maximum tool life for TOOL CALL

Display of the programmed tool and the (next) replacement tool

Coordinate transformations

Tool measurement

Main program name

Coordinates of the datum shift

Angle of basic rotation

Mirrored axis

Scaling factor(s)

Scaling datum

Number of the tool to be measured

Measured MIN and MAX values of the single cutting edges and the result of measuring the rotating tool

Display whether the tool radius or the tool length is being measured

When working with the TT 110: Cutting edge number with the corresponding measured value. If the measured value is followed by an asterisk, the allowable tolerance defined in the tool table was exceeded.

TNC 425/TNC 415 B/TNC 4071-28

1 Introduction

1.5 Interactive Programming Graphics

The TNC’s two-dimensional interactive graphics generates the part contour as it is being programmed.

The TNC provides the following features with the interactive graphics for the PROGRAMMING AND EDITING operating mode:

• Detail magnification

• Detail reduction

• Block number display ON/OFF

• Restoring incomplete lines

• Clearing the graphic

• Interrupting graphics

The graphic functions are selected exclusively with soft keys.

To work with interactive graphics you must switch the screen layout to PGM + GRAPHICS (see page 1-6).

To generate graphics during programming:

Fig. 1.37: Interactive graphics

AUTO DRAW ON does not simulate program section repeats.

Shift the soft-key row.

Select/deselect graphic generation during programming. The default setting is OFF.

Generating a graphic for an existing program

To generate a graphic up to a certain block:

GOTO

e.g.

4 7

TNC 425/TNC 415 B/TNC 407 1-29

Select the desired block with the vertical cursor keys.

Enter the desired block number, e.g. 47.

Generate a graphic from block 1 to the entered block. The AUTO DRAW soft key must be set to ON.

1 Introduction

1.5 Interactive Programming Graphics

Function Soft key

• Generate interactive graphic blockwise

• Generate a complete graphic or complete it after RESET + START

• Interrupt interactive graphics

The STOP soft key appears while the TNC generates the interactive graphic.

To magnify/reduce a detail:

Fig. 1.38: Detail from an interactive graphic

Shift the soft-key row.

Show the frame overlay and move vertically.

Show the frame overlay and move horizontally.

. . .

TNC 425/TNC 415 B/TNC 4071-30

1 Introduction

1.5 Interactive Programming Graphics

. . .

To undo a change in the section area:

To erase the graphic:

Reduce or enlarge the frame overlay.

Confirm the selected section.

Restore the original section.

Shift the soft key row.

Block number display ON/OFF

Erase the graphic.

Fig. 1.39: Text with block numbers

Show or omit block numbers in the program text display.

TNC 425/TNC 415 B/TNC 407 1-31

1 Introduction

1.6 Files

Programs, texts and tables are written as files and stored in the TNC.

A file is identified by PROG15 .H

File name File type

To open a new file you must enter a file name consisting of from one to 16 characters (letters and numbers), depending on MP7222.

The file types are listed in the table at right.

File directory

The TNC can store up to 100 files at one time. You can call up a directory of these programs by pressing the PGM NAME key. To delete one or more programs, press the CL PGM key.

The file directory contains the following information:

• File name

• File type

• File size in bytes (=characters)

• File status

Further information is shown at the top of the screen:

• Selected file storage

- TNC memory

- External storage via RS-232 interface

- External storage via RS-422

• Interface mode, e.g. FE1, EXT1 for external storage

• File type, e.g. ❊ .H is shown if only HEIDENHAIN dialog programs are shown

Files in the TNC Type

Programs

• in HEIDENHAIN plain language dialog .H

• according to ISO .I

Tables for

• Tools .T

• Pallets .P

• Datums .D

• Contour points (TM 110 digitizing range) .PNT

Texts as

• ASCII files .A

Fig. 1.40: TNC file types

File.. Mode of Call file direc-

operation tory with . . .

PGM

... create new file ...

... edit ...

... erase ...

... test ...

... execute ...

Fig. 1.41: File management functions

NAME

PGM

NAME

PGM

NAME

PGM

NAME

Example:

RS 422/EXT1: ❊ .T is displayed. This means that only those files are shown that have the extension .T and are located in an external storage device, (e.g. a PC), that is connected to the TNC through the RS-422 interface (see also Chapter 10).

A soft key calls the file directory of an external data storage medium. The screen is then divided into two columns.

Select the file directory:

Show the file directory in one or two columns. The selected layout is shown in the soft key.

Fig. 1.42: Files are sorted alphabetically and according to

type

TNC 425/TNC 415 B/TNC 4071-32

1 Introduction

1.6 Files

File status

The letters in the STATUS column give the following information about the files:

E: File is selected in the PROGRAMMING AND EDITING mode of

operation S: File is selected in the TEST RUN operating mode M: File is selected in a program run operating mode P: File is protected against editing and erasure IN: File contains inch dimensions W: File has been transferred to external storage and cannot be run

Selecting a file

PGM

NAME

Call the file directory.

At first only HEIDENHAIN dialog (type .H) files are shown. Other files are shown via soft key:

Select the file type.

Show all files.

You select a file by moving the highlight bar:

Function Key / Soft key

• Move the highlight bar vertically to the desired file

• Move pagewise down/up through the file directory

• Select the highlighted file

TNC 425/TNC 415 B/TNC 407 1-33

1 Introduction

1.6 Files

To copy a file:

Mode of operation: PROGRAMMING AND EDITING.

Move the highlight bar to the file that you wish to copy, for example a type .H file.

DESTINATION FILE = . H

Type the new file name into the highlight bar in the screen headline, the file type remains unchanged.

To erase a file:

You can erase files in the PROGRAMMING AND EDITING operating mode.

PGM

NAME

ENT

Call the file directory.

Select the copying function.

Copy the file. The original file is not deleted.

PGM

Call the file directory.

Move the highlight to the file that you wish to delete.

Erase the file.

To erase a protected file:

A protected file (status P) cannot be erased. If you are sure that you wish to erase it, you must first remove the protection (see p. 1-35, “To cancel file protection”).

TNC 425/TNC 415 B/TNC 4071-34

1 Introduction

1.6 Files

Protecting, renaming, and converting files

In the PROGRAMMING AND EDITING operating mode you can:

• convert files from one type to another

• rename files

• protect files from editing and erasure

PGM

NAME

Call the program directory.

Switch the soft-key row.

To protect a file:

The file receives the status P and cannot be accidentally changed or erased.

Move the highlight to the file that you wish to protect.

Press the PROTECT soft key. The file is then protected. The protected file is displayed in bright characters.

To cancel file protection:

Move the highlight to the file with status P whose protection you wish to remove.

Press the UNPROTECT soft key.

CODE NUMBER =

75368

ENT

Type the code number 86357 into the highlight bar in the screen headline.

Cancel the file protection. The file no longer has the status P.

You can unprotect other files by simply marking them and pressing the UNPROTECT soft key.

TNC 425/TNC 415 B/TNC 407 1-35

1 Introduction

1.6 Files

To rename a file:

Move the highlight to the file that you wish to rename.

DESTINATION FILE = . H

Type the new file name into the highlight in the screen headline. The file type cannot be changed.

Press the RENAME soft key.

ENT

Rename the file.

To convert a file:

Text files (type .A) can be converted to all other types. Other types can be converted only into ASCII text files. They can then be edited with the alphanumeric keyboard.

Part programs that were created with FK free contour programming can also be converted to HEIDENHAIN dialog programs.

Move the highlight to the file that you wish to convert.

Press the CONVERT soft key.

Select the new file type, here an ASCII text file (type .A).

DESTINATION FILE = . A

Type the new file name into the highlight bar in the screen headline.

ENT

Convert the file.

TNC 425/TNC 415 B/TNC 4071-36

1 Introduction

1.6 Files

File management for files on an external data medium

You can erase and protect files stored on the FE 401B floppy disk unit from HEIDENHAIN. You can also format a floppy disk from the TNC. To do this you must first select the PROGRAMMING END EDITING mode of operation.

EXT

To erase a file on the FE 401B

Call the program directory for external files.

Move the highlight to the right onto the external file.

Select one-window mode.

Move the highlight to the unwanted file.

Erase the file in the highlight.

To protect or unprotect a file on FE 401B

Switch to the next soft-key row.

Files are protected with the PROTECT soft key; file protection is removed with the UNPROTECT soft key. The functions for setting and removing file protection are the same as for files stored in the TNC (see p. 1-35).

TNC 425/TNC 415 B/TNC 407 1-37

1 Introduction

1.6 Files

To format a floppy disk in the FE 401 B

NAME OF DISKETTE =

Switch to the next soft-key row.

Select the formatting function.

e.g.

To convert and transfer files

The CONVERT soft key is only available if the selected file is in the memory of the TNC, i.e. if it is displayed on the left side of the screen.

ENT

EXT

Enter a name and start formatting with ENT.

Call the program directory of the external data medium.

Switch the soft-key row.

DESTINATION FILE =

e.g.

ENT

Convert file and save it on the external data medium.

Select the type of the target file, e.g. .A.

Enter the new file name and start conversion with ENT.

TNC 425/TNC 415 B/TNC 4071-38

2 Manual Operation and Setup

2.1 Moving the Machine Axes

Traversing with the machine axis direction buttons:

Traversing with the machine axis direction buttons depends on the individual machine tool. See your machine tool manual.

MANUAL OPERATION

e.g.

You can move several axes at once in this way.

For continuous movement:

MANUAL OPERATION

e.g.

together

You can move several axes at a time in this way.

Press the machine axis direction button and hold it as long as you wish the axis to move.

Press and hold the machine axis direction button, then press the machine start button: The axis continues to move after you release the keys.

To stop the axis, press the machine STOP button.

TNC 425/TNC 415 B/TNC 4072-2

2 Manual Operation and Setup

2.1 Moving the Machine Axes

Traversing with the electronic handwheel:

ELECTRONIC HANDWHEEL

INTERPOLATION FACTOR: X = 3

e.g.

Now move the selected axis with the electronic handwheel. If you are using the portable handwheel, first press the enabling switch on its side.

Interpolation

factor

0 1

2 3 4

5 6 7

8 9

Traverse in mm per

revolution

ENT

20.000

10.000

5.000

2.500

1.250

0.625

0.312

0.156

0.078

0.039

0.019

Enter the interpolation factor (see table).

Select the axis that you wish to move: for portable handwheels at the handwheel, for integral handwheels at the TNC keyboard.

The smallest programmable interpolation factor depends on the individual machine tool. See your machine tool manual. It is also possible to move the axes with the handwheel during a program run (see page 5-70).

Using the HR 330 electronic handwheel

The HR 330 is equipped with an enabling switch. The enabling switch is located opposite the side with the knob and the EMERGENCY STOP switch. The machine axes can only be moved when the enabling switch is depressed.

• The enabling switch is automatically depressed when the handwheel is mounted on the machine.

• Mount the handwheel on the machine on the magnetic pads such that it cannot be operated unintentionally.

• When you remove the handwheel from its position, be careful not to accidentally press the axis direction keys while the enabling switch is still depressed.

Fig. 2.2: HR 330 electronic handwheelFig. 2.1: Interpolation factors for handwheel speed

TNC 425/TNC 415 B/TNC 407 2-3

2 Manual Operation and Setup

2.1 Moving the Machine Axes

Incremental jog positioning

If your machine tool has been set for incremental jog positioning, a machine axis will move by a preset increment each time you press the corresponding machine axis direction button.

8 8

Fig. 2.3: Incremental jog positioning in the

ELECTRONIC HANDWHEEL

INTERPOLATION FACTOR: X = 4

Select incremental jog positioning by pressing the key as determined

by the machine tool builder, e.g.

ELECTRONIC HANDWHEEL

JOG-INCREMENT: 4 8

e.g.

ENT

Enter the jog increment (here 8 mm).

Press the machine axis direction button as often as desired.

X axis

816

• Incremental jog positioning must be enabled by the machine tool manufacturer, see your machine tool manual.

• The machine manufacturer determines whether the interpolation factor for each axis is set at the keyboard or through a manual switch.

Positioning with manual data input (MDI)

Machine axis movements can also be programmed in the $MDI file (see page 5-74).

Since the programmed movements are stored in memory, you can recall them and run them afterward as often as desired.

TNC 425/TNC 415 B/TNC 4072-4

2 Manual Operation and Setup

100

15050

S %

100

15050

F %

2.2 Spindle Speed S, Feed Rate F and Miscellaneous Functions M

These are the soft keys in the MANUAL OPERATION and ELECTRONIC HANDWHEEL modes:

With these functions and with the override knobs on the TNC keyboard you can change and enter:

• the spindle speed S

• the feed rate F (can be changed but not entered)

• miscellaneous functions M

These functions are entered directly in a part program in the PROGRAMMING AND EDITING mode.

To enter the spindle speed S:

The machine manufacturer determines what spindle speeds S are available on your TNC. See your machine tool manual.

SPINDLE SPEED S =

e.g.

1 0 0 0

The spindle speed S with the entered rpm is started with an M function.

To change the spindle speed S

ENT

Fig. 2.4: Knobs for spindle speed and feed

rate overrides

Select S for spindle speed.

Enter the desired spindle speed (here 1000 rpm).

Press the machine START button to confirm the entered spindle speed.

100

15050

S %

The override knob for spindle speed can only vary the spindle speed on machines with a stepless spindle drive.

Turn the knob for spindle speed override: You can vary the speed from 0 to 150% of the last valid speed.

TNC 425/TNC 415 B/TNC 407 2-5

2 Manual Operation and Setup

2.2 Spindle Speed S, Feed Rate F and Miscellaneous Functions M

To change the feed rate F

In the MANUAL OPERATION mode the feed rate is set by a machine parameter.

100

15050

F %

Turn the knob for feed rate override. You can vary the feed rate from 0% to 150% of the set value.

To enter a miscellaneous function M

The machine manufacturer determines which M functions are available on your TNC and what functions they have.

Select M for miscellaneous function.

MISCELLANEOUS FUNCTION M =

e.g.

ENT

Chapter 12 contains a list of M functions.

Enter the miscellaneous function (here M6).

Press the machine START button to activate the miscellaneous function.

TNC 425/TNC 415 B/TNC 4072-6

2 Manual Operation and Setup

2.3 Setting the Datum Without a 3D Touch Probe

You fix a datum by setting the TNC position display to the coordinates of a known point on the workpiece. The fastest, easiest and most accurate way of setting the datum is by using a 3D touch probe system from HEIDENHAIN (see page 9-11).

To prepare the TNC:

Clamp and align the workpiece.

Insert the zero tool with known radius into the spindle.

Select the MANUAL OPERATION mode.

Ensure that the TNC is showing the actual values (see page 11-9).

Setting the datum in the tool axis

Fragile workpiece? If the workpiece surface must not be scratched,

you can lay a metal shim of known thickness d on it. Then enter a tool axis datum value that is larger than the desired datum by the value d.

Move the tool until it touches the workpiece surface.

e.g.

Fig. 2.5: Workpiece setting in the tool axis: right with protective

Select the tool axis.

shim.

DATUM SET Z =

e.g.

TNC 425/TNC 415 B/TNC 407 2-7

ENT

Zero tool: Set the display to Z = 0 or enter the thickness d of the shim.

Preset tool: Set the display to the length L of the tool, (here Z= 50 mm) or enter the sum Z=L+d.

2 Manual Operation and Setup

2.3 Setting the Datum Without a 3D Touch Probe

To set the datum in the working plane:

Move the zero tool until it touches the side of the workpiece.

e.g.

DATUM SET X =

Fig. 2.6: Setting the datum in the working plane; plan view (upper

Select the axis (here X).

right)

–R

e.g.

Repeat the process for all axes in the working plane.

ENT

Enter the position of the tool center (here X = -5 mm) including the proper sign.

TNC 425/TNC 415 B/TNC 4072-8

2 Manual Operation and Setup

2.4 Tilting the Working Plane (not on TNC 407)

The functions for tilting the working plane are adapted to the TNC and the machine by the machine manufacturer.

The TNC supports machine tools with swivel heads (the tool is tilted) and/or swivel tables (the workpiece is tilted).

The program is written as usual in a main plane, such as the X/Y plane, but is executed in a plane that is tilted relative to the main plane.

Typical applications for this function:

• Oblique holes

• Contours in an oblique plane

There are two ways to tilt the working plane:

• 3D ROT soft key in the MANUAL OPERATION and ELECTRONIC HANDWHEEL operation modes

• Cycle 19 WORKING PLANE in the part program (see page 8-55)

The TNC functions for tilting the working plane are coordinate transformations. The transformed tool axis (i.e., as calculated by the TNC) always remains parallel to the actual tool axis (the axis corresponding to the positioning). The working plane is always perpendicular to the direction of the tool axis.

When tilting the working plane, the TNC differentiates between two machine types:

• Machines with swivel tables

• Machines with swivel heads

For machines with swivel tables:

• You must bring the workpiece into the desired position for machin-

ing by positioning the swivel table, for example with an L block.

• The position of the transformed tool axis does not change in relation

to the machine-based coordinate system. Thus for example if you rotate the swivel table – and therefore the workpiece – by 90°, the coordinate system does not rotate. If you press the Z+ axis direction button in the MANUAL OPERATION mode, the tool moves in Z+ direction.

• In calculating the transformed coordinate system the TNC considers

only the mechanically influenced offsets of the particular swivel table (the so-called "translational" components).

For machines with swivel heads:

• You must bring the tool into the desired position for machining by

positioning the swivel head, for example with an L block.

• The position of the transformed tool axis (like the position of the tool)

changes in relation to the machine-based coordinate system. Thus for example if you rotate the swivel head – and therefore the tool – in the B axis by +90°, the coordinate system rotates also. If you press the Z+ axis direction button in the MANUAL OPERATION mode, the tool moves in X+ direction of the machine-based coordinate system.

• In calculating the transformed coordinate system the TNC considers

both the mechanically influenced offsets of the particular swivel head (the so-called "translational" components) and the offsets caused by tilting of the tool (3D tool length compensation).

TNC 425/TNC 415 B/TNC 407 2-9

2 Manual Operation and Setup

2.4 Tilting the Working Plane (not on TNC 407)

Traversing the reference marks in tilted axes

With tilted axes, you use the machine axis direction buttons to cross over the reference marks. The TNC interpolates the corresponding axes. Be sure that the function for tilting the working plane is active in the manual operating mode and the actual angle of the angular axis was entered in the menu field (see page 2-11).

Setting the datum in a tilted coordinate system

After you have positioned the tilted axes, set the datum in the same way as for non-tilted axes—either manually by touching the workpiece with the tool (see page 2-7) or, much more easily, by allowing the part program to automatically set the datum with the aid of the HEIDENHAIN 3D touch probe system (see page 9-11).

The TNC then converts the datum for the tilted coordinate system. The angular values for this calculation are taken from the menu for manual tilting, regardless of whether the tilting function is active or not.

The angle values entered in the menu for manual tilting (see page 2-11) must match the actual position of the angular axes. Otherwise the TNC will calculate an incorrect datum.

Position display in the tilted system

The positions displayed in the status window (NOML and ACTL) are in the tilted coordinate system.

Limitations on working with the tilting function

• The touch probe function BASIC ROTATION cannot be used.

• PLC positioning (determined by the machine tool builder) is not possible.

TNC 425/TNC 415 B/TNC 4072-10

2 Manual Operation and Setup

2.4 Tilting the Working Plane (not on TNC 407)

To activate manual tilting

Select menu for manual tilting.

Select the tilt axis.

Enter the tilt angle, here 45°.

Set TILT WORKING PLANE to ACTIVE.

e.g.

oder

ENT

Terminate input.

A symbol for the tilted plane is shown in the status display whenever the TNC is moving the machine axes in the tilted plane.

If you set the function TILT WORKING PLANE for the operating mode PROGRAM RUN to ACTIVE, the tilt angle entered in the menu becomes active in the first block of the part program. If you are using cycle 19 WORKING PLANE in the part program, the angle values defined in the cycle (starting at the cycle definition) are effective. Angle values entered in the menu will then be overwritten.

To reset

Set TILT WORKING PLANE to INACTIVE.

Fig. 2.7: Menu for manual tilting in the MANUAL

OPERATION mode

TNC 425/TNC 415 B/TNC 407 2-11

3 Test Run and Program Run

3.1 Test Run

In the TEST RUN mode of operation the TNC checks programs and program sections for the following errors without moving the machine axes:

• Geometrical incompatibility

• Missing data

• Impossible jumps

The following TNC functions can be used in the TEST RUN operating mode:

• Blockwise test run

• Test interruption at any block

• Optional block skip

• Blockwise transfer of very long programs from external storage

• Functions for graphic simulation

• Measuring machining time

• Additional status display

To run a program test:

• If the central tool file is active, the tool table for the program test must have the status S (see page 1-33).

• With the SET DATE MOD function you can activate a working-time control for the program test (see page 11-8).

TEST RUN

Select the program in the file directory.

GOTO

Functions Soft key

• Test the entire program

• Test each block individually

• Show the blank form and test the entire

program

ENT

Go to the program beginning.

3-2

• Interrupt the test run

TNC 425/TNC 415 B/TNC 407

3 Test Run and Program Run

3.1 Test Run

To do a test run up to a certain block:

With the STOP AT N function the TNC does a test run up to a certain block with the block number N.

Select the TEST RUN mode and go to the program beginning.

STOP AT: N =

PROGRAM =

REPETITIONS =

Select a partial test run.

ENT

e.g.

1 2 3

e.g.

The display functions for test run

In the TEST RUN operating mode the TNC offers functions for displaying a program in pages.

Enter the block number N at which you wish the test to stop.

Enter the name of the program that contains the block with the block number N.

If N is located in a program section repetition, enter the number of repetitions that you wish to run.

Test the program up to the entered block.

Shift the soft-key row.

Function Soft key

• Go back in the program by one screen page

• Go forward in the program by one screen page

• Go to the program beginning

• Go to the program end

TNC 425/TNC 415 B/TNC 407 3-3

3 Test Run and Program Run

3.2 Program Run

In the PROGRAM RUN / FULL SEQUENCE mode of operation the TNC executes a part program continuously to its end or up to a program stop.

In the PROGRAM RUN / SINGLE BLOCK mode of operation you execute each block separately by pressing the machine START BUTTON.

The following TNC functions can be used during a program run:

• Interrupt program run

• Start program run from a certain block

• Blockwise transfer of very long programs from external storage

• Block skip

• Editing and using the tool table TOOL.T

• Checking/changing Q parameters

• Functions for graphic simulation

• Additional status display.

To run a part program:

• Clamp the workpiece to the machine table.

• Set the datum.

• Select the necessary tables and pallet files.

PROGRAM RUN / SINGLE BLOCK

PROGRAM RUN / FULL SEQUENCE

Select the part program and the necessary tables and pallet files in the file directory.

GOTO

ENT

Only in mode

PROGRAM RUN /

SINGLE BLOCK

Go to the first block of the program.

Run the part program.

Run each block of the part program separately.

3-4

for each block

Feed rate and spindle speed can be changed with the override knobs. You can superimpose handwheel positioning onto programmed axis movements during program run (see page 5-70).

TNC 425/TNC 415 B/TNC 407

3 Test Run and Program Run

3.2 Program Run

Interrupting machining

There are various ways to interrupt a program run:

• Programmed interruptions

• Machine STOP key

• Switching to PROGRAM RUN / SINGLE BLOCK

If the TNC registers an error during program run, it automatically interrupts machining.

Programmed interruptions

Interruptions can be programmed directly in the part program. The part program is interrupted at a block containing one of the following entries:

• STOP

• Miscellaneous function M0, M02 or M30

• Miscellaneous function M06, if the machine tool builder has assigned it a stop function

To interrupt or abort machining immediately:

The block which the TNC is currently executing is not completed.

Interrupt machining.

The ❊ sign in the status display blinks.

The part program can be aborted with the INTERNAL STOP function.

Abort machining.

The ❊ sign in the status display goes out.

To interrupt machining at the end of the current block:

You can interrupt the program run at the end of the current block by switching to the PROGRAM RUN / SINGLE BLOCK mode.

Select PROGRAM RUN / SINGLE BLOCK.

TNC 425/TNC 415 B/TNC 407 3-5

3 Test Run and Program Run

3.2 Program Run

Moving machine axes during an interruption

You can move the machine axes during a program interruption in the same way as in the MANUAL OPERATION mode. Simply enable the machine axis direction buttons by pressing the MANUAL OPERATION soft key.

Example: retracting the spindle after a tool breaks

Interrupt machining.

Enable the machine axis direction buttons.

e.g.

On some machines you may have to press the machine START button after the MANUAL OPERATION soft key to enable the axis direction buttons. See your machine tool manual.

Move the axes with the machine axis direction buttons.

Resuming program run after an interruption

• If a program run is interrupted during a fixed cycle, the program must be resumed from the beginning of the cycle. This means that some machining operations will be repeated.

• If the program run is interrupted during a program section repeat or during a subprogram, you must use the function RESTORE POS AT N to resume program run from the same point.

When a program run is interrupted the TNC stores:

• The data of the last called tool

• Active coordinate transformations

• The coordinates of the last defined circle center

The stored data are used for returning the tool to the contour after manual machine axis positioning during an interruption (RESTORE POSITION).

3-6

Resuming program run with the START button.

You can resume program run by pressing the machine START button if the program was interrupted in one of the following ways:

• Pressing the machine STOP button

• A programmed interruption

TNC 425/TNC 415 B/TNC 407

3 Test Run and Program Run

3.2 Program Run

Resuming program run after an error

• If the error message is not blinking:

Remove the cause of the error.

Clear the error message from the screen.

Restart the program, or resume program run at the place at which it was interrupted.

• If the error message is blinking:

ON0I

OFF

Switch off the TNC and the machine.

Remove the cause of the error.

Start again.

• If you cannot correct the error:

Write down the error message and contact your repair service agency.

TNC 425/TNC 415 B/TNC 407 3-7

3 Test Run and Program Run

3.2 Program Run

Mid-program startup

The RESTORE POS AT N function must be enabled by the machine tool manufacturer.

With the RESTORE POS AT N feature (block scan) you can run a part program beginning at any desired block. The TNC internally scans the program blocks up to that point. The workpiece machining can be graphically simulated.

If a part program has been interrupted with an INTERNAL STOP, the TNC automatically offers the interrupted block N for mid-program startup.

• Mid-program startup must not begin in a subprogram.

• All necessary programs, tables and pallet files must be selected in a program run

mode of operation.

• If the part program contains a programmed interruption before the startup block, the

block scan is interrupted. Press the machine START key to continue the block scan.

• After a block scan, return the tool to the calculated position with RESTORE

POSITION.

• If a program is nested, you can use machine parameter 7680 to determine whether the block scan should

start at block 0 of the main program or at block 0 of the last interrupted program.

GOTO

ENT

START-UP AT: N =

PROGRAM =

REPETITIONS =

3 4

ENT

e.g.

1 8

Go to the first block of the current program to start a block scan.

Select mid-program startup.

Enter the block number N at which the block scan should end.

Enter the name of the program containing the block N.

If block N is located in a program section repetition, enter the number of repetitions to be calculated in the block scan.

Start the block scan.

3-8

Return to the contour (see next page).

TNC 425/TNC 415 B/TNC 407

3 Test Run and Program Run

3.2 Program Run

Returning to the contour

With the RESTORE POSITION function, the TNC returns the tool to the workpiece contour in the following situations:

• Return to contour after the machine axes were moved during a

program interruption

• Return to the position that was calculated for mid-program startup

Select a return to contour.

Move the axes in the sequence that the TNC proposes on the screen.

Move the axes in any sequence.

. . .

Resume machining.

TNC 425/TNC 415 B/TNC 407 3-9

3 Test Run and Program Run

3.3 Optional Block Skip

In a test run or program run, the TNC can skip over blocks that you have programmed with a "/" character.

This function does not work for TOOL DEF blocks.

Shift the soft-key row.

Run or test the program with/without blocks preceded by a "/".

3-10

TNC 425/TNC 415 B/TNC 407

3 Test Run and Program Run

3.4 Blockwise Transfer: Testing and Executing Long Programs

Part programs that occupy more memory than the TNC provides can be "drip fed" block by block from an external storage device.

During program run, the TNC transfers program blocks from a floppy disk unit or PC through its data interface, and erases them after execution. This frees memory space for new blocks. Coordinate transformations remain active even when the cycle definition is erased.

To prepare for blockwise transfer:

• Configure the data interface with the MOD function RS-232/422-SETUP (see page 11-4).

• If you wish to transfer a part program from a PC, adapt the TNC and PC to each other (see pages 10-5 and 12-3).

• Ensure that the transferred program meets the following requirements:

- The program must not contain subprograms.

- The program must not contain program

section repetitions.

- All programs that are called from the trans-

ferred program must be selected (Status M).

Fig. 3.1: TNC screen during blockwise transfer

PROGRAM RUN / SINGLE BLOCK

PROGRAM RUN / FULL SEQUENCE

TEST RUN

EXT

Select the program.

PROGRAM RUN:

Show directory of files in external storage. The soft-key row shifts.

Start data transfer.

Transfer and execute the program blocks.

TEST RUN:

Transfer and test the program blocks.

If the data transfer is interrupted, press the START key again.

TNC 425/TNC 415 B/TNC 407 3-11

3 Test Run and Program Run

3.4 Blockwise Transfer: Testing and Executing Long Programs

Jumping over blocks

The TNC can jump over blocks to begin transfer at any desired block. These blocks are then ignored during a program run or test run.

Select the program and start data transfer.

GOTO

e.g.

1 5 0

PROGRAM RUN:

ENT

Go to the block number at which you wish to begin data transfer, for example 150.

Execute the transferred blocks, starting with the block number that you entered.

TEST RUN:

A tool can be replaced automatically if the maximum tool life (TIME1 or TIME2) has been reached (see page 4-16).

You can use machine parameters (see page 12-11) to define the memory range to be used during blockwise transfer. This prevents the transferred program from filling the program memory and disabling the background programming feature.

As an alternative, you can call the external program with CALL PGM EXT (see page 6-8) and perform a mid-program startup (see page 3-8).

Example: To perform a mid-program start-up from block 12834 of external

program GEH35K1 proceed as follows:

Test the transferred blocks, starting with the block number that you entered.

– Write the following short program:

0 BEGIN PGM START-UP MM 1 CALL PGM EXT:GEH35K1 2 END PGM START-UP MM

– Select the START-UP program in the PROGRAM RUN/FULL SEQUENCE mode of operation.

– Select the RESTORE POS AT N function and enter the desired block number, here 12834, for START-UP AT and the

desired program, here GEH35K1, for PROGRAM.

– Start block scan with the NC START key.

3-12

TNC 425/TNC 415 B/TNC 407

4 Programming

In the PROGRAMMING AND EDITING mode of operation (see page 1-32) you can

• create files,

• add to files, and

• edit files.

This chapter describes the basic functions and input that do not yet cause machine axis movement. The entry of geometry for workpiece machining is described in the next chapter.

4.1 Creating Part Programs

Layout of a program

A part program consists of individual program blocks. The TNC numbers the blocks in ascending sequence. Program blocks contain units of information called

words

Block:

10 L X+10 Y+5 R0 F100 M3

Plain language dialog

You initiate a dialog for conversational programming by pressing a function key (see inside front cover). The TNC then asks you for all the information necessary to program the desired function. After you have answered all the questions, the TNC automatically ends the dialog.

If only a few of the words in a block need be programmed, you can cut off the dialog and end the block before the dialog is finished.

Function Key

• Continue the dialog

• Ignore the dialog question

Path function Block Words number

Fig. 4 1: Program blocks contain words of specific information

ENT

• End the dialog immediately

• Abort the dialog and erase the block

END

DEL

TNC 425/TNC 415 B/TNC 4074-2

4 Programming

4.1 Creating Part Programs

Editing functions

Editing means entering, adding to or changing commands and information for the TNC.

The TNC enables you to

• Enter data with the keyboard

• Select desired blocks and words

• Insert and erase blocks and words

• Correct erroneously entered values and commands

• Easily clear TNC messages from the screen

Types of input

Numbers, coordinate axes and radius compensation are entered directly by keyboard. You can set the algebraic sign either before, during or after a numerical entry.

Selecting blocks and words

• To call a block with a certain block number:

GOTO

e.g.

ENT

The highlight jumps to block number 10.

• To move one block forwards or backwards:

Press the vertical cursor keys.

• To select individual words in a block:

Press the horizontal cursor keys.

• To find the same word in other blocks:

For this function the AUTO DRAW soft key must be set to OFF.

Select the word in the block.

Find the same word in other blocks.

Inserting a block

Additional program blocks can be inserted behind any existing block (except the PGM END block).

GOTO

Select the block in front of the desired insertion.

Program the new block.

The block numbers of all subsequent blocks are automatically increased by one.

4-3TNC 425/TNC 415 B/TNC 407

4 Programming

4.1 Creating Part Programs

Editing and inserting words

Highlighted words can be changed as desired: simply overwrite the old value with the new one. Plain language dialog indicates the type of information required. After entering the new information, press a horizontal cursor key or the END key to confirm the change.

In addition to changing the existing words in a block, you can also add new words with the aid of the plain language dialog.

Erasing blocks and words

Function Key

• Set the selected number to 0

• Erase an incorrect number

• Clear a non-blinking error message

• Delete the selected word

• Delete the selected block

• Erase cycles and program sections:

First select the last block of the cycle or program section to be erased.

ENT

DEL

TNC 425/TNC 415 B/TNC 4074-4

4 Programming

4.2 Structuring Programs

The most convenient way to structure programs is to switch the screen layout to PGM+SECTION (see page 1-6).

To keep track of long programs you can enter structuring blocks as texts in the TNC program. The TNC then displays these structuring blocks in the right screen window. To page through the program you can:

• Scroll up and down in the program NC block by NC block in the left screen window

• Scroll up and down in the program structuring block by structuring block in the right window

If you are scrolling through the program block by block in the right screen window, the TNC at the same time automatically moves the corresponding NC blocks in the left window. This way you can skip any desired number of NC blocks by simply pressing a key. With the aid of the CHANGE WINDOW soft key, you can switch from the left to the right window, and vice versa. The background color of the screen window can be selected through machine parameters.

Fig. 4.2 TNC screen for structuring programs: left screen

window is active

The CHANGE LEVEL soft key determines for which of the two available levels a structuring block is defined. The second level is indented in the screen window (see Fig. 4.3).

You can edit existing structuring texts and the level of a structuring block for both windows by moving the highlight with the horizontal cursor keys to the block to be changed.

Inserting a structuring block in the left screen window

You initiate the dialog for structuring block entry by pressing the INSERT SECTION soft key. The structuring block is inserted behind the current block.

STRUCTURING TEXT ?

Enter the structuring text with the ASCII keyboard (244 characters maximum).

Fig. 4.3 TNC screen for structuring programs: right screen window is active

If necessary, change the level of the structuring block. You can choose from two levels.

Inserting a structuring block in the right screen window

Simply enter the text with the ASCII keyboard; the TNC automatically inserts the new structuring block behind the active structuring block.

4-5TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

Each tool is identified by a number.

The tool data, consisting of the:

• length L, and

• radius R

are assigned to the tool number.

The tool data can be entered:

• into the individual part program in a TOOL DEF block, or

• once for each tool into a common tool table that is stored as a type .T file.

Once a tool is defined, the TNC then associates its dimensions with the tool number, and accounts for them when executing positioning blocks.

The way the tool is used is influenced by several miscellaneous functions (see page 12-14).

Setting the tool data

Tool numbers

Each tool is designated with a number between 0 and 254.

With TOOL CALL and TOOL DEF the tool with the number 0 is automatically defined 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 radius R

The radius of the tool is entered directly.

Tool length L

The compensation value for the tool length is measured

• as the difference in length between the tool and a zero tool, or

• with a tool pre-setter.

A tool pre-setter eliminates the need to define a tool in terms of the difference between its length and that of another tool.

TNC 425/TNC 415 B/TNC 4074-6

4 Programming

4.3 Tools

Oversizes for lengths and radii – Delta values

In tool tables and in a TOOL CALL block you can enter so-called delta values for tool length and radius.

• Positive delta values - tool oversize

• Negative delta values- tool undersize The TNC adds the delta values from the table and

the TOOL CALL block.

Applications

• Undersize in the tool table for wear

• Oversize in the TOOL CALL block, for example as a finishing allowance during roughing.

Delta values can be numerical values, Q parameters (only in a TOOL CALL block) or the value 0. Maximum permissible oversize or undersize is +/- 99.999 mm.

DR<0

DR>0

DL<0

Fig. 4.4: Oversizes DL, DR on a toroid cutter

DL>0

Determining tool length with a zero tool

For the sign of the tool length L:

L > L L < L

Move the zero tool to the reference position in the tool axis (e.g. workpiece surface with Z = 0).

If necessary, set the datum in the tool axis to 0.

Change tools.

The tool is longer than the zero tool

The tool is shorter than the zero tool

Fig. 4.5: Tool lengths are entered as the difference from the zero tool

L >0

L <0

Move the new tool to the same reference position as the zero tool.

The TNC displays the compensation value for the length L.

Write the value down and enter it later.

Enter the display value by using the “actual position capture” function (see page 4-30).

4-7TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

Entering tool data into the program

The following data can be entered once for each tool in the part program:

• Tool number

• Tool length compensation value L

• Tool radius R

To enter tool data in the program block:

TOOL

DEF

TOOL NUMBER ?

e.g.

ENT

Designate the tool with a number, for example 5.

TOOL LENGTH L ?

e.g.

1 0

ENT

Enter the compensation value for the tool length, e.g. L = 10 mm.

TOOL RADIUS R ?

e.g.

ENT

Enter the tool radius, e.g. R = 5 mm.

Resulting NC block: TOOL DEF 5 L+10 R+5

You can enter the tool length L directly in the tool definition by using the “actual position capture” function (see page 4-30).

TNC 425/TNC 415 B/TNC 4074-8

4 Programming

4.3 Tools

Entering tool data in tables

A tool table is a file in which the tool data for all tools are stored commonly. The maximum number of tools per table (0 to 254) is set in machine parameter MP 7260.

On machines with automatic tool changers, the tool data must be stored in tool tables. You can edit tool tables using special, time-saving editing functions.

Types of tool tables

Tool table TOOL.T

• is used for machining

• is edited in a program run mode of operation

All other tool tables

• are used for test runs and archiving

• are edited in the PROGRAMMING AND EDITING mode of operation

If you copy a tool table into TOOL.T for a program run, the old TOOL.T will be erased and overwritten.

Editing functions for tool tables

The following functions help you to create and edit tool tables:

Function Key / Soft key

• Move the highlight

• Go to the beginning/end of the table

• Go to the next/previous table page

• Go to the beginning of the next line

• Look for the tool name in the tool table

4-9TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

To edit the tool table TOOL.T:

To edit any other tool table:

PROGRAM RUN / SINGLE BLOCK

PROGRAM RUN / FULL SEQUENCE

Select the tool table TOOL.T.

Switch the EDIT soft key to ON.

PROGRAMMING AND EDITING

PGM

NAME

Call the file directory.

Shift the soft-key row and show file type .T.

FILE NAME = .T

Select the tool table.

Enter a new file name and create a new table.

TNC 425/TNC 415 B/TNC 4074-10

4 Programming

4.3 Tools

Tool data in tables

The following information can be entered in tool tables:

• Tool radius and tool length: R, L

• Curvature radius of the tool point for threedimensional tool compensation: R2 For graphic display of machining with a spherical cutter, enter R2 = R.

• Oversizes (delta values) for tool radii and tool lengths: DR, DR2, DL

• Length of the tool cutting edge: LCUTS

• Maximum plunge angle: ANGLE

• Tool name: NAME

• Maximum and current tool life: TIME1, TIME2, CUR.TIME

• Number of a Replacement Tool: RT

• Tool Lock: TL

• Tool comment: DOC

• Information on this tool for the Programmable Logic Control (PLC — adapts the TNC to the machine tool): PLC

Fig. 4.6: Left part of the tool table

The TNC needs the following tool data for automatic tool measurement:

• Number of teeth: CUT

• Wear tolerance for tool length: LTOL

• Wear tolerance for tool radius: RTOL

• Cutting direction for dynamic tool measurement: DIRECT

• Offset of the tool from center of stylus to center of tool: TT:R-OFFS Default value: Tool radius R

• Offset of the tool from top of stylus to the tool tip: TT:L-OFFS Default value: 0

• Breakage tolerance for tool length: LBREAK

• Breakage tolerance for tool radius: RBREAK

A general user parameter (MP7266) defines which data can be entered in the tool table and in which sequence the data is displayed.

The sequence of the information in the tool table shown in the illustrations to the right is only one example out of many possibilities.

If all the information in a table no longer fits on one screen, this is indicated with a ">>" or "<<" symbol in the line with the table name.

Fig. 4.7: Right part of the tool table

To read-out or read-in a tool table (see page 10-2):

EXT

Select external data input/output directly from the table.

Read-out the table.

Read-in the table (only possible if EDIT ON is selected).

4-11TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

Overview: Information in tool tables

Abbrev. Input Dialog

T Number by which the tool is called in the program – NAME Name by which the tool is called in the program TOOL NAME ? L Value for tool length compensation TOOL LENGTH L ? R Tool radius R TOOL RADIUS R ? R2 Tool radius R2, for toroid cutters (only for 3D radius

DL Delta value for tool length TOOL LENGTH OVERSIZE ? DR Delta value for tool radius R TOOL RADIUS OVERSIZE ? DR2 Delta value for tool radius R2 TOOL RADIUS OVERSIZE 2 ? LCUTS Length of tool's cutting edge: required by the TNC for

ANGLE Maximum plunge angle of the tool for reciprocating plunge MAXIMUM PLUNGE ANGLE ? TL Tool lock TOOL LOCKED

RT Number of a Replacement Tool, if available (see also TIME2) REPLACEMENT TOOL ? TIME1 Maximum tool age in minutes.

TIME2 Maximum tool life in minutes during TOOL CALL:

CUR.TIME Time in minutes that the tool has been in use:

DOC Comment on tool (up to 16 characters) TOOL DESCRIPTION ? PLC Information on this tool that should be transferred to the PLC PLC STATUS ?

compensation or graphical representation of a machining operation with spherical or toroid cutters) TOOL RADIUS 2 ?

Cycle 22 TOOTH LENGTH IN THE TOOL AXIS ?

YES=ENT/NO=NOENT

The meaning of this information can vary depending on the individual machine tool. Your machine manual provides more information on TIME1. MAXIMUM TOOL AGE ?

If the current tool life exceeds this value, the TNC changes the tool during the next TOOL CALL (see also CUR.TIME). MAX. TOOL AGE FOR TOOL CALL ?

The TNC automatically counts the current tool life. A starting value can be entered for used tools. CURRENT TOOL AGE ?

TNC 425/TNC 415 B/TNC 4074-12

4 Programming

4.3 Tools

Information in tool tables

Abbrev. Input Dialog

CUT. Number of teeth that are measured in automatic tool

measurement (max. 20 teeth) NUMBER OF TEETH ?

LTOL Permissible deviation from tool length L during automatic tool

measurement. If the entered value is exceeded, the TNC locks the tool (status L). Input range: 0 to 0.9999 mm WEAR TOLERANCE: LENGTH ?

RTOL Permissible deviation from tool radius R during automatic tool

measurement. If the entered value is exceeded, the TNC locks the tool (status L). Input range: 0 to 0.9999 mm WEAR TOLERANCE: RADIUS ?

DIRECT. Automatic tool measurement: Cutting direction of the

tool for dynamic tool measurement CUTTING DIRECTION ( M3 = – ) ?

TT:R-OFFS Automatic tool length measurement: Offset of the tool

between the stylus center and the tool center. Default setting: tool radius R TOOL OFFSET: RADIUS ?

TT:L-OFFS Automatic tool radius measurement: tool offset in addition

to the value in MP 6530 (see S. 12-6) between the stylus top and the tool tip. Default setting: 0 TOOL OFFSET: LENGTH ?

LBREAK Automatic tool measurement: permissible deviation from

the tool length L for breakage detection. If the entered value is exceeded, the TNC locks the tool (Status L). Input range: 0 to 0.9999 mm BREAKAGE TOLERANCE: LENGTH ?

RBREAK Automatic tool measurement: permissible deviation from

the tool length R for breakage detection. If the entered value is exceeded, the TNC locks the tool (Status L). Input range: 0 to 0.9999 mm BREAKAGE TOLERANCE: RADIUS ?

(continued

)

4-13TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

Pocket table for tool changer

The TOOL_P in a program run operating mode.

The NEW POCKET TABLE or also the RESET POCKET TABLE soft key is for erasing an existing pocket table and writing a new one. Like the tool table, a pocket table can also be read-in and read-out directly through the data interface (see page 4-11).

To select the pocket table:

table (for tool pocket) is programmed

Select tool table.

Fig. 4.8: Pocket table for the tool changer

Select pocket table.

Set the EDIT soft key to ON.

To edit the pocket table:

Abbrev. Input Dialog

P Pocket number of the tool in the tool magazine – T Tool number TOOL NUMBER F Fixed tool number. The tool is always returned to the same pocket. FIXED TOOL

YES = ENT / NO = NOENT

L Locked pocket POCKET LOCKED

YES = ENT / NO = NOENT

ST Special Tool

If this ST requires also the pockets in front of and behind its own pocket, then lock the appropriate number of pockets. SPECIAL TOOL

PLC Information on this tool that should be sent to the PLC PLC STATUS

Overview: Data in the pocket table

TNC 425/TNC 415 B/TNC 4074-14

4 Programming

4.3 Tools

Calling tool data

The following data can be programmed in the TOOL CALL block:

• Tool number, Q parameter or tool name (name only if a tool table is active)

• Spindle axis

• Spindle speed

• Oversize for the tool length DL

• Oversize for the tool radius DR

D represents the Greek letter delta, which is used as a symbol for differences and deviations.

To call tool data:

TOOL CALL

TOOL NUMBER ?

Enter the number of the tool as defined in the tool table or in a TOOL DEF block, for example 5.

Enter the spindle axis, e.g. Z.

Enter the spindle speed, e.g. S=500 rpm.

Enter delta values for the tool length, e.g. DL = 0.2 mm.

e.g.

ENT

e.g.

WORKING SPINDLE AXIS X/Y/Z?

SPINDLE SPEED S=?

e.g.

TOOL LENGTH OVERSIZE ?

e.g.

TOOL RADIUS OVERSIZE ?

e.g.

ENT

Enter delta values for the tool radius, e.g. DR = –1 mm.

Resulting NC block: TOOL CALL 5 Z S500 DL+0.2 DR–1

Tool pre-selection with tool tables

If you are using tool tables, you use TOOL DEF to pre-select the next tool. Simply enter the tool number, a tool name, or a corresponding Q parameter.

4-15TNC 425/TNC 415 B/TNC 407

4 Programming

4.3 Tools

Tool change

Tool change is a machine tool dependent function. See your machine tool manual.

Automatic tool change

If your machine is built for automatic tool changing, the TNC controls the replacement of the inserted tool by another from the tool magazine. The program run is not interrupted.

Manual tool change

To change the tool manually, stop the spindle and move the tool to the tool change position. Sequence of action:

• Move to the tool change position (under program control, if desired)

• Interrupt program run (see page 3-5)

• Change the tool

• Continue the program run (see page 3-6)

Tool change position

A tool change position must lie next to or above the workpiece to prevent tool collision. With the miscellaneous functions M91 and M92 (see page 5-65) you can enter machine-referenced 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.

TNC 425/TNC 415 B/TNC 4074-16

4 Programming

4.3 Tools

Automatic tool change: M101

M101 is a machine tool dependent function. See your machine tool manual.

Standard behavior — without M101

If the tool reaches the maximum tool life (TIME1) during program run, the TNC internally flags this data. The machine tool builder determines how the machine tool reacts to this information.

Automatic tool change – with M101

The TNC automatically changes the tool if the tool life (TIME1 or TIME2) expires during program run. The tool is not changed immediately upon expiry, but – depending on the workload of the processor – a few NC blocks later.

Duration of effect

M101 is reset with M102.

Standard NC blocks with radius compensation R0, RR, RL

The radius of the replacement tool must be the same as that of the original tool. If the radii are not equal, the TNC displays an error message and does not replace the tool.

NC blocks with surface-normal vectors and 3D compensation

The radius of the replacement tool can differ from the radius of the original tool. The tool radius is not included in program blocks transmitted from CAD systems. A negative delta value (DR) can be entered in the tool table.

If DR is positive, the TNC displays a message and does not change the tool. You can suppress this message with the M function M107, and reactivate it with M108.

4-17TNC 425/TNC 415 B/TNC 407

4 Programming

4.4 Tool Compensation Values

For each tool, the TNC adjusts the spindle path in the tool axis by the compensation value for the tool length. In the working plane it compensates for the tool radius.

When up to five axes are being programmed in one block (rotary axes are also permitted) the TNC accounts for the tool radius compensation value only in the working plane.

If a part program generated by CAD system contains surface-normal vectors, the TNC can also perform threedimensional tool compensation (see page 4-21).

Fig. 4.9: The TNC must compensate the length and radius of the tool

Effect of tool compensation values

Tool length

The compensation value for the tool length is calculated as follows:

Compensation value = L + DL_TC + DL_TAB

where L: is the tool length L (from the TOOL DEF block or

DL_TC: is the oversize for length DL in the TOOL CALL

DL_TAB: is the oversize for length DL in the tool table

Length compensation becomes effective automatically as soon as a tool is called and the tool axis moves. Length compensation is cancelled by calling a tool with the length L = 0.

If a positive length compensation was in effect before TOOL CALL 0, the clearance to the workpiece is reduced. If the tool is traversed to incremental positions in the tool axis after TOOL CALL, the TNC not only moves the tool according to the programmed value but also accounts for the difference between the length of the old tool and that the new one.

Tool radius

The compensation value for the tool radius is calculated as follows:

Compensation value = R + DR_TC + DR_TAB

the tool table)

block

where R: is the tool radius R (from the TOOL DEF block or

the tool table)

DR_TC: is the oversize for radius DR in the TOOL CALL

block

DR_TAB: is the oversize for radius DR in the tool table

Radius compensation becomes effective as soon as a tool is called and is moved in the working plane with RL or RR. Radius compensation is cancelled by programming a positioning block with R0.

TNC 425/TNC 415 B/TNC 4074-18

4 Programming

4.4 Tool Compensation Values

Tool radius compensation

A tool movement can be programmed:

• Without radius compensation: R0

• With radius compensation: RL or RR

• As single-axis movements with R+ or R-

Tool movement without radius compensation: R0

The tool center moves to the programmed coordinates.

Applications:

• Drilling and boring

• Pre-positioning

To position without radius compensation:

TOOL RADIUS COMP.RL/RR/NO COMP.?

Fig. 4.10: Programmed contour (—, +) and the path of the tool

center (- - -)

Fig. 4.11: These drilling positions are entered without radius

compensation

ENT

Select tool movement without radius compensation.

. . .

4-19TNC 425/TNC 415 B/TNC 407

4 Programming

4.4 Tool Compensation Values

Tool movement with radius compensation RR, RL

The tool center moves to the left (RL) or to the right (RR) of the programmed contour at a distance equal to the radius. Right or left is meant as seen in the direction of tool movement as if the workpiece were stationary.

Fig. 4.12: The tool moves to the left (RL) or to the right (RR) of the workpiece during milling

To position with radius compensation:

. . .

TOOL RADIUS COMP.RL/RR/NO COMP.?

Select tool movement to the left of the programmed contour.

• Between two program blocks with different radius compensation values you must program at least one block without radius compensation (that is, with R0).

• Radius compensation is not in effect until the end of the block in which it is first programmed.

• The TNC always positions the tool perpendicular to the starting or end point during activation and deactivation of radius compensation. Always position the tool in front of the first contour point (or behind the last contour point) so that the tool will not gouge the workpiece.

Select tool movement to the right of the programmed contour.

TNC 425/TNC 415 B/TNC 4074-20

4 Programming

4.4 Tool Compensation Values

Shortening or lengthening single-axis movements R+, R-

This type of radius compensation is possible only for single-axis movements in the working plane: The programmed tool path is shortened (R-) or lengthened (R+) by the tool radius.

Applications:

• Single-axis machining

• Occasionally for pre-positioning the tool, such as for a SLOT MILLING cycle.

• You can enable R+ and R- by opening a positioning block with an orange axis key.

• The machine tool builder can set machine parameters to inhibit the possibility of programming single-axis positioning blocks

Machining corners

If you work without radius compensation, you can influence the machining of outside corners with M90 (see page 5-62).

Outside corners

The TNC moves the tool in a transitional arc around outside corners. The tool “rolls around” the corner point.

If necessary, the feed rate F is automatically reduced at outside corners to reduce machine strain, for example at very great changes in direction.

Fig. 4.13: The tool “rolls around” outside corners

Do not place the starting point (or end point) on a corner of an internal contour. Otherwise the TNC may gouge the contour.

Inside corners

The TNC calculates the intersection of the tool center paths at inside corners. From this point it then starts the next contour element. This prevents damage to the workpiece.

RLRL

The permissible tool radius, therefore, is limited by the geometry of the programmed contour.

S S

Fig. 4.15: Tool path for inside corners

4-21TNC 425/TNC 415 B/TNC 407

4 Programming

4.5 Three-Dimensional Tool Compensation (Not on TNC 407)

This TNC feature uses straight-line blocks that include tool radius compensation in terms of surface-normal vectors (see below) that have been calculated by a CAD system.

The TNC calculates a three-dimensional (3D) tool compensation so that tools can be used that have slightly different dimensions than the one originally used.

3D compensation can be performed for the tool shapes illustrated in Fig. 4.16

11 2 3

Fig. 4.15: Tool shapes for 3D compensation: end mill (1),

spherical cutter (2), toroid cutter (3)

Defining tool shapes for 3D compensation

Two types of radii, R and R2, can be entered in the tool table:

• TOOL RADIUS – R Distance from the tool axis to the tool circumference (tool "thickness").

• TOOL RADIUS 2 – R2

Dimension for the curvature of the tool point: distance from the center of a circle derived from the arc of curvature to the curve itself.

The second radius value (R2) determines the shape of the tool:

• End mill R2 = 0

• Toroid cutter 0 < R2 < R

• Spherical cutter R2 = R

Fig. 4.16: Tool datum P, tool radii R and R2 on end mills, spherical and

toroid cutters

Surface-normal vectors NX, NY, NZ

For 3D compensation the TNC uses three additional words in the NC block (NX, NY and NZ): one for each compensated axis in the Cartesian coordinate system.

The CAD system calculates NX, NY and NZ, which are transferred to the TNC together with the contouring commands.

NX, NY and NZ are the "components" of the directional data for 3D compensation. Such directional data is called a "vector."

Fig. 4.17: Surface-normal vectors and tool

position during 3D compensation

TNC 425/TNC 415 B/TNC 4074-22

4 Programming

4.5 Three-Dimensional Tool Compensation (not on TNC 407)

A vector always has

• a magnitude (e.g. a distance) and

• a direction (e.g. away from the workpiece)

If a vector is perpendicular ("normal") to a surface, it is called a surface- normal vector.

The TNC can compensate small differences in tool sizes in the surfacenormal vector NX, NY, NZ. It calculates NX, NY and NZ up to an accuracy of seven places behind the millimeter decimal point.

Target direction of the surface-normal vector

The surface-normal vectors point from the workpiece surface to the tool datum P

On spherical cutters and toroid cutters, P axis where the curvature begins.

(see Fig. 4.16 and 4.17).

lies on the tool axis. On end mills it lies on the surface of the tool end.

lies at the point on the tool

• The coordinates for the X, Y, Z positions and the normal vector components NX, NY, NZ must be in the same sequence in the NC block.

• 3D compensation with normal vectors is only available for coordinates X, Y and Z.

• The TNC will not display an error message if an entered tool oversize would cause contour error.

• Machine parameter MP 7680 defines whether the postprocessor accounts for the center of sphere or the south pole of the sphere when calculating the tool length.

Compensating other tool dimensions by entering delta values

In some cases you may want or have to use a tool with different dimensions than those originally entered for 3D compensation.

You can adjust these dimensions by entering delta values (oversize and undersize) in the tool table.

Delta values (DL for length, DR and DR2 for the radii) can be entered up to +/– 99.999 mm (3.9 in.).

• A positive delta value is an oversize, which means that the tool is larger than the original tool.

• A negative delta value is an undersize, which means that the tool is smaller than the original

DL>0

tool.

The TNC corrects the tool position by the delta

Fig. 4.18: Delta values for oversize and undersize

values and the normal vector.

DR2>0

4-23TNC 425/TNC 415 B/TNC 407

4 Programming

4.5 Three-Dimensional Tool Compensation (only TNC 425, TNC 415 B)

NC Block

Example of an NC block with a surface-normal vector:

LN X+31.737 Y+21.954 Z+33.165 NX+0.2637581....

.... NY+0.0078922 NZ–0.8764339 F1000 M3

LN Straight line with 3D compensation X, Y, Z Compensated coordinates of the straight-line end points NX, NY, NZ Components of the surface-normal vector F Feed rate M Miscellaneous function

The feed rate F and miscellaneous function M can be entered and changed in the PROGRAMMING AND EDITING mode of operation. The coordinates of the straight-line end point and the components of the surface-normal vector are calculated only by the CAD system.

TNC 425/TNC 415 B/TNC 4074-24

4 Programming

4.6 Program Initiation

Defining the blank form – BLK FORM

If you wish to use the TNC's graphic workpiece simulation you must first define a rectangular workpiece blank. Its sides lie parallel to the X, Y and Z axes and can be up to 30,000 mm long.

The dialog for blank form definition starts automatically at every program initiation. It can also be called with the BLK FORM soft key.

The ratio of the blank-form side lengths must be less than 200:1.

MIN and MAX points

The blank form is defined by two of its corner points:

MIN

Fig. 4.19: MIN and MAX points define the

blank form.

MAX

• The MIN point — the smallest X, Y and Z coordinates of the blank form, entered as absolute values.

• The MAX point — the largest X, Y and Z coordinates of the blank form, entered as absolute or incremental values.

4-25TNC 425/TNC 415 B/TNC 407

4 Programming

4.6 Program Initiation

To create a new part program:

PGM

NAME

Select the file directory.

Select any type .H file, for example OLD.H.

FILE NAME = OLD .H

e.g.

N WE

ENT

Enter the name of the new file, for example NEW.H.

MM = ENT / INCH = NO ENT

ENT

Indicate whether the dimensions will be entered in millimeters or inches.

WORKING SPINDLE AXIS X / Y / Z ?

e.g.

Enter the working spindle axis, e.g. Z.

DEF BLK FORM: MIN-CORNER ?

e.g.

0 0

ENT

Enter in sequence the X, Y and Z coordinates of the MIN point, e.g. X=0 mm, Y=0 mm, Z=-40 mm.

DEF BLK FORM: MAX-CORNER ?

e.g.

1 0 0 1 0 0

ENT

Enter in sequence the X, Y and Z coordinates of the MAX point, e.g. X=100 mm, Y=100 mm, Z=0 mm.

TNC 425/TNC 415 B/TNC 4074-26

4 Programming

4.6 Program Initiation

The following blocks then appear on the TNC screen as program text:

0 BEGIN PGM NEW MM

Block 0: Program begin, name, unit of measure

1 BLK FORM 0.1 Z X+0 Y+0 Z-40

Block 1: Tool axis, MIN point coordinates

2 BLK FORM 0.2 X+100 Y+100 Z+0

Block 2: MAX point for coordinates

3 END PGM NEW MM

Block 3: Program end, name, unit of measure

Block numbers, as well and the BEGIN and END blocks are automatically generated by the TNC. The unit of measure used in the program appears behind the program name.

4-27TNC 425/TNC 415 B/TNC 407

4 Programming

4.7 Entering Tool-Related Data

Besides the tool data and compensation, you must also enter the following information:

• Feed rate F

• Spindle speed S

• Miscellaneous function M

Feed rate F

The feed rate is the speed (in mm/min or inch/min) at which the tool center moves.

Input range: F = 0 to 300,000 mm/min or 11,811 ipm.

The maximum feed rate is set individually for each axis in machine parameters.

S S

Fig. 4.20: Feed rate F and spindle speed S of the tool

To set the feed rate:

Answer the following dialog question in the positioning block:

FEED RATE F = ? / F MAX = ENT

e.g.

1 0

The question does not always appear with F MAX.

Rapid traverse

If you wish to program rapid traverse, press ENT for FMAX. If you know the maximum traverse speed, you can also program it directly. FMAX is effective only for the block in which it is programmed.

Duration of feed rate F

A feed rate which is entered as a numerical value remains in effect until a block with another feed rate is reached.

If the new feed rate is FMAX, the feed rate returns to the previous feed rate after the block is executed.

ENT

Enter the feed rate, for example F = 100 mm/min.

Changing the feed rate F

You can vary the feed rate by turning the knob for feed rate override on the TNC keyboard (see page 2-6).

TNC 425/TNC 415 B/TNC 4074-28

4 Programming

4.7 Entering Tool-Related Data

Spindle speed S

You enter the spindle speed S in revolutions per minute (rpm) in the TOOL CALL block.

Input range: S = 0 to 99 999 rpm

To change the spindle speed S in the part program:

TOOL

CALL

Press the TOOL CALL key.

TOOL NUMBER ?

ENT

Ignore the request for the tool number.

WORKING SPINDLE AXIS X/Y/Z ?

ENT

Ignore the request for the tool axis.

SPINDLE SPEED S=?

e.g.

END

001

Enter the spindle speed S, for example 1000 rpm.

Resulting NC block: TOOL CALL S1000

To change the spindle speed S during program run:

100

15050

S %

You can vary the spindle speed S on machines with stepless leadscrew drives by turning the spindle speed override knob on the TNC keyboard.

4-29TNC 425/TNC 415 B/TNC 407

4 Programming

4.8 Entering Miscellaneous Functions and STOP

Some M functions are not effective on certain machines. The machine tool builder may also add some of his own M functions. See your machine tool manual.

The M functions (M for miscellaneous) affect:

• Program run

• Machine function

• Tool behavior On the inside back cover of this manual you will find a list of M functions

that are predetermined for the TNC. The list indicates whether an M function begins at the start, or at the end of the block in which it is programmed.

Answer the following requests in a positioning block:

. .

MISCELLANEOUS FUNCTION M?

e.g.

ENT

Enter the miscellaneous function, for example M3 (spindle ON, clockwise rotation).

. .

To enter an M function in a STOP block:

MISCELLANEOUS FUNCTION M?

e.g.

ENT

Enter the miscellaneous function, for example M5 (spindle STOP).

Resulting NC block: STOP M5

If the M function was programmed in a STOP block, program run will be interrupted at that block.

Some M functions are not effective on certain machines. The machine tool builder may also add some of his own M functions.

A program run or test run is interrupted when it reaches a block containing the STOP function.

An M function can be programmed in a STOP block.

If you wish to interrupt the program run or program test for a certain duration, use the cycle 9: DWELL TIME (see page 8-56).

To enter a STOP function:

STOP

Press the STOP key.

MISCELLANEOUS FUNCTION M ?

e.g.

ENT

Enter an M function, if desired, for example M6 (tool change).

Resulting NC block: STOP M6

TNC 425/TNC 415 B/TNC 4074-30

4 Programming

4.9 Actual Position Capture

Sometimes you may want to enter the actual position of the tool in a particular axis as a coordinate in a part program. Instead of reading the actual position values and entering them with the number keys, you can simply press the “actual position capture” key. You can use this feature to

• enter a single coordinate into a highlighted block

• generate an L block if you have not marked a specific word with the highlight

L = –5

TOOL DEF 3 L–5 R

The L block is inserted after the block that is active in the PROGRAMMING AND EDITING mode of operation. It only contains the coordinates that were selected with the MOD function (see page 11-10).

To capture a single coordinate:

MANUAL OPERATION

Move the tool to the position that you wish to capture.

PROGRAMMING AND EDITING

Select or create the block in which you wish to enter the actual position of the tool.

COORDINATES ?

e.g.

Fig. 4.21: Storing the actual position in the TNC

Select the axis in which you wish to capture a coordinate, for example X.

Transfer the actual position coordinate to the program.

Enter the radius compensation according to the position of the tool relative to the workpiece.

To generate a new L block with the actual position coordinates:

MANUAL OPERATION

Move the tool to the position that you wish to capture.

PROGRAMMING AND EDITING

Select the block after which the L block should be inserted.

The actual position coordinate is entered in a new L block.

4-31TNC 425/TNC 415 B/TNC 407

4 Programming

4.10 Marking Blocks for Optional Block Skip

You can mark program blocks so that the TNC will skip them during a program or test run whenever the block skip option is active (see page 3-10). The interactive graphics, however, ignores the marked blocks whether the block skip option is active or not.

To mark blocks:

Select the block that should not always be run.

• TOOL DEF blocks cannot be skipped.

• To skip a cycle, place the "/" character in the first cycle block

To delete the "/" character:

Select block from which "/" character is to be deleted.

Mark the block with the "/" character on the alphabetic keyboard.

Delete the character.

TNC 425/TNC 415 B/TNC 4074-32

4 Programming

4.11 Text Files

You can use the TNC's text editor to write and edit texts.

Typical applications:

• Recording test results

• Documenting working procedures

• Keeping formulas and creating cutting data diagrams

The text editor can edit only type .A files (text files). If you wish to edit other types of files with the text editor you must convert them first (see page 1-36).

The typewriter-style keyboard provides letters, symbols and function keys that you need to create and change texts. The soft keys enable you to move around in the text and to find, delete, copy and insert letters, words, sections of text (text blocks), or entire files.

To create a text file:

PGM

NAME

PROGRAMMING AND EDITING

Show text files (type .A files).

FILE NAME = .A

e.g.

A B C

ENT

Enter a file name, for example ABC, and confirm.

The following information is visible in the highlighted line at the top of the text window:

• FILE: Name of the current text file

• LINE: Line in which the cursor is

presently located

• COLUMN: Column in which the cursor is

presently located

• INSERT: Insert new text, pushing the

old text aside

• OVERWRITE: Write over the existing text,

erasing it where it is replaced with the new text.

You can toggle between the INSERT and OVERWRITE modes with the soft key at the far left. The selected mode is shown enclosed in a frame.

To leave a text file:

PGM

NAME

Select another file type, such as a conversational program.

Select the desired program.

Fig. 4.22: Text editor screen

4-33TNC 425/TNC 415 B/TNC 407

4 Programming

4.11 Text Files

Entering text

The text that you type always appears on the screen where the cursor is located. You can move the cursor with the cursor keys and the following soft keys:

Function Soft key

• Move one word to the right

• Move one word to the left

• Move to the next screen page

• Move to the previous screen page

• Move to beginning of file

• Move to end of file

In each screen line you can enter up to 77 characters from the alphanumeric keyboard.

The keyboard offers the following function keys for editing text:

Function Key

• Begin a new line

• Erase the character to the left of the cursor

RET

(backspace)

• Insert an empty space

SPACE

Exercise text:

Write the following text in the file ABC.A. You will need it for the exercises in the next few pages.

*** JOBS *** !! IMPORTANT:

MACHINE THE CAMS (ASK THE BOSS?!) PROGRAM 1375 .H; 80% OK BY LUNCH

TOOLS TOOL 1 DO NOT USE TOOL 2 CHECK REPLACEMENT TOOL: TOOL 3

Fig. 4.23: Text editor screen with exercise text

TNC 425/TNC 415 B/TNC 4074-34

4 Programming

4.11 Text Files

Finding text sections

You can search for a desired character or word with the FIND soft key at the far right of the first soft-key row:

Finding the current word

You can search for the next occurrence of the word in which the cursor is presently located.

Exercise: Find the word TOOL in the file ABC.A

Move the cursor to the word TOOL.

Select the search function.

FIND TEXT : TOOL

To find any text:

FIND TEXT :

Enter the text that you wish to find.

To leave the search function:

Find the word TOOL where it next appears in the text.

Select the search function.

Find the text.

Terminate the search function.

4-35TNC 425/TNC 415 B/TNC 407

4 Programming

4.11 Text Files

To erase and insert characters, words and lines:

Move the cursor to the text that you wish to erase, or to the place where you wish to insert text.

Function Soft key

• Delete a character

• Delete and temporarily store a word

• Delete and temporarily store a line

• Insert a line/word from temporary storage

Shift the soft-key row.

Exercise: Delete the first line of ABC.A and insert it behind BY LUNCH

Move the cursor to any position in the line *** JOBS ***.

Shift the soft-key row.

Delete the line and store temporarily.

Move the cursor to the beginning of the line behind BY LUNCH.

Insert the line *** JOBS *** at the cursor position.

Temporarily stored words and lines can be inserted as often as desired.

TNC 425/TNC 415 B/TNC 4074-36

4 Programming

4.11 Text Files

Editing sections of text

With the editor, text sections (blocks) of any size can be

• selected

• deleted

• inserted at the same or other locations

• copied (even whole files)

Function Soft key

• To select a block:

Place the cursor at one end of the block and press SELECT BLOCK. Then move the cursor to the other end. The selected block has a different color than the rest of the text.

• Delete the selected text and store temporarily

• Insert the temporarily stored text at the cursor

location

• Store marked block temporarily without erasing

Shift the soft-key row.

• Transfer the selected text to another file:

Write the name of the target file in the screen dialog line and press ENT. The TNC adds the selected text to the end of the specified file. You can also create a new file with the selected text in this way.

• Insert another file at the cursor position:

Write the name of the source file in the screen dialog line and press ENT.

4-37TNC 425/TNC 415 B/TNC 407

4 Programming

4.11 Text Files

Exercise:

Move the last four lines in the file ABC.A to the beginning of the file, then copy them into a new file WZ.A.

• Move the text to the beginning of the file:

Move the cursor to the “T” of TOOLS.

Activate the selecting function.

Move the cursor to the end of the block.

repeatedly

Erase the text and store temporarily.

Move the cursor to the beginning of the file.

repeatedly

Insert the stored text. Note: The stored block is inserted above the cursor and may be off screen.

• Select the text again and copy it into a new/another file:

Mark the text block as described above.

Select the function for copying to another file.

DESTINATION FILE =

ENT

Write the name of the file into which you wish to copy the block, for example WZ.

Copy into a new/another file. Text block remains marked.

TNC 425/TNC 415 B/TNC 4074-38

4 Programming

4.12 Creating Pallet Files

Pallet files are used with machining centers and contain the following information:

• Pallet number PAL

• Part program name PGM-NAME

• Datum table DATUM

To edit pallet files:

PROGRAMMING AND EDITING

PGM

NAME

Call the file directory.

Shift the soft-key row and show the .P type pallet files.

FILE NAME = .P

Select a pallet file or enter a new file name and create a new file.

To link programs and datum tables:

PROGRAM NAME ?

Enter the name of a part program that belongs to this pallet file.

DATUM TABLE ?

Enter the name of the datum table for the program.

if necessary

Create more pallet files.

Pallet files are managed and output as determined in the PLC. See your machine tool handbook.

4-39TNC 425/TNC 415 B/TNC 407

4 Programming

4.12 Creating Pallet Files

The following functions help you to create and change pallet tables:

Function Key/

Move highlight vertically

Move highlight horizontally

Go to beginning of table

Go to end of table

Go to next page of the table

Go to previous page of the table

Soft key

Insert line at the end of the table

Delete the last line in the table

Go to the beginning of the next line

To leave a pallet file:

PGM MGT

Select another file type, such as a conversational program.

Select the desired program.

TNC 425/TNC 415 B/TNC 4074-40

4 Programming

4.13 Adding Comments to the Program

You can add comments to the part program in the PROGRAMMING AND EDITING mode of operation.

Applications:

• To explain steps of the program

• To make general notes

Adding comments to program blocks

You can add comments to a program block immediately after entering the data by pressing the semicolon key ";" on the alphabetic keyboard.

Pressing the key brings the dialog prompt:

C O M M E N T ?

Input:

• Enter your comment and conclude the block by pressing the END key.

• If you decide not to comment after all, press the END or NO ENT key: this will conclude the block with the entered NC data.

If you wish to add a comment to a block that has already been entered, select the block and press a horizontal arrow key until the semicolon and the dialog prompt appear.

To enter a comment as a separate block:

;

Enter your comment on the alphanumeric keyboard.

END

Comments are added behind the entered blocks.

Example

. . .

70 L X+0 Y–10 FMAX

80 ; PRE-POSITIONING ........................................... A comment is indicated by a semicolon at the beginning of

90 L X+10 Y+0 RL F100 the block.

. . .

Start a new block by pressing the semicolon key.

Close the block.

Fig. 4.24: Dialog for entering comments

4-41TNC 425/TNC 415 B/TNC 407

HEIDENHAIN TNC 407 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual