Pilot

TNC 310
NC-Software
286 140-xx

6/2000
The Pilot Contents

Contents
... is your concise programming guide for the HEIDENHAIN Fundamentals ................................................................... 4
TNC 310 contouring control. For more comprehensive informa-
tion on programming and operating, refer to the TNC User's Contour Approach and Departure ..................................... 1 3
Manual. There you will find complete information on the central Path Functions .................................................................. 1 8
tool file.
Subprograms and Program Section Repeats ................... 25
Certain symbols are used in the Pilot to denote specific types
Working with Cycles ........................................................ 28
of information:
Drilling Cycles ................................................................... 30
Important note Pockets, Studs, and Slots ................................................. 38
Point Patterns ................................................................... 47
Multipass Milling .............................................................. 49
Warning: danger for the user or the machine.
Coordinate Transformation Cycles ................................... 51
The TNC and the machine tool must be prepared by Special Cycles ................................................................... 55
the machine tool builder to perform these functions.
Graphics and Status Displays ........................................... 5 7
Chapter in User's Manual where you will find more
Miscellaneous Functions M ............................................. 5 9
detailed information on the current topic.

This Pilot describes the operation of the TNC 310 as of the

following software number:
Control NC Software Number
TNC 310 286 140-xx

3
 Fundamentals Files in the TNC File type
Fundamentals

Programs in
Programs/Tables
• HEIDENHAIN format .H
Programs and tables are stored in the TNC as files. The file name is
composed of two parts: Tables for
• Tools TOOL .T
3546351.H

File name File type

Maximum length: see table at right
8 characters

Creating a New Part Program

Enter a new file name
Initiate a conversational program.
Select unit of measure for dimensions (mm or inches)

Define the blank form (BLK) for graphics:

Enter the spindle axis
Enter coordinates of the MIN point:
the smallest X, Y and Z coordinates
Enter coordinates of the MAX point:
the greatest X, Y and Z coordinates

1 BLK FORM 0.1 Z X+0 Y+0 Z-50

4 2 BLK FORM 0.2 X+100 Y+100 Z+0
Choosing the screen layout

Fundamentals
See Chapter 1, “Introduction” in the User’s Manual.

Show soft keys for setting the screen layout

Mode of operation Options

Program run, Full Seq. Program
Program run, single block
Test run
Program at left
Program information at right
Program at left
Program at left, tool information at right
Additional position display
at right
Program at left
Tool information at right
Program at left
Active coordinate
transformations at right
Continued on next page

5
 Mode of operation Options
Fundamentals

Programming and editing Program

Programming graphics

Program at left
Programming graphics right
Program at left
Graphics illustrating input
parameters at right

You cannot change the screen layout in the manual and Program at left, graphic support at right
positioning with MDI modes.

6
Absolute Cartesian Coordinates

Fundamentals
The dimensions are measured from the current datum.
The tool moves to the absolute coordinates.

Programmable axes in an NC block

Linear motion: any 3 axes
Circular motion: 2 linear axes in a plane

Incremental Cartesian Coordinates

The dimensions are measured from the last programmed position of
the tool.

The tool moves by the incremental coordinates.

7
 Circle Center and Pole: CC
Fundamentals
The circle center (CC) must be entered to program circular tool move-
ments with the path function C (see page 17). CC is also needed to
define the pole for polar coordinates.

CC is entered in Cartesian coordinates*.

An absolutely defined circle center or pole is always measured from

the workpiece datum.

An incrementally defined circle center or pole is always measured from

the last programmed position of the workpiece.

Angle Reference Axis

Angles – such as a polar coordinate angle PA or an angle of rotation
ROT – are measured from the angle reference axis.

Working plane Ref. axis and 0° direction

X/Y X
Y/Z Y
Z/X Z

8 *Circle center in polar coordinates: See FK programming

Polar Coordinates

Fundamentals
Dimensions in polar coordinates are referenced to the pole (CC).
A position in the working plane is defined by
• Polar coordinate radius PR = Distance of the position from the pole
• Polar coordinate angle PA = Angle from the angle reference axis to
the straight line CC – PR
Incremental dimensions
Incremental dimensions in polar coordinates are measured from the
last programmed position.
Programming polar coordinates
Select the path function

Press the P key

Answer the dialog prompts

Defining Tools
Tool data
Every tool is designated by a tool number between 1 and 254.

Entering tool data

You can enter the tool data (length L and radius R) either:
• centrally in a table (tool file TOOL.T) for common use
by all programs
or
• locally in TOOL DEF blocks within each part program

9
 Tool number
Fundamentals
Tool length
Tool radius R

Program the tool length as its difference ∆L to the zero tool:

∆L>0: The tool is longer than the zero tool
∆L<0: The tool is shorter than the zero tool

With a tool presetter you can measure the actual tool length, then
program that length.

Calling the tool data

Tool number
Working spindle axis: tool axis
Spindle speed S Oversizes on an end mill
Oversize for the tool length DL (e.g. for wear)
Oversize for the tool radius DR (e.g. for wear)
3 TOOL DEF 6 L+7.5 R+3
4 TOOL CALL 6 Z S2000 DL+1 DR+0.5
5 L Z+100 R0 FMAX
6 L X-10 Y-10 R0 FMAX M6
Tool change
• Beware of tool collision when moving to the tool change
position.
• The direction of spindle rotation is defined by M function:
M3: Clockwise
M4: Counterclockwise
• Oversizes for tool length or radius cannot exceed
10 ±99.999 mm!
Tool Compensation

Fundamentals
The TNC compensates the length L and radius R of the tool during
machining.

Length compensation
Beginning of effect:
Tool movement in the spindle axis

End of effect:
Tool exchange or tool with the length L=0

Radius compensation
Beginning of effect:
Tool movement in the working plane with RR or RL

End of effect: S = Start; E = End

Execution of a positioning block with R0

Working without radius compensation (e.g. drilling):

Tool movement with R0

11
 Datum Setting Without a 3D Touch Probe
Fundamentals
During datum setting you set the TNC display to the coordinates of a
known position on the workpiece:
Insert a zero tool with known radius
Select the manual operation or electronic handwheel mode
Touch the reference surface in the tool axis with the tool and enter
its length
Touch the reference surface in the working plane with the tool and
enter the position of the tool center

Datum Setting with a 3D Touch Probe

The fastest, simplest and most accurate way to set a datum is to use a
HEIDENHAIN 3D touch probe.

The following probe functions are provided by the manual operation

and electronic handwheel modes of operation:

Basic rotation

Datum setting in one axis

Datum setting at a corner

Datum setting at a circle center

12
Contour Approach and Departure

Contour Approach and Departure

Starting point P S
PS lies outside of the contour and must be approached without radius
compensation.
Auxiliary point P H
PH lies outside of the contour and is calculated by the TNC.
The tool moves from the starting point PS to the auxiliary point
PH at the feed rate last programmed feed rate!
First contour point P A and last contour point P E
The first contour point PA is programmed in the APPR (approach) block.
The last contour point is programmed as usual.
End point P N
PN lies outside of the contour and results from the DEP (departure)
block. PN is automatically approached with R0.

Path Functions for Approach and Departure

Press the soft key with the desired path function:

Straight line with tangential connection

Straight line perpendicular to the

contour point
Circular arc with tangential connection
Straight line segment tangentially
connected to the contour through an arc
• Program a radius compensation in the APPR block!
• DEP blocks set the radius compensation to 0! 13
 Approaching on a Straight Line with
Contour Approach and Departure
Tangential Connection
Coordinates for the first contour point PA
Distance len (length) from PH to PA
Enter a length Len > 0
Tool radius compensation RR/RL

7 L X+40 Y+10 R0 FMAX M3

8 APPR LT X+20 Y+20 LEN 15 RR F100
9 L X+35 Y+35

Approaching on a Straight Line Perpendicular to

the First Contour Element
Coordinates for the first contour point PA
Distance len (length) from PH to PA
Enter a length Len > 0
Radius compensation RR/RL

7 L X+40 Y+10 R0 FMAX M3

8 APPR LN X+10 Y+20 LEN 15 RR F100
9 L X+20 Y+35

14
Approaching Tangentially on an Arc

Contour Approach and Departure

Coordinates for the first contour point PA
Radius R
Enter a radius R > 0
Circle center angle (CCA)
Enter a CCA > 0
Tool radius compensation RR/RL
Tool radius compensation RR/RL

7 L X+40 Y+10 R0 FMAX M3

8 APPR CT X+10 Y+20 CCA 180 R10 RR F100
9 L X+20 Y+35

Approaching Tangentially on an Arc

and a Straight Line
Coordinates for the first contour point PA
Radius R
Enter a radius R > 0
Tool radius compensation RR/RL

7 L X+40 Y+10 R0 FMAX M3

8 APPR LCT X+10 Y+20 R10 RR F100
9 L X+20 Y+35

15
 Departing Tangentially on a Straight Line
Contour Approach and Departure
Distance len (length) from PE to PN
Enter a length LEN > 0

23 L X+30 Y+35 RR F100

24 L Y+20 RR F100
25 DEP LT LEN 12.5 F100 M2

Departing on a Straight Line

Perpendicular to the Last Contour Element
Distance len (length) from PE to PN
Enter a length LEN > 0

23 L X+30 Y+35 RR F100

24 L Y+20 RR F100
25 DEP LN LEN+20 F100 M2

16
Departing Tangentially on an Arc

Contour Approach and Departure

Radius R
Enter a radius R > 0
Circle center angle (CCA)

23 L X+30 Y+35 RR F100

24 L Y+20 RR F10
25 DEP CT CCA 180 R+8 F100 M2

Departing on an Arc Tangentially Connecting

the Contour and a Straight Line
Coordinates of the end point PN
Radius R
Enter a radius R > 0

23 L X+30 Y+35 RR F100

24 L Y+20 RR F100
25 DEP LCT X+10 Y+12 R8 F100 M2

17
 Path Functions for Positioning Blocks Path Functions
Path Functions

See “Programming: programming contours”

Straight line Page 19
Programming the Direction of Traverse
Regardless of whether the tool or the workpiece is actually moving,
you always program as if the tool is moving and the workpiece is Chamfer between two
Page 20
stationary. straight lines

Entering the Target Positions

Target positions can be entered in Cartesian or polar coordinates –
Corner rounding Page 20
either as absolute or incremental values, or with both absolute and
incremental values in the same block.

Entries in the Positioning Block Circle center or pole for

Page 21
A complete positioning block contains the following data: polar coordinates
• Path function
• Coordinates of the contour element end points (target position)
• Radius compensation RR/RL/R0 Circular path around the Page 21
• Feed rate F circle center CC
• Miscellaneous function M

Before you execute a part program, always pre-position the tool Circular path with
Page 22
to prevent the possibility of damaging the tool or workpiece. known radius

Circular path with

tangential connection Page 23
to previous contour

18
Straight Line

Path Functions
Coordinates of the straight line end point
Tool radius compensation RR/RL/R0
Feed rate F
Miscellaneous function M

With Cartesian coordinates:

7 L X+10 Y+40 RL F200 M3
8 L IX+20 IY-15
9 L X+60 IY-10

With polar coordinates:

12 CC X+45 Y+25
13 LP PR+30 PA+0 RR F300 M3
14 LP PA+60
15 LP IPA+60
16 LP PA+180

• You must first define the pole (CC) before you can program
polar coordinates.
• Program the pole only in Cartesian coordinates!
• The pole remains effective until you define a new one.

19
 Inserting a Chamfer Between Two Straight Lines
Path Functions
Chamfer side length
Feed rate F for the chamfer

7 L X+0 Y+30 RL F300 M3

8 L X+40 IY+5
9 CHF 12
10 L IX+5 Y+0

• You cannot start a contour with a CHF block.

• The radius compensation before and after the CHF block
must be the same.
• An inside chamfer must be large enough to accommodate
the current tool.

Corner Rounding
The beginning and end of the arc extend tangentially from the previous
and subsequent contour elements.

Radius R of the circular arc

Feed rate F for corner rounding

5 L X+10 Y+40 RL F300 M3

6 L X+40 Y+25
7 RND R5 F100
8 L X+10 Y+5

An inside arc must be large enough to accommodate the

20 current tool.
Circular Path Around the Circle Center CC

Path Functions
Coordinates of the circle center CC

Coordinates of the arc end point

Direction of rotation DR

C and CP enable you to program a complete circle in one block.

With Cartesian coordinates:

5 CC X+25 Y+25
6 L X+45 Y+25 RR F200 M3
7 C X+45 Y+25 DR+

With polar coordinates:

18 CC X+25 Y+25
19 LP PR+20 PA+0 RR F250 M3
20 CP PA+180 DR+

• Define the pole (CC) before programming polar coordinates.

• Program the pole only in Cartesian coordinates.
• The pole remains effective until you define a new one.
• The arc end point can be defined only with the polar
coordinate angle (PA).

21
 Circular Path with Known Radius (CR)
Path Functions
Coordinates of the arc end point
Radius R
If the central angle ZW > 180, R is negative.
If the central angle ZW < 180, R is positive.
Direction of rotation DR

10 L X+40 Y+40 RL F200 M3 Arc starting point

11 CR X+70 Y+40 R+20 DR- Arc 1 or
11 CR X+70 Y+40 R+20 DR+ Arc 2

Arcs 1 and 2 Arcs 3 and 4

10 L X+40 Y+40 RL F200 M3 Arc starting point
11 CR X+70 Y+40 R-20 DR- Arc 3 or
11 CR X+70 Y+40 R-20 DR+ Arc 4

22
Circular Path CT with Tangential Connection

Path Functions
Coordinates of the arc end point
Radius compensation RR/RL/R0
Feed rate F
Miscellaneous function M

With Cartesian coordinates:

5 L X+0 Y+25 RL F250 M3
6 L X+25 Y+30
7 CT X+45 Y+20
8 L Y+0

With polar coordinates:

12 CC X+40 Y+35
13 L X+0 Y+35 RL F250 M3
14 LP PR+25 PA+120
15 CTP PR+30 PA+30
16 L Y+0

• Define the pole (CC) before programming polar coordinates.

• Program the pole only in Cartesian coordinates.
• The pole remains effective until you define a new one.

23
 Helix (Only in Polar Coordinates)
Path Functions
Calculations (upward milling direction)
Path revolutions: n = Thread revolutions + overrun at start and
end of thread
Total height: h = Pitch P x path revolutions n
Incr. coord. angle: IPA = Path revolutions n x 360°
Start angle: PA = Angle at start of thread + angle for
overrun
Start coordinate: Z = Pitch P x (thread revolutions + thread
overrun at start of thread)
Shape of helix
Internal thread Work direction Rotation Radius comp.
Right-hand Z+ DR+ RL
Left-hand Z+ DR– RR
Right-hand Z– DR– RR
Left-hand Z– DR+ RL
External thread
Right-hand Z+ DR+ RR
Left-hand Z+ DR– RL
Right-hand Z– DR– RL
Left-hand Z– DR+ RR

M6 x 1 mm thread with 5 revolutions :

12 CC X+40 Y+25
13 L Z+0 F100 M3
14 LP PR+3 PA+270 RL
15 CP IPA-1800 IZ+5 DR- RL F50
24
Subprograms and Program Section

Subprograms
Repeats
Subprograms and program section repeats enable you to program a
machining sequence once and then run it as often as needed.

Working with Subprograms

1 The main program runs up to the subprogram call CALL LBL1.
2 The subprogram – labeled with LBL1 – runs through to its end
(LBL0).
3 The main program resumes.

It's good practice to place subprograms after the end of the main
program (M2).
S = Jump; R = Return jump
• Answer the dialog prompt REP with the NOENT key.
• You cannot call LBL0.

Working with Program Section Repeats

1 The main program runs up to the call for a section repeat
CALL LBL1 REP2/2.
2 The program section between LBL1 and CALL LBL1 REP2/2 is
repeated the number of times indicated with REP.
3 After the last repetition the main program resumes.
Altogether, the program section is run once more than the
number of programmed repeats.
25
 Subprogram Nesting:
Subprograms
A Subprogram within a Subprogram
1 The main program runs up to the first subprogram call CALL LBL1.
2 Subprogram 1 runs up to the second subprogram call CALL LBL2.
3 Subprogram 2 runs to its end.
4 Subprogram 1 resumes and runs to its end.
5 The main program resumes.

• A subprogram cannot call itself.

• Subprograms can be nested up to a maximum depth of
8 levels.

26 S = Jump; R = Return jump

Any Program as a Subprogram

Subprograms
1 The calling program 1 runs up to the program call CALL PGM 21.
2 The called program 21 runs through to its end.
3 The calling program 1 resumes.

The called program must not be ended with M2 or M30!

S = Jump; R = Return jump

27
 Working with Cycles Drilling
Working with Cycles
1 PECKING Page 30
Certain frequently needed machining sequences are stored in the TNC 200 DRILLING Page 31
as cycles. Coordinate transformations and some special functions are 201 REAMING Page 32
also available as cycles. 202 BORING Page 33
203 UNIVERSAL DRILLING Page 34
• In a cycle, positioning data entered in the tool axis are always 204 BACK BORING Page 35
incremental, even without the I key. 2 TAPPING Page 36
• The algebraic sign for the cycle parameter DEPTH defines 17 RIGID TAPPING Page 37
the working direction! Pockets, Studs, and Slots

Example 4 POCKET MILLING Page 38

212 POCKET FINISHING Page 39
6 CYCL DEF 1.0 PECKING 213 STUD FINISHING Page 40
7 CYCL DEF 1.1 SET UP 2 5 CIRCULAR POCKET MILLING Page 41
8 CYCL DEF 1.2 DEPTH -15 214 CIRCULAR POCKET FINISHING Page 42
9 CYCL DEF 1.3 PECKG 10 215 CIRCULAR STUD FINISHING Page 43
... 3 SLOT MILLING Page 44
210 SLOT WITH RECIP. PLUNGE Page 45
Feed rates are entered in mm/min, the dwell time in seconds. 211 CIRCULAR SLOT Page 46
Point Pattern
Defining cycles
220 CIRCULAR PATTERN Page 47
Select the desired cycle: 221 LINEAR PATTERN Page 48
Multipass Milling
Select the cycle group 230 MULTIPASS MILLING Page 49
231 RULED SURFACE Page 50
Select the cycle
Continued on next page

28
 Cycles for Coordinate Transformations

Working with Cycles

7 DATUM SHIFT Page 51
8 MIRROR IMAGE Page 52
10 ROTATION Page 53
11 SCALING FACTOR Page 54
Special Cycles
9 DWELL TIME Page 55
12 PGM CALL Page 55
13 ORIENTED SPINDLE STOP Page 56

Graphically assisted cycle programming

Select the PGM+FIGURE screen layout.

A graphic illustrates the input parameters for cycle definition.

Calling a Cycle
The following cycles are effective as soon as they are defined:
• Cycles for coordinate transformations
• DWELL TIME cycle
• The SL cycle CONTOUR GEOMETRY
• Point patterns

All other cycles go into effect when they are called through
• CYCL CALL: effective for one block
• M99: effective for one block
• M89: effective until canceled (depends on machine parameter
settings) 29
 Drilling Cycles
Drilling Cycles

PECKING (1)
CYCL DEF: Select Cycle 1 PECKING
Setup clearance: A
Total hole depth (Distance from the workpiece surface to
the bottom of the hole): B
Pecking depth: C
Dwell time in seconds
Feed rate F

If TOTAL HOLE DEPTH is greater than or equal to the PECKING

DEPTH, the tool drills the entire hole in one plunge.

6 CYCL DEF 1.0 PECKING

7 CYCL DEF 1.1 SET UP 2
8 CYCL DEF 1.2 DEPTH -15
9 CYCL DEF 1.3 PECKG 7.5
10 CYCL DEF 1.4 DWELL 1
11 CYCL DEF 1.5 F80
12 L Z+100 R0 FMAX M6
13 L X+30 Y+20 FMAX M3
14 L Z+2 FMAX M99
15 L X+80 Y+50 FMAX M99
16 L Z+100 FMAX M2

30
DRILLING (200)

Drilling Cycles
CYCL DEF: Select Cycle 200 DRILLING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Dwell time at top: Q210
Surface coordinate: Q203
2nd set-up clearance: Q204

The TNC automatically pre-positions the tool in the tool axis. If the
DEPTH is greater than or equal to the PECKING DEPTH, the tool drills
to the DEPTH in one plunge.

11 CYCL DEF 200 DRILLING

Q200 = 2 ;SET-UP CLEARANCE
Q201 = -15 ;DEPTH
Q206 = 250 ;FEED RATE FOR PLUNGING
Q202 = 5 ;PECKING DEPTH
Q210 = 0 ;DWELL TIME AT TOP
Q203 = +0 ;SURFACE COORDINATE
Q204 = 100 ;2ND SET-UP CLEARANCE
12 L Z+100 R0 FMAX M6
13 L X+30 Y+20 FMAX M3
14 CYCL CALL
15 L X+80 Y+50 FMAX M99
16 L Z+100 FMAX M2
31
 REAMING (201)
Drilling Cycles
CYCL DEF: Select Cycle 201 REAMING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Dwell time at depth: Q211
Retraction feed rate: Q208
Surface coordinate: Q203
2nd set-up clearance: Q204

The TNC automatically pre-positions the tool in the tool axis.

11 CYCL DEF 201 REAMING

Q200 = 2 ;SET-UP CLEARANCE
Q201 = -15 ;DEPTH
Q206 = 100 ;FEED RATE FOR PLUNGING
Q211 = 0.5 ;DWELL TIME AT DEPTH
Q208 = 250 ;RETRACTION FEED RATE
Q203 = +0 ;SURFACE COORDINATE
Q204 = 100 ;2ND SET-UP CLEARANCE
12 L Z+100 R0 FMAX M6
13 L X+30 Y+20 FMAX M3
14 CYCL CALL
15 L X+80 Y+50 FMAX M99
16 L Z+100 FMAX M2
32
BORING (202)

Drilling Cycles
Danger of collision! Choose a disengaging direction that
moves the tool away from the wall of the hole.

CYCL DEF: Select Cycle 202 BORING

Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of
hole: Q201
Feed rate for plunging: Q206
Dwell time at depth: Q211
Retraction feed rate: Q208
Surface coordinate: Q203
2nd set-up clearance: Q204
Disengaging directn (0/1/2/3/4) at bottom of hole: Q214

The TNC automatically pre-positions the tool in the tool axis.

11 CYCL DEF 202 BORING

Q200 = 2 ;SET-UP CLEARANCE
Q201 = -15 ;DEPTH
Q206 = 100 ;FEED RATE FOR PLUNGING
Q211 = 0.5 ;DWELL TIME AT DEPTH
Q208 = 250 ;RETRACTION FEED RATE
Q203 = +0 ;SURFACE COORDINATE
Q204 = 100 ;2ND SET-UP CLEARANCE
Q214 = 1Di ;DISENGAGING DIRECTION
12 L Z+100 R0 FMAX M6
13 L X+30 Y+20 FMAX M3
14 CYCL CALL
15 L X+80 Y+50 FMAX M99
16 L Z+100 FMAX M2 33
 UNIVERSAL DRILLING (203)
Drilling Cycles
CYCL DEF: Select Cycle 203 UNIVERSAL DRILLING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Dwell time at top: Q210
Surface coordinate: Q203
2nd set-up clearance: Q204
Decrement after each pecking depth: Q212
Nr of breaks – Number of chip breaks before retraction: Q213
Min. pecking depth if a decrement has been entered:
Q205
Dwell time at depth: Q211
Retraction feed rate: Q208

The TNC automatically pre-positions the tool in the tool axis. If the
DEPTH is greater than or equal to the PECKING DEPTH, the tool drills
to the DEPTH in one plunge.

34
COUNTERBORE BACK (204)

Drilling Cycles
CYCL DEF: Select Cycle 204 COUNTERBORE BACK
Set-up clearance: Q200
Depth of counterbore: Q249
Material thickness: Q250
Tool edge off-center distance: Q251
Tool edge height: Q252
Feed rate for pre-positioning: Q253
Feed rate for counterboring: Q254
Dwell time at counterbore floor: Q255
Workpiece surface coordinate: Q203
2nd set-up clearance: Q204
Disengaging direction (0/1/2/3/4): Q214
• Danger of collision! Select the disengaging direction that
gets the tool clear of the counterbore floor!
• Use this cycle only with a reverse boring bar!

11 CYCL DEF 204 COUNTERBORE BACK

Q200 = 2 ;SET-UP CLEARANCE
Q249 = +5 ;DEPTH OF COUNTERBORE
Q250 = 20 ;MATERIAL THICKNESS
Q251 = 3.5 ;OFF-CENTER DISTANCE
Q252 = 15 ;TOOL EDGE HEIGHT
Q253 = 750 ;F PRE-POSITIONING
Q254 = 200 ;F COUNTERBORING
Q255 = 0.5 ;DWELL TIME
Q203 = +0 ;SURFACE COORDINATE
Q204 = 50 ;2ND SET-UP CLEARANCE
Q214 = 1 ;DISENGAGING DIRECTN
35
 TAPPING with Floating Tap Holder (2)
Drilling Cycles
Insert the floating tap holder
CYCL DEF: Select Cycle 2 TAPPING
Set-up clearance: A
Total hole depth (thread length) = Distance between the
workpiece surface and the end of the thread: B
Dwell time in seconds (a value between 0 and 0.5 seconds)
Feed rate F = Spindle speed S x thread pitch P

For tapping right-hand threads, actuate the spindle with M3,

for left-hand threads use M4.

25 CYCL DEF 2.0 TAPPING

26 CYCL DEF 2.1 SET UP 3
27 CYCL DEF 2.2 DEPTH -20
28 CYCL DEF 2.3 DWELL 0.4
29 CYCL DEF 2.4 F100
30 L Z+100 R0 FMAX M6
31 L X+50 Y+20 FMAX M3
32 L Z+3 FMAX M99

36
RIGID TAPPING (17)

Drilling Cycles
• Machine and TNC must be prepared by the machine tool
builder to perform rigid tapping.
• In rigid tapping, the spindle speed is synchronized with the
tool axis feed rate.

CYCL DEF: Select Cycle 17 RIGID TAPPING

Set-up clearance: A
Tapping depth = Distance between workpiece surface and end of
thread: B
Thread pitch: C
The algebraic sign determines the direction of the thread:
• Right-hand thread: +
• Left-hand thread: –

37
 Pockets, Studs, and Slots
Pockets, Studs, and Slots

POCKET MILLING (4)

This cycle requires either a center-cut end mill (ISO 1641) or
pilot drilling at the pocket center.
The tool begins milling in the positive axis direction of the longer side.
In square pockets it moves in the positive Y direction.
Pre-position over the pocket center with radius compensation at R0
CYCL DEF: Select Cycle 4 pocket milling
Set-up clearance: A
Milling depth (depth of the pocket): B
Pecking depth: C
Feed rate for pecking
First side length (length of the pocket, parallel to the first main
axis of the working plane): D
Second side length (width of pocket, sign always positive): E
Feed rate
Rotation clockwise: DR–
Climb milling with M3: DR+
Up-cut milling with M3: DR–
12 CYCL DEF 4.0 POCKET MILLING
13 CYCL DEF 4.1 SET UP 2
14 CYCL DEF 4.2 DEPTH -10
15 CYCL DEF 4.3 PECKG 4 F80
16 CYCL DEF 4.4 X+80
17 CYCL DEF 4.5 Y+40
18 CYCL DEF 4.6 F100 DR+
19 L Z+100 R0 FMAX M6
20 L X+60 Y+35 FMAX M3
38 21 L Z+2 FMAX M99
POCKET FINISHING (212)

Pockets, Studs, and Slots

CYCL DEF: Select Cycle 212 POCKET FINISHING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Feed rate for milling: Q207
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nc axis: Q217
First side length: Q218
Second side length: Q219
Corner radius: Q220
Allowance in 1st axis: Q221

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. If the depth is greater than or equal to the pecking
depth, the tool drills to the depth in one plunge.

39
 STUD FINISHING (213)
Pockets, Studs, and Slots
CYCL DEF: Select Cycle 213 STUD FINISHING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Feed rate for milling: Q207
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nd axis: Q217
First side length: Q218
Second side length: Q219
Corner radius: Q220
Allowance in 1st axis: Q221

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. If the depth is greater than or equal to the pecking
depth, the tool drills to the depth in one plunge.

40
CIRCULAR POCKET MILLING (5)

Pockets, Studs, and Slots

This cycle requires either a center-cut end mill (ISO 1641)
or pilot drilling at pocket center.
Pre-position over the pocket center with radius compensation at R0
CYCL DEF: Select Cycle 5
Set-up clearance: A
Milling depth (depth of the pocket): B
Pecking depth: C
Feed rate for pecking
Circle radius R (radius of the pocket)
Feed rate
Rotation clockwise: DR–
Climb milling with M3: DR+
Up-cut milling with M3: DR–

17 CYCL DEF 5.0 CIRCULAR POCKET

18 CYCL DEF 5.1 SET UP 2
19 CYCL DEF 5.2 DEPTH -12
20 CYCL DEF 5.3 PECKG 6 F80
21 CYCL DEF 5.4 RADIUS 35
22 CYCL DEF 5.5 F100 DR+
23 L Z+100 R0 FMAX M6
24 L X+60 Y+50 FMAX M3
25 L Z+2 FMAX M99

41
 CIRCULAR POCKET FINISHING (214)
Pockets, Studs, and Slots
CYCL DEF: Select Cycle 214 CIRCULAR POCKET FINISHING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Feed rate for milling: Q207
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nd axis: Q217
Workpiece blank dia.: Q222
Finished part dia.: Q223

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. If the depth is greater than or equal to the pecking
depth, the tool drills to the depth in one plunge.

42
CIRCULAR STUD FINISHING (215)

Pockets, Studs, and Slots

CYCL DEF: Select Cycle 215 CIRCULAR STUD FINISHING
Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for plunging: Q206
Pecking depth: Q202
Feed rate for milling: Q207
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nd axis: Q217
Workpiece blank dia.: Q222
Finished part dia.: Q223

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. If the depth is greater than or equal to the pecking
depth, the tool drills to the depth in one plunge.

43
 SLOT MILLING (3)
Pockets, Studs, and Slots
• This cycle requires either a center-cut end mill (ISO 1641)
or pilot drilling at the starting point.
• The cutter diameter must be smaller than the slot width
and larger than half the slot width.

Pre-position the tool over the center of the slot with tool radius
compensation at R0
CYCL DEF: Select Cycle 3 SLOT MILLING
Safety clearance: A
Milling depth (depth of the slot): B
Pecking depth: C
Feed rate for pecking (traverse velocity for plunging)
First side length? (length of the slot): D
The algebraic sign determines the first cutting direction
Second side length? (width of the slot): E
Feed rate (for milling)

10 TOOL DEF 1 L+0 R+6

11 TOOL CALL 1 Z S1500
12 CYCL DEF 3.0 SLOT MILLING
13 CYCL DEF 3.1 SET UP 2
14 CYCL DEF 3.2 DEPTH -15
15 CYCL DEF 3.3 PECKG 5 F80
16 CYCL DEF 3.4 X+50
17 CYCL DEF 3.5 Y+15
18 CYCL DEF 3.6 F120
19 L Z+100 R0 FMAX M6
20 L X+16 Y+25 R0 FMAX M3
44 21 L Z+2 M99
SLOT WITH RECIPROCATING PLUNGE-CUT (210)

Pockets, Studs, and Slots

The cutter diameter must be no larger than the width of the
slot, and no smaller than one third!

CYCL DEF: Select Cycle 210 SLOT RECIP. PLNG

Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for milling: Q207
Pecking depth: Q202
Machining operation (0/1/2) – 0 = roughing and finishing,
1 = roughing only, 2 = finishing only: Q215
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nd axis: Q217
First side length: Q218
Second side length: Q219
Angle of rotation (angle by with the slot is rotated): Q224

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. During roughing the tool plunges obliquely into the
metal in a back-and-forth motion between the ends of the slot. Pilot
drilling is therefore unnecessary.

45
 CIRCULAR SLOT with reciprocating plunge (211)
Pockets, Studs, and Slots
The cutter diameter must be no larger than the width of the
slot, and no smaller than one third!

CYCL DEF: Select Cycle 211 CIRCULAR SLOT

Set-up clearance: Q200
Depth – Distance between workpiece surface and bottom of hole:
Q201
Feed rate for milling: Q207
Pecking depth: Q202
Machining operation (0/1/2) – 0 = roughing and finishing,
1 = roughing only, 2 = finishing only: Q215
Surface coordinate: Q203
2nd set-up clearance: Q204
Center in 1st axis: Q216
Center in 2nd axis: Q217
Pitch circle dia.: Q244
Second side length: Q219
Starting angle of the slot: Q245
Angular length of the slot: Q248

The TNC automatically pre-positions the tool in the tool axis and in the
working plane. During roughing the tool plunges obliquely into the
metal in a back-and-forth helical motion between the ends of the slot.
Pilot drilling is therefore unnecessary.

46
Point Patterns

Point Patterns
CIRCULAR PATTERN (220)
CYCL DEF: Select Cycle 220 CIRCULAR PATTERN
Center in 1st axis: Q216
Center in 2nd axis: Q217
Angle of rotation: Q244
Starting angle: Q245
Stopping angle: Q246
Stepping angle: Q247
Nr of repetitions: Q241
Set-up clearance: Q200
Surface coordinate: Q203
2nd set-up clearance: Q204

• Cycle 220 POLAR PATTERN is effective immediately upon

definition!
• Cycle 220 automatically calls the last defined fixed cycle!
• Cycle 220 can be combined with Cycles 1, 2, 3, 4, 5, 17,
200, 201, 202, 203, 204, 212, 213, 214, 215
• In combined cycles, the set-up clearance, surface coordinate
and 2nd set-up clearance are always taken from Cycle 220!

The TNC automatically pre-positions the tool in the tool axis and in the
working plane.

47
 LINEAR PATTERN (221)
Point Patterns
CYCL DEF: Select Cycle 221 LINEAR PATTERN
Starting pnt 1st axis: Q225
Starting pnt 2nd axis: Q226
Spacing in 1st axis: Q237
Spacing in 2nd axis: Q238
Number of columns: Q242
Number of lines: Q243
Angle of rotation: Q224
Set-up clearance: Q200
Surface coordinate: Q203
2nd set-up clearance: Q204

• Cycle 221 LINEAR PATTERN is effective immediately upon

definition!
• Cycle 221 automatically calls the last defined fixed cycle!
• Cycle 221 can be combined with Cycles 1, 2, 3, 4, 5, 17,
200, 201, 202, 203, 204, 212, 213, 214, 215
• In combined cycles, the set-up clearance, surface coordinate
and 2nd set-up clearance are always taken from Cycle 221!

The TNC automatically pre-positions the tool in the tool axis and in the
working plane.

48
Multipass Milling

Multipass Milling
MULTIPASS MILLING (230)
From the current position, the TNC positions the tool
automatically at the starting point of the first machining
operation, first in the working plane and then in the tool axis.
Pre-position the tool in such a way that there is no danger
of collision with the workpiece or fixtures.

CYCL DEF: Select Cycle 230 MULTIPASS MILLING

Starting point in 1st axis: Q225
Starting point in 2nd axis: Q226
Starting point in 3rd axis: Q227
First side length: Q218
Second side length: Q219
Number of cuts: Q240
Feed rate for plunging: Q206
Feed rate for milling: Q207
Stepover feed rate: Q209
Set-up clearance: Q200

49
 RULED SURFACE (231)
Multipass Milling
Starting from the initial position, the TNC positions the tool at
the starting point (point 1), first in the working plane and then
in the tool axis. Be sure to pre-position the tool in such a way
that there is no danger of collision with the workpiece or
fixtures.

CYCL DEF: Select Cycle 231 RULED SURFACE

Starting point in 1st axis: Q225
Starting point in 2nd axis: Q226
Starting point in 3rd axis: Q227
2nd point in 1st axis: Q228
2nd point in 2nd axis: Q229
2nd point in 3rd axis: Q230
3rd point in 1st axis: Q231
3rd point in 2nd axis: Q232
3rd point in 3rd axis: Q233
4th point in 1st axis: Q234
4th point in 2nd axis: Q235
4th point in 3rd axis: Q236
Number of cuts: Q240
Feed rate for milling: Q207

50
Cycles for Coordinate Transformation

Transformations
Cycles for coordinate transformation permit contours to be
• Shifted Cycle 7 DATUM SHIFT
• Mirrored Cycle 8 MIRROR IMAGE
• Rotated (in the plane) Cycle 10 ROTATION
• Enlarged or reduced Cycle 11 SCALING
Cycles for coordinate transformation are effective upon definition until
they are reset or redefined. The original contour should be defined in a
subprogram. Input values can be both absolute and incremental.

Cycles for Coordinate

DATUM SHIFT
CYCL DEF: Select Cycle 7 DATUM SHIFT
Enter the coordinates of the new datum
To cancel a datum shift: Re-enter the cycle definition with the input
value 0.

9 CALL LBL1 Call the part subprogram

10 CYCL DEF 7.0 DATUM SHIFT
11 CYCL DEF 7.1 X+60
12 CYCL DEF 7.2 Y+40
13 CALL LBL1 Call the part subprogram

When combining transformations, the datum shift must be

programmed before the other transformations. 51
 MIRROR IMAGE (8)
Transformations

CYCL DEF: Select Cycle 8 MIRROR IMAGE

Enter the mirror image axis: Either X, Y, or both

To reset the mirror image, re-enter the cycle definition with NO ENT.

15 CALL LBL1
16 CYCL DEF 7.0 DATUM SHIFT
17 CYCL DEF 7.1 X+60
18 CYCL DEF 7.2 Y+40
19 CYCL DEF 8.0 MIRROR IMAGE
20 CYCL DEF 8.1 Y
Cycles for Coordinate

21 CALL LBL1

• The tool axis cannot be mirrored.

• The cycle always mirrors the original contour (in this example
in subprogram LBL1).

52
ROTATION (10)

Transformations
CYCL DEF: Select Cycle 10 ROTATION
Enter the rotation angle:
• Input range –360° to +360°
• Reference axes for the rotation angle
Working plane Reference axis and 0° direction
X/Y X
Y/Z Y
Z/X Z

To reset a ROTATION, re-enter the cycle with the rotation angle 0.

Cycles for Coordinate

12 CALL LBL1
13 CYCL DEF 7.0 DATUM SHIFT
14 CYCL DEF 7.1 X+60
15 CYCL DEF 7.2 Y+40
16 CYCL DEF 10.0 ROTATION
17 CYCL DEF 10.1 ROT+35
18 CALL LBL1

53
 SCALING (11)
Transformations

CYCL DEF: Select Cycle 11 SCALING

Enter the scaling factor (SCL):
• Input range 0.000001 to 99.999999:
To reduce the contour ... SCL < 1
To enlarge the contour ... SCL > 1

To cancel the SCALING, re-enter the cycle definition with SCL1.

11 CALL LBL1
12 CYCL DEF 7.0 DATUM SHIFT
13 CYCL DEF 7.1 X+60
Cycles for Coordinate

14 CYCL DEF 7.2 Y+40

15 CYCL DEF 11.0 SCALING
16 CYCL DEF 11.1 SCL 0.75
17 CALL LBL1

SCALING can be effective in the working plane only or in all

three main axes (depending on machine parameter 7410)!

54
Special Cycles

Special Cycles
DWELL TIME (9)
The program run is interrupted for the duration of the DWELL TIME.

CYCL DEF: Select Cycle 9 DWELL TIME

Enter the dwell time in seconds.

48 CYCL DEF 9.0 DWELL TIME

49 CYCL DEF 9.1 DWELL 0.5

PGM CALL (12)

CYCL DEF: Select Cycle 12 PGM CALL

Enter the name of the program that you wish to call

Cycle 12 PGM CALL must be called to become active.

7 CYCL DEF 12.0 PGM CALL

8 CYCL DEF 12.1 LOT31
9 L X+37.5 Y-12 R0 FMAX M99

55
 Spindle ORIENTATION
Special Cycles

CYCL DEF: Select Cycle 13 ORIENTATION

Enter the orientation angle referenced to the angle reference axis
of the working plane:
• Input range 0 to 360°
• Input resolution 0.1°
Call the cycle with M19

The machine and TNC must be prepared for spindle orientation

by the machine tool builder.

12 CYCL DEF 13.0 ORIENTATION

13 CYCL DEF 13.1 ANGLE 90

56
Graphics and Status Displays

Graphics and Status Displays

Defining the Workpiece in the Graphic Window

See “Test run and program run, graphics”

In the open program, press the BLK FORM soft key

Spindle axis
MIN and MAX POINT

Interactive Programming Graphics

Select the PGM+GRAPHICS or GRAPHICS screen layout.

The TNC can generate a two-dimensional graphic of the contour while

you are programming it:

Graphic is generated during program input

Graphic is regenerated

Graphic is generated block by block

57
 Test Graphics
Graphics and Status Displays
In the test run mode the TNC can graphically simulate the machining
process. The following display types are available via soft key:

Plan view

Projection in three planes

3D view

Status Displays
Select a screen layout showing the status information that
you need.
In the lower part of the screen in the program run modes the TNC
shows information on
• tool positions
• feed rate
• active miscellaneous functions

Additional status information can be called with the following

soft keys:
Program
Tool data
information
Coordinate
Tool positions
transformations
58
Miscellaneous Functions M

Functions
M00 Stop program run/Stop spindle/Coolant off M93 In the positioning block: coordinates are
M01 Optional program-stop referenced to the current tool position.
M02 Stop program run/Stop spindle/Coolant off Effective in blocks with R0, R+ and R–
Jump back to block 1/Clear status display M94 Reduce rotary axis display to a value below 360°
(depending on machine parameters) M95 Reserved
M03 Spindle on clockwise M96 Reserved

Miscellaneous
M04 Spindle on counterclockwise M97 Machine small contour steps
M05 Stop spindle M98 Suspend tool path compensation
M06 Tool change/Stop program run M99 Cycle call, effective blockwise
(depending on machine parameters)/Stop spindle
M08 Coolant on
M09 Coolant off
M13 Spindle on clockwise/Coolant on
M14 Spindle on counterclockwise/Coolant on
M30 Same function as M02
M89 Vacant miscellaneous function or Cycle call,
modally effective (depending on machine
parameters)
M90 Constant contour speed at corners
(effective only in lag mode)
M91 Within the positioning block: Coordinates are
referenced to the machine datum
M92 Within the positioning block: The coordinates are
referenced to a position defined by the machine
tool builder

59
DR. JOHANNES HEIDENHAIN GmbH
Dr.-Johannes-Heidenhain-Straße 5
83301 Traunreut, Germany
{ +49 (86 69) 31-0
| +49 (86 69) 50 61
E-Mail: info@heidenhain.de
Technical support | +49 (86 69) 31-10 00
E-Mail: service@heidenhain.de
Measuring systems { +49 (86 69) 31-31 04
E-Mail: service.ms-support@heidenhain.de
TNC support { +49 (86 69) 31-31 01
E-Mail: service.nc-support@heidenhain.de
NC programming { +49 (86 69) 31-31 03
E-Mail: service.nc-pgm@heidenhain.de
PLC programming { +49 (86 69) 31-31 02
E-Mail: service.plc@heidenhain.de
Lathe controls { +49 (7 11) 95 28 03-0
E-Mail: service.hsf@heidenhain.de
www.heidenhain.de

Ve 00
331 959-20 · 5/2000 · pdf · Subject to change without notice