ISO syntax

Keys

You can use the following keys to insert ISO syntax:

Key

ISO syntax

Further information

Tool call T

Tool definition G99

Straight line G01

Chamfer G24

Rounding arc G25

Circular arc G02

Circular arc G03

Circular arc G05

Tangential arc G06

Label G98

Subprogram call and program-section repeat L

Stop in the NC program G38

Absolute and incremental input

The control provides the following possibilities to enter dimensions:

Syntax

Meaning

G90

Absolute input always references an origin. For Cartesian coordinates, the origin is the datum and for polar coordinates the origin is the pole and the angle reference axis.

G91 corresponds to the I Klartext syntax

Incremental input always references the previously programmed coordinates. For Cartesian coordinates, these are the values in the X, Y, and Z axes, and for polar coordinates, the values of the polar coordinate radius R and the polar coordinate angle H.

Tool axis

In some NC functions, you can select a tool axis in order, for example, to define the working plane.

 
Machine

The control’s full range of functions is available only if the Z tool axis is used (e.g., PATTERN DEF).

Restricted use of the tool axes X and Y is possible when prepared and configured by the machine manufacturer.

The control differentiates between the following tool axes:

Syntax

Working plane

G17 corresponds to the Z tool axis

XY, as well as UV, XV, UY

G18 corresponds to the Y tool axis

ZX, as well as VW, YW, VZ

G19 corresponds to the X tool axis

YZ, as well as WU, ZU, WX

Workpiece blank

Use the G30 and G31 NC functions to define a cuboid workpiece blank for simulation in the NC program.

You define the cuboid by entering a MIN point for the bottom front left corner and a MAX point for the top rear right corner.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N10 G30 G17 X+0 Y+0 Z-40

; Define MIN point

N20 G31 X+100 Y+100 Z+0

; Define MAX point

G30 and G31 correspond to the Klartext syntax BLK FORM 0.1 and BLK FORM 0.2.

Defining a workpiece blank with BLK FORM

With G17, G18, and G19, you define the tool axis.

Tool axis

With the Klartext syntax, you can additionally define the following workpiece blanks:

Tools

Tool call

Cutting data

Spindle speed

The spindle speed S is defined as spindle revolutions per minute (rpm).

Alternatively, the constant cutting speed VC in meters per minute (m/min) can be defined.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 T1 G17 S( VC = 200 )

; Tool call with constant cutting speed

Spindle speed S

Feed rate

The feed rate for linear axes is defined in millimeters per minute (mm/min).

In inch programs, the feed rate must be defined in 1/10 inch/min.

The feed rate for rotary axes is defined in degrees per minute (°/min).

The feed rate can be defined with an accuracy of three decimal places.

Feed rate F

Tool definition

With the G99 NC function, you can define the dimensions/allowance of a tool.

 
Machine

Refer to your machine manual.

A tool definition created with G99 is a machine-dependent function.

HEIDENHAIN recommends using tool management for the definition of tools instead of G99!

Tool management

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

110 G99 T3 L+10 R+5

; Define tool

G99 corresponds to the TOOL DEF Klartext syntax.

Tool pre-selection using TOOL DEF

Tool pre-selection

When you use the G51 NC function, the control prepares a tool in the magazine, thus reducing the tool-change time.

 
Machine

Refer to your machine manual.

A tool pre-selection defined with G99 is a machine-dependent function.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

110 G51 T3

; Tool pre-selection

G51 corresponds to the TOOL DEF Klartext syntax.

Tool pre-selection using TOOL DEF

Path functions

Straight line

Cartesian coordinates

With the G00 and G01 NC functions, you program a straight movement in rapid traverse or with a machining feed rate in any desired direction.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G00 Z+100 M3

; Straight line at rapid traverse

N120 G01 X+20 Y-15 F200

; Straight line at machining feed rate

If the feed rate was programmed using a numerical value, it is active only up to the NC block in which a new feed rate is programmed. G00 is active only for the NC block in which it was programmed. When the NC block programmed with G00 has been executed, the feed rate programmed most recently with a numerical value becomes active again.

 
Tip

Make sure to program rapid traverse movements exclusively with the G00 NC function instead of very high numerical values. This is the only way to ensure that rapid traverse is active on a block-by-block basis and that you can control rapid traverse independently of the machining feed rate.

G00 and G01 correspond to the L Klartext syntax with FMAX and F.

Straight line L

Polar coordinates

With the G10 and G11 NC functions, you program a straight movement in rapid traverse or with a machining feed rate in any desired direction.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 I+0 J+0

; Pole

N120 G10 R+10 H+10

; Straight line at rapid traverse

N130 G11 R+50 H+50 F200

; Straight line at machining feed rate

The polar coordinate radius R corresponds to the PR Klartext syntax.

The polar coordinate angle H corresponds to the PA Klartext syntax.

G10 and G11 correspond to the LP Klartext syntax with FMAX and F.

Straight line LP

Chamfer

With the G24 NC function, you can insert a chamfer between two straight lines. The chamfer size references the point of intersection you are programming using the straight line.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 X+40 Y+5

; Straight line at machining feed rate

N120 G24 R12

; Chamfer at machining feed rate

N130 G01 X+5 Y+0

; Straight line at machining feed rate

The value following the R syntax element corresponds to the chamfer size.

G24 corresponds to the CHF Klartext syntax.

Chamfer CHF

Rounding arc

With the G25 NC function, you can insert a rounding arc between two straight lines. The rounding arc references the point of intersection you are programming using the straight line.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 X+40 Y+25

; Straight line at machining feed rate

N120 G25 R5

; Rounding arc at machining feed rate

N130 G01 X+10 Y+5

; Straight line at machining feed rate

G25 corresponds to the RND Klartext syntax.

The value following the R syntax element corresponds to the radius of the rounding arc.

Rounding RND

Circle center

Cartesian coordinates

With the I, J, and K or G29 NC functions, you define the circle center.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 I+25 J+25

; Circle center in the XY plane

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G00 X+25 Y+25

; Pre-positioning on a straight line

N120 G29

; Circle center at the last position

  • I, J, and K
  • The circle center is defined in this NC block.

  • G29
  • The control assumes the most recently programmed position as the circle center.

I, J, and K or G29 correspond to the CC Klartext syntax with or without axis values.

Circle center point CC

 
Tip

With I and J, you define the circle center in the X and Y axes. In order to define the Z axis, program K.

Circular path in another plane

Polar coordinates

With the I, J, and K or G29 NC functions, you define a pole. All polar coordinates reference the pole.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 I+25 J+25

; Pole

  • I, J, and K
  • The pole is defined in this NC block.

  • G29
  • The control takes over the most recently programmed position as the pole.

I, J, and K or G29 correspond to the CC Klartext syntax with or without axis values.

Polar coordinate datum at pole CC

Circular arc with center

Cartesian coordinates

With the G02, G03, and G05 NC functions, you program a circular path around a circle center.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 I+25 J+25

; Circle center

N120 G03 X+45 Y+25

; Circular path around circle center

  • G02
  • Circular path in clockwise direction, corresponds to the C Klartext syntax with DR–.

  • G03
  • Circular path in counterclockwise direction, corresponds to the C Klartext syntax with DR+.

  • G05
  • Circular path without direction of rotation, corresponds to the C Klartext syntax without DR.

  • The control uses the most recently programmed direction of rotation.

Circular path C

 
Tip

When you program a radius R, there is no need to define a circle center.

Circular arc with a defined radius

Polar coordinates

With the G12, G13, and G15 NC functions, you program a circular path around a defined pole.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 I+25 J+25

; Pole

N120 G13 H+180

; Circular path around pole

  • G12
  • Circular path in clockwise direction, corresponds to the CP Klartext syntax with DR–.

  • G13
  • Circular path in counterclockwise direction, corresponds to the CP Klartext syntax with DR+.

  • G15
  • Circular path without direction of rotation; corresponds to the CP Klartext syntax without DR.

  • The control uses the most recently programmed direction of rotation.

The polar coordinate angle H corresponds to the PA Klartext syntax.

Circular path CP around pole CC

Circular arc with a defined radius

Cartesian coordinates

With the G02, G03, and G05 NC functions, you program a circular path with a defined radius. If you are programming a radius, no circle center is required.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G03 X+70 Y+40 R+20

; Circular path with a defined radius

  • G02
  • Circular path in clockwise direction, corresponds to the CR Klartext syntax with DR–.

  • G03
  • Circular path in counterclockwise direction, corresponds to the CR Klartext syntax with DR+.

  • G05
  • Circular path without direction of rotation; corresponds to the CR Klartext syntax without DR.

  • The control uses the most recently programmed direction of rotation.

Circular path CR

Circular arc with a tangential transition

Cartesian coordinates

With the G06 NC function, you program a circular path with a tangential transition to the previous path function.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 X+25 Y+30 F300

; Straight line

N120 G06 X+45 Y+20

; Circular path with tangential transition

G06 corresponds to the CT Klartext syntax.

Circular path CT

Polar coordinates

With the G16 NC function, you program a circular path with a tangential transition to the previous path function.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 G42 X+0 Y+35 F300

; Straight line

N120 I+40 J+35

; Pole

N130 G16 R+25 H+120

; Circular path with tangential transition

The polar coordinate radius R corresponds to the PR Klartext syntax.

The polar coordinate angle H corresponds to the PA Klartext syntax.

G16 corresponds to the CTP Klartext syntax.

Circular path CTP

Contour approach and departure

With the G26 and G27 NC functions, you can approach or depart the contour smoothly using a circle segment.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 G40 G90 X-30 Y+50

; Starting point

N120 G01 G41 X+0 Y+50 F350

; First contour point

N130 G26 R5

; Tangential approach

* - ...

N210 G27 R5

; Tangential exit

N220 G00 G40 X-30 Y+50

; End point

HEIDENHAIN recommends the use of the more powerful APPR and DEP NC functions. In some cases, these NC functions combine multiple NC blocks for approaching and departing the contour.

G41 and G42 correspond to the RL and RR Klartext syntax.

Approach and departure functions with Cartesian coordinates

You can also use polar coordinates when programming the APPR and DEP NC functions.

Approach and departure functions with polar coordinates

Programming techniques

Subprograms and program-section repeats

Programming techniques are useful in structuring your NC program and avoiding unnecessary repeats. By using subprograms, you need to define machining positions for multiple tools only once, for example. Program-section repeats, on the other hand, help you avoid multiple programming of identical, successive NC blocks or program sequences. By combining and nesting these two programming techniques, you can keep your NC programs rather short and restrict changes to a few central program locations.

Subprograms and program section repeats with the label LBL

Defining labels

With the G98 NC function, you define a new label in the NC program.

Each label must be unambiguously identifiable in the NC program by its number or name. If a number or a name exists twice in an NC program, the control shows a warning before the NC block.

If you define a label after M30 or M2, it corresponds to a subprogram. Subprograms must always be concluded with a G98 L0. This number is the only one which may exist any number of times in the NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G98 L1

; Start of subprogram defined by a number

N120 G00 Z+100

, Retract at rapid traverse

N130 G98 L0

; End of subprogram

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G98 L "UP"

; Start of subprogram defined by a name

G98 L corresponds to the LBL Klartext syntax.

Defining a label with LBL SET

Calling a subprogram

With the L NC function, you call a subprogram programmed after M30 or M2.

When the control reads the L NC function, it will jump to the defined label and continue execution of the NC program from this NC block. When the control reads G98 L0, it will jump back to the next NC block after the call with L.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 L1

; Call subprogram

L without G98 corresponds to the CALL LBL Klartext syntax.

Calling a label with CALL LBL

 
Tip

In order to define a certain number of desired repetitions (e.g., L1.3), program a program-section repeat.

Program-section repeat

Program-section repeat

Program-section repeats allow you to have a particular program section executed any number of times. The program section must start with a G98 L label definition and end with L. With the numeral after the decimal point, you can define optionally how often you want the control to repeat this program section.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 L1.2

; Call label 1 twice

L without 98 and the numeral after the decimal point correspond to the CALL LBL REP Klartext syntax.

Program-section repeats

Selection functions

Calling an NC program

With the % NC function, you can call another, separate NC program from within an NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 %TNC:\nc_prog\reset.i

; Call NC program

% corresponds to the CALL PGM Klartext syntax.

Calling an NC program with CALL PGM

Activating a datum table in the NC program

With the %:TAB: NC function, you can activate a datum table from within an NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 %:TAB: "TNC:\table\zeroshift.d"

; Activate datum table

%:TAB corresponds to the SEL TABLE Klartext syntax.

Activating a datum table in the NC program

Selecting a point table

With the %:PAT: NC function, you can activate a point table from within an NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 %:PAT: "TNC:\nc_prog\positions.pnt"

; Activate point table

%:PAT corresponds to the SEL PATTERN Klartext syntax.

Selecting the point table in the NC program with SEL PATTERN

Selecting an NC program with contour definitions

With the %:CNT: NC function, you can select another NC program with a contour definition from within an NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 %:PAT: "TNC:\nc_prog\contour.h"

; Select NC program with contour definition

The Contour graphics workspace

%:CNT corresponds to the SEL CONTOUR Klartext syntax.

Selecting an NC program with contour definition

Selecting and calling an NC program

With the %:PGM: NC function, you can select another, separate NC program. With the %<>% NC function, you call the selected NC program at a different location in the active NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 %:PGM: "TNC:\nc_prog\reset.i"

; Select NC program

* - ...

N210 %<>%

; Call the selected NC program

%:PGM: and %<>% correspond to the SEL PGM and CALL SELECTED PGM Klartext syntax.

Calling an NC program with CALL PGM

Selecting an NC program and calling it with SEL PGM and CALL SELECTED PGM

Defining an NC program as a cycle

With the G: : NC function, you can define another NC program as a machining cycle from within an NC program.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G: : "TNC:\nc_prog\cycle.i"

; Define NC program as a machining cycle

G: : corresponds to the SEL CYCLE Klartext syntax.

Defining and calling an NC program as cycle

Cycle call

For cycles that remove material, you have to enter not only the cycle definition, but also the cycle call in the NC program. The call always refers to the machining cycle that was defined last in the NC program.

The control provides the following options for calling a cycle:

Syntax

Meaning

G79 corresponds to the CYCL CALL Klartext syntax

The control calls the most recently programmed machining cycle at the last programmed position.

G79 PAT corresponds to the CYCL CALL PAT Klartext syntax

The control calls the most recently programmed machining cycle at all positions you have defined in a point table.

G79|G00 corresponds to the Klartext syntax CYCL CALL POS with FMAX

The control calls the most recently programmed machining cycle at the position you defined in the NC block with G79|G00. The control moves to the defined position at rapid traverse.

G79|G01 corresponds to the Klartext syntax CYCL CALL POS with F

The control calls the most recently programmed machining cycle at the position you defined in the NC block with G79|G01. The control moves to the defined position at the machining feed rate.

M89 and M99

With M99, the control executes the most recently programmed machining cycle at the most recently programmed position.

With M89, the control executes the most recently programmed machining cycle after each positioning block until it reads M99.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G79 M3

; Call cycle

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G79 PAT F200 M3

; Call cycle at all positions in the point table

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G79|G01 G90 X+0 X+25

; Call cycle at the defined position

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 G01 X+0 X+25 M89

; Call cycle at the defined position and for each new positioning block

N120 G01 X+25 Y+25

N130 G01 X+50 Y+25 M99

; Call cycle for the last time at the defined position

Calling cycles

Tool radius compensation

When tool radius compensation is active, the control will no longer reference the positions in the NC program to the tool center point, but to the cutting edge.

An NC block can contain the following tool radius compensations:

Syntax

Meaning

G40 corresponds to the R0 Klartext syntax

Reset an active tool radius compensation, positioning based on the tool center point

G41 corresponds to the RL Klartext syntax

Tool radius compensation, on the left of the contour

G42 corresponds to the RR Klartext syntax

Tool radius compensation, on the right of the contour

Tool radius compensation

Miscellaneous functions (M functions)

Programming variables

The control provides the following options for programming variables in ISO programs:

Function group

Further information

Basic arithmetic operations

Trigonometric functions

Circle calculations

Jump commands

Special functions

String functions

Corresponds to the Klartext syntax

String functions

Counters

Corresponds to the Klartext syntax

Defining counters with FUNCTION COUNT

Calculations using formulas

Corresponds to the Klartext syntax

Formulas in the NC program

Function for the definition of complex contours

Corresponds to the Klartext syntax

Complex contour formula

The control distinguishes between the Q, QL, QR, and QS variable types (parameter types).

Programming with variables

 
Tip

Not all NC functions for programming variables are available in ISO programs (e.g., accessing tables with SQL statements).

Table access with SQL statements

Basic arithmetic operations

With the D01 through D05 functions, you can calculate values within your NC program. If you want to calculate with variables, you need to assign an initial value to each variable by means of the D00 function.

The control provides the following functions:

Syntax

Meaning

D00

Assignment

Assign a value or the Undefined status

D01

Addition

Calculate and assign the sum of two values

D02

Subtraction

Calculate and assign the difference of two values.

D03

Multiplication

Calculate and assign the product of two values.

D04

Division

Calculate and assign the quotient of two values

Restriction: You cannot divide by 0

D05

Square root

Calculate and assign the square root of a number

Restriction: You cannot calculate a square root from a negative value

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D00 Q5 P01 +60

; Assignment Q5 = 60

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D01 Q1 P01 –Q2 P02 –5

; Addition Q1 = –Q2+(–5)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D02 Q1 P01 +10 P02 +5

; Subtraction Q1 = +10–(+5)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D03 Q2 P01 +3 P02 +3

; Multiplication Q2 = 3*3

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D04 Q4 P01 +8 P02 +Q2

; Division Q4 = 8/Q2

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D05 Q20 P01 4

; Square root Q20 =4

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

The Basic arithmetic folder

 
Tip

HEIDENHAIN recommends direct formula input, as this allows you to program multiple arithmetic operations in one NC block.

Formulas in the NC program

Trigonometric functions

You can use these functions to calculate trigonometric functions for purposes such as programming variable triangular contours.

The control provides the following functions:

Syntax

Meaning

D06

Sine

Calculate and assign the sine of an angle in degrees

D07

Cosine

Calculate and assign the cosine of an angle in degrees

D08

Root of the sum of squares

Calculate and assign the length based on two values (e.g., to calculate the third side of a triangle).

D13

Angle

Calculate and assign the angle from the opposite side and the adjacent side using arctan or from the sine and cosine of the angle (0 < angle < 360°)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D06 Q20 P01 –Q5

; Sine, Q20 = sin(–Q5)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D07 Q21 P01 –Q5

; Cosine, Q21 = cos(–Q5)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D08 Q10 P01 +5 P02 +4

; Root of the sum of squares, Q10 = (52+42)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D13 Q20 P01 +10 P02 –Q1

; Angle, Q20 = arctan(25/–Q1)

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

The Trigonometric functions folder

 
Tip

HEIDENHAIN recommends direct formula input, as this allows you to program multiple arithmetic operations in one NC block.

Formulas in the NC program

Circle calculation

These functions allow you to calculate the center of a circle and the radius of the circle based on the coordinates of three or four points on the circle (e.g., the position and size of a circle segment).

The control provides the following functions:

Syntax

Meaning

D23

Circle data from three points on the circle

The control saves the determined values in three successive Q parameters so that you only need to program the number of the first variable.

D24

Circle data from four points on the circle

The control saves the determined values in three successive Q parameters so that you only need to program the number of the first variable.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D23 Q20 P01 Q30

; Circle data from three points on the circle

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D24 Q20 P01 Q30

; Circle data from four points on the circle

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

The Circle calculation folder

Jump commands

In if-then decisions, the control compares a variable or fixed value with another variable or fixed value. If the condition is fulfilled, the control jumps to the label programmed for the condition.

If the condition is not fulfilled, the control continues with the next NC block.

The control provides the following functions:

Syntax

Meaning

D09

Jump if equal

If both values are equal, the control jumps to the defined label.

Jump if undefined

If the variable is undefined, the control jumps to the defined label.

Jump if defined

If the variable is defined, the control jumps to the defined label.

D10

Jump if not equal

If both values are not equal, the control jumps to the defined label.

D11

Jump if greater than

If the first value is greater than the second one, the control jumps to the defined label.

D12

Jump if less than

If the first value is less than the second one, the control jumps to the defined label.

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D09 P01 +Q1 P02 +Q3 P03 “LBL“

; Jump if equal

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D09 P01 +Q1 IS UNDEFINED P03 “LBL“

; Jump if undefined

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D09 P01 +Q1 IS DEFINED P03 “LBL“

; Jump if defined

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D10 P01 +10 P02 -Q5 P03 10

; Jump if not equal

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D11 P01 +Q1 P02 +10 P03 QS5

; Jump if greater than

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D12 P01 +Q5 P02 +0 P03 “LBL“

; Jump if less than

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

The Jump commands folder

Functions for freely definable tables

You can open any free definable table and subsequently write to it or read from it.

The control provides the following functions:

Syntax

Meaning

D26

D27

D28

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D26 TNC:\DIR1\TAB1.TAB

; Open a freely definable table

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 Q5 = 3.75

; Define the value for the Radius column

N120 Q6 = -5

; Define the value for the Depth column

N130 Q7 = 7,5

; Define the value for the D column

N140 D27 P01 5/“Radius,Depth,D“ = Q5

; Write defined values to the table

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D28 Q10 = 6/“X,Y,D“*

; Read numerical values from the X, Y, and D columns

N120 D28 QS1 = 6/“DOC“*

; Read the alphanumeric value from the DOC column

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

Special functions

The control provides the following functions:

Syntax

Meaning

D14

D16

D18

D19

D20

D29

D37

D38

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D14 P01 1000

; Output error message no. 1000

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D16 P01 F-PRINT TNC:\mask.a / TNC: \Prot1.txt

; Display the output file with D16 on the control screen

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D18 Q25 ID210 NR4 IDX3

; Save the active dimension factor of the Z axis in Q25

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

N110 D38 /"Q-Parameter Q1: %F Q23: %F" P02 +Q1 P02 +Q23

; Write the values of Q1 and Q23 to the log

D corresponds to the FN Klartext syntax.

The numbers of the ISO syntax correspond to the numbers of the Klartext syntax.

P01, P02 etc. are considered as placeholders (e.g., for arithmetic operators included in the Klartext syntax).

 
Notice
Danger of collision!
Changes to the PLC can result in undesired behavior and serious errors (e.g., the control might become inoperable). For this reason, access to the PLC is password-protected. The functions D19, D20, D29, and D37 enable HEIDENHAIN, the machine manufacturer, and suppliers to communicate with the PLC from within an NC program. It is not recommended that machine operators or NC programmers use this function. There is a danger of collision during the execution of these functions and during the subsequent machining operations!
  1. Only use the function in consultation after checking with HEIDENHAIN, the machine manufacturer, or the third-party provider.
  2. Comply with the documentation from HEIDENHAIN, the machine manufacturer, and third-party providers