Fundamentals

Application

The ISO 6983 standard defines a universal NC syntax.

ISO example

On the TNC7 basic, you can program and execute NC programs using the supported ISO syntax elements.

Description of function

In connection with ISO programs, the TNC7 basic provides the following possibilities:

Contents of an ISO program

An ISO program is structured as follows:

ISO syntax

Function

I

File type

ISO programs have an *.i file name extension.

%NAME G71

Start and end of the program

G71

Unit of measure: mm

G70

Unit of measure: Inch

N10

N20

N30

...

NC block numbers

In the optional machine parameter blockIncrement (no. 105409), you define the increment between the block numbers.

N99999999

NC block number for the end of the program

An NC program is incomplete without this NC block number.

The control adds and updates the NC block numbers within the file automatically. The Program workspace exclusively shows successive numbers without taking the defined increment into account.

G01 X+0 Y+0 ...

NC functions

Contents of an NC program

Contents of an NC block

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 G90 X+10 Y+0 G41 F3000 M3

An NC block contains the following syntax elements:

ISO syntax

Function

G01

Syntax initiator

G90

Absolute or incremental input

Absolute and incremental input

X+10 Y+0

G41

Tool radius compensation

Tool radius compensation

F3000

Feed rate

Feed rate

M3

Miscellaneous functions (M functions)

Miscellaneous Functions

ISO example

Example task 1338459

Example solution 1338459

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.

% 1339889 G71

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

; Workpiece blank definition

N20 G31 X+100 Y+100 Z+0

; Workpiece blank definition

N30 T16 G17 S6500

; Tool call

N40 G00 G90 Z+250 G40 M3

; Clearance height in the tool axis

N50 G00 X-20 Y-20

; Pre-positioning in the machining plane

N60 G00 Z+5

; Pre-positioning in the tool axis

N70 G01 Z-5 F3000 M8

; Feed to working depth

N80 G01 X+5 Y+5 G41 F700

; First contour point

N90 G26 R8

; Approach function

N100 G01 Y+95

; Straight line

N110 G01 X+95

N120 G24 R10

; Chamfer

N130 G01 Y+5

N140 G24 R20

N150 G01 X+5

N160 G27 R8

; Departure function

N170 G01 X-20 Y-20 G40 F1000

; Clearance height in the machining plane

N180 G00 Z+250

; Clearance height in the tool axis

N190 T6 G17 S6500

; Tool call

N200 G00 G90 Z+250 G40 M3

N210 G00 X+50 Y+50 M8

N220 CYCL DEF 254 CIRCULAR SLOT ~

Q215=+0

;MACHINING OPERATION ~

Q219=+15

;SLOT WIDTH ~

Q368=+0.1

;ALLOWANCE FOR SIDE ~

Q375=+60

;PITCH CIRCLE DIAMETR ~

Q367=+0

;REF. SLOT POSITION ~

Q216=+50

;CENTER IN 1ST AXIS ~

Q217=+50

;CENTER IN 2ND AXIS ~

Q376=+45

;STARTING ANGLE ~

Q248=+225

;ANGULAR LENGTH ~

Q378=+0

;STEPPING ANGLE ~

Q377=+1

;NR OF REPETITIONS ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-5

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q369=+0.1

;ALLOWANCE FOR FLOOR ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q338=+5

;INFEED FOR FINISHING ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q366=+2

;PLUNGE ~

Q385=+500

;FINISHING FEED RATE ~

Q439=+0

;FEED RATE REFERENCE

N230 G79

; Cycle call

N240 G00 Z+250 M30

N99999999 % 1339889 G71

Notes