Program defaults for cycles

Overview

Some cycles always use identical cycle parameters, such as the set-up clearance Q200, which you must enter for each cycle definition. With the GLOBAL DEF function you can define these cycle parameters at the beginning of the program, so that they are globally effective for all cycles used in the NC program. In the respective cycle you then use PREDEF to simply reference the value defined at the beginning of the program.

The following GLOBAL DEF functions are available:

Cycle

Call

Further information

100

GENERAL

Definition of generally valid cycle parameters

  • Q200 SET-UP CLEARANCE
  • Q204 2ND SET-UP CLEARANCE
  • Q253 F PRE-POSITIONING
  • Q208 RETRACTION FEED RATE

DEF-active

105

DRILLING

Definition of specific drilling cycle parameters

  • Q256 DIST FOR CHIP BRKNG
  • Q210 DWELL TIME AT TOP
  • Q211 DWELL TIME AT DEPTH

DEF-active

110

POCKET MILLING

Definition of specific pocket-milling cycle parameters

  • Q370 TOOL PATH OVERLAP
  • Q351 CLIMB OR UP-CUT
  • Q366 PLUNGE

DEF-active

111

CONTOUR MILLING

Definition of specific contour-milling cycle parameters

  • Q2 TOOL PATH OVERLAP
  • Q6 SET-UP CLEARANCE
  • Q7 CLEARANCE HEIGHT
  • Q9 ROTATIONAL DIRECTION

DEF-active

125

POSITIONING

Definition of the positioning behavior with CYCL CALL PAT

  • Q345 SELECT POS. HEIGHT

DEF-active

120

PROBING

Definition of specific touch probe cycle parameters

  • Q320 SET-UP CLEARANCE
  • Q260 CLEARANCE HEIGHT
  • Q301 MOVE TO CLEARANCE

DEF-active

Entering GLOBAL DEF definitions

  1. Select Insert NC function
  2. The control opens the Insert NC function window.
  3. Select GLOBAL DEF
  4. Select the desired GLOBAL DEF function (e.g., 100 GENERAL)
  5. Enter the required definitions

Using GLOBAL DEF information

If you entered the corresponding GLOBAL DEF functions at program start, you can reference these globally valid values for the definition of any cycle.

Proceed as follows:

  1. Select Insert NC function
  2. The control opens the Insert NC function window.
  3. Select and define GLOBAL DEF
  4. Select Insert NC function again
  5. Select the desired cycle (e.g., 200 DRILLING)
  6. If the cycle includes global cycle parameters, the control superimposes the selection possibility PREDEF in the action bar or in the form as a selection menu.

  1. Select PREDEF
  2. The control then enters the word PREDEF in the cycle definition. This creates a link to the corresponding GLOBAL DEF parameter that you defined at the beginning of the program.
 
Notice
Danger of collision!
If you later edit the program settings with GLOBAL DEF, these changes will affect the entire NC program. This may change the machining sequence significantly. There is a danger of collision!
  1. Make sure to use GLOBAL DEF carefully. Simulate your program before executing it
  2. If you enter fixed values in the cycles, they will not be changed by GLOBAL DEF.

Global data valid everywhere

Parameters valid for all machining cycles 2xx and the touch probe cycles 451, 452

Help graphic

Parameter

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999

Q204 2nd set-up clearance?

Distance in the tool axis between the tool and the workpiece (fixtures) at which no collision can occur. This value has an incremental effect.

Input: 0...99999.9999

Q253 Feed rate for pre-positioning?

Feed rate at which the control moves the tool within a cycle.

Input: 0...99999.999 or FMAX, FAUTO

Q208 Feed rate for retraction?

Feed rate at which the control retracts the tool.

Input: 0...99999.999 or FMAX, FAUTO

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.

Example

11 GLOBAL DEF 100 GENERAL ~

Q200=+2

;SET-UP CLEARANCE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q253=+750

;F PRE-POSITIONING ~

Q208=+999

;RETRACTION FEED RATE

Global data for drilling operations

The parameters apply to the drilling, tapping, and thread milling cycles 200 to 209, 240, 241, 262 to 267.

Help graphic

Parameter

Q256 Retract dist. for chip breaking?

Value by which the control retracts the tool during chip breaking. This value has an incremental effect.

Input: 0.1...99999.9999

Q210 Dwell time at the top?

Time in seconds that the tool remains at set-up clearance after having been retracted from the hole for chip removal.

Input: 0...3600.0000

Q211 Dwell time at the depth?

Time in seconds that the tool remains at the hole bottom.

Input: 0...3600.0000

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.

Example

11 GLOBAL DEF 105 DRILLING ~

Q256=+0.2

;DIST FOR CHIP BRKNG ~

Q210=+0

;DWELL TIME AT TOP ~

Q211=+0

;DWELL TIME AT DEPTH

Global data for milling operations with pocket cycles

The parameters apply to the cycles 208, 232, 233, 251 to 258, 262 to 264, 267, 272, 273, 275, and 277

Help graphic

Parameter

Q370 Path overlap factor?

Q370 x tool radius = stepover factor k.

Input: 0.1...1999

Q351 Direction? Climb=+1, Up-cut=-1

Type of milling operation. The direction of spindle rotation is taken into account.

+1 = climb milling

–1 = up-cut milling

(If you enter 0, climb milling is performed.)

Input: -1, 0, +1

Q366 Plunging strategy (0/1/2)?

Type of plunging strategy:

0: Vertical plunging. The control plunges perpendicularly, regardless of the plunging angle ANGLE defined in the tool table.

1: Helical plunging. In the tool table, the plunging angle ANGLE for the active tool must be defined as not equal to 0. Otherwise, the control will display an error message

2: Reciprocating plunge. In the tool table, the plunging angle ANGLE for the active tool must be defined as not equal to 0. Otherwise, the control will display an error message. The reciprocation length depends on the plunging angle. As a minimum value the control uses twice the tool diameter.

Input: 0, 1, 2

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.

Example

11 GLOBAL DEF 110 POCKET MILLING ~

Q370=+1

;TOOL PATH OVERLAP ~

Q351=+1

;CLIMB OR UP-CUT ~

Q366=+1

;PLUNGE

Global data for milling operations with contour cycles

The parameters apply to the cycles 20, 24, 25, 27 to 29, 39, and 276

Help graphic

Parameter

Q2 Path overlap factor?

Q2 x tool radius = stepover factor k

Input: 0.0001...1.9999

Q6 Set-up clearance?

Distance between tool tip and the top surface of the workpiece. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q7 Clearance height?

Height at which the tool cannot collide with the workpiece (for intermediate positioning and retraction at the end of the cycle). This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q9 Direction of rotation? cw = -1

Machining direction for pockets

  • Q9 = –1 up-cut milling for pocket and island
  • Q9 = +1 climb milling for pocket and island

Input: -1, 0, +1

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.

Example

11 GLOBAL DEF 111 CONTOUR MILLING ~

Q2=+1

;TOOL PATH OVERLAP ~

Q6=+2

;SET-UP CLEARANCE ~

Q7=+50

;CLEARANCE HEIGHT ~

Q9=+1

;ROTATIONAL DIRECTION

Global data for positioning behavior

The parameters apply to each fixed cycle that you call with the CYCL CALL PAT function.

Help graphic

Parameter

Q345 Select positioning height (0/1)

Retraction in the tool axis at the end of a machining step, return to the 2nd set-up clearance or to the position at the beginning of the unit.

Input: 0, 1

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.

Example

11 GLOBAL DEF 125 POSITIONING ~

Q345=+1

;SELECT POS. HEIGHT

Global data for probing functions

The parameters apply to all touch-probe cycles 4xx and 14xx as well as the Cycles 271, 1271, 1272, 1273, 1274, 1278

Help graphic

Parameter

Q320 Set-up clearance?

Additional distance between touch point and ball tip. Q320 is active in addition to the SET_UP column in the touch probe table. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q260 Clearance height?

Coordinate in the tool axis at which no collision between touch probe and workpiece (fixtures) can occur. This value has an absolute effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q301 Move to clearance height (0/1)?

Define how the touch probe will move between the measuring points:

0: Move to measuring height between measuring points

1: Move to clearance height between measuring points

Input: 0, 1

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.

Example

11 GLOBAL DEF 120 PROBING ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q301=+1

;MOVE TO CLEARANCE