Program defaults for cycles

Entering GLOBAL DEF definitions

SF_4_NCFunktion_Einfuegen

  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:

SF_4_NCFunktion_Einfuegen

  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.
SF_4_24_11_Aktionsleiste_PREDEF

  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

These parameters are valid for all 2xx machining cycles as well as for Cycles 880, 1017, 1018, 1021, 1022, 1025 and touch probe cycles 451, 452, 453

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 probing functions

These parameters are valid for all touch probe cycles 4xx and 14xx as well as for Cycles 271, 286, 287, 880, 1021, 1022, 1025, 1271, 1272, 1273, 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)?

Specify how the touch probe moves between measuring points:

0: Move at measuring height between measuring points

1: Move at 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