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
| DEF-active | |
105 | DRILLING Definition of specific drilling cycle parameters
| DEF-active | |
110 | POCKET MILLING Definition of specific pocket-milling cycle parameters
| DEF-active | |
111 | CONTOUR MILLING Definition of specific contour-milling cycle parameters
| DEF-active | |
125 | POSITIONING Definition of the positioning behavior with CYCL CALL PAT
| DEF-active | |
120 | PROBING Definition of specific touch probe cycle parameters
| DEF-active |
Entering GLOBAL DEF 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:
|
|
- Make sure to use GLOBAL DEF carefully. Simulate your program before executing it
- 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.
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.
11 GLOBAL DEF 100 GENERAL ~ | ||
| ||
| ||
| ||
|
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.
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.
11 GLOBAL DEF 105 DRILLING ~ | ||
| ||
| ||
|
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.
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.
11 GLOBAL DEF 110 POCKET MILLING ~ | ||
| ||
| ||
|
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
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.
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.
11 GLOBAL DEF 111 CONTOUR MILLING ~ | ||
| ||
| ||
| ||
|
Global data for positioning behavior
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.
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.
11 GLOBAL DEF 125 POSITIONING ~ | ||
|
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.
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.
11 GLOBAL DEF 120 PROBING ~ | ||
| ||
| ||
|