Point tables

Application

With a point table you can execute one or more cycles in sequence on an irregular point pattern.

Description of function

Coordinates in a point table

If you are using drilling cycles, the coordinates of the working plane in the point table represent the hole centers. If you are using milling cycles, the coordinates of the working plane in the point table represent the starting point coordinates of the respective cycle (e.g., center coordinates of a circular pocket). The coordinates of the spindle axis correspond to the coordinate of the workpiece surface.

The control retracts the tool to the clearance height when traversing between the starting points. Depending on which is greater the control uses either the tool axis coordinate from the cycle call or the value from cycle parameter Q204 2ND SET-UP CLEARANCE.

 
Notice
Danger of collision!
If you program a clearance height for individual points in a point table, the control will ignore the value from the cycle parameter Q204 2ND SET-UP CLEARANCE for all points!
  1. Program the function GLOBAL DEF 125 POSITIONING so that the control will take into account the clearance height only for the respective point.

Effect with cycles

SL cycles and Cycle 12

The control interprets the points in the point table as an additional datum shift.

Cycles 200 to 208, 262 to 267

The control interprets the points of the working plane as coordinates of the hole centers. If you want to use the coordinate defined in the point table as the starting point coordinate in the tool axis, you must define the coordinate of the workpiece upper edge (Q203) as 0.

Cycles 210 to 215

The control interprets the points as an additional datum shift. If you want to use the points defined in the point table as the starting point coordinates, you must program the starting points and the coordinate of the workpiece upper edge (Q203) in the respective milling cycle as 0.

 
Tip

You can no longer insert these cycles on the control, but you can edit and run them in existing NC programs.

Cycles 251 to 254

The control interprets the points on the working plane as coordinates of the cycle starting point. If you want to use the coordinate defined in the point table as the starting point coordinate in the tool axis, you must define the coordinate of the workpiece upper edge (Q203) as 0.

Selecting the point table in the NC program with SEL PATTERN

To select the point table:

    1. Select Insert NC function
    2. The control opens the Insert NC function window.

    1. Select SEL PATTERN

    1. Select File selection
    2. The control opens a window for the file selection.

    1. Select the desired point table through the file structure
    2. Confirm your input
    3. The control concludes the NC block.

    If the point table is not stored in the same directory as the NC program, you must define the complete path name. In the Program settings window you can define whether the control creates absolute or relative paths.

    Settings in the Program workspace

    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

    7 SEL PATTERN “TNC:­\nc_prog­\Positions.PNT

    Calling the cycle with a point table

    If you want to call a cycle at the points that you defined in the point table, then program the cycle call with CYCLE CALL PAT.

    CYCL CALL PAT enables the control to execute the point table that you defined last.

    To call a cycle in conjunction with a point table:

      1. Select Insert NC function
      2. The control opens the Insert NC function window.

      1. Select CYCL CALL PAT
      2. Enter a feed rate
      3.  
        Tip

        The control will use this feed rate to traverse between the points of the point table. If you do not enter a feed rate, the control moves the tool at the feed rate last defined.

      4. Define miscellaneous functions, if necessary
      5. Confirm your input with the END key

      Notes

      • In the GLOBAL DEF 125 function you can use the setting Q435=1 to force the control to always move to the 2nd set-up clearance from the cycle during the positioning between the points.
      • If you want to move at reduced feed rate when pre-positioning in the tool axis, program the M103 miscellaneous function.
      • With CYCL CALL PAT the control runs the point table that you last defined, even if you defined the point table with an NC program that was nested with CALL PGM.