Tool-oriented machining

Application

Tool-oriented machining allows you to machine several workpieces together even on a machine without pallet changer, which reduces tool-change times. You can thus use the pallet management feature even on machines without a pallet changer.

Requirements

Description of function

The following columns of the pallet table apply to tool-oriented machining:

  • W-STATUS
  • METHOD
  • CTID
  • SP-X to SP-W
  • You can enter safety positions for the axes. The control only approaches these positions if the machine manufacturer processes them in the NC macros.

Pallet table *.p

In the Job list workspace, you can activate or deactivate tool-oriented machining for each NC program via the context menu. This will also cause the control to update the METHOD column.

Context menu

Sequence of tool-oriented machining

  1. The entries TO and CTO tell the control that tool-oriented machining is in effect for these rows of the pallet table
  2. The control executes the NC program with the entry TO up to the TOOL CALL
  3. The W-STATUS changes from BLANK to INCOMPLETE and the control enters a value into the CTID field
  4. The control executes all other NC programs with the entry CTO up to the TOOL CALL
  5. The control uses the next tool for the following machining steps if one of the following situations applies:
    • The next table row contains the entry PAL
    • The next table rowcontains the entry TO or WPO
    • There are rows in the table that do not yet contain the entry ENDED or EMPTY
  6. The control updates the entry in the CTID field with each machining operation
  7. If all table rows of the group contain the entry ENDED, the control processes the next rows of the pallet table

Mid-program startup with block scan

You can also return to a pallet table after an interruption. The control can show the rows and the NC block at which the interruption occurred.

The control saves the mid-program startup information in the CTID column of the pallet table.

If you use the block scan to start in a pallet table, the control will always execute the chosen row in the pallet table as a workpiece-oriented process.

After a block scan, the control can resume tool-oriented machining if the tool-oriented machining method TO and CTO is defined in the subsequent rows.

Pallet table *.p

 
Machine

Refer to your machine manual.

Tool-oriented machining is a machine-dependent function. The standard functional range is described below.

Tool-oriented machining allows you to machine several workpieces together even on a machine without pallet changer, which reduces tool-change times.

 
Notice
Danger of collision!
Not all pallet tables and NC programs are suitable for tool-oriented machining. With tool-oriented machining, the control no longer executes the NC programs continuously, but divides them at the tool calls. The division of the NC programs allows functions that were not reset to be in effect across programs (machine states). This leads to a danger of collision during machining!
  1. Consider the stated limitations
  2. Adapt pallet tables and NC programs to the tool-oriented machining
    • Reprogram the program information after each tool in every NC program (e.g., M3 or M4).
    • Reset special functions and miscellaneous functions before each tool in every NC program (e.g. Tilt working plane or M138)
  3. Carefully test the NC program or program section in the Single Block mode

The following functions are not permitted:

  • FUNCTION TCPM, M128
  • M144
  • M101
  • M118
  • Changing the pallet preset

The following functions require special attention, particularly for mid-program startup:

  • Changing the machine statuses with a miscellaneous function (e.g. M13)
  • Writing to the configuration (e.g. WRITE KINEMATICS)
  • Traverse range switchover
  • Cycle 32
  • Tilting the working plane

Unless the machine manufacturer has made a different configuration, you need the following additional columns for tool-oriented machining:

Column

Meaning

W-STATUS

The machining status defines the machining progress. Enter BLANK for an unmachined (raw) workpiece. The control changes this entry automatically during machining.

The control differentiates between the following entries

  • BLANK / no entry: Workpiece blank, requires machining
  • INCOMPLETE: Partly machined, requires further machining
  • ENDED: Machined completely, no further machining required
  • EMPTY: Empty space, no machining required
  • SKIP: Skip machining

METHOD

Indicates the machining method

Tool-oriented machining is also possible with a combination of pallet fixtures, but not for multiple pallets.

The control differentiates between the following entries

  • WPO: Workpiece oriented (standard)
  • TO: Tool oriented (first workpiece)
  • CTO: Tool oriented (further workpieces)

CTID

The control automatically generates the ID number for mid-program startup with block scan.

If you delete or change the entry, mid-program startup is no longer possible.

SP-X, SP-Y, SP-Z, SP-A, SP-B, SP-C, SP-U, SP-V, SP-W

The entry for the clearance height in the existing axes is optional.

You can enter safety positions for the axes. The control only approaches these positions if the machine manufacturer processes them in the NC macros.

Notes

 
Notice
Danger of collision!
Not all pallet tables and NC programs are suitable for tool-oriented machining. With tool-oriented machining, the control no longer executes the NC programs continuously, but divides them at the tool calls. The division of the NC programs allows functions that were not reset to be in effect across programs (machine states). This leads to a danger of collision during machining!
  1. Consider the stated limitations
  2. Adapt pallet tables and NC programs to the tool-oriented machining
    • Reprogram the program information after each tool in every NC program (e.g., M3 or M4).
    • Reset special functions and miscellaneous functions before each tool in every NC program (e.g. Tilt working plane or M138)
  3. Carefully test the NC program or program section in the Single Block mode
  • If you want to start machining again, change the W-STATUS to BLANK or remove the previous input.

Notes on mid-program startup

  • The entry in the CTID field remains there for two weeks. After this time, mid-program startup is no longer possible.
  • Do not change or delete the entry in the CTID field.
  • The data from the CTID field become invalid after a software update.
  • The control saves the preset numbers for mid-program startup. If you change this preset, machining is shifted, too.
  • Mid-program startup is no longer possible after editing an NC program within tool-oriented machining.