Datum shift with TRANS DATUM

Application

The TRANS DATUM function allows you to shift the workpiece datum by either entering fixed or variable coordinates or by specifying a table row in the datum table.

Use the TRANS DATUM RESET function to reset the datum shift.

Description of function

TRANS DATUM AXIS

You can define a datum shift by entering values in the respective axis with the TRANS DATUM AXIS function. You can define up to nine coordinates in one NC block, and incremental entries are possible.

The control displays the result of the datum shift in the Positions workspace.

The Positions workspace

TRANS DATUM TABLE

You can use the TRANS DATUM TABLE function to define a datum shift by selecting a row from a datum table.

Optionally, you can set the path to a datum table. If you do not define a path, the control will use the datum table that has been activated with SEL TABLE.

Activating a datum table in the NC program

The control displays the datum shift and the path to the datum table on the TRANS tab of the Status workspace.

The TRANS tab

TRANS DATUM RESET

Use the TRANS DATUM RESET function to cancel a datum shift. How you previously defined the datum is irrelevant.

Input

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.

11 TRANS DATUM AXIS X+10 Y+25 Z+42

; Shift the workpiece datum in the X, Y and Z axes

To navigate to this function:

Insert NC function All functions Special functions Functions Coordinate transformations TRANS TRANS DATUM

The NC function includes the following syntax elements:

Syntax element

Meaning

TRANS DATUM

Syntax initiator for a datum shift

AXIS, TABLE or RESET

Datum shift with coordinate input, with a datum table or reset of the datum shift

X, Y, Z, A, B, C, U, V or W

Possible axes for coordinate input

Fixed or variable number

Only if AXIS has been selected

TABLINE

Row in the datum table

Fixed or variable number

Only if TABLE has been selected

Name or Parameter

Path to the datum table

Fixed or variable path

Selection by means of a selection window

Optional syntax element

Only if TABLE has been selected

Notes

  • The TRANS DATUM function replaces Cycle 7 DATUM SHIFT. If you import an NC program from an older control, then, during editing, the control turns Cycle 7 into the TRANS DATUM NC function.
  • If you execute an absolute datum shift with TRANS DATUM or Cycle 7 DATUM SHIFT, then the control overwrites the values of the current datum shift. The control adds the incremental values to the values of the current datum shift.
  • Absolute values reference the workpiece preset. Incremental values reference the workpiece datum.
  • Presets in the machine

  • A datum shift in the axes A, B, C, U, V and W is effective as an offset. HEIDENHAIN recommends inclining rotary axes using the PLANE functions or a 3D basic rotation.
  • Comparison of offset and 3D basic rotation

  • In machine parameter transDatumCoordSys (no. 127501), the machine manufacturer defines the reference system referred to by the values in the position display.
  • Reference systems