Creating a Sequential Axial Operation with the Legacy Interface

You can create a Sequential Axial operation.

See Also
Sequential Axial and Sequential Groove Operations
  1. From the Axial Machining section, select Sequential Axial then a position in the Manufacturing Program.

    A typical part to machine with Sequential Axial looks like this:

    • A Sequential Axial entity is added to the Manufacturing Program.
    • The Sequential Axial dialog box opens directly at the Geometry tab . This tab includes a sensitive icon to help you specify the geometry.
    • Areas colored red, or texts such as No point and No geometrical feature has been selected, indicated that geometry is required.
  2. Still in the Geometry tab, which comprises a Global and a Local tab:
    1. In the Global tab, select the red hole depth representation then select the three holes.

      See Selecting Geometry for more information.



      The sensitive icon is updated with information such as:

      • The number of machining points.
      • The depth and diameter of the first selected hole.
      • The counterbore depth.
      • The angle.

    2. In the Local tab, select the plane representations in the sensitive icon, and the required planes in the part.


    3. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
    4. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
  3. Select the Strategy tab to specify the following parameters.
    • Power
    • Approach clearance (A)
    • Compensation parameters, such as First Compensation and Compensation Application Mode. These depend on those available on the tool.
    • Automatic ROTABL
    • Output CYCLE syntax
  4. Select the Motions tab in the Strategy tab and define the required motions.
    1. Click the icon corresponding to the required motion.
    2. From the lists, select or enter the values.
    3. Click OK to add the motion.

    For example:

    Motion Icon Syntax Parameter
    1st Spindle Speed SPINDL/ 60,000,RPM,CLLW

    Spindle Mode = Local Spindle (60tr/mn)

    Way of Rotation=CCLW
    2nd Go to Plane -

    Plane number=1

    Feedrate Mode = Local Feedrate (50mm_mn)
    3rd PP Word COOLNT/CENTER,70
    4th Delay DELAY/ 3.000000

    Spindle Dwell Time=By Time

    Spindle Dwell Time (3s)
    5th Go to Plane -

    Plane number=3

    Feedrate Mode = Machining
    6th Go to Clearance -

    Feedrate Mode = Local Feedrate (50 mm_mn

    The motions are added and listed in the dialog box.
  5. Select the Tool tab and choose a tool.

    Note: The following mill tools available:
    • Drill
    • Multidiameter drill
    • Spot drill
    • Center drill
    • Countersink
    • Two sides chamfering
    • Boring and chamfering
    • Boring bar
    • Reamer
    • T-slotter
    • end mill
    • Face mill
    • Thread mill
    • Conical mill
    • Counterbore

    See Assigning a Tool Element to a Machining Operation.

  6. Select the Feeds and Speeds tab to specify the feedrates and spindle speeds for the operation.
  7. Select the Macros tab to specify the required transition paths.

    See Defining and Editing Macros

  8. Click Display or Simulate to verify the validity of the operation.

    See Simulating the Tool Path.

    • The progress indicator appears.
    • You can cancel the tool path computation at any moment before 100% completion.
  9. Click OK to create the operation.
    Note: If your PP table is configured with the following statement for Sequential Axial operations: 
    CYCLE/SEQAXIAL, %MFG_TOTAL_DEPTH, %MFG_CLEAR_TIP

    A typical NC data output is as follows: 

    CYCLE/SEQAXIAL, 40.00000, 3.0000

    For more information on the parameters available for PP word syntaxes for this type of operation, see NC_SEQAXIAL.