Creating a Spot Drilling Operation

You can create a Spot Drilling operation.

This task shows you how to:

Before you begin: Create a machining pattern as explained in Defining Machining Patterns.

Creating a Spot Drilling Operation

  1. From the Axial Machining section of the action bar, select Spot Drilling , then select a position in the manufacturing program.

    The Spot Drilling workflow appears in the work area.

  2. In the Tool Search dialog box that appears:
    1. Select the tool type.
    2. Select the required tool or tool assembly and click one of the following:
    OptionDescription
    Select in Session Select an existing tool or tool assembly from the Resource Configuration View.
    Search in Database Select a tool or a tool assembly from the database.
    Look Into Catalog Browse for a tool or a tool assembly in the catalog.
  3. Optional: Close the Tool Search dialog box by pressing Esc. Then, click Search Tool to research a tool in the database.
  4. Follow the workflow instructions to select hole positions, or select an existing manufacturing pattern from the Manufacturing View.
  5. Double-click anywhere in the work area.

    A Spot Drilling entity is added to the Manufacturing Program.

    The Spot Drilling dialog box appears directly in the Geometry tab .

  6. Click in the title bar of the dialog box to edit the name of the manufacturing pattern, such as SpotDrilling.x.
  7. Optional: Click New Feature to apply a machining area feature.

    Note: You can export a feature by clicking Export Feature .

  8. In the Mandatory section, verify the mandatory input parameters.

    Note: The following icons are used to describe the status of a parameter:
    Icon Description
    Parameter defined.
    Mandatory parameter not defined.
    Optional parameter not defined.
    Parameter not up to date.
    Broken link.

  9. Optional: Do any of the following:
    1. Click to remove the input parameter.
    2. Click to display additional information on the parameter in the work area.
    3. Click to display the parameter's context menu.
  10. In the Optional section, verify the optional input parameters.
  11. In the Parameters section, verify additional parameter inputs.
  12. Verify the parameters in the following tabs:

    • Tool: Select a tool.
    • Strategy: Select a Tool path style.
    • Feeds and Speeds: Specify the feedrates and spindle speed.
    • Macros: Specify transition paths.

  13. Click Edit Cycle to edit or choose output syntaxes.
  14. Click Compute to compute the tool path with the specified parameters.
  15. Click OK to validate and exit the dialog box.
  16. Click Cancel to exit the dialog box without saving.

The spot drilling operation is created as SpotDrilling.x. It is visible in the Activities Process Tree.

Creating a Spot Drilling Operation with the Legacy Interface

  1. From the Axial Machining section, select Spot Drilling then a position in the Manufacturing Program.
    • A Spot Drilling entity is added to the Manufacturing Program.
    • The Spot Drilling dialog box opens directly at the Geometry tab . This tab includes a sensitive icon to help you specify the geometry.
    • Areas colored red, texts such as No point and No geometrical feature has been selected indicated that geometry is required.
  2. Still in the Geometry tab.
    1. Select red hole depth representation, then select the points to be spot drilled.

      See Selecting Geometry for more information.

      Tip: Select the circular edges of holes: The circle centers are taken as the points to be spot drilled.



  3. Optional: According to your needs:
    1. Click the tool axis to invert the tool axis direction
    2. Double-click Jump distance in the sensitive icon then specify a clearance value in the Edit Parameter dialog box that appears.
    3. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
  4. Select the Strategy tab to specify the following parameters:
    • Approach clearance (A)
    • Depth mode (By tip (Dt) or By shoulder (Ds))
      Note: The depth value used is the one specified in the Geometry tab.
    • Plunge mode (None, By tip, By diameter)
    • Dwell mode (None, By revolutions, By time units).
    • Compensation parameters depending on those available on the tool.
    • Activation of the Automatic ROTABL and Output CYCLE syntax.

    The other parameters are optional in this case.

  5. Select the Tool tab and choose a tool.

    Drill, spot drill, center drill, multi diameter drill, conical mill tools are supported. 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.

    Exemple for 3 machining points:

    • Machining feedrate from 1 to 2
    • Dwell for the specified duration
    • Retract feedrate from 2 to 3.

  7. Select the Macros tab to specify the desired transition paths.

    See Defining and Editing Macros

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

    See Simulating the Tool Path.

    • The tool path is computed.
    • A progress indicator is displayed.
    • 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 Spot Drilling operation: 
    CYCLE/SPDRL, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
&MFG_FEED_UNIT, %MFG_CLEAR_TIP, DWELL, %MFG_DWELL_REVOL

    A typical NC data output is as follows: 

    CYCLE/SPDRL, 25.000000, 500.000000, MMPM, 5.000000, DWELL,
3

    The parameters available for PP word syntaxes for this type of operation are described in the NC_SPOT_DRILLING section of the NC Machining Apps Common Services User's Guide.

  10. Click Edit Cycle to edit or choose output syntaxes.