Creating a Boring and Chamfering Operation with Legacy Interface

From the Axial Machining section, select Boring and Chamfering

then a position in the Manufacturing Program.

A Boring and Chamfering entity is added to the Manufacturing Program.
The Boring and Chamfering 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.

Still in the Geometry tab:

Select the red hole depth representation then select hole geometry.
See Selecting Geometry

The sensitive icon is updated with information such as the number of selected holes, the depth and diameter of the first selected hole, ...
Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
Optional: Select the check boxes below the sensitive icon to modify the corresponding data.

Select the Strategy tab

and specify the following parameters:

Approach clearance (A) and Approach clearance 2 (A2)
Depth mode (By tip (Dt) or By shoulder (Ds))
Note: The depth value used is the one specified in the Geometry tab.
Breakthrough (B)
Plunge mode (None, By tip, By diameter)
Note: If a Plunge mode is selected (By Tip or By Diameter), deselect the Plunge for chamfering check box to deactivate the plunge motion for the chamfering phase of the operation, if needed. In this case, the plunge motion is done for the boring phase only.
Dwell mode (None, By revolutions, By time units) and the corresponding values.
First compensation for top chamfering
Second compensation for bottom chamfering.

Note: In the tool path represented in the Strategy tab, tool motion is as follows.

Select the Tool tab

and choose a tool.

Boring and chamfering, multi diameter drill tools are supported.

See Assigning a Tool Element to a Machining Operation.

Select the Feeds and Speeds tab

and specify the feedrates and spindle speeds for the operation.

You can specify a machining feedrate for the boring phase of the operation and a chamfering feedrate for the chamfering phase. Similarly, you can specify a machining spindle speed for the boring phase and a smaller spindle speed for the chamfering phase.

Example for 3 machining points:

Boring phase:
- Motion at machining feedrate from 1 up to the position where hole is to be bored
- Possibly, activation of second tool compensation number
- Rapid feedrate up to a clearance position before start of chamfering.
Chamfering phase:
- Motion at chamfering feedrate from clearance position to 2
- Dwell for specified duration
- Possibly, activation of first tool compensation number
- Retract at retract feedrate from 2 to 3.

Select the Macro tab

and add approach and retract motions to the operation.

See Defining and Editing Macros

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.

Click OK to create the operation.

Note: If your PP table is configured with the following statement for Boring and Chamfering operations:

CYCLE/BORE, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
%MFG_CHAMFERFEED_VALUE, &MFG_FEED_UNIT,%MFG_SPINDLE_MACH_VALUE,
%MFG_SPINDLE_LOW_VALUE, &MFG_SPNDL_UNIT, %MFG_CLEAR_TIP,
DWELL,%MFG_DWELL_REVOL

A typical NC data output is as follows:

CYCLE/BORE, 25.000000, 500.000000, 150.000000, MMPM,
70.000000, 40.000000, RPM, 5.000000, DWELL, 3

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

Click Edit Cycle

to edit or choose output syntaxes.