Creating a Boring Operation

You can create a Boring operation.

This task shows you how to:

Creating a Boring Operation
Creating a Boring Operation with the Legacy Interface

Creating a Boring Operation

You can create a Boring, Boring Spindle Stop, or Back Boring operation

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

The Boring workflow appears in the work area.

In the Tool Search dialog box that appears:

Select the tool type.
Select the required tool or tool assembly and click one of the following:

Option	Description
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.

Optional: Close the Tool Search dialog box by pressing Esc. Then, click Search Tool to research a tool in the database.
Follow the workflow instructions to select hole positions, or select an existing manufacturing pattern from the Manufacturing View.
Double-click anywhere in the work area.

A Boring entity is added to the Manufacturing Program.

The Boring dialog box appears directly in the Geometry tab .
Click in the title bar of the dialog box to edit the name of the manufacturing pattern, such as Boring.x.
Optional: Click New Feature to apply a machining area feature.

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

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.

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.
In the Optional section, verify the optional input parameters.
In the Parameters section, verify additional parameter inputs.
Verify the parameters in the following tabs:
- Tool: Select a tool.
- Strategy: Select a Tool path style and Boring Mode: Boring, Boring Spindle Stop, or Back Boring.
- Feeds and Speeds: Specify the feedrates and spindle speed.
- Macros: Specify transition paths.
Click Edit Cycle to edit or choose output syntaxes.
Click Compute to compute the tool path with the specified parameters.
Click OK to validate and exit the dialog box.
Click Cancel to exit the dialog box without saving.

The boring operation is created as Boring.x. It is visible in the Activities Process Tree.

Creating a Boring Operation with the Legacy Interface

You can create a Boring operation.

From the Axial Machining section, select Boring then a position in the Manufacturing Program.
- A Boring entity is added to the Manufacturing Program.
- The Boring 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:
1. Select a machining pattern of 10 holes from the list.
  The sensitive icon is updated with information such as the depth and diameter of the first selected feature, the hole extension type, the number of machining points, ...
2. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction, if required.
3. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
Select theStrategy tab to specify the following machining 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.
- Breakthrough (B) distance
- Dwell mode (None, By revolutions, By time units).
- Compensation parameters depending on those available on the tool.
The other parameters are optional in this case.
Select the Tool tab and choose a tool.
Boring and chamfering, boring bar and end mill tools are supported.
See Assigning a Tool Element to a Machining Operation.
Notes:
For boring bar tools:
- You cannot set the nominal diameter to less than the minimum diameter or more than the maximum diameter. The nominal diameter value truncates to the minimum or maximum value depending on the value you entered.
- The lowest point of the tool is taken into account while calculating the tool path.
- The distance ld representing the material below the cutting point of the tool, is taken into account while calculating the tool path.
Select the Feeds and Speeds tab and specify the feedrates and spindle speeds for the operation.
Example for 3 machining points:
- Motion at machining feedrate from 1 to 2
- Dwell for specified duration
- 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.

Note: Boring bars are not supported during material removal simulation.

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 operations:
```
CYCLE/BORE, %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/BORE, 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_BORING section of the NC Machining Apps Common Services User's Guide.
Click Edit Cycle to edit or choose output syntaxes.