Creating a Drilling Deep Hole Operation with the Legacy Interface

From the Axial Machining section of the action bar, select Drilling Deep Hole then a position in the manufacturing program.
- The Drilling Deep Hole operation appears under the manufacturing program. The Drilling Deep Hole 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.
In the Geometry tab, do the following:
1. Select the red hole depth representation then select the hole features.
  For more information, see Selecting Geometry.
  
  The sensitive icon is updated with information such as the number of machining points, the depth, and diameter of the first selected hole.
2. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
3. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
In the Strategy tab , specify parameters such as the following ones:
- 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
- Maximum depth of cut (Dc) and Retract offset (Or)
- Decrement rate and Decrement limit.
- Dwell mode (None, By revolutions, By time units).
- DeepHole LeadIn: Specify the split-tool path distance when entering into material after passing through an already drilled hole.
- DeepHole LeadOut: Specify the split-tool path distance before entering into an already drilled hole.
- NoRetract motion: If a drilling tool path involves progressive drilling passes within an already machined hole, then these passes will be removed as there is no material to remove.
- Compensation parameters depending on those available on the tool.
The other parameters are optional in this case.
In the Tool tab , choose a tool.
Drill, spot drill, center drill, multidiameter drill, and end mill tools are supported. For more information, see Assigning a Tool Element to a Machining Operation.
In the Feeds and Speeds tab , specify the feedrates and spindle speeds.
In the Feedrate tab, specify the DeepHole Feed Reduction parameter.
This option reduces the feed rate by the specified value for the pass within an already drilled hole.
In the Macros tab, specify the required transition paths.
For more information, see Defining and Editing Macros.
Click Display or Simulate to check the validity of the operation.
For more information, 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 Drilling Deep Hole operations:
```
CYCLE/DEEPHL, %MFG_TOTAL_DEPTH, INCR, %MFG_AXIAL_DEPTH, 
%MFG_FEED_MACH_VALUE, &MFG_FEED_UNIT,
%MFG_CLEAR_TIP, DWELL, %MFG_DWELL_REVOL
```
A typical NC data output is as follows:
```
CYCLE/DEEPHL, 25.000000, INCR, 5.000000, 500.000000, MMPM,
5.000000, DWELL, 3
```
For more information, see NC_DEEPHOLE.
Click Edit Cycle to edit or choose output syntaxes.

Notes:

Holes must be created as machining axial features.
Reducing the feed rate is only available when all drilling operations are designed with MAFs.
To compute the tool path of a deep hole drilling operation, you must force the tool path computation of the manufacturing program and generate the APT source output.
To generate a correct APT output for DeepHole LeadIn and DeepHole LeadOut, clear the Output CYCLE syntax check box. For more information, see 2.5 to 5-Axis Drilling Operations Dialog Box.
Machining Operation dependency is only supported when intermediate stock is used.