Creating a Circular Milling Operation

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

The Circular Milling 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 Circular Milling entity is added to the Manufacturing Program.

The Circular Milling 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 CircularMilling.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.
- 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 circular milling operation is created as CircularMilling.x. It is visible in the Activities Process Tree.

Creating a Circular Milling Operation with the Legacy Interface

From the Axial Machining section, select Circular Milling then a position in the Manufacturing Program.
- A Circular Milling entity is added to the Manufacturing Program.
- The Circular Milling 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 the red hole depth representation then select the hole feature.
  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 hole extension type, ...
2. Optional: Double-click Offset on Bottom and enter a value.
3. Optional: Double-click Offset on Contour and enter a value.
4. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
5. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
Select the Strategy tab and select a Machining mode (Standard or Helical).
Still in the Strategy tab , specify the machining strategy and stepover parameters.

The following are common to both machining modes:
- Approach clearance (A)
- Plunge mode
- Machining tolerance
- Direction of cut
- Percentage overlap
- Compensation number depending on those available on the tool
- Compensation app mode (Output point or Guiding point)
- Compensation output to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output.
When Machining mode is set to Standard, the Stepover parameters are:
- Breakthrough (B)
- Distance between paths (Dp) and Number of paths (Np)
- Axial mode (Maximum depth of cut or Number of levels (with or without top))
- Sequencing mode ( Axial first or Radial first)
- Automatic draft angle.
- Spring pass
When Machining mode is set to Helical, the Stepover parameters are:
- Breakthrough (B)
- Distance between paths (Dp) and Number of paths (Np)
- Helix mode (By angle or By pitch)
- Angle (Ang) or Pitch (P) value.
- Spring pass
  Warning: In Helical mode with 2 radial paths, the Spring pass should be computed only on the end full circle, not on the entire helix.
Select the Tool tab and choose a tool.
End mill, T-Slotter, conical mill, spot drill, countersink, drill and face mill tools are supported.
See Assigning a Tool Element to a Machining Operation.
Select the Feeds and Speeds tab to specify the feedrates and spindle speeds for the operation.
Example for 5 machining points:
- Motion at machining feedrate from 1 to 2
- Motion at feedrates defined on macros from 2 to 3, 3 to 4, 4 to 2, 2 to 3 and 3 to 4
- Retract at retract feedrate from 4 to 5.
Select the Macro tab to add approach and retract motions to the operation.
See Defining and Editing Macros
1. When Machining mode is set to Standard, select Predefined-Helix to insert a helix approach macro.
  The Predefined-Helix mode is available for approach macro and the return between levels approach macro in Standard machining mode.
  
  The representation of the macro changes accordingly.
2. In this representation, double-click the figure representing the helix radius to edit its value.
3. Double-click Macro Ramping Angle to edit its value.
4. Click the toggle Absolute Helix Radius/ Radius difference vs next path to select the required status, or double-click it to edit the status and the values in the dialog box that appears.
5. Right-click an arc of helix representation to define the Feedrate type from the context menu.
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 Circular Milling operations:
```
CYCLE/CIRCULARMILLING, %MFG_TOTAL_DEPTH,
%MFG_FEED_MACH_VALUE,&MFG_FEED_UNIT, %MFG_CLEAR_TIP
```
A typical NC data output is as follows:
```
CYCLE/CIRCULARMILLING, 38.500000, 500.000000, MMPM, 2.500000
```
The parameters available for PP word syntaxes for this type of operation are described in the NC_CIRCULAR_MILLING section of the NC Machining Apps Common Services User's Guide.
Click Edit Cycle to edit or choose output syntaxes.