Use the Edit Cutting Data dialog to enter and edit the cutting data displayed on the Cutting Data tab. Adding cutting data is useful if want to reuse the tool in the future.
To display the Edit Cutting Data dialog, click 
on the Cutting Data tab of the Tool dialog.
The dialog contains the following:
Toolpath Type — Displays the type of toolpath that is cut with the tool. You can specify the toolpath type by using the Toolpath Properties options on the Feeds and Speeds dialog.
Operation — Displays the cutting mode of the tool. You can specify the toolpath type by using the Toolpath Properties options on the Feeds and Speeds dialog.
Tool Properties — This summarises information that is specified on the Tip and Cutting Data tabs.
Tool ID — This is specified on the Cutting Datatab of the Tool dialog.
Diameter — This is specified on the Tip tab of the Tool dialog.
Tool Family — This is specified on the Cutting Data tab of the Tool dialog.
Number of Flutes — This is specified on the Tip tab of the Tool dialog.
Tool/Material Properties
Axial Depth of Cut — Enter the depth of cut measured along the tool axis.
- The symbol ap represents this value in calculations.
- The flute length of a solid cutter or the inserts fitted limit the maximum value.
- Typically, use this value to determine the maximum Stepdown for area clearance and constant Z machining.
Radial Depth of Cut — Enter the depth of cut measured normal to the tool axis.
- The symbol ae represents this value in calculations.
- Typically, this value determines the Stepover for machining.
Surface Speed — Enter the speed of the tool during material removal.
- In calculations, this value is represented by the symbol vc.
- The surface speed represents the rate at which the cutting edges of the tool can be driven through the material.
- Any changes made to the Surface Speed value recalculates the Spindle Speed, Cutting Feed Rate, and Plunging Feed Rate.
Feed/Tooth — Enter the cutting feed per tooth.
- In calculations, this value is represented by the symbol fz.
- The feed per tooth is determined by the construction of the tool, and may be limited by the strength of the cutting edges or the capacity of the tool to remove swarf.
- Any changes made to the Feed/Tooth value recalculates the Cutting Feed Rate and Plunging Feed Rate.
Load Cutting Data From Active Toolpath — Click to load the Surface Speed and Feed/Tooth from the active toolpath (these values are specified on the Feeds and Speeds dialog).
Edit Feed/Tooth and Depth of Cut in TDU — Select to display the Feed/Tooth and the depth of cut values in tool diameter units rather than actual values.
Tool Diameter Units is the distance relative to the tool diameter. So with a 10 mm tool and a TDU of 0.5, this gives an actual value of 5 mm.
Cutting Conditions
Spindle Speed — Enter the rotation of the spindle, measured in revolutions per minute. If you edit this value then the Surface Speed value automatically updates to reflect your change.
The Spindle Speed is Surface Speed x 1000/3.14 x Tool diameter or, as a formula: n = Vc.1000/(
.Dc). Editing either the Spindle Speed or Surface Speed automatically updates the other.
Cutting Feed Rate — Enter the cutting feed rate.
The Cutting Feed Rate is Number of teeth x Feed per tooth x Spindle Speed or, as a formula: Vf = Zn.fz.n. Editing either the Cutting Feed Rate or the Feed/Tooth automatically updates the other.