General tab

Parameter	Explanation
Description	A textual description of the tool. This description is included in the tool name shown throughout CAM.
Vendor	The manufacturer or vendor of the tool. Use this to identify the source for purchasing this specific tool.
Product id	The vendor's identifier (ID) for the tool. This can be the catalog, model, or part number of this tool.
Product Link	The vendor's website or contact information to acquire this tool. This link will appear in the Info tab on the tool library. Selecting this link will take you to the suppliers external website.

Cutter tab

Parameter	Explanation
Type	Use this to change the form of the selected tool type, for example, ball, flat, bullnose, tapered, and so on.
Unit	The tool unit of measurement (Millimeters or Inches)
Clockwise spindle rotation	Enable for right handed tools and a Clockwise (CW) spindle rotation. Disable for left handed tools and a Counter Clockwise (CCW) spindle rotation.
Number of flutes	The number of cutting edges on the tool. Some tools refer to them as "teeth".
Material	Select the material of the tool. Options include - Unspecified, HSS, Ti Coated, Carbide or Ceramic.

Geometry group

Parameter	Explanation
Diameter	The cutting diameter of the tool
Shaft diameter	The diameter of the tools clamping surface. Also called the shaft or arbor.
Overall length	The length of the entire tool.
Length below holder	The length of the tool that protrudes from the holder.
Shoulder length	The length above of the cutting edge of the tool.
Flute length	The length of the cutting edge of the tool.
Corner radius	The radius on the corner of the cutter.
Tip angle	The angle of the tool tip. Used to calculate Chamfers, Spot drill depths and Drill through distances.
Tip diameter	The diameter at the tip of the cutter. Used for Engrave/Chamfer tools.
Tip length	The length of the tip. Used for Center Drills.
Taper angle	The total Included angle of the cutting tip ÷ 2.
Included angle	The total angle of the tip. Equal to the Taper angle x 2.
Thread pitch	The distance between teeth for a tap or thread mill. Inch= 1/Threads per Inch. MM = actual pitch.
Number of teeth	The number of teeth for a thread mill.
Thread profile angle	The angle of the thread tooth. Typically 60° for standard threads.

Shaft

A shaft is an extension that fits between the Tool and the Holder. Click or to add or remove a segment. Selecting a segment and pressing + inserts a copy of the current segment below your current location.

Parameter	Explanation
Height	The height of the selected tool shaft segment.
Upper diameter	The upper diameter of the selected tool shaft segment.
Lower diameter	The lower diameter of the selected tool shaft segment.

Holder

Holders are not required, but they do provide a visual reference and can be used for collision detection. The available tool holders are shown in the left side column. Use the Search function to limit the display. | Parameter | Explanation | | ----------------- | --------------------- | | Holder description | A textual description of the tool holder.| | Holder product ID | The vendor's identifier (ID) for the tool holder. | | Holder product link | Web site product information link.| | Holder vendor | The vendor of the tool holder.| | Select Holder | Applies the currently selected holder to the current tool. | | Remove Holder | Removes the currently active holder from the current tool.|

Cutting data

Speed group

Set default Spindle Speeds for the tool.

Parameter	Explanation
Spindle speed	The rotational speed of the spindle given in Rotations Per/Min (RPM).
Surface speed	The spindle speed expressed as the speed of the tool on the surface, or Surface Speed/Min. It is Ft/Min for Inch tool and Meter/Min for Metric tools.
Ramp spindle speed	The rotational speed of the spindle when performing ramp movements (RPM).

Feedrates group

Set default feedrates for the tool.

Parameter	Explanation
Cutting feedrate	Feed used in cutting moves.
Feed per tooth	The amount of material to advance for each flute of the cutter.
Lead-in feedrate	Feed used when leading in to a cutting move.
Lead-out feedrate	Feed used when leading out from a cutting move.
Ramp feedrate	Feed used when doing helical ramps into stock.

Vertical feedrates group

Parameter	Explanation
Plunge feedrate	Feed used when plunging into stock.
Feed per revolution	The plunge feedrate expressed as the feed per revolution.

Passes and linking group

Parameter	Explanation
Use stepdown	Select the box and in the Stepdown field, enter the desired cut distance.
Use stepover	Select the box and in the Stepover field, enter the desired cut distance.
Coolant	Select the type of coolant to use with the tool. Not all options will be available for all NC machines.

Post processor

Set the tool number and other conditions triggered by the post processor.

Parameter	Explanation
Number	The number used to identify the tool in the NC program.
Length offset	The number used to identify the tool length offset in the NC program.
Diameter offset	The number used to identify the Cutter Radius Compensation offset in the NC program.
Turret	Specifies the turret position of the tool on the NC machine.
Comment	A text comment for the tool. The comment is typically output to the NC program.
Manual tool change	Enables you to force a manual tool change. Disable for machines with an automatic tool changer.
Live Tool	Specifies that the tool spins. Important if this milling/drilling tool will be used on a lathe with live tooling.
Break control	Enables you to check for tool breakage after use. This sends an output to the post that tells the machine to check for a broken tool. This is a machine-dependent function.