Parameters: Threading Tools
Use this tab to set default threading parameters for the tool. When you select this tool while creating a toolpath, many of the values that you enter here will automatically transfer to the parameters for the new toolpath. Use the Machine Group Properties to enable or disable this feature. Any time you create a toolpath, you can override the values in this tab.
Tool number
Lathe turning system tools are stored in a turret. Each position in the turret is described as a station. When a tool is placed in a turret station, it is given a one- or two-digit identifying number. The tool number identifies in which turret station the tool is placed.
Tool offset number
This number corresponds to a value that the programmer uses to define the offset value from the center of the turret to the programmed point on the tool.
Tool station number
Auxiliary number used to define the turret face into which the tool is loaded. If you select Station Number Equals Tool Number in Machine Group Properties, this number defaults to the default tool number. If you deselect this option, the number defaults to -1.
Tool back offset number
This option is unavailable for threading tools.
Feed rate
You can choose to use this value as the default feed rate whenever the tool is selected for an operation as set in the Tool Settings tab of the Machine Group Properties. Enter the default feed rate value and choose the unit:
- in/rev or mm/rev: Calculates the value in inches per revolution or millimeters per revolution.
- in/min or mm/min: Calculates the value in inches per minute or millimeters per minute.
Plunge rate
This option is not available for threading tools, drills, taps, and reamers.
% of Material feed/rev
This option is unavailable for threading tools.
Spindle speed
Enter a default spindle speed for the tool. You can choose to use this value as the default whenever the tool is selected for an operation, as set in the Tool Settings tab of the Machine Group Properties. Enter a spindle speed value in revolutions per minute (RPM). The CSS option is unavailable when defining threading tools, drills, taps, and reamers.
% of Material CS
This option is unavailable for threading tools, drills, taps, and reamers.
Coolant
Click to select default coolant options for the tool. You can choose to use these settings as the default coolant options whenever the tool is selected for an operation, as set in the Tool Settings tab of the Machine Group Properties. Be careful when selecting coolant options that are machine dependent or that are not available in all of your machine definitions. When you select this tool for an operation, Mastercam will match the default coolant selected here to the coolant options available on the machine solely by its number. For example, if you select the 4th coolant option here as the default, when you select this tool for an operation, Mastercam will try to activate the 4th coolant option in the active machine definition, if it has been defined.
Compute from material
This option is unavailable for threading tools.
Amount of 1st cut
Enter a default value to determine the amount of stock to be removed with the first cut. Mastercam uses this value as the default whenever the tool is selected for an operation if you select Use tools's step, peck coolant in the Tool Settings tab of the Machine Group Properties.
Amount of last cut
Determines the amount of stock to be removed with the last cut. This value is expressed as a radius. Mastercam determines the number of cuts it takes to remove all of the stock using the first cut value, the last cut value, and the depth of the thread. Most post processors make a gradual transition between the first and last cut.
Finish pass allowance
Determines the amount of stock to leave for spring cuts. This value is expressed as a radius.
Anticipated pull-off
Determines how far from the end of the thread that the tool starts to pull up out of the thread. This option is only available in canned (G76) threading.
Number of spring cuts
The number of cuts the tool needs to make during a pass at finish depth to remove the finish pass allowance.
Compensation options
These options are unavailable for threading tools, drills, taps, and reamers.
Tool clearance
This option is unavailable for threading tools, drills, taps, and reamers.
Metric values
Select to interpret values you enter as metric values.
Tool name
Enter a name for the tool, using up to 75 characters. Lathe tools must have a name. If you do not enter one, a warning prompts you to enter a tool name.
Manufacturer's tool code
Enter a comment of up to 75 characters that is displayed in the setup sheet to be used by the operator. This comment is not reflected in the toolpath.
Requires tool locator
This option is only used by Mill-Turn, for tools that will be mounted in a tool spindle or B-axis head. Select this option for tools (such as stick tools) that require a tool locator to be properly mounted in a tool spindle. Leave this unselected for tools that do not require a tool locator, such as HSK or Capto tools.
Save to library
Saves the current tool and its settings to a tool library. You can select a different library if you wish. If you do not click this button, the tool definition or any changes you have made will only be saved to the copy of the tool stored in the machine group, and will be unavailable to other Mastercam files.
Draw tool
Displays the tool geometry in the graphics window.
To save the tool geometry to a Mastercam file or to a level in the part file, use the Tool Manager. Right-click on the tool and choose the desired save option.
Setup tool
Opens the Lathe Tool Setup dialog box where you can choose the default mounting position, tool angle, spindle rotation direction, turret, active spindle and home position for programming the tool.





