Parameters: Drills, Taps, and Reamers
Use this tab to set default drilling parameters for the tool. When you select this tool while creating a toolpath, many of the values that you enter here automatically transfer to the parameters for the new toolpath. Use 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.
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 a default feed rate for the tool 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 unavailable for threading tools, drills, taps, and reamers.
% of material feed/rev
Determines what percentage of the base material feed/rev value will be used. Mastercam uses this value when you tell it to automatically calculate a feed rate from the selected stock material.
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
Sets the feeds and speeds to those set in the material definition. If no material has been selected in the Machine Group Properties for the active machine group, you will be prompted to select a material. This option is unavailable for threading tools.
First peck
Determines how deep the tool will pierce the stock on the first peck. This is a positive incremental number that also represents the amount of material removed.
Subsequent peck
Determines how deep the tool will pierce the stock for all peck moves after the first peck. This is a positive incremental number that also represents the amount of material removed with each peck.
Peck clearance
Sets the depth that the tool rapids to between peck moves. The value is added to the previously drilled peck depth.
Retract amount
Sets the amount that the drill will retract every time it makes a peck move. It is positive and incremental.
Dwell
Determines the amount of time, in seconds, that the tool pauses at the bottom of a drilled hole.
Cycle
Select a drill cycle from the drop-down list. This becomes the default cycle in drilling toolpaths whenever this tool is selected for an operation.
Tip
Programs the toolpath from the tip of the tool corner radius. This is the only Compensation option available 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.





