Plunge clearance — This is the distance above an operation at which the tool starts to feed. In the case of deep hole drilling, the drill retracts to this distance between pecks. For milling features, the default is to use the same value for roughing and finishing. As a result, the tool feeds from the top of a pocket to the floor before cutting. To make the tool feed down into the feature, set the Plunge clearance for an operation to a negative value, but make sure the value is above the floor of the feature.
2nd offset reg. increment — When using a 2nd offset register for grooving tools, the 2nd Length offset register in the Tool Mapping dialog is calculated as the Length offset register plus the 2nd offset reg. increment.
Swiss Safety Allowance — Specify an additional safety allowance to increase the length of stock exposed past the chuck, which increases the minimum distance between the chuck and the guide bushing to prevent collisions.
Tool program point — Specify the program point for turning tools, select from:
Turnmilling program point — Specify the program point for turnmilling tools, select from:
Feed from start point or curve — Select this option to use a feed move from the Start point or the end of the Start curve, to the beginning of the toolpath. If you are using a start curve, you have two further options:
Turret direction — Select Auto to enable FeatureCAM to calculate the best direction for a particular operation. You can also explicitly set this option to CW (clockwise) or CCW (counter-clockwise).
RPM Range — If your machine has explicit spindle speed ranges, you can set this option.
Remachining — This automatically sets the boundaries for subsequent operations that use the same curve. This minimizes air cutting and works between Turn features, Bore features and between Holes and Bore features. The same curve must be used in both features. ID features use the results of a previous turn drill operation if such a feature exists. The stock curve that results from the first operation is the result of undercut clipping with the tool geometry and nothing more than that.
Constant Surface Speed — Select this option to specify the speed as a constant surface speed.
Use IPR/MMPR — The default feed units are IPM (inches per minute) or MMPM (mm per minute). Select this option to use IPR (inches per revolution) or MMPR (mm per revolution).
Do feed reduction for small moves — This attribute helps FeatureCAM cut small features properly. It is typically applied to small chamfers or small radii but affects any small move. If Do feed reduction for small moves is selected, then any move with fewer revolutions than the Threshold, is reduced by the Feed rate %.
Calculate index radius from solid stock outline — Select this option to determine the index height directly from the stock solid, instead of calculating it above a square bounding box.
Automatic tool orientation — Select this option to use a turning tool in any orientation without needing to create duplicates. When this option is selected, only tools in the default orientation are displayed in the tool crib and available for selection. When this option is deselected, all tools are available, but each tool can only be used in the orientation selected on the Orientation tab of the Tool Properties dialog.