Tool Offset

When pocketing or contouring, the system calculates a tool offset amount based on the radius of the tool. This is the amount the finishing pass of the toolpath (the only pass if contouring) will be offset from the selected part geometry. If a stock amount is entered for the process, that stock amount will be added to the tool radius offset.

When milling with tapered or pointed tools, the system calculates the tool offset based on the Floor Z compared against the Surface Z. The Surface Z is the top surface of the material. The Floor Z specifies the finished depth of the pocket or contour. These values are entered in the Contouring and Roughing Process dialogs in the Entry/Exit Clearance Diagram.

The tool diameter used to calculate the offset amount is the diameter of the tool at the Surface Z. In order for the system to correctly calculate the tool offset when using these tools, accurate Floor Z and Surface Z positions must be entered in the Process dialogs.

When milling with tools (both tapered and non-tapered) that have a bottom corner radius, the system checks the bottom corner radius at the Floor Z compared against the Surface Z and adjusts the tool offset amount accordingly.

This offset calculation is useful when cutting pockets shallower than the corner radius on the tool. Also, chamfering a pocket is easily accomplished by entering accurate Z positions in the process dialog and entering a negative Stock value equal to the desired chamfer amount. The system will correctly calculate the tool offset from the geometry when creating the toolpath in order to correctly machine the chamfer.

Offset calculation with tapered tools are only made when Tool Center is selected for the Contour Cutter Comp Preference.

Cutter Radius Compensation (CRC)

The File > Machining Preferences > Contour Cutter Comp h specifies how the system will handle CRC with Contouring and Roughing operations. From Tool Center is the GibbsCAM recommended option because this is what is displayed by the orange toolpath lines. If From Tool Edge is selected, the toolpath lines are still displayed as "tool center". From Tool Edge only affects the posted code.

When the From Tool Center item is selected, the numbers generated in the posted code will be calculated from the geometry, offset by a tool radius (providing the Stock amount is 0). When the From Tool Edge item is selected, the numbers generated in the posted code will be the same as the blueprint numbers.

Roughing operations will always be calculated from the tool center. If the From Tool Edge item is selected for this preference, CRC should be turned off in all roughing operations.

When using From Tool Center, the offset in the CRC register at the control should be the difference between the radius of the actual tool used and the radius of the tool programmed in the system. If the tools are identical, the CRC offset number should be 0. If the actual tool is smaller, a negative value can be used.

When using From Tool Edge, the radius of the actual tool used should be entered in the CRC register. If tapered tools or tools with corner radii are used, the user must calculate the appropriate offset amount based on the taper.

The toolpath offset is better than the majority of controls. Regardless of the setting made in this preference, all toolpath drawing and cut part rendering will be displayed to the center of the tool.