3D Trace

3D Trace is closely related to 2D Engraving but allows for 3D movement of the cutting tool.

3D Trace can be applied to all types of open and closed curves. The tool will follow the curves as direct guide of cutting motion - or can be offset to the left it right of the curve if required.

You will need to place the curves to be cut into the following layer in the Rhino document:

KaroroCAM/3D Trace

Tool Position

You can choose for the path to be centered or on the left or right of the selected curves - with the offset being half the tool diameter:

Tolerance

KaroroCAM uses polylines (collections of line segments) to create toolpaths. All curves are converted to segments using this Tolerance setting as a guide. The Number represents the maximum deviation from the input curve to the final polyline.

The green toolpath curves in these two pictures show the extreme of the 1mm vs 0.01mm settings:

TIP: Use a tolerance one decimal place better than your machines smallest movement step - ie for most CNC routers 0.01 is recommended Tolerance

NOTE: Tight tolerances can lead to large file sizes and slow machine movement while cutting 

Outside Corners

This menu allows you to switch between Sharp and Round outside corners on your toolpaths. 2D Profile Cutting toolpaths are an offset from your input curve - based on the tool radius and stock to leave settings - with the two options being the difference in how offsets can be calculated on external offsets. 

NOTE: Rounded corners tend to be a better choice on angles less than 90 deg. Sharp corners can lead to smaller G-code files on cutting jobs that are mostly 90 deg corners.

NOTE: Rounded corners are effected by the toolpath Tolerance setting. 

Tool

Tool Shape

For the engraving toolpath three styles of tool bit are available:

Engrave Bit Angle

Sets the angle of the engraving bit tip.

Tool Diameter

Sets the diameter of your tool bit in mm.

Tool Number

Select Tool number that matches the tool spec'd in your tool path - mostly important for machines with auto tool change ability.

Spindle Speed

Sets the spindle speed for this operation in your GCode output file

Stock to Leave

Stock to Leave

This setting allows you set an additional offset to your Trace path  when using Left or Right Offset.

Cutting Depth

Cutting Depth Offset

Allows for a Z offset from your Trace toolpath

Multiple Depths

USE MULTIPLE DEPTHS

Check this box to enable multiple depth tracing

Step Down

Sets the depth of each pass when doing multi depth Trace toolpaths

Number of Steps

Number of Z steps to take when using multiple depth Trace paths.

NOTE: Total depth of cutting will be Step Down x Number of steps

Post Process

Post Process 3D Trace

Click this button to proceed to the Post Process Selection and Gcode File saving