The 3-Axis Wizard provides the ability to define a 3-axis machining strategy, associate the geometry, and define the parameters for every tool used in the machining process. The wizard allows you to first specify what type of machining feature, then specify the geometry you want to machine, select boundaries, followed by cycling through the tool and machining parameters of each type of operation contained inside the machining feature.
To access the 3-Axis Wizard right-click Milling Stock in the CAM tree tab and select Mill 3 Axis. Before any machining parameters can be defined, the machining strategy and geometry must be defined. This is accomplished is the first stage of the 3-Axis Wizard.
The first step to any 3-axis machining is selecting what type of machining strategy to use. The following machining features are available on the first page of the 3-Axis Wizard.
Mill Standard
Z-Level Rough - The Z-Level Rough is a roughing toolpath that machines the surfaces of a part at one constant Z-depth after another as if each pass were a basic pocket mill.
Z-Level Finish - The Z-Level Finish is more a semi-finish toolpath that machines the surfaces of a part at one constant Z-depth after another as if each pass were a basic profile mill.
Slice Planar - The Slice Planar toolpath divides the part into several straight slices and machines it one step over at a time.
Slice Spiral - Slice Spiral machines the part in a continuously spiralling motion over all 3 axes.
Slice Radial - Slice Radial can begin the toolpath either in the center of the part or at the edges, but the toolpath radiates out from the center.
Plunge Rough - The Plunge Rough is used to rough surfaces and solids using multiple vertical, or Z moves, and rapid moves above the part in the X and Y axes.
Mill Pro
Advanced Rough - The Advanced Rough is a roughing toolpath strategy which machines the surfaces at one constant Z-depth after another. However, this process recognizes open areas of the model and also offers semi-finishing within the same toolpath result. This 3-axis toolpath is available in the BobCAM PRO upgrade.
Flatlands - The Flatlands toolpath automatically detects any flat areas in the model, and provides an efficient cutting strategy for finishing the flat areas of the part. This 3-axis toolpath is available in the BobCAM PRO upgrade.
Equidistant - The Equidistant Offset is a finishing toolpath that maintains a constant step over on the surface of the part. The result is a part with a constant surface finish over its entirety. This 3-axis toolpath is available in the BobCAM PRO upgrade.
Pencil - The Pencil toolpath is a finishing toolpath used for machining internal corners and fillets that could not be cut previously by larger tools. This 3-axis toolpath is available in the BobCAM PRO upgrade.
Other - These options are categorized by themselves due to the fact that they require wireframe input instead of solids.
Engrave - This 3D Engrave feature allows to draw any 3D wireframe and trace it in a toolpath.
V-Carve - The V-Carve toolpath is a specialized toolpath used for creating sharp corners using a v-tool.
After selecting the machining strategy, click Next to move to the Geometry Selection page.
Select Geometry - Click to enable selection mode, allowing you to select any number of surfaces and solids.
Select Boundary
- Click to enable selection mode, allowing you to select the
geometry to specify a boundary chain when needed.