Cut Out Toolpath

Watch tutorial: How to use the Cutout Toolpath

The Cut-Out toolpath is used to machine around selected vectors to cut shapes out from the material.

Basic Usage

Select the vectors you wish to cut out.
Choose a Start Depth. This is the depth at which you wish the cut to begin. A start depth of 0 means the cut will start at the material surface. Anything greater means the cut will start within the material, and so that material should already have been removed.
Choose an Overcut. An overcut of 0 means the tool cuts through the material exactly. Anything more will overcut to ensure the whole area is cleared. Anything less will leave unmachined material, which may be desirable for maintaining a vacuum.
Select your Tool
Press Calculate to calculate the toolpath.

Object Selection

Vectors can be selected for machining in one of two ways:

Manually using the selection tool.
Automatically by choosing a layer from the dropdown menu

If you choose to use the automatic selection then all of the vectors on the chosen layer are machined at the point of toolpath calculation.

Note

The automatic selection works at the point of calculation. If you add or remove vectors from a layer you need to recalculate the toolpaths.

Machine Vectors

This option determines which side of the selected vectors the tool will machine, controlled by the radio buttons. Choose Outside/Right to machine around the outside of the selection, or Inside/Left to machine within it.

Cut Direction

This option sets the direction the tool travels relative to the material as it cuts. There are two choices: climb or conventional.

With climb cutting, the tool rotates in the same direction as it is fed along the vector. Each cutting edge enters the material at the thickest part of the chip and exits at the thinnest. This generally produces a cleaner surface finish and reduces tool wear, and is usually the preferred choice on modern, rigid machines.

With conventional cutting, the tool rotates against the direction of feed. Each cutting edge enters the material at the thinnest part of the chip and builds to the thickest. This can produce more rubbing and heat, but tends to be more forgiving on less rigid machines or where there is backlash in the machine's drive.

Tip

If you are unsure which to use, climb cutting is the most common choice for CNC routing and typically gives the best finish.

Ramps

Use the Ramps toggle to add ramps. When ramps are enabled, rather than plunging directly downwards between passes, the toolpath will smoothly transition between passes.

Tabs

Use the Tabs toggle to add tabs, which hold the cut-out piece in place during machining. Specify the length and thickness of the tabs in the displayed boxes.

Click the Edit Tabs button to dynamically add and remove tabs from within the design view:

Tabs can be added by clicking anywhere on one of the selected vectors.
Tabs can be removed by clicking again on an existing tab.
Tabs can be moved by holding and dragging to slide the tab along the contour.
To add multiple tabs quickly, use line mode: click on a point that is not on one of the selected vectors, then choose another point. A line will be shown, and any time this line intersects a selected contour a tab will be added.

Toolpath Name

A toolpath can be given a descriptive name using the Toolpath Name input.