Pocket Toolpath

The Pocket toolpath clears away the material contained inside selected vectors, machining a flat-bottomed recess down to a chosen depth. The software automatically compensates for the tool geometry, so the finished pocket matches your vectors exactly.

Watch tutorial: How to use the Pocket Toolpath

Basic Usage

1. Select the closed vectors you wish to pocket out.
2. Choose a Start Depth. This is the depth at which the pocket calculation begins. A start depth of 0 cuts from the material surface; a greater value is used when machining into a pocket that has already been cleared.
3. Choose a Cut Depth, measured down from the Start Depth.
4. Select your Tool.
5. Press Calculate to create 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.

Tools

More than one tool can be used to clear a single pocket. The first tool removes the bulk of the material, and each subsequent, smaller tool clears the areas the previous tool could not reach.

• Select opens the Tool Database to add a tool to the list.
• Edit adjusts the cutting parameters for this toolpath without changing the master database entry.
• Remove deletes the selected tool from the list.
• Use the arrow buttons to change the order in which the tools are used.

Clearance Strategy

Choose how the enclosed area is cleared:

• Offset — clears the pocket with passes offset progressively inwards from the boundary. When the stepover is more than 50% of the tool diameter, small moves are added into the corners to clear the remaining material.
• Raster — clears the pocket with back-and-forth passes at a configurable angle between 0 and 90 degrees. The profile pass along the boundary can be machined First, Last, or not at all.

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.

Pocket Allowance

A pocket allowance leaves a thin layer of material on the walls of the pocket for a final profile pass to remove, producing a cleaner finished edge.

Ramps

Use the Ramps toggle to add ramps. When ramps are enabled, the tool eases gradually into the material between passes rather than plunging straight down, reducing heat and load on both the tool and the spindle.

Toolpath Name

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