How to use the pocket toolpath in Vectric software | 2D Toolpaths

Overview

The Pocket toolpath clears material from inside selected vectors to a specified cut depth. This guide covers tool and depth settings, offset/raster clearing strategies, stepover and pass depth effects, profile passes, ramp entries, and pocket allowance.

Steps

1. Open the Pocket Toolpath example file and switch to the Toolpath commands tab. Use the 3D view and make sure vectors are visible.
2. In Toolpath Operations, click the Pocket toolpath icon to open the Pocket toolpath form.
3. Select the vector(s) to machine.
4. Set Start Depth to 0 when starting from the top of the material. Set a different value if you have already cut into the material.
5. Set Cut Depth to the total depth to machine, e.g. 0.25".
6. Choose a tool:
   • If no tool is listed, click Select to open the tool database.
   • If the desired tool is already listed, click Edit to review its settings.
   • Check Pass Depth: the maximum safe Z depth per pass.
   • Check Stepover: the horizontal distance between passes.
7. Choose a clearing strategy:
   • Offset: clears from the center outward, following the contour of the selected shape.
   • Raster: clears in a back-and-forth pattern. Set 0° for passes parallel to the X-axis, or 90° for parallel to the Y-axis.
8. Enter a toolpath name and click Calculate.
9. Preview the result. Use Ctrl+Calculate to quickly recalculate and view changes without opening the preview form.

Key Points / Warnings

• If Pass Depth equals Cut Depth, the pocket is cleared in one single Z pass. Reducing pass depth creates multiple depth passes.
• Stepover controls the spacing between toolpath lines. A smaller stepover produces denser toolpaths and a smoother finish, but increases machining time.
• Editing a tool inside the Pocket toolpath form only changes the tool for that toolpath; it does not modify the saved tool database entry.
• A raster strategy with a round tool can leave cusping on vertical walls. Enable Profile Pass to clean up edges.
  • Profile passes can be run first or last; the best choice depends on the material and whether the edges may chip.
• Enable Ramp Plunge Move to add a diagonal entry into the cut. This reduces tool wear compared to a vertical plunge. Specify the ramp distance.
• Pocket Allowance:
  • A positive value undercuts the pocket, making it smaller.
  • A negative value overcuts, making it larger.
• Pocket corners will always have a radius equal to the tool radius. Using smaller tools can reduce, but not eliminate, this effect.
• Always confirm that all tool settings are safe and appropriate for the machine, material, and tool setup.