How to use the chamfer toolpath in Vectric software | 2.5D Toolpaths

Overview

This tutorial demonstrates how to create chamfer toolpaths in Vectric Aspire V12 using V-bits, including inside/outside slope options, combining chamfers with profile toolpaths, and using a chamfer width measurement to create countersunk holes.

Steps

1. Open the example file: Chamfer Toolpath Guide Example Number One.
2. Switch to the Toolpath tab and open Material Setup:
   • Thickness: 0.5
   • XY datum: bottom left
   • Z zero: material surface
   • Confirm rapid z gaps are appropriate for your machine.
3. Select the Chamfer Toolpath icon and select the vector(s) to machine. Tiling the 2D and 3D views makes it easier to see the cut direction.
4. Under Tool, click Select and choose a suitable tool. This example uses a 60° quarter-inch V-bit. Verify the feeds, speeds, and tool settings for your setup.
5. Set Chamfer Dimensions:
   • Angle is automatically grayed out when using a V-bit because the angle comes from the tool definition.
   • Enter either Width or Cut Depth; the other value updates automatically based on the tool angle.
   • To cut to the full material thickness, use Z= in the cut depth field.
6. Set Overcut if needed. This is useful for V-bits with a flat tip; it compensates by moving the tool and cutting slightly deeper.
7. Check Max Cut Depth:
   • Read-only field showing the actual full depth of the cut.
   • For V-bits, it matches the cut depth. For ball nose tools or overcut, it will be slightly deeper.
8. Choose a Chamfer Type:
   • Inside or Outside
   • Slope Upwards or Slope Downwards
   • The arrow tip in the 2D view represents the deepest point of the chamfer.
9. For the first example, use Inside / Upwards, then click Calculate.
   • If the software warns that the toolpath will cut through the material, this is expected when intentionally cutting through the full thickness.
10. Click Preview Selected Toolpath to review the chamfer cut.
11. To also cut out the finished part:
    • Use the same vector with a Profile Toolpath.
    • Set Start Depth to 0 and Cut Depth to Z=.
    • Choose an end mill and cut Outside the vector.
    • Calculate and preview.
12. For the Inside / Downwards example:
    • Reopen the Chamfer Toolpath with the same settings, choose Downwards, calculate, and preview.
13. To create a countersunk hole:
    • Copy the Width value from the Chamfer Toolpath.
    • Return to the Design tab and use Offset Vectors.
    • Paste the width as the offset distance, set offset direction to Inwards, and click Offset.
    • Select the new vector and create a Pocket Toolpath.
    • Set Cut Depth to Z=, remove any unused tools, calculate, and preview.

Key Points / Warnings

• Always set Z zero to the material surface before using the chamfer toolpath.
• Double-check rapid z gaps and tool parameters for your specific machine.
• V-bit angle is locked to the tool database angle; ball nose tools allow you to enter a custom chamfer angle.