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

Overview

This video demonstrates how to set up and use the Profile Toolpath in Vectric Aspire V12 to machine around or along vectors. It covers toolpath creation, cut depth settings, tool selection, pass steps, ramp plunge moves, and adding tabs to hold parts in place.

Steps

1. Open the Profile Toolpath

   • Open the Toolpaths tab on the right.
   • In Toolpath Operations, click the first icon: Profile Toolpath.

2. Select the vector(s)

   • Choose the vector(s) you want to cut around or along. Example: a square to be cut out.

3. Set Start Depth

   • Leave at 0 when cutting from the material surface.
   • Set a positive value only when the toolpath must start below the surface, e.g. inside an already-machined pocket.

4. Set Cut Depth

   • Enter the total depth to cut into the material.
   • Tip: type Z= in the field to automatically insert the material thickness saved in the software.

5. Select a tool

   • Click Select to open the tool database.
   • Choose a suitable tool, e.g. 1/4" end mill.
   • Use Edit to adjust toolpath-specific settings without changing the stored tool database defaults.

6. Set Pass Step / Number of Passes

   • In the tool Edit window, set the Pass Step to control how deep each Z pass is.
   • Example: 0.125" pass step on a 0.5" cut depth produces four passes.

7. Choose Machining Side

   • Select Outside, Inside, Left, Right, or On the vector.
   • For cutting a part out, choose Outside.

8. Set Direction

   • Choose Climb or Conventional.
   • Test on scrap material to see which gives the best finish for your tool/material.

9. Name and Calculate

   • Name the toolpath, e.g. Profile 1.
   • Click Calculate to generate the toolpath preview.

10. Preview and Verify

    • Use the toolpath preview to inspect plunges, passes, and cut direction.
    • Slow down the preview if needed.
    • Reset/close the preview form when done.

11. Edit Toolpath if Needed

    • Double-click the toolpath in the Toolpaths list to reopen it.
    • Change the pass step if safe, e.g. from 0.125" to 0.25" to reduce passes.
    • Recalculate to apply changes.

12. Add Ramp Plunge Moves (Optional)

    • Check Apply Ramp Plunge Move to ramp into the material instead of plunging straight down.
    • Set a ramp distance, e.g. 1".
    • This creates a zigzag angled descent to the first pass depth, reducing tool stress.

13. Add Tabs (Optional)

    • Check Add Tabs to Toolpath to hold parts in place.
    • Set tab Length and Thickness.
    • Click Edit Tabs to place tabs manually or automatically:
      • Use constant number of tabs.
      • Or use constant distance between tabs.
      • Use Avoid corners and curved regions to prevent tabs in difficult areas.
    • Click Add Tabs to apply.

Key Points / Warnings

• The Profile Toolpath requires at least one selected vector.
• Start Depth should normally be 0 unless machining below an existing surface/pocket.
• Z= in the cut depth field inserts the material thickness automatically.
• Use the Edit button to modify tool settings for the current toolpath only; the original tool database values remain unchanged.
• Pass Step determines the Z increment per pass. Larger pass steps mean fewer passes but more tool load.
• For cutouts, machine Outside the vector so the part keeps its intended size.
• Climb vs conventional milling can affect finish; run test cuts to compare.
• Ramp plunge moves reduce tool wear but require space for the horizontal ramp distance.
• Add tabs when no vacuum hold-down is available; otherwise the cut part may move or break free on the final pass.
• Tabs must be removed manually after machining, leaving small marks that need finishing.