Importing vectors and create profile toolpaths in Vectric software | Getting Started

Overview

This video demonstrates how to import an existing DXF file, verify and adjust job setup, isolate a smaller sample section for machining, and create a profile toolpath with tabs for cutting out the part on a CNC machine.

Steps

1. Open the DXF file

   • In a fresh Vectric desktop product, choose Open and select GardenPanel-Vectors.dxf from the tutorials folder.
   • Note the variety of supported file formats in the open dialog for future reference.

2. Acknowledge the toolpath size warning

   • When using desktop products, toolpaths cannot exceed the machine area limit (e.g., 25“ x 25“ or 625mm x 625mm) without using toolpath tiling. Click OK.

3. Check and correct job setup

   • Open Job Setup and verify units. The imported file appears to be in millimeters, not inches. Switch units to millimeters.
   • Set material thickness to 11.5 mm.
   • Keep Z zero at the material surface.
   • For XY datum position, disable the Use Offset option so the job is positioned at the bottom-left corner.
   • Set modeling resolution to Standard unless 3D content is present.
   • Select material type (e.g., Canadian maple) and click OK.

4. Verify import accuracy

   • Select the bottom-right panel and confirm the dimensions match the drawing (e.g., 550 x 550 mm).

5. Clean up layers

   • Open the Layers tab.
   • Delete the empty layer “0” by right-clicking and choosing Delete.
   • Keep design and dimension layers as needed; dimensions can be hidden/shown via their layer visibility.

6. Create and organize sheets

   • Rename sheet 1 to Design.
   • Add a new sheet and rename it to Sample.
   • Edit the sample sheet size to 600 x 600 mm to stay within the allowable toolpath area. Keep thickness and datum settings consistent.

7. Copy the desired part to the sample sheet

   • Double-click the Design sheet, select the region to cut (e.g., the lower-right panel).
   • Right-click and choose Copy to Sheet → Sample.
   • Switch to the Sample sheet, select all copied vectors, and use the Alignment tools to center them on the sheet.

8. Hide the design sheet and focus

   • Hide the Design sheet via the Sheets dropdown.
   • Press F to fit/zoom to the visible sample sheet.

9. Verify toolpath material setup

   • Open the Toolpaths tab and confirm material thickness (11.5 mm), XY datum (bottom-left), Z zero (material surface), and rapid Z gap values are appropriate for your machine.

10. Create the profile toolpath

    • Select all vectors for the part.
    • Click Profile Toolpath.
    • Set cutting depth from 0 to 11.5 mm (through material).
    • Choose a suitable end mill from the tool database; verify feeds/speeds for your material and machine.
    • Set Cut Side to Outside.
    • Disable ramping/plunge moves unless required.
    • Enable Tabs – set length to 25 mm and thickness to 1 mm.

11. Manually place tabs

    • Use the tab editing dialog to add tabs in the 2D view.
    • Click along vector edges to place tabs. Position them in flat, accessible areas for easy removal.
    • Close the tab editor.

12. Calculate and preview

    • Name the toolpath (e.g., “Cut Out”).
    • Click Calculate.
    • Use Preview Visible Toolpaths to verify the cut, tabs, and waste material retention.

13. Save the toolpath

    • Close the preview.
    • Click Save Toolpath.
    • Ensure only the selected toolpath is saved.
    • Choose the correct machine and post processor.
    • Save the G-code file to a USB drive or transfer location.
    • Refer to your machine controller guide for final loading and running.

Key Points / Warnings

• Desktop Vectric products enforce a maximum toolpath area (25“ x 25“ or 625mm x 625mm) unless toolpath tiling is used.
• Always verify units after importing; DXF files may default to the wrong unit system.
• Disable the XY datum Use Offset option so the part aligns to the bottom-left corner of the machine.
• Imported DXF layers may include empty layers or dimension layers that should be deleted or hidden to keep the project clean.
• Use a separate smaller sheet for a sample part to avoid tiling and keep operations manageable.
• Tabs are essential for holding the part in place when cutting through material, especially without vacuum hold-down.
• Manually placed tabs should be in flat, easy-to-sand areas for clean removal.
• Always preview the toolpath before saving to catch any issues with tabs, cut side, or depth.
• Confirm the post processor matches your machine’s controller.