2D machining wizard

The 2D Machining Wizard provides a fully automated nested-based manufacturing solution for makers of custom furniture and cabinetry.

Using layered Drawing Interchange Format (.dxf) files originating from a variety of CAD systems, including the KCDw Cabinetmakers software, the 2D Machining Wizard nests vector artwork representing each cabinet component across multiple sheets, grouping them by material and thickness.

The 2D Machining Wizard then generates optimized toolpaths using pre-defined templates, assigning any combination of machining strategy, cutting tool and machining parameters to each Drawing Interchange Format (.dxf) layer in the design.

The calculated toolpaths can be simulated before being sent to the machine. More than 180 machine tool control options are supported, including automatic tool changing.

You can generate sheet reports for your nested design and outputs panel label data compatible with several third-party labelling packages, streamlining the process for the machine operator.

To use the 2D Machining Wizard:

  1. In the Project Tree, click the Toolpaths item. The Toolpaths panel is displayed.
  2. In the 2D Toolpaths area of the Toolpaths panel, click the Open 2D Machining Wizard button to display the 2D Machining Wizard panel.
  3. Click Browse in the Project CSV File area to choose the file from which you want to create the job. This displays the Select Project File dialog.
    Note: By default, ArtCAM lists Text Documents only (.txt). You can list Comma Separated Variable (.csv) files instead by clicking on the Files of type list followed by the Project Files (.csv) option.
  4. When you have located the text file from which you want to create the job, click its file name to select it. This text file must be located in the same folder as the Drawing Interchange Format (.dxf) files to which it refers. Its name is displayed in the File name box.
  5. Click Open to import the selected text file into the Choose Project CSV File area of the 2D Machining Wizard panel and close the Select Project File dialog. ArtCAM identifies the total number of panels, different types of material and different types of parts within the selected text file and displays these details in the Message Area window.
    Tip: If ArtCAM cannot find any .dxf files referenced in the selected text file, an error message is displayed in the Message Area window warning that the files are not recognized.
    Tip: Typically, an error is displayed when the text file and its associated .dxf file are stored in different folders or when the name of the .dxf file does not match the reference in he selected text file.
  6. Click View Log to display a text file in a new Internet Explorer window containing all data currently recorded in the Message Area window.
  7. In the DXF file units area, select whether you want to import the file as millimetres or inches.
  8. Click Browse in the Choose Toolpath Template area to display the Choose Toolpath Template dialog.
  9. Navigate to the folder containing the Toolpath Template (.tpl) file that you want to use.
  10. Click Open to import the selected toolpath template file into the Choose Toolpath Template area of the 2D Machining Wizard panel and close the Choose Toolpath Template dialog.
  11. In the Length alignment area, choose the appropriate axis to match your .dxf data:
    • If the length of the part is aligned with the X-axis, select Length in X.
    • If the length of the part is aligned with the Y-axis, select Length in Y.
  12. In the Nesting Clearance box, enter the offset distance applied to the nested panel artwork. This should at least be equal to the diameter of the profiling tool referenced in the toolpath template (.tpl) file used when machining the nested panel artwork.
  13. In the Edge Clearance box, enter the offset distance at which the nested panel artwork is set from the edge of the material sheet. This value can be 0.
  14. From the Machine Type list, select the post-processor that is compatible with your machining tool.
  15. If you are using a drilling bit separate from the router-head, select Use Optional Drilling Type, then select the appropriate post-processor from the list.
  16. Click Browse in the Select GCode Folder area to display the Browse for Folder dialog. This is the location the toolpath output files will be saved after the toolpaths are calculated.
  17. Select the folder which you want to use and click OK to close the dialog. The path of the chosen GCode folder is displayed on the settings page. For example, C:\Users\Public\Documents\ArtCAM Files\Toolpaths\GCode.
  18. Click Check Files to search the selected project csv file (.txt or .csv) for the .dxf files referenced within it.
  19. Click Calculate to begin the 2D Machining Wizard calculation process.
  20. Simulate the toolpaths for the vector artwork displayed on the active sheet.
  21. In the Project panel, select a Sheet item to display its options below the splitter bar.
  22. Click the Sheet Report button to display a sheet report for the active sheet in a new window. The report contains a preview of the vector artwork associated with the sheet, data concerning the sheet dimensions and toolpath data associated with the sheet. The report can be saved or sent to any printer installed on your computer.
  23. If you want to simulate the toolpaths associated with other sheets in the model:
    1. Right-click on the Toolpaths item in the Project Tree to display its context menu.
    2. Select Reset Simulation to delete the simulated toolpaths shown in the 3D view.
    3. In the Project Tree, select a different sheet to make it active and repeat steps 19 and 20.

See also

Topics in this section
Parent topic: 2D toolpaths