If you want to review and archive the Gerber data you provide to your fabricator you can load the Gerber data back into PCB Editor as described below. 


Note: OrCAD PCB Editor only supports the importation of Gerber data was was generated by either Cadence PCB Editor or OrCAD PCB Editor.

  1. Create the Gerber data for the design.  

    1. Selecting the menu items Export > Gerber. Your selection opens the Artwork Control Form.

    2. Open the General Parameters tab and set the parameters for the Device type, Output Units, and Format in the Artwork Control Form.

    3. Open the Film Control tab.

    4. Set the undefined line width. An undefined line width of zero is not plotted.

    5. Select the film layers to be included in your Gerber data and then click the Create Artwork button to generate the Gerber data.

    6. Click the OK button to close the dialog.
  2. Create a user-defined subclass for which you can reload the Gerber data back into the design without causing DRC conflicts.

    1. Select the menu items: Setup > More > Subclasses. Your selection opens the Define Subclass dialog.

    2. Click the BOARD GEOMETRY button. This opens the Define Subclass dialog.

    3. Add a new subclass by entering a subclass name and pressing your keyboard Tab key which inserts the new layer name into the stackup listing. Add as many subclasses/layers as desired.

      The screen image above, for example, shows the additional new layers BOTTOM, GND, TOP, and VCC.
  3. Import the film layer back into PCB Editor.

    1. Select the Import > More > Artwork menu. Your selection opens the Load Cadence Artwork dialog.

    2. Click the Filename Ellipsis button and browse to the file you want to import.

    3. Select the appropriate Class and Subclass of the file.

    4. Click the Load file button to import the file.

      The outline of the data attaches to your cursor. Use your left mouse button to place the file data. Or you can select Snap pick to from your right mouse pop-up menu.

      After the artwork is placed the command line message "Photoplot file loading completed with no errors" displays and you are prompted to select another film if desired.