[17.4] OrCAD PCB Walk-through: Manufacturing Preparation

This OrCAD PCB Editor tutorial demonstrates how to prepare your board for manufacturing and generate manufacturing data.  After you complete PCB Walkthrough 8 you will be able to:

  • Add dimensions and titleblock for fabrication
  • Create a Drill Chart and Cross Section Chart
  • Setup Artwork Films

If you would like to follow along with this tutorial, you can visit our walk-through page to view video tutorials and download design files.

To follow the instructions presented in this tutorial, continue using the design you completed in PCB Walkthrough 7 or open the provided board file in the folder directory, PCB Walkthrough 8_Manufacturing Preparation.   

  1. Select the Color button from the toolbar.

  1. Select the Nets tab and select Clear all Nets.
  2. Select Yes to clear the nets and click OK.
  3. Select Setup > Application Mode > General Edit from the menu.

  1. In the Visibility tab, set Global Visibility to On.

  1. In the Find tab, select All On.
  2. Highlight the board.
  3. Select the Move button on the toolbar.
  4. Click the canvas to place your board at a new location.
  5. Zoom in to the bottom of the board.
  6. Select Setup > Change Origin from the menu.

  1. Right click the corner of the board and select Snap Pick to > Segment Vertex
  2. Select Place > Component Manually from the menu.

  1. In the Advance Settings tab, select Library.

  1. In the Placement List tab, select Format symbols from the drop-down.
  2. Select the box next to ASIZEH.
  3. Click the canvas to place.
  4. Close the placement window.
  5. Select Add > Text from the menu.

  1. In the Options tab, select Drawing Format and Title_Block as the Active Class and Subclass.
  2. Set the Text Block to 6.
  3. Click the canvas and type the desired text.
  4. Right click and select Done.

  1. In the Visibility tab, select Last.
  2. In the Find tab, select All Off then select Text.
  3. Edit the text on the board as needed.

Note: To delete, right click and select delete.  To move, click and drag. To rotate select the text, right click and choose spin.

  1. Select Edit > Change Object from the menu.
  2. Uncheck the line width box and select Text Block.
  3. Change the Text Block to 2.
  4. Click on the reference designator text for each component.
  5. Select Manufacture > Customize Drill Table from the menu.

  1. Select Validate.
  2. Select Auto generate Symbols and Yes.  Click OK.
  3. In the Design Workflow, select Manufacturing Preparation > Documentation > Drill Chart.
  4. Leave the defaults and click OK to create drill chart.
  5. Click the canvas to place the drill chart.
  6. In the Design Workflow, select Manufacturing Preparation > Documentation > Cross Section Detail.
  7. Set the Text Block to 3.
  8. Click OK and click the canvas to place.
  9. Select Manufacture > Dimension Environment from the menu.
  10. Right click and select Linear Dimension.

  1. Click corners of the board to dimension. Click to place the dimension.
  2. Right click and select Done.
  3. Select Setup > User Preferences from the menu.

  1. Select File_management > Output_dir.
  2. Add the text .\artwork to the first input field. Click OK.

Note: This will create a folder for your exported artwork.

  1. Select the Color button from the toolbar.
  2. Select Off for Global Visibility.

Note: This will turn off all layers and ensue only the necessary layers are selected.

  1. In Drawing Format, select All.
  2. In Manufacturing, select NClegend1-3 and Xsection_Chart.
  3. In Geometry, select Design_Outline and Dimension.
  4. Select Apply.
  5. In the Design Workflow, select Manufacturing Preparation > Documentation > Artwork (Film Records) Setup.

  1. Right click in the film window and select Add.
  2. Assign FAB as the film name and click OK.
  3. Change the Undefined line width to 0.127.
  4. Complete this process for all the Artwork Films using the provided table below:

Note: If you need to make changes to existing films, expand the film name. Add or cut layers as needed. To view a film in the PCB Window, right click and select display for visibility or in the Visibility Tab, select from the films in the drop-down.

  1. Close the Artwork setup window and the Color window.

 

Previous Article
[17.4] OrCAD PCB Walk-through: Manufacturing Export
[17.4] OrCAD PCB Walk-through: Manufacturing Export

This OrCAD PCB Editor tutorial demonstrates how to generate manufacturing export files.

Next Article
[17.4] OrCAD PCB Walk-through: Design Rule Check
[17.4] OrCAD PCB Walk-through: Design Rule Check

This OrCAD PCB Editor tutorial conducts a final design rule check (DRC) which is necessary to prepare the b...

OrCAD Free Trial

Try OrCAD Today