PCB Walk-through 1: PCB Setup

This walk-through demonstrates how to setup the board configuration. After you complete this topic, you will be able to:  

  • Setup and edit design parameters  
  • Add a layer to the board stack up  

To follow along, open the provided PCB TUTORIAL.brd file in the folder directory, PCB Walkthrough 1: PCB Setup.  

If design files were not downloaded at the beginning of the walk-through, they can be accessed through the Materials tab above.

Open in New Window

  1. Select Display > Windows > Design Workflow from the menu. 
  1. In the Design Workflow, select Setup > Design Parameters.  

Note: In the Design Parameter window, you can specify parameters for display, design, text, shapes, routing, and manufacturing. 

  1. Select the Design tab. 
  1. Set the User Units to Millimeter
  1. Click OK
  1. In the Design Workflow, select Grids.  
  1. For Non-Etch, set the Spacing to 1 for both X and input fields. 
  1. Click OK
  1. In the Design Workflow, select Colors

Note: Here you can specify colors in the design for layers, nets and more. 

  1. Leave the default settings and close the window. 
  1. In the Design Workflow, expand Database Preparation
  1. Select Board Outline > Create > Automatically

Note: Make sure Create is checked in the Design Outline window. 

  1. Enter 0.3 MM for the Design Edge Clearance
  1. Select Place Rectangle
  1. Enter 100 MM for the Width
  1. Enter 50 MM for the Height.  
  1. Click the design canvas to place the board outline. 
  1. Click OK
  1. In the Design Workflow, select Cross Section (Stack-up) > Create
  1. Right Click in the name column and Select Add Layers
  1. Assign POWERPLANE as the Name Prefix. 
  1. Select Below selected Dielectric as the New Layer Position. 
  1. For Layer Type, select Plane
  1. Click Add and Exit

Note: This has added the plane and dielectric layer. 

  1. Click OK to close out of the cross-section window. 

Note: If you need to import a netlist, select Netlist > Import in the Design Workflow. Select Design Entry CIS and set the import directory as the folder location of your netlist. Click Import. 

EMA Design Automation