Embedded Systems Design Resources

Introduction

In order to create a PCB, you must first prepare the schematic and check for errors, export a netlist of the schematic, import the netlist into PCB editor, and design the PCB. A netlist is a file that describes interconnections among components in a circuit. This tutorial describes the process of transferring a schematic to PCB Editor. It is assumed that you have a completed schematic (see example, Figure 1) before trying to migrate to PCB Editor.

Figure 1: Example schematic ready for transfer to PCB Editor

Video Walkthrough

1. Create Custom Footprints

All schematic symbols need a footprint. If you created any custom schematic symbols, you likely need to create a custom footprint for each one. For most ICs, you can use the Package Designer application to make custom footprints. For all other components, you can make custom footprints manually.

2. Open Project and Set Root Design

a) In Windows, open your project in the Design Entry CIS program.

b) For complex designs (see example, Figure 2), you may have multiple folders with multiple schematic sheets in each folder in the project explorer. Right-click on the folder you want to prepare for transfer to PCB Editor and choose "Make Root". This will set Cadence to generate a netlist only for the schematics inside the root folder (which will have a / through the folder symbol). This feature can be useful when your team is working on multiple break-out boards simultaneously before integrating them into one full design.

Figure 2: Example folder hierarchy for complex schematic

3. Assign Footprints to Components

c) Open the schematic and select all components on the page by choosing "Edit > Select All". Right-click and choose "Edit Properties..." (see Figure 3) to batch-edit the footprint information. The batch component property editing window will appear (see Figure 4). Click the Parts tab to show the parts in the schematic. Click the "Pivot" button to see the part information vertically instead of horizontally.

Figure 3: "Edit Properties..." menu option

Figure 4: Batch component property editing window

d) Enter footprint names (built-in or custom) for each component. For more information on finding the names of built-in footprints, see the "Where can I find a list of PCB footprints built-in to Cadence?" section on the Cadence PCB Tutorials page. Repeat until all components have footprints.

4. Run Design Rules Check

f) In the project explorer window, left-click on your schematic (see Figure 7) and choose "PCB menu > Design Rules Check" (see Figure 8). (If the Design Rules Check option is dimmed, then you have selected the wrong icon in the project explorer window). Figure 8 shows the Design Rules Check window. Leave the default options selected and click OK to continue.