Archives | Feedback

Schematic capture packages contain various tools and features that make the process of entering a schematic and documenting a circuit easy on the designer. One common feature among popular schematic capture packages is an array of libraries. Another is the ability to output netlists that are compatible with various simulation and PCB layout packages. The schematic capture process creates a database of symbolized parts and a netlist describing the connections between the symbols.

PCB layout packages have their own suite of tools and features designed to streamline the creation, verification, and documentation of a physical printed circuit board. All the board designer needs to do is define the outline of the board, add footprints from a decal library, import the netlist, and route the connections. Netlist comparisons will verify that the board matches the schematic. Online error checking warns of open or short circuit conditions. Design rules can be set up to check things such as matched net lengths, routing stubs, and parallelism.

Sounds simple, doesn’t it? Draw a schematic, output the netlist, and sit back to wait for your prototype assemblies. Simple that is, until the call from the assembly shop tells you that a part does not match its footprint, or you spend hours tracking down a diode or capacitor that was laid out backwards. An understanding of the process that takes place when exporting a schematic netlist is necessary to ensure your board layout will be correct.

Schematic Libraries

Schematic libraries are based on familiar symbols such as those shown on Figure 1:

Figure 1: A Typical Schematic Library

The symbol libraries are generic by nature. They are intended as building blocks for various part types. Schematically speaking, the same resistor symbol can be used for an eight- watt surface mount or 100-watt chassis mount device. The op-amp symbol could be a single device in a five-pin SOT package or a dual device in an eight-pin DIP. At a minimum, to create a valid schematic part, these symbols must have electrical pin numbers assigned and be saved in part type library. Quite often, this is the extent of the part type libraries supplied with the schematic capture tool (Figure 2).

Figure 2: Typical Part Type Library

Enough information is given to allow the designer to create a schematic, but information required to create a printed circuit board is missing. As with the symbol library, the vendor supplied part type libraries are intended as a starting point for a customized user library.

Customizing a vendor-supplied library requires that the user assign attributes detailing the specific part to be used in the design. A generic vendor supplied part type "Resistor" for example, could be copied to a customized user library, be given a footprint attribute "1206", and then be renamed to part type "RES_1206_SMT". When this new part is called from the user library, it would always require that a 1206 size surface-mount footprint be used to represent this device on the printed circuit board.

PCB Libraries

The PCB libraries are based on the footprints designated by industry standards. They usually include common surface-mount and through-hole devices. To create a footprint, or decal, pads are arranged in a specific pattern and designated with an electrical pin number. Figure 3 is an example of some common footprints shipped with most PCB design tools.

Figure 3: Common Footprints Shipped with PCB Design Tools

As with the schematic symbol library, one PCB decal can be associated with many different part types. The layout database relies on the pin numbers defined in the schematic library for mapping to a footprint in the PCB library. This process allows two completely different eight-pin devices to use the same eight-pin PCB decal.

Understanding the importance of this philosophy becomes even more obvious when you consider parts such as diodes or electrolytic capacitors. A generic schematic part called "DIODE" for instance, could be assigned a PCB decal called "D0-41" (Figure 4). If the diode is designated in the schematic library as having electrical pin 1 being the anode and electrical pin 2 the cathode, the associated D0-41 footprint must also have the same designations. Having the pins reversed on the PCB footprint can cause serious problems, which can be difficult to debug on an assembled board. Error checking will not catch this type of problem.

Figure 4: Generic Schematic Part (left) Translated
into a Specific PCB Decal (right)

The Netlist File

The netlist file is where the schematic and PCB databases come together. The output from a schematic database is formatted to meet the needs of a specific PCB layout package, and contains several specialized sections.

The first section usually describes the PCB decals that are needed in the design. If a decal does not exist in the PCB library, the desired part cannot be placed on the board. All schematic part types must be assigned a valid PCB decal before the schematic netlist can be imported to the PCB design database. Most PCB design packages will immediately flag an error and stop processing the netlist file if a decal is missing.

The next section of the netlist file contains the connection, or "rubber band", information. If a decal could not be found, there can be no connections to route. Other sections may include PCB routing directives, simulation directives, or detailed information for power and ground connections.

Save Time and Avoid Errors

Avoid using different platforms to produce your schematic and PCB designs. Most EDA vendors can provide bundled schematic capture and PCB layout packages that are designed to work together. These integrated packages provide a common shell that allows for easier verification of the schematic and board files, and makes processing engineering changes relatively painless. Integrated packages usually allow "back-annotation" as well, so that changes made in a PCB design can be reflected back to the schematic.

The use of a common library can help prevent problems. Develop a system where one regularly updated library serves the needs of all persons involved in design activities. Multiple people creating the same devices in individual libraries will only lead to errors and confusion at layout. If a new part needs to be constructed, build it in a central library so everyone can use it. Review all newly created parts and their associated PCB footprints for accuracy.

PCB layout tools will normally present an error or warning if the schematic part references a PCB footprint with fewer electrical pins than described in the schematic netlist. For example, if a fourteen-pin device were assigned to an eight-pin decal, there would be an error mapping the ninth through fourteenth pins described in the schematic. If, on the other hand, a fourteen-pin decal is assigned to an eight-pin device, error flags are not necessarily raised. A PCB decal can have more pins than electrically represented in a schematic--mounting or alignment holes for instance are part of a decal. This type of error often goes unnoticed as well. It is usually found after the PCB is fabricated when someone tries to mount a 14-pin device in a 16-pin decal.

Many companies’ use outside sources to design printed circuit boards. If you use an external design house to provide your printed circuit board layouts, make sure your engineers are familiar with the tools they use. Sending out a netlist file in the correct format will save time and money. Share your libraries with your vendor so they can save time and avoid having to re-create parts. Create your schematic libraries so that they reference the PCB footprint libraries of your design house.

Click here to view this column in .pdf format. (24k)

Analog Main | Product of the Week | Columns | Editorial | Tech Notes