Home | Contact Us
  Learn More Try Now
        Product Costs
        Contact Us
Article Index


An introduction to schematic symbols


Like the PCB symbol editors, BoardMaker3 has a flexible system for handling schematic components. Components are divided into two parts. The first of these is the symbol which is the logical element of the component together with its graphical representation. In the case of an opamp for example, the graphic is drawn with three pins. The functions of these pins are "Non-Inverting Input", "Inverting Input" and "Output".


The second part of a component is called a package and this is a separate library object. The package links the symbol to a physical device. In the operational amplifier example, the device might have one, two, four or more opamps and it is the package which specifies which pins of the device are associated with which gates. The package also links up with a PCB footprint. When a symbol is packaged, BoardMaker3 identifies the pin numbers for the gate and annotates the schematic diagram automatically. A symbol might have two or more alternative PCB footprints, for example, a QFP44, a PLCC44 or a DIP40. When a symbol is packaged in the QFP package, it will adopt the QFP pin numbering scheme, similarly, if the same symbol is packaged in the DIP40 device, it will adopt the DIP pin number scheme.

Pin numbering

In order to avoid repetition and reduce the chance of error when creating a package, the pin names for a package are automatically derived from the PCB footprint. Pin names in BoardMaker3 can be alphanumeric, with full support for PGAs, BGAs etc, but equally, using alphanumeric on simple parts can often reduce errors associated with devices such as TO92s where (B,C,E is often better than 1,2,3).


Annotation (or packaging) is the process whereby symbols are added into packages. BoardMaker3 will automatically annotate symbols that have been given a "default package" attribute (see attributes below) using the auto-annotate tool.
Other symbols can be packaged using a single keystroke and BoardMaker3 will present a list of existing components which have unused compatible gates in them or allow the user to create a new component from a compatible package. The software will automatically assign designator numbers to the package or this can be entered manually.

Equally, BoardMaker3 will assign gates automatically or specific gates can be selected. The unused gates can be tracked using the packager window since it is often desirable not to have any unused gates on a schematic invisible. Unused gates are also flagged as warnings at the netlist generation stage.


The symbol/package mechanism described above has a number of advantages :

  • You only need to draw a symbol of a particular type once. New footprint variants can be quickly defined simply by creating a new package data.
  • The package can contain additional information specific to a physical device such as exact order code, customer part number etc (see attributes below)
  • Schematic styles (compact, ANSI, IEEE91 etc) can be chosen to suit the user/project without having to redesign the packages
  • Using suitably descriptive function names will ensure that only the correct symbols can be packaged into particular devices.
  • No need to select the specific device whilst designing. Packaging is a separate step.
  • No need to delete and re-insert a part if the physical device needs to be changed. Just repackage in the new device.

Power & Ground

BoardMaker3 offers several mechanisms to deal with power and ground connections for a component. Some users prefer to keep connections for power and ground hidden and BoardMaker3 supports this with the "global net" mechanism. The default power and ground connections can be defined as part of the package mechanism (described above).

Once a symbol has been packaged in a schematic, the user can modify the connected nets if necessary. The advantage with this mechanism if that the schematic drawing remains uncluttered but the drawback is that the connections are not visible on the final schematic so BoardMaker3 provides a tool which will dynamically track the global net connections and display them in text form (a "global net locator") associated with the symbol.

Other users prefer to draw the power and ground connections explicitly for each component. BoardMaker3 supports this mechanism whilst still allowing various package configurations to be supported with a single symbol (often there are more or less power connections on alternative packages). BoardMaker3 even supports this mechanism for distributed gates where one or more of the gates can support the power connections.

A final option supported by BoardMaker3 allows the power and ground connections to be treated as separate gates. Often the "power gates" will be located on a separate page along with the "power gates" from all the other components.

Naming nets

BoardMaker3 supports three mechanisms for naming nets on a schematic. A standard net name can be added next to the wire to be named. Nets which are given the same names are merged together at the netlist generation stage.

Nets can also be named by adding a graphical symbol which conveys the name. The classic example of this is the "standard ground" symbol which consists of a short vertical line with three or more tapering parallel horizontal lines beneath it. The design of graphical net names is left to the user, although a set of standard designs are supplied.

Nets can also be name using a "named IO port". IO ports are the objects which link nets across multiple pages of a schematic. Regular IO port derive their name automatically from the wire to which they are attached, but on tight diagrams, this can clutter the display with a net name and an IO port being placed close together both conveying the same information. A named IO port is simply an IO port and a net name in a single object.

Home | Contact Us
@Copyright 2014 by Tsien (UK) Ltd. All rights reserved.