Page 1 of 4
An introduction to schematic symbols
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".
Packages 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.
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
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.
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
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.