A symbol for the schematic is created in its own library
from Project > Libraries > Add New SCH Library. The symbol is formed
using functionality from the Home > Place ribbon. Pre-defined symbol forms
can be used from Home > Templates > Symbol and IEEE Symbols from Home
> Place IEEE Symbols. The symbol will contain shapes, pins, text and symbol
marks. Here is a ‘non-descript’ four pin symbol for example purposes:
A footprint for the PCB is created in its own library from
Project > Libraries > Add New PCB Library. The footprint is formed using
functionality from the Home > Place ribbon. The footprint will contain
shapes, pads and text, plus other items. The footprint may also carry a height.
Here is a ‘non-descript’ four pin footprint for example purposes:
A component is created around a symbol for the schematic.
Using the example above, on opening its Component Properties, we see the
properties, parameters and models for the component:
In the example component, the following detail is used for these
Designator: Logical (Reference) designator such as R, C, IC etc.
Comment: Meaningful comment such as ‘0402 Resistor’ or its manufacturers part
Detailed description that appears in reports etc.
Standard component or other available types such as ‘mechanical’
Link: Component name within the library
List of applied parameters for other data, such as MRP Number
Define Footprint, 3D model and Simulation model
Through the ‘Edit Pins…’ button, the symbol pins and
footprint pads are mapped together and defined by ‘Type’ etc:
Using a XC9536-5CS48C from a Xilinx library as an example, this
device has seven individual symbols (A to G) representing its schematic
The Properties for Gate A, shows that it is Part 1 of 7:
Here are the mapped Pins, showing pin D6 (I/O) of Gate A
above (the rows with white backgrounds show the current selected gate pins) and
their display states:
numbering can be letter/number form for PLCC type devices.
Swapping can occur between pins, pairs and parts when in the
PCB, if defined within a component:
3D SOLIDWORKS Models are attached and physically positioned
on to the footprint using available functions. Attached models can appear both
in the 3D view in SWPCB and in the corresponding assembly of the board in SW.
Within a design project, libraries are referenced so that
the components can be added. New symbol libraries can be added through the
Libraries Panel, Libraries… button:
The libraries can be added directly to the current project,
where their order dictates their influence. Installed libraries list those that
are available to the workspace i.e. available to the project from the system
level, thus available to all projects. Added
Part (Component) in the schematic.
symbol and footprint libraries may be combined into an Integrated Library
(.intlib), which ensures ALL the relevant data moves together, including 3D
models etc. This process is achieved by creating a Library Package project from
File > New Integrated Library. Once created, save the project and add the
schematic and footprint libraries to it. The integrated library is then created
by compiling from right-mouse-button on the project in the Projects Panel and
Compile Integrated Library **.LibPkg. The resultant integrated library will be
found within an ‘Outputs’ sub-folder under the folder where the Library Package
was saved. Add this integrated library to your libraries folder or install it
within the Libraries panel.
Ensure multiple libraries, which includes the same devices,
are not available to the project. Or ensure their order of influence is
Component Supplier Links:
Supplier Links can be added to components, which provides
access to ‘live’ manufacturer’s component data, including price, availability
etc. Supplier links can be added to Parts (components) in a design or in a