In addition to graphic information about the symbols of the components and their arrangement on the page, a schematic also includes electrical information and in particular a schematic provides information about the existing connections between the components. A connection is the list of all the pins that are connected together. The netlist is the list of existing connections in a schematic.
The electrical terminals
All electrical objects (symbols, wires, ports, etc.) have attachment points, called pins or terminals, which allow the electrical connection between the objects.
To better highlight the existence of the connection between the pins, a circle is drawn around the unconnected electrical terminals. In the following figure, there is a connection between R1 and R3, between R2 and R3 but not between R2 and R1.
 Tip: |
|---|
The circle style indicating a free terminal can be set in the Schematics tab in the Document Properties dialog box. Set the value of the field Style of: Pin Free. The dialog can be activated by selecting the command Settings » Document Properties or by using the key combination CTRL+ALT+D. |
Non-active electrical terminals
Input pins belonging to a component that do not need to be connected must be explicitly declared as inactive pins.
When a pin is declared inactive, it is highlighted with the following symbol 
and excluded from operations such as ERC control, netlist generation, etc.
To declare that a pin is not active you must set the option Pin electrically not connected
in the Type tab of the Pin Properties dialog.
| Tip: |
|---|
The style for the inactive pin symbol can be set in the Schematics tab in the Document Properties dialog box. Set the value of the field Style of: Pin Unconnected. The dialog can be activated by selecting the command Settings » Document Properties or by using the key combination CTRL+ALT+D. |
Electrical connections
The connections between the electrical terminals of the components can be physical or logical.
Physical connections
The necessary but not sufficient condition to realize a physical connection between two electrical terminals is that they are physically in contact or that the coordinates of the end points coincide. The simple overlapping of the electrical terminals does not make the connection but it is necessary that the objects have been actually connected. The connection between the electrical objects is made automatically during the creation and positioning of the objects. If the objects are already positioned in the schematic, the connection must be made explicitly.
To connect a component
-
Select the object to connect and do one of the following:
Choose the command Schematic » Connect or click the
tool in the toolbar.
Press the key combination CTRL+L.
To disconnect a component
-
Select the object to disconnect and do one of the following:
Choose the Schematic » Disconnect command or click the
tool in the toolbar.
Press the key combination CTRL+U.
Logical connections
A logical connection is made by means of the following objects: Net Labels, Ports, Sheet Entries, Bus Entries, Power Ports and Hidden Pins. To make a logical connection it is not necessary that the electrical terminals are physically in contact but it is sufficient that they belong to connections having the same name.
In the following figure, the pair of resistors R1 and R2 (physically connected to each other) and the pair of resistors R3 and R4 (physically connected to each other) are connected by a logical connection in figures A and B and a physical connection in figure C. All connections with the same name (Net1) belonging to the same page are always connected together, i.e. they form a single connection. All the Ports with the same name (A1) belonging to the same page are always connected together.
Names of connections
During the generation of the netlist, each connection is automatically assigned a name except in cases where one of the following objects is connected to the connection:
| Object | Description |
|---|---|
|
Net Label |
A net label object allows you to assign a certain name to a connection. If you want to assign a name to a connection, you must hook a net label object to a wire that is part of the connection. By naming a connection, you can make logical connections between portions of a schematic that are not physically connected. |
|
Bus Entry |
A Bus Entry object is a terminal for entering and exiting signals from a Bus and is represented with a 45ยบ line attached to the outer edge of the Bus. Bus Entry objects, such as Net Label objects, give their name to the connection. |
|
Hidden pins |
Hidden pins of components, such as power supply pins (VCC and GND), give their name to the connection. Power port objects (present in libraries) contain a hidden pin and consequently assign their name to the connection. Connections whose name is determined by a hidden pin are always globally valid, i.e. they are valid on all project pages. |
The name of the connections is automatically generated based on the parameters specified in the tab Schematics in the Project Properties dialog box. The dialog can be activated by selecting the command Settings » Project Properties or by using the key combination CTRL+ALT+P.
Validity range of connection names
The names of the connections can have a local validity, that is limited to the page, or global validity and therefore extended to the whole project:
|
Local |
Connection names are only valid within the page where they are defined. All connections with the same name belonging to the same page are always linked together. Connections with the same name but belonging to different pages are not linked together. |
|
Global |
The names of the connections are valid on all pages of the project. All connections with the same name belonging to the same page or different pages are linked together. Connections whose name is determined by a hidden pin always have global validity. |
| Tip: |
|---|
The validity range of the connection names can be set on the Schematics tab in the Project Properties dialog box. Set the parameters in the group Compiling Netlist. The dialog can be activated by selecting the command Settings » Project Properties or by using the key combination CTRL+ALT+P. |
Connections in Multi-Sheet projects
When a schematic is divided into several pages, the connections between the pins of components belonging to different pages are made as follows:
|
Using the names of the connections |
The names of the connections can be used to connect portions of the schema belonging to different pages
only if they have extended validity to the project, in this case all the connections with the same name belonging
to the same page or to different pages are linked together and constitute a single connection.
|
|
Port to Port Connection |
Ports allow you to extend a connection. By means of the ports it is possible to connect to each other electrical terminals not connected by a wire. The ports can be used to connect portions of the schematic belonging to different pages only if they have extended validity to the project. The port name is independent of any name assigned to the connection, it is only used to define which ports must be connected. |
|
Sheet Entry to Port Connection |
Sheet Entry objects are Ports that are attached to the inside of the Sheet objects and of which they constitute the entry and exit ports. Each Sheet Entry must correspond to a Port, with the same name, present in the child sheet associated with the Sheet object. |
|
Hidden pins |
Hidden pins of components such as power supply pins (VCC and GND) assign their name to the connection and always have global validity, i.e. they are valid on all project pages. |
|
Power Port |
Power port objects contain a hidden pin and consequently assign their name to the connection and always have global validity, i.e. they are valid in all project pages. |
Horizontal connections
Connections between different pages made using connection names or Port to Port connections are called horizontal connections. A project in which connections between pages are made horizontally is called Flat because all the sheets of the schematic are on the same level.
Vertical connections
The connections between different pages made by connecting the Sheet Entries with the Ports having the same name and belonging to the associated child sheet are called vertical connections. A project in which the connections between the pages are made vertically is called Hierarchical because the entire project can be represented by a tree structure in which the different sheets can be found on different levels.