Further Information

In this topic:

How Symbols are Stored

When a symbol is placed on a schematic, a copy of that symbol definition is stored locally. This makes it possible to open the schematic even if some of the symbols it uses are not available in the symbol library. However, if you edit a symbol definition for a schematic that is saved, when you open that schematic, it has a choice between its local copy of the symbol or the copy in the library. Which it chooses depends on an option chosen when the symbol is saved. When saving the symbol with the graphical editor, you will see the check box All references to symbols automatically updated. If this is checked then the schematic editor will always use the library symbol if present. If not, it will use its local copy.

If a schematic is using a local copy and you wish to update it to the current library version, select the symbol or symbols then select the popup menu Update Symbol. Note that all instances of the symbol will be updated. It is not possible to have two versions of a symbol on the same schematic.

Important Note

Note, that only the symbol geometry, pin definitions and protected properties of a schematic instance will be changed when its symbol definition is edited.

Unprotected properties will remain as they are. For example, the standard NPN bipolar transistor symbol has an initial value property of Q2N2222 so when you place one of these on the schematic from the Place menu or tool bar, this is the value first displayed. This can of course be subsequently changed. The initial value of Q2N2222 is defined in the NPN symbol. However, if you edit the symbol definition and change the initial value to something else - say - BC547, the value of the value property for any instances of that symbol that are already placed will not change.

You can use the popup menu Restore Properties... to restore properties to their symbol defined values. For more information, see Restoring Properties.

If you wish a property value to always follow the definition in the symbol, then you must protect it. See Defining Properties for details.

Summary of Simulator Devices

The following information is needed to define schematic symbols for the various devices supported by the simulator.

In order to be able to cross-probe pin currents, the pin names for the schematic symbol must match up with those used by the simulator. So for a BJT (bipolar junction transistor) the simulator refers to the four pins as 'b', 'c', 'e' and 's' for base, collector, emitter and substrate. The same letters must also be used for the pin names for any schematic BJT symbol. The simulator device pin names are listed below.

The model property is the schematic symbol property which describes what type of device the symbol refers to. SPICE uses the first letter of the part reference to identify the type of device. The SIMetrix netlist generator prefixes the model property (and a '$' symbol) to the part reference to comply with this. This makes it possible to use any part reference on the schematic.

Device	Model property	Pin no.	Pin names	Pin function
XSPICE device	A
Arbitrary Sources	B	1	p
		2	n
Bipolar junction transistors	Q	1	c	Collector
		2	b	Base
		3	e	Emitter
		4	s	Substrate
Capacitor	C	1	p
		2	n
Current Controlled Current Source (2 terminal)	F	1	p
		2	n
Current Controlled Current Source (4 terminal)	F	1	p	+ output
		2	n	- output
		3	any	+ control
		4	any	- control
Current Controlled Voltage Source (2 terminal)	H	1	p
		2	n
Current Controlled Voltage Source (4 terminal)	H	1	p	+ output
		2	n	- output
		3	any	+ control
		4	any	- control
Current Source	I	1	p	+
		2	n	-
Diode	D	1	p	Anode
		2	n	Cathode
GaAs FETs	Z	1	d	Drain
		2	g	Gate
		3	s	Source
Inductor	L	1	p
		2	n
Junction FET	J	1	d	Drain
		2	g	Gate
		3	s	Source
MOSFET	M	1	d	Drain
		2	g	Gate
		3	s	Source
		4	s	Bulk
Resistors	R	1	p
Transmission Line	T (lossless)	1	p1	Port 1 Term 1
		2	n1	Port 1 Term 2
	O (lossy)	3	p2	Port 2 Term 1
		4	n2	Port 2 Term 2
Voltage Controlled Current Source	G	1	p	+ output
		2	n	- output
		3	cp	+ control
		4	cn	- control
Voltage Controlled Switch	S	1	p	Switch term 1
		2	n	Switch term 2
		3	cp	+ control
		4	cn	- control
Voltage Controlled Voltage Source	E	1	p	+ output
		2	n	- output
		3	cp	+ control
		4	cn	- control
Voltage Source	V	1	p	+ output
		2	n	- output
Subcircuits	X	Pins can be given any name. Numbering must be in the order that pins appear in the .subckt control which defines the subcircuit. SIMetrix uses a special extension of the netlist format to tell the simulator what the pin names are.
Verilog-A device	U (recommended)	Pin count, names and order must match ports in Verilog module statement. See Verilog-A User Manual for details.
VSXA (Verilog-HDL device)	U	Pin count, names and order must match ports in Verilog module statement. See VSXA device in the Simulator Reference Manual.
AC Table Lookup	U	Pin count = 2 x number of ports. This device does not currently provide current readback. Pin names can thus be assigned arbitrarily.

◄ Using Schematic Editor for CMOS IC Design

Creating Schematic Symbols - Overview ▶