This dialog box allows you to construct the symbol to be associated with the component. At least one symbol must be associated with each component. The symbols are used to represent the components in the wiring diagrams.
Define the symbol
Electrical symbols are groupings of objects that include one or more Pin objects. They are inserted in the document as Symbol objects and are defined and exported through the Frame objects.
Internal symbols
For components that have specific features, you need to draw a special symbol to represent them in the schematics. In this case, the symbol can be defined in the same library in which the component is defined. The symbols are defined in the wiring diagram documents. See To create a library of electrical symbols.
External symbols
For components that have common functionalities, the same symbol can be used to represent them in the schematics. In this case, a symbol defined in an external symbol library can be used. For example, the NPN symbol can be used for a transistor, and the SW-SPST symbol can be used for a switch, both defined in a different library from the one in which the component is defined. The external libraries used must be declared in the Job Properties » Libraries dialog box.
Associating the symbol to a single component
Individual components are components that contain a single functional unit. The symbol of these components represents the entire component. An example of this type of components are resistors, transistors, capacitors and integrated circuits type 74LS138 and 74HC4060.
For this type of component, simply specify the name of the symbol in the Name box.
If the symbol has several shapes, you can also specify the shape by separating it from the name with the character $. For example: LED$RED activates the RED shape of the LED symbol.
You can also specify the name of the page where the symbol is contained. Use the @ character to separate the page name from the symbol name. For example: LED$RED@LEDS activates the RED shape of the LED symbol defined in the LEDS page.
If the symbol is internal
Draw the symbol. See Draw symbols of individual components.
Do one of the following:
Specify the symbol name in the Name box.
Scroll through the tree structure and select the symbol then click the Set symbol button.
If the symbol is external
Click the Open library button. The dialog box for selecting the file opens.
In the dialog box, select the library where the symbol is present and click on Open. The library is opened.
Scroll through the tree structure and select the symbol then click the Set symbol button.
Associating the symbol with a multi-part component
Multi-part components are components that contain multiple functional units of the same type. For example, component 74HC00 contains four two-input NAND ports. It is possible to represent this component with a single symbol, but in many cases it is more convenient to draw the four NAND ports separately so that each door can be positioned independently of the others at any point in the schematic.
For this type of components you can perform one of the following procedures:
Draw a multi-part symbol as described in Draw symbols of multi-part components and specify the symbol name in the Name box.
Construct the multi-part symbol from a simple symbol and specifying the number of parts that make up the component. For example, to construct the complete symbol of component 74HC00 you can use the symbol of a two-input NAND port and specify the number of parts that make up the component. Do the following:
Click the Open library button. The dialog box for selecting the library file opens.
In the dialog box, select the "Logic" symbol library and click the Open button. The library is opened.
Scroll through the tree structure and select the symbol "NAND_2INP" then click on the button Add section. A new section is added.
In the section line, click on the Parts box and set 4 parts.
In the section line, click on the Index box and choose Prefix. If you choose Prefix, the pin names are prefixed with the index of the part.
In the Name box, specify a name for the symbol.
Click on OK.
Associating the symbol with a multifunctional component
Multifunctional components are components that contain several different functional units. For example, component 74HC7075 contains two inverters, two NAND ports with two inputs and two D-type flip-flops. It is possible to represent this component with a single symbol but in many cases it is more convenient to be able to draw the individual parts separately so as to be able to position each port independently of the others at any point of the schematic.
For this type of components you can perform one of the following procedures:
Draw a multi-functional symbol as described in Draw multi-functional component symbols and specify the symbol name in the Name box.
Construct the multifunctional symbol by specifying the symbols of the different functional blocks that make up the component. For example, to construct the complete symbol for component 74HC7075, do the following:
Click the Open library button. The dialog box for selecting the library file opens.
In the dialog box, select the "Logic" symbol library and click the Open button. The library is opened.
Scroll through the tree structure and select the "INVERTER" symbol then click on the Add section button. A new section is added.
In the section line: click on the Parts box and set 2 parts; click on the Index box and choose Prefix. If you choose Prefix, the pin names are prefixed with the index of the part.
Scroll through the tree structure and select the symbol "NAND_2INP" then click on the button Add section. A new section is added.
In the section line: click on the Parts box and set 1 part; click on the Index box and choose Prefix. If you choose Prefix, the pin names are prefixed with the index of the part.
Scroll through the tree structure and select the symbol "DFF_CPQNQ" then click on the button Add section. A new section is added.
In the section line: click on the Parts box and set 2 parts; click on the Index box and choose Prefix. If you choose Prefix, the pin names are prefixed with the index of the part.
Scroll through the tree structure and select the symbol "NAND_2INP" then click on the button Add section. A new section is added.
In the section line: click on the Parts box and set 1 part; click on the Index box and choose Prefix. If you choose Prefix, the pin names are prefixed with the index of the part.
In the Name box, specify a name for the symbol.
Click on OK.