Per piazzare un simbolo nello schema elettrico si può usare il pulsante o il tasto A. Appare la finestra di dialogo Scegli simboli che consente di scegliere il simbolo da aggiungere. I simboli sono raggruppati per libreria.

By default, only the symbol/library name and description columns are shown. Additional columns can be added by right-clicking the column header and selecting Select Columns.

La finestra di dialogo di scelta del simbolo filtrerà i simboli per nome, parolechiave, descrizione e tutti i campi simbolo aggiuntivi, a seconda di quanto si inserirà nel campo di ricerca.

Alcuni filtri avanzati sono disponibili:

Se il simbolo specifica un’impronta predefinita, questa verrà visualizzata in anteprima in basso a destra. Se il simbolo include filtri impronta, è possibile selezionare impronte alternative che soddisfano i filtri impronta nel menu impronta a discesa a destra.

Dopo aver selezionato un simbolo da posizionare, il simbolo verrà attaccato al cursore. Facendo clic con il pulsante sinistro del mouse sulla posizione desiderata nello schema, il simbolo viene inserito nello schema. Prima di posizionare il simbolo nello schema elettrico, è possibile ruotarlo, renderlo speculare e modificarne i campi, usando i tasti comando o il menu contestuale del tasto destro. Queste azioni possono essere eseguite anche dopo il posizionamento.

Se l’opzione Posiziona copie ripetute è selezionata, dopo aver posizionato un simbolo, KiCad inizierà a posizionare un’altra copia del simbolo. Questo processo continua finché l’utente non preme Esc.

Per i simboli con più unità, se l’opzione Posiziona tutte le unità è selezionata, dopo aver posizionato il simbolo KiCad inizierà a posizionare l’unità successiva nel simbolo. Ciò continuerà fino a quando l’ultima unità sarà stata posizionata o sino a quando l’utente premerà Esc.

Un simbolo di potenza è un simbolo che rappresenta una connessione a un collegamento di potenza (N.d.T. come un’alimentazione). I simboli sono raggruppati nella libreria power, quindi possono essere posizionati utilizzando il selettore simboli. Tuttavia, poiché i posizionamenti di simboli potenza sono frequenti, è disponibile lo strumento . Questo strumento è simile, tranne per il fatto che la ricerca viene eseguita direttamente nella libreria power e in qualsiasi altra libreria che contenga simboli di potenza.

I simboli possono essere spostati utilizzando gli strumenti Sposta (M) o Trascina (G). Questi strumenti agiscono sul simbolo selezionato, oppure se nessun simbolo fosse stato selezionato, agiscono sul simbolo sotto il cursore.

Lo strumento Sposta sposta il simbolo stesso senza mantenere connessioni cablate ai piedini del simbolo.

Lo strumento Trascina sposta il simbolo senza interrompere le connessioni cablate ai suoi piedini, e quindi sposta anche i fili collegati.

You can also Drag symbols by clicking and dragging them with the mouse, depending on the Left button drag gesture setting in the Mouse and Touchpad section of Preferences.< Si può anche trascinare i simboli facendo clic e trascinandoli con il mouse, a seconda dell’impostazione Gesture trascinamento del pulsante sinistro nella sezione Mouse e touchpad delle Preferenze.

Symbols can also be rotated (R) or mirrored in the X (X) or Y (Y) directions.

A symbol’s fields can be edited in the symbol’s Properties window. Open the Symbol Properties window for a symbol with the E hotkey or by double-clicking on the symbol.

The Symbol Properties window displays all the fields of a symbol in a table. New fields can be added, and existing fields can be deleted, edited, reordered, moved, or resized.

Il nome e il valore di ciascun campo possono essere visibili o nascosti e sono disponibili diverse opzioni di formattazione: allineamento orizzontale e verticale, orientamento, posizione, carattere, colore del testo, dimensione del testo ed enfasi in grassetto/corsivo. Il posizionamento automatico del campo può anche essere abilitato in base al campo. La posizione visualizzata è sempre indicata per un simbolo visualizzato normalmente (nessuna rotazione o specularità) ed è relativa al punto di ancoraggio del simbolo.

The Update Symbol from Library…​ button is used to update the schematic’s copy of the symbol to match the copy in the library. The Change Symbol…​ button is used to swap the current symbol to a different symbol in the library. These functions are described later.

Edit Symbol…​ opens the Symbol Editor to edit the copy of the symbol in the schematic. Note that the original symbol in the library will not be modified. The Edit Library Symbol…​ button opens the Symbol Editor to edit the original symbol in the library. In this case, the symbol in the schematic will not be modified until the user clicks the Update Symbol from Library…​ button.

Symbols have several attributes that affect how the symbols are treated by other parts of KiCad.

Exclude from simulation prevents the symbol from being included in SPICE simulations.

Exclude from bill of materials prevents the component from being included in BOM exports.

Exclude from board means that the symbol is schematic-only, and a corresponding footprint will not be added to the PCB.

Do not populate means that the component should not be attached to the PCB, although a corresponding footprint should still be added to the board. DNP symbols appear desaturated and with a red "X" over them in the schematic, as shown below.

When a symbol is added to the schematic, KiCad embeds a copy of the library symbol in the schematic so that the schematic is independent of the system libraries. Symbols that have been added to the schematic are not automatically updated when the library changes. Library symbol changes are manually synced to the schematic so that the schematic does not change unexpectedly.

To update symbols in the schematic to match the corresponding symbol, use Tools → Update Symbols from Library, or right click a symbol and select Update Symbol from Library. You can also access the tool from the symbol properties dialog.

The top of the dialog has options to choose which symbols will be updated. You can update all symbols in the dialog, update only the selected symbols, or update only the symbols that match a specific reference designator, value, or library identifier. The reference designator and value fields support wildcards: * matches any number of any characters, including none, and ? matches any single character.

The middle of the dialog has options to control what parts of the symbol will be updated. You can select specific fields to update or not update, which properties of the fields to update (text, visibility, size and style, and position), and how to handle fields that are missing or empty in the library symbol. You can also choose whether to update symbol attributes, such as do not populate and exclude from simulation / bill of materials / board.

The bottom of the dialog displays messages describing the update actions that have been performed.

To change an existing symbol to a different symbol, use Edit → Change Symbols…​, or right click an existing symbol and select Change Symbol…​. This dialog is also accessible from the symbol properties dialog.

The options for the Change Symbols dialog are very similar to the Update Symbols from Library dialog.

Another way to swap existing symbols for new ones is to use Tools → Edit Symbol Library Links…​. This dialog contains a table of every symbol in the design, grouped by current library symbol. By choosing a new symbol in the New Library Reference column, you can make all instances of the existing symbol instead point to the new symbol. If the Update symbol fields from new library option is used, the contents of the existing symbols' fields will be updated to match the new symbols' fields.

The Map Orphans button attempts to automatically remap orphaned symbols to symbols with the same name in an active library. For example, if there is a symbol with the current library reference mylib:symbol123, but the mylib library cannot be found, the Map Orphans button will attempt to find a symbol named symbol123 in any of the libraries that are present. This button is only enabled if orphaned symbols are present in the schematic (see the legacy schematics section).

This dialog is primarily useful for managing symbols that appear in multiple libraries, when you want to switch from one library to another. For example, if a schematic uses symbols that are in both a global library and a project-specific library, the Symbol Library References dialog could be used to switch between using the global symbols or the equivalent project-specific symbols. It does not have features for fine-grained control of how fields are updated; for that, use the Change Symbols dialog.

The Symbol Fields Table allows you to view and modify field values for all symbols in a spreadsheet interface. You can open the Symbol Fields Table with the button.

Cells are navigated with the arrow keys, or with Tab / Shift+Tab to move right / left and Enter / Shift+Enter to move down / up, respectively.

A range of cells can be selected by clicking and dragging. The whole range of selected cells will be copied (Ctrl+C) or pasted into (Ctrl+V) on a copy or paste action. Copying a range of cells from the table can be useful for creating a BOM. More details of copying and pasting cells are described below.

Any symbol field can be shown or hidden using the Show checkboxes on the left, or by right-clicking on the header of the table. New symbol fields can be added using the Add Field…​ button.

Similar symbols can optionally be grouped by any symbol field using the Group By checkboxes. Grouped symbols are shown in a single row in the table. The grouped row can be expanded to show the individual symbols by clicking the arrow at the left of the row. The Group Symbols checkbox enables or disables symbol grouping, and the button recalculates groupings.

Symbols can be filtered using the Filter textbox at the top. The filter supports wildcards: * matches any number of any characters, including none, and ? matches any single character.

You can use the Export as CSV…​ button to save the symbol fields to an external file. This can be used as a simple BOM generation tool, although the BOM tool provides better control over the generated output.

When auto-annotation is enabled, symbols will be automatically annotated when they are added to the schematic. You can enable auto-annotation by checking the Automatically annotate symbols checkbox in the Schematic Editor → Annotation Options pane in Preferences. Auto-annotation can also be toggled using the button in the left toolbar.

When multiple symbols are added simultaneously, they are annotated according to the Order setting, sorted by either X or Y position.

The Numbering option sets the starting number for new reference designators. This can be the lowest available number, or a number based on the sheet number.

For more information about annotation options, see the documentation for the Annotation tool.

Lo strumento di annotazione assegna automaticamente i riferimenti a simboli nello schema. Per eseguire lo strumento di annotazione fare clic sull’icona nella barra strumenti in alto.

The tool provides several options to control how symbols are annotated.

Scope: Selects whether annotation is applied to the entire schematic, to only the current sheet, or to only the selected symbols. If the Recurse into subsheets option is selected, symbols in subsheets of the selected scope will be reannotated; otherwise symbols in subsheets will not be reannotated. For example, if Recurse into subsheets and Selection only selected, symbols in any selected subsheets will be reannotated.

Options: Selects whether annotation should apply to all symbols and reset *existing reference designators, or apply only to unannotated symbols.

Order: Chooses the direction of numbering. If symbols are sorted by X position, all symbols on the left side of a schematic sheet will be lower numbered than symbols on the right side of the sheet. If symbols are sorted by Y position, all symbols on the top of a sheet will be lower numbered than symbols at the bottom of the sheet.

Numbering: Selects the starting point for numbering reference designators. The lowest unused number above the starting point is picked for each reference designator. The starting point can be an arbitrary number (typically zero), or it can be the sheet number multiplied by 100 or 1000 so that each part’s reference designator corresponds to the schematic page it is on.

The Clear Annotation button clears all reference designators in the selected scope.

Annotation messages can be filtered with the checkboxes at the bottom or saved to a report using the Save…​ button.

I fili vengono utilizzati per stabilire direttamente collegamenti elettrici tra due punti. Per stabilire una connessione, un segmento di filo deve essere collegato per la sua estremità a un altro segmento o ad un pin. Solo le estremità dei fili creano connessioni; se un filo attraversa il centro di un altro filo, non verrà effettuata una connessione.

Unconnected wire ends have a small square that indicates the connection point. The square disappears when a connection is made to the wire end. Unconnected pins have a circle, which also disappears when a connection is made.

Labels are used to assign net names to wires and pins. Wires with the same net name are considered to be connected, so labels can be used to make connections without drawing direct wire connections.

Una net può avere un solo nome. Se due etichette diverse vengono posizionate sulla stessa rete, verrà generata una violazione ERC. Nella netlist verrà utilizzato solo uno dei nomi di net. Il nome della net finale è determinato in base alle regole descritte di seguito.

There are three types of labels, each with a different connection scope.

I bus sono un modo per raggruppare segnali in relazione tra loro in uno schema elettrico, in modo da semplificare i progetti complessi. I bus possono essere disegnati come i fili usando lo strumento bus , e i loro nomi vengono assegnati usando le etichette allo stesso modo di come si fa con i fili dei segnali.

Nello schema elettrico seguente, molti piedini sono connessi a dei bus, cioè le linee spesse blu al centro.

When the power pins of a symbol are visible, they must be connected, as with any other signal. However, symbols such as gates and flip-flops are sometimes drawn with hidden power input pins which are connected implicitly.

KiCad automatically connects invisible pins with type "power input" to a global net with the same name as the pin. For example, if a symbol has a hidden power input pin named VCC, this pin will be globally connected to the VCC net on all sheets.

It may be necessary to join power nets of different names (for example, GND in TTL components and VSS in MOS components). To accomplish this, add a power symbol for each net and connect them with a wire.

Se vengono usati pin di potenza nascosti, non è raccomandabile usare etichette locali per le connessioni di potenza, dato che queste ultime non connetterebbero i piedini di potenza nascosti su altri fogli.

Power symbols are symbols that are conventionally used to represent a connection to a power net, such as VCC or GND. In addition to being a visual indicator that the attached net is a power rail, power symbols make global connections: two power symbols with the same pin name connect to each other anywhere in the schematic, regardless of sheet.

Power symbols are virtual: they do not represent a physical component on the PCB.

In the figure below, power symbols are used to connect the positive and negative terminals of the capacitors to the VCC and GND nets, respectively.

In the KiCad standard library, power symbols are found in the power library, but power symbols can be created in any library.

To create a custom power symbol, make a new symbol with a power input pin that is set to be invisible. Name the pin according to the desired power net. In addition, set the "Define as power symbol" symbol property. As described in the hidden power pins section, invisible power input pins make global connections based on the hidden power pin’s name. The process of creating a power symbol is described in more detail in the Symbol Editor section.

Every net in the schematic is assigned a name, whether that name is specified by the user or automatically generated by KiCad.

When multiple labels are attached to the same net, the final net name is determined in the following order, from highest priority to lowest:

If there are multiple labels of one type attached to a net, the names are sorted alphabetically and the first is used.

If a net travels through multiple sheets of a hierarchy, it will take its name from the highest level of the hierarchy where it has a hierarchical label or local label. As usual, local labels take priority over hierarchical labels.

If none of the label types above are attached to a net, the net’s name is automatically generated based on the connected symbol pins.

Due simboli PWR_FLAG sono visibili nella schermata soprastante. Essi indicano all’ERC che le due net di potenza VCC e GND sono effettivamente connesse ad una sorgente di potenza, dato che non c’è una sorgente di potenza esplicita come l’uscita di un regolatore di tensione collegata a nessuno dei due collegamenti.

Without these two flags, the ERC tool would diagnose: Error: Input Power pin not driven by any Output Power pins.

The PWR_FLAG symbol is found in the power symbol library. The same effect can be achieved by connecting any power output pin to the net.

No-connection flags () are used to indicate that a pin is intentionally unconnected. These flags prevent "unconnected pin" ERC warnings for pins that are intentionally unconnected.

Note that no-connection flags are distinct from the "unconnected" symbol pin type, although they both prevent "unconnected pin" ERC warnings on the pin in question.

Netclasses are managed in the Net Classes panel of the Schematic Setup dialog.

The top pane lists the netclasses that exist in the design. The Default netclass always exists, and you can add additional netclasses with the button or remove the selected netclass with the button.

Each netclass can have unique graphic properties that determine how wires of that netclass are displayed in the schematic. Wire and bus thicknesses, color, and line style (solid, dashed, dotted, etc.) can all be adjusted. Setting the color to transparent will use the theme’s default wire/bus color for the netclass, which is configurable in Preferences.

You can also set board design rules for each netclass, although the DRC fields are hidden by default. Right click the header row to show or hide additional columns. For more information about setting netclass design rules, see the PCB editor documentation.

The bottom pane lists pattern-based netclass assignments. Each row has a net name pattern and a netclass; nets with names that match the pattern are assigned to the specified netclass. If a net matches multiple patterns, the first match is used. Pattern-based netclass assignments are dynamic: when a new net is added that matches an existing pattern, it will be assigned to the associated netclass automatically. Net patterns can use both wildcards (* to match any number of any characters, including none, and ? to match any character) and regular expressions. The nets that match the selected pattern are displayed to the right of the pattern list.

For example, the net* pattern matches nets named net, net1, network, and any other net name beginning with net. Because * has a slightly different meaning in a regular expression (* matches zero or more of the preceding character), the net* pattern would also match a net named ne.

Use the button to add a net class assignment pattern or the button to remove a pattern.

Instead of adding netclass patterns in the Schematic Setup dialog, you can directly create netclass patterns from the schematic canvas. Right click a net and select Assign Netclass…​ to bring up the Add Netclass Assignment dialog. The netclass pattern is pre-filled with the name of the selected net, but the pattern can be changed if desired. All nets matching the pattern are displayed in the dialog.

As an alternative to pattern-based netclass assignment, netclasses can be graphically assigned to nets in the schematic using either net class directives or labels. Netclasses must be created in Schematic Setup before they can be assigned graphically.

In the image below, a net class directive is used to assign signals to the 50R netclass.

Net class directives are added with the button in the right toolbar. They behave like labels, except that they cannot be used to name a net. The attached net is assigned a netclass according to the value of the directive’s Net Class field. The Net Class field presents a dropdown list of all the net classes in the design.

If a directive is attached to a bus, all members of the bus are assigned to the specified net class.

In addition to the associated netclass, you can edit the directive’s shape (dot, circle, diamond, or rectangle), orientation, pin length, and color in the directive’s properties.

Net labels can also be used to assign netclasses to nets by adding a Net Class field to the label.

If more than one different netclass is graphically assigned to a single net, ERC will report an issue. Graphical netclass assignments override pattern-based assignments: if a net matches a netclass pattern assignment and also has a netclass assigned graphically, the graphically assigned netclass will be used.

Two kinds of text can be added to schematics, which are referred to as text () and text boxes (). Both are added using their respective buttons in the right toolbar.

Both kinds of text item support multiline text and basic formatting features, but text boxes wrap text to fit in the outline and have additional formatting options. All text has adjustable fonts, color, size, bold and italic emphasis, left and right alignment, and vertical and horizontal orientation. Text boxes additionally support horizontal centering, vertical alignment options, and colored borders and fill.

Graphic rectangles (), circles (), arcs (), and lines () can all be added using their respective buttons in the right toolbar.

Line width, color, and style (solid, dashed, or dotted) can be configured in the properties dialog for each shape (E). Rectangles, circles, and arcs can also have a fill color set and have their outlines removed.

Setting a shape’s line width to 0 uses the schematic default line width, which is configurable in Schematic Setup. Spacing for line dashes is also configurable there. Removing a line or fill color uses the color theme’s graphics color, which is configurable in Preferences.

Like wires, graphic lines obey the line drawing mode setting (90 degree, 45 degree, or free angle), which you can set using the toggle buttons on the left toolbar (, , and , respectively). Shift+Space cycles through the modes.

As with PCB tracks, the / hotkey switches line posture.

Bitmap images can be added to the schematic with the button. Images in the schematic can be moved and scaled. The properties dialog allows setting a location and scale as well as converting the image to greyscale.

Properties of text and graphics can be edited in bulk using the Edit Text and Graphic Properties dialog (Tools → Edit Text and Graphic Properties…​). The tool can also modify visual properties of wires and buses.

Il riquadro iscrizioni viene modificato con lo strumento per le inpostazioni pagina ().

Each field in the title block can be edited, as well as the paper size and orientation. If the Export to other sheets option is checked for a field, that field will be updated in the title block of all sheets, rather than only the current sheet.

You can set the date to today’s or any other date by pressing the left arrow button next to Issue Date. Note that the date in the schematic will not be automatically updated.

A drawing sheet template file can also be selected.

The sheet number (Sheet X/Y) is automatically updated, but sheet page numbers can also be manually set using Edit → Edit Sheet Page Number…​.

The formatting panel contains settings for the appearance of symbols, text, labels, graphics, and wires.

Symbol unit notation sets how each unit of a multi-unit symbol is referred to in its reference designator. By default, a different letter for each unit is appended to the reference designator with no separator, for example U1B for the second unit of symbol U1, but this can be changed. Numbers can be used instead of letters, and various separators can be used between the symbol designator and the unit identifier (., -, _, or none).

Default text size sets the default text height used by the text, text box, and label tools. Label offset ratio controls the vertical spacing between a local label’s text and the attached wire, relative to the label’s text size. This also affects the spacing between symbol pins and their pin number. Global label margin defines the size of the box around a global label, relative to the global label’s text size. Increasing the margin may be useful to avoid overlapping text with overbars (~{}) or letters with descenders, but this may cause closely packed global labels to overlap with each other.

Default line width sets the default line width for symbol graphics, if the symbol does not override the default line width. Pin symbol size scales symbol pin graphic style annotations, such as the bubble on an inverted pin.

Junction dot size sets the schematic’s default wire junction dot size. The default size can be overridden by editing an individual junction dot’s properties.

Show inter-sheet references enables or disables the display of inter-sheet references, which are a list of page numbers next to a global labels that link to other places in the schematic where the same global label appears. Show own page reference controls whether the current page is included in the list of page numbers. Standard and abbreviated determine whether to display the complete list of page numbers or only the first and last page numbers. The prefix and suffix fields add optional characters before and after the list of page numbers. In the image of an inter-sheet reference below, a prefix and suffix of [ and ], respectively, have been added.

Dashed line appearance is controlled in the Formatting section. Dash length controls the length of dashes, while Gap length controls the spacing between dashes and dots. The dash and gap lengths are relative to the line width: a gap length of 2 means twice the width of the line.

Field name templates are empty symbol fields that are automatically added to all symbols in the schematic. These can be useful when every symbol in the schematic needs additional fields beyond the fields that are defined in the library symbols, for example a field for the manufacturer’s part number.

Template fields can be set as visible or invisible, and can also be set as URL fields.

Field name templates that are defined in schematic setup apply only to the current project. Field name templates can also be defined in Preferences, which apply to all projects edited on your computer.

The Violation Severity panel lets you configure what types of ERC messages should be reported as Errors, Warnings, or ignored.

The Pin Conflicts Map allows you to configure connectivity rules to define electrical conditions for errors and warnings based on what types of pins are connected to each other. For example, by default an error is produced when an output pin is connected to another output pin.

These panels are explained in more detail in the ERC section.

The Net Classes panel allows you to manage netclasses for the project and assign nets to netclasses with patterns. Managing netclasses in this panel is equivalent to managing them in the Board Setup dialog. Nets can also be assigned to netclasses in the schematic using graphical assignments with net class directives or net labels.

Pattern-based netclass assigment is explained in more detail in the net classes section.

The Bus Alias Definitions panel allows you to create bus aliases, which are names for groups of signals in a bus. For more information about bus aliases, see the bus alias documentation.

Text replacement variables can be created in the Text Variables section. These variables allow you to substitute the variable name for any text string. This substitution happens anywhere the variable name is used inside the variable replacement syntax of ${VARIABLENAME}.

For example, you could create a variable named VERSION and set the text substitution to 1.0. Now, in any text object on the PCB, you can enter ${VERSION} and KiCad will substitute 1.0. If you change the substitution to 2.0, every text object that includes ${VERSION} will be updated automatically. You can also mix regular text and variables. For example, you can create a text object with the text Version: ${VERSION} which will be substituted as Version: 1.0.

Text variables can also be created in Board Setup. Text variables are project-wide; variables created in the schematic editor are also available in the board editor, and vice versa.

There are also a number of built-in system text variables.

Modern versions of KiCad can open schematics created in versions prior to KiCad 6.0, but the cache library file (<projectname>-cache.lib) must be present to load the schematic correctly.

Since version 6.0, KiCad stores all symbols used in a project in the schematic. This means that you can open a schematic made in KiCad 6.0 or later on any computer, even if the libraries used in the project are not installed or have changed. Modern KiCad schematic files use the .kicad_sch extension.

Prior to version 6.0, KiCad did not store symbols in the schematic. Instead, KiCad stored references to the symbols and their libraries. It also stored a copy of every symbol used by the project in a separate cache library file (<projectname>-cache.lib). As long as the cache library was included with the project, the project could be distributed without the system library files, because KiCad could load any needed symbols from the cache library as a fallback if the libraries referenced in the schematic were missing. Legacy KiCad schematic files use the .sch extension.

When you open a legacy schematic, KiCad will look in the cache library to find all of the symbols used in the schematic in the cache library. When you save the legacy schematic, KiCad will save it as a new file in the modern schematic format (.kicad_sch), with the necessary symbols embedded in the schematic itself. The original legacy schematic and the cache library will remain, unmodified, but they are no longer necessary once the schematic has been saved in the modern format.

When you open a legacy schematic, KiCad may display the Project Rescue Helper dialog. This means that one or more symbols in the cache library do not match the corresponding symbol in the external library. The dialog helps you "rescue" symbols from the cache library into your schematic, if desired. You can also open the rescue dialog at any time using Tools → Rescue Symbols…​. The cache library file must be present in order to use the rescue tool.

The rescue dialog lists all symbols that don’t match between the cache library and the external symbol library. The discrepancy can be because:

For each symbol in the list, selecting the symbol displays the reference designator and value for each instance of the symbol, and shows a visual preview of the symbol. If a corresponding symbol exists in the system symbol library, the dialog shows both copies of the symbol for comparison. If the symbol only exists in the cache library, the dialog only shows the cached symbol.

In this example, the project originally used a diode with the cathode facing left, but the library now contains one with the cathode facing right. This change would break the design, so it would be important to use the cached symbol as the original designer intended.

Pressing Rescue Symbols here will cause the selected symbols from the cache library to be saved into a special rescue library (<projectname>-rescue.kicad_sym). The corresponding symbols in the schematic will be updated to use the newly rescued symbols. Any unselected symbols will not be rescued, but their symbol linkage can be updated in the schematic later.

Alternatively, pressing Skip Symbol Rescue will exit the dialog without rescuing any symbols. KiCad will use the versions of the symbols found in the external libraries. You can run the rescue function again with Tools → Rescue Symbols…​, or manually edit symbol linkage in the symbol’s properties.

If you would prefer not to see this dialog, you can press Never Show Again. This has the same effect as pressing Skip Symbol Rescue for the current schematic and all future schematics.

If a symbol in a legacy schematic cannot be found in either the cache library or the external library, KiCad cannot rescue that symbol. A placeholder symbol is inserted into the schematic in its place, as shown below.

You can attempt to remap these orphaned symbols using the Change Symbols or Edit Symbol Library Links dialogs, but either option may require manual corrections to the schematic. These tools are explained in more detail in the Updating and exchanging symbols section.

Modern versions of KiCad can open schematics created in versions prior to KiCad 5.0, but you will need to go through a symbol remapping process to open the schematic without losing symbol information.

Since version 5.0, KiCad schematics refer to specific symbols using both the symbol and library name. Even if multiple libraries each contain a symbol with the same name, the designer’s intended symbol is unambiguously specified.

Prior to version 5.0, KiCad schematics stored only the symbol name, not the library name. Symbols in the schematic were indirectly mapped back to the original library by searching through the project’s library list for a matching symbol. When you open a pre-5.0 schematic, KiCad will attempt to automatically "remap" the symbols so that each bare symbol name is replaced with a fully-specified symbol library and symbol name pair. The original schematics will be backed up in a rescue-backup folder.

You can skip the automatic remapping, but you will need to remap the symbols yourself using the Change Symbols dialog. You can also re-run the Remap Symbols tool using Tools → Remap Legacy Library Symbols…​.

Electrical connections between sheets are made with labels. There are several kinds of labels in KiCad, each with a different connection scope.

After placing hierarchical labels within the subsheet, matching hierarchical pins can be added to the subsheet symbol in the parent sheet. You can then make connections to the hierarchical pins with wires, labels, and buses. Hierarchical pins in a subsheet symbol are connected to the matching hierarchical labels in the subsheet itself.

Per ogni etichetta gerarchica nel sottofoglio, importare il pin gerarchico corrispondente nel simbolo del foglio facendo clic sul pulsante nella barra degli strumenti a destra, quindi facendo clic sul simbolo del foglio. Un segnaposto per la prima etichetta gerarchica senza corrispondenza verrà attaccato al puntatore, dove può essere posizionato ovunque lungo il bordo del simbolo del foglio. Facendo nuovamente clic con lo strumento si continuerà ad importare ulteriori pin del foglio fino a quando non ci saranno più pin gerarchici da importare dal sottofoglio. I pin foglio possono essere importati anche selezionando Importa pin fogli nel menu contestuale del simbolo del foglio.

You can edit the properties of a sheet pin in the Sheet Pin Properties dialog. Open this dialog by double-clicking a sheet pin, selecting a sheet pin and using the E hotkey, or right-clicking a sheet pin and selecting Properties…​.

The sheet pin’s name can be edited in the textbox or by selecting from the dropdown list of hierarchical labels in the subsheet. A sheet pin’s name has to match the corresponding hierarchical label in the subsheet, so if a pin name is changed the label must change as well.

Shape changes the shape of the sheet pin, and has no electrical effect. It can be set to Input, Output, Bidirectional, Tri-state, or Passive. The pin’s font, text size, color, and emphasis (bold or italic) can also be changed.

An example of a simple hierarchy is the video demo project included with KiCad. The root sheet contains seven unique subsheets, each with hierarchical labels and sheet pins linking the sheets to each other in the root sheet. Two of the subsheet symbols are shown below.

The complex_hierarchy demo project is an example of a complex hierarchy. The root sheet contains two subsheet symbols, which both refer to the same sheet file (ampli_ht.kicad_sch). This allows the design to include two copies of the same amplifier circuit. Although the two sheet symbols refer to the same filename, the sheet names are unique (ampli_ht_vertical and ampli_ht_horizontal). Inside each subsheet the circuits are identical except for the reference designators, which as always are unique.

This project contains no sheet pin connections. The only connections between the root sheet and the subsheets are global power connections made with power symbols. However, sheets in a complex hierarchy could include sheet pin connections if appropriate for the design.

The flat_hierarchy demo project is an example of a flat hierarchy. The root sheet contains two unique subsheet symbols with no hierarchical sheet pins. The root sheet in this project does nothing except hold the subsheets, and the subsheets are used only as additional pages in the schematic.

There are three errors in the screenshot above.

Selecting an ERC marker displays a description of the violation in the message pane at the bottom of the window.

It is common to have an "Input Power pin not driven by any Output Power pins" error on power pins, as shown in the example below, even though the power pins seem to be properly connected to a power rail. This happens in designs where the power is provided through connectors or other components that are not marked as power outputs. In these cases ERC won’t detect any Output Power pins connected to the net and will determine the Input Power pin is not driven by a power source.

To avoid this warning, connect the net to PWR_FLAG symbol on such a power net as shown in the following example. The PWR_FLAG symbol is found in the power symbol library. Alternatively, connect any power output pin to the net; PWR_FLAG is simply a symbol with a single power output pin.

Le reti di massa spesso necessitano anche di un PWR_FLAG, poiché i regolatori di tensione hanno uscite dichiarate come uscite di potenza, ma i loro pin di massa sono tipicamente contrassegnati come ingressi di alimentazione. Pertanto le masse possono apparire non collegate a una fonte a meno che non venga utilizzato un simbolo PWR_FLAG.

For more information about power pins and power flags, see the PWR_FLAG documentation.

Il pannello Importanza violazione nella Impostazione dello schema permette di configurare che tipo di messaggi ERC devono essere riportati come errori, come semplici avvertimenti o ignorati.

Il pannello Mappa conflitti pin nelle Impostazioni dello schema, permette di configurare le regole di connessione per definire le condizioni elettriche per il controllo di errori e avvertimenti in base al tipo di pin connesso uno con l’altro. Ad esempio, per impostazione predefinita viene prodotto un errore quando un pin di uscita è collegato a un altro pin di uscita.

Le regole si possono cambiare facendo clic sul riquadro desiderato della matrice, in modo ciclare la scelta desiderata: normale, avvertimento, errore.

The table below lists the electrical rules that KiCad checks and the default violation severity for each check. All severities are configurable.

Un file di rapporto ERC può essere generato e salvato facendo clic sul pulsante Salva…​ nella finestra di dialogo ERC. L’estensione file per i file rapporto ERC è .rpt. Ecco un file rapporto ERC di esempio.

Anziché modificare singolarmente le proprietà di ciascun simbolo, è possibile utilizzare la Tabella campi simbolo per visualizzare e modificare le proprietà di tutti i simboli nel disegno da un unico posto. Ciò include l’assegnazione di impronte modificando il campo Impronta di ciascun simbolo.

La tabella campi simbolo è accessibile tramite Strumenti → Modifica i campi del simbolo…​, o con il pulsante nella barra in alto.

Il campo Impronta qui si comporta come nella finestra delle proprietà del simbolo: può essere modificato direttamente o le impronte possono essere selezionate visivamente con l’Esploratore librerie di impronte.

Per ulteriori informazioni sulla tabella dei campi dei simboli, vedere la sezione modifica proprietà simboli.

L’immagine sottostante mostra la finestra principale dello strumento assegnamento impronte.

La barra superiore contiene i seguenti comandi:

La seguente tabella elenca i comandi da tastiera per l’assegnamento impronte.

Per associare manualmente una impronta ad un componente, bisogna prima selezionare un componente nel pannello componenti (centro). Poi selezionare un’impronta nel pannello delle impronte (destra) facendo doppio clic con il pulsante sinistro del mouse sul nome dell’impronta desiderata. L’impronta verrà assegnata al componente selezionato, ed il prossimo componente senza un’impronta assegnata verrà automaticamente selezionato.

Quando a tutti i componenti sono state assegnate impronte, fare clic sul pulsante OK per salvare le assegnazioni e uscire dallo strumento. In alternativa, fare clic su Annulla per eliminare le assegnazioni aggiornate o su Applica, salva schema e continua per salvare le nuove assegnazioni senza uscire dallo strumento.

Lo strumento di assegnazione impronte consente di memorizzare le assegnazioni delle impronte in un file esterno e di caricare le assegnazioni in un secondo momento, anche in un progetto diverso. Ciò consente di associare automaticamente i simboli alle impronte appropriate.

Il file esterno viene definito come un file di equivalenza e memorizza una mappatura di un simbolo ad un’impronta corrispondente. I file di equivalenza in genere utilizzano l’estensione di file .equ. I file di equivalenza sono file di testo semplice con una sintassi semplice e devono essere creati dall’utente utilizzando un editor di testo. La sintassi è descritta di seguito.

È possibile selezionare i file di equivalenza da utilizzare facendo clic su Preferenze → Gestisci file associazione impronte nello strumento di assegnazione impronte.

Le variabili ambiente rilevanti sono mostrate nella parte inferiore della finestra. Quando l’opzione percorso Relativo è selezionata, queste variabili ambiente verranno automaticamente utilizzate per creare percorsi ai file di equivalenze selezionati relativi al progetto o alle librerie di impronte.

Una volta che i file di equivalenze desiderati sono stati caricati nell’ordine corretto, l’associazione automatica delle impronte può essere eseguita facendo clic sul pulsante nella barra degli strumenti superiore dello strumento di assegnazione delle impronte.

Tutti i simboli con un valore trovato in un file di equivalenze caricato avranno le loro impronte assegnate automaticamente. Tuttavia, i simboli che hanno già impronte assegnate non verranno aggiornati.

Lo strumento di assegnazione delle impronte contiene un visualizzatore di impronte. Facendo clic sul pulsante nella barra degli strumenti in alto si avvia il visualizzatore di impronte e si mostra l’impronta selezionata.

La barra superiore contiene i seguenti comandi:

La barra strumenti di sinistra contiene i seguenti comandi:

The tool has several options to control its behavior.

The tool has several options to control its behavior.

Select changes can also be synced from the PCB back to the schematic by exporting a CMP file from the PCB editor (File → Export → Footprint Association (.cmp) File…​) and importing it in the Schematic Editor (File → Import → Footprint Assignments…​).

Stampa del foglio di disegno: include la stampa del bordo del foglio e del riquadro iscrizioni nella stampa dello schema.

Modalità d’uscita: stampa lo schema a colori o in bianco e nero.

Print background color: Include the background color in the printed schematic. This option is only enabled if Print in black and white only is disabled.

Use a different color theme for printing: Select a different color scheme for printing than the one selected for display in the Schematic Editor.

Page Setup…​: Opens a page setup dialog for setting paper size and orientation.

Preview: Opens a print preview dialog.

Close: Closes the dialog without printing.

Print: Opens the system print dialog.

Output directory: Specify the location to save plotted files. If this is a relative path, it is created relative to the project directory.

Output Format: Select the format to plot in. Some formats have different options than others.

Page size: Sets the page size to use for the plotted output. This can be set to match the schematic size or to another sheet size.

Plot drawing sheet: Include the drawing sheet border and title block in the printed schematic.

Output mode: Sets the output to color or black and white. Not all output formats support color.

Plot background color: Includes the schematic background color in the plotted output. The background color will not be plotted if the output format does not support color or the output mode is black and white.

Color theme: Selects the color theme to use for the plotted output.

Default line width: Selects the default width for lines without a specified thickness (lines that have thickness set to 0). Lines that have a set thickness will be plotted at that thickness instead.

Position and units: Sets the plotter origin and units. This option only applies for HPGL output.

Pen width: Sets the plotter’s pen width. This option only applies for HPGL output.

Open file after plot: automatically opens the plotted output file when plotting is complete.

I PDF tracciati hanno diverse caratteristiche interattive.

By default, the BOM tool presents three output script options.

Additional generator scripts are installed with KiCad but are not populated in the generator script list by default. The location of these scripts depends on the operating system and may vary based on installation location.

Ulteriori script possono essere aggiunti all’elenco degli script del generatore DIBA facendo clic sul pulsante . Gli script possono essere rimossi facendo clic sul pulsante . Il pulsante apre lo script selezionato in un editor di testo.

For more information on creating and using custom BOM generators, see the advanced documentation.

KiCad offers several additional ways to generate a BOM, although the BOM tool is recommended.

Netlists are exported with the Export Netlist dialog (File→Export→Netlist…​).

KiCad supports exporting netlists in several formats: KiCad, OrcadPCB2, CADSTAR, Spice, and Spice Model. Each format can be selected by selecting the corresponding tab at the top of the window. Some netlist formats have additional options.

Clicking the Export Netlist button prompts for a netlist filename and saves the netlist.

Custom generators for other netlist formats can be added by clicking the Add Generator…​ button. Custom generators are external tools that are called by KiCad, for example Python scripts or XSLT stylesheets. For more information on custom netlist generators, see the section on adding custom netlist generators.

Below is the schematic from the sallen_key project included in KiCad’s simulation demos.

La netlist in formato KiCad per questo schema è la seguente:

In formato Spice, la netlist è la seguente:

The first time the KiCad Schematic Editor is run and the global symbol table file sym-lib-table is not found in the KiCad configuration folder, KiCad will guide the user through setting up a new symbol library table. This process is described above.

Symbol libraries can only be used if they have been added to either the global or project-specific symbol library table.

Aggiungere una libreria facendo clic sul pulsante selezionando una libreria o facendo clic sul pulsante e digitando il percorso di un file di libreria . La libreria selezionata verrà aggiunta alla tabella della libreria attualmente aperta (globale o specifica del progetto). Le librerie possono venir rimosse selezionando le voci della libreria desiderate e facendo clic sul pulsante .

The and buttons move the selected library up and down in the library table. This does not affect the display order of libraries in the Symbol Library Browser, Symbol Editor, or Add Symbol tool.

Libraries can be made inactive by unchecking the Active checkbox in the first column. Inactive libraries are still in the library table but do not appear in any library browsers and are not loaded from disk, which can reduce loading times.

A range of libraries can be selected by clicking the first library in the range and then Shift-clicking the last library in the range.

Each library must have a unique nickname: duplicate library nicknames are not allowed in the same table. However, nicknames can be duplicated between the global and project library tables. Libraries in the project table take precedence over libraries with the same name in the global table.

Gli identificatori di libreria non devono essere correlati al nome file o al percorso della libreria. Il carattere due punti (:) non può essere utilizzato negli identificatori di libreria o nei nomi dei simboli perché viene utilizzato come separatore tra identificatori e simboli.

Each library entry must have a valid path. Paths can be defined as absolute, relative, or by environment variable substitution.

The appropriate library format must be selected in order for the library to be properly read. "KiCad" format is used for KiCad version 6+ libraries (.kicad_sym files), while "Legacy" format is used for libraries from older versions of KiCad (.lib files). Legacy libraries are read-only, but can be migrated to KiCad format libraries using the Migrate Libraries button (see section Migrating Legacy Libraries).

Esiste un campo optionale per la descrizione della voce di libreria. Il campo opzioni non viene usato al momento perciò aggiungere opzioni non ha alcun effetto sul caricamento delle librerie.

Le tabelle delle librerie di simboli supportano la sostituzione delle variabili ambiente, che consente di definire variabili ambiente contenenti percorsi personalizzati in cui sono archiviate le librerie. La sostituzione delle variabili ambiente è supportata usando la sintassi ${ENV_VAR_NAME} nel percorso della libreria dei simboli.

By default, KiCad defines several environment variables which are described in the project manager documentation. Environment variables can be configured in the Preferences → Configure Paths…​ dialog.

Using environment variables in the symbol library tables allows libraries to be relocated without breaking the symbol library tables, so long as the environment variables are updated when the library location changes.

${KIPRJMOD} is a special environment variable that always expands to the absolute path of the current project directory. ${KIPRJMOD} allows libraries to be stored in the project folder without having to use an absolute path in the project library table. This makes it possible to relocate projects without breaking their project library tables.

Le librerie di simboli si possono definire sia globalmente che specificatamente al progetto correntemente caricato. Le librerie di simboli definite nella tabella globale dell’utente sono sempre disponibili e vengono memorizzate nel file sym-lib-table nella cartella di configurazione di KiCad dell’utente. La tabella delle librerie di simboli specifica del progetto è attiva solamente per il file progetto aperto al momento.

Ci sono vantaggi e svantaggi per ogni metodo. Definire tutte le librerie nella tabella globale significa che queste saranno sempre disponibili alla bisogna. Lo svantaggio di ciò è aumenterà che il tempo di caricamento.

Definire tutte le librerie di simboli su base specifica del progetto significa che si avranno solamente le librerie necessarie per quel progetto e ciò diminuirà il tempo di caricamento dei simboli. Lo svantaggio è che sarà sempre necessario ricordarsi di aggiungere ogni libreria di simboli necessaria per ogni progetto.

Uno schema di utilizzo potrebbe essere quello di definire le librerie di uso comune a livello globale e le librerie richieste solo per il progetto nella tabella della libreria specifica del progetto.

Legacy libraries (.lib files) are read-only, but they can be migrated to KiCad version 6 libraries (.kicad_sym). KiCad version 6 libraries cannot be viewed or edited by KiCad versions older than 6.0.0.

Legacy libraries can be converted to KiCad 6 libraries by selecting them in the symbol library table and clicking the Migrate Libraries button. Multiple libraries can be selected and migrated at once by Ctrl-clicking or shift-clicking.

Libraries can also be converted one at a time by opening them in the Symbol Editor and saving them as a new library.

Quando si carica uno schema creato prima dell’implementazione della tabella delle librerie di simboli, KiCad cercherà di rimappare i collegamenti alle librerie di simboli presenti nello schema ai simboli nella tabella librerie appropriati. Il successo di questo processo dipende da diversi fattori:

A symbol is a schematic representation of a component. A symbol is composed of:

Una libreria di simboli è composta da uno o più simboli. Generalmente i simboli sono raggruppati per funzione, tipo e/o produttore.

I simboli possono essere derivati da un altro simbolo nella stessa libreria. I simboli derivati condividono la forma grafica e le definizioni dei pin del simbolo di base, ma possono sovrascrivere i campi delle proprietà del simbolo di base (valore, impronta, filtri impronta, documentazione, descrizione, ecc.). I simboli derivati possono essere utilizzati per definire simboli simili ad una parte di base. Ad esempio, i simboli 74LS00, 74HC00 e 7437 potrebbero essere tutti derivati da un simbolo 7400. Nelle versioni precedenti di KiCad, i simboli derivati erano chiamati alias.

KiCad provides a symbol editing tool that allows you to create libraries, add, delete or transfer symbols between libraries, export symbols to files, and import symbols from files.

In general, the flow for designing a symbol involves:

The Symbol Editor main window is shown below. It consists of three toolbars for quick access to common features and a symbol viewing/editing area. Not all commands are available on the toolbars, but all commands are available in the menus.

The button displays or hides the list of available libraries, which allows you to select an active library. When a symbol is saved, it will be placed in this library.

Clicking the icon on the left toolbar toggles the treeview of libraries and symbols. Clicking on a symbol opens that symbol.

Dopo la modifica, un simbolo può essere salvato nella libreria corrente o in una nuova libreria.

Per salvare il simbolo modificato nella libreria corrente, fare clic sull’icona . Le modifiche verranno scritte sul simbolo esistente.

Per salvare i cambiamenti del simbolo in un nuovo simbolo, fare clic su File → Salva con nome…​. Il simbolo può essere salvato nella libreria corrente o in una diversa libreria. Si può impostare anche un nuovo nome per il simbolo.

Per creare un nuovo file contenente solo il simbolo corrente, fare clic su File → Esporta → Simbolo…​. Questo file sarà un file di libreria standard che conterrà solo un simbolo.

Gli elementi grafici formano la rappresentazione di un simbolo e non contengono informazioni di connessioni elettriche. Vengono creati usando i seguenti strumenti:

La barra strumenti verticale sul lato destro della finestra principale permette di piazzare tutti gli elementi grafici richiesti per progettare la rappresentazione di un simbolo.

I simboli possono avere fino a due rappresentazioni simboliche (una standard e una alternativa, spesso chiamata "equivalente DeMorgan") e/o avere più di una unità per contenitore (per esempio le porte logiche). Alcuni simboli possono avere più di una unità per ogni contenitore con simboli e configurazioni di piedinatura differenti.

For example, consider a relay with two switches, which can be designed as a symbol with three different units: a coil, switch 1, and switch 2. Designing a symbol with multiple units per package and/or alternate body styles is very flexible. A pin or a body symbol item can be common to all units or specific to a given unit or they can be common to both symbolic representation so are specific to a given symbol representation.

By default, pins are specific to a unit and body style. When a pin is common to all units or all body styles, it only needs to be created once. This is also the case for the body style graphic shapes and text, which may be common to each unit, but typically are specific to each body style.

To add additional units to a symbol, set the Number of Units property to the appropriate number in the Symbol Properties dialog. By default, symbol units are named Unit A, Unit B, etc., but you can set an arbitrary name for the current unit using Edit → Set Unit Display Name…​.

To add an alternate body style, set the Has alternate body style (De Morgan) property in the Symbol Properties dialog.

You can create and insert a pin by clicking on the button. Pin properties can be edited by double clicking on the pin. You can also delete or move pins that you have already added. Pins must be created carefully, because any error will have consequences on the PCB design.

All library symbols are defined with four default fields. The reference designator, value, footprint assignment, and datasheet link fields are created whenever a symbol is created or copied. Only the reference designator is required.

The Footprint field, if used, contains a reference to a footprint for the symbol. The format is LIBNAME:FOOTPRINTNAME, where LIBNAME is the name of the footprint library in the footprint library table (see the Footprint Library Table section in the PCB Editor manual) and FOOTPRINTNAME is the name of the footprint in the library LIBNAME.

I simboli definiti nelle librerie sono in genere definiti solo con questi quattro campi predefiniti. Campi aggiuntivi come fornitore, numero di parte, costo unitario, ecc. possono essere aggiunti ai simboli della libreria, ma generalmente questo viene fatto nell’editor dello schema in modo che i campi aggiuntivi possano essere applicati a tutti i simboli nello schema.

Power symbols are symbols that are used to label a wire as part of a global power net, like VCC or GND. The behavior of power symbols is described in the electrical connections section. Power symbols are handled and created the same way as normal symbols, but there are several additional considerations described below.

It may be useful to place power symbols in a dedicated library. KiCad’s symbol library places power symbols in the power library, and users may create libraries to store their own power symbols. If the Define as power symbol box is checked in a symbol’s properties, that symbol will appear in the Schematic Editor’s Add Power Symbol dialog for convenient access.

Di seguito è riportato un esempio di simbolo di potenza GND.

Power symbols consist of a pin of type "Power input" that is marked invisible. They must also have the Define as power symbol property checked. Invisible power input pins have a special property of making implicit global connections based on the pin name.

Per creare un simbolo di potenza, seguire questi passi:

An easier method to create a new power symbol is to use another symbol as a starting point, as described earlier.

The Symbol Editor can check for common issues in your symbols. Run the symbol checker using the button in the top toolbar.

The symbol checker checks for:

Resistor, inductor, and capacitor models can be inferred, which means that KiCad will detect that they are passives and automatically assign an appropriate simulation model. Therefore they do not require any special settings; users only need to set the Value field of the symbol.

KiCad infers simulation models for symbols based on the following criteria:

Inferred models are ideal models. If the simulation requires a non-ideal model, you must explicitly assign a model.

KiCad offers several standard simulation models. They do not require an external model file. The following devices are available:

To add a built-in model to a symbol, open the Simulation Model Editor dialog (Symbol Properties → Simulation Model…​) and select Built-in SPICE model.

Refer to the ngspice documentation for more details about these models.

Device sets the type of device to simulate: a resistor, BJT, voltage source, etc. This value is stored in the symbol’s Sim.Device field.

Type selects the type of model to use for the device. Most devices have several types of models to choose from, which may vary in their degree of accuracy, which characteristics they are optimized for, and what parameters they have available. Refer to the ngspice documentation for details. This value is stored in the symbol’s Sim.Type field.

The parameters tab displays the parameters of the model and lets you edit them. For example, a resistor’s resistance, a voltage source’s waveform, a MOSFET’s width and length, etc. Any parameters that differ from the model’s defaults are stored in the symbol’s Sim.Params field.

The code tab displays the generated SPICE model as it will be written to the SPICE netlist for simulation.

The Save parameter '<parameter name>' in Value field checkbox uses the symbol’s Value field for storing parameters instead of the Sim.Params field. This may make it easier to edit simple models from the schematic, without opening the Simulation Model Editor. This option is only available for ideal passive models (R, L, C) and DC sources. If the field Sim.Params exists in the symbol, it will take priority over the Value field.

KiCad can load SPICE models from external files. The models must be in a standard SPICE format and not encrypted.

To load a model from an external file, open the Simulation Model Editor dialog (Symbol Properties → Simulation Model…​) and select SPICE model from file.

File is the path to the model file to use. The path can be absolute or relative to the project folder. The path can also be relative to the value of SPICE_LIB_DIR if you have defined that path variable. The library filename is saved in the symbol’s Sim.Library field.

Model is the name of the desired model in the model file. If the file contains multiple models, they will all be listed in the dropdown. The selected model is listed in the symbol’s Sim.Name field.

Parameters can be overridden (or additional parameters specified) using the parameters tab. All parameters specified in the selected model or the parameters tab are stored in the symbol’s Sim.Params field.

The code tab displays the generated SPICE model as it will be written to the SPICE netlist for simulation.

IBIS (I/O Buffer Information Specification) files are an alternative to SPICE models for modeling the behavior of input/output buffers on digital parts. In order to load an IBIS file, users should follow the procedure for SPICE library models, but provide a .ibs file.

File is the path to the model file to use. The path can be absolute or relative to the project folder. The path can also be relative to the value of SPICE_LIB_DIR if you have defined that path variable. The library filename is saved in the symbol’s Sim.Library field. If an IBIS model file is loaded, the remaining fields in the dialog will relate to the IBIS model.

Component selects which component from the IBIS file to use, as IBIS files can contain multiple components. The component name is saved in the symbol’s Sim.Name field.

Pin selects which pin in the IBIS model to simulate. The selected pin must be mapped to a symbol pin in the Pin Assignments tab. The chosen pin’s number is saved in the symbol’s Sim.Ibis.Pin field.

Model is the list of models available for the selected pin, for example an input or an output. The chosen model name is saved in the symbol’s Sim.Ibis.Model field.

Type selects what the pin should do in the simulation. A pin can be a passive device that doesn’t drive any value; it can be a DC driver that drives high, low, or high-impedance; or it can be a rectangular wave or PRBS driver. This value is stored in the symbol’s Sim.Type field.

The Parameters tab lets you see and edit the parameters of the model. For each parameter, you can switch between a minimum, typical, or maximum value, as defined in the IBIS file. You can also choose the parameters of the driven waveform, depending on the pin’s chosen type. Any parameters that differ from the defaults are stored in the symbol’s Sim.Params field.

Simulation models may have their pins numbered differently than the corresponding symbol. For example, SPICE models for diodes usually consider pin 1 to be the anode, while schematic symbols are usually drawn with pin 1 as the cathode.

You can use the Simulation Model Editor’s Pin Assignments tab to map the symbol’s pins to the simulation model pins.

The left column displays the name and number of each symbol pin. For each symbol pin, you can select the corresponding pin from the simulation model in the dropdown in the right column.

When you use a subcircuit model, the dialog displays the model’s code under the pin assignments for use as a reference while assigning pins.

To run a simulation, open the SPICE simulator dialog by clicking Inspect → Simulator in the schematics editor window or using the button in the top toolbar.

La finesta è divisa in diverse sezioni:

Workbooks are files that store information about the simulation environment, including simulation setup parameters and the list of displayed signals. They can be used to store the setup for a set of analyses, which can then be reloaded and rerun at a later time.

You can save and load a workbook using File → Save Workbook and File → Open Workbook.

Before running a simulation, you need to select a simulation type and choose the simulation parameters. This can be done using Simulation → Settings…​ or the Sim Command button () and then selecting one of the available analysis types:

Analysis types are further explained in the ngspice documentation.

An alternative way to configure a simulation is to type SPICE directives into text fields on schematics. Any text field directives related to a simulation command are overridden by the settings selected in the dialog. This means that once a simulation has run, the dialog overrides the schematic directives until the simulator is reopened.

Once the simulation command is set, users can start a simulation with Simulation → Start Simulation (Ctrl+R) or the Run/Stop Simulation button ().

It is possible to change passive (R, L, C) values using sliders to graphically adjust them. Whenever the slider is set to a new position, the simulation is run with the new parameters and plots are updated. In order to add a slider for a component, use Simulation → Tune Component Value or the button in the toolbar, and then click on the component to tune.

KiCad’s simulator offers two ways to export results:

To create a database library, you must create a configuration file that contains the necessary information for KiCad to connect to your database and retrieve data from tables. Copy the template below into a new file and save it with a kicad_dbl extension. You can then add this file to your global symbol library table using the Configure Symbol Libraries dialog.

After creating your configuration file and adding it to your symbol library table, you can place parts from the database tables using the Symbol Chooser. Parts placed from a database library can be updated using the Update Symbols from Library function, which will update any fields that were changed in the database as well as updating the underlying symbol if it was changed in the source library.

Note that any source library referenced by a database table must also be present in the symbol library table for the database library to function. If you want to use a library only as a source of symbols for a database library, you can hide it from the Symbol Chooser by clearing the "Visible" checkbox in the Manage Symbol Libraries dialog.

I nuovi generatori di netlist vengono aggiunti alla finestra di dialogo Esporta netlist facendo clic sul pulsante Aggiungi generatore…​.

I nuovi generatori richiedono un nome e un comando. Il nome viene mostrato nell’etichetta della scheda e il comando viene eseguito ogni volta che si fa clic sul pulsante Esporta netlist.

Quando viene generata la netlist, KiCad crea un file XML intermedio che contiene tutte le informazioni della netlist dallo schema. In successione viene eseguito il comando generatore per trasformare la netlist intermedia nel formato netlist desiderato.

Il comando netlist deve essere impostato correttamente in modo che lo script del generatore di netlist prenda il file netlist intermedio come ingresso ed emetta il file netlist desiderato. L’esatto comando netlist dipenderà dallo script generatore utilizzato. Il formato del comando è descritto di seguito.

Python e XSLT sono strumenti comunemente usati per creare generatori di netlist personalizzate.

KiCad usa il file netlist intermedio anche per generare le distinte materiali con lo strumento generatore di DIBA.

Ulteriori script possono essere aggiunti all’elenco degli script del generatore DIBA facendo clic sul pulsante . Gli script possono essere rimossi facendo clic sul pulsante . Il pulsante apre lo script selezionato in un editor di testo.

Gli script generatori in Python e XSLT possono contenere una intestazione di commento per descrivere funzione e uso del generatore. Questa intestazione di commento viene visualizzata nella finestra di dialogo DIBA come descrizione per ciascun generatore. L’intestazione di commento deve contenere la stringa @package. Tutto ciò che segue quella stringa fino alla fine del commento viene usato come descrizione per il generatore.

KiCad riempie automaticamente il campo della riga di comando quando viene aggiunto un nuovo script generatore, ma potrebbe essere necessario regolare manualmente la riga di comando a seconda dello script. KiCad tenta di determinare automaticamente l’estensione del file di output dalla riga di comando di esempio nell’intestazione dello script generatore.

La riga di comando per un esportatore di netlist o DIBA definisce il comando che KiCad eseguirà per generare il file di uscita selezionato.

Per un esportatore di netlist che utilizza xsltproc, un esempio è:

xsltproc -o %O.net /usr/share/kicad/plugins/netlist_form_pads-pcb.asc.xsl %I

Per un esportatore DIBA che usa Python, un esempio è:

/usr/bin/python3 /usr/share/kicad/plugins/bom_csv_grouped_by_value.py "%I" "%O.csv"

Alcune sequenze di caratteri come %I e %O hanno un significato speciale nella riga di comando, dato che KiCad le sostituisce con un nome file o un percorso prima di eseguire il comando.

Quando si esportano file DIBA e netlist, KiCad crea un file netlist intermedio e quindi esegue uno strumento separato che post-elabora la netlist intermedia nel formato netlist o DIBA desiderato.

La netlist intermedia usa la sintassi XML. Essa contiene una grande quantità di dati sul progetto. A seconda del risultato (distinta materiali o netlist), differenti sottoinsiemi dell’intero file di netlist intermedia saranno inseriri nel file finale risultante.

La struttura del file della netlist intermedia è descritta in dettaglio sotto.

Poiché la conversione dal file della netlist intermedia alla netlist di uscita o DIBA è una trasformazione da testo a testo, il filtro di post-elaborazione può essere scritto utilizzando Python, XSLT o qualsiasi altro strumento in grado di accettare XML come ingresso.

Questo campione dà un’idea del formato del file netlist.

Alcuni esportatori di netlist di esempio che usano XSLT sono inclusi sotto.

XSLT è di per sè un linguaggio XML molto adatto alle trasformazioni XML. Il programma xsltproc può essere usato per leggere in ingresso il file XML di netlist intermedio, applicare un foglio di stile per trasformare l’ingresso, e salvare il risultato in un file in uscita. L’uso di xsltproc richiede un file foglio di stile che usi le convenzioni XSLT. L’intero processo di conversione viene gestito da KiCad, dopo essere stato configurato per l’esecuzione di xsltproc in modo specifico.

Il documento che descrive le trasformazioni XSL (XSLT) è disponibile qui: http://www.w3.org/TR/xslt