Left button

Right button

You can move, drag, copy and delete selected areas in all Eeschema menus.

Areas are selected by drawing a box around items using the left mouse button.

Holding Shift'', Ctrl'', or ``Shift + Ctrl'' during selection respectively performs copying, dragging and deletion:

When dragging or copying, you can:

If a block move command has started, another command can be selected using the right-click pop-up menu.

Eeschema uses two library tables to store the list of available symbol libraries, which differ by the scope:

Libraries listed in the Global Libraries table are available to every project. They are saved in sym-lib-table in your home directory (exact path is dependent on the operating system; check the path above the table).

Libraries listed in Project Specific Libraries table are available to the currently opened project. They are saved in sym-lib-table file in the project directory (check the path above the table).

You can view either list by clicking on "Global Libraries" or "Project Specific Libraries" tab below the library table.

Errors are displayed in the Electrical Rules Checker dialog:

Option:

Commands:

This tab allows you to define the connectivity rules between pins; you can choose between 3 options for each case:

Each square of the matrix can be modified by clicking on it.

Option:

Commands:

There are several special copy/paste methods in spreadsheet. They may be useful when entering field values that are repeated in a few components.

These methods are illustrated below.

The icon launches the back-annotate tool.

This tool allows footprint changes made in PcbNew to be imported back into the footprint fields in Eeschema.

The global symbol library table contains the list of libraries that are always available regardless of the currently loaded project file. The table is saved in the file sym-lib-table in the user’s home folder. The location of this folder is dependent upon the operating system being used.

The project specific symbol library table contains the list of libraries that are available specifically for the currently loaded project file. The project specific symbol library table can only be edited when it is loaded along with the project file. If no project file is loaded or there is no symbol library table file in the current project path, an empty table is created which can be edited and later saved along with the project file.

The first time Eeschema is run and the global symbol table file sym-lib-table is not found in the user’s home folder, Eeschema will attempt to copy the default symbol table file sym-lib-table stored in the system’s KiCad template folder to the file sym-lib-table in the user’s home folder. If the default template sym-lib-table file cannot be found, a dialog will prompt for an alternate location for the sym-lib-table file. If no sym-lib-table is found or the dialog is dismissed, an empty symbol library table will be created in the user’s home folder. If this happens, the user can either copy sym-lib-table manually or configure the table by hand.

In order to use a symbol library, it must first be added to either the global table or the project specific table. The project specific table is only applicable when you have a project file open.

Each library entry must have a unique nickname.

This does not have to be related in any way to the actual library file name or path. The colon ':' and '/' characters cannot be used anywhere in the library nickname. Each library entry must have a valid path and/or file name depending on the type of library. Paths can be defined as absolute, relative, or by environment variable substitution (see section below).

The appropriate plug in type must be selected in order for the library to be properly read. KiCad currently supports only legacy symbol library files plug-in.

There is also a description field to add a description of the library entry. The option field is not used at this time so adding options will have no effect when loading libraries.

One of the most powerful features of the symbol library table is environment variable substitution. This allows for definition of custom paths to where symbol libraries are stored in environment variables. Environment variable substitution is supported by using the syntax $\{ENV_VAR_NAME\} in the library path.

By default, at run time KiCad defines two environment variables:

You can override KICAD_SYMBOL_DIR by defining it yourself in preferences/ Configure Path which allows you to substitute your own libraries in place of the default KiCad symbol libraries.

KIPRJMOD allows you to store libraries in the project path without having to define the absolute path (which is not always known) to the library in the project specific symbol library table.

Symbol libraries can be defined either globally or specifically to the currently loaded project. Symbol libraries defined in the user’s global table are always available and are stored in the sym-lib-table file in the user’s home folder. The project specific symbol library table is active only for the currently open project file.

There are advantages and disadvantages to each method. Defining all libraries in the global table means they will always be available when needed. The disadvantage of this is that load time will increase.

Defining all symbol libraries on a project specific basis means that you only have the libraries required for the project which decreases symbol library load times. The disadvantage is that you always have to remember to add each symbol library that you need for every project.

One usage pattern would be to define commonly used libraries globally and the libraries only required for the project in the project specific library table. There is no restriction on how to define libraries.

When loading a schematic created prior to the symbol library table implementation, Eeschema will attempt to remap the symbol library links in the schematic to the appropriate library table symbols. The success of this process is dependent on several factors:

To load a symbol into your schematic you can use the icon . A dialog box allows you to type the name of the symbol to load.

The Choose Symbols dialog will filter symbols by name, keywords, and description according to what you type into the search field. Advanced filters can be used just by typing them:

Before placing the symbol in the schematic, you can rotate it, mirror it, and edit its fields, by either using the hotkeys or the right-click context menu. This can be done the same way after placement.

Here is a symbol during placement:

A power port symbol is a symbol (the symbols are grouped in the “power” library), so they can be placed using the symbol chooser. However, as power placements are frequent, the tool is available. This tool is similar, except that the search is done directly in the ``power'' library.

There are two ways to edit a symbol:

When a symbol has just been placed, you may have to modify its value (particularly for resistors, capacitors, etc.), but it is useless to assign to it a reference number right away, or to select the unit (except for components with locked units, which you have to assign manually). This can be done automatically by the annotation function.

All these drawing elements can also be placed with the tools on the vertical right toolbar.

These elements are:

There are two ways to establish connection:

The following figure shows the two methods:

Note 1:

The point of “contact” of a label is the lower left corner of the first letter of the label. This point is displayed with a small square when not connected.

This point must thus be in contact with the wire, or be superimposed at the end of a pin so that the label is seen as connected.

Note 2:

To establish a connection, a segment of wire must be connected by its ends to an another segment or to a pin.

If there is overlapping (if a wire passes over a pin, but without being connected to the pin end) there is no connection.

Note 3:

Wires that cross are not implicitly connected. It is necessary to join them with a junction dot if a connection is desired.

The previous figure (wires connected to DB25FEMALE pins 22, 21, 20, 19) shows such a case of connection using a junction symbol.

Note 4:

If two different labels are placed on the same wire, they are connected together and become equivalent: all the other elements connected to one or the other labels are then connected to all of them.

In the following schematic, many pins are connected to buses.

When the power pins of the symbols are visible, they must be connected, as for any other signal.

Symbols such as gates and flip-flops may have invisible power pins. Care must be taken with these because:

And moreover, it would be a bad idea to make them visible and to connect them like the other pins, because the schematic would become unreadable and not in accordance with usual conventions.

Eeschema automatically connects invisible power pins of the same name to the power net of that name. It may be necessary to join power nets of different names (for example, "GND" in TTL components and "VSS" in MOS components); use power ports for this.

It is not recommended to use labels for power connection. These only have a “local” connection scope, and would not connect the invisible power pins.

The figure below shows an example of power port connections.

In this example, ground (GND) is connected to power port VSS, and power port VCC is connected to VDD.

Two PWR_FLAG symbols are visible. They indicate that the two power ports VCC and GND are really connected to a power source. Without these two flags, the ERC tool would diagnose: Warning: power port not powered.

All these symbols can be found in the ``power'' symbol library.

These symbols are very useful to avoid undesired ERC warnings. The electrical rules check ensures that no connection has been accidentally left unconnected.

If pins must really remain unconnected, it is necessary to place a "No Connect" flag (tool ) on these pins. These symbols do not have any influence on the generated netlists.

It can be useful (to aid in understanding the schematic) to place annotations such as text fields and frames. Text fields (tool ) and Polyline (tool ) are intended for this use, contrary to labels and wires, which are connection elements.

Here you can find an example of a frame with a textual comment.

The title block is edited with the tool .

The sheet number (Sheet X/Y) is automatically updated.

Local labels, tool , are connecting signals only within a sheet. Hierarchical labels (tool ) are connecting signals only within a sheet and to a hierarchical pin placed in the parent sheet.

Global labels (tool ) are connecting signals across all the hierarchy. Power pins (type power in and power out) invisible are like global labels because they are seen as connected between them across all the hierarchy.

Here are some comments on various ways to provide connections, other than wire connections.

Global labels that have an identical name are connected across the whole hierarchy.

(power labels like vcc …​ are global labels)

This example shows 5 elements placed, but not annotated.

After the annotation tool Is executed, the following result is obtained.

Sort by X position.

Sort by Y position.

You can see that four 74LS00 gates were distributed in U1 package, and that the fifth 74LS00 has been assigned to the next, U2.

Here is an annotation in sheet 2 where the option use first free number in schematic was set.

Option start to sheet number*100 and use first free number give the following result.

The option start to sheet number*1000 and use first free number gives the following result.

Many software tools that use netlists do not accept spaces in the component names, pins, nets or other informations. Avoid using spaces in labels, or names and value fields of components or their pins to ensure maximum compatibility.

In the same way, special characters other than letters and numbers can cause problems. Note that this limitation is not related to Eeschema, but to the netlist formats that can then become untranslatable to software that uses netlist files.

For the Pspice simulator, you have to include some command lines in the netlist itself (.PROBE, .AC, etc.).

Any text line included in the schematic diagram starting with the keyword -pspice or -gnucap will be inserted (without the keyword) at the top of the netlist.

Any text line included in the schematic diagram starting with the keyword +pspice or +gnucap will be inserted (without the keyword) at the end of the netlist.

Here is a sample using many one-line texts and one multi-line text:

For example, if you type the following text (do not use a label!):

a line .PROBE will be inserted in the netlist.

In the previous example three lines were inserted at the beginning of the netlist and two at the end with this technique.

If you are using multiline texts, +pspice or +gnucap keywords are needed only once:

creates the four lines:

Also note that the GND net must be named 0 (zero) for Pspice.

You can add a new netlist plug-in via the Add Plugin button.

Here is the plug-in PadsPcb setup window:

The setup will require:

When the netlist is generated:

Here is an example, using xsltproc.exe as a tool to convert .xsl files, and a file netlist_form_pads-pcb.xsl as converter sheet style:

f:/kicad/bin/xsltproc.exe -o %O.net f:/kicad/bin/plugins/netlist_form_pads-pcb.xsl %I

With:

For a schematic named test.sch, the actual command line is:

f:/kicad/bin/xsltproc.exe -o test.net f:/kicad/bin/plugins/netlist_form_pads-pcb.xsl test.tmp.

This is a very simple piece of software, because its purpose is only to convert an input text file (the intermediate text file) to another text file. Moreover, from the intermediate text file, you can create a BOM list.

When using xsltproc as the converter tool only the sheet style will be generated.

See Chapter 14 for more explanations about xslproc, descriptions of the intermediate file format, and some examples of sheet style for converters.

Sheet size is normally checked. In this case, the sheet size defined in the title block menu will be used and the chosen scale will be 1. If a different sheet size is selected (A4 with A0, or A with E), the scale is automatically adjusted to fill the page.

For all standard dimensions, you can adjust the offsets to center the drawing as accurately as possible. Because plotters have an origin point at the center or at the lower left corner of the sheet, it is necessary to be able to introduce an offset in order to plot properly.

Generally speaking:

To set an offset:

The main tool bar typically located at the top of the main window shown below consists of the library management tools, undo/redo commands, zoom commands, and symbol properties dialogs.

The vertical toolbar typically located on the right hand side of the main window allows you to place all of the elements required to design a symbol. The table below defines each toolbar button.

The vertical tool bar typically located on the left hand side of the main window allows you to set some of the editor drawing options. The table below defines each tool bar button.

When you edit a symbol you are not really working on the symbol in its library but on a copy of it in the computer’s memory. Any edit action can be undone easily. A symbol may be loaded from a local library or from an existing symbol.

A new symbol can be created by clicking the . You will be asked for a symbol name (this name is used as default value for the value field in the schematic editor), the reference designator (U, IC, R…​), the number of units per package (for example a 7400 is made of 4 units per package) and if an alternate body style (sometimes referred to as DeMorgan) is desired. If the reference designator field is left empty, it will default to "U". These properties can be changed later, but it is preferable to set them correctly at the creation of the symbol.

A new symbol will be created using the properties above and will appear in the editor as shown below.

Often, the symbol that you want to make is similar to one already in a symbol library. In this case it is easy to load and modify an existing symbol.

Symbol properties should be carefully set during the symbol creation or alternatively they are inherited from the copied symbol. To change the symbol properties, click on the to show the dialog below.

It is very important to correctly set the number of units per package and the alternate symbolic representation, if enabled, because when pins are edited or created the corresponding pins for each unit will be affected. If you change the number of units per package after pin creation and editing, there will be additional work to add the new unit pins and symbols. Nevertheless, it is possible to modify these properties at any time.

The graphic options "Show pin number" and "Show pin name" define the visibility of the pin number and pin name text. This text will be visible if the corresponding options are checked. The option "Place pin names inside" defines the pin name position relative to the pin body. This text will be displayed inside the symbol outline if the option is checked. In this case the "Pin Name Position Offset" property defines the shift of the text away from the body end of the pin. A value from 30 to 40 (in 1/1000 inch) is reasonable.

The example below shows a symbol with the "Place pin name inside" option unchecked. Notice the position of the names and pin numbers.

If the symbol has more than one symbolic repersentation, you will have to select one representation to edit them. To edit the normal representation, click the .

To edit the alternate representation, click on the . Use the shown below to select the unit you wish to edit.

Each graphic element (line, arc, circle, etc.) can be defined as common to all units and/or body styles or specific to a given unit and/or body style. Element options can be quickly accessed by right-clicking on the element to display the context menu for the selected element. Below is the context menu for a line element.

You can also double-left-click on an element to modify its properties. Below is the properties dialog for a polygon element.

The properties of a graphic element are:

The allows for the creation of graphical text. Graphical text is always readable, even when the symbol is mirrored. Please note that graphical text items are not fields.

This is an example of a relay defined with three units per package, switch 1, switch 2, and the coil:

Option: pins are not linked. One can add or edit pins for each unit without any coupling with pins of other units.

All units are not interchangeable must be selected.

Unit 1

Unit 2

Unit 3

It does not have the same symbol and pin layout and therefore is not interchangeable with units 1 and 2.

A pin is defined by its graphical representation, its name and its "number". The pin’s "number" is defined by a set of 4 letters and / or numbers. For the Electrical Rules Check (ERC) tool to be useful, the pin’s "electrical" type (input, output, tri-state…​) must also be defined correctly. If this type is not defined properly, the schematic ERC check results may be invalid.

Important notes:

The pin properties dialog allows you to edit all of the characteristics of a pin. This dialog pops up automatically when you create a pin or when double-clicking on an existing pin. This dialog allows you to modify:

Shown in the figure below are the different pin graphical styles. The choice of graphic styles does not have any influence on the pin’s electrical type.

Choosing the correct electrical type is important for the schematic ERC tool. The electrical types defined are:

You can modify the length or text size of the name and/or number of all the pins using the Global command entry of the pin context menu. Click on the parameter you want to modify and type the new value which will then be applied to all of the current symbol’s pins.

Symbols with multiple units and/or graphical representations are particularly problematic when creating and editing pins. The majority of pins are specific to each unit (because their pin number is specific to each unit) and to each symbolic representation (because their form and position is specific to each symbolic representation). The creation and the editing of pins can be problematic for symbols with multiple units per package and alternate symbolic representations. The symbol library editor allows the simultaneous creation of pins. By default, changes made to a pin are made for all units of a multiple unit symbol and both representations for symbols with an alternate symbolic representation.

The only exception to this is the pin’s graphical type and name. This dependency was established to allow for easier pin creation and editing in most of the cases. This dependency can be disabled by toggling the on the main tool bar. This will allow you to create pins for each unit and representation completely independently.

A symbol can have two symbolic representations (representation known as``DeMorgan'') and can be made up of more than one unit as in the case of symbols with logic gates. For certain symbols, you may want several different graphic elements and pins. Like the relay sample shown in the previous section, a relay can be represented by three distinct units: a coil, switch contact 1, and switch contact 2.

The management of the symbols with multiple units and symbols with alternate symbolic representations is flexible. A pin can be common or specific to different units. A pin can also be common to both symbolic representations or specific to each symbolic representation.

By default, pins are specific to each representation of each unit, because their number differs for each unit, and their design is different for each symbolic representation. When a pin is common to all units, it only has to drawn once such as in the case of power pins.

An example is the output pin 7400 quad dual input NAND gate. Since there are four units and two symbolic representations, there are eight separate output pins defined in the symbol definition. When creating a new 7400 symbol, unit A of the normal symbolic representation will be shown in the library editor. To edit the pin style in alternate symbolic representation, it must first be enabled by clicking the button on the tool bar. To edit the pin number for each unit, select the appropriate unit using the drop down control.

To edit an existing symbol field, right-click on the field text to show the field context menu shown below.

To edit undefined fields, add new fields, or delete optional fields on the main tool bar to open the field properties dialog shown below.

Fields are text sections associated with the symbol. Do not confuse them with the text belonging to the graphic representation of this symbol.

Important notes:

Keywords allow you to search in a selective way for a symbol according to specific selection criteria (function, technological family, etc.)

The Eeschema research tool is not case sensitive. The most current key words used in the libraries are

The line of comment (and keywords) is displayed in various menus, particularly when you select a symbol in the displayed symbols list of a library and in the ViewLib menu.

If this Doc. file exists, it is also accessible in the schematic capture software, in the pop-up menu displayed by right-clicking on the symbol.

Indicates an attached file (documentation, application schematic) available ( pdf file, schematic diagram, etc.).

You can enter a list of allowed footprints for the symbol. This list acts as a filter used by CvPcb to display only the allowed footprints. A void list does not filter anything.

Wild-card characters are allowed.

S014* allows CvPcb to show all the footprints with a name starting by SO14.

For a resistor, R? shows all the footprints with a 2 letters name starting by R.

Here are samples: with and without filtering

With filtering

Without filtering

A symbol can be exported with the button . You can generally create only one graphic, also it will be a good idea to delete all pins, if they exist.

Importing allows you to add graphics to a symbol you are editing. A symbol is imported with the button . Imported graphics are added as they were created in existing graphics.

The corresponding intermediate netlist (using XML syntax) of the circuit above is shown below.

The pads-pcb format is comprised of two sections.

Immediately below is a style-sheet which converts the Intermediate Netlist file to a pads-pcb netlist format:

And here is the pads-pcb output file after running xsltproc:

The command line to make this conversion is:

The Cadstar format is comprised of two sections.

Here is the style-sheet file to make this specific conversion:

Here is the Cadstar output file.

This format has only one section which is the footprint list. Each footprint includes its list of pads with reference to a net.

Here is the style-sheet for this specific conversion:

Here is the OrcadPCB2 output file.

Intermediate Netlist converters can be automatically launched within Eeschema.

Because the intermediate netlist file contains all information about used components, a BOM can be extracted from it. Here is the plug-in setup window (on Linux) to create a customized Bill Of Materials (BOM) file:

The path to the style sheet bom2csv.xsl is system dependent. The currently best XSLT style-sheet for BOM generation at this time is called bom2csv.xsl. You are free to modify it according to your needs, and if you develop something generally useful, ask that it become part of the KiCad project.

The intermediate Netlist accounts for five sections.

The file content has the delimiter <export>

The header has the delimiter <design>

This section can be considered a comment section.

The component section has the delimiter <components>

This section contains the list of components in your schematic. Each component is described like this:

The libparts section has the delimiter <libparts>, and the content of this section is defined in the schematic libraries. The libparts section contains

Lines like <pin num="1" type="passive"/> give also the electrical pin type. Possible electrical pin types are

The libraries section has the delimiter <libraries>. This section contains the list of schematic libraries used in the project.

The nets section has the delimiter <nets>. This section contains the "connectivity" of the schematic.

This section lists all nets in the schematic.

A possible net contains the following.

xsltproc is a command line tool for applying XSLT style-sheets to XML documents. While it was developed as part of the GNOME project, it can operate independently of the GNOME desktop.

xsltproc is invoked from the command line with the name of the style-sheet to be used followed by the name of the file or files to which the style-sheet is to be applied. It will use the standard input if a filename provided is - .

If a style-sheet is included in an XML document with a Style-sheet Processing Instruction, no style-sheet needs to be named in the command line. xsltproc will automatically detect the included style-sheet and use it. By default, the output is to stdout. You can specify a file for output using the -o option.

-V or --version

Show the version of libxml and libxslt used.

-v or --verbose

Output each step taken by xsltproc in processing the stylesheet and the document.

-o or --output file

Direct output to the file named file. For multiple outputs, also known as ``chunking'', -o directory/ directs the output files to a specified directory. The directory must already exist.

--timing

Display the time used for parsing the stylesheet, parsing the document and applying the stylesheet and saving the result. Displayed in milliseconds.

--repeat

Run the transformation 20 times. Used for timing tests.

--debug

Output an XML tree of the transformed document for debugging purposes.

--novalid

Skip loading the document’s DTD.

--noout

Do not output the result.

--maxdepth value

Adjust the maximum depth of the template stack before libxslt concludes it is in an infinite loop. The default is 500.

--html

The input document is an HTML file.

--param name value

Pass a parameter of name name and value value to the stylesheet. You may pass multiple name/value pairs up to a maximum of 32. If the value being passed is a string rather than a node identifier, use --stringparam instead.

--stringparam name value

Pass a paramenter of name name and value value where value is a string rather than a node identifier. (Note: The string must be utf-8.)

--nonet

Do not use the Internet to fetch DTD’s, entities or documents.

--path paths

Use the list (separated by space or column) of filesystem paths specified by paths to load DTDs, entities or documents.

--load-trace

Display to stderr all the documents loaded during the processing.

--catalogs

Use the SGML catalog specified in SGML_CATALOG_FILES to resolve the location of external entities. By default, xsltproc looks for the catalog specified in XML_CATALOG_FILES. If that is not specified, it uses /etc/xml/catalog.

--xinclude

Process the input document using the Xinclude specification. More details on this can be found in the Xinclude specification: http://www.w3.org/TR/xinclude/

--profile --norman

Output profiling information detailing the amount of time spent in each part of the stylesheet. This is useful in optimizing stylesheet performance.

--dumpextensions

Dumps the list of all registered extensions to stdout.

--nowrite

Refuses to write to any file or resource.

--nomkdir

Refuses to create directories.

--writesubtree path

Allow file write only within the path subtree.

--nodtdattr

Do not apply default attributes from the document’s DTD.

xsltproc returns a status number that can be quite useful when calling it within a script.

0: normal

1: no argument

2: too many parameters

3: unknown option

4: failed to parse the stylesheet

5: error in the stylesheet

6: error in one of the documents

7: unsupported xsl:output method

8: string parameter contains both quote and double-quotes

9: internal processing error

10: processing was stopped by a terminating message

11: could not write the result to the output file

libxml web page: http://www.xmlsoft.org/

W3C XSLT page: http://www.w3.org/TR/xslt

Passive tab allows the user to assign a passive device model (resistor, capacitor or inductor) to a component. It is a rarely used option, as normally passive components have models assigned implicitly, unless component reference does not match the actual device type.

Model tab is used to assign a semiconductor or a complex model defined in an external library file. Spice model libraries are often offered by device manufacturers.

The main text widget displays the selected library file contents. It is a common practice to put models description inside library files, including the node order.

Source tab is used to assign a power or signal source model. There are two sections: DC/AC analysis and Transient analysis. Each defines source parameters for the corresponding simulation type.

Source type option applies to all simulation types.

Refer to the ngspice documentation, chapter 4 (Voltage and Current Sources) for more details about sources.

The top toolbar provides access to the most frequently performed actions.

Visualizes the simulation results as plots. One can have multiple plots opened in separate tabs, but only the active one is updated when a simulation is executed. This way it is possible to compare simulation results for different runs.

Plots might be customized by toggling grid and legend visibility using View menu. When a legend is visible, it can be dragged to change its position.

Plot panel interaction:

Output console displays messages from the simulator. It is advised to check the console output to verify there are no errors or warnings.

Shows the list of signals displayed in the active plot.

Signals list interaction:

Shows the list of cursors and their coordinates. Each signal may have one cursor displayed. Cursors visibility is set using the Signals list.

Displays components picked with the Tuner tool. Tune panel allows the user to quickly modify component values and observe their influence on the simulation results - every time a component value is changed, the simulation is rerun and plots are updated.

For each component there a few controls associated:

The three text fields recognize Spice unit prefixes.

Tuner tool lets the user pick components for tuning.

To select a component for tuning, click on one in the schematics editor when the tool is active. Selected components will appear in the Tune panel. Only passive components might be tuned.

Probe tool provides an user-friendly way of selecting signals for plotting.

To add a signal to plot, click on a corresponding wire in the schematics editor when the tool is active.

Simulation settings dialog lets the user set the simulation type and parameters. There are four tabs:

The first three tabs provide forms where simulation parameters might be specified. The last tab allows the user to type in custom Spice directives to set up a simulation. You can find more information about simulation types and parameters in the ngspice documentation, chapter 1.2.

An alternative way to configure a simulation is to type Spice directives into text fields on schematics. Any text field directives related to simulation type are overridden by the settings selected in the dialog. It means that once you start using the simulation dialog, the dialog overriddes the schematics directives until the simulator is reopened.

There are two options common to all simulation types: