Eeschema Reference manual - General Top Toolbar - 《KiCad v6.0 Documentation》

General Top Toolbar

Sheet management

The Sheet Settings icon () allows you to define the sheet size and the contents of the title block.

Sheet numbering is automatically updated. You can set the date to today by pressing the left arrow button by “Issue Date”, but it will not be automatically changed.

Search tool

The Find icon () can be used to access the search tool.

You can search for a reference, a value or a text string in the current sheet or in the whole hierarchy. Once found, the cursor will be positioned on the found element in the relevant sub-sheet.

Netlist tool

The Netlist icon () opens the netlist generation tool.

The tool creates a file which describe all connections in the entire hierarchy.

In a multisheet hierarchy, any local label is visible only inside the sheet to which it belongs. For example: the label LABEL1 of sheet 3 is different from the label LABEL1 of sheet 5 (if no connection has been intentionally introduced to connect them). This is due to the fact that the sheet name path is internally associated with the local label.

Even though there is no text length limit for labels in Eeschema, please take into account that other programs reading the generated netlist may have such constraints.

Avoid spaces in labels, because they will appear as separated words in the generated file. It is not a limitation of Eeschema, but of many netlist formats, which often assume that a label has no spaces.

Option:

Default Format

Check to select Pcbnew as the default format.

Other formats can also be generated:

Orcad PCB2
CadStar
Spice (simulators)

External plugins can be added to extend the netlist formats list (PadsPcb Plugin was added in the picture above).

There is more information about creating netlists in Create a Netlist chapter.

Annotation tool

The icon launches the annotation tool. This tool assigns references to components.

For multi-part components (such as 7400 TTL which contains 4 gates), a multi-part suffix is also allocated (thus a 7400 TTL designated U3 will be divided into U3A, U3B, U3C and U3D).

You can unconditionally annotate all the components or only the new components, i.e. those which were not previously annotated.

Scope

Use the entire schematic	All sheets are re-annotated (default).
Use the current page only	Only the current sheet is re-annotated (this option is to be used only in special cases, for example to evaluate the amount of resistors in the current sheet.).
Keep existing annotation	Conditional annotation, only the new components will be re-annotated (default).
Reset existing annotation	Unconditional annotation, all the components will be re-annotated (this option is to be used when there are duplicated references).
Reset, but do not swap any annotated multi-unit parts	Keeps all groups of multiple units (e.g. U2A, U2B) together when reannotating.

Annotation Order

Selects the order in which components will be numbered (either horizontally or vertically).

Annotation Choice

Selects the assigned reference format.

Electrical Rules Check tool

The icon launches the electrical rules check (ERC) tool.

This tool performs a design verification and is able to detect forgotten connections, and inconsistencies.

Once you have run the ERC, Eeschema places markers to highlight problems. The error description is displayed after left clicking on the marker. An error report file can also be generated.

Main ERC dialog

Errors are displayed in the Electrical Rules Checker dialog:

Total count of errors and warnings.
Errors count.
Warnings count.

Option:

Create ERC file report

Check this option to generate an ERC report file.

Commands:

Delete Markers	Remove all ERC error/warnings markers.
Run	Start an Electrical Rules Check.
Close	Close the dialog.

Clicking on an error message jumps to the corresponding marker in the schematic.

ERC options dialog

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

No error
Warning
Error

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

Option:

Test similar labels	Report labels that differ only by letter case (e.g. label/Label/LaBeL). Net names are case-sensitive therefore such labels are treated as separate nets.
Test unique global labels	Report global lables that occur only once for a particular net. Normally it is required to have at least two make a connection.

Commands:

Initialize to Default

Restores the original settings.

Bill of Material tool

The icon launches the bill of materials (BOM) generator. This tool generates a file listing the components and/or hierarchical connections (global labels).

Eeschema’s BOM generator makes use of external plugins, either as XSLT or Python scripts. There are a few examples installed inside the KiCad program files directory.

A useful set of component properties to use for a BOM are:

Value - unique name for each part used.
Footprint - either manually entered or back-annotated (see below).
Field1 - Manufacturer’s name.
Field2 - Manufacturer’s Part Number.
Field3 - Distributor’s Part Number.

For example:

On MS Windows, BOM generator dialog has a special option (pointed by red arrow) that controls visibility of external plugin window.
By default, BOM generator command is executed console window hidden and output is redirected to Plugin info field. Set this option to show the window of the running command. It may be necessary if plugin has provides a graphical user interface.