Headings:

4 - General Toolbar

4.1 - Sheet Management

4.2 - Research tool

4.3 - Netlist tool

4.4 - Annotation tool

4.5 - E.R.C tool

4.5.1 - Main folder/dialog

4.5.2 - Options folder/dialog

4.6 - BOM (Bill of Material) tool

General Toolbar

Sheet Management

Access to page settings:

Sheet size and title block editing.

The date is automatically updated.

Total number of sheets and sheet number are automatically updated.

Research tool

To access this tool.

You can search a component, a value, or a text string in the current sheet or in the whole hierarchy.

The cursor will be positioned on the found element, in the concerned sub-sheet.

Netlist tool

Gives access to the netlist tool.

This netlist file can apply to the whole hierarchy (usual option), or only to the current sheet (the netlist is then partial, but this option can be useful for some software).

In a multisheet hierarchy, any local label is known only inside the sheet to which it belongs.

Thus the label TOTO of sheet 3 is different from the label TOTO of sheet 5 (if no connection has been intentionally introduced to connect them).

This is due to the fact that the sheet number (updated by the annotate command) is associated with the local label. In the previous example, the first label TOTO is actually TOTO_3, and the second label TOTO is actually TOTO_5.

This association can be inhibited if it is wished, but be aware of possible undesired connections.

Notice 1:

Label lengths have no limitations in EESchema, but the software exploiting the generated netlists can be limited on this point.

Notice 2:

Avoid spaces in the labels, because they then appear as separated words. It is not a limitation of Eeschema, but of many netlist formats, which often suppose 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, for the Spice simulator.

Annotation tool

To access the annotation tool.

This tool performs an auto incrementing designation of the 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..

annotate:

project:

All the sheets are re-annotated (usual Option).

Current sheet:

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.).

select items:

All components:

Unconditional annotation, all the components will be re-annotated (this option is to be used after block copy for example, when there are duplicated references).

new components only:

Conditional annotation, only the new components will be re-annotated (usual option).

Buttons:

Annotate:

Execute annotation.

Del Annotate:

Delete component annotation.

E.R.C tool

To access E.R.C tool.

This tool performs a design verification (known as Electrical Rules Check).

This function is particularly useful to detect forgotten connections, and inconsistencies.

Eeschema places markers on the pins or labels able to pose a problem.

The diagnosis can then be given by left clicking on the marker.

An errors file can also be generated.

Main folder/dialog

Errors are displayed in the Erc Diags dialog box :

- Errors and warnings count.

- Errors count.

- Warnings count.

Write ERC report : check to generate an ERC report file.

ERC Test button : to perform an Electrical Rules Check.

Del Markers : to remove all ERC markers.

Exit : to exit this dialog box.

Options folder/dialog

This Setup ERC dialog box allows you to establish 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 it.

BOM (Bill of Material) tool

This menu allows the generation of a file listing of the components and/or hierarchical connections (global labels).

The components can be sorted by :

Reference.

Value.

and multi-part components can be detailed.

The global labels can be sorted by :

Alphabetical classification.

Sub-sheet.

Different sortings can be used simultaneously.

The options are:

Components by Reference	Bill of Material sorted by Reference.
Component by Value	Bill of Material sorted by Value.
Sub components	The BOM shows every device of multi-part components (ex U2A, U2B…).
Hierarchy Pins by name	Hierarchical connections sorted alphabetically.
Hierarchy Pins by Sheet	Hierarchical connections sorted by sheet number.

EESchema

Commands	Page 4 - 1

LTIRF

1996-09-02T17:35:00