The user-specific file eaglerc stores various settings defined during the work with Electronics. Among them you find some expert settings that can be adjusted in this file directly. The most important of them are listed here.

Since version 5.2 it is possible to change these parameters with the help of the SET command in the command line. Please see the help function about the SET command for details.

CAM Processor – suppress drills/holes warning

If you want to suppress the warning that you should activate the Drills and the Holes layer for generating Drill data, write the following line in the eaglerc file:

Warning.Cam.DrillsAndHolesConcurrent = "0"

Change component value warning

Some users don't want the warning message about a part not having a user definable value, so this warning can be disabled by appending the following line to the file:

Warning.PartHasNoUserDefinableValue = "0"

Consistency check

In order to handle Board/Schematic pairs that have only minor inconsistencies, the user can enable a dialog that allows him to force the editor to perform Forward&Back Annotation, even if the ERC detects that the files are inconsistent. This can be done by appending the following line:

Erc.AllowUserOverrideConsistencyCheck = "1"

Delete wire joints

If you absolutely insist on having the DELETE command delete wire joints without pressing the Ctrl key, you can append the following line to the file:

Cmd.Delete.WireJointsWithoutCtrl = "1"

Device name as value for all components

Some users always want to use the device name as part value, even if the part needs a user-supplied value. Those who want this can append the following line to the file:

Sch.Cmd.Add.AlwaysUseDeviceNameAsValue = "1"

Disable Ctrl for radius mode

If you don't like the special mode in wire drawing commands that allows for the definition of an arc radius by pressing the Ctrl key when placing the wire, you can add the following line to the file:

Cmd.Wire.IgnoreCtrlForRadiusMode = "1"

This will turn this feature off for all commands that draw wires.

Group selection

Since the context menu function on the right mouse button interferes with the selection of groups, a group is now selected with Ctrl + Right mouse button. If you want to have the old method of selecting groups back, you can add the following line to the file:

Option.ToggleCtrlForGroupSelectionAndContextMenu = "1"

This will allow selecting groups with the right mouse button only and require Ctrl + Right mouse button for context menus.

Load matching file automatically

If you have a board and schematic editor window open and load another board (or schematic) in one of these windows, and if that other drawing has a matching schematic (or board), Electronics asks whether that other drawing shall also be loaded. To suppress this query and always load the file, set the following option:

Option.AutoLoadMatchingDrawingFile = "1"

Name of net, busses, signals and polygons

If a net consists of more than one segment, the NAME command by default acts only upon the selected segment. To rename the entire net, set this option:

Cmd.Name.RenameEntireNetByDefault = "1"

This parameter also applies to busses.

If a signal contains a polygon, and the NAME command is applied to that polygon, by default only the polygon gets renamed. To make the NAME command act upon the entire signal by default, set this option:

Cmd.Name.RenameEntireSignalByDefault = "1"

Open project

The automatic opening of the project folder at program start (or when activating a project by clicking onto its gray button) can be disabled by appending the following line to the file:

ControlPanel.View.AutoOpenProjectFolder = "0"

Panning drawing window

Panning can be done with the Ctrl button (as in previous versions) by writing this option into the file:

Interface.UseCtrlForPanning = "1"

Note that the Ctrl key is now used for special functions in some commands, so when using these special functions (like selecting an object at its origin in MOVE) with this parameter enabled you may inadvertently pan your drawing window.

Polygon edges as continuous lines

If you don't like the way unprocessed polygons display their edges (as dotted lines), you can add the following line:

Option.DrawUnprocessedPolygonEdgesContinuous = "1"

The edges of polygons will then be displayed as continuous lines.

Reposition of the mouse cursor

Normally Electronics does not automatically position the mouse cursor. However, if you prefer the cursor to be repositioned to the point where it has been before a context menu in the drawing editor was opened, add the following line:

Option.RepositionMouseCursorAfterContextMenu = "1"

Units in dialogs

The automatic unit determination in dialog input fields can be controlled by appending the following line to the file:

Interface.PreferredUnit = "x"

Here "x" can be

• 0 for automatic unit determination (default)
• 1 for imperial units
• 2 for metric units