What's new in version 4.0?

A detailed list of all changes since version 4.0 can be found in the UPDATE file that comes with the current EAGLE installation archive.

Control Panel

• The Control Panel now has a "Tree View" which provides an overview over all areas of EAGLE, like Libraries, User Language Programs, Projects etc.
• The Control Panel's tree view supports "Drag&Drop" to copy or move files and directories. Files (like ULPs or scripts) can also be dragged over an editor window and dropped there; this results in the file being RUN or executed by the SCRIPT command inside the respective window. Devices and packages can also be dragged and dropped onto editor windows. Dropping an entire library onto a board or schematic editor window will perform a library update.
• Objects in the tree view have a context menu that can be accessed by pressing the right mouse button.
• The menu option "Save project as..." is no longer available. New projects can now be created via the context menu in the "Projects" tree item, or by selecting "File/New/Project" from the Control Panel.
• The path settings in "Options/Directories" can now use the special names "$HOME" and "$EAGLEDIR" to access the user's home directory or the EAGLE installation directory, respectively.
• The new "Auto backup" feature will automatically save any modified drawing into a safety backup file after a certain time. See "Help/Automatic backup" for details.

New Project Structure

• The names of files that are under the current project directory are no longer written as absolute paths into the 'eagle.epf' file, but rather relative to the project directory. This allows for complete project directories to be easily copied or renamed.
• A project is now held in a subdirectory that contains a file named 'eagle.epf' (which stores the location and settings of open windows).

Converting projects from previous versions

• Previous versions of EAGLE used individually named project files (*.epf) to store project information. Beginning with version 4 a project is stored entirely in a subdirectory, and that directory contains a file with the fixed name 'eagle.epf'.
• The easiest way to convert projects from older versions is to create one directory for each project and copy that project's '.epf' file into this directory under the name 'eagle.epf'. The name of the project in version 4 is the name of the project's directory.
• In the Control Panel use the "Options/Directories" dialog to enter the name of the directory that contains your project subdirectories into the "Projects" field.

User Interface

• The textual command menu can now be configured to display aliased command buttons as well as submenus (see HELP MENU for details).
• Changes made in the "Options/User interface" dialog now take effect immediately for open editor windows.
• The cursor inside a layout or schematic editor window can now be set to a "large" crosshair cursor (see "Options/User interface").
• The "Delete" icon was changed from a pencil with an eraser to an 'X'.
• The "Split" icon was changed to better indicate what will happen.

Keyboard and mouse control

• Alt-0 no longer popups up the window list, but leads directly to the Control Panel.
• Pressing the Ctrl key while moving the mouse now scrolls the draw window in any direction.
• The mouse wheel now zooms in and out in editor windows (zoom factor can be adjusted in "Options/User interface/Mouse wheel zoom", a value of '0' disables this feature and the sign of this factor defines the direction of the zoom operation).

Screen display

• The default for "minimum visible text size" has been changed to 3.
• The display mode parameter FAST has been dropped.
• By default the zoom factor in editor windows is limited so that the resulting virtual drawing area does not exceed the 16-bit coordinate range. This is necessary to avoid problems with graphics drivers that are not 32-bit proof. If the graphics driver on a particular system can handle coordinates that exceeed the 16-bit range, "Options/User interface/Limit zoom factor" can be switched off allow larger zoom factors.

Design Rules

• EAGLE now supports a full set of Design Rules that are stored inside the board file (and can also be saved to disk files). Both the Design Rule Check and the Autorouter will use the same set of rules.
• Newly created boards take their design rules from the file 'default.dru', which is searched for in the first directory listed in the "Options/Directories/Design rules" path.
• Cream mask values are now measured "inwards" and thus have a positive sign.
• The parameters AnnulusConduct and ThermalConduct are no longer available. There are now checkboxes in the Design Rules dialog's "Supply" tab that define whether a Thermal or Annulus symbol shall have a "Restring" or not.
• In order to assure that existing boards yield the same results when producing CAM data after they have been updated to version 4, the minimum restring parameters for the outer layers are set to 0 in the design rules (this allows the existing pads and vias to keep their defined diameters). The user should adjust these parameters to some reasonable values and run a design rule check after adding new parts from version 4 libraries. Also, the new design rule parameter that controls the minimum distance between objects in signal layers and the board dimensions (default: 40mil) will be set to 0 if a board that is updated from an older version contains any signal polygons. The reason for this is that in previous versions polygons didn't take the board dimensions into account when they were calculated, but starting with version 4 polygons keep the minimum distance defined in "Edit/Design rules/Distance/Copper/Dimensions" from the boards dimensions. In order to guarantee that updated boards will yield the same results when producing CAM data with version 4 this parameter is set to 0. Note that this will also have an impact on the autorouter, so the user should adjust this parameter to some reasonable value.

Net Classes

• Nets and Signals now have a new parameter called "Net Class".
• The new command CLASS is used to define and select net classes.
• The CHANGE command has a new option 'class' to change the net class of a net or signal.

Polygons

• When calculating polygons, the minimum distances defined in the design rules and net classes will be taken into account. Therefore the default value for the Isolate parameter of newly created polygons is now 0. If a particular polygon is given an Isolate value that exceeds that from the design rules and net classes, the larger value will be taken.
• The new parameter 'rank' defines if and how polygons are subtracted from each other. When updating existing files, polygons in signals will get a rank of '1', while polygons in packages will get rank '7'.
• Polygons are now checked in the Design Rule Check if they have the same 'rank'.
• Sometimes the polygon subtractor didn't go through a gap where, according to the actual widths and minimum distances, it should have.

Design Rule Check

• The DRC now runs a lot faster.
• Progress is now displayed in a progress bar (the progress rectangles are no longer displayed and the SET variables DRC_SHOW and DRC_COLOR are now obsolete).
• Since the DRC is now much faster its error messages are no longer stored in a separate '*.drc' file (this separate file sometimes caused board and DRC error messages to be out of sync).
• Polygons from different signals with the same 'rank' are checked against each other.
• All objects in layers Top..Bottom (including arcs, circles etc.) are now checked.
• The 'overlap' and 'minimum distance' check are no longer separate checks.
• The DRC no longer checks an individual signal against everything else. The newly introduced "Net Classes" can be used to do this.
• The rectangle for a selective DRC can now be defined with "click&drag" (just as in the WINDOW command).
• Holes are no longer checked in the "Grid" check (only pads, vias, smds and wires in signal layers are checked).
• Any objects in signal layers within a package are now checked against each other.
• Several new checks have been added (see the DRC dialog for more information about the new parameters).
• Due to a calculation problem the DRC sometimes reported very small errors where in reality there were no errors.

Long strings

• All names, values and texts can now be of any length.
• The User Language constants regarding name lengths still exist, but the program uses these constants only for formatted output as in the EXPORT command. They are still present for compatibility only.
• There is no more limit to the number of members in a bus (bus index values are limited to 0..511).
• Bus member names can now contain any characters, except ':', ',', '[', ']' and blanks.

Wire styles

• Wires now have a new parameter 'Style', which can be set to one of the following values:

      Continuous      _______________  (default)
      LongDash        ___ ___ ___ ___
      ShortDash       _ _ _ _ _ _ _ _
      DashDot         ___ . ___ . ___
      

• The variable for setting the bend type of a wire has been renamed from Wires_Style to Wire_Bend to avoid confusing the two parameters.
• Note that the DRC and Autorouter will always treat wires as "Continuous", even if their style is different. Wire styles are mainly for electrical and mechanical drawings and should not be used on copper layers. It is an explicit DRC error to use a non-continuous wire as part of a signal that is connected to any pad.

Text fonts

• Texts can now have three different fonts: 'Vector' the program's internal vector font (as used in previous versions) 'Proportional' a proportional pixel font (usually 'Helvetica') 'Fixed' a monospaced pixel font (usually 'Courier')
• When updating drawings from older versions, all texts are converted to 'Proportional' font, except for those in layers Top...Bottom, tRestrict and bRestrict, since these texts probably need to be subtracted from signal polygons, which only works with the 'Vector' font.
• The program makes great efforts to output texts with fonts other than 'Vector' as good as possible. However, since the actual font is drawn by the system's graphics interface, 'Proportional' and 'Fixed' fonts may be output with different sizes and/or lengths. See HELP TEXT if you don't want texts to be displayed with fonts other than 'Vector'. You can set the user interface option "Always vector font" to always have texts output with the builtin vector font.
• When creating output files with the CAM Processor, texts with fonts other than 'Vector' may be output using the 'Vector' font instead. This happens if the actual output device is unable to produce texts with different fonts.
• If a text with a font other than 'Vector' is subtracted from a signal polygon, only the surrounding rectangle is subtracted. Due to the above mentioned possible size/length problems, the actually printed font may exceed that rectangle. Therefore, if you need to subtract a text from a signal polygon it is recommended that you use the 'Vector' font.
• The 'Ratio' parameter has no meaning for texts with fonts other than 'Vector'.
• The CHANGE command has a new option "Font".

Pads and Vias

• The diameter of pads and vias is now derived from the drill diameter using the Design Rules (the pad and via diameter '0' is now allowed and results in a diameter that is derived from the current design rules). If a pad is defined with a diameter that exceeds the one that would result from the current design rules, the larger diameter is taken. The default value for the diameter of newly created pads and vias is now '0' to allow the Design Rules to define the actual diameters.
• Pads can have different shapes on Top and Bottom (they will always be 'round' on the inner layers).
• The via shape now only applies to the outer layers (they will always be 'round' on the inner layers).
• The diameter of pads with shape X/YLongOct now defines the smaller side of the pad (formerly the wider side). Existing files will be modified accordingly during the update.
• By default vias no longer generate Thermal symbols in supply layers. There is a new design rules parameter that enables Thermal symbols to be generated for vias in supply layers and signal polygons.
• When updating files from older versions, pads and vias with diameter <= drill will be replaced with a 'hole' of that drill diameter. This only works for unconnected pads; if a pad is connected to a pin (in a library or schematic) or to a signal (in a board) it can't be converted to a hole and the user must decide what to do in such a case. This conversion has become necessary because pads and vias now always have a 'restring' that is determined by the design rules. If a consistent board/schematic pair is updated to version 4 and such pads are replaced with holes in only one of the drawings, the board/schematic pair will become inconsistent. If that happens you will need to modify the respective package/device definition to make things consistent again.

Round SMDs

• SMDs have a new parameter "Roundness", which can range between 0 and 100 and defines the percentage by which the corners are "rounded". A value of 0 (default) results in a rectangle, while a value of 100 results in a circular shape (if the x and y dimension of the SMD are the same), which can be used for BGAs.
• The SMD command accepts roundness values as numbers with a leading '-' (to be able to distinguish it from the SMD size values).
• The CHANGE command has a new option "Roundness".

New Library structure

• What was called a "Device" in previous versions is now called a "Device Set". A "Device Set" consists of the gate definitions and several actual devices, implemented through "Package Variants"
• The PACKAGE command can now assign several different package variants to a device (as in 7400N, 7400D,...).
• The new command TECHNOLOGY can be used to define various "technology" variants for a device's package variants (as in 74LS00N, 74S00N,...).
• The CHANGE command has the new options PACKAGE and TECHNOLOGY, which can be used to select from the packages and/or technologies a device set defines. This can be done from within the schematic or board.
• The new command DESCRIPTION can be used to provide detailed textual information about a device, package or library.
• The CONNECT dialog now allows copying pin/pad connections from an other package variant. Only those package variants are offered in the "Copy from" combo box that have the same pad names as the current package variant (only connected pads are checked).
• The CONNECT dialog now asks the user if he want's to discard any changes before cancelling the dialog.
• The CONNECT command can now handle gate names that contain periods.
• The device editor now displays a list of package variants, a preview of the current package and the description of the device.
• Since it is now possible to "completely" define a device with all package and technology variants, the default setting of the "Value" parameter has been changed to "Off".
• The meaning of the "Value" parameter in a device set is now as follows:
  • "Value Off" means there is no user definable value, i.e. the value of a part is defined by the dievice name (including, if present, technology and package variant). A device like "74LS00N" would be an example.
  • "Value On" means this device needs a user defined value to be fully specified. A resistor is an example.
  Even in the "value off" case the user can (after a confirmation dialog) change a part's value to handle any special cases that might otherwise cause problems. Any CHANGE TECHNOLOGY or CHANGE PACKAGE command that is executed after such a change will set the value back to the device name.

Automatic Library update

• If a library has been modified after parts or packages from it have been added to a schematic or board, the new command UPDATE can be used to automatically update all used library objects with their latest version (see "Help Update").
• The UPDATE command can be selected from the "Library" pulldown menu in a board or schematic, or from the context menu of a library in the Control Panel. It is also possible to drag&drop a library from the Control Panel onto a schematic or board drawing and perform the update that way.

Bill Of Material

• The User Language Program 'bom.ulp' to generate the "Bill Of Material" has been rewritten. It now has a dialog in which the user can interactively generate the BOM, pulling in additional data from a user defined database file. Use "RUN bom.ulp" and click on the "Help" button for more information.

Generating Outlines for milling prototypes

• The User Language Program 'outlines.ulp' can be used to generate the data necessary to control a milling machine for generating a prototype board.

User Language

• The User Language now supports user defined dialogs as well as standard file dialogs and message boxes.
• The RUN command now accepts additional arguments that are available to the ULP as 'argc' and 'argv' parameters.
• Data can now be read into a ULP.
• The new lookup() function can be used to perform database lookups.
• The new fileglob() function can be used to do a directory search.
• The new fileerror() function can be used check for I/O errors.
• The 'exit()' function can now have a string parameter which is sent to the editor window and executed as a command string.
• ULPs can now include other ULP files with the new #include directive.
• The new #usage directive can be used to provide information about a ULP.
• The new object UL_DEVICESET is used to access device sets in a library.
• The builtin statement device() has been renamed to deviceset() to conform with the new library structure.
• UL_POLYGON has a new member 'rank'.
• UL_POLYGON has new members 'contours()' and 'fillings()' to access the calculated polygon data. The 'dxf.ulp' now uses these new members to draw the actual shape of calculated polygons.
• The new object UL_CLASS is used to access net classes.
• UL_BOARD and UL_SCHEMATIC have new members 'classes()'.
• UL_NET and UL_SIGNAL have new members 'class'.
• UL_WIRE has new members 'style' and 'pieces()'.
• UL_TEXT has a new member 'font'.
• The data members 'diameter' and 'shape' of UL_PAD and UL_VIA are now layer dependent and thus require the layer number for which the data shall be retrieved, because depending on the new Design Rules diameters and shapes of pads and vias can be different in the various layers. The syntax is now, e.g., pad.diameter[LAYER_TOP] to get the pad diameter in layer 1. Existing User Language Programs need to be edited to conform to this new syntax. See "Help UL_PAD/UL_VIA" for further details. The 'dxf.ulp' now generates the pads and vias separately in each active layer, including stopmask layers.
• The data members UL_SMD.dx and UL_SMD.dy can now have an optional layer index to retrieve the dimensions in the t/bStop and t/bCream mask layers. The 'dxf.ulp' now generates mask data if those layers are active.
• New builtin constants INT_MAX, INT_MIN, REAL_EPSILON, REAL_MAX and REAL_MIN (see "Help/User Language/Builtins/Builtin Constants").
• New data members UL_PART.deviceset, UL_DEVICESET.library, UL_DEVICE.library and UL_SYMBOL.library.
• When running a ULP the internal search path for images will now be set to the ULP's directory.
• The help page for Rich Text now contains a list of the supported image formats for the "<img...>" tag.
• The new member function UL_LAYER.used can be used in a ULP to check if a given layer is actually used in a drawing.
• The new builtin constants "path_...[]" and "used_libraries[]" can be used to determine the entries in the "Options/Directories" dialog and the currently used libraries from within a ULP. See "Help/User Language/Builtins/Builtin-Constants".
• The new mode character 'F' in the 'output()' statement of the User Language can be used to force opening a file with an otherwise protected extension (*.brd, *.sch or *.lbr).

Script files

• Script files can now call other scripts (as long as no recursive call is made).
• Script files can now contain comments. Everything after (and uncluding) a '#' character will be ignored. '#' characters inside quotes have no special meaning. Note that script labels (e.g. "BRD:") and continuation characters ('\') must not be followed by anything else than white space, and therefore can not be followed by comments (otherwise they loose their special meaning).
• The 'eagle.scr' file is now first searched for in the current project directory (which is equal to the current working directory in case there is no project open) and then in the directories listed in the Control Panel's "Options/Directories/Scripts".

Autorouter

• The Autorouter can now route "through" signal polygons (this can be controlled by the new cost factor 'cfPolygon'). A side effect of this is that a connection that has been made by the polygon before the Autorouter was started may be lost if a track generated by the Autorouter "splits" the polygon. Therefore, even if the Autorouter reaches 100%, the final result (after recalculating the polygon by RATSNEST) may be below 100%.
• The Autorouter control parameters are now stored inside the board file. They can be saved to and loaded from external files via the Autorouter dialog. Existing control files will be automatically read and stored in the board file when updating files from previous versions (the old *.ctl file then becomes obsolete and will not be read when the autorouter is started - any changes made to such a file with a text editor are ignored!).
• The Autorouter and DRC now use the same set of Design Rules. The old Autorouter parameters are stored in their corresponding DRC parameters, except for the following:
  • Instead of the separate 'mdWireDimension' and 'mdViaDimension' there is now only a single 'Copper/Dimension' parameter. This parameter will be set to the last of the two 'md*' parameters from the *.ctl file (which typically is 'mdViaDimension').
  • The 'mdWireRestrict' and 'mdViaRestrict' parameters are ignored because the minimum distance between any copper (except pads and smds) and a restrict area is now 0.
  • The 'tpViaDiameter' parameter is ignored because the actual via diameter is now generated from the via drill and the restring parameters.
  • The 'tpWireWidth' and 'tpViaDrill' parameters are stored in the default net class 0.
  When saving Autorouter control parameters to disk, the minimum distance parameters are no longer part of that file.
• There can now be any number of 'Optimize' passes. By default there are now 4 'Optimize' passes.
• Each pass can be separately activated or deactivated.
• The Autorouter can now route different wire widths and minimum distances simultaneously by using "Net Classes".
• The minimum distance parameters are no longer defined in the Autorouter dialog, but rather in the Design Rules dialog.
• The track parameters (wire width and via diameter) are now defined in the Design Rules dialog (absolute minimums) and the Net Classes dialog.
• The minimum routing grid is now 0.02mm (about 0.8mil).
• The default control parameters and the internal handling of cfChangeDir have been modified to avoid jagged tracks.
• The value 99 for the cfNonPref parameter now causes the router to completely avoid traces that are not in the preferred direction of the respective layer. You should carefully decide if this behaviour is really what you want. To avoid unexpected effects with existing boards, the value 99 will be silently changed to 98 when updating older files.
• With very small routing grids the Autorouter sometimes routed a little bit too close towards round pads/vias.
• Sometimes the autorouter didn't go through a gap where, according to the actual widths and minimum distances, it should have.

ADD command

• The ADD command can now be used with wildcards ('*' or '?') to find a specific device. The ADD dialog offers a tree view of the matching devices, as well as a preview of the device and package variant.
• To add directly form a specific library, the command syntax

         ADD devicename@libraryname
      

  can be used. 'devicename' may contain wildcards and 'libraryname' can be either a plain library name (like "ttl" or "ttl.lbr") or a full file name (like "/home/mydir/myproject/ttl.lbr" or "../lbr/ttl").
• If a device or package shall be added, and there is already such an object (with the same name from the same library) in the drawing, an automatic library update will be performed which replaces the existing object in the drawing with the current version from the library.
• The new command UPDATE can be used to update all parts in a board or schematic with modified library versions (see "Help Update").
• The ADD command can now fetch a particular gate from a device, without automatically fetching the MUST and ALWAYS gates, too.

CHANGE command

• CHANGE LAYER for wires and polygons now works between any layers within packages and symbols.

CONNECT command

• Pressing the SPACE key in the CONNECT dialog while a list element has the focus will now perform the 'connect' or 'disconnect' action, respectively.

DELETE command

• If the last supply symbol of a given type is deleted from a net segment that has the same name as the deleted supply pin, that segment is now given a newly generated name (if there are no other supply symbols still attached to that segment) or the name of one of the remaining supply symbols.
• The DELETE command now deletes an entire part when clicking on a gate with the Shift key pressed. In that case, the wires connected to the element in the board will not be ripped up.
• The DELETE command now deletes the entire polygon when clicking on a polygon wire with the Shift key pressed.
• The DELETE command now deletes the entire net or bus segment when clicking on a net or bus wire with the Shift key pressed.
• Net segments connected to a bus now keep their name when splitting segments.

DISPLAY command

• The new parameters '?' and '??' can be used to control what happens if a layer that is given in a DISPLAY command does not exist in the current drawing. See "Help Display" for details.

GROUP command

• If the selected group is empty, the GROUP command no longer displays a message box saying "Group is empty". It rather prompts that message in the status bar (with a beep) and stays active for a new group definition.

ERC command

• The ERC now lists the package names when reporting parts/elements with inconsistent packages.
• The ERC now detects inconsistencies between the implicit power and supply pins in the schematic and the actual signal connections in the board. Such inconsistencies can occur if the supply pin configuration is modified after the board has been created with the BOARD command. Since the power pins are only connected "implicitly", these changes can't always be forward annotated. If such errors are detected, forward-/backannotation will still be performed, but the supply pin configuration should be checked!
• The ERC now checks for missing junctions and overlapping wires and pins.
• The ERC now reports uninvoked MUST gates as errors.
• The ERC now reports an error if supply pins with the same name are overwritten with more than one signal.

ERRORS command

• The ERRORS dialog is no longer modal (it stays "on top" of the editor window) and can be kept open while resuming normal editing in the editor window.
• The various error types are now listed more detailed.

EXPORT command

• The EXPORT can now export image files (BMP, PNG, etc.). See "Help/EXPORT" for details.
• The EXPORT SCRIPT command now sets the grid unit to 'mm' if the current grid isn't metric, in order to avoid loss of precision.

INFO command

• The INFO command now displays the layer name.
• The INFO command now displays the VIA diameter separately for outer and inner layers (as determined by the Design Rules), plus the value that has been originally defined by the user.

LAYER command

• The new option '??' can be used to suppress error messages when deleting a layer.

NET and BUS command

• If a net wire is placed at a point where there is already another net or bus wire or a pin, the current net wire will be ended at that point (in previous versions the user had to click twice to end a net wire). The same applies to a bus wire that is placed at a point where there is already another bus wire. This function can be disabled with "SET AUTO_END_NET OFF;", or by unchecking "Options/Set/Misc/Auto end net and bus".
• If a net wire is placed at a point where there are at least two other net wires and/or pins, a junction will automatically be placed. This function can be disabled with "SET AUTO_JUNCTION OFF;", or by unchecking "Options/Set/Misc/Auto set junction".

OPTIMIZE command

• The OPTIMIZE command now also optimizes the "flat" wires in a board (i.e. those not being part of a signal).

PACKAGE command

• The PACKAGE dialog now accepts an empty "Variant name" field and no longer requires the explicit entry of '' (two single quotes) to define a package variant with an "empty" name.

PASTE command

• When pasting objects into a drawing that already contains earlier (different) versions of these objects, an automatic library update will be performed which replaces the existing objects in the drawing with the new versions from the paste buffer.

PRINT command

• The PRINT dialog's "Page setup" now allows border values that are smaller than the initial values derived from the printer driver. To get back to the original default you can enter '0'. Note, though, that your actual printer may not be able to print that close to the page limits.
• The printer settings are no longer stored in the project file, but are now stored in the user parameters ('eaglerc').
• Version 3.5 stored the binary printer setup in the Windows registry in order to remember which printer was last used in EAGLE. This, however, has frequently caused problems, sometimes even total system crashes. As of version 4 EAGLE (like most other Windows applications) no longer stores the used printer and always starts up with the system default printer.

REMOVE command

• The REMOVE command can now handle device, symbol and package names with extension (for example REMOVE name.pac). If the name is given without extension, you have to be in the respective mode to remove an object (i.e. editing a package if you want to remove packages).

RENAME command

• The RENAME command now allows '.' in names.
• The RENAME command can now handle device, symbol and package names with extension (for example RENAME name1.pac name2[.pac] - note that the extension is optional in the second parameter). If the first parameter is given without extension, you have to be in the respective mode to rename an object (i.e. editing a package if you want to rename packages).

REPLACE command

• The REPLACE command can no longer be used with active forward- and backannotation. This is due to the now complete definition of a device set with all its package variants. Use the CHANGE PACKAGE command to select one of the defined package variants, or use the UPDATE command to update a package with a modified version from the same library.

SET command

• The SET options for Thermal and Annulus parameters as well as the Solder Stop and Cream mask data have been removed. These values are now defined in the Design Rules.
• The SET variables DRC_SHOW and DRC_COLOR are now obsolete (progress in the Design Rule Check is now displayed in a progress bar).
• The SET variable MAX_ERROR_ZOOM is now obsolete. The ERRORS dialog is no longer modal (it stays "on top" of the editor window) and zooming can be done with the usual WINDOW commands or buttons.

SHOW command

• Highlighted objects are now kept highlighted during subsequent window operations.
• Pressing ESCape in the SHOW command now lowlights the currently highlighted object.

TECHNOLOGY command

• The TECHNOLOGY command no longer asks before removing a Technology from a device.

USE command

• The USE command is now mainly for use in script files.
• The actually used libraries can now be comfortably selected in the Control Panel.

WIRE command

• In order to speed up execution of large scripts that produce many wires, 'Set Optimizing Off' now also disables automatic wire splitting in scripts.

CAM Processor

• The CAM Processor no longer supports matrix printers. Use the PRINT command to print to the system printer.
• The command line option -I is no longer available, since the CAM Processor can now be used freely in the Freeware version.
• Output is now only possible into files. If data shall be sent to a COM or LPT port under Windows the UNC filename of a queue attached to that port has to be used.
• If the "Section" text in a CAM Processor section consists of a string like "Title: Descriptive text...", the "Title" will appear on the section's tab, while the "Descriptive text..." will only be visible in the "Section" field.
• CAM Processor jobs can now have a description.
• The diameter of octagonal pads in RS274-X has been increased by a factor of 1.08239 to compensate for the different interpretation of pad diameters in EAGLE and RS274-X.
• Wires are no longer shortened in the CAM Processor in order to keep the drills open. Only devices that can actually remove pixels from the output can now keep the drills open (currently only the Postscript devices "PS" and "EPS" can do this).
• The new CAM Processor device PS_INVERTED can be used to produce inverted Postscript output.

Parameter storage

• User specific parameters are now stored in an "eaglerc" file. At program start, parameters are read (in the given sequence) from the files

        prgdir/eaglerc                 (Linux and Windows)
        /etc/eaglerc                   (Linux only)
        $HOME/.eaglerc                 (Linux)
        $HOME/eaglerc.usr              (Windows)
      

  where prgdir means the directory that contains the EAGLE program file. If no environment variable HOME is defined, the prgdir will be used instead. When the program ends, the current values of all parameters (if any of them have changed) are written to the eaglerc file in the HOME directory. Under Linux "$HOME" stands for the environment variable HOME. Under Windows "$HOME" is either the environment variable HOME (if set) or the value of the registry key "HKEY_CURRENT_USER\Software\Microsoft\ Windows\CurrentVersion\Explorer\Shell Folders\Personal", which contains the actual name of the "My Documents" directory.
• The file 'eagle.cfg' is not read any more.
• Key assignments made with the ASSIGN command are now stored in the user specific parameters.

Command line options

• The options '-A' and '-T' are now obsolete (thermal and annulus data is now defined in the Design Rules).
• The options '-B' and '-M' are now obsolete (solder stop and cream mask data is now defined in the Design Rules).
• The option '-C' is now obsolete, since the CAM Processor no longer supports matrix printers (all printing is done with the PRINT command).
• The options '-Z' and '-Y' are now obsolete (drill symbols are configured in "Options/Set/Drill" and are stored in the user specific "eaglerc" file).

Miscellaneous

• The DOS and OS/2 platforms are no longer supported.
• Due to changes in the file data structure you will most likely be asked whether to run the ERC when loading a board/schematic pair created with an earlier version of EAGLE.
• Files from earlier versions of EAGLE may contain library objects with the same names. This was caused by PASTE or ADD operations with modified devices or packages. Version 4 no longer allows this to happen, and therefore needs to make sure updated files do not contain multiple objects with the same name. In order to assure this, the update routine adds the '@' character and a number to the names of such library objects.
• The library editor can now edit devices and symbols, even if the user's license does not contain the schematic module.
• Avoiding multiple 'Save?' prompts for boards and schematics that are connected via f/b annotation.
• When a file is modified while updating from a previous version the resulting update report is now presented in a separate text window.
• Improved selectability of arcs.
• The vector font characters '&', '@' and '~' have been improved.
• Junctions are now also set automatically when a part is placed, and they will be automatically deleted if a part or a net wire is deleted.
• Improved speed of CAM Processor.
• NET and SIGNAL commands are no longer terminated when cancelling a 'Connect...?' dialog.
• Pad and via drill holes are no longer subtracted from polygons.
• Polygons that would completely disappear after being calculated with RATSNEST are now shown on the screen with their original outlines. This allows editing or deleting them.
• The string edit dialog now adjusts its width to completely show longer strings (for instance when editing a long bus name).
• Command text buttons (defined with the MENU command) now stay pressed to indicate the currently active command (this does not apply to buttons that result in a submenu).
• The Windows file dialog no longer checks for the existence of a file, thus allowing the user to leave out the filename extension when typing in a file name.
• The command button groups are now separated by horizontal lines, which saves space in the command menu.
• The default value for the solder stop mask ("Edit/Design rules/Masks/Stop") has been changed to a fixed value of 4mil.
• The size of SMD names displayed when SET PAD_NAMES is on is now limited to 20mil.
• The "Description" field in the library editor and the right pane in the Control Panel can now be completely minimized with the splitter.
• If a package variant or technology is no longer there (e.g. because it has been deleted or renamed) the user can now select a different one in the library update.
• The automatic unit determination in dialog input fields can now be controlled by adding the line

      Interface.PreferredUnit = "x"
      

  to the eaglerc file, where "x" can be
  "0" for automatic unit determination (default)
  "1" for imperial units
  "2" for metric units.
• The 'dxf.ulp' now has radio buttons to choose the unit of the generated data ('mm' or 'inch'), and outputs data in 'mm' with 4 decimal digits instead of 3.