What's new in version 4.0?
Here's a list of all the new features and modifications in EAGLE 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.
- 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
- 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
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"
- 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
- 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).
- 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.
- 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
- 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.
- 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.
- 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
- 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
- Due to a calculation problem the DRC sometimes reported very small errors where in
reality there were no errors.
- 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
- Bus member names can now contain any characters, except ':', ',', '[', ']' and blanks.
- 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.
- 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'
- 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
- The via shape now only applies to the outer layers (they will always be 'round' on the
- 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.
- 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
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.
- The User Language now supports user defined dialogs as well as standard file dialogs and
- 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
- 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
- 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
- When running a ULP the internal search path for images will now be set to the ULP's
- The help page for Rich Text now contains a list of the supported image formats for the
- 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
- 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 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".
- 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
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 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 LAYER for wires and polygons now works between any layers within packages and
- Pressing the SPACE key in the CONNECT dialog while a list element has the focus will now
perform the 'connect' or 'disconnect' action, respectively.
- 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
- 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.
- 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.
- 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.
- The ERC now lists the package names when reporting parts/elements with inconsistent
- 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
- 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.
- 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.
- The EXPORT can now export image files (BMP, PNG, etc.). See "Help/EXPORT" for
- 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.
- 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
- 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
- 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
- The OPTIMIZE command now also optimizes the "flat" wires in a board (i.e.
those not being part of a signal).
- 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
- 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.
- 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
- 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
- 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
- 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.
- 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.
- Highlighted objects are now kept highlighted during subsequent window operations.
- Pressing ESCape in the SHOW command now lowlights the currently highlighted object.
- The TECHNOLOGY command no longer asks before removing a Technology from a device.
- The USE command is now mainly for use in script files.
- The actually used libraries can now be comfortably selected in the Control Panel.
- In order to speed up execution of large scripts that produce many wires, 'Set Optimizing
Off' now also disables automatic wire splitting in scripts.
- 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
- 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
- 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)
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
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"
- 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
- 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
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.
Cadsoft Main Page |
Back to Testech Home Page