|
|
|
What's new in version 4.1?
Here's a list of new features and modifications in EAGLE version 4.1
The list of changes in version 4.0 can be found here.
If you have an EAGLE license for version 4.0 or earlier, please contact
your local dealer for an update.
Changes that are available only as of release 4.13 are shown in different color.
Platforms
- EAGLE now also runs on Mac OS X (with X11).
Library Management
- Packages and Device Sets can now be copied into the currently edited
library from other libraries, either through Drag&Drop from the Control
Panel or by using the COPY command's new extended syntax (see "Help Copy").
- New package variants can now be created by directly using packages from
other libraries, either through Drag&Drop from the Control Panel or by
using the PACKAGE command's new extended syntax.
- The packages of the currently edited library can now be updated with those
from other libraries, either through Drag&Drop from the Control Panel or
by using the UPDATE command's new extended syntax.
Blind & buried vias
- The program can now handle so-called "blind & buried" vias. "Blind" vias
are those that are not drilled all the way through the current layer stack.
"Buried" vias are produced by drilling through the entire current layer
stack. Vias that go all the way through the complete board are basically
the same as "buried" vias, but sometimes are also referred to as "through"
vias. "Micro vias" are small blind vias that go from one layer to the next
inner layer. These are typically used to connect SMD pads to an inner layer,
without having to run a wire away from the SMD.
- The Design Rules dialog now has a new tab named "Layers", in which the
layer setup can be defined. The minimum drill size and aspect ratio for
blind vias can be defined on the "Sizes" tab.
- When updating an existing board from an older version, the layer setup
will be determined by the layers that are actually in use (either because
there are objects in them, or they are supply layers, or they are used by
the Autorouter setup). The layer stack will consist of a sequence of
"core" and "prepreg" material (with the thickness of the individual layers
chosen so that the final board results in a thickness between 1mm and 1.5mm),
and which allows a via that goes through all layers.
After loading an old board into this version you should verify the layer
setup in the Design Rules and adjust it to your actual needs.
- The DISPLAY and LAYER dialogs (and related combo boxes) will only display
those signal layers that are used in the layer setup.
- The CHANGE LAYER and ROUTE command only set the minimum necessary vias
(according to the layer setup in the Design Rules). It may happen that an
already existing via of the same signal is extended accordingly, or that
existing vias are combined to form a longer via if that's necessary to
allow the desired layer change.
- The VIA command has a new parameter that defines the layers this via shall
cover. The syntax is from-to, where 'from' and 'to' are the layer numbers
that shall be covered. For instance 2-7 would create a via that goes from
layer 2 to layer 7 (7-2 would have the same meaning). If that exact via is
not available in the layer setup of the Design Rules, the next longer via
will be used (or an error message will be issued in case no such via can be
set).
- The Autorouter cannot work with supply layers and non-through vias at the
same time. In such cases you need to replace the supply layers with signal
polygons accordingly.
- The CHANGE command has a new option named VIA, which can be used to change
the layers a via covers. The syntax is
CHANGE VIA from-to *
where 'from' and 'to' are the layer numbers the via shall cover. If that
exact via is not available in the layer setup of the Design Rules, the
next longer via will be used (or an error message will be issued in case
no such via can be set).
- The User Language object UL_VIA, now has two new data members 'start' and
'end', which return the layer numbers in which that via starts and ends.
The value of 'start' will always be less than that of 'end'. Note that the
data members 'diameter' and 'shape' will always return the diameter or shape
that a via would have in the given layer, even if that particular via doesn't
cover that layer (or if that layer isn't used in the layer setup at all).
- The DRC now checks whether all vias and objects in signal layers correspond
to the actual layer setup. If they don't, a "Layer Setup" error is flagged.
- If the layer setup of a board contains blind or buried vias, the CAM
Processor generates a separate drill file for each via length that is
actually used in the board (see "CAM Processor").
- The DRC performs new checks for blind vias: vias that don't pass the check
against the "Minimum Drill" parameter and are blind vias that are exactly
one layer deep (so-called "micro vias") are checked against the "Min.
Micro Via" parameter. Blind vias that pass these tests will further be
checked to see whether they have a drill diameter that conforms to the
"Min. Blind Via Ratio" parameter in "Edit/Design Rules/Sizes".
Arbitrary angles
- Texts and elements in a board context can now be rotated by any angle,
in steps of 0.1 degrees (see "Help Add" for a description of the
"orientation" flags).
- The new "Spin" flag in orientations can be used to disable the function
that keeps texts readable from the bottom or right side.
- Pads and SMDs can now be placed with arbitrary angles.
Arcs and Wires
- In many aspects Arcs are now treated the same way as Wires. They are
part of a signal when drawn in a signal layer, they can be used when
drawing a polygon, and they now also have a wire style.
- The endings of arcs can now be either round or flat. You should use
flat arc endings only when absolutely necessary (round endings have
advantages when generating, e.g., Gerber files).
- The end points of an arc can now be moved independently, just like those
of wires. When moving such points, the radius of the arc will be scaled
accordingly.
- All commands that draw wires can now draw arcs by using the new 'curve'
or '@radius' parameter (see "Help/Editor Commands/WIRE").
- There are no more 'arcs()' loop members in the User Language. Any ULPs
that used to loop through arcs must now check the new data member
UL_WIRE.arc when looping through the wires (see "Help/User Language/Object
Types/UL_WIRE"). The "User Language" section below contains an example
that shows how to adapt existing ULPs.
- The new command MITER can be used to take the edge off wire joins
(see "Help Miter").
- The wire bend styles 0, 1, 3 and 4 now use an additional miter radius as
defined with the MITER command.
Additional flags for pads, vias and smds
- Pads, Vias and SMDs now have additional flags that control the generation
of the stop and cream masks, the thermals and the shape of the "first" pad
within a package.
- The User Language objects UL_PAD, UL_VIA and UL_SMD have a new data member
'flags', which returns the setting of these flags (see "Help/User
Language/Object Types/UL_PAD", "Help/User Language/Object Types/UL_VIA" and
"Help/User Language/Object Types/UL_SMD").
- The PAD and SMD commands support the new options NOSTOP, NOTHERMALS,
NOCREAM, and FIRST, respectively, to define these flags. The VIA command
supports the new option STOP.
- The CHANGE command has the new options STOP, CREAM, and FIRST to modify
these flags (the THERMALS option already exists).
User definable colors
Control Panel
- The tree view in the Control Panel can now be sorted by 'name' or by
'type' via the pulldown menu option "View/Sort".
- The Control Panel's pulldown menu option "File/Refresh tree" has been
moved to "View/Refresh".
- Directory entries in the Control Panel's tree view which can contain
libraries now all have the "Use all" and "Use none" options in their
context menus.
- New context menu options for libraries, device sets and packages as well
as Drag&Drop features for copying and updating library objects, and for
creating new package variants.
- Drag&Drop of a board, schematic or library file into the appropriate
editor window now loads the file into that window for editing. The
previous functionality of performing a library update when dropping a
library into any editor window has been removed.
- The Control Panel now has a new menu item "File/Open recent projects".
Design Rules
- The new Design Rule parameters Shapes/Elongation can be used to define
the elongation of Long and Offset shaped Pads. Valid values are from 0 to
200, where 0 results in a regular octagon shape (no elongation) and 100
gives you a side ratio of 2:1 (100% elongation), which is the ratio that
has been hard-coded in previous program versions.
- The Design Rules dialog now has a new tab named "Layers", which defines
the layer setup for multilayer boards (see "Help/Design Checks/Design Rules").
- The Design Rules tab "Shapes" contains a new combo box named "First", which
defines the shape of the "first" pad within a package.
- The Design Rules tab "Sizes" contains the two new parameters "Min. Micro Via"
and "Min. Blind Via Ratio".
- The Design Rules tab "Restring" contains a new set of restring parameters
for micro vias.
- Increased the maximum copper thickness in the layer setup of the Design
Rules to 1mm.
User Language
- The User Language member functions UL_PAD.shape and UL_VIA.shape now return
PAD_SHAPE_ANNULUS, PAD_SHAPE_THERMAL, VIA_SHAPE_ANNULUS and
VIA_SHAPE_THERMAL, respectively, if their shape is requested for a supply
layer (see Help/User Language/Object Types/UL_PAD and UL_VIA).
- The User Language dialog object dlgListView now accepts a new parameter
that defines the column and direction to use for sorting.
- The User Language functions strchr(), strstr(), strrchr() and strrstr()
now accept an 'index' parameter to start the search at a given position.
- Opening the same file concurrently in two output() statements in a User
Language Program is now treated as an error.
- The User Language objects UL_HOLE, UL_PAD and UL_VIA now have a new
data member 'drillsymbol'.
- A User Language Program can now be aborted even if it is currently
executing a lengthy 'for' or 'while' loop.
- The new ULP function status() can be used to display a message in the
editor window's status bar.
- The User Language dialog function dlgTextView now accepts a second
parameter to support hyperlinks in Rich Text (see "Help/User
Language/Dialogs/Dialog objects/dlgTextView()").
- The User Language dialog function dlgMessageBox can now add an icon
to the message box by prepending the message string with one of the
characters '!', ';' or ':' (see "Help/User Language/Dialogs/Predefined
Dialogs/dlgMessageBox()").
- Due to the implementation of arbitrary angles and "spin" the following new
member functions have been added to the User Language:
UL_PAD.angle, UL_SMD.angle, UL_RECTANGLE.angle, UL_ELEMENT.angle,
UL_ELEMENT.spin and UL_TEXT.spin.
Make sure you take these into account in your own ULPs as necessary,
otherwise boards containing objects with these new features may be handled
incorrectly. See the 'dxf.ulp' for an example.
- Due to the modifications of pad shapes, the User Language constants
PAD_SHAPE_XLONGOCT and PAD_SHAPE_YLONGOCT have been replaced with
PAD_SHAPE_LONG, and the new constant PAD_SHAPE_OFFSET has been introduced.
- The new User Language member function UL_PAD.elongation returns the
elongation value for pads with shapes Long or Offset.
- The User Language object UL_VIA, now has two new data members 'start' and
'end', which return the layer numbers in which that via starts and ends.
The value of 'start' will always be less than that of 'end'. Note that the
data members 'diameter' and 'shape' will always return the diameter or shape
that a via would have in the given layer, even if that particular via doesn't
cover that layer (or if that layer isn't used in the layer setup at all).
- Due to the implementation of different arc cap styles the member function
UL_ARC.cap has been added to the User Language.
- The loop member functions UL_BOARD.arcs(), UL_PACKAGE.arcs(), UL_SHEET.arcs()
and UL_SYMBOL.arcs() no longer exist, since arcs are now treated a lot like
wires. Any ULPs that used to loop through arcs must now check the new data
member UL_WIRE.arc when looping through the wires (see "Help/User
Language/Object Types/UL_WIRE").
To convert an existing ULP that uses the arcs() loop member functions
consider the following example:
Assume you have a ULP that looks like this:
void ProcessArc(UL_ARC A) { /* do something with the arc */ }
void ProcessWire(UL_WIRE W) { /* do something with the wire */ }
board(B) {
B.arcs(A) ProcessArc(A);
B.wires(W) ProcessWire(W);
}
To make it run with EAGLE version 4.1 you need to eliminate the 'arcs()'
call and move the actual arc processing into the ProcessWire() function:
void ProcessArc(UL_ARC A) { /* do something with the arc */ }
void ProcessWire(UL_WIRE W)
{
if (W.arc)
ProcessArc(W.arc);
else
/* do something with the wire */
}
board(B) {
B.wires(W) ProcessWire(W);
}
Note that you only need this explicit handling of arcs if you actually
need to gain access to parameters only the UL_ARC can provide. If you are
not interested in that kind of information, you can handle the arcs just
like ordinary wires, using the parameters the UL_WIRE provides.
- To be able to handle any UL_ARC on UL_WIRE level the UL_WIRE object now
has the two additional members 'cap' and 'curve'.
- The User Language objects UL_PAD, UL_VIA and UL_SMD have a new data member
'flags', which returns the setting of the flags that control mask and
thermal generation (see "Help/User Language/Object Types/UL_PAD",
"Help/User Language/Object Types/UL_VIA" and "Help/User Language/Object
Types/UL_SMD").
- The User Language object UL_HOLE has a new data member 'diameter[]' which
returns the diameter of the solder stop masks.
- The output() statement in a User Language Program now supports the new
mode character 'D', which causes the file to be automatically deleted at
the end of the EAGLE session (see "Help/User Language/Builtins/Builtin
Statements/output()").
- The User Language object UL_GRID now has an additional data member named
'unitdist', which returns the grid unit that was used to define the actual
grid distance (see "Help/User Language/Object Types/UL_GRID).
- The new User Language function language() can be used to internationalize
ULPs (see "Help/User Language/Builtins/Builtin Functions/Miscellaneous
Functions/language()").
- The User Language directive #usage can now handle internationalized
texts (see "Help/User Language/Syntax/Directives/#usage").
- The new User Language directive #require can be used to tell the user that
a ULP requires at least the given version of EAGLE (see "Help/User
Language/Syntax/Directives/#require").
Autorouter
- The Autorouter no longer attempts to route within the borders of the
signal's surrounding rectangle first, because that way it sometimes was
forced to take an "expensive" path, which it would have avoided if it
had been allowed to use the entire board area in the first place. This
may cause longer routing times in some cases, but may just as well speed
up the routing, especially on complex boards.
- The Autorouter now optionally runs even if a signal layer that contains
objects is not activated.
- When routing from a pad that covers more than one raster point, the
Autorouter now tries to lay out the wire at the middle of the pad.
- The Autorouter now applies the cfSmdImpact parameter to SMDs that are
placed at angles of 45, 135, 225 or 315 degrees.
CAM Processor
Text editor
- Setting the font in a text editor window is now done via the pulldown
menu option "File/Font..." and no longer via the printer setup. The
selected font is now also used in the text editor window.
ADD command
- The ADD command now mirrors the object that is attached to the cursor
when the center mouse button is pressed.
- Changed the meaning of the wildcards ('*' and '?') in the ADD command.
They used to match [a-z0-9_] and will now match any non-whitespace
character.
- The ADD dialog now has a checkbox that allows the pattern search in the
descriptions to be turned off.
ARC command
- Arcs are now part of a signal if drawn in a signal layer of a board.
When updating an existing board drawing, arcs in signal layers are
transferred into signals (either newly generated ones or the ones that
the arcs are apparently connected to by sharing the same end points).
- The ARC command now accepts a signal name (just like the WIRE command).
- The endings of arcs can now be either round or flat (the ARC command
therefore accepts the new parameters ROUND and FLAT).
When updating an existing drawing, the 'cap' parameter of all arcs in
boards, packages and symbols, that have their endings covered by other
objects (like wires or vias) will be set to 'round'. This allows them
to be drawn more easily on the various output devices.
BUS command
- The BUS command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/BUS").
BOARD command
- The BOARD command now places elements in the third and, if necessary,
fourth quadrant of the newly created board in case there are too many
of them to fit into the second quadrant.
CHANGE command
- When changing the layer of a signal wire, only the minimum necessary
via will be set (according to the layer setup in the Design Rules). It may
happen that an already existing via of the same signal is extended
accordingly, or that existing vias are combined to form a longer via if
that's necessary to allow the desired layer change.
- The CHANGE command has a new option named VIA, which can be used to change
the layers a via covers. The syntax is
CHANGE VIA from-to *
where 'from' and 'to' are the layer numbers the via shall cover. If that
exact via is not available in the layer setup of the Design Rules, the
next longer via will be used (or an error message will be issued in case
no such via can be set).
- The CHANGE command can now change the cap style of arcs by using
CHANGE CAP ROUND | FLAT
- The CHANGE command has the new options STOP, CREAM, and FIRST to modify
the new pad/smd flags (the THERMALS option already exists).
- The parameters Spacing and Isolate in the CHANGE popup menu now present
a list of predefined values (just like, for instance, the Width parameter).
All such popup menus now contain the entry "..." at the bottom, which
brings up a dialog to enter a new value.
COPY command
- The COPY command can now copy parts in a schematic (see "Help Copy").
- The COPY command can now copy packages and device sets from other
libraries into the currently edited library (see "Help Copy").
- The COPY command now mirrors the object that is attached to the cursor
when the center mouse button is pressed.
DELETE command
DISPLAY command
DRC command
- The DRC now checks for objects in the Pads and Vias layer that are not
Pads or Vias (i.e. wires, rectangles etc.) and flags them as "Layer Abuse"
errors. The reason for this is that EAGLE does not handle these object
in any special way, so they might cause short circuits. If you get such
an error from the DRC, you should move the object in question into the
proper signal layer(s).
- The DRC now checks objects in the t/bKeepout layers only if the
respective layer is activated.
- The DRC now checks whether all vias and objects in signal layers correspond
to the actual layer setup. If they don't, a "Layer Setup" error is flagged.
- The new options LOAD and SAVE in the DRC command can be used to load the
Design Rules from or save them to a given file.
- The DRC no longer checks objects that have no electrical potential (like
wires in packages, rectangles, circles and texts) against each other for
clearance errors.
- The DRC dialog now has a 'Check' button instead of 'OK'.
- The DRC no longer checks polygons in packages against objects that have no
electrical potential for clearance errors.
EXPORT command
- The EXPORT IMAGE command can now create TIFF files.
GRID command
- The GRID command accepts the new option 'alt', which allows you to define
an "alternate" grid that will be used whenever you press the Alt key while
selecting or moving objects. The alternate grid can have its own size and
unit, and is typically used to temporarily switch into a finer grid if the
normal grid is too coarse. See "Help/Editor Commands/GRID".
- The GRID dialog has been changed to allow the user to enter the alternate
grid parameters.
INFO command
- The INFO command now also displays the data of the part when selecting a
text from a smashed part.
INVOKE command
- The INVOKE command now mirrors the object that is attached to the cursor
when the center mouse button is pressed.
MIRROR command
- The MIRROR command now accepts the name of an element in a board, just
like the MOVE command.
MITER command
- The new command MITER can be used to "take the edge off" wire joins
(see "Help Miter").
- Changed the default values for "miter radius" to some typical grid values.
MOVE command
- When picking up an object with the MOVE command, the status line now
displays the same information as the SHOW command (currently this only
works if the "User guidance" is turned off).
- If an Arc is selected at one of its end points, that point can now be moved
freely (just like that of a Wire). The Radius of the Arc is then scaled
accordingly.
- The MOVE command now mirrors the object that is attached to the cursor
when the center mouse button is pressed.
- The MOVE command can now select objects at their origin by pressing the
Ctrl key (see "Help/Editor Commands/MOVE").
- Moving texts of a smashed part now draws a line to the part's origin
so that the user can see which part this text belongs to.
NET command
- The NET command now displays information about the current net in the
status line.
- The NET command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/NET").
- When drawing a net wire that connects two segments of different nets, the
question "Connect Nets?" was changed to "Connect Net Segments?" in order
to make it clear that only the two segments involved are concerned, and
not the entire nets.
PACKAGE command
- The PACKAGE command can now create package variants with packages from
other libraries (see "Help Package").
PAD command
- The PAD command can now create pads with arbitrary angles and therefore
accepts an "orientation" parameter (See "Help Pad").
- The pad shapes XLongOct and YLongOct have been renamed to Long. When
updating an existing drawing from a previous version, XLongOct pads will
be converted to Long pads with an angle of 0 degrees, and YLongOct pads
will become Long with 90 degrees.
- The new pad shape "Offset" can be used to have pads that have the shape as
defined by Long, but extend only to one side.
- The PAD command supports the new options NOSTOP, NOTHERMALS and FIRST to
define the new 'flags' (see "Help/Editor Commands/PAD").
PASTE command
- The PASTE command now mirrors the object that is attached to the cursor
when the center mouse button is pressed.
POLYGON command
- The 'width' and 'layer' can now be changed at any time while drawing a
polygon.
- The POLYGON command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/POLYGON").
PRINT command
- The selected printer, paper size and orientation are now also saved and
restored under Windows.
RATSNEST command
- The RATSNEST command now processes all points of a signal, even if that
signal is very complex (in previous versions it dropped wire end points
from processing if the total number of connection points exceeded 254).
This requires more memory when calculating the ratsnest. In case this
is a problem on your system, you can revert to the original method
by appending the line
Option.RatsnestLimit = "254"
to the eaglerc file. The value given
here is the number of connection points up to which all wire end points
will be taken into account and thus limits the amount of memory used
(processing will use up to the square of this value in bytes, so a value
of 1024 will limit the used memory to 1MB). A value of "0" means there is
no limit. A value of "1" will result in airwires being connected only to
pads, smds and vias.
- RATSNEST no longer marks the board drawing as modified, since the
calculated polygon data (if any) is not stored in the board, and the
recalculated airwires don't really constitute a modification of the drawing.
- Unnecessary thermal stubs that could occur around pads, vias and smds when
calculating signal polygons are now avoided. Note that due to this
modification there may be cases where a pad, via or smd that used to be
considered connected to the polygon is now no longer actually connected
and the RATSNEST command will generate an airwire.
WARNING: If you send a board file created with this version of EAGLE to
a boardhouse for manufacturing, and they will produce the CAM data
themselves, please make sure that they use EAGLE version 4.11r05 or higher.
Otherwise the manufactured board may contain thermal stubs even though
you didn't see them in your version of EAGLE.
RENAME command
- If the RENAME command is entered without any additional parameters in
a package, symbol or device drawing, a dialog now pops up that requests
the input of the new name for this object.
ROTATE command
- The ROTATE command now accepts an "orientation" parameter (e.g. SMR359.9).
- The ROTATE command now accepts the name of an element in a board, just
like the MOVE command.
- The ROTATE command can now be used with Click&Drag to rotate objects or
groups by any angle (see "Help Rotate").
ROUTE command
- The ROUTE command now dynamically recalculates the current airwire while
routing. In doing so, it also takes into account points along a wire, if
those are closer to the cursor than the ends of that wire. If there is
a pad, via or smd that is at most Snap_Length away from the end of the
airwire (in the current layer), that end will now snap to the center of
the object.
- The ROUTE command no longer automatically sets a Via at the end point
of a wire. If you want to place a Via at the end point of a routed wire
you can do so by holding the Shift key down while clicking at the end
point.
- When determining the layer in which to route, the ROUTE command now also
considers Wires (not only SMDs).
- When changing the layer in the ROUTE command, only the minimum necessary
via will be set (according to the layer setup in the Design Rules). It may
happen that an already existing via of the same signal is extended
accordingly, or that existing vias are combined to form a longer via if
that's necessary to allow the desired layer change.
- The ROUTE command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/ROUTE").
- The ROUTE command now creates a new airwire if necessary when Ctrl is
pressed while selecting the starting point (see "Help/Editor Commands/ROUTE").
SET command
- The SET USED_LAYERS command also takes into account the layers from the
new multilayer setup in the Design Rules and keeps them in the menus.
- The SET WIRE_BEND command accepts the two new values 5 and 6 to define
bend styles that start or end in a 90 degree arc, plus the new value 7
for a bend style that results in an arc that exactly fits to the wire at
the starting point. If there isn't exactly one wire at the starting point,
a straight wire is drawn. This bend style can be used to draw wires in sort
of a "freehand" way.
- The special character '@' can be used with the SET WIRE_BEND command to
define which bend styles shall actually be used when switching with the
right mouse but (as in SET WIRE_BEND @ 1 2 4 5;).
- The SET command now restores the program default values for the parameter
menus when executed as, for instance,
SET WIDTH_MENU;
(i.e. without any values). This applies to all *_WIDTH parameters.
SHOW command
- The SHOW command now displays the net class (in case of a net or signal)
and the gate name (in case of a multi gate part).
SMASH command
- The SMASH command can now be applied to a GROUP.
- Pressing the Shift key while clicking on a part or group with the SMASH
command will now "un-smash" the object.
- The >PART and >GATE parameters are now also smashed.
SMD command
- The SMD command supports the new options NOSTOP, NOTHERMALS and NOCREAM to
define the new 'flags' (see "Help/Editor Commands/SMD").
SPLIT command
- The SPLIT command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/SPLIT").
UPDATE command
- The UPDATE command can now update packages in a library (see "Help Update").
- The UPDATE command's new syntax 'old_library_name = new_library_name' can
be used to update a library in a board or schematic with the contents of
an other library (see "Help Update").
VIA command
- The VIA command has a new parameter that defines the layers this via shall
cover. The syntax is from-to, where 'from' and 'to' are the layer numbers
that shall be covered. For instance 2-7 would create a via that goes from
layer 2 to layer 7 (7-2 would have the same meaning). If that exact via is
not available in the layer setup of the Design Rules, the next longer via
will be used (or an error message will be issued in case no such via can be
set).
- The VIA command supports the new option STOP to define the new 'flags'
(see "Help/Editor Commands/VIA").
- The VIA command now activates the layers that correspond to the length
of the via in case none of these layers is active and the Vias layer
is set to color 0.
- When placing a via at a point where an SMD exists that is connected to
a signal, the via is now automatically added to that signal.
WINDOW command
- 'WINDOW (@)' no longer reacts if the cursor is outside the editor window.
WIRE command
- The WIRE command now has an extended syntax to allow drawing arcs (see
"Help/Editor Commands/WIRE").
Miscellaneous
- If a net gets renamed because a Supply pin was placed on it, the user is
now notified of this.
- Improved part placement in BOARD and PASTE command.
- The files created with EXPORT IMAGE now contain the image resolution in
case the image format supports this.
- The RIPUP command can now be interrupted.
- The cursor is now switched to the "hour glass" while the Autorouter run.
- The size of the text origins is now limited to the actual size of the text.
- There is now a new item "Stop command" in the "Edit" pull down menu which
has the same effect as the "Stop" button in the action toolbar.
- When printing on DOS based Windows systems (Windows 95, 98, ME) EAGLE can
now render the drawing in memory and send the complete bitmap to the printer
in order to overcome problems with printing texts on some printer drivers.
This slows down printing, but at least it produces correct results. If you
happen to have a printer driver that doesn't work correctly, you can
turn this workaround on by setting the parameter
Printer.InternalRendering
in the eaglerc file to a value other than
the default "0".
The individual bits in the number each stand for a specific Windows version:
00000001 = Win32s
00000010 = Windows 95
00000100 = Windows 98
00001000 = Windows Me
00010000 = Windows NT
00100000 = Windows 2000
01000000 = Windows XP
You can use any combination of these bits in order to turn InternalRendering
on or off for specific platforms. For instance the setting
Printer.InternalRendering = "6"
would turn this feature on only for Windows 95 and Windows 98.
If you had "Options/User interface/Always vector font" active because
your printer wouldn't print non-vector fonts correctly, you may want to
turn that option off now and try printing non-vector fonts. You may also
need to turn off the "Persistent in this drawing" option for a particular
drawing. Selecting the "Black" option in the PRINT dialog may speed up
printing (in case you are printing to a black&white device).
- Printing under Linux now supports CUPS.
- When selecting an object in a densly populated area, the "Select
highlighted object" message now also displays the information about
that object, as would the SHOW command.
- Opening the same file concurrently in two output() statements in a User
Language Program is now treated as an error.
- Error message dialogs now use the system defined sound effects.
- When connecting net segments the user is now always informed about the
resulting name.
- The SIGNAL and PINSWAP commands now offer a selection if there are, for
instance, two SMD pads on Top and Bottom at the same location.
- The DELETE command can now be interrupted when deleting a GROUP.
- The cursor now changes to the "hour glass" while processing polygons.
- Improved selecting smashed names/values in densely populated areas.
- If changing a package in a board results in connected pads of that
element being moved outside of the allowed board area of the Light or
Standard edition, the wires attached to these pads are now ripped up
in order to comply with the board area limitations.
- Fixed handling of '\' at the end of script lines (the '\' inserted an
additional blank, which caused problems with 'Description' lines in muliple
EXPORT/SCRIPT of a library).
- An airwire in a dense area now triggers the selection mechanism even if the
other objects belong to the same signal.
- Avoiding flickering status bar in library script with many EDIT commands.
- Changed mouse button handling under Windows to improve application
button selectability.
- The progress bar in the status line of an editor window is now only
displayed when it is actually active, and the percentage value is
displayed outside of the bar under Windows.
- When moving a part in a schematic causes net wires to be automatically
generated, both ends of these wires are now checked to see if any
junctions are missing or can be deleted (this only works if
"Options/Set.../Misc/Auto set junction" is active).
- Improved ERC's checks for unconnected net wires and missing junctions.
- The parameter toolbar in board context now contains a combo box where
angles can be selected and entered (instead of the former four buttons
for R0...R270).
- Panning is now done through Click&Drag with the center mouse button (no
longer with the Ctrl button). If you want to have the old functionality
back you can add the line
Interface.UseCtrlForPanning = "1"
to your eaglerc file. Note, though, 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 draw window.
- Zero length airwires are now displayed as X-shaped crosses to improve their
visibility.
- The new fill styles Stipple1, Stipple2, Stipple3 and Stipple4 (numerical
values 12..15) can be used to have layers be drawn and erased without
disturbing each other.
- Improved library update in case of device sets with a large number of
package variants.
- When switching through the wire bend styles with the right mouse button
(for instance in the WIRE command), the Shift key reverses the direction
and the Ctrl key toggles between corresponding bend styles.
- When a Mark is active, the relative coordinates are now also displayed as
"polar coordinates" (radius + angle), indicated by "(P ...)" in the
coordinate display. This can also be used to measure the distance between
any two points.
- Coordinates entered in the command line or in scripts can now be given
relative to the mark, as polar coordinates, and can simulate a right mouse
button click, which is mainly useful to select a group (see "Help/Editor
Commands/Command Syntax").
- Dialog input fields that accept decimal numbers now automatically
convert the ',' (or whatever the local decimal point is set to) into
a real decimal point ('.').
- When loading a board/schematic pair that doesn't indicate consistency, a
consistency check will now be performed automatically.
- The sheet selection combo box in the action toolbar now contains an entry
named "remove", which can be used to remove the current sheet from the
schematic.
- The highlighted objects from SHOW now stay hightlighted if a WINDOW
command is given.
- The Rich Text tag <author> no longer uses a smaller font.
- The relative coordinate display now uses at least the mark's precision.
- Editor windows now have a new menu entry "File/Open recent" which allows
to easily reload recently used files.
- Increased grid display pecision for mil and inch.
- No more popup message for undefined or empty group, rather 'beep' and
status message.
- Avoiding unnecessary backups (for instance "*.b#1") when saving files
that have not been modified.
- Fixed EXPORT PARTLIST in case of long names or values.
- When renaming a signal the new name is now the default when the user
is prompted whether to combine two signals.
- The list of layers in the CAM Processor is now always wide enough to
display the full layer names.
- The CAM Processor now only prompts once per job (not once per job section)
whether the current file should be reloaded.
- When clicking into the drawing area of an editor window in order to
activate that window, an active command in that window now ignores that
mouse click to avoid unintended effects (like, for instance, inadvertently
deleting an object).
- Speeded up ratsnest calculation for large signals.
- The "File/Open recent" list is now also updated in case of a "File/Save as"
operation.
- Changes to the visibility of toolbars made through the toolbar context
menu are now also stored in the eaglerc file.
- When mirroring a part where wires connected to that part change their
layer, vias at the far ends of these wires are now placed/removed as
necessary.
- The program now uses German menu texts if the system is set to a
German environment.
- The window title now displays the program version number.
- If an error is detected while calculating polygons, the editor window
now zooms to one of the offending polygon edges.
- Fixed the width of some characters in the vector font.
WARNING: Note that due to this change some texts may turn out longer
than they used to! If you have vector font texts on any of your
signal layers, make sure you do a DRC before manufacturing the
board with this new version!
- If the center mouse button is used to pan the editor window, any special
function of that mouse button (like bringing up the layer dialog) will
now be performed if the panning distance doesn't exceed 10 pixel.
- When panning the editor window with the center mouse button, the movement
can now exceed the limits defined by the scroll bars if the Shift key is
held down while panning.
- If EAGLE is called with an eagle.epf file as argument, the respective
project will now be opened.
- If EAGLE is called with the name of a project that is contained in one
of the directories listed in "Options/Directories/Projects", that project
will now be opened.
- Improved selecting objects in densely populated areas with click&drag.
- The splitter position in the Control Panel and the Help window (Linux only)
is now stored in the eaglerc file.
- 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 line
Cmd.Wire.IgnoreCtrlForRadiusMode = "1"
to the eaglerc file. This will turn this
feature off for all commands that draw wires.
- With active f/b annotation any operations that would combine two signals
in the board and would result in combining two nets in the schematic are
now forbidden and need to be done in the schematic.
- Changed the default entries in the drill diameter menus to metric values.
- It is now possible to zoom into a drawing up to a factor where the
internal editor resolution (0.1 micron) is visible. The checkbox
"Options/User interface/Limit zoom factor" is still present and checked
by default, but there is no more warning message when it is turned off.
- When running as user 'root' under Linux and Mac OS X (which is only
necessary to do the licensing and should be avoided under normal operation),
EAGLE no longer sets the "Projects" path to avoid a popup message at program
start, and it also doesn't save the ~/.eaglerc file any more.
- Improved opening the Control Panel's "File/Open/Project" menu in case
there are many subdirectories that do not contain EAGLE projects.
- Coordinates are no longer snapped to the current grid if they are entered
textually with the '>' modifier, as in (> 1 2).
|
|
