version 4.1

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.

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

The layer, background and grid colors are now completely user definable.
There are now three "palettes" for black, white and colored background, respectively. Each palette has 64 color entries, which can be set to any RGB value. The palette entry number 0 is used as the background color (in the "white" palette this entry cannot be modified, since this palette will also be used for printing, where the background is always white).

The color palettes can be modified either through the dialog under "Options/Set.../Colors" or by using the command

    SET PALETTE <index> <rgb>
where <index> is a number in the range 0..63 and <rgb>  is a hexadecimal RGB value, like 0xFFFF00 (which would result in a bright  yellow). Note that the RGB value must begin with "0x", otherwise it would be  taken as a decimal number. You can use

    SET PALETTE BLACK|WHITE|COLORED
to switch to the black, white or colored background palette,  respectively. Note that there will be no automatic window refresh after this  command, so you should do a WINDOW; command after this.

By default only the palette entries 0..15 are used and they contain the same colors as previous versions.
The palette entries are grouped into "normal" and "highlight" colors. There are always 8 "normal" colors, followed by the corresponding 8 "highlight" colors. So colors 0..7 are "normal" colors, 8..15 are their "highlight" values, 16..23 are another 8 "normal" colors with 24..31 being their "highlight" values and so on. The "highlight" colors are used to visualize objects, for instance in the SHOW command.
The background color for layout and schematic can now be set to any color. Note, though, that in case the background color is neither pure black nor pure white, the drawing will be displayed layer by layer, which usually makes a window refresh slower than with black or white background.
Changes to the "Options/Set..." dialog: + The "Grid" Tab has been renamed to "Colors". + The minimum visible grid size parameter has been move to the "Misc" tab.
The new User Language builtin function 'palette()' can be used to determine the currently used palette as well as the palette entries (see "Help/User Language/Builtins/Builtin Functions/Miscellaneous Functions/palette()").

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

The new parameter MaxApertureSize can be used in the 'eagle.def' file to define an upper limit for the size of the generated apertures for the GERBERAUTO and GERBER_RS274X devices. If objects larger than this limit are to be displayed, apertures will be emulated for them.

If the 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. The file names are built by adding the number of the start and end layer to the base file name, as in

    boardname.drd.0104
which would be the drill file for the layer stack 1-4. If you want  to have the layer numbers at a different position, you can use the placeholder  %L, as in

    .%L.drd
which would result in

    boardname.0104.drd
The drill info file name is always generated without layer numbers,  and any '.' before the %L will be dropped. Any previously existing files that  would match the given drill file name pattern, but would not result from the  current job, will be deleted before generating any new files. There will be one  drill info file per job, which contains (amoung other information) a list of all  generated drill data files.

The aperture wheel file is now checked for duplicate D-codes (see "Help/Generating Output/CAM Processor/Output Device/Device Parameters/Aperture Wheel File").
The CAM Processor now also has a "File/Open recent" menu.
The CAM Processor now always prints all vias (even blind or buried) if the Vias layer is active, but none of the layers 1..16 is active.
Added a note to the CAM Processor's "Photoplotter Info File" regarding missing apertures in case they were requested in a non-orthogonal angle.
The CAM Processor no longer deselects all layers when clicking into some empty space of the "Layers" list.
Implemented some overlap when filling polygons with Postscript in the CAM Processor to avoid small gaps on some output devices.
The EXCELLON device in the CAM Processor now writes the actual drill sizes into the output file, so you no longer need to send the "drill rack" file to the board manufacturer. If you don't like this, you can disable this feature by deleting or commenting out the line
```
    DrillSize  = "%sC%0.4f\n"        ; (Tool code, tool size)
in the eagle.def file.  
```
The EXCELLON device in the CAM Processor now automatically generates the drill size definitions according to the actual values used in the board, so you no longer need a drill rack file. If you don't like this feature, you can disable it by deleting or commenting out the line
```
    AutoDrill  = "T%02d"             ; (Tool number)
in the eagle.def file. Existing CAM jobs that have a drill rack  file defined will continue to use that file.  
```
The device EXCELLON_RACK has been introduced to still have the old functionality with user supplied rack file available.
The new drill station parameter BeginData can be used to define a string that is output before the actual drill data (the EXCELLON device now outputs a '%' here).
Added M48 and M72 to the EXCELLON Init string.

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

The option "SIGNALS" must now be written in full.
The DELETE command now combines two wires if applied to their joining point with the Ctrl key pressed. If you want to have this functionality without pressing the Ctrl key, you can append the line
```
    Cmd.Delete.WireJointsWithoutCtrl = "1"
to the eaglerc file. 
```

DISPLAY command

The automatic enabling/disabling of related layers when activating or deactivating the t/bPlace or Symbols layer in the DISPLAY command can now be turned off by appending the line
```
    Option.DisplayRelatedLayers = "0"
to the eaglerc file. 
```

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).

Cadsoft Main Page | Back to Testech Home Page | Compiler | RTOS | Emulator/Debugging