fped - Footprint editor ======================= fped is an editor that allows the interactive creation of footprints of electronic components. Footprint definitions are stored in a text format that resembles a programming language. The language is constrained such that anything that can be expressed in the textual definition also has a straightforward equivalent operation that can be performed through the GUI. This README describes only the footprint definition language. A description of the GUI can be found here: http://downloads.qi-hardware.com/people/werner/fped/gui.html This work is distributed under the terms of the GNU GENERAL PUBLIC LICENSE, Version 2: This program is free software; you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation; either version 2 of the License, or (at your option) any later version. For your convenience, a copy of the complete license has been included in the file COPYING.GPLv2. Building -------- Prerequisites: - bash - flex - bison - fig2dev (transfig) - ImageMagick - Netpbm - Gtk+ 2.x development package (libgtk2.0-dev or similar) - Liberation Fonts (ttf-liberation or similar) Check out the repository: git clone git://projects.qi-hardware.com/fped.git cd fped Get updates: git pull Compile: make Run an example: ./fped examples/qfn.fpd Motivation ---------- KiCad already includes a footprint ("module") editor, so why do we need a new one ? The issue with footprint generation for KiCad is that the built-in module editor is basically a drawing program that only captures the result of the module author's interpretation of a footprint drawing, but does not include the steps that led to this construction. Furthermore, accurate measuring of dimensions in the drawing can only be done manually in the module editor, which makes review difficult and time-consuming. In fped, the construction process is made explicit and each step can be expressed in terms of the parameters that appear in the vendor's drawing. Dimensions can be explicitly measured and the results can be included in the graphical output generated by fped. Directly using parameters and construction steps from the reference drawing reduces the risk of mistakes. Visualizing the construction process and verificative measurements helps efficient and accurate review. Leveraging the work already done, and growing the intellectual commons of available footprints has motivated the addition of an export to gEDA pcb format option. Single or multiple footprints are exported in a gEDA PCB layout (.pcb) file. A select all command can be used, followed by a "disperse elements" command, to allow viewing of multiple elements in the gEDA layout editor. An element can then be selected, cut to buffer, and exported to a footprint (.fp) file with the usual menu commands. gEDA PCB format footprints are exported in centimil units. Pads with offset centre holes are not faithfully reproduced; the pad is exported with minimum dimensions and centred on the hole. Trapezoidal and roundrect pads are not supported in gEDA. Footprint definition file format -------------------------------- Footprint definitions are stored in text files. The program "fped" reads and (soon) writes such files, visualizes their content, and provides a graphical editor for them. The syntax is unique and draws from elements of a variety of languages commonly found on unix systems. One specialty is that there are no reserved words - the language keywords appear only at the beginning of a line and can thus be recognized as such without restricting their use for identifiers. This reduces the risk of creating incompatibilities with existing designs when introduction future language features. fped uses the C preprocessor for comments, conditional compilation, and - to a limited extent - also macros. Long lines can be split by ending them with a backslash. If multiple items need to be placed in a single line, e.g., in a macro, they can be separated with semicolons. The file has the following structure: frame definitions ... package name setup objects ... Geometry model -------------- The geometry model consists of frames, vectors, and objects. The shape of objects is defined by a number of points. These points are produced by concatenating vectors. E.g., to draw a line from (1mm, 1mm) to (2mm, 2mm), one would make a vector from the origin to (1mm, 1mm) and one either from the origin or from the previous vector to (2mm, 2mm), and then make a line connecting the two points. Setup - - - The setup section defines settings that affect the entire footprint. It is optional and can contain a "unit" directive and an "allow" directive. Units - - - fped can calculate in mm and mil. Units are specified by following a number with "mm", "um", or "mil", separated by zero or more spaces or tabs. Examples: 1mm 2 mil Units can be mixed in calculations, e.g., set a = 1mm+20mil set b = 10*1mm All values used as dimensions must be either mm or mil. The default unit can be set with one of the following directives: unit mm unit mil unit auto If the "unit" directive is omitted, fped defaults to millimeters. When saving a footprint definition, the default unit is set to the unit set in the GUI. Allow - - - fped normally disallows overlapping pads. This restriction can be relaxed with the "allow" directive. allow touch Allows pads touching but not having more than their border in common. allow overlap Do not check for overlaps at all. If the "allow" directive is omitted, fped defaults to allowing neither overlap nor touch. There is also the following experimental directive that can be used alone or without one of the overlap-checking directives: allow holes Allow multiple holes per pad. Vectors - - - - Vectors can be anonymous or they can be named for future reference: vec ( , ) : vec ( , ) The base can be one of the following items: - @ is the origin of the frame containing the vector - . is the end of the previous vector in this frame - is the name of a previous vector in the same frame The following example would draw the line described in the previous section: a: vec @(1mm, 1mm) b: vec .(1mm, 1mm) line a b Silk screen objects - - - - - - - - - - The output of fped is a footprint definition that contains pads and silk screen drawings (we may add more layers in the future). These items are called "objects". Their geometry is defined through points obtained with vectors. A line connects two points: line [] The points can be specified with @, ., and an identifier, just like a vector base. The option width specifies the thickness of the silk screen line. If omitted, a hard-coded default of 15 mil is used. A rectangle has sides parallel to the x and y axis and is defined by two diagonally opposite corners: rect [] A circle is defined by its center and a point on the circle: circ
[] This example draws a unit circle: vec @(1mm, 0mm) circ @ . An arc is like a circle, but the part of the circle drawn is determined by two points. The first point determines the radius and the starting angle. The second point only determines the end angle but its distance from the center is ignored. arc
[] The arc is drawn in a counter-clockwise direction. The following example draws an arc of the unit circle in the x > 0, y > 0 quadrant: from: vec @(1mm, 0mm) to: vec @(0mm, 1mm) arc @ from to Pads - - Pads are similar to rectangles, but they also have a name. pad "" [] Variables can be expanded in a pad's name by prefixing their name with a dollar sign. The ${name} syntax is also available. Example: vec @(1mm, 1mm) pad "1" @ . Pads normally affect the surface copper layer, the solder mask layer, and the solder paste layer. This can be modified with the optional type argument: Type Layers --------- ------------------------------------- (default) copper, solder mask, and solder paste bare copper and solder mask trace copper without solder mask opening paste solder paste mask solder mask Typical uses: - "bare": connectors printed directly on the PCB - "trace": connections or antennas - "paste": sparse solder paste, e.g., for QFN center pads - "mask": non-standard mask openings, e.g., for solder mask defined pads Rounded pads - - - - - - Rounded pads are like rectangular pads except that they end with a semi-circle at each of the smaller sides of the enclosing rectangle. If enclosed in a square, rounded pads form a circle. rpad "" [] Holes - - - Holes can be used for through-hole pins or for mechanical support. In the former case, the hole must be placed inside a pad. Only one hole per pad is allowed. Mechanical holes must be outside any pads. Through-hole pads are always present on both sides of the board, i.e., when fped generates a KiCad module, the surface layers of a pad containing a hole are propagated to the opposite side of the board. Holes have the same shape as a rounded pad and their geometry is defined in the same way: hole Measurements - - - - - - *** This is obsolete - see the section on new-style mesurements at the end. *** Measurements show the distance between two points: meas The offset is the distance from the imaginary line connecting points A and B the measurement line is draw: - if the offset is 0mm, the line will connect A and B - if the offset is positive, the line would be on the left-hand side when traveling from A to B - if the offset is negative , the line would be on the right-hand side when traveling from A to B Example: a: vec @(-1mm, 1mm) b: vec @(1mm, 1mm) meas a b 0.2 mm Package name - - - - - - The package name is a non-empty string of printable ASCII characters, including spaces. If the "package" directive is omitted, fped defaults to using the name "_". package "" Examples: package "48-SSOP" package "0603" Like in pad names, variables are expanded in package names. This allows the generation of multiple packages from a single definition. Frames - - - Frames are used to group things and to reuse them multiple times. Frames must be defined before they can be used: frame { ... items ... } Once defined, a frame is placed at a given location with frame The frame definitions must precede all other items in a footprint description. Frames cannot be defined inside other frames, but frames can invoke each other recursively. For example, this puts two unity squares, one centered at (0 mm, 0 mm), the other at (2 mm, 0 mm): frame unit_square { a: vec @(-0.5mm, -0.5mm) b: vec .(1mm, 1mm) rect a b } frame unit_square @ vec @(2mm, 0mm) frame unit_square . Names and variables ------------------- fped uses several name spaces: - frame names occupy one global name space - vector names occupy name spaces delimited by the frame they're contained in. A vector name is only visible inside the frame in which it is defined. - variable names occupy name spaces delimited by the frame they're contained in. A variable lookup starts in the frame in which the corresponding expression appears and propagates to outer frames until the variable is found. - pads occupy one global name space (this is currently not enforced) Note that names cannot be redefined. E.g., this does not work: set a = 1 set a = a+1 The names spaces of frames, vectors, variables, and pads are separate from each other. Simple variables - - - - - - - - A variable with a single value is defined with the following assignment syntax: set = Example: set a = b+2 Loops - - - A loop is a variable with a range of values: loop = , The variable assumes all the values i for <= i <= , in increments of one. E.g., loop n = 1, 3 and loop n = 1, 3.5 both assign the values 1, 2, and 3 to the variable "n". The following loop would not execute at all: loop n = 1, 0 This can be used to implement conditional execution. For example, the items in the following frame would be instantiated if the variable "enable" is set to 1 but not it is set to 0: frame ... { loop dummy = 1, enable ... } When a loop is executed, the objects contained in the body of the enclosing frame are generated for each value of the variable. If a frame contains multiple loops, all possible combinations of the values are generated. The following example draws three concentric circles around the origin, with radii 1, 2, and 3: loop x = 1, 3 vec @(x*1mm, 0mm) circ @ . Tables - - - Tables combine values for multiple variables. Like loops, they are used to iteratively generate objects. A table begins with a row of variable names, followed by one or more rows with values. Rows are enclosed in curly braces and their elements are separated by commas. table { , ... } { , ... } ... Like loops, tables are iterated to generate objects. The following example is equivalent to the one in the previous section: table { x } { 1mm } { 2mm } { 3mm } vec @(x, 0mm) circ @ . Note that we can set the unit of the values directly in this case. Iteration is performed over rows. All variables of the table are set to the value in the respective row at the same time. For example, in table { x, y } { 1, 2 } { 3, 4 } (x, y) assume the values (1, 2) and (3, 4). Tables can also be used to provide information that depends on other variables. The value of such a variable acts as a key, and a row is only selected if all the keys in that row match the respective variables. To mark a variable as being used as key, its name it prefixed with a question mark. Example: loop n = 1, 2, 3 table { ?n, name } { 1, "one" } { 2, "two" } { 3, "three" } Expressions ----------- Expressions can contain numeric constants (in non-exponential notation), variable names, the arithmetic operations +, -, *, /, unary -, and the functions sin(), cos(), sqrt(), and floor(). Parentheses can be used to change precedence. The argument of sin and cos is a dimensionless number that specifies the angle in degrees. E.g., sin(90) yields 1. The argument of sqrt() can be dimensionless or have a dimension with an exponent that's a multiple of two. E.g., sqrt(2) and sqrt(2mm*3mm) are valid expressions, sqrt(2mm) isn't. The function floor() returns the next integer that is below or equal to the argument. If the argument has a dimension, that dimension is preserved. E.g., floor(-1.2) returns -2, floor(4.7mm) returns 4mm. GUI --- Part of the GUI is described in http://downloads.qi-hardware.com/people/werner/fped/gui.html Keyboard shortcuts - - - - - - - - - Space reset user coordinates +, = zoom in (like mouse wheel forward) - zoom out (like mouse wheel backward) . cursor position to screen center (like middle click) * zoom and center to extents # zoom and center to currently active frame instance U undelete the previously deleted object / Switch between variables, code, and packages display. Canvas - - - To create a new object, click on the corresponding tool icon, move the mouse to the base point of the new object, then drag to the object's second point. Frame references are created as follows: - select the frame you want to add - click on the frame icon. A black dot should appear on the icon. - select the frame on which you want to add the new reference. The black dot should change to a green dot. If the current frame is a child of the selected frame, the dot remains black. - click on the desired base location To change a point of an object, select the object, then drag the point to its new location. To edit the object's parameters, select it and make the changes in the input area at the bottom. To delete an object, select the delete tool and click on the object. Deleted objects can be undeleted by pressing "u". If any other changes have been made since deletion, fped may misbehave. If deleting a vector, all items that reference it are deleted as well. Experimental: new-style measurements ------------------------------------ New-style measurements can measure the distance between various pairs of points, not only between points in the same instance and the same frame. They operate on the set of points produced during instantiation. New-style measurements are placed in the root frame after all other items. Known issues: - they currently can't be edited through the GUI - tie-breaking heuristics don't always do what one expects Syntax: [