gEDA tutorial

This is a short tutorial on using gEDA for round-trip engineering.

Contents

• Creating schematics
• Creating a .pcb from a .sch
• Round-trip engineering
• Ground pours
• Creating gschem symbols
• Creating pcb footprints
• Publishing schematics
• Notes

Creating schematics

Start gschem with:

gschem  my-schematic.sch

• Press [I] to insert a part. The text input focus will be in the Filter field. Start typing a part code and the tree in the main view will simmer down to show only matching parts. Some common parts are:
  • resistor, capacitor, diode
  • pnp, npn
  • gnd, vcc, vdd, 12V-plus
  • connector
• Press [OK] to select a part and then use the left mouse button to add parts of that kind. Press [Esc] when finished
• The short text such as D? next to the part is the reference designator, or refdes. It can be selected independent of the part and edited with [E] then [X]. The size and alignment of the text can be changed in that dialog too
• Zoom with the mouse wheel and scroll around by holding down the middle mouse button
• Press [N] to start laying a net in order to connect parts. Press [Esc] when finished laying a net
• A net can be named by pressing [A] twice when a net is selected. Nets with the same name are connected. Using Vcc or GND for net names causes the net to be connected to those rails
• Click or drag the left mouse button to select elements. Hold down the Shift key while doing this to add to the selection instead of replacing it

Save the schematic and use:

refdes_renum  my-schematic.sch

..to automatically number all reference designators that end with "?".

Some useful keys ( Note: "v, e" means press [V] then [E])

Keys	Effect
v, e	View Extents: Zoom so that the whole schematic is in view
w	Choose an area of the view to zoom in to
u	Undo
Shift+R	Redo

Some useful keys that affect the selected parts:

Keys	Effect
m	Move
Delete	Delete
e, r	Rotate
e, i	Mirror
e, c	Copy
e, e	Edit attributes
a, a	Add attribute
t, u	Auto-number text

Common attributes:

Attribute	Purpose
footprint	Indicates the physical plan of the part on the PCB. DIP28N for example
value	The value of a resistor or capacitor. Used to generate the BOM

Common footprints:

Footprint	Usage
AXIAL_LAY s	s is the pin separation, e.g. AXIAL_LAY 300
RADIAL_CAN d	d is the diameter of the package, not the pin separation. RADIAL_CAN 200
TO92
TO220
DIP20	For a 20-pin dual in-line package
JUMPER4	For a 4-pin header
LED d	d is the outside diameter of the LED in mils, e.g. LED 197 for a 5mm LED
HEADER10_2	10-way header with 2 rows, i.e. 5x2 header

Creating a .pcb from a .sch

Ensure that each part has a unique refdes and then:

gsch2pcb  my-schematic.sch

Scan the output for errors ( which are usually about missing footprints), correct and then re-run. If gsch2pcb outputs:

...
/usr/bin/m4:stdin:22: bad expression in eval:  /4
...

..then possibly a footprint is LED-197 when it should be LED 197.

Open the new PCB with:

pcb  my-schematic.pcb

• Zoom with the mouse wheel and scroll around by dragging with the right mouse button
• Set the grid size to 100 mils and enable the visible grid
• Disperse all elements
• Untick Auto enforce DRC clearance but tick Crosshair shows DRC clearance
• Tick New lines, arcs clear polygons
• Load the netlist from my-schematic.net
• Press [O] to show the "rats nest", which shows which pins should be connected to which others
• Rotate the parts and drag them around so as to untangle the rats nest
• Watching what the auto-router does can teach valuable tricks but the most elegant boards are laid out by hand
• Choose and edit a Route Style before drawing lines. For home-made circuit boards, Line width and Clearance of 20 mils or greater is prudent
• Press [O] after drawing each line to see the rats nest get tidier
• The PCB Log window shows how many rat lines remain to be routed and if any nets are shorted
• The Design Rule Checker checks that the layout meets the specifications in Preferences, Sizes

Some useful keys:

Key	Effect
F1	Via tool
F2	Line tool
F4	Text tool
F5	Rectangle tool ( for ground pours)
F9	Rotate tool
/	Changes where the line bends
m	Move the element under the cursor to the current layer
M	Move selected elements to the current layer
o	Show the rats nest
e	Hide the rats nest
Tab	Show the other side of the board
u	Undo
R	Redo
B	Move selected elements to the other side of the board

Round-trip engineering

Sometimes the schematic changes after some of the PCB has been laid out.

• New parts might be added
• Existing parts might have their footprint changed
• Parts might be deleted

Once the schematic has been updated, ensure that the latest changes to the PCB have been saved and then re-run:

gsch2pcb  my-schematic.sch

gsch2pcb will edit my-schematic.pcb in-place to remove parts that have been deleted or had their footprint changed but it will put new parts and parts with new footprints in my-schematic.new.pcb. Assuming my-schematic.pcb is already open:

• Use Load layout to reload the my-schematic.pcb file
• Use Load layout data to paste buffer to load the my-schematic.new.pcb file
• Click somewhere on the PCB where there is space to place the new or updated parts
• Select the newly added parts and choose Disperse selected elements
• Reload the netlist with Load netlist file if it has changed
• Press [O] to update the rats nest and then lay out the newly added parts

Ground pours

A ground pour makes routing easier because GND traces need not be laid out at all. Where a ground plane is present on a four-layer board, the signal will return through the ground plane directly underneath the trace above. A more roundabout return can cause RF problems in high-frequency boards. Pours are still good for conserving etchant though.

• Open the Netlist dialog from the Window menu
• Double-click on the GND net so that it has a * next to it
• Close the dialog and press [O]
• The GND rat lines will be absent from the nest
• Make doubly sure that New lines, arcs clear polygons is ticked
• Lay out the rest of the traces
• Draw a rectangle on layer 2 that covers the whole board. This is the ground pour
• Untick New lines, arcs clear polygons and draw lines to connect those pins to the ground pour that should be tied to GND

Creating gschem symbols

gEDA has a symbol creation guide.

To configure gschem to use a local component library, ensure that ~/.gEDA/gafrc contains something like:

(component-library "/home/neil/electronics/symbols")

Create a symbol with:

gschem BC549.sym

The .sym rather than .sch causes gschem to realise you'd like a symbol rather than schematic.

1. select Add Pin to draw pins. Add boxes and lines too. For each pin:
2. set pinnumber and pinseq to the same value (counting up starting at 1)
3. set pintype to one of:
   • in: input
   • out: output
   • io: input/output
   • oc: open collector
   • oe: open emitter
   • pas: passive
   • tp: totem pole
   • tri: tristate (high impedance)
   • clk: clock
   • pwr: power/ground
4. add attributes:
5. device=BC549
6. author=Neil Stockbridge <neil@example.com>
7. numslots=0
8. net=Vcc:7
9. footprint=TO92
10. refdes=U?
11. Use:

    gsymcheck -vv BC549.sym

12. Choose Symbol Translate from the Edit menu and use a value of 0

Add attributes above or to the right of the symbol otherwise they will be obscured when the symbol is translated.

Creating pcb footprints

When pcb has no footprint for your part, just make one!

mkdir ~/electronics/footprints/mine

..then in pcb, go to:

File , Preferences... , Library , Element Directories

..and change it to include:

~/electronics/footprints

..then make a file in ~/electronics/footprints/mine/BSA325.fp like so:

# Element( flags description blank blank mark_x mark_y text_x text_y text_direction text_scale text_flags
# Pin( x y thickness clearance mask drillhole name number flags
# ElementLine( x1 y1 x2 y2 thickness)
# ElementArc( centre_x centre_y radius_x radius_y startAngle deltaAngle thickness)  startAngle in degs, 0=East, +ve deltaAngle anti-clockwise
# Measurements are taken from the datasheet
#
Element( 0x00 "BS-A325* small seven-segment display" "" "BS-A325" 0 0 150 100 3 100 0x00)
(
  Pin(   0   0  60  70   0  28 "Common Anode"  "1" 0x101)
  Pin(   0 100  60  70   0  28 "f"             "2" 0x001)
  Pin(   0 200  60  70   0  28 "g"             "3" 0x001)
  Pin(   0 300  60  70   0  28 "e"             "4" 0x001)
  Pin(   0 400  60  70   0  28 "d"             "5" 0x001)
  Pin( 200 400  60  70   0  28 "Common Anode"  "6" 0x001)
  Pin( 200 300  60  70   0  28 "dp"            "7" 0x001)
  Pin( 200 200  60  70   0  28 "c"             "8" 0x001)
  Pin( 200 100  60  70   0  28 "b"             "9" 0x001)
  Pin( 200   0  60  70   0  28 "a"            "10" 0x001)
  ElementLine( -45 -70 -45 470 10)  # left, starting top-left going anti-clockwise
  ElementLine( -45 470 245 470 10)  # bottom
  ElementLine( 245 470 245 -70 10)  # right
  ElementLine( 245 -70 -45 -70 10)  # top
)

Values for thickness, drillhole and mask are diameters yet the clearance of a pin is specified as twice the minimum clearance, so a "clearance" of 30 tells the Design Rule Checker that there must be at least 15 mils between the edge of the pad and any other copper.

Thickness and clearance apply to DRC. Mask, thickness and drillhole apply to fabrication. Thickness is the diameter of the pad and "mask" the diameter of the hole in the solder mask:

When specifying drill diameters, add 19 mils to compensate for through-plating if having PCBs fabricated.

Don't forget when running gsch2pcb to specify the elements directory like so:

gsch2pcb -d ~/electronics/footprints  twin-bcd.sch

Publishing schematics

The built-in Write image feature produces lacklustre results with bitmap formats. Here's how to get better results, even if in monochrome:

• Choose Write image... from the File menu. For Image type, choose Encapsulated Postscript and press [Save]
• Open the .eps file with GIMP. Choose Strong antialiasing for both Text and Graphics
• Use [R] to select the area of the schematic to be published
• Choose Crop to Selection from the Image menu
• Choose Autocrop Image from the Image menu
• Choose Scale Image from the Image menu
• Choose the final resolution of the published image, press [Scale] and then save the image

Having a board fabricated

• Ensure that all component-side layers are in layer group #1 and all solder-side layers in group #2
• Double-check drill hole diameters against measurements from the actual components and then add 5 mils
• Ensure that no Design Rules are broken and that the design rules are within the tolerances specified by the fabricator
• Many fabricators only process plated drill holes. Ensure that no pins have the "hole" flag
• Create an outline. Summary: draw a rectangle in a layer called "outline" in layer group #3
• File > Export layout... [gerber]
• Leave the default settings ( for OSH Park anyway). Prefix the file path with /tmp/ if desired
• Check your gerbers for common sense before sending them to the fabricator. Use gerbv /tmp/<board-name>* to see all layers at once

Notes

• Both .sch and .pcb files are plain text files. They can be edited manually or processed with scripts to do things such as change the clearance of the pins of parts
• To remove the reference designators from the silkscreen, choose View, Displayed element name, Value and then go round selecting the values, pressing n and deleting the values. Don’t delete the designators or the descriptions otherwise round-trip engineering stops working