* __

Kicad library (schematic) for the Cypress CYWM6935 radio module: (2007.10.25:1)

http://1010.co.uk/cywm6935.lib

[For physical module in pcbnew used 2x6M header from Eagle libraries and changed first pad.]

A few Kicad/schematic notes: (2007.10.24:1)

1] For both the battery power management and USb interface boards the tantalum SMDs were two small on the PCB. Within pcbnew can replace old part with the right sized (chosen now as C package - 6032) package by selecting [edit module] followed by [change module]. All the different surface mount packages (SMD) were found in:

http://library.oshec.org/library/rc-master.mod

which we load by hand for the project.

2] With the new part inserted connections are lost (eg. netlist, rat's nest). To remedy this, right click on appropriate pad and select [edit pad] option and change pad-net-name to appropriate net (eg. GND, N-00004)

3] To fix our custom, Eagle-imported module [CR2450_KEYSTONE battery halter/holder from Farnell] so that pads are on component surface edited the module file itself (_custom.mod) and changed:

At SMD N 00000000

to:

At SMD N 00888000

KiCad: (2007.09.24:3 pcb#14 schematics#11 tech_notes2#12)

1] Plot -> PDF route sometimes chops board - simply reposition on grid

2] Remember to mark tracks/pads which should be attached to the (GROUND) fill before filling the zone

Kicad shortcuts: (2007.06.12:1 scrying_tech_notes#16 schematics#10 tech_notes2#8)

In PCBNEW:

PgUp and PgDn or Shift V to switch component/copper side when laying tracks and vias (to place via start on component side, drag track, right click to place via and then track continues on copper side)

F1 zoom in

F2 zoom out

F3 redraw (across also all kicad apps)

F4 centre at cursor

and further see also: http://xtronics.com/reference/kicad.html

TODO: check SMD sizes and quartz surface mount footprint

Messy first draft for main scrying board: (2007.06.11:3 scrying_tech_notes#15 schematics#9)

http://1010.co.uk/images/scrymain.pdf

Notes:

1] All power/conditioning is done on power module board (but thinking about it maybe put some capacitors across Vcc/GND close by - maybe not- TODO) - thus we expose 5v/3.3v input - 8x ADC, 8x digital pins, serial stuff

Kicad/scrying boards... (2007.06.11:1 scrying_tech_notes#13 schematics#8 tech_notes2#7)

Notes:

1] Plenty of very useful libraries inc. for ATmega128 and the Hitachi 32Kx8 Static RAM: 62256 (also from Reichelt) at:

http://library.oshec.org/

The ATmega128 at: http://library.oshec.org/library/avr.lib

62256: http://library.oshec.org/library/memory-hitachi.lib

2] Making and connecting buses:

From Kicad online help:

In fact, due to the repetition command (Insert key), connections can be very quickly made in the following way, if component pins are aligned in increasing order (a common case in practice on components such as memories, microprocessors…):

Place the first label (for example PCA0)

Use the repetition command as much as needed to place members. EESchema will automatically create the next labels (PCA1, PCA2…) vertically aligned, theorycally on the position of the other pins.

Draw the wire under the first label. Then use the repetition command to place the other wires under the labels.

If needed, place the bus entries by the same way (Place the first entry, then use the repetition command).

Which boils down to:

• Add bus [right hand bus icon]
• Add label (right hand icon)
• Insert to repeat/edit if needed
• Make first wire to bring pin close to bus
• Insert to repeat
• Add wire to bus entry (wires are purely aesthetic)

  KiCad/GIMP printing: (2007.05.09:1 pcb#6 tech_notes2#5 schematics#7)

1] When we export by way of plot option and then ps2pdf and then into GIMP the image is too small. We need to scale X and Y in the plot option to 1.08.

2] To test boards with three options:

a) latest foggy transparency paper

b) clear OHP film

c) foggy as diffuser and then with clear OHP film

... for SMT, double-sided, new VLF design, spectral boards (inc. TV transmitter)

Further KiCad use for VLF board: (2007.05.08:1)

1] In Pcbnew app now we need to fix on trace sizes for non_SMT/D parts:

0.8mm track

0.8mm via drill

0.2mm clearance (or thicker 0.035inch tracks)

We set this in: Top menu: Dimensions. Then Tracks and Vias.

2] Set page-size when we start to A4 under: Top toolbar - page settings icon

3] We needed to add a module which wasn't in the netlist/schematic - it was easy to add using right hand add-module-icon but adding a track wouldn't work - to do this we needed to turn off DRC in Top menu: Preferences and the General Options (or use left hand top icon)

4] We follow tutorial instructions for fill - use right hand zones icon, trace round board size and then right click and fill but it ignores our new tracks (see 3]): (as a compromise we can use the Fill Zone include pads option which leaves the centre free)

• see pcb for plotting and printing...

[below:

Printing for PCB machen from PCBNEW/KiCad: (2007.01.16:1 tech_notes#10 pcb#2)

1] Straight print from PCBNEW menu under a range of options is unusable (tracks joined, offset and pads connected randomly).

2] Choose plot with Postscript option from file menu and write (in this case) xxxxx-Component.ps. Printing from this using gv is better but unusable also.

3] Run ps2pdf on this .ps and open resulting .pdf with xpdf. Print from this.

(further notes: print command for our CUPS shared printer is lpr -P printer, resolution was set by way of web interface to 600 dpi)

Printing for PCB machen - foto resist using the Gimp: (2007.04.23:2 pcb#5 tech_notes2#3)

1) Import the PDF into the Gimp (open and set resolution to 600). Manipulate and copy as required as a layer.

2) Print settings: Set Image to line and output to Black and White

KiCad and AVR/USB schematics: (2007.01.23:1 schematics#5 tech_notes#16)

1] Added library for the older but more manageable FT232BL USB UART (USB to serial) component using online library component builder at:

http://www.rohrbacher.net/kicad/quicklib.php

library is at:

http://1010.co.uk/images/FT232BL.lib

packaging is TQFP32

2] Schematic is at:

http://1010.co.uk/images/atmega8usb.pdf

(note older PCB screenshot is incorrect)

3] 3 projected boards - independent UART and ATmega8 with circles for cpu_model, and both combined as above for 8 bit data interface sans parallel port

KiCad notes: (2007.01.11:1 tech_notes#7 schematics#4)

Loosely following excellent tutorial at:

http://www.kicadlib.org/Fichiers/:_Tutorial.pdf

as referenced from:

http://www.kicadlib.org/

• step one: use of EESchema to construct/edit schematic is simple enough. remember to annotate schematic - use schematic annotation icon in top bar and select annotate - this gives all components unique identifiers. then use generate netlist icon and save netlist
• step two: next up schematic modules have to be associated with physical representation/footprints - run Cvpcb from icons. we have a list of parts and we need to associate these with scrolling left hand list of footprints (double click on appropriate footproint when we have component selected). save this new netlist
• step three: we run Pcbnew from icons. we need to set paper size from icon and dimensions of tracks and the like from top menu item. Click read netlist button, select approrpiate list and hit read. options for ratnesting are specified in the tutorial - move modules into centre of sheet and manipulate (move, rotate) until number of crossing points is reduced. autoroute functionality appears missing as we do not have the anneal code (?). route by hand using right add tracks icon. for smd we are working on component level. to print use accurate scale 1 option.

[question remains of how to adapt drawing for mandalas offering up GND, 5V, TX, RD serial circling the central processor - perhaps making use of graphic drawing (only of use on silkscreen layers) and print these at same time]

KiCad mini tutorial: (2007.01.10:4 tech_notes#6 schematics#3)

http://kicad.bokeoa.com/wiki/index.php/Mini_tutorial

schematics link - using gschem and gattrib as part of geda GNU electronics stuff (2007.01.08:2)

Using gschem (as part of geda) part one (2007.01.08:3 pcb#1 tech_notes#335 schematics#1)

to edit a schematic and generate a netlist before we make a PCB design in pcb (all GNU free software) - pcb is installed under Gentoo with seperate emerge command.

gschem (also gattrib for editing attributes of .sch files)

• documentation is hard to find. Here is good though:

http://geda.seul.org/wiki/geda:gschem_ug

and the warmup:

http://www.geda.seul.org/docs/current/tutorials/gsch2pcb/gschem-warmup.html

• crashing constantly (if select update component, deleting some nets (meaning wires), undo option sometimes, ag shortcut for add image

perhaps try CVS version

Progress so far:

• Add component:

What are the differences here between Default - reference component, embed component and component as individual objects (latter option seperates out and can thus be edited)?

Use reference I think...

ATmega8 component lacks VCC and GND and pin 1 is in an awkward place. First two remedied by modal operation/keystroke driven approach ... where we want pin ap keys and pull line with left mouse into body of chip. middle mouse to stop behaviour. an to add net/wire with similar results. select object with left mouse squaring over and add aa to attach/add attribute such as a pin number. ea to edit attributes of selected piece/element.

er to rotater elements, fs to save, z and Z to zoom, w to zoom next selected square, ve to view extents (?)

But how do we edit the ATmega8 stuff as it stands to switch pin 1?

(only problem is crashes on update)

see Wiki above:

Update Component (ep)

warmup above is a good place to start for simple operations.

note also:

it only makes sense to create pins while creating or editing symbol files...

note also url for gattrib: http://www.brorson.com/gEDA/gattrib/