Re: gEDA-user: PCB footprints & polygons question

[kai-martin knaak <kmk@xxxxxxxxxxxxxxx>]

michalwd1979 wrote:

> In my current design I wanted ton create footprint (for "touch key")
> that would have normal pin and some copper tracks connected to this
> pin. Is it possible? Tracks automatically became pads in footprint
> so then I have DRC errors.

Give all connected pads the same pin number (use the [n] key on them). 
For those parts that should behave like tracks, you can set mask 
clearing to zero. (activate the solder mask layer and repeatedly do 
[shift-k] on them until the hole in the mask vanishes)


> In general is it possible to create footprint that will have
> everything like normal board (pins,pads,tracks,ect.) not just 
> pins & pads?

No. The footprint format of pcb is pretty restrictive :-|
Text and arcs are not allowed either.


> On my boards I almost always use ground planes (polygons). When
> drawing a polygon PCB removes copper "islands" that are not connected
> to anything - Is it possible to turn off this feature?

Activate "New polygons are full ones" in the settings menu to disable 
removal of islands for new polygons. For existing polgons you can add 
the fullpoly flag in a text editor. 

Note to Peter Clifton: This does not work in the OpenGL enables 
version. Polygon snippets are removed no matter what the fullpoly flag 
says.


> When talking about polygons there are also some features the I 
remember from old protel (2.8 or something like that - I used protel 
before gEDA) that I missing now. It was possible to switch "remove dead 
copper" on and off and it was also possible to select the net to which 
the polygon was connected and program added thermals as needed. When 
net was selected it also was possible to choose "pour over same net" 
option - when selected polygon was not cleared by tracks and vias that 
was on chosen net.
> Then I could draw a board, also routing GND net to see if there are 
no islands and then add a polygon that was connected to GND net, with 
all thermals added that was not cleared by existing GND tracks. Do You 
think that something similar is possible with PCB?

In pcb polygons do not have a preferred net. Instead, it is connected 
to whatever connects to it. See the FAQ:
http://geda.seul.org/wiki/geda:pcb_tips#how_can_i_connect_tracks_pads_or_vias_to_my_polygon

Because a polygon does not know, what net it should connect to, it 
cannot automatically add thermals. You have to add them manually. The 
same goes for tracks. You don't have to add the join flag individually 
for every segment, though:

1) Select all GND tracks with the net window. Alternatively type [f] on 
on a GND track to select all connected copper. 

2) Type [:] to bring up the command line interface. Give the command 
SetFlag(selected, join)


> Or maybe it is a feature that will be in next release :-).

I don't know about any plans to add net properties to polygons.

 
> Working with PCB I sometimes have troubles with rat lines. When
> there a lot off pads in a line that should be connected in some
> way rats are very hard to follow because they are all in the same
> place. I remember that in my old program there was an option that
> was really helpful. It was "manual route" - first You needed to
> select a rat and start drawing a track. Program was drawing that
> rat from the cursor (end point of track) to its destination. In 
> this way You knew where track should go even when rats was mixed
> at the start.

During manual routing pcb highlights all objects with the same net as 
the point you started at. The setting "auto_enforece_DRC_clearence" has 
to be activated to make this work.

---<)kaimartin(>---
-- 
Kai-Martin Knaak
Öffentlicher PGP-Schlüssel:
http://pgp.mit.edu:11371/pks/lookup?op=get&search=0x6C0B9F53



_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user