[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]
Re: gEDA-user: Problem With SOT23-5? Invisible "Guardband" Around Landpattern; Arcs in Silkscreen
Gus Fantanas wrote:
> 1. The SOT23-5 footprint (Linear Tech package footprint) from John
> Luciani's site
> (http://www.luciani.org/geda/pcb/footprints-gif/SOT-gif.html) seems to
> confuse gsch2pcb. gsch2pcb skips the part with that footprint, not
> referring to it. If, in gschem, I declare that part to have another
> five-pin footprint, e.g., SC70_5, it works fine. I am buffled by this.
This is the nasty hyphen-in-footprint-name bug, again. If the footprint
name contains a hyphen, gnetlist refers it internally to an M4 engine.
This M4 engine misreads the name and returns garbage. If this garbage
makes it into the layout and can create all kinds of non-specific havoc.
You have three options:
1) rename the footprint and put it in your local library.
2) switch off M4 processiong with options given in the project file
3) use a version of PCB that was build this year. IIRC, the bug was
fixed at the end of 2010.
Although I tend to use current developers snapshots, I have no experience
with 3). Since the bug bit me in 2006, I always put the option kip-m4 in my
project files.
> I finally solved the problem by creating my own SOT23-5 footprint.
It is ok to have digits after the hyphen. The problem shows with letters.
> 2. The standard footprints for 0201..1210 (and probably others, too) in
> the pcb library do not show up with a "guardband" around them when
> placed.
You can add such a guardband in the silk of the footprints:
1) Open PCB
2) Choose the footprint from the lib
3) Do break-element-into-pieces from the buffer menu
4) paste buffer to canvas
5) draw the guardband in silk
5a) Unfortunately, the found-bug raises its head and the new silk lines
will remain in found-color indefinitely. Cut the lines to buffer and
paste them back on canvas to get rid of the found color.
6) cut the whole footprint to buffer
7) do convert-buffer-to-element from the buffer menu
8) paste buffer to canvas. Unfortunately, some properties got lost by
the two converts. To add it again, you can:
9) type q over the round pads to make them square
10) type n over the pads to give the correct number to the pad
11) type n somewhere where no pad is, but still inside the guardband.
This will pop up a dialog to give the name of the footprint. Move the
name to some decent place
12) copy the footprint to buffer
13) do save-buffer-elements-to-file from the buffer menu. Save it to
where yous local footprint lib resides. Add the parent dir of this
dir to the library setting in File->Preferences if you use "import_schematics"
Add the path to your project file if you go the gsch2pcb way.
BTW, did you already check out http://gedasymbols.org?
Shameless plug: My 0805 and 0603 footprints contain an outline in silk.
> 3. I tried to draw a semicircular arc on the silkscreen perimeter
> around some footprints I created (to help identify the side of the
> package defined by the first and last pins). However, they did not
> carry into the final element (created from the buffer), although the
> straight line segments did. How can I make an arc part of the
> silkscreen pattern of a footprint I create?
You can't. Footprints are strictly made from lines and rectangles.
No arcs, no text, no weird polygons.
> I am running gEDA packaged with the latest version of Ubuntu (11.04
> "Natty"), if that helps.
Theoretically,
pcb --version
should return the version of the PCB binary you are running. In reality,
this version is sticking at 1.99z since a few years. There are different
releases, though. Check the name of the ubuntu package for a string of
numbers that can be interpreted as a date. E.g. "20100926" This is the
revision you are running.
Hope, this helps,
---<)kaimartin(>---
--
Kai-Martin Knaak
Email: kmk@xxxxxxxxxxxxxxx
http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53
not happy with moderation of geda-user
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user