Roger

On Sep 4, 2020, at 8:47 AM, = Chad

(parker DOT charles AT gmail DOT com) [via geda-help AT delorie DOT com] <geda-help AT delorie DOT com> wrote:

Rodger-

Sorry for the delay in responding.

I = don't think pcb actually checks to see if the pads are overlapping, but = maybe I just haven't found that corner of the code yet. It should let = you do more or less whatever you want.

The error message your = getting is in the log window? When do you get it?
An alternative, albeit a little less = convenient might be the attached. I made the footprint to contain the = outline and pads one and two, and then left the other segments as lines. = You can go File > Load layout to buffer, and then paste it in. It's = less convenient because if you want to move it you have to select all = the pieces, but you can box select, so, maybe it's not that annoying. = Since the segments are traces now, they have rounded end caps, but don't = you usually want that for RF applications anyway?
If this doesn't work for you, please = let me know. If you can send a minimal complete example (schematic, = commands and scripts used, etc.) I can try to dig in and see what I can = do.

Thanks,
--Chad

On Thu, Sep 3, 2020 at 3:13 AM Erich = Heinzle (a1039181 AT gmail DOT com) [via geda-help AT delorie DOT com] <geda-help AT delorie DOT com> wrote:
There = are two other things to know for these sorts of applications

1) inkscape2pcb now exports (v0.92 inkscape) simple polygons = to pcb-rnd footprints, as well as paths, allowing application note = designs like this to be converted fairly easily from source documents to = copper polygons. Footprints can then be scaled in x, y or both = directions in pcb-rnd too.

https://github.com/erichVK5/inkscape2pcb

2) pstoedit can do similar exports of postscript features to = pcb layouts, and the next release should include code for a plugin that = exports polygons to pcb-rnd footprints.

http://www.calvina.de/pstoedit/pstoedit.htm

The look and feel is much the same for pcb-rnd vs PCB, but = keyboard shortcuts have had to evolve to keep up with the = features.

Regards,

Erich

On Thu, 3 = Sep 2020 15:16 Roger Traylor (traylor AT engr DOT orst DOT edu)= [via geda-help AT delorie DOT com], <geda-help AT delorie DOT com> wrote:
Erich,

Thanks for the info. I figured pcb-rnd could probably handle = this situation.

Right now however, I need to get a job done. I=E2=80=99d = like to try pcb-rnd as I've
followed the = development for a while but it feels like the =E2=80=9Ctrain has left = the
station=E2=80=9D as far as I=E2=80=99m = concerned. It looks daunting to get started with and I
see no on-ramp for beginners. Maybe for the next = project.

Thanks = again,
Roger

On Sep = 2, 2020, at 4:37 PM, Erich Heinzle (a1039181 AT gmail DOT com) [via geda-help AT delorie DOT com] <geda-help AT delorie DOT com> = wrote:

pcb-rnd allows polygons within footprint = elements, as well as lines and arcs, which, in combination with = terminals, can produce the sorts of structures you are playing with more = easily.

Importantly, there is also an "intnoconn" attribute that can = be used on copper features within the footprint

http://repo.hu/cgi-bin/pool.cgi?cmd=3Dshow&node=3Dintnoconn=

That can be used, for = example within a pcb spiral inductor, so that the copper does not look = like a short across the terminals.

With the gEDA PCB = footprint data model, you will have to paint the features with pads, = will end up with a short with DRC, and will have a limited ability to = manipulate the solder mask over the features, if needed.

Regards,

Erich

On Thu, 3 Sep 2020 08:43 Roger Traylor = (traylor AT engr DOT orst DOT edu) [via geda-help AT delorie DOT com], <geda-help AT delorie DOT com> wrote:
Gang,
A quick question for PCB = gurus:

I have = a =E2=80=9Cfolded F=E2=80=9D antenna for 2.4Ghz. It has one open = end, one input for the signal
and one matching stub = that is to be connected to ground.

I drew this in PCB as a series of = =E2=80=9Cpads=E2=80=9D. I attempted to make one pad =E2=80=9C1=E2=80=9D = the input,
and pad =E2=80=9C2=E2=80=9D as = ground. gschem did not complain about the symbol, but PCB = complains
about not being able to find pad = "2" (the ground pin).

Could this be because PCB sees all the pads overlapping as = one pad? If so, how can
I overcome this = problem?

Thanks,
Roger Traylor

Footprint file is = below:

Element[0x00000000 "" "" "" 0 0 0 0 0 100 = 0x00000000]
#Flipped Meander antenna for CC2500 =
#R. Traylor 7.27.2020
#50 = ohm feed point is at end of segment 10
#requires via to = ground plane at bottom of segment 11
#silk at bottom = marks the edge of the ground plane
#see TI/Chipcon = Application Note AN043
#This is the = flipped version of the original meander antenna
#
(
# = X1 Y1 = X2 Y2 thick clear = mask name numb flag
# = right side from origin
= Pad[ 0 0 = 8661 0 1969 0 = 10000 "1" "1" 0x00000100] #segment = 0
Pad[ 8661 = 0 8661 -10394 1969 = 0 10000 "1" "1" 0x00000100] #segment = 1
Pad[ 8661 = -10394 18504 -10394 1969 0 = 10000 "1" "1" 0x00000100] #segment 2
Pad[ 18504 -10394 = 18504 0 1969 0 = 10000 "1" "1" 0x00000100] #segment = 3
Pad[ 18504 = 0 27165 0 = 1969 0 10000 "1" "1" 0x00000100] = #segment 4
= Pad[ 27165 0 27165 = -15512 1969 0 10000 "1" "1" = 0x00000100] #segment 5
# left side from = origin = =
Pad[ = 0 0 0 -10394 = 1969 0 10000 "1" "1" = 0x00000100] #segment 6
= Pad[ 0 -10394 -9843 = -10394 1969 0 10000 "1" "1" = 0x00000100] #segment 7
= Pad[-9843 -10394 -9843 0 = 1969 0 10000 "1" "1" = 0x00000100] #segment 8
= Pad[-9843 0 -27559 = 0 1969 0 10000 = "1" "1" 0x00000100] #segment 9
Pad[-18504 -787 = -18504 -19281 1969 0 10000 "1" = "1" 0x00000100] #segment 10
= Pad[-26772 -787 -26772 -18504 = 3543 0 10000 "2" "2" 0x00000100] = #segment 11
#silk = lines
ElementLine[-30197 2559 = 29725 2559 700] = #top
ElementLine[ 29725 2559 = 29725 -18307 700] = #right
ElementLine[-30118 2559 = -30118 -18307 700] = #left
ElementLine[-30118 -18307 = -29724 -18307 700] #bottom starting from = left
ElementLine[-23798 -18307 = -20678 -18307 700] #segment between vertical = pieces
ElementLine[-16318 -18307 = 29564 -18307 700] #right-most = segement
)
# antenna = layout
#
# * =3D = origin
# -------s9-- = *--s0--- ----s4--|
# = | | | = | | | = |
# | | s8 = s6 s1 s3 = |
# | | = | | | = | s5
# s11 = | |---s7---| |---s2--- = |
# | | = = |
# = | s10 = = |
# | | = = |
# = | |
#