Roger Traylor

On Sep = 8, 2020, at 10:47 AM, Chad Parker (parker DOT charles AT gmail DOT com) [via geda-help AT delorie DOT com] <geda-help AT delorie DOT com> wrote:

Okay, so in terms of urgency here, these = warnings are not interfering with the design you're trying to build. pcb = isn't preventing you from drawing the circuit you need to draw, it's = just throwing these warnings. Correct?

The first one worries me a little, but = the second two I actually think are appropriate. You may be doing it = deliberately in a controlled way, but you are shorting two nets together = and I think it's appropriate for pcb to throw a warning there. If for no = other reason then to remind you to check that it is actually being done = the way you think it is.

The first warning about not finding pin 2 is surprising to = me. Even if the pin is shorted to something else, it should still be = found. I have a hunch about this, but I think it's worth filing a bug = report.

If you need microcontroller lab ideas, = I've got a slew of them :)

Cheers,
--Chad

On Mon, Sep 7, 2020 at 5:02 PM Roger = Traylor (traylor AT engr DOT orst DOT edu) [via geda-help AT delorie DOT com] <geda-help AT delorie DOT com> wrote:
Chad,
Sorry for the late = reply. Its been a busy season for me.

Yes, the message I see is in the log = window. When I do make the connection,
matching= L and C to antenna input pin 1, and ground pin 2 on the = antenna,
the log window says:

Can't find U11 pin = 2 called for in netlist.
Warning! Net "GND" = is shorted to net "unnamed_net75"
Warning! Net = "unnamed_net75" is shorted to net "GND"

Pin 2 is the one I = wanted to ground as it is the matching stub.

I will try your attached .pcb file and = see how that looks.

One other thing I was going to try was to (in gschem) ground = the input to the
antenna, and also connect it to = antenna pin 1. Then, grounding pin 2 should
cause = no conflicts.

I will try to get back to this soon. Trying to set up a = lab-based micro-controller
class for 100% remote = learning. Its kicking my backside.

Thanks again,
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 = = |
# | | = = |
# = | |
#

<antennalayout.pcb>