Re: RF Connector Type ID

Am 09.06.24 um 17:03 schrieb john larkin:

 Our boards are mostly 0.062" thick, and I like layer 2 to be a solid
ground plane. Some internal layers are power planes. If you solder an
edge-launch SMA or SMB connector to layer 1, the layer 2 ground plane
is too close to the center pin of the connector, so that bit of the
signal path is too low impedance. So one does creative shaped cutouts
in the various layers to keep the impedance uniform and the
reflections down. We did e-m simulations (with ATLC) and test boards
to get that right.
 The cheaper connectors have a giant round center pin, which requires
attention.
 https://www.dropbox.com/scl/fi/vfi56wy5hkwva51bx77z6/SS_SMA_Edge.JPG?rlkey=nbmbyb0f54uslcpc0nh7rs21p&raw=1
 That pin is around 100 ohms in free space!
 There are more expensive conectors with a tiny flat pin that
theoretically matches a layer 1 trace width directly, but I haven't
found them to be worth it on FR4 boards and 30 ps edges.
 https://www.dropbox.com/scl/fi/rptmh5f4umscqqpegatw6/Mueller_SMA.JPG?rlkey=1eonuljqekvrszyb9tce5s1hr&raw=1

That giant center pad gives away the advantage that you could have
from the costly SMA connector.
< https://www.flickr.com/photos/137684711@N07/51843174578/in/datetaken/    >
This is nearly as bad as the unpopulated SMA at the right end of the line. The left SMA is one with a thick center pin. Unsuitable on this
cheap JLCPCB 4 layer board. you even see the amount of solder.
This is the next try:   (4 TI LM2594/95 synthesizers + test stuctures)
< https://www.flickr.com/photos/137684711@N07/51844498620/in/datetaken/     >
red = top, green = bottom, inner layers cut out.
setup on tdr refl. + transmission:
< https://www.flickr.com/photos/137684711@N07/53780177186/in/dateposted-public/     >
result:
< https://www.flickr.com/photos/137684711@N07/53780597885/in/dateposted-public/       >
The SMAs are at division 7 and 8. Very slightly overcompensated,
it could also mean that I need some more GND vias.
The microstrip is slightly more than 50 Ohms. JLCPCB's calculator
says 11.5 mil for 50, it took only 10 to see if I can easily escape
a BGA.  The funny bends are not really punished.
The 10 cm of FR4 do not demolish the rise time. Not bad for
€1.40 per 4 layer board.
regards,
Gerhard