Path: ...!Xl.tags.giganews.com!local-2.nntp.ord.giganews.com!nntp.supernews.com!news.supernews.com.POSTED!not-for-mail
NNTP-Posting-Date: Sun, 09 Jun 2024 20:51:37 +0000
From: john larkin <jl@650pot.com>
Newsgroups: sci.electronics.design
Subject: Re: RF Connector Type ID
Date: Sun, 09 Jun 2024 13:51:36 -0700
Message-ID: <625c6jdqe8f577kh5ik3bkq4p1aqugb4sc@4ax.com>
References: <v426ri$2ni84$1@dont-email.me> <f1d96jtvb2pokgermt7fqt751ed9gpjfcn@4ax.com> <v42jgp$2gbeq$1@dont-email.me> <v42ju0$2gbeq$2@dont-email.me> <97s96j5fajs26f6eg9odqs48skgghoson5@4ax.com> <v43vk8$3dhg7$2@dont-email.me> <ntfb6jlp9g4i62rdkjv3fr692jm46u541i@4ax.com> <v453sq$1dufm$1@solani.org>
User-Agent: ForteAgent/8.00.32.1272
MIME-Version: 1.0
Content-Type: text/plain; charset=ISO-8859-1
Content-Transfer-Encoding: 8bit
Lines: 84
X-Trace: sv3-CejEOl5aqaCKksMD4UuAcMHNgnQYnEolwMFZWTCbdGSzEcMlK6qocJoBOWAXFF5ikzNDdEuQBab6d6W!7XizLizUrzMk5xEAIq7MQ37mrK2WTZ6Yi1Jwz7sUv5Oczl8+1Git0DID8/atyWqHnd0UCjrVnh+g!Rwx6Eg==
X-Complaints-To: www.supernews.com/docs/abuse.html
X-DMCA-Complaints-To: www.supernews.com/docs/dmca.html
X-Abuse-and-DMCA-Info: Please be sure to forward a copy of ALL headers
X-Abuse-and-DMCA-Info: Otherwise we will be unable to process your complaint properly
X-Postfilter: 1.3.40
Bytes: 4162

On Sun, 9 Jun 2024 22:38:50 +0200, Gerhard Hoffmann <dk4xp@arcor.de>
wrote:

>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.

That pic was the connector on a PCB that was intended for the big-pin
part. A skinny trace would be appropriate for the Mueller SMA, but in
real life the cheaper big-pin part TDRs about the same.

>
>< 
>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.

We tweak the pad stack to compensate for the big pad. That works
pretty well.

>
>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/ 

Big improvement.

>      >
>
>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.

Short traces on cheap boards are pretty good.

>
>regards,
>Gerhard
>
>
>
>