RE: [SI-LIST] : SMA test connector PCB layout

About this list Date view Thread view Subject view Author view

From: Larry Miller (ldmiller@rhapsodynetworks.com)
Date: Wed Jan 03 2001 - 11:33:41 PST


Thanks! That's exactly what I ordered.

I agree about "caring about" discontinuities on TDR measurements. However,
they are not so hidden from E-Z view in TDR as in a frequency-domain
measurement.

I've had a number of 1 Gb SERDES manufacturers' evaluation boards with
conventional SMA connectors with no problem (as well as the end-fire setups)
but these were comparatively short trace lengths, etc., etc.

Larry Miller
  -----Original Message-----
  From: owner-si-list@silab.eng.sun.com
[mailto:owner-si-list@silab.eng.sun.com]On Behalf Of Bob Lewandowski
  Sent: Wednesday, January 03, 2001 10:41 AM
  To: Larry Miller
  Cc: Si-List (E-mail)
  Subject: Re: [SI-LIST] : SMA test connector PCB layout

  Johnson Components has an "end launch" SMA that fits into a slot in the
board edge, with a pin to contact a top surface microstrip trace. It's
application is independent of board thickness. Johnson P/N 142-0721-88x.
Their web site is: http://www.johnsoncomp.com/sma.htm. A front view
picture is shown as "End Launch". The pin diameter is 30 mils, so some
adjustment of the launch must be made for trace widths less than 30 mils.
Connection from the body to ground is also a significant issue with this
type of connector. An edge plated slot that ties directly to the ground
layers is best, both electrically and mechanically.
  Your other choice, the 4 ground pin through hole type is difficult to
match to FR-4 or similar Er materials. The best possible application is to
a back side microstrip with minimum center conductor hole and pad diameters.
No pads on inner layers. Clear ground pads on all layers back as far as
possible, and drill holes after plating between the center pin and the
corner pins to reduce capacitance. With careful layout you can get a
reflection coefficient of better than 10%.

  Incidentally, you should care about bad launches with a TDR because a
large launch discontinuity masks (attenuates) downstream reflections.

  ---Bob Lewandowski
      Vixel Corp.

  Larry Miller wrote:

    I need to make some measurements on PC boards up to 5 GHz using a
network
    analyzer. In the past I didn't care that much because I was doing TDR
    measurements.
    Unfortunately, the boards I will be looking at are too thick to use the
"SMA
    edge connector" trick.

    Does anyone have a pointer to a good PCB footprint that will not have
    impedance discontinuities. The connector I want to mount is the familiar
    center pin + 4 ground pins vertical SMA style.

    Thanks in advance for any help,

    Larry Miller

    **** To unsubscribe from si-list or si-list-digest: send e-mail to
    majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
    si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
    si-list archives are accessible at http://www.qsl.net/wb6tpu
    ****

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:33 PDT