Re: AW: [SI-LIST] : SMA test connector PCB layout

About this list Date view Thread view Subject view Author view

From: William Devey (deveyw@us.ibm.com)
Date: Wed Jan 03 2001 - 08:41:32 PST


I agree with Ulrich. I laid out a signal itegrity test board using SMA
through-holes, believing
the data sheet data which indicated good performance to 1.8Ghz and above. I
also tried the
vertical surface mount version (Johnson PN 142--0711-201)

I was shocked at how wretched the transition was between high quality 50
ohm coax and
my ~50 ohm strip line using both of the above. I was able to achieve a much
better transition
by carefully dressing a bare coax cable end with lead lengths less than .1
inch and carefully
soldering these to two .013"x.026" vias spaced .100", and connented to the
stripline and ground plane respectively.

A board edge SMA connector exists (Johnson PN 142-0701-851, or
142-0701-801) for
.063" thick boards. They also exit for thinner board material. I have not
tried these
but now believe that they have MORE potential for a clean transition than
any through
hole deviece.

Regards,

Bill DeVey
IBM Staff (Linear) Systems Engineer
15450 SW Koll Parkway
Beaverton, OR 97006
Phone: 503-578-5728
FAX: 503-578-5797
Cell: 503-936-8226
deveyw@us.ibm.com

"Wallenhorst, Ulrich" <Ulrich.Wallenhorst@HARTING.com>@silab.eng.sun.com on
01/03/2001 06:02:04 AM

Please respond to "Wallenhorst, Ulrich" <Ulrich.Wallenhorst@HARTING.com>

Sent by: owner-si-list@silab.eng.sun.com

To: "'Si-List (E-mail)'" <si-list@silab.eng.sun.com>
cc:
Subject: AW: [SI-LIST] : SMA test connector PCB layout

Larry,

I recommend to avoid any plated through-hole SMA-launcher. The thicker the
boards the more critical the degrading capacitive effects will be with not
real chance to compensate with tricks like counter drilling or higher
inductive trace-impedance in mm-distance from the signal-pad. You can
indeed use SMA edge-connectors. You have to use the version with only 2
ground pins and solder it properly on the boards and guarantee a very low
inductive path by e.g. using self-build metal-blocks. If this option is not
suitable for Your application the remaining alternative are low-capacitance
probe tips.

Best regards

Ulrich Wallenhorst

HARTING KGaA
Dept.:   Electronic Connectors Division
Director of Advanced Interconnection Solutions
E-Mail:  ulrich.wallenhorst@HARTING.com
http://www.HARTING.com
Phone: +49 57 72 47-294
Mobile: +49 160 533 6786
Fax.:    +49 57 72 47-471

   ----------
   Von:    Larry Miller[SMTP:ldmiller@rhapsodynetworks.com]
   Antwort an:     Larry Miller
   Gesendet:       Mittwoch, 3. Januar 2001 14:38
   An:     Si-List (E-mail)
   Betreff:        [SI-LIST] : SMA test connector PCB layout

   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 - 14:30:32 PDT