Thanks much , Gert .
Yes , our launch showed less than 2 ohms of variation @ 100 PS, Pulse .Launch
does not look to bethe issue .Problem seems to be with the RF traces .
Fab's carry out the measurement through TDR , which is more like static .The
measurements are made on the test coupons , where the traces look much Isolated
& straight ,compared to the actual traces on the PCB. The freq response on the
VNA is what is bothersome .
On the CPW lines - One clarification is that , we use CPW with G .Meaning the
trace is referenced to the second layer (also) , which is a continuous Gnd .
As an example , Trace width = 10 mil , Trace to Gnd clearance on either of
thetrace is 18 mil . Fr4 , Prepeg to second layer is 5 mil thick.We
deliberatelymade the Gnd separation as 18 mil to reduces the Radiation lossesÂ
( if theRF trace is very close to Gnd ).
Based on your input , we will try with lesser gaps to Gnd.
I'am not looking for any ideal RF traces . A return loss of around 15 dB @ 2 to
6 Ghz , wouldbe sufficient .
RegardsSunil.B
From: "Havermann, Gert" <Gert.Havermann@xxxxxxxxxxx>
To: "dmarc-noreply@xxxxxxxxxxxxx" <dmarc-noreply@xxxxxxxxxxxxx>;
"tom@xxxxxxxxxxxxxxxxx" <tom@xxxxxxxxxxxxxxxxx>
Cc: si-list <si-list@xxxxxxxxxxxxx>
Sent: Tuesday, December 20, 2016 3:30 PM
Subject: [SI-LIST] Re: 50 ohm - RF Impedance Traces
I think that the topology is the problem. Coplanar waveguides are not easy to
control, especially when the clearance to GND is too tight or too large, and 18
mil is really large. Just imagine that the electrical field will be active in
an area at least 3 times the GND- distance all around your trace. When there
are other traces/circuits underneath, or some mechanical parts (table, skrews,
housings....) then they all influence the Impedance.
You also need to take into account that in reality you will not see an perfect
open in the smith chart just because the trace has an open end somewhere. You
need to take the trace inductance and capacitance into account, and electrical
length also changes the "dot" smith chart. The Laminate itself is also
frequency dependent so it will be almost impossible to create an perfect open
with a long trace.
Please define " the launch does not look bad either". What is the TDR Risetime
and what kind of impedance deviations do you measure? For 6GHz you should test
with at least 100ps Risetime, and a decent launch should then vary by less than
5 Ohm. A good launch will vary in the 1ohm range. If you plan on even higher
frequencies, then the same applies for 30ps risetime. And thatâs just some
rule of thumb without knowing all the details it is hard to really give a
recommendation right on the spot.
BR
Gert
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of sunil bharadwaz
Sent: Tuesday, December 20, 2016 8:38 AM
To: tom@xxxxxxxxxxxxxxxxx; dmarc-noreply@xxxxxxxxxxxxx
Cc: si-list <si-list@xxxxxxxxxxxxx>
Subject: [SI-LIST] Re: 50 ohm - RF Impedance Traces
Hello Tom ,
Thanks much for your response .Thanks much to all ,who have replied to this
thread.
The launch is a proper SMA connector . The final board is going to carry this
RF connector . On the TDR , the launch does not look bad either .However , one
observation is that , the larger the 50 ohm traces , worse is thereturn loss @
5 Ghz & above .
I'am checking @ Test coupon as well as the actual board .On the actual board
,the RF trace has a SMA connector on one side & the other end is open .On the
VNA , when we check the S11 @ Smith chart , ideal Transmission line should have
a dot to the right extreme indicating that the line is open .However , i see
all kinds of shapes @ frequency.
Can we get the solder mask done in normal way or do we have to take any special
care in getting the solder mask done on the RF traces ?
We generally use Co planar Waveguide traces (with ground ) , for 50 ohms lines.
Typically , theRF trace widths are 15 mil @ 18 mil distance from ground running
on either sides . We did extractthe S-parameters before sending the Layout for
Fab . Fab of course did send us the impedance report (measured on TDR ).
RegardsSunil.B
   From: Tom Dagostino <tom@xxxxxxxxxxxxxxxxx>
To: dmarc-noreply@xxxxxxxxxxxxx
Cc: si-list <si-list@xxxxxxxxxxxxx>
Sent: Sunday, December 11, 2016 11:47 PM
Subject: [SI-LIST] Re: 50 ohm - RF Impedance Traces
How good is your launch into your test trace? If it has a large discontinuity
it may be masking the true impedance. Try looking at the trace with a TDR
display and see what the trace impedance is.
Tom Dagostino
Teraspeed LabsOn Dec 11, 2016 8:17 AM, sunil bharadwaz
<dmarc-noreply@xxxxxxxxxxxxx> wrote:
------------------------------------------------------------------
Hello Group ,
We seem to be running into issues while getting PCB's fabricated with 50 ohm
lines.Our Freq band of interest is 2 Ghz to 6 Ghz.Tried checking these traces
on a VNA.The return loss looks decent @ 2 Ghz , but seldom looks good at 5Ghz
& above .
The fabricator does send test coupons & impedance reports @ TDR .This does
notcover the freq response .
This is not issue with any single fab . This seems to be a general problem ,
where return loss isnot flat across freq band .
Wanted to check if there are ways to tackle this issue .
Thanks much.
RegardsSunil.B
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
        http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
