Electronics > PCB/EDA/CAD

Measurement of different PCB trace width with R&S ZLNE-3 VNA / JLCPCB

<< < (12/12)

Gerhard_dk4xp:
Everybody seems to do just this. We just had a discussion about solder mask effects
on usenet sci.electronics.design which is mirrored by google groups.
JL found out that the solder mask has no visible effect on the TDR (other manufacturer).
JohnL also said that the SMAs with the thick inner conductor have 100 Ohms in air
already without any board attached. I believe that.

I also tested the JLCPCB process with an Agilent 54754A TDR.
The 11.5 mil trace  seems to be absolutely correct. I drew it as 12 mil
in Altium, that makes it maybe a tad lower impedance when the
50 Ohm line in the 54754A is taken as a reference.

My SMA launchers were a disaster. I took the ones for a 2 layer board
and the center conductor was much too large.
The next board is on its way, with GND cut outs in the SMAs. I have no
idea where. Shipment tracking says it was in in Leipzig, Germany and
somehow it has jumped back to Hong Kong???
The board is a 15 GHz LMX2594 synthesizer to be shown in DUBUS 1/22
so I can't be too verbose bc I have promised the ius primae noctis to
Dubus , but methinks they'll tolerate a picture for a discussion.

Cheers, Gerhard

rfclown:
Notice that Gerhard_dk4xp's board does not have ground on the top layer near the trace. This is microstrip. With ground on either side you have a grounded coplaner waveguide which has more capacitance per unit length than microstrip and therefore lower impedance (Zo=SQRT(L/C)) given the same dimensions (width, height). Solder mask has minimal effect. Conductor thickness has more effect than mask, which is why you need to calculate with the finished thickness (after plating). When doing boards with a thin dielectic on the top layer which makes for a thin 50 ohm line, if the pad for the SMA edge launch pin needs to be wider, you can eliminate ground directly under the pin pad to increase the dielectric thickness. I'll calculate what the pin pad width will be (to get 50 ohms) if the ground is on layer 3, or 4, or 5... I'll chose a ground reference layer for the pin pad that gives me an appropriate width for soldering the SMA pin.

Navigation

[0] Message Index

[*] Previous page

There was an error while thanking
Thanking...
Go to full version