Re: [SI-LIST] : Does solder mask reduce trace impedance ?

Kenneth Willis (kwillis@cadence.com)
Tue, 9 Dec 1997 07:10:59 -0500 (EST)

Hi,

My first job out of school was with a PCB fabricator, and I used to be
responsible for building impedance-controlled boards. I know that putting
solder mask on external traces definitely reduces the impedance, as I had to
characterize this effect. It is dependent to some degree on the geometry of
the conductors, but for a 6 mil trace, 1/2 oz copper plated up,
6 mil FR4 dielectric, it was not uncommon to see drops of 4-5 ohms.

Putting solder mask on turns your surface microstrip into a buried microstrip.
Instead of having air above the conductor (which most equations assume), you
have a thin dielectric with an Er > air. This increases the effective
permittivity seen by the conductor and the impedance dives a bit. What most
good fabricators will do is characterize this and add some fudge factor to
their equations.

But a 9 ohm drop sounds like too much just because of the mask. It sounds more
like either a heavier copper weight was used on the external layers, or maybe
the conductors got over-plated. If the impedance coupons are on the outside
edges of the board, this could be the case. The coupons may measure too low
but the actual traces in the middle of the board may even be OK.

Good luck,

Ken Willis
Sr Eng Manager
High Speed R&D
Cadence Design Systems

> From owner-si-list@silab.Eng.Sun.COM Mon Dec 8 20:52 EST 1997
> Errors-To: si-list-approval@silab.Eng.Sun.COM
> From: John Lin - TAO <LinJohn@digital.com>
> To: "'SI_LIST'" <si-list@silab.Eng.Sun.COM>
> Subject: [SI-LIST] : Does solder mask reduce trace impedance ?
> X-Mailer: Microsoft Exchange Server Internet Mail Connector Version 4.0.996.35
> Mime-Version: 1.0
> Content-Transfer-Encoding: 7bit
> Sender: owner-si-list@silab.Eng.Sun.COM
> Precedence: bulk
> X-Lines: 28
>
> Dear all SI experts,
>
> Does solder mask covering PCB reduce the impedance of trace?
> If yes, then what will be the amount of impedance changed.
>
> Previously, we have SCSI back plane. We control the stackup to obtain
> 90 +/- 6 ohms impedance.
>
> After measuring the impedance of real back planes sent back from a
> manufacture, we found the impedance is lower than that of our
> expectation. It is about 81 ohms. The manufacture analyzed the
> backplane by studying the profile of PCB and material used and were
> sure that the impedance should be about 89 ohms.
>
> The engineers of PCB manufacture told us the solder mask covering the
> PCB will reduce the impedance up to 9 ohms.
>
> I just wonder the solder mask affects the impedance so much for a
> PCB board.
>
>
> JOHNLIN
> CAE Engineer of EDA Department
> Digital Equipment Corp. Taiwan Branch
> Email: Linjohn@mail.dec.com
> TEL: 1-886-3-3900000 ext. 2152
>
>
>