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

Ravinder Ajmani ([email protected])
Tue, 9 Dec 1997 15:11:49 -0500

I too have observed an impedance drop of 8-9 Ohms due to various manufa=
process variations, including solder mask. I use an impedance calculat=
program from SMT Plus, Inc., which is written by Lee Ritchey and James
Blankenhorn. The authors claim that their program takes into account i=
variations due to manufacturing processes, and provides most accurate i=
This is a DOS based program with very few features, but I have found th=
results obtained very close to our actual PC Boards impedance. Using t=
parameters of your backplane with this program, I got an impedance valu=
e of
82.7 Ohms for 13.2 mil dielectric thickness, and 81.7 Ohms for 12.8 mil=
dielectric thickness, which are quite close to what you have actually m=
with TDR. The program has a field for entering solder mask thickness, =
but this
figure doesn't change the impedance value because as per the authors, t=
program takes into account thin solder mask.
Even with the best impedance calculator program, you may still see vari=
in impedance due to liberal tolerances in PCB manufacturing. If you ar=
e using
same fab all the time then the best thing to do is to characterize thei=
r PCBs
by making actual TDR measurements, and then using the same factor to ca=
the impedance for a new stackup. We have used this methodology success=
for normal, and differential signal traces. If you are interested in g=
the software from SMT Plus, Inc. then you can write to them at P.O. Box=
San Jose, CA 95161-2314.

Regards, Ravinder
EMC & Signal Integrity Engineer
PCB Development and Design Department
Voice : (408) 256-7956 T/L : 276-7956 Fax : (408) 256-0550=

Email: [email protected]

[email protected] on 12/09/97 01:41:43 AM
Please respond to [email protected] @ internet
To: [email protected] @ internet, [email protected] @ internet
cc: [email protected] @ internet
Subject: RE: [SI-LIST] : Does solder mask reduce trace impedance ?

Dear Dr. Wheatley,

Thanks for your valuable opinions.
Sorry for not providing detail information.

The stackup is SCSI single end backplane. The impedance is needed to
be controlled around 90 ohms +/- 10 ohms for most of signals and +/- 6
ohms for two control signals.

The solder mask here is a green paint covering all over PCB except the
solder pad. to isolate copper surface, microstrip line, from air.

Several SI books provide formula to calculate microstrip impedance,
ex. High Speed Digital Design by Howard W. Johnson.
They don't mention about the effect of the green paint in their
formula. I simply consider this factor is omissible.

The measurement values for impedance parameters are

4 layer structures :
Layer 1 ----------------- (Signal) 1.8 mils
FR-4 13.2 mils (Er=3D4.5)
Layer 2 ------------------ (Ground) 1.2 mils
FR-4 61 mils
Layer 3 ------------------ (Power) 1.2 mils
FR-4 12.8 mils
Layer 4 ------------------- (Signal) 1.8 mils

Trace width is 5.5 mils.
Based on the measurement values and the formula, the impedance should
be 89.9 ohms for traces on Layer 1 and 4.

Then, I use TDR to measurement the impedance. It is only 81 ohms.


CAE Engineer of EDA Department
Digital Equipment Corp. Taiwan Branch
Email: [email protected]
TEL: 1-886-3-3900000 ext. 2152

-----Original Message-----
From: [email protected] [SMTP:[email protected]]
Sent: Tuesday, December 09, 1997 10:43 AM
To: John Lin - TAO
Subject: Re: [SI-LIST] : Does solder mask reduce trace impedance ?

Hello John,

You do not provide enough details for me to give you a definite
answer but
I strongly suspect that your impedance change is due to the frequency
dependence of the inductance of your traces.

There are two possible effects here and I cannot tell which is most
impportant in your case without calculations.

a) Adding the solder mask will increase the size of the conductor
and thus reduce the inductance and impedance below that calculated
the solder mask.

b) More likely, I suspect someone calculated the low frequency
impedance for
you and you are measuring the impedance at a much higher frequency.
impedance of all transmission lines made with solid conductors will
have a
constant low frequency impedance, a transition frequency range (where
skin depth is approximately equal to the conductor thickness), and a
constant but lower high frequency value. This is due to the inductance
the line changing with frequency which in turn is due to the skin
The decrease in impedance in commonly used structures is typically 10%
is what you observed.

I can calculate this for your particular structure if you need a
quantitative answer.

Hope this helps.


Eric Wheatley Ph.D. (760) 942-9426 (phone)
Alterra Technology Co. (760) 942-2366 (fax)
Encinitas, CA 92024 [email protected]

At 09:19 AM 12/9/97 +0800, you wrote:
>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.
>CAE Engineer of EDA Department
>Digital Equipment Corp. Taiwan Branch
>Email: [email protected]
>TEL: 1-886-3-3900000 ext. 2152