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=4.5)
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.
Thanks,
JOHNLIN
CAE Engineer of EDA Department
Digital Equipment Corp. Taiwan Branch
Email: Linjohn@mail.dec.com
TEL: 1-886-3-3900000 ext. 2152
-----Original Message-----
From: alterra@adnc.com [SMTP:alterra@adnc.com]
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
slightly
and thus reduce the inductance and impedance below that calculated
without
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.
The
impedance of all transmission lines made with solid conductors will
have a
constant low frequency impedance, a transition frequency range (where
the
skin depth is approximately equal to the conductor thickness), and a
constant but lower high frequency value. This is due to the inductance
of
the line changing with frequency which in turn is due to the skin
effect.
The decrease in impedance in commonly used structures is typically 10%
which
is what you observed.
I can calculate this for your particular structure if you need a
quantitative answer.
Hope this helps.
Eric
---------------------------------------------------------------
Eric Wheatley Ph.D. (760) 942-9426 (phone)
Alterra Technology Co. (760) 942-2366 (fax)
Encinitas, CA 92024 alterra@adnc.com
---------------------------------------------------------------
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.
>
>
>JOHNLIN
>CAE Engineer of EDA Department
>Digital Equipment Corp. Taiwan Branch
>Email: Linjohn@mail.dec.com
>TEL: 1-886-3-3900000 ext. 2152
>