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

[email protected]
Tue, 09 Dec 1997 18:22:16 -0800


Thank you for the details of your structure. I took a look at the top layer
with the 13.2 mil FR-4 thickness, assumed the ground plane below was
infinitely wide, and used your value for the permittivity of FR-4 so this is
simply a microstrip structure with no coating. I evaluated the line
parameters using the Ansoft 2D simulator as a function of frequency from
100kHz up to 500 MHz with the following results:

R is ohms/m
L is nH/m
C is pF/m

f R L C Z
100k 2.839 609.0 61.77 99.29
1MHz 2.895 588.2 " 97.58
10MHz 3.960 571.6 " 96.20
30MHz 6.149 556.7 " 94.93
100MHz 11.05 543.5 " 93.80
200MHz 15.50 538.6 " 93.38
500MHz 24.46 534.2 " 92.99
limit 529.0 " 92.54

The characteristic line impedance was taken from just the L and C values
since above 10 MHz the resistance does not contribute significantly to the
impedance. As you can see, the characteristic impedance decreases about 6.3
ohms over this frequency range for your structure which is what led to my
original speculation about the cause of your low impedance.

You do not say what the solder mask thickness is nor its permittivity so I
cannot give you any quantitative feedback on the coated structure. However,
as others have pointed out, the presence of the coating will certainly
increase the capacitance and lower the impedance at all frequencies. For
example, if the coating was sufficient to increase the line capacitance to
75 pF/m, then the impedance would be 90 ohms at 100 kHz (again neglecting
the resistive part) and would be 84 ohms at 500 MHz. The important point in
all this is to make sure you know whether your design software is giving you
low or high frequency limiting values for your line parameters when
impedance must be closely controlled.

In addition to everyone else's comments regarding material property
variations or geometry variations (which I agree with) I would also like to
point out that a TDR measurement gives you an averaged result over a broad
frequency range. It may not be meaningful at the particular operating
frequency of interest. When accuracy is important as it is in your case, I
recommend that you use a single frequency technique (e.g. a network
analyzer) to measure the line impedance at a frequency which is important in
your system.

Best regards,


PS What specific formula did you use to get the expected impedance value of
89.9 ohms?

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

At 05:01 PM 12/9/97 +0800, you wrote:
>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=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.