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

Fred Balistreri (*fred@apsimtech.com*)

*Tue, 09 Dec 1997 09:34:50 -0800*

John Lin - TAO 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.*

*> *

*> 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*

*> >*

John, I ran an experiment with a field solver. Your "green" paint would

have to be roughly the same thickness of the trace, about 1.8 mils and

have a dielectric constant of around 5 in order to reduce the impedance

by 9 ohms. It is most likely that the impedance mismatch is due to

serveral factors one of which is solder mask. The other culprits are

likely to be the FR4, assumed to be 4.5 may actually be a bit higher,

distance to the planes assumed to be around 13 mils may actually be

smaller, and the actual width of the traces may be a bit wider than

thought. The thickness of the copper will not play a factor but etching

of the width would. Over etched would cause the impedance to go up not

down of course.

But the results clearly show that solder mask will cause impedance

changes. How much depends on the dielectric constant of the paint and

how thick it is applied. Hope this helps.

Best Regards,

--
Fred Balistreri
fred@apsimtech.com
http://www.apsimtech.com