Perhaps someone from Polar would like to comment, especially about the
source for their equations?
Andrew Preston,
Micromass Ltd,
Wythenshawe, tel: +44 161 718 4593
Manchester. fax: +44 161 998 8915
M23 9LZ, UK e-mail: Andrew.Preston@micromass.co.uk
> ----------
> From: John Lin - TAO[SMTP:LinJohn@digital.com]
> Sent: 09 December 1997 09:01
> To: 'alterra@adnc.com'; 'SI_LIST'
> Cc: Bg Fan
> 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=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
> >
>
>