FreeLists / si-list / [SI-LIST] Re: PCB Trace impedance algorithms - Free trace calculator

["Dennis Han" <Dennis.Han@xxxxxxxxxxxxxxx>]

Allegro uses a 2D field solver, unless you are using an old version,=0D=0A
probably less than 15.0.  It is more accurate than closed-form equations=0D=
=0A
as long as a good stack-up is built in it.  Just remember to add solder=0D=
=0A
mask (called conformal coating in Allegro).  Here is what I use based on=0D=
=0A
data received from Multek:=0D=0A
=0D=0A
-- Solder mask is 0.7 mils thick, dielectric constant is 3.75, loss=0D=0A
tangent is 0.02 (Allegro uses 0.79 mils thick and 3.00 as defaults for=0D=
=0A
conformal coating).=0D=0A
-- Use 3.75 and 0.02 on each side of the microstrip since solder mask=0D=0A
will flow around it (Allegro uses 1.0 and 0 as defaults).=0D=0A
-- Compensate for how prepreg forms around conductors by using a=0D=0A
dielectric constant of 3.05 and a loss tangent of 0.014 on each side of=0D=
=0A
embedded microstrip, stripline, and off-center stripline (Allegro uses=0D=
=0A
1.0 and 0 as defaults).=0D=0A
-- 0.5 oz/sq ft of copper is 0.6 mils thick (matches Allegro's default).=0D=
=0A
-- 1.0 oz/sq ft of copper is 1.2 mils thick (matches Allegro's default).=0D=
=0A
-- Plating on the outside layers is 1.2 to 1.4 mils thick depending on=0D=
=0A
the stack-up.  Add this thickness to the base copper.  For example, if=0D=
=0A
the base is 0.5 oz/sq ft, then the overall thickness of the conductor is=0D=
=0A
1.8 to 2.0 mils (Allegro uses 2.1 mils as a default for copper foil).=0D=0A
-- The dielectric constant and loss tangent for high-temperature FR4 are=0D=
=0A
4.0 and 0.014, respectively (Allegro uses 4.5 and 0.035 as defaults and=0D=
=0A
these are too high).=0D=0A
-- Disadvantage is the field solver in Allegro cannot tell you easily=0D=0A
how far away to keep adjacent lines.=0D=0A
=0D=0A
Dennis=0D=0A
=0D=0A
=0D=0A
-----Original Message-----=0D=0A
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]=0D=
=0A
On Behalf Of Salkow, Steven=0D=0A
Sent: Friday, March 02, 2007 12:46 PM=0D=0A
To: si-list@xxxxxxxxxxxxx=0D=0A
Subject: [SI-LIST] Re: PCB Trace impedance algorithms - Free trace=0D=0A
calculator=0D=0A
=0D=0A
Dear Sam:=0D=0A
What is important is that the trace widths you initially throw down on=0D=
=0A
your PCB meet the following concurrent requirements:=0D=0A
1.      Satisfy your board's house minimum trace width when the trace is=0D=0A
over etched by 10% =0D=0A
2.      Are lower in initial impedance so they may be etched to your=0D=0A
required impedance accuracy=0D=0A
3.      Meet your companies' manufacturing standards for reliability=0D=0A
4.      Use different trace widths for differential or single ended=0D=0A
signals on the same layer having the same target impedance=0D=0A
=0D=0A
No matter which ECAD tools or calculator you use to determine the cross=0D=
=0A
section of your traces, these initial values will be adjusted by the PCB=0D=
=0A
fabricator. When the Gerber files get to the fabricator, there are no=0D=0A
net names that relate back to your original design in a meaningful way,=0D=
=0A
hence, you fabrication drawing will be forced to make statements such as=0D=
=0A
"all 9.75 mils line on microstrip layers are differential and 50 ohms=0D=0A
+/- 10%." This allows the pcb fabricator to grab the 9.75 mils traces on=0D=
=0A
all surface layers and tweak their widths according to their process=0D=0A
adjusting for etch and dielectric constant and variation is lamination=0D=
=0A
thicknesses.=0D=0A
=0D=0A
Tools you may have may not account for the soldermask when calculating=0D=
=0A
microstrip. Other calculators such as=0D=0A
mine(http://www.bychoice.com/stripline.exe), defaults to a soldermask=0D=0A
thickness of 1 mil and er =3D 4.7. When evaluating calculators, compare=0D=
=0A
several to Cadence Allegro over the RANGE YOU INTEND TO USE. =0D=0A
  =0D=0A
I have made a comparisons of several tools over a limit range=0D=0A
http://www.bychoice.com/microstrip_calculations_for_embedded_circuits_su=0D=
=0A
mmary.xls=0D=0A
=0D=0A
Any tool that is within 2% should meet your needs fine. My calculator is=0D=
=0A
not only free but shows the equations.=0D=0A
=0D=0A
In the above comparisons, I am attempting to create a new equation for=0D=
=0A
embedded microstrip that will do a better job with varying thicknesses=0D=
=0A
of soldermask. If any one want to help, its fine with me.=0D=0A
=0D=0A
Steven Salkow=0D=0A
Lockheed IS&S=0D=0A
3130 Zanker Rd, San Jose=0D=0A
Ca. 95134=0D=0A
=0D=0A
steven.salkow@xxxxxxxx=0D=0A
salkow@xxxxxxxxxxxx=0D=0A
=0D=0A
=0D=0A
=0D=0A
-----Original Message-----=0D=0A
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]=0D=
=0A
On Behalf Of Sam Sam=0D=0A
Sent: Monday, January 22, 2007 7:35 PM=0D=0A
To: si-list@xxxxxxxxxxxxx=0D=0A
Subject: [SI-LIST] PCB Trace impedance algorithms=0D=0A
=0D=0A
Dear si-list members,=0D=0A
   =0D=0A
  I am learning tool support for pcb designs. I have some questions=0D=0A
regarding calculating impedance of a traces in PCB. I use allegro's=0D=0A
built impedance calculator. I am also aware that there are various other=0D=
=0A
calculator tools from UltraCAD, Polar Instruments etc. I am wondering=0D=0A
how efficient and accurate these calculations are. I guess most of them=0D=
=0A
use some kind of assumptions and have simplified closed form formulas to=0D=
=0A
qucikly extimate the impedance. But can you people guide me as what is=0D=
=0A
the exact technique or algorithm to calculate the impedance of a pcb=0D=0A
trace say for a microstrip structure. Any papers or links to this study=0D=
=0A
would be appreciated. In specific, since i am using allegro 's=0D=0A
calculator i would like to know how they calculate the impedance and=0D=0A
what are the assumptions they take. I have seen most calculator allow=0D=0A
single ended and differential trace calculations. Is it possible to=0D=0A
extend these techniques to multiple traces. More importantly the=0D=0A
accuracy of the  formulas is of concern to me. When compared to full=0D=0A
wave results these formulas from different tools give different result.=0D=
=0A
So i am looking to learn what is the background behind these? Please=0D=0A
advise me on this.=0D=0A
Thanks in advance. Looking forward for your answers....=0D=0A
   =0D=0A
   =0D=0A
  Sam=0D=0A
                =0D=0A
---------------------------------=0D=0A
All new Yahoo! Mail=0D=0A
---------------------------------=0D=0A
Get news delivered. Enjoy RSS feeds right on your Mail page.=0D=0A
=0D=0A
------------------------------------------------------------------=0D=0A
To unsubscribe from si-list:=0D=0A
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field=0D=0A
=0D=0A
or to administer your membership from a web page, go to:=0D=0A
http://www.freelists.org/webpage/si-list=0D=0A
=0D=0A
For help:=0D=0A
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field=0D=0A
=0D=0A
=0D=0A
List technical documents are available at:=0D=0A
                http://www.si-list.net=0D=0A
=0D=0A
List archives are viewable at:     =0D=0A
                http://www.freelists.org/archives/si-list=0D=0A
or at our remote archives:=0D=0A
                http://groups.yahoo.com/group/si-list/messages=0D=0A
Old (prior to June 6, 2001) list archives are viewable at:=0D=0A
                http://www.qsl.net/wb6tpu=0D=0A
  =0D=0A
=0D=0A
------------------------------------------------------------------=0D=0A
To unsubscribe from si-list:=0D=0A
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field=0D=0A
=0D=0A
or to administer your membership from a web page, go to:=0D=0A
http://www.freelists.org/webpage/si-list=0D=0A
=0D=0A
For help:=0D=0A
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field=0D=0A
=0D=0A
=0D=0A
List technical documents are available at:=0D=0A
                http://www.si-list.net=0D=0A
=0D=0A
List archives are viewable at:     =0D=0A
                http://www.freelists.org/archives/si-list=0D=0A
or at our remote archives:=0D=0A
                http://groups.yahoo.com/group/si-list/messages=0D=0A
Old (prior to June 6, 2001) list archives are viewable at:=0D=0A
                http://www.qsl.net/wb6tpu=0D=0A
  =0D=0A
=0D=0A
=0D=0A
Legal Disclaimer:=0A
The information contained in this message may be privileged and confident=
ial. It is intended to be read only by the individual or entity to whom i=
t is addressed or by their designee. If the reader of this message is not=
 the intended recipient, you are on notice that any distribution of this =
message, in any form, is strictly prohibited. If you have received this m=
essage in error, please immediately notify the sender and delete or destr=
oy any copy of this message=0D=0A
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field


List technical documents are available at:
                http://www.si-list.net

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu