Re: SPICEing The Inductance of a Trace Over a Ground Plane?

On Mon, 17 Sep 2007 14:33:30 -0700, "Joel Kolstad"
<JKolstad71HatesSpam@xxxxxxxxx> wrote:

"D from BC" <myrealaddress@xxxxxxxxx> wrote in message
news:l3lte35q2676mf35tb042v8qcqnhq4dfj8@xxxxxxxxxx
I've yet to see a number of how far away that ground plane really is..

It can be whatever you'd like.

I put in:
w = 20mil trace width = 0.000508meters
t= 1oz copper = 0.0014in = 0.0000356 meters
h = 0.8mm = 0.0008 meters
ur = 1

I get an error! Fk...??

That much separation is (0.8mm ~= 32mils) is higher than most people would
use, but certainly within the realm of possibility. (Although your air
dielectric there seems a little unlikely...)

That or bad coding..

Bad coding. A lot of these programs use "curve-fitted" equations that become
highly inaccurate or impossible outside of the original domain of the fit...
and unfortunately over time the limits of that domain tend to get lost.

You might try a program such as
http://web.appwave.com/Products/Microwave_Office/Feature_Guide.php?bullet_id=9
-- it has no (immediate) problem with your dimensions, giving a
characteristic impedance of 152 ohms... which is probably a bit inaccurate, as
experience indicates it's generally somewhat difficult to achieve line
impedances that high (i.e., the actual impedance is probably a bit lower,
although in air... maybe not...)

How are designers selecting how far away the ground plane should be?

If you're doing RF designs, you generally have some specified impedance you're
shooting for. With digital designs, you often look at the minimum trace width
you'd like to use and then set the ground planes such that you get some
"reasonable" impedance (100 ohms is a popular target...). But there's also
the consideration that moving the ground plane closer to the trace gets you
tighter coupling (between a signal net and the plane) and hence a little
better isolation (less noise) between traces, whereas moving the planes closer
together couples them more tightly and thereby provides more decoupling
capacitance. Generally on 4-layer boards you don't really have the option to
stick the planes particularly close together because it leds to signal traces
being much wider (>>10 mils, say) than you'd prefer for the sake of signal
routing density. (And providing decoupling in the form of discrete caps is
cheap and easy.)

The rule of thumb is that, in FR-4 (relative permittivity ~ 4.7), using trace
width equal to distance from the plane gives an impedance of ~70 ohms, whereas
using trace width twice the distance from the plane gets you ~50 ohms -- both
quite workable values.

I'm trying to spice trace inductance over a ground plane.

OK... programs like TxLine will give you characteristic impedance and the
*effective* dielectric constant. Using Z0=sqrt(L/C) and v (signal of light in
the medium)=1/sqrt(permittivity*permeability), you can play with the algebra
and come up with inductance (per unit length) as Z0/v and capacitance as
1/(Z0*v). Example: Using W=20 mils, H=10 mils, TxLine says you have a
microstrip line with impedance of 47.2 ohms and effective dielectric constant
= 3.586. v=3e8/sqrt(dielectric constant)=158.4 m/s, so you have inductnace =
Z0/v = 298nH/m and capacitance = 1/(Z0*v) = 133.7pF/m. So, something like a
10cm trace at low frequencies (low enough that the trace can be considered a
lumped element) could be modeled as a series 2.98uH inductor along with a
parallel 13.4pF capacitor... which can be neglected at "low enough"
frequencies.

Note that In Real Life there are all sorts of little corrections you have to
do to account for end effects any time the trace changes direction or shape
(including at the beginning and end), but these can be ignored in most cases
until you're up in the hundreds of MHz or so regions. (By the time you hit a
GHz, this is all a Very Big Deal...)

---Joel


Wow... hey thanks that's alot of info..
Thanks..


Using your example...
10cm of the specified trace looks like this in spice:


+ ---------| 13.4pF|----+
| |
+-----////2.98uH///-----+-----------+
| |
| |
pulse load
| |
| gnd
gnd


for low frequencies as mentioned above..
(R neglected.)


I thought it would be some long repeating LRC network ..


D from BC
.

Loading