<!DOCTYPE html PUBLIC "-//W3C//DTD HTML 4.01 Transitional//EN">
<html>
<head>
<meta content="text/html;charset=ISO-8859-1" http-equiv="Content-Type">
<title></title>
</head>
<body bgcolor="#ffffff" text="#000000">
<meta content="text/html;charset=ISO-8859-1" http-equiv="Content-Type">
<title></title>
Dear All,<br>
<br>
I'm reading a lot off discussions about the self-inductance caused by
PCB tracks and so on leading to capacitors. Using a large surface area
will lower the self-inducttance, true. However, instead of using a
large area (either bij large diameter (via's) or by using wide tracks)
there is another solution. Parallelling multiple "inductors", so
instead of using one big hole, a large numer of small holes (probably
consuming the same amount of baord-space) will give the same or a
better result. The same is true for parallelling multiple PCB tracks.
This will give less coupling capacitance to e.g. other tracks......<br>
<br>
I did some research into ground-leads (part of an ESD protection
project) and it turned out that it was better to use a multicore (each
core insulated) cable than a "solid" copper cable with the same
diameter. The parallel inductance of the single thin wires together
turned out to give better performance than a very thick, not so
flexible, copper cable.<br>
Hope this might add something usefull for the discussion/design. Good
luck!<br>
<br>
Best regards, 73's, Jeroen PE1RGE<br>
<br>
Ray Anderson wrote:<br>
<blockquote
cite="midBD06837F0655E84288539771399A41FF0148EC00@XSJ-EXCHVS1.xlnx.xilinx.com"
type="cite">
<pre wrap="">***** High Performance Software Defined Radio Discussion List *****
</pre>
<blockquote type="cite">
<pre wrap="">.Thanks a million for the links to the papers Ray, they have been very
informative.
</pre>
</blockquote>
<pre wrap=""><!---->
</pre>
<blockquote type="cite">
<pre wrap="">One thing that I haven't come across is the size of the via (drill
</pre>
</blockquote>
<pre wrap=""><!---->size). >I would think for the lowest impedance, you would want as large
a drill >size you can have for the layout. The same could be said for
inductance, >the larger the drill, the lower the inductance. Any
thoughts on via sizes?
</pre>
<blockquote type="cite">
<pre wrap="">In the Xilinx app note, how did they calculate the percentages in Table
</pre>
</blockquote>
<pre wrap=""><!---->6?
</pre>
<blockquote type="cite">
<pre wrap="">- Steve N7HPR
</pre>
</blockquote>
<pre wrap=""><!---->
Steve-
The mounted inductance of a decoupling capacitor is comprised of several
partial inductances: the intrinsic inductance of the capacitor itself
(what the capacitor marketeers put in their databook), the vertical
inductance contributed by the vias, and the horizontal inductance
(spreading inductance of the planes).
In the grand scheme of things the intrinsic inductance is pretty small,
the vertical inductance is a smallish number too (unless you have a very
thick stackup where it then becomes significant), the spreading
inductance is a function of both the separation between the planes and
the mounting pads escape geometry.
So, yes you can minimize via inductance if you have a large hole in the
via (since the majority of the current will flow on the outer surface of
the 'pipe') however unless the stackup is pretty thick and stacked such
that you need to descend deeply into the stack then the via contribution
will be a relatively small part of the total inductance.
Another thing to consider is that if you have a large diameter via drill
you will also need larger diameter via pads and anti-pads. The larger
anti-pads will effectively 'swiss cheese' the associated planes if there
are a significant number of them and can increase the spreading
inductance by as much as a factor of 3-4 X (there ain't no free
lunch!). Large diameter vias also can't be put real close together so
you are limited in the ability to minimize the current loop size.
>From a practical standpoint, to minimize decap inductance I've found it
best to:
1) Keep the vias short (i.e. place planes near the surface of
The stackup)
2) Keep your mounting pad escapes close together and short
(broadside
escapes work well)
3) Use multiple escapes and vias per pad.
Regarding Table 6 in the Xilinx app note:
I think someone came up with those numbers empirically. I
wouldn't put much stock in them. There are several ways to determine how
many decaps you need. Rule-of-thumb tables aren't one of the preferred
methods.
See the following Designcon papers by Steve Weir and Scott McMorrow
(terraspeed Consulting) for a good treatment of decoupling capacitor
selection:
<a class="moz-txt-link-freetext"
href="http://www.teraspeed.com/papers/High%20Performance%20FPGA%20Bypass%20Fil">http://www.teraspeed.com/papers/High%20Performance%20FPGA%20Bypass%20Fil</a>
ter%20Networks%20Paper.pdf
<a class="moz-txt-link-freetext"
href="http://www.teraspeed.com/papers/capacitor_placement_public.pdf">http://www.teraspeed.com/papers/capacitor_placement_public.pdf</a>
They discuss via inductance calculations amongst other factors.
Also see the papers Istvan Novak (Sun Microsystems) has on his web site:
<a class="moz-txt-link-freetext"
href="http://home.att.net/%7Eistvan.novak/papers.html">http://home.att.net/~istvan.novak/papers.html</a>
-Ray WB6TPU
_______________________________________________
HPSDR Discussion List
To post msg: <a
class="moz-txt-link-abbreviated" href="mailto:hpsdr@hpsdr.org">hpsdr@hpsdr.org</a>
Subscription help: <a
class="moz-txt-link-freetext"
href="http://lists.hpsdr.org/listinfo.cgi/hpsdr-hpsdr.org">http://lists.hpsdr.org/listinfo.cgi/hpsdr-hpsdr.org</a>
HPSDR web page: <a
class="moz-txt-link-freetext" href="http://hpsdr.org">http://hpsdr.org</a>
Archives: <a
class="moz-txt-link-freetext"
href="http://lists.hpsdr.org/pipermail/hpsdr-hpsdr.org/">http://lists.hpsdr.org/pipermail/hpsdr-hpsdr.org/</a>
</pre>
</blockquote>
<br>
<pre class="moz-signature" cols="72">--
Ing. Jeroen Bastemeijer
Delft University of Technology
Department of Electrical Engineering
Electronic Instrumentation Laboratory
Mekelweg 4, Room 13.090
2628 CD Delft
The Netherlands
Phone: +31.15.27.86542
Fax: +31.15.27.85755
E-mail: <a
class="moz-txt-link-abbreviated"
href="mailto:J.Bastemeijer@EWI.TUDelft.nl">J.Bastemeijer@EWI.TUDelft.nl</a>
</pre>
</body>
</html>