[SI-LIST] Re: RF Layout - Via spacing
- From: arvind yadav <arvind.yad1983@xxxxxxxxx>
- To: wolfgang.maichen@xxxxxxxxxxxx
- Date: Thu, 22 Oct 2009 23:12:06 +0530
Thanks for the help wolfgang .
On Thu, Oct 22, 2009 at 10:59 PM, <wolfgang.maichen@xxxxxxxxxxxx> wrote:
>
> Hello Arvind,
>
> ok, that's different. What you describe is a transmission line structure
> called "coplanar waveguide with ground". This is a signal line with ground
> planes on either side (that would constitute the coplanar waveguide) plus a
> ground plane underneath. It's basically a mixture between a coplanar
> waveguide and a microstrip line.
>
> In order for the two ground strips on either side to be truly ground, it is
> important that they be closely tied to the actual ground plane (better:
> "reference plane") underneath. If you forgot to do that the ground strips
> would just act as two additional transmission lines (with a line impedance
> significantly larger than zero) coupled to the center line, but not a ground
> references (with impedance ideally = zero). So in a simple picture your line
> impedance would be higher than you would expect. Second, current entering
> into them would have no way of redistributing itself into the ground plane
> underneath, resulting in additional distortion. If your total line length
> approaches lambda/4 or more you would see resonance effects in those
> "ground" strips - you'd basically have a coupler with unterminated outputs.
> With vias spaced to far apart the same applies but not as severe.
>
> Any transmission line calculator (or 2D field solver) assumes that you tie
> every structure denotes as grounf very closely to ground. Only then your
> actual transmission line impedance will match the one you calculate.
>
> In order for a structure to act as ground the ground return path must be
> short against the shorest wavelength of interest (approximately given by the
> frequency 0.33/rise_time, i.e. by your rise time and NOT by e.g. you clock
> frequency or data rate). lambda/20 is quite conservative in that respect and
> in practice you will be able to get away with wider spacing (somewhere
> between lambda/4 and lambda/10). Also note that the vias add additional
> metal close to the signal trace which will lower your inductance compared to
> what your 2D solver will predict. To be safe, keep the vias at sufficient
> distance from the trace - about 3 trace widths would be the minimum - or
> even better, use a 2.5D or 3D field solver to simulate the actual structure
> including the vias.
>
> Wolfgang
>
>
>
>
>
> *arvind yadav <arvind.yad1983@xxxxxxxxx>*
>
> 10/22/2009 10:12 AM
> To
> wolfgang.maichen@xxxxxxxxxxxx, si-list@xxxxxxxxxxxxx cc
> Subject
> Re: [SI-LIST] RF Layout - Via spacing
>
>
>
>
> Hello Wolfgang ,
>
> Thanks for the reply .
>
> In my case i dont have a signal via . What i have is a RF signal in top
> layer and around that two strips of ground traces .
>
> In that GND track we have placed vias and some guidelines says to
> maintain lambda/20 rule between the two same gnd vias .
>
> Can you please explain this .
>
> Thanks
> Arvind.H
>
> On Thu, Oct 22, 2009 at 10:34 PM,
> <*wolfgang.maichen@xxxxxxxxxxxx*<wolfgang.maichen@xxxxxxxxxxxx>>
> wrote:
>
> Hello Arvind,
>
> the goal in designing a clean (reflection-free) signal path is to have
> homogeneous characteristic impedance all along the path (typically ZoP Ohm
> unless you are working with TV signals that use 75 Ohms).
>
> The characteristic impedance is determined by the ratio of inductance Lu
> per unit length and capacitance Cu per unit length:
>
> Zo=sqrt(Lu/Cu)
>
> A signal via and its closest return via (or vias) are just part of that
> path. Changing the distance d between signal and return via changes both
> capacitance C and inductance of that via structure (C decreases with d, and
> L increases with D), so you can use that to tune the impedance of the via
> structure. Ideally you'll achieve 50 Ohms although this is hard to do with
> just a single return via. In that ideal case (ZoP Ohms) the via structure
> becomes completely transparent to the signal, i.e. it only causes delay
> (delta_t = sqrt(C x L)) but no reflections.
>
> Designing a well-matched via structure is a challenge and typically need
> either a good 3D simulation tool or a few test boards to get it right at
> high data rates. Rules of thumb ar hardly sufficient although they can
> provide at least a goot starting point as well as show the "knobs" you can
> use to adjust the impedance (for via structure, there a are many knobs - via
> diameter and distance, stub or stub drilling, pad/antipad diamaters, and so
> on).
>
> The lambda/20 rule you mention comes from the fact that typically
> structures that are very short against the shorted wavelength (highest
> frequency) of interest only have negligible influence on the waveform, i.e.
> produce only minimal reflections even when they are mismatched (Zo <> 50
> Ohms). This is of course just a crude rule of thumb.
>
> Whatthe lambda/20 rule achieves very nicely is that it forces you to place
> a return via close to every signal via. This is important - current is
> always flowing in a loop so if there is no return via close by, the return
> current has to "go looking" for the nearest return path which may be quite a
> detour - this will cause a large parasitic inductance in the path (because
> the current now encloses a large loop are) and resulting large reflection
> and reduced bandwidth.
>
> Wolfgang
>
>
>
>
>
> *arvind yadav <**arvind.yad1983@xxxxxxxxx* <arvind.yad1983@xxxxxxxxx>*>*
> Sent by: *si-list-bounce@xxxxxxxxxxxxx* <si-list-bounce@xxxxxxxxxxxxx>
>
> 10/22/2009 09:45 AM
>
> To
> *si-list@xxxxxxxxxxxxx* <si-list@xxxxxxxxxxxxx> cc
> Subject
> [SI-LIST] RF Layout - Via spacing
>
>
>
>
>
>
> Hello All,
> I am working on a RF Layout. I looked into some design guidelines and had
> some doubt on gnd via spacing requirement .
>
> Guideline said that ë/20 distance has to be maintained between gnd vias
> that
> are stitched on either side of the RF signal
>
> Can any one please let me know the reason for this requirement ?
>
> I also would like to know what would be the gnd backoff distance from the
> RF signal and the reason .
>
> Thanks
>
> Arvind.H
>
>
> ------------------------------------------------------------------
> To unsubscribe from si-list:*
> **si-list-request@xxxxxxxxxxxxx* <si-list-request@xxxxxxxxxxxxx> with
> 'unsubscribe' in the Subject field
>
> or to administer your membership from a web page, go to:*
> **//www.freelists.org/webpage/si-list*<//www.freelists.org/webpage/si-list>
>
> For help:*
> **si-list-request@xxxxxxxxxxxxx* <si-list-request@xxxxxxxxxxxxx> with
> 'help' in the Subject field
>
>
> List technical documents are available at:
> *http://www.si-list.net* <http://www.si-list.net/>
>
> List archives are viewable at:
> *
> //www.freelists.org/archives/si-list*<//www.freelists.org/archives/si-list>
> or at our remote archives:
> *
> http://groups.yahoo.com/group/si-list/messages*<http://groups.yahoo.com/group/si-list/messages>
> Old (prior to June 6, 2001) list archives are viewable at:
>
> *http://www.qsl.net/wb6tpu*<http://www.qsl.net/wb6tpu>
>
>
>
>
>
------------------------------------------------------------------
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:
//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:
//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
Other related posts:
