Impedance of complanar traces on PCB surface?
in [Design]
|
From: Andy on 8 Feb 2005 12:27 Don Pearce wrote: > On Tue, 08 Feb 2005 07:49:25 -0800, Chris Carlen > <crcarle(a)BOGUS.sandia.gov> wrote: > > >>>This is quite normal as there is usually a ground plane somewhere >>>about - if just the screening box. Make the calculation with the >>>ground plane at an appropriate distance for this, and all should be >>>well. >> >>But some formulas, being approximate models that fit fairly well over a >>limited geometrical domain, might deviate too much from meaningful >>results when taken far from their intended domain of usefulness. >> >>Might it be better to find expressions for the transmission line >>parameters based solely on the adjacent rectangular cross section >>conductors that the OP is working with, considering no ground plane? >> > > > As I remember it, a distant ground plane was not one of the limit > conditions that gave rise to large errors. Areas of importance are > close traces, and finite thicknesses of traces. Thank you. I will try the formulas that are given for PCBs with the ground plane. But how about the presence of two different materials - the FR4 and the air? -- Andy > He could always do a finite element analysis based on Laplace's > equation. Most CAD packages offer some sort of field evaluator that > works that way. Mostly they are a bit clunky, and you need to > calculate odd and even modes separately, but they do give the right > answers. > > d > > Pearce Consulting > http://www.pearce.uk.com
From: Don Pearce on 8 Feb 2005 12:36 On Tue, 08 Feb 2005 18:27:57 +0100, Andy <andy(a)nodomain.nod> wrote: > > >Don Pearce wrote: >> On Tue, 08 Feb 2005 07:49:25 -0800, Chris Carlen >> <crcarle(a)BOGUS.sandia.gov> wrote: >> >> >>>>This is quite normal as there is usually a ground plane somewhere >>>>about - if just the screening box. Make the calculation with the >>>>ground plane at an appropriate distance for this, and all should be >>>>well. >>> >>>But some formulas, being approximate models that fit fairly well over a >>>limited geometrical domain, might deviate too much from meaningful >>>results when taken far from their intended domain of usefulness. >>> >>>Might it be better to find expressions for the transmission line >>>parameters based solely on the adjacent rectangular cross section >>>conductors that the OP is working with, considering no ground plane? >>> >> >> >> As I remember it, a distant ground plane was not one of the limit >> conditions that gave rise to large errors. Areas of importance are >> close traces, and finite thicknesses of traces. > >Thank you. I will try the formulas that are given for PCBs with the >ground plane. But how about the presence of two different materials - >the FR4 and the air? > Provided the FR4 is really thin, you can almost ignore it. Performance is better that way too, as you work in true TEM mode, rather than the quasi TEM that happens if odd and even mode velocities are not the same. Most CAD packages will treat mixed mode dielectrics in some reasonable fashion, though. d Pearce Consulting http://www.pearce.uk.com
From: John Larkin on 8 Feb 2005 13:14 On Tue, 08 Feb 2005 08:48:33 +0100, Andy <andy(a)nodomain.nod> wrote: >Hello: > >I want to lay out a couple of traces on the FR4 PCB, to provide a >transmission line of specific impedance for a differential-mode signal. > >The impedance calculation formulas that I have found so far, for the >common-mode and differential impedance, concern the traces with the >ground plane underneath. I think I don't want the ground plane >underneath, to minimise the common-mode capacitance, and I am looking >for the formula for the coplanar traces on one side of the PCB, with no >metal (copper) in the other PCB layers in the vicinity of the trace. > >Can somebody help? > >Thank you. > >-- Andy Do you have a specific reason to minimize the even-mode capacitance? In the case of a typical geometry, deleting the bottom ground plane won't make a lot of difference, unless the board is thin. To reduce the even-mode capacitance and keep your target differential impedance, you could just make the traces skinnier and closer together. John
From: Andy on 8 Feb 2005 14:00 John Larkin wrote: > On Tue, 08 Feb 2005 08:48:33 +0100, Andy <andy(a)nodomain.nod> wrote: > > >>Hello: >> >>I want to lay out a couple of traces on the FR4 PCB, to provide a >>transmission line of specific impedance for a differential-mode signal. >> >>The impedance calculation formulas that I have found so far, for the >>common-mode and differential impedance, concern the traces with the >>ground plane underneath. I think I don't want the ground plane >>underneath, to minimise the common-mode capacitance, and I am looking >>for the formula for the coplanar traces on one side of the PCB, with no >>metal (copper) in the other PCB layers in the vicinity of the trace. >> >>Can somebody help? >> >>Thank you. >> >>-- Andy > > > Do you have a specific reason to minimize the even-mode capacitance? The signal source is a differential current source, with each output loaded with a resistance (R) connected to a common DC reference point. I wanted this combined source see mostly the differential load, with the impedance Z=2R. A microstrip with a ground plane would present the differential mode impedance significantly different from two times the common mode one, unles one distances the strips by several millimeters - which is not practical in my case. A possibility there is to try to match the source to the microstrip impedance, by attaching a resistance between the differential outputs, but I don't like that much as I don't know what effect this would have on the accuracy of the signal. > In the case of a typical geometry, deleting the bottom ground plane > won't make a lot of difference, unless the board is thin. > To reduce the even-mode capacitance and keep your target differential > impedance, you could just make the traces skinnier and closer > together. > I will study this. But the first try is not promising: with 0.2 mm-wide, 0.2mm-spaced traces with the ground 1.6mm away across the FR4, the common Z is about 136Ohm, and the differential - 154 ; I need 124 Ohm differential one. Thanks. -- Andy > John > > >
From: John Larkin on 8 Feb 2005 15:55
On Tue, 08 Feb 2005 20:00:11 +0100, Andy <andy(a)nodomain.nod> wrote: >John Larkin wrote: > >> On Tue, 08 Feb 2005 08:48:33 +0100, Andy <andy(a)nodomain.nod> wrote: >> >> >>>Hello: >>> >>>I want to lay out a couple of traces on the FR4 PCB, to provide a >>>transmission line of specific impedance for a differential-mode signal. >>> >>>The impedance calculation formulas that I have found so far, for the >>>common-mode and differential impedance, concern the traces with the >>>ground plane underneath. I think I don't want the ground plane >>>underneath, to minimise the common-mode capacitance, and I am looking >>>for the formula for the coplanar traces on one side of the PCB, with no >>>metal (copper) in the other PCB layers in the vicinity of the trace. >>> >>>Can somebody help? >>> >>>Thank you. >>> >>>-- Andy >> >> >> Do you have a specific reason to minimize the even-mode capacitance? > >The signal source is a differential current source, with each output >loaded with a resistance (R) connected to a common DC reference point. I >wanted this combined source see mostly the differential load, with the >impedance Z=2R. A microstrip with a ground plane would present the >differential mode impedance significantly different from two times the >common mode one, unles one distances the strips by several millimeters - >which is not practical in my case. A possibility there is to try to >match the source to the microstrip impedance, by attaching a resistance >between the differential outputs, but I don't like that much as I don't >know what effect this would have on the accuracy of the signal. > > >> In the case of a typical geometry, deleting the bottom ground plane >> won't make a lot of difference, unless the board is thin. >> To reduce the even-mode capacitance and keep your target differential >> impedance, you could just make the traces skinnier and closer >> together. >> >I will study this. But the first try is not promising: with 0.2 mm-wide, > 0.2mm-spaced traces with the ground 1.6mm away across the FR4, the >common Z is about 136Ohm, and the differential - 154 ; I need 124 Ohm >differential one. > >Thanks. > >-- Andy > >> John >> Cranking up Txline, it recommends 0.32 mm trace widths to get 124 diff z (62 odd mode impedance), with an opposite ground plane and your other dims. Even mode impedance is 203 ohms. I doubt that eliminating the ground plane would change these numbers a lot. John |