PCB layout with diff pairs

In my opinion, the "high end" packages barely handle differential pairs. All PCB software I've used (and I've used a lot) are all abominable hunkering piles of festering garbage. Either made by people who have no idea what is really required for efficient work, or by monstrous corporations with better salesmen than programmers.

Anyways, can you grab two traces at a time and route them in your PCB software? There's nothing magic about "impedance controlled" lines, you have to enter spacing and width rules and where to apply them. The software does nothing more than enforce the rules. Some software comes with field solvers etc, but this is often useless as the trace info eventually comes from the PCB shop, who often ends up tweaking your layout to match their process.

The real work is done at the PCB shop who has to

1) Supply you with rules for their process for them to give you the impedance 2) Has to know their process to give you the impedance

Anyways, one trick I've used in the past is to route the pair as one fat trace with an thinner anti-etch routed over the same coords. It ends up as a perfect diff pair, but without DRC enforcement.

Just do it. Decide on a dielectric and pcb stack, run a program like Txline to get a suitable trace width and spacing, and plunk down the traces.

John

Yep, I'll second that. It's like driving a stick-shift car, it can be done :-)

--
Regards, Joerg (who drives a stick-shift car)

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

I'll third that. Differential runs are pretty trivial to do by hand. You need to talk to your board house about stackup dimensions. Your board house can usually recommend trace parameters if you don't have the ability to do calculate. Polar Instruments seems to be a popular program with the board houses.

--
Mark, who drives a stick shift

,

t try

Pulsonix does them automatically, and isn't too expensive:

Leon

Also, look at the price list and then back off 2mils or so from the pitch/width margin where pricing begins to hurt. My layouter is great but he usually starts out with really small defaults. So we always have a brief discussion at the outset about trace width, sometimes followed by a few minutes of politics ;-)

Good!

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

But keep in mind FR4 (the material most PCBs are made of) has tolerances a well so don't expect to get the exact impedance.

--
Failure does not prove something is impossible, failure simply
indicates you are not using the right tools...
                     "If it doesn\'t fit, use a bigger hammer!"
--------------------------------------------------------------

,

t try

As everybody else has told you, work out the dielectric thicknes between your tracks and the ground plane, find out the dielectric constant of the material, work out the track width to get the impedance you want, and lay out the two tracks to run parallel with each other.

Try and avoid vias.

The only time this approach didn't work for me was when the printed circuit board department ignored my carefully specified layer build-up and substituted their own, so that what should have been controlled impedance tracks running directly above a buried ground plane were routed over a power plane several layers further into the board.

It took several weeks for us to realise what they had done - the engineer working on the board had printed out the various layers and stapled them together, and it every time I saw him I'd remark that he'd got the layers in the wrong order, and it took a while before he got around to checking what I was telling him. The board didn't work until we replaced all the critical tracks with lengths of minature coax.

It was a very expensive board, but the loss of development time was a lot more expensive still.

-- Bill Sloman, Nijmegen

Check out this blurb by the notorious Dr. Howard Johnson (aka HoJo).

Bob

--
== All google group posts are automatically deleted due to spam ==

HoJo likes to make up numbers, like the 99.9% thing. And he still has that strange return current fixation.

John

I agree that his statement is confusing about the return current's longer path causing additional delay. It obviously results in a change in characteristic impedance on that trace, but delay? I dunno.

One thing he said that is interesting is regarding the driving of a tightly-couple twisted pair single endedly and seeing a resulting differential signal at the far end. I had to think about this, but it seems to make sense if you look at it from a reverse point of view in that any common-mode component headed in the direction of the grounded lead would result in an upside-down reflection on that lead. I may just try this and see if any fruit sprouts. What do you think?

Bob

--
== All google group posts are automatically deleted due to spam ==

I can't see any change in impedance either. Isn't the system physically symmetric? Do the electrons remember the power and ground connections of the chip that launched them?

HoJo fixates on bypass capacitors and ignores plane-plane capacitance. Look at the size of the traces, then look at the size of the planes.

I think that a twisted pair has some differential behavior and some independent propagation behavior, and the ratio depends on the relative dielectric constants of plastic and air, and that 1000:1 is a silly number.

You can launch a single-ended signal into a twisted pair and see it as differential on the other end, at least the fast parts. It's more wideband if you pass it through a ferrite core or two.

You can also invert a pulse with just coax:

==================================== in-------------------------------------============================== ====================================-------------------------------out | ============================== gnd | gnd

John

Yes. If you need more exact performance you'd had to go to other material such as Rogers.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

PC,

try

I can usually hit trace impedances to within about 10%, using regular "FR4" callouts and just giving the stackup, without the board house knowing that I'm trying to control impedances. That's good enough for most purposes.

Very few "50 ohm" devices are. Most mmics have input impedances closer to 30.

John

PC,

try

Same here. In the olden days it was even done on phenolic. Still got some examples in the garage. Microstrip baluns and that sort of thing.

Another reason why I prefer discrete solutions :-)

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

Doesn't current have a 90-day return policy?

--
SCNR, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

In article , snipped-for-privacy@highNOTlandTHIStechnologyPART.com says...>

PC,

try

A lot of higher end ASICs and memory devices have active controls on output impedances. Having said that, 10% is usually good enough for even those devices.

I think you're confusing that with the audiophile version of Kirchhoff's current law:

?I=0 ±3dB

Bob

--
== All google group posts are automatically deleted due to spam ==

So where are the price tags?