Issue with impedance matching of differential pair

The guidance is a bit misleading.  You don't *require* 45 ohm single ended.  You do need 90 ohm differential.  The 90 ohm diff pair can be achieved with a tightly coupled pair on the top.  You could do CPWG as suggested by excelon or you can widen slightly and do just an edge-coupled microstrip pair.  

If you had a line which was 45 ohm single ended, and 90 ohm differential then that would suggest an uncoupled pair and those dimensions are not practical on a 2 layer board again as excelon has mentioned.

What tools were you using to check your impedance?  The calculator in Allegro/Orcad will get you the right values assuming your stackup has been entered correctly.

Okay!

Yes,I am using the calculator in Allegro/Orcad. I ma using same values but still not able to resolve the issue.

Thanks

The Allegro PCB calculator, I have found does not do coplanar wave guide impedance.  I believe you would need the sigrity tool, or go to the Ansys modelers.

Try this: https://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm

We have used this and it has been very accurate, verified measurements on a TDR.
Also the Saturn PCB toolkit comes up with similar results: saturnpcb.com/.../

Can you take a screenshot?  Make sure you have the BOTTOM layer marked as "PLANE" otherwise the trace calculator won't work -- but this also means that the the bottom is really ground in your design on the bottom (under the USB traces).  Also, soldermask over trace will pull the impedance slightly.  You can adjust that later -- let's get your calculator working

Cadence does not support the CPWG construction but it does support edge-coupled traces properly.  You really don't *need* CPWG for the USB application.  Lots of manufacturers out there are building 2 layer boards with USB that work great.

Make sure your settings look like mine.  You should get the same values.

I did the same but still having same problem.

I have one question. when I have created diff pair set in Electrical Constraints, in that I have declared the impedance of diff pair 90 ohms with 15% tolerance. 

Is that right thing to do ??

I did the same but still having same problem.

I have one question. when I have created diff pair set in Electrical Constraints, in that I have declared the impedance of diff pair 90 ohms with 15% tolerance. 

Is that right thing to do ??

Any chance you can post a zip of your board?  I also do as excellon says which means I use physical construction.  And, depending on how critical the impedance measurement needs to be I might have my fabricator do their own calculation to see what their final impedance value will be.  That's not really necessary for this design however.

I see that your "target" impedance is set to 90 and Cadence thinks it's 178(in the DRC).  That is telling me that Allegro is calculating with the wrong reference to the signal.

Red this is very curious. In 16.6 the stack up manager agrees fairly closely to the RF-Sim though it is off by 7 ohms or so. Not a big deal. By default that stackup manager assigns a dialectic constant to the conductor. Seems odd to do this but fudging that value of 4.5 to 8 brings the diff line impedance in line with the rf sim. Last I checked the dialectic constant of copper was infinity.

Plugging in a mask layer above reduces the impedance too.

Ignoring the CPWG for the moment and just going with std edge coupled lines  Cadence reports 103.34 Z for the diff pair using a trace width of 10Mil and space of 6mil.

When DRC reports your error is it reporting on the single line impedance or the actual calculated diff pair impedance ?. 178 divided by 2 = 89 which is very close to 90 ohms, assuming similar to what I have in the stackup.

I live more in the world of the physical than the CM for certain things but initially I got DRC errors too. My line impedance reported by the drc was based on the single line impedance. I had to plug in the single line impedance and not the actual required Diff-Pair impedance to make the drc go away. The DRC looks to report only single line impedance not the actual Diff-Pair as one would think if analysis mode is enabled for impedance.

Note the single line impedance matches the spreadsheet and all is good.

While I typically don't use the Stack up manager for impedance control for certain things it looks to me that while it can provide diff-pair info the DRC is all based on just the single line impedance only.

Maybe you can confirm that to be the case as a sanity check.

Thanks.

Hi excellon, I get the same results as you.  I was kind of hinting at the fact it was only single-ended based on the 90/180.  And now, from what I can see it appears that the impedance rule really only applies to the single-ended variant and CM does not understand a diff-pair impedance.

So...as you said earlier.  Stick with the physical rule definition... let's see if the OP has any more questions on that. 

Thank you Excellon and Redwire!

From all this what you have explained, I think that I have made mistake in setting the impedance of diff pair to 90 ohms in constraint manager.

In picture below, I have set the single-line impedance of the diff pair C-set to 90 ohms  in the electrical constraints. 

How much value should I set to the single-line impedance ?

Thanks Red.

The diff pair is kind of confusing in that the actual CM has no clue as to what it is because the CM lives in the world of single ended impedance only. It threw me for a loop too