9 Replies Latest reply on Jun 6, 2013 7:24 AM by veronika.anisoveca

differential trace impedance calculation

Hello!

I am confused about the correct PCB stack-up for 100 Ohm differential trace impedance.

Can you describe me the basic rules for this and advise relevant links?

For example, I have differential stripline signals, which should be 100 Ohm impedance.

Dielectric thickness may vary, but at the moment I have 4mils.

Trace thickness is 0.6mils.

So I need to choose the correct trace width/spacing, am I right?

Previously I was used 5mils width and 6mils spacing differential traces.

But when I put all these values to some calculator it gives me only 72 Ohm of differential impedance.

What could be wrong and what should I change in my values in order to have about 100 Ohm impedance?

Should I trust to such kind of calculators?

Veronika

• 1. Re: differential trace impedance calculation

Hello Veronica,

Before I can answer you question, lets go a little bit in the the theory.

A signal travels along the trace and is influenced by the path it is traveling (the trace) and the neighborhood that influences the path (the stackup, the material, other traces or planes, etc)

To describe what a signal "sees", one practical value is the impedance. If the signal travels together with another they build a differential pair and we speak of a differential impedance.

So the impedance is dependent

1) on the material characteristics (the trace material (copper, aluminum, other metals), the prepreg above or below, the core material above or below, the air above or.... etc...) and

2) on the geometries (trace width, height, distance to the next plane, distance to the other trace(for differential pairs) and distance from other traces, etc...)

The stackup defines the most important parameters of the geometries: the trace height, the distance to planes and traces. And also it defines the material characteristics. A prepreg has a different characteristic than a core.

So the first step to calculate a normal or diff. impedance is to know how is the stackup build and what material is you board made of. Ask the manufacturer to give you the detailed stackup with measures and the material parameters that are used for the calculations. They are typically the dielectric constant  and the tangent loss. They vary for different thickness of the material.

The seconds step is to use any tool to calculate the needed trace widths and insulations. You can trust most of today's impedance calculators if you give in all the right values.

Remember that usually at the end you will want to do a small rounding. IF for example the calculator tells you to have a trace of 3.87548234mils, you can simplify it to 3.9mils. If you do the reverse calculation you will see that the error is small. And remember that etching can not be so precise either, so you usually accept a tolerance of about 10%. IF you need better then make special arrangements with your board producer.

The third step is to use this in your design.

Remember that if the signal changes layer then the parameter will change. You have to calculate the trace and space for every layer that you use in the design.

In you example you said that you used to use 5mils width and 6mils spacing differential traces for your design. What you didn't tell was what is your stackup, what is the material used, what is the layer on which this trace and space is valid, and so on. The same trace and space with the same stackup but with different material will have different impedances.

I hope this will clarify some. IF you have more questions feel free to ask and to read some other books or take some classes on this.

Welcome in the world of signal integrity.

Bye

Matija

• 2. Re: differential trace impedance calculation

Thank you very much!

But the problem is that after I finish the PCB another person will look for some manufacturer. So I cannot ask them now about the materials...

I need to calculate trace geometry according to my stack-up and some assumptions. After that manufacturer will choose the correct materials in order to make the required values of impedance.

• 3. Re: differential trace impedance calculation

For general FR-4 material, The Dk value be 4.1~4.4, varied on different Core/PP type and the resin content. You can use 4.3 as an average value. Important thing is that you should carefully select Core/PP thickness while arranging the stackup. Also it's better to get 2-4 ohm lower than 100 ohm target  in Hyperlynx solver (considering etch factor).

Hyperlynx is an excellent tool, it support you do sweep on width/space,so you can design a good stackup, width/space which fabs only slightly modify it(within 5%). Mentor Supportnet have good technotes and white paper about this topic.

Yanfeng

• 4. Re: differential trace impedance calculation

Attached is an example stackup for 26L backplane using Megtron-6(7mil Z0=52 ohm 7mil/9mil Zdiff=94 ohm), it's ready to fab.

Yanfeng

• 5. Re: differential trace impedance calculation

how can I open this file? What program should I use?

• 6. Re: differential trace impedance calculation

If you have Hypelrynx Linesim, you can import this file by clicking menu stackup -> import.

Yanfeng

• 7. Re: differential trace impedance calculation

Ok, thank you. Tomorrow I will ask for trial license for Hyperlynx, so I could have a look on your file tomorrow!

• 8. Re: differential trace impedance calculation

Hello Veronika,

We had this discussion years ago in our company too. It turns out there is a learning in all people involved, that will lead to a change in the way you order PCB.

First of all, you have to educate all the people involved with the PCB. Start with the responsible in procurement, explain that from now on, a PCB is not "something you just order", but it has some "new" properties that they have to take care of. You will have to follow the life of the product too.

Second you have to make sure that you step in contact with the board manufacturer. Ask if they have experience in controlled impedance design and accept their suggestions. This means that from now on the first question when you start a new design will be: "Who will produce the board and with what kind of material?". You will have to work out the material, the stackup, and all the design rules (trace-space,etc..). Remember that there will be always a material-stackup connection. Keep prices in check by using the most common material that still allows for your impedance requirements.

Third is the most important: put a clear documentation on the materail used for calculation and make this visible to the procurement people.

They will have to get used to the fact that a board can be only build with a material that is approved by you and/or the design engineer.

We put an additional text file in the Gerber disk, that looks similar to this:

Stackup:

Material: Panasonic: 1766M

Dielectric constant and Tangent loss for 1GHz:

FR4 Core
Name        Thickness        Dk           Df
R-1766M     200um            4,75         0,017

Prepreg
Name      Thickness +/-10%   Dk           Df

R-1661M    73um  1080/62%    4,4          0,022
R-1661M   191um  7628/44%    4,77         0,016

Multi-Layer structure:

thickness   Layer Film           usage

12µ  ^^^^^      AS-010         solder resist
18µ  -----      plating
35µ  -----  1   AT-010         power
73µ  .....      Prepreg 1080
191µ  .....      Prepreg 7628
18µ  -----  2   A2-FCE-010     signal
200µ  \\\\\      Core
18µ  -----  3   A3-010         signal
73µ  .....      Prepreg 1080
191µ  .....      Prepreg 7628
35µ  -----  4   A4-010         power
200µ  /////      Core
35µ  -----  5   A5-010         power
191µ  .....      Prepreg 7628
73µ  .....      Prepreg 1080
18µ  -----  6   A6-010         signal
200µ  \\\\\      Core
18µ  -----  7   A7-010         signal
191µ  .....      Prepreg 7628
73µ  .....      Prepreg 1080
35µ  -----  8   AB-010         power
18µ  -----      plating
12µ  ^^^^^      AR-010         solder resist

----------------------------------------------------------

Controlled impedance list:

Material: Panasonic R-1755M

Net_Type: Diff_Pair_100Ohm

Layer  Target  Trace  Space  Calculated

1      100     120    200    99,9 not used

2      100     150    190    99,3
3      100     150    190    99,3
4      100     120    200    99,9 not used
5      100     120    200    99,9 not used
6      100     150    190    99,3
7      100     150    190    99,3

8      100     120    200    99,9 not used

Net_Type: Diff_Pair_130Ohm

Layer  Target  Trace  Space  Calculated

1      130     100    400    123,7 not used

2      130     100    340    128,4
3      130     100    340    128,4
4      130     100    400    123,7 not used
5      130     100    400    123,7 not used
6      130     100    340    128,4
7      130     100    340    128,4

8      130     100    400    123,7 not used

Make sure that the board manufacturer sees, reads and understands this file. Als them if the information given is good enough for them to produce impedance controlled boards. Ask them if they can keep up with this specifications. Check on what is the expected tollerance of the finished board.

Fourth is to be prepared to talk to the board manufacturer if they do not have the same material that you have.

We usually ask the board manufacturer to give us a new stackup and a new calculation of the impedance. They will do it for you. Since the board is already routed and you can not change trace-space of the signals, you can play around with different thicknesses and other materials. There will be small differences in the calculations. It is now you task to make sure that those differences will not change the behavior of the board. If a design engineer is involved in the design you have to talk with him and clarify what this changes in impedance mean to the overall functioning of the boards. Many times it will be unimportant.

Some manufacturer will even change the trace-space on the manufacturing Gerber to comply with your requirement. Here be careful that both understand which traces get changed and which not. This will usually take some e-mail going back and forth between you and the board producer, but keep procurement informed when you reach a technical agreement, as they usually need to know this so that the delivery time starts form that moment on.

On additional step (for advanced impedance control and traceability) is how much do you trust your board manufacturer. Do you assume that the board will be right because the manufacturer will follow your design? This is usual.

Or do you want to have proof that the impedances are (tightly) met? In this case you may choose to ask them to report and/or send you along the board also the test coupons of the manufacturing panel. Or you may choose to add some test and measurement structure on the board or on the break-away tab to test that the manufacturer really met the impedance. And if you are really paranoid make the measurement yourself instead of relaying on the manufacturing measurement report.

The last step is to update the documentation in the section of allowed material and stackup. The new documentation must reach procurement, so they will now have an other option to ask for quotes.

Also don't forget to instruct the quality control people to check that the board was really made with the ordered material and has the right stackup. This means confronting the manufacturer report with your documentation. Your organization will have to make sure the QA people get the Gerber documentation too.

And as before, if you are paranoid make a microsection of the board and measure yourself the distances in the stackup.

Be patient on the first few boards that you order with this method, as this is a big change for your organization. But at the end it will be worth it.

Hope this helps

Matija