# What does impedance control on a PCB mean [closed]

I understand that when the electrical length is less than 1/10 of the trace length I would have to go in for impedance matching. A PCB impedance is controlled by its stack up. THat is thickness of prepreg, copper etc. So when a factory says it does impedance control , does it mean that they do that kind of a stack up? What does it mean when a factory says they will not do impedance control? Is it that they cannot do that stackup? If so , sticking to a normal 4 layer board stack is sufficient? What is th main FR4 specification that determines the impedance? Because right now I have a boards which has a stack up for 4 layers with thickness of each layer. DO I have to send this stack up to every PCB house and ask if they do this? How do I build these boards?

## closed as too broad by Matt Young, PeterJ, Peter Smith, Daniel Grillo, Dave Tweed♦Mar 31 '16 at 13:14

Please edit the question to limit it to a specific problem with enough detail to identify an adequate answer. Avoid asking multiple distinct questions at once. See the How to Ask page for help clarifying this question. If this question can be reworded to fit the rules in the help center, please edit the question.

• Trace impedance is typically only considered for high speed signals. Does your circuit contain high speed signals? – Dan Laks Mar 31 '16 at 2:40
• USB and DDR signals, so yes high speed – red car Mar 31 '16 at 2:42
• Do you understand the basic concepts of impedance matching and high-speed signal routing? It's not clear from you question if you have experience here. But routing DDR signals would imply you do have experience. – Dan Laks Mar 31 '16 at 2:44
• Honestly, there are too many misconceptions and lack of understanding to answer this question reasonably. – Matt Young Mar 31 '16 at 4:11
• @derstrom8 - the question does not propose that trace length would control impedance, rather it proposes that trace length (relatively to an admittedly odd statement of wavelength) would determine if impedance matching is important. And that is correct. – Chris Stratton Apr 1 '16 at 3:47

I understand that when the electrical length is less than 1/10 of the trace length I would have to go in for impedance matching.

You have this backwards, the common rule is to use impedance control when the electrical length of the trace is more than 1/10 of a wavelength at the frequency of interest. (Like Rolf points out in his answer, the "frequency of interest" is more related to the rise and fall times of a digital signal than to the data rate)

So when a factory says it does impedance control , does it mean that they do that kind of a stack up?

It means they can control the thickness of the dielectric layer and the width of the trace with close enough tolerance to guarantee impedance matching to within some specified limits (often +/- 10%)

Also, like the other answer points out, they should have test equipment to allow them to verify the boards they produce.

What does it mean when a factory says they will not do impedance control?

It means they can't control the geometry closely enough to guarantee the impedance is within tolerance.

Is it that they cannot do that stackup?

No the stackup doesn't change, it's how well controlled the geometry is.

If so , sticking to a normal 4 layer board stack is sufficient?

No, you need to control the geometry well to be able to get the required impedance.

What is th main FR4 specification that determines the impedance?

Dielectric constant, often designated $\epsilon_r$ or $D_k$ is the critical material parameter.

The thickness of the dielectric is also critical.

Because right now I have a boards which has a stack up for 4 layers with thickness of each layer. DO I have to send this stack up to every PCB house and ask if they do this?

You just have to send it to one board shop that knows how to do impedance control, or 2 or 3 if you want to get competitive bids.

Many many board shops are capable of impedance control, including many of the modest-priced shops that advertise online. Only the most low-cost shops (and probably most of the hobbyist shops that charge by the square centimeter and combine your design with others) can't do it.

How do I build these boards?

Send the manufacturing files to a board shop with capabilities that match your requirements, and pay them to build them for you.

• Not 100% in agreement here, but liked the format. So I created a separate answer. – Rolf Ostergaard Mar 31 '16 at 9:22
• I would note that it is highly unlikely that any two PCB houses will specify the same stack and track rules for a given impedance. – Peter Smith Mar 31 '16 at 9:23
• This is a very good answer. I would like to add, however, that the manufacturer may suggest different stackups that are easier for them to manufacture, in which case you may need to change the geometry of your traces (the widths, primarily) to make sure the impedance is matched properly. I use the EEWeb calculator at work: eeweb.com/toolbox/microstrip-impedance . I generally aim for a trace width that gives me an impedance 10% higher than the target because surrounding traces will reduce the impedance of a particular trace. – DerStrom8 Mar 31 '16 at 11:56
• @PeterSmith, I guess that's true. I tend to work where I determine the stack up (down to the laminate product number, consulting with the board shop to see what they stock), and use a calculator to find a "close-enough" trace width. Then the board shop runs Polar to get a final trace width, usually within a half a thou of what my calculation gave. – The Photon Mar 31 '16 at 17:06
• No, the poster doesn't have it backwards. They are just using odd terminology - clearly the mentioned "electrical length" is the wavelength in a conductor. And the important question is if the trace length is more than a meaningful fraction of that, as correctly stated. – Chris Stratton Apr 1 '16 at 3:49

I understand that when the electrical length is less than 1/10 of the trace length I would have to go in for impedance matching.

Actually what you should look at is the risetime compared to the lenght of the traces. So if you have 200-300ps risetime and you have a 100-150ps long trace or shorter this may go fine without termination.

So when a factory says it does impedance control , does it mean that they do that kind of a stack up?

It most likely means they have a TDR to verify impedance of test traces after they build the board. Often from Polar Instruments

What does it mean when a factory says they will not do impedance control? It means they can't control the geometry closely enough to guarantee the impedance is within tolerance.

That this is a cheap shop that is not fit for building high speed boards.

If so , sticking to a normal 4 layer board stack is sufficient?

Depends on your definition of normal. Roughly speaking - and you will have to do the calculations - if you route on the two outer layers only you will need a prepreg thickness between the outer layers and your two inner layer power/gnd planes similar to the trace width. So for 6mil traces, about 6mil thick prepreg. Again: You will have to do the calculation - and it's easy to do with a free tool you can find on the net called TNT.

What is th main FR4 specification that determines the impedance?

Since the dielectric constant, often designated ϵr or Dk is almost the same for all material (around 4), the most important thing is the thickness.

Because right now I have a boards which has a stack up for 4 layers with thickness of each layer. DO I have to send this stack up to every PCB house and ask if they do this?

See the answer from "The Proton".

How do I build these boards?

See the answer from "The Proton".

Let me know if this helped, or you have further questions?

Also, strongly consider an 8L board (routing-gnd-pwr-routing-(fat core)-routing-pwr-gnd-routing) as it's much easier to route AND get the power distribution (PDN) right. Without good PDN you quickly run into trouble getting the thing to run fast reliably.

Disclaimer: I teach courses in SI and often have Polar Instruments as a sponsor - but I do not receive any kickback.

• Regarding TNT, are you referring to this software? – dionys Mar 31 '16 at 8:50
• I think TNT is technically speaking the graphical front-end for MMTL :) @dionys – Rolf Ostergaard Mar 31 '16 at 11:05