Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I'm doing a bit of RF PCB design, and one of the things that caught my eye is the "Controlled Impedance" option. Checking more boxes always costs more, so I want to know if this is worth the extra money to ensure functionality on arrival. For the RF portion, I'm using 50 ohm microstrip-line on a 4 layer board. (Top layer [1] is signal, top inner layer [2] is a ground plane)

Most board vendors have made their laminate stack-up contents and thicknesses available on their website, and I have been able to calculate the width of the transmission line to my satisfaction using their numbers.

  • What is the benefit of using "controlled impedance" or "controlled dielectric"?
  • At small distances (about 1/10 wavelength), would the impedance bump matter? (I get about 2 ohms difference in Zo from changing the dielectric constant by +-0.4)
  • Is this something that should be done for production boards but isn't necessary for one-off prototypes?
  • Have you ever used this feature?
share|improve this question
1  
Your title is an "it depends" question. –  Brian Carlton May 6 '11 at 23:07
3  
I'll be sure to ask only yes/no questions in the future. –  W5VO May 7 '11 at 0:39
add comment

2 Answers

up vote 7 down vote accepted

If you specify controlled impedance/controlled dielectric, they will test your board to ensure that the traces are at the specified impedance. In your fabrication notes on your PCB printout, specify the nets and their targeted impedance (with tolerance, e.g., 50 ohms +/- 2 ohms).

They will either test a small test strip that is manufactured on the same panel as your boards; or they will test all nets as needed. This will help catch boards that do not meet spec, before they end up being stuffed with components.

BTW, the "weave" of the board may affect the actual impedance of any particular trace, even when the traces are built to spec (see http://www.altera.com/literature/an/an528.pdf).

share|improve this answer
    
The weave of the board can affect the impedance of a trace? That makes me cringe. –  Kevin Vermeer May 10 '11 at 16:06
    
@Kevin -- it's because FR-x materials are composites consisting of glass fibers (the F) and resin (the R). If you want consistent performance use a substrate that is more homogenous like a ceramic-filled resin (ex. Rogers). –  DrFriedParts Mar 25 '13 at 17:23
add comment

For a controlled dielectric board, they probably take more care in doing the stackup, as well as using better materials. I'm currently using controlled impedance boards, but have skipped it in the past at 1.8 GHz for Cell phones.

For short runs, you likely won't see much of an issue for an impedance bump. If you're going to do it in production, then you should prototype with it as well.

If you're doing small boards and short traces, then you probably can skip the controlled impedance and live with what you get. You may see some slightly higher trace insertion losses with an uncontrolled board, but that might not matter.

share|improve this answer
    
Dave - Thanks for the voice of experience! However, "they probably take more care" isn't very authoritative or specific. Can you point to some evidence of this? –  Kevin Vermeer May 10 '11 at 16:01
    
Also, the tagline is unnecessary - Your signature is already at the bottom right, with an avatar, information on your badges/rep, and a link to your profile. –  Kevin Vermeer May 10 '11 at 16:01
    
Here's an interesting link I came across freelists.org/post/si-list/Fr-4-Er-variation that should help with this. –  Dave May 12 '11 at 0:36
add comment

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.