I am a bit confused with the implementation of a microstrip line to an u.FL connector. In order to maintain a 50Ohm line, the trace width would need to be ~0.1 inches wide, I have a pi matching network for 'just in case' implemented in line with the u.FL connector. Where I get confused is how would you do microstrip to something like a 0402 package resistor? Is this where co-planar wave guides perform better because they match up to component packages better? I would have to image a lot of reflection would occur hitting a component so much smaller then the trace width?

Also I have wondered this for a long time, and never found a good answer. For a very short run in terms of wave length, such as 1% the wavelength, is trace impedance control needed? My evidence for this though is the following: $$ Z_\mathrm{in} (\ell)=Z_0 \frac{Z_L + jZ_0\tan(\beta \ell)}{Z_0 + jZ_L\tan(\beta \ell)} $$

For a short wavelength say 1/100 \$\lambda\$, the equation becomes for following: $$ Z_\mathrm{in} (\ell)=Z_0 \frac{Z_L}{Z_0} $$

My antenna to be plugged into the connector is 50Ohm, so I believe that would be the load? or would \$Z_l\$ actually be the trace impedance?

The reason I ask is that I am basically running from a GSM modem to a u.FL connector, and It would be very easy to run a trace with ~100ohm impedance (using co-planar wave guide) instead of a huge wide 0.1 in trace for micro-strip.

update: Since it was asked, my frequencies of interest are L1 GPS (1.575GHz) and GSM spectrum (800-2100MHz).

  • 3
    \$\begingroup\$ 1. Use a thinner board, or a multilayer board to get a narrower microstrip. 2. Use bigger components like 0805 or 2012. \$\endgroup\$
    – The Photon
    Commented Nov 23, 2015 at 6:15
  • \$\begingroup\$ What frequency are you using? \$\endgroup\$
    – Andy aka
    Commented Nov 23, 2015 at 8:59
  • \$\begingroup\$ You can use two components in parallel if you're worried about package parasitics of a larger component. But I would make the dielectric height smaller, as @ThePhoton recommends. A 100 mil trace seems like you're using a 62 mil board? A 15 mil board (or 15 mil gap between layer 1 and 2, which would be your reference plane) lets you use something more like a 20 mil trace. \$\endgroup\$
    – scld
    Commented Nov 23, 2015 at 14:24
  • \$\begingroup\$ I was looking at useing 63mil board, but I'm thinking maybe I really should shift to a much smaller board thickness... And the larger components should still be OK, if not the purpose of them being there is to match the impedances... So I can tweak them. \$\endgroup\$
    – MadHatter
    Commented Nov 23, 2015 at 14:26
  • 2
    \$\begingroup\$ It is true that for very short (relative to wavelength) runs, impedance doesn't matter as much, but I would still try to match it somehow. I agree that 100 mil trace width is kind of ridiculous. Also, regarding the component size/trace width issue, it would be best to avoid large size differences, but when the necked-down area is much shorter than a wavelength, it will cause minimal reflection. There is a relationship between resolving power of reflected EM waves and wavelength. Objects much smaller than a wavelength do not cause a strong reflection. \$\endgroup\$
    – user57037
    Commented Nov 23, 2015 at 16:27

2 Answers 2


Generally, your assumptions are correct. When connecting a microstrip to a component, how closely you are able to match the physical size and shape of that microtrip plays the biggest role. Package size, termination style, and trim method for a series resistor are what matters.

Your other assumption that you can pretty much ignore transmission line effects for short runs is also correct. Often you'll see 1/4th of a wavelength used as the line between a 'short' transmission line (too short to matter) or 'long' (matters) in regards to the signal propagating through it, but I wouldn't suggest that as a rule of thumb. 1/10th the wavelength and below is where even phase delay becomes inconsequential and you can sigh with relief - you can just ignore transmission line theory completely and you probably won't go to engineer hell or otherwise be a bad engineer for doing so.

An easier way to think about this is with light. @mkeith gets credit for his comment where he mentions 'resolving' stuff. Take a lesson from optical microscopes: they can resolve smaller details if you use violet light, but there is just a limit where everything is too small to be resolved, and that's because it's too small relative to the wavelength to interact with the wave in a meaningful way. This applies to discontinuities for the most part - if its much smaller than the wave, then the wave isn't going to care.

Note: below, I am going to give more general tips on microstripping, but it will apply more or less depending on the wavelength at hand.

Now, back to the first part part, my recommendation on how to connect a 50Ω characteristic microstrip to an 0402 is simply not to. There are two things you have to think about whenever you must cause a discontinuity, reflection and parasitics.

Reflection is easy - keep the instantaneous (characteristic) impedance of a transmission line as close to the same for every step a wave propagating down it has to take, and make sure the other end is terminated with a matched load impedance, and all is well. And the moment you have to put any component in series, that happy dream is screwed. When connecting and layout this stuff, its best to view it in terms of damage control.

If your microstrip narrows, that will cause a potentially large impedance discontinuity. If your microstrip is 0.1" wide, you never want to do anything that will cause it to narrow or widen, except when you're mitering a corner of course. This means you really really should use an SMD package whose terminals are the same width as your microstrip (or combine parallel packages to simulate this), and one that has a high aspect ratio in the direction of the strip. And also as thin as possible. Basically, you want this thing to seem as if it is just another length of copper microstrip as you can manage. Obviously, a 1210 sized package would be perfect for a 0.1" wide microstrip. It's the same width, and it's aspect ratio is what you want too.

Anyway, the goal is always to minimize all the ways you might be introducing any sort of discontinuity in the characteristic impedance. You're causing damage, but try to do as little as possible. Damage control.

Now, the second issue is parasitics. A passive generally consists of two terminals, and the pads for them. If it is a series passive, you're going to have to create a gap in the microstrip where the passive is placed across. Which means we just created a little series capacitor too! Booooo! If you use a passive wider than the strip, you'll create larger 'plates', and also parasitics between the wider pads and the ground plane, relative to the microstrip. So one series parasitic capacitor with the gap and the two ends of the microstrip and ones to ground at either pad as well. If the pads are not wider, then you mainly just have to worry about that series parasitic capacitance. If the component has a longer aspect ratio, that makes the gap larger, and the larger the gap, the lower the capacitance. So this helps to minimize that.

One final oft overlooked thing (not to say you are doing this, but someone delivered here by the helpful guidance of google and reading this might): When using that 1/10th wavelength rule of thumb, that's 1/10th the wave length in the transmission line medium, not a vacuum. It's a little complex to figure out exactly what this is since a microstrip propagates the wave partially through the FR4 material and partially through air (and soldermask and cat dander or whatever is sitting on top of it), but it's usually within a few % of

$$ V_{p}=\frac{c}{\sqrt{\varepsilon _{re}}} $$

Vp of course being phase velocity, c being the speed of light, and ε_re being the relative dielectric coefficient, which usually is around 4.2 for FR4. Theoretically. Probably. Maybe? In the case of a microstrip, the dielectric coefficient must be corrected since only some of the wave is traveling through the FR4. There are several different ways to go about this using the width of the microstrip to help determine the 'effective' dielectric coefficient. But really, for the uses of figuring out if you even need to worry about any of this or not, its ok to ball park it usually.

Oh, I almost forgot about the antenna! No, the line is never the load impedance. The load impedance is an actual load - the characteristic impedance of a transmission line is the instantaneous impedance (the wave 'sees' 50 ohms impeding it's propagation at any given point along the line. It does not mean there is 50 ohms of impedance between one end and the other end, but that regardless of how far or close from the load the wavefront is, it always seems that same 50 ohm instantaneous impedance). The 50 ohm connector simply maintains this characteristic, but it is not in anyway a load. The antenna is the load, and it will have significant reactive impedance (at least, assuming the antenna is a useful one at your frequency). Anyway, as long as the antenna is a 50 Ω one, you'll be fine. If it's not....you'll need to match the impedance, and this beyond the scope of this answer. And yes, that means if nothing is connected to the antenna jack, you have an unterminated line that is reflecting crap and spraying crap out the end, which is why there are 50Ω termination end caps that too often people don't use but they should! EMC and all that.


Reduce the line width to 100 by chamfer over the last 1/8 w/l and use copper tape to stub match out the reactance. slide bit of various sized copper tape to get the best power transfer or lowest reflection coefficient.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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