Very short traces impedance on RF board - Page 1
Forum section: electronics / rf-microwave

author: Miti
author_rank: Super Contributor
timestamp: December 10, 2019, 03:27:12 am
content: Hi,Is it a good idea to place RF components very close to each other, when possible, to avoid the need for controlled impedance traces? For example, a 0805 attenuator very close to the input of an amplifier, then the amplifier very close to a mixer, the mixer very close to a LPF?I've seen that even on professional RF boards, the 50Ohm traces are narrowed to the width of the component terminal. I'm saying the last 1 - 2 mm.How much will this approach mess up with the impedance matches?I will post screenshots once I have something.Thanks,Miti

author: bob91343
author_rank: Super Contributor
timestamp: December 10, 2019, 07:45:14 am
content: It's true that the shorter the path, the less critical the detail. If you can jam the parts together there is no need for impedance control.Try it and see.

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: December 10, 2019, 09:20:19 am
content: But sometimes, you may not have a choice to keep the components together. For e.g. a PA placed very close to the VCO can pull the VCO frequency when it is transmitting. But in general, use smallest possible components, 0402 , 0201 etc and place them as close as possible to the devices. That will minimize errors due to trace impedance mismatch.Regarding the trace width, it is recommended to match the width of the trace to the width of the components used. For e.g. when using 0402 components in series, it is recommended to keep the width of the trace close to 20mils. That way parasitic capacitance and inductance isreduced.

author: tggzzz
author_rank: Super Contributor
timestamp: December 10, 2019, 09:59:55 am
content: Quote from: Miti on December 10, 2019, 03:27:12 amIt depends on the frequency. For examples of how to use the phenomenon, see microstrip filters.

author: Miti
author_rank: Super Contributor
timestamp: December 10, 2019, 11:40:45 am
content: Thank you All!Yes, I realized after I posted that I should have mentioned the frequency range. It is 2 - 6 GHz.

author: iMo
author_rank: Super Contributor
timestamp: December 10, 2019, 11:44:19 am
content: There is a rule of thumb the traces should be shorter than 1/10 of the wavelength (where the impedance matching is not necessary)..

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 10, 2019, 11:47:43 am
content: Matching might be less critical but you are still incurring total trace length, also you have less shielding between traces because grounds are shorter or thinner. There's only so much you can pack together, of course.1/2 wave multiples have no transformation effect (Zin = Zout) but this doesn't help much if your signals are wideband.Tim

author: Berni
author_rank: Super Contributor
timestamp: December 10, 2019, 11:57:07 am
content: Well i would say that keeping them bellow 1/10th the wavelength would avoid the need for any impedance matching. Besides once the signal gets to the component pin the dimensions are different so its no longer matched anyway. Tho GHz range chips usually are tiny QFNs or BGAs to minimize that.But indeed what you have to watch out for is RF isolation. Keeping traces short also means running traces carrying different signals close to each other. Sometimes this might not matter much like the LO for a mixer since lots of that will get into your signal due to the mixer not being perfect anyway. But when you have things like chains of amplifiers this could result in feedback from the output back into the input and turning that amplifier chain into a oscillator. Depending on the amplifier choice this 'oscillator' could potentially reach rather large output power that gets fed into whatever is down the chain and blowing it up.But don't worry about it too much. Try it and see what happens, boards are cheap these days.

author: Miti
author_rank: Super Contributor
timestamp: December 10, 2019, 01:21:32 pm
content: I didn't know the "1/10 of wavelength" rule of thumb. Very interesting. Lots of good info!

author: virtualparticles
author_rank: Regular Contributor
timestamp: December 10, 2019, 03:31:41 pm
content: The 1/10 of a wavelength is an excellent rule of thumb. One other thing to consider which I've seen. When laying out an LC filter I've seen designers try to use 50 ohm traces in between the components. Don't do that it just adds stray capacitance. It's much better to use skinny traces and deal with a little inductance. The rule of thumb there is about 25 nH per inch. Jam the components together if possible.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 10, 2019, 04:29:37 pm
content: Quote from: virtualparticles on December 10, 2019, 03:31:41 pmMore specifically -- the impedance in the middle of a filter may be very different from Zo, above or below by some ratio. This is especially true of sharp filters, where you can get some very dumb values in the conventional ladder configuration. (Like a bandpass calling for 10uH inductors in series with 0.1pF capacitors -- you'll have more than that from the inductor to its surroundings, and in parallel with itself; the circuit is not simply a ladder circuit anymore! The cure is to transform branches between series or parallel, and transform overall filter, or individual stage, impedances, using a few theorems.) Knowing that impedance, gives you a better idea what the local trace width should ideally be.If the filter can be constructed in less than, say, 1/4 or 1/8th wavelength overall, yeah, pack it together and you should be fine. If you need some space, you can approximate thin traces as inductance, and lump them in series with series inductors (adjust the values as needed, of course!), and thick traces as capacitance.Note that SMT pads and bodies are usually larger than Zo trace width anyway, so a tightly packed filter will tend towards a lower Zo. Adjust accordingly, if you can (either by guessing the equivalent capacitances, or simulating the layout). And use small (0402 or less) parts, if acceptable.Tim

author: ejeffrey
author_rank: Super Contributor
timestamp: December 10, 2019, 08:11:04 pm
content: If the transmission line is < lambda/10 you can neglect transmission line effects but that doesn't mean you can neglect the impedance. Trace and lead parasitic inductance and capacitance still affect performance well into the sub-wavelength region -- you just get to treat them as lumped elements instead of transmission lines which makes it easier to compensate.

author: graybeard
author_rank: Frequent Contributor
timestamp: December 28, 2019, 11:11:56 am
content: I have always used 1/20 of a wavelength as my personal rule of thumb for when lumped element models work. When I look at distances greater than 1/20 less than 1/10 I sometimes break things into multiple lumped elements or not depending on where they are in circuit. Some simulators like ADS have distributed models built-in that are sometimes easier to use than trying to calculate or estimate lumped elements. So the choice can be determined by the simulation software you have at hand.

author: David Hess
author_rank: Super Contributor
timestamp: December 29, 2019, 10:53:44 am
content: Quote from: virtualparticles on December 10, 2019, 03:31:41 pmThat can include cutting the ground plane out from under those nodes to reduce stray capacitance. In other cases like with low impedance circuits, it may be necessary to sandwich the nodes between ground planes to reduce parasitic inductance.