Routing with RF Shields - Page 1
Forum section: electronics / beginners

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 11, 2025, 09:16:15 pm
content: I'm looking at RF shields to integrate into my project, but I have a question about them. For reference, theMS230-10Sis what I'm playing around with. I can see why they're needed at times, but I'm confused by two things.First, the footprint shows (what I assumed to be) exposed copper for the ground layer along with two through-holes for their little stubs. I guess you're supposed to solder the shield to the exposed ground as well as the through-hole places, but is it enough to just have the through-holes and not the exposed copper?I guess that brings me to my second question: how does one normally route a signal from outside the shield to the inside? I'm assuming that for the shield's proper footprint, the exposed copper is also populated with lots of ground vias. I've seen pictures of boards with exposed copper like that. In cases like that, do you route on an internal layer weaving in between the shield's surrounding ground vias and reaching inside the shield? You can't route on top, else you'd break the copper shield ring. Is the "standard" practice?

author: ataradov
author_rank: Super Contributor
timestamp: March 11, 2025, 10:59:10 pm
content: It all depends on your design requirements and frequencies involved. In most cases you only need to solder the mounting points. This shield lets you solder all around if necessary. But in many cases those shields have gaps between the mounting pins, which let you safely route things on the top layer.This specific shield would only allow routing on the inner layers or on the other side. You can't route on the top not because of ring breaking, but because of potential shorts.

author: thm_w
author_rank: Super Contributor
timestamp: March 11, 2025, 11:52:29 pm
content: Dave and Shahriar have a ton of good examples of these in products. Most of the scope ones seem to have a cutout on one side.https://www.youtube.com/c/Thesignalpathhttps://www.flickr.com/photos/eevblog/45806000321/in/album-72157701904033821https://www.flickr.com/photos/eevblog/53984557831/in/album-72177720320207221http://www.kerrywong.com/2022/01/07/teardown-of-a-nanovna-f-v2-vector-network-analyzer/

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 12, 2025, 01:49:41 am
content: Thanks. That helps clarifies things. Only other shield I've worked with had extended corner edges to fit into a slot, so seeing one like this is new to me.Since you mentioned how it's meant to be soldered on inner layers, it's now making me think more about the idea, whether it would beat soldering on top layer only.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 12, 2025, 01:50:07 am
content: Thank you. This is interesting.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 17, 2025, 10:18:51 pm
content: Kinda curious. I don't really see a lot of RF shields with soldering slots at the corners only. Any particular reason for that? Just feels that the options that I see aren't so....cheap and user friendly, for a lack of a better term.

author: ataradov
author_rank: Super Contributor
timestamp: March 17, 2025, 10:37:31 pm
content: If you only solder at the corners, you leave a consistent gap. That gap may decrease the performance or even become a secondary radiator.Shields are also big mechanical components, they need to be solidly mounted. Especially shields with caps designed to be removable. If you solder those just by the corners, mechanical pressure needed to remove the cover will rip the base off the PCB.

author: mtwieg
author_rank: Frequent Contributor
timestamp: March 17, 2025, 11:08:14 pm
content: Quote from: LoveLaika on March 11, 2025, 09:16:15 pmNo, typically these would only be soldered at the through hole pads. The shaded area in their footprint drawings is likely a suggested keepout, not a copper feature.I mean, sure you could probably put exposed ground plane there and solder it all the way around with a soldering iron if you really want. But that's not how they're intended to be used.The effectiveness of a shield with only two pins is somewhat dubious.edit: actually it seems they do make parts which have no through hole pads and are advertised as "SMT", so maybe I'm wrong about their intended use. Their website seems to make no recommendations about processes for these parts though...QuoteDepending on the application routing through the shield on outer layers is fine. Just have to make sure those signals can't act as a path for EMI to bypass the shield.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 18, 2025, 03:42:07 pm
content: Thanks. A trade off between ease of use and reduced functionality. Guess that last shield I worked with was pretty cheap. Guess there's no ways about it then. If I have to use a shield, I'd better use the right footprint for it...Would a removable shield can and shield clips (soldered to the PCB) be a good alternative to one that's soldered to the board?

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 18, 2025, 08:58:43 pm
content: Quote from: mtwieg on March 17, 2025, 11:08:14 pmThanks for your response. This would be for an RF amplifier at 4 GHz. I added via stitching appropriately and spaced out components accordingly, but I wanted to add the option of an RF shield just in case. I just can't find any good ways to integrate a shield easily. What concerns me is...repairability at this point. If you have to solder the shield to the PCB board, it would make it more difficult to remove if you need to replace the amplifier or anything. Through-hole shield are cheap, but a bit of a pain for routing. The one I selected needs you to solder all around the shield, so you'd have to route on internal layers. An easily removable shield would be nice, but I don't see anything like that.

author: ataradov
author_rank: Super Contributor
timestamp: March 18, 2025, 09:14:24 pm
content: There a a lot of shields with removable cover. Something like thishttps://www.masach.com/rf-shield-ms415-10c-ns-emi-shield-can.htmlUnless your design is really packed, it is fine for rework. The central circle part is for pick and place machines and may be removed for rework access. I worked with plenty of boards using those and never had any issues. Access is not as good as a plain PCB, of course, but it is workable.And if you are not sure that you need a shield in a first place, get the one with corner alignment pins and only solder those pins. If you find out that you actually need to solder it to get the performance you want, then you don't have too many options, you will have to solder something.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 18, 2025, 09:49:19 pm
content: Thanks. I didn't know that the center circle part was removable. I thought it was part of the frame. It would have been annoying if that 8mm circle was in the way of your component. Knowing that makes me feel better about considering that idea.Like the one you showed me, the frame has alignment holes but recommends soldering all around. If you have to have some traces to pass through the shield on the top layer (like, say the input signal or perhaps power), would it harm anything if you don't fully enclose the shield (i.e., make it so you only solder at say the corners along with the alignment pins), or would it be better to route on internal layers to pass the shield? I don't see a lot of shields with just corner alignment pins only.

author: ataradov
author_rank: Super Contributor
timestamp: March 18, 2025, 10:31:23 pm
content: It is part of the frame, but we have wire cutters. It is only necessary during assembly. And if you are doing rework, the thing is not going to be like new anyway.It is like fine to pass on the top layer, but you are risking a short, since you would be relying on the solder mask for insulation.The same style of shield exists with notches on the bottom to leave a gap for the traces.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: March 18, 2025, 11:04:58 pm
content: Yeah. It would be really bad if it accidentally shorted. And, thanks for clarifying that with the shield. That will be rough. It looks like I'll have to route on an internal layer as you suggested. (On that note, know any reliable asymmetrical stripline calculators? There's a difference in height for my 4-layer stackup)Searching onDigikey, all the cheap RF shields seem to be the same, where you solder all around. There's very few through-hole shields surprisingly when you search for through-hole shields. Plus, they are not cheap. Perhaps I'm looking at the wrong parameters in my search?

author: Bud
author_rank: Super Contributor
timestamp: March 18, 2025, 11:29:36 pm
content: Speaking from experience: 200MHz and above you want the shield soldered all around, no gaps. Any gap no matter how small will radiate.

author: mtwieg
author_rank: Frequent Contributor
timestamp: March 19, 2025, 12:03:25 pm
content: Quote from: LoveLaika on March 18, 2025, 08:58:43 pmQuote from: LoveLaika on March 18, 2025, 11:04:58 pmOk I have to ask: what specifically is a shield on a linear RF amplifier meant to achieve? I'm assuming both the input and output of this amplifier is going to have to penetrate the shield somewhere.In theory if you were to route the input/output on inner layers as striplines, then you could think of this as an extension of the shielding, but eventually those traces will need to surface somewhere anyways.And trying to route the input/output on inner layers for a 4GHz amplifier likely to cause far more problems than it solves, especially if you only have four layers with through-hole vias. Those layer transitions are going to disturb your input/output matching. Perhaps worst of all, routing on inner layers means those inner layers won't have nice uninterrupted reference planes, which is one of the cornerstones of good PCB layout.

author: newbrain
author_rank: Super Contributor
timestamp: March 19, 2025, 01:29:34 pm
content: I'll bring my limited, hobbyist experience.I have designed a short wave RX board - 4 layers: signal/GND/Power/I²C,control - where I have shielded with Masach frames+covers the most sensitive parts (input filters and LNA) and the most EMI generating part (Si5351 + buffers used for LOs).Are they useful?Yes, the effect is directly measurable.With the screen off the clock generator the S/N ratio is about 2 dB worse.With the screen on the LNA/filter block it improves by an additional dB.Routing:I just broke the ground trace and routed in and out the needed signals (LO clocks, antenna in, input to IF stages - all control signals are on the bottom layer).I'm relying on the soldermask and a bit of sandpaper to leave a minimal space on the screen bottom.Traces are designed for 50 Ω, but given the relatively low frequencies at play, I think the impedance discontinuity brought by the screen is negligible.Soldering:Screens are soldered all around, but in any case the larger one (MS737) would be very wobbly on just two pins without any other anchorage. Especially, as nctnico says, since they have removable covers. I feel that the two pins are just for positioning, not though to be the only GND contact points, not even in the smallerMS270.See the highlighted footprints in the PCB top layer below, board dimensions 8×10 cm².Disclaimer: this is what worked for me, first time I design anything vaguely RF related, this is not medical, legal, financial or mechanical advice, YMMV...

author: mtwieg
author_rank: Frequent Contributor
timestamp: March 19, 2025, 06:18:52 pm
content: Quote from: newbrain on March 19, 2025, 01:29:34 pmInteresting, thanks for sharing.Were the shields handled with a normal reflow process, or did you solder them by hand? If the former, any suggestions on paste stencil thickness/design? How much clearance is there between the edge of the shield and the board above the gaps where traces escape?

author: newbrain
author_rank: Super Contributor
timestamp: March 20, 2025, 07:40:21 am
content: Quote from: mtwieg on March 19, 2025, 06:18:52 pmI used 0805 passives for convenience as everything is soldered by hand, mostly with a soldering iron (classic Hakko 888D) and regular 63/37 Stannol, while the chips with an exposed pad (voltage regulators, LED driver - used as PIN diode driver - bottom left, QFN-24 RF attenuator mid right) using Sn/Pb paste and a hot air gun (Atten ST-862D).So no, I did not have stencils made.The clearance is much less than 1 mm, I just made sure the shields were not pressing or scratching on the soldermask.Just rolled very fine sandpaper on a 4 mm drill bit and used that. Yes, I should get a Dremel...Of course, powers and frequencies are very low, so I was not extra worried.As said, take this as just an example, I'm quite sure I have committed unspeakable sins on that PCB, this would just add to the list.OTOH, I'm quite happy with the results, feeding a -126 dBm signal to the antenna port, I get a sizeable signal on the last IF (24 kHz, to feed to an audio ADC and SDR) with > 20 dB S/N ratio.