Why are the this TX lines necked down? - Page 1
Forum section: electronics / rf-microwave

author: eecook
author_rank: Regular Contributor
timestamp: June 25, 2021, 09:50:57 pm
content: Hi All,I took the lid off of an RF switch and I see that the microstrip lines are necked down as shown in the picture. Any idea as to what that is for?

author: Kerlin
author_rank: Regular Contributor
timestamp: June 25, 2021, 11:52:11 pm
content: I was once asked this exact question in a job interview for a Senior RF Engineer, with a high profile RF company.I didn't know the answer but a friend of mine who went for the same interview told me that he said it was to broadband the line and they told him he was correct.Without knowing the operating frequency, dielectric constants and the stripline measurements I would not try to guess the original design.My experience, especially were I was wrong, tells me not to guess especially since the image doesn't even show underneath it which is important.It's probably for impedance matching or broad banding,or maybe both.It is a stripline not a microstrip line, a microstrip is sandwiched between two planes.Every inductance has a capacitance and every capacitance has an inductance and is resonant some where so the techniques used are not always totally clear by inspection.The company running that interview made microwave cavity filters like this one. It gets much worse when trying to sort these out.This image is a filter for a cellular base station. They are often site specific as they filter out other carriers by introducing very high attenuation at carrier frequencies on the same mast and let one through with very low loss, all with no cross mod or mixing.Its CNC made and no tuning is allowed in case it needs to be mass produced. So Engineers employed for such designs do exact calculations. Such RF Engineers are really mathematicians, no guesses.Glad I didn't get the job, I went into Avionics RF and digital stuff much better than punching a calculator and using CAD packages all day.

author: WideBandwidth
author_rank: Contributor
timestamp: June 26, 2021, 12:34:04 am
content: A small notch in a microstrip line creates a small length of high impedance -- effectively an inductance. Seems like the most reasonable reason to have an inductance there is for impedance matching.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 26, 2021, 02:38:06 am
content: There's an equivalence between LC and transmission line networks. The wider pads of the connectors may have a low impedance, acting as a capacitor, in which case the length of narrow trace may help to balance that (as an L-match network). Or perhaps it's more for the coupling capacitor (same idea, but its body width/height acts to reduce Zo). Or it might be to tweak an HF cutoff (frequency response).More generally, an alternating wide/thin transmission line has a lowpass characteristic; the amount of attenuation available isn't very much (because the ratio of impedances isn't very large, that is to say, the filter Q is small), but it's cheap to do, so often such a filter might be constructed with like 10 poles or more. Just doing one or two, it would act more to tweak frequency response, without having a huge effect overall.I suspect it's not so much about the connectors, as the lengths (between narrow segment, capacitor and connector pad) don't really follow. Normally, connectors are kept stable by removing ground plane under the pad, compensating for the width. So it might be about the capacitor.Tim

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: June 28, 2021, 07:56:12 am
content: Quote from: T3sl4co1l on June 26, 2021, 02:38:06 amI was thinking the same - usually you cut your ground plane, but it this case it seems like the PCB is solidly connected to a metal enclosure. So it might simply not be possible to cut the ground to induce inductance/reduce parasitic pad capacitance here.

author: Joel_Dunsmore
author_rank: Regular Contributor
timestamp: July 03, 2021, 11:27:55 pm
content: Very likely compensation (in for form of a short section of higher Z line) following the mono-block capacitor next too it. Even though the mono-block sits within the line, it very likely causes impedance of the line to be too low, so following with a bit of high-Z line can compensate match up to some corner frequency where it will form the stop-band of an LPF. Hard to tell but it looks like coplaner line at the PCB launch and if that was also made to be a little higher Z than Z0, then you have a LCL structure which can have good match across a band of frequency until it reaches it's natural corner freq.That, or someone, once in the distance past, built that launching structure and found he could improve some aspect by scraping away a bit line must past the cap, and then made it part of his standard design toolkit.OR and this might also be a possibility, it is there to add a wee matching capacitor to ground. I've seen production processes that have little structures like that where the test tech has sets of small (0.5 steps form 0.5 to 2 pf) caps on the end of tooth picks that they put on the line to see which one gives the best performance, then take a real part and solder it in. I've seen much worse than that too.