RF related question - Page 1
Forum section: electronics / projects

author: ealex
author_rank: Frequent Contributor
timestamp: March 31, 2017, 02:16:02 pm
content: helloi have the following board that i'm working on:board description:- U4, next to C17 and C8 is an AD8302 detector chip.- U4 is ~50mm away from the input side of the board - the right side (board size 100x50).- the lower-right side section that contains R6, R4, etc is a fixed 30dB attenuator- the upper-right side contains 2 chained 30dB attenuators ( R2+R3+R5 and R9+R10+R11 ) that can be bypassed by the relays marked as U1 and U3- the maximum input signal is 0dBm, from an already build DDS.- the board size is 100x50mm, imposed by another board.- maximum frequency will be 50MHz- the RF track with is 1mm, all parts are 0805.- the relays arehttp://www.mouser.com/ds/2/89/9007_series_reed_relay_datasheet-772252.pdfmy initial thought is to keep the parts spaced apart as you see, so i can solder some copper foil shields over them - shield the relays and each attenuator.is it a good idea or should i push U4 to the right where R15 and keep al RF stuff as close as possible?do you have any advice on how to proceed ?

author: radar_macgyver
author_rank: Frequent Contributor
timestamp: March 31, 2017, 02:40:44 pm
content: Reduce the trace lengths between the resistors in the attenuator. The impedance will not be 50 ohm 'inside' the attenuator, so the 1mm trace will present as a mismatch. Reducing the trace length minimizes this.Minimize the stub lengths. Right now, you have fairly long stubs on your signal path between R9 and U3, and R11 and U3. One way to completely eliminate stubs is to use two SPDT relays per attenuator. Input goes to the common of relay 1, NC of relay 1 is the bypass path to NC of relay 2, NO of relay 1 goes through the 30 dB pad to NO of relay 2, output is the common of relay 2. You could also use a DPDT relay, like the Omron G6K-2F-RF-S.Consider making the attenuator 'symmetric', by allowing more than one resistor to ground. In other words, if the original looked like a 'pi' shape, turn it into an 'H' shape, and use 2x the original resistor value. At 50 MHz, this may not make too much of a difference.

author: Zero999
author_rank: Super Contributor
timestamp: March 31, 2017, 03:34:10 pm
content: The wavelength of 50MHz is about 6m so your whole board is1/60of a wavelength, which should be small enough not to worry about impedance controlled traces.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 31, 2017, 04:14:49 pm
content: Not having seen the circuit, just looking at what's here: I don't see how the relays can bypass the resistors, when the resistors are hard wired into the input and output traces.Impedance control and shielding is probably of very little importance here. That said, you might consider some lowpass filtering, to ensure that your bandwidth is actually what you think it is. The motivating concern, if any, would be that the DDS or detector could pass clock edges, or generate harmonics, that would be more of a concern with respect to shielding and impedance.The "probably" is: if your application demands high precision, then impedance control becomes more of an issue, even at relatively low frequencies such as this. YMMV.Is this microstrip only, or CPW (top side ground fill)? I would recommend the latter; which will also reduce your required trace width somewhat, and offer better self shielding.I wouldn't worry about shielding, as the isolation between traces, separated by lots of stitched ground plane, will be very large indeed, probably in the range of 100dB. That's nothing, compared to the 30 or 60dB attenuation you have, which I guess would be the susceptible target? (However, if you were attenuating to nearly that level, i.e., 90dB+, it would be a concern. Or if you need precision amplitude and phase response in the 60dB+ range, it would also be a concern.)Tim

author: ealex
author_rank: Frequent Contributor
timestamp: March 31, 2017, 04:36:43 pm
content: thanks for all your answersT3sl4co1l : you've made me look over it again and i'm an idiot : by only shorting out R3 and R10 i'll just get a 14 ohm resistor and make the external device under test sad->back to the drawing board ...the board will be 2 layers FR4.the bottom layer will be ground - at least under the RF section.it's only a personal project, to try and see if i can make it work.i've checked the generator and looks ~ ok, still i might add an input filter section for both inputs.i'll fix it and come back with a proper schematicanother thing : any good and ~ cheap RF relay ? Omron G6K-2F-RF-S is expensive, at least for my pockets

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 31, 2017, 06:13:16 pm
content: Telecom and signal relays are reported as quite good, even at modest RF (100s MHz). You see them used in o-scope front ends, for instance.Again, transmission line effects won't be a big deal, so use capacitance specs (or estimates of them) to determine the crosstalk of the relay contacts.Tim

author: ealex
author_rank: Frequent Contributor
timestamp: March 31, 2017, 07:55:04 pm
content: this one looks interesting: ARE1012 series:http://www.mouser.com/ds/2/315/are-catalog-1075931.pdfthe graph "Isolation characteristics" at page 3 looks promising, i'll keep lookingor axicom 1462042-6http://www.mouser.com/ds/2/418/NG_SS_108-98025_E-934265.pdf- cheaper and in stock2pF at 50MHz ~= 1592 ohms

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 01, 2017, 10:39:06 am
content: If this PCB will be manufactured at a pcbhouse, I'd suggest using CPW with a good lot of viastitching. Depending on the application, it can be better to use a taper to a thinner line and put stuff closer together. The longer your lines, the more they can potentially radiate, although I doubt you'll be coupling significantly enought to worry about it. By making traces shorter you have less area to pick up noise.If you really want to go all out and use 50 Ohm lines:-Inside the attenuator, you don't have 50 Ohms, but an impedance defined by your attentuation. You should select a matching value of microstrip line.-Avoid sharp points. They like to radiate like there's no tomorrow. Manually go and add tapers to connect to components.-Make sure you get good RF capacitors and resistors. Gennerally, smaller components perform better in this regard (asin, average 0402 capacitor will behave itself better than a 0805).-Your connectors are going to desire a (grounded)CPW mode of propagation (ground - signal - ground). Ideaily, you should use a taper away from the connectors to transition to the microstrip mode.-C13 and C11 seem to be very close to your RF lines. What are their purpose? If they are there for decoupleing of your detector, move them to the other side.-Perhaps run your final lines to the detectors at 45degrees right up to the detector. This can give you two benifits: They are further away from all your other pcb area, and they are orthogonal to each other, which minimizes coupling even further.All of that said, I still think just making the signal section smaller is the better approach - the less or a fraction of a wavelength you have to deal with on your board, the better it will be performing without having to take into account all the impedance issues. I very much doubt you will be able to measure that fraction of a db of losses that you are going to get from mismatch.

author: ealex
author_rank: Frequent Contributor
timestamp: April 03, 2017, 04:13:47 pm
content: i've applied most of the advises you gave me :- input filter : the part values are already tested on the DDS part- DPDT relays to bypass the attenuators- better placement- C13 and C11 are "AC grounding pins" so i need to keep them close to the pinsi'll try adding tapers, i need to check if kicad supports them - i don't know if they will do anything at 50MHzi will rotate RL1 and RL2 so the control traces come from the top -> there is no need to interrupt the ground plane for those tracesi'll make the pcb at eurocircuits - they are ~ expensive but fast, no FR special stuff in the price rangei can afford -> plain 1.6mm FR4, etc.i will add via stitching later - i need to be careful so eurocircuits tools will accept my pcb - their DRC is very strict.updated schematic attached.