SMA thruhole connector - how to use on 9GHz - will the stub be an issue? - Page 1
Forum section: electronics / rf-microwave

author: daqq
author_rank: Super Contributor
timestamp: March 16, 2020, 09:45:45 am
content: Hi guys,First HF design, I'm trying to determine whether the following structure of a PCB will have any too bad issues:The board is a 4 layer stackup, with only the upper most layer being meant for the RF signal. This is OK since all of the componentsasidefrom the connectors are going to be SMD. I would greatly prefer the connectors to be thruhole, mostly due to mechanical rigidity.This structure would however create a small stub (2.3mm with typical SMA connector) on the bottom of the PCB. @ 9-10 GHz the wavelength in air is ~3cm, so it should not be that much of an issue, but I'm not sure how the rest of the structure would affect the working of the device.Would cutting the stub off help, or is it simply OK to ignore this stub completely?There are SMA SMD-thruhole hybrids such as the 32K141-40ML5 connector, but they are fairly exotic and nonstandard, where as the simple ones likehttps://www.farnell.com/cad/1510247.pdfare cheap and plentiful and interchangeable. Sadly, the connector needs to be mounted pretty much in the middle of the PCB, so that removes the options of edge launch connectors.Thanks,David

author: ejeffrey
author_rank: Super Contributor
timestamp: March 16, 2020, 03:35:19 pm
content: It's the capacitance of the rest of the pin (and PTH) inside the PCB that is the biggest problem when doing this. Reduce or eliminate the annular rings on the additional layers, and cut away additional ground and power planes as far as practical. Where is the ground reference? If you are doing a microstrip between the top layer and inner plane 1, consider launching to a microstrip with bottom ground.Can you flip the board over so the connector is on the bottom side and the signal comes out the top? That is ideal for these connectors.

author: daqq
author_rank: Super Contributor
timestamp: March 16, 2020, 07:54:02 pm
content: ejeffrey, Thanks for the reply.The ground reference plane is directly below the top layer, so, INNER 1. I am hoping to confine all of the RF on the TOP layer with INNER 1 used as a ground plane..The target structure is a coplanar waveguide.QuoteUnfortunately the board cannot be flipped, there can't be any parts on the bottom aside from the soldered pins.QuoteGreat advice, thanks, will do that. Would internal milling be of any use? Cut around the pad completely?

author: ejeffrey
author_rank: Super Contributor
timestamp: March 17, 2020, 11:46:09 pm
content: Quote from: daqq on March 16, 2020, 07:54:02 pmThat's kind of what I guessed. CPWG is kind of the worst case for these connectors in my experience. Can you have a different structure near the connector launch? I think (based on measurements and simulations I have done on similar setups) that you would get better performance if you launch with a microstrip. Its not hard to do a transition. In fact, a nice trick I have used is to launch with a microstrip on the bottom layer referenced against inner_layer1. Then you can transition the signal from bottom to top, again referenced against inner_layer1. Since you use the same reference plane for both structures it is much easier to handle the transition as you don't have to provide ground vias. Since you want to go to CPWG you will still need ground vias to the top layer, but it is still quite a bit easier to manage. This all takes up a lot of space, and needs adequate shielding to prevent RF getting in and out of your bottom layers, but might be worth the effort if you want high performance at 9 GHz with this connector.Milling around the center pin could help -- maybe a lot. I haven't tried it or simulated it, but reducing Er by a factor of 4 will definitely reduce capacitance.One more thing: if you do use the hybrid surface mount signal + through hole ground connectors double check the assembly notes with your fab. I have received boards back using those where they didn't place the connectors for the reflow phase. The center pin wasn't actually soldered but would make intermittent contact.

author: daqq
author_rank: Super Contributor
timestamp: March 18, 2020, 09:09:59 am
content: QuoteYes. A microstrip could be used, there is space on the board. Gonna have to read up on those (still trying to wrap my head around even the most basic concepts), but according to the calculator (Saturn PCB calculator) the width for the path is not that different from a CPW structure (for 50 Ohm and 0.191mm substrate thickness it's ~0.39mm for a CPW and 0.45mm for a stripline). How much of a distance (D) should there be between the ground on the top layer and the signal?QuoteThanks for the tip! Though at the moment the fab will be me sitting like the hunchback for several hours with a soldering iron

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 19, 2020, 09:05:52 am
content: Quote from: daqq on March 18, 2020, 09:09:59 amI assume you refer to conductor-backed/grounded CPW, and not 'real' CPW? if so, it makes sense that microstrip and CB-CPW approach the same conductor width for such a gap: the capacitance from your ground plane is going to dominate the impedance. The distance of the side to a (CB)-CPW is given by your calculator. With microstrip, you can always use a CBCPW calculator and just plug in a gap distance, and see what impact it has on the impedance.Note that some of the CBCPW calculators online become inaccurate when this is the case, the equations they use are based on a number of assumptions (I can't recall them off the top of my head, but I have seen them disagree with true EM solvers by a factor of 2 - so that 50 ohm transmission line ends up actually being 100 ohm...)Do you have any simulation software to quickly verify performance?

author: daqq
author_rank: Super Contributor
timestamp: March 20, 2020, 12:04:33 pm
content: Thanks for the info!QuoteWow, that bad? I'm using the Saturn PCB calculator and it seems to be OK - I have confirmed this with my PCB manufacturer.QuoteAt the moment I'm battling with OpenEMS. It's winning.

author: khach
author_rank: Contributor
timestamp: March 20, 2020, 04:12:08 pm
content: Like that 2.4mm connector with vias ringMore athttps://www.intel.com/content/www/us/en/programmable/documentation/joc1462311266908.html

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 20, 2020, 04:16:00 pm
content: Quote from: khach on March 20, 2020, 04:12:08 pmProblem with all these examples is that they are really only applicable to the specific stackup used for that footprint. The only way to really know what the performance will be is to get the 3D model from the manufacturer (which is also why good manufacturers should provide you with a suitably accurate 3D model of the connector) and put it all together in a 3D EM simulator. At frequencies where you use SMA it is probably not that vital, but once you get into the realm where you use 2.92mm etc, you really need to model this transition.