First RF PCB Review - Page 1
Forum section: electronics / rf-microwave

author: MAntunes
author_rank: Regular Contributor
timestamp: August 03, 2018, 03:56:00 pm
content: Hi guys!If this is not the right place to post this tell me so.Could you guys take a look at my first RF PCB? It's a breakout board for the Microchip RN2483 LoRa Transceiver (868MHz).My main question is about the antenna part: is it well done? The trace is 0.75mm, the vias are spaced 1mm and there are ground planes on top and bottom.Any questions please tell me.Thank you very much,Miguel

author: daqq
author_rank: Super Contributor
timestamp: August 03, 2018, 05:54:40 pm
content: A bit of a via overkill situation on most of the board. No decoupling capacitors (or any supporting components) are present.For proper trace impedance we also need the board thickness and the distance between the ground and the trace (that said, on such a small length it should not matter that much).

author: the_janitor
author_rank: Newbie
timestamp: August 03, 2018, 06:46:16 pm
content: Not much to review given the simplicity. Maybe provide the stackup so people can check if Z0 = 50 ohm. Also, you should add some impedance matching topology (L, Pi, T, ...) between the module and the antenna. And yea, way too many vias.

author: MAntunes
author_rank: Regular Contributor
timestamp: August 04, 2018, 09:45:01 pm
content: Thank you guys!Quote from: daqq on August 03, 2018, 05:54:40 pmI agree, it was a bit overkill. The board is going to be regular 1.6mm board with 1oz copper.The distance between the ground plane and the trace is 6mil.About the capacitors and other passives the datasheet says that they are not needed. But I still put one near the VDD pin.Quote from: the_janitor on August 03, 2018, 06:46:16 pmDo I really need to impedance match? I followed the example on the datasheet.Here is the new version of the board, this time with silkscreen.

author: the_janitor
author_rank: Newbie
timestamp: August 05, 2018, 07:28:03 pm
content: You may need to impedance match depending on the antenna that you choose. It's not uncommon that antennas advertised as 50 ohm impedance at a certain freq. aren't really 50 ohm (it's always better to measure it yourself with a VNA). Anyway, just put a Pi or 2L matching circuit, and, if you don't need it, you just don't populate it (and use 0-ohm resistors for the RF path).

author: yl3akb
author_rank: Regular Contributor
timestamp: August 05, 2018, 07:51:59 pm
content: Quote from: MAntunes on August 03, 2018, 03:56:00 pmIt most probably does not matter in this case, but You nicely tried to calculate correct trace width and then placed 3x wider SMA pad with in series, which kind of defeats the purpose of effort to use correct impedance transmission line.

author: MAntunes
author_rank: Regular Contributor
timestamp: August 06, 2018, 01:45:29 pm
content: Quote from: the_janitor on August 05, 2018, 07:28:03 pmThank you! I'll keep that in mind. I don't have a VNA on my lab though :/Quote from: yl3akb on August 05, 2018, 07:51:59 pmThank you! I used the footprint given by the connector datasheet (https://www.molex.com/pdm_docs/sd/732511150_sd.pdf). What should I do?I am now trying to calculate the trace impedance and it gives me a value of around 95 Ohm using this calculator:http://www.hughescircuits.com/index.php/fr/support/impedance-calculatorI used a dielectric thickness of 1.6mm, trace thickness of 3.5mil and trace width of 0.75mm.

author: eb4fbz
author_rank: Regular Contributor
timestamp: August 07, 2018, 02:02:15 pm
content: I prefer not to use thermal relief on RF connector ground tabs. They add inductance to the RF path. I even put ground vias right under those pads!

author: mik4el
author_rank: Contributor
timestamp: August 08, 2018, 10:26:40 am
content: Quote from: yl3akb on August 05, 2018, 07:51:59 pmThanks for your comment.I'm also a newbie in higher frequency RF. I'm having similar issues I think with a much bigger central sma edge connector footprint than the coplanar waveguide transmission line for a pcb I'm trying to optimize the RF part on.What is the general advice, should one keep the transmission line width the same as the sma edge center pin width and then calculate the transmission line characteristics from that? Or should one put an impedance matching circuit between transmission line and sma edge center pin? Or something else? =)

author: Rerouter
author_rank: Super Contributor
timestamp: August 08, 2018, 10:34:42 am
content: For transmission lines, you plan your widths based on the PCB, once the signal gets to the connector you can consider it matched by design.If you want to get crazy, you can neck the trace down near to the pin width as you enter the connector (ground above connector lowers the width you need for a given impedance.

author: mik4el
author_rank: Contributor
timestamp: August 08, 2018, 06:39:30 pm
content: Sorry to hijack the thread with my question, but to clarify, I've uploaded a screen grab of my board around the sma edge connector.I have a transmission line calculated to be 50 ohm (the thin red line) coming in to the sma edge central pin footprint (the big red block). Am I wrong to assume that there is an impedance discontinuity between the transmission line and the sma edge central pin footprint that causes reflections? Is this an ok layout for higher frequencies? How would you have done this part of the board?

author: Rerouter
author_rank: Super Contributor
timestamp: August 09, 2018, 09:30:16 am
content: Yes there would be, there is also a high risk of pad tearing due to the sharp corners, Looks like your using KicadIf your using Kicad, you can decrease the sharpness of the discontinuity by drawing a zone over the effected area, a trapezoid between the trace and the pad,If you wanted to go the whole hog you could create a partial void of ground near to where your trapezoid begins, widening towards the pad, that way you could maintain the same impedance for the entire termination, but even I have not walked that road yet.

author: izsurk
author_rank: Newbie
timestamp: August 09, 2018, 09:39:26 am
content: Quote from: mik4el on August 08, 2018, 06:39:30 pmJust a hint to check your impedance calculation again. The trace looks very small to me (for FR4). Width of course depends on your layer stack. If you're using a multilayer (4 layers or more) that might be ok. If you're using 2 layers only, the trace looks too small. Are you using FR4 or some special material (Rogers, etc.)? Just a hint.

author: mik4el
author_rank: Contributor
timestamp: August 09, 2018, 10:24:32 am
content: Thanks for your comments! I'll definitely try this for the next board iteration.Quote from: izsurk on August 09, 2018, 09:39:26 amI use oshpark's 4 layer pcb which uses FR408 (https://docs.oshpark.com/services/four-layer/). I've attached my calculations below fromhttp://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm

author: yl3akb
author_rank: Regular Contributor
timestamp: August 09, 2018, 10:29:08 am
content: Quote from: mik4el on August 08, 2018, 06:39:30 pmIdeally You would like to use SMA connectors designed for thin traces, like these, but they are very expensive:https://www.amphenolrf.com/media/downloads/7780/C901-10513-1.pdfOr here is the option for ~1.1mm trace width:https://www.mouser.com/ds/2/643/pi-CCS-JOHN-142-0701-881-1290308.pdfOf course You should estimate if and how much that particular length of mismatched line affects matching at your operating frequency. First step would be to carry out simple model based simulation. Maybe mismatch caused is not important in Your case.Yes, tapered transition would be better than abrupt impedance step if no option for more adequate connector existsYou can also consider method to remove the ground plane below wide section to bring impedance up to desired:http://citeseerx.ist.psu.edu/viewdoc/download?doi=10.1.1.399.4140&rep=rep1&type=pdfI would check and tune it in EM simulator though.

author: hagster
author_rank: Frequent Contributor
timestamp: August 09, 2018, 12:13:10 pm
content: Firstly at 868MHz and with the length on the track and size of connector pin, I don't think there is likely to be a huge amount to be gained by improving the design.Second, If you really think you need to worry so much about the characteristic impedance of the track you need to take the top copper flood fill into account. the current spacing is much less than the 1.6mm PCB thickness. What you actually have is a Grounded Coplanner Waveguide (G-CPW). There are online calculators for this. You can make the track the same width as the RF module pad and adjust the flood fill gap to get the correct impedance.Third, As a CPW, most of the return current is flowing on the top layer. Adding vias to the ground pads of the SMA wont help much as return signals that pass through these have and extra 3.2mm before they return to the RF module. Best to sought out a better solution for the thermal spokes (which will help a lot with soldering).

author: LukeW
author_rank: Frequent Contributor
timestamp: August 17, 2018, 04:59:12 am
content: Other people have basically said the same, but:- You don't need that many overkill vias, especially away from the RF area.- I would put footprints for a general pi network in the RF path, even if you just load it with 0series and no shunts- Use 0402 for the pi network footprints- Maybe smooth curves instead of 45 degree bends, but it will make bugger-all difference.- No thermal relief in the RF area- Make the SMA centre pad the same width as the microstrip line- Personally I would fill in the whole area around the SMA ground pins with vias which adds mechanical strength as well as electrical stitching.(Hard to solder and impossible to desolder, though.)