Dielectric thickness of RF pcb, how to choose it ? - Page 1
Forum section: electronics / rf-microwave

author: jujun
author_rank: Regular Contributor
timestamp: February 03, 2020, 12:37:32 pm
content: Hello,How the dielectric thickness should be choosen ?My guess is that it's interesting to choose it to have a 50ohm trace on the PCB that have a size similar to the other components that will be on the PCB.For example: to choose a very slim dielectric, so the 50ohm track have almost the size of a 0402 capacitor/inductor.Is it right ?Then, about the losses, it seems that if the dielectric is very slim the losses are higher, but my guess is that it's a lot worse if the 50ohm track don't have at all the same width as the components on it.I also guess that if the 50 ohm track is small, it must be more electric losses in the conductor ?So, what is the best deal ?What is the most common way to choose the dielectric thickness and 50ohm track width ?Thank you for your help

author: OwO
author_rank: Super Contributor
timestamp: February 03, 2020, 01:32:59 pm
content: Usually it's based on what stackups are available or common. If this is a 4 layer board, top and bottom prepreg are either 0.2mm or 0.1mm thick. The 0.2mm option is more suited to RF work because the losses are lower and 50ohm microstrips are 0.3mm which is easy to work with. For high speed digital you will want 0.1mm thickness because the 0.12mm 50ohm trace width makes wide busses easy to route.If this is a 2 layer board, don't go below 1.0mm thickness. It makes the board mechanically flimsy.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 03, 2020, 01:34:52 pm
content: How much does it matter that components are Zo sized? You can always use wider components and traces, and body length and width are only important up to some threshold in accuracy and bandwidth.Note that you aren't usually putting single components in series with traces (or parallel), in isolation. More often you're grouping some together say for a filter, in which case the overall size of the filter matters, and this drives component size as well as layout. It does not drive trace width or pad size very much, as those can be corrected for, given a suitable simulation environment.Tim

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: February 03, 2020, 01:49:29 pm
content: Even if you use only 2 layers, Signal + GND, it is still recommended to use a 4 layer stack-up as it gives reasonable widths for the RF traces.For e.g. if you use a 10mil dielectric, the width of the RF trace is roughly 20 mils and this will match the 0402 component width. With the matched width, the pads for the components would no longer act like lumped cap or inductors.The loss is mostly a function of the loss tangent of the dielectric and not much dependent on the dielectric height. If you make the RF trace too skinny (like 4 mil) then the loss would be higher. This is due to skin effect losses as well as non uniform etch effects.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 03, 2020, 02:01:45 pm
content: There is the case where, if you can freely choose your system impedance, it's much easier to accommodate thicker boards with fewer layers. Like 2-layer 0.8 or 1mm, or even 1.6mm.Average traces here will be 80-150 ohms (give or take trace width, and microstrip vs. CPW geometry), so a higher system impedance is very attractive.Obviously, this affects selection of components. Inductor Cp is more critical; mixers and baluns designed for 50 ohms won't work as well; off-the-shelf filters are out; etc. Components with enough freedom, are fine. Say, a DDS chip with balanced current source outputs, and adequate compliance voltage range, can simply be terminated into the higher impedance without problems. Narrowband filters can still be used verbatim, if their impedances are well known and a suitable matching network is employed (an L-match with series L and parallel C, or vice versa, at each port). And for that matter, trace impedances themselves can be adjusted similarly, if a suitable simulator is available.There are many options to explore in that way; it's still much easier of course to stick with 50 ohms, so if you don't have the experience, or the time budget, multilayer boards are a small price to pay for that confidence!Tim

author: thinkfat
author_rank: Unknown
timestamp: February 03, 2020, 02:25:43 pm
content: Recent example in one of my own projects: I needed to make a 50antenna feed line for a GPS antenna on a board that was otherwise two layers (1.6mm thick). For stability reasons I could not reduce the thickness.I checked my options for the feed line, a 50 Ohm stripline would have been rather wide. I looked at GCPW geometry, but it's a bit difficult regarding connectors. Optimally, you use a PCB edge connector, which I could not do mechanically. Standard vertical through-hole connectors are tricky, CPW mode has an electrical field above the trace and a vertical connector would short out this field with its base plate.In the end I opted for a small break-out board for the GPS only and used a 4 Layer stack-up, and a regular bare-skin stripline for the antenna feed line...

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: February 03, 2020, 02:31:18 pm
content: In such extreme cases, it is better off to use a micro coax connector and perform the routing on the cable, rather than on the PCB. A U.FL connector on the PCB connecting to the GPS antenna would be a better option on 2 layer PCBs. This is possible only if the antenna is having a coax connector.