FR4 Dielectric constant - Page 1
Forum section: electronics / rf-microwave

author: woffermom
author_rank: Newbie
timestamp: February 23, 2023, 04:31:27 pm
content: Am planning to build a microstrip directional coupler using FR4 material. I know that the dielectric constant of FR4 can vary depending upon the fiberglass mix used to produce the pcb material.Does anyone know of a FR4 source on eBay or Amazon who can deliver FR4 material with a known, specific dielectric constant?Al Burke / woffermom

author: Hamelec
author_rank: Regular Contributor
timestamp: February 23, 2023, 07:02:07 pm
content: I know my answer isnt helpful for you, but unfortunately it is "No"..

author: dmowziz
author_rank: Contributor
timestamp: February 23, 2023, 07:59:40 pm
content: Seehttps://www.eevblog.com/forum/rf-microwave/copper-tape-microstrip-prototyping-on-a-pcb-of-unknown-dielectric-substrate/

author: switchabl
author_rank: Frequent Contributor
timestamp: February 23, 2023, 08:54:27 pm
content: This. Even if you get brand-name FR4 with a proper datasheet, you will find that permittivity is not exactly tightly specified.Look at this example from Technolam:https://www.technolam.de/fileadmin/user_upload/FR-4-11PYTL__FR-4-11PYR__FR-4-11PYB.pdfThey guarantee a maximum value of 5.4 @1 MHz (4.4 typical). At 1 GHz there is just a supplementary specification (4.0 typical). And that's it. So you will want to measure a test PCB and adjust your design accordingly in any case. Mind you, a quality laminate is still likely to have better consistency within and across batches.If you need tight tolerances (and lower loss), you need to look at ceramic substrates (Rogers etc.).

author: floobydust
author_rank: Super Contributor
timestamp: February 23, 2023, 09:13:08 pm
content: I did one 800-2,400MHz project using cheapola FR-4.What we did is characterize (across the band) some popular laminates, and then specified use of that laminate to the PCB fab.At first I was sticking to higher quality like Isola or Panasonic R1755V (spec Dk=4.31@1GHz) but one build had fake Panasonic laminate, even sent it to Panasonic for confirmation.The cheap laminates use a lot of resin (compared to fiberglass) so a bit worse Dk. It was actually difficult for PCB fabs to stock/use odd or specialty laminates.At the end it wasVentec VT-47(Dk=4.28@1GHz, max. 5.2) that we used successfully. Kingboard or Nanya were also contenders but a bit too cheap.Ask your PCB fab what they commonly use, characterize it and go that way assuming your stripline can work with slop in Dk.

author: Gerhard_dk4xp
author_rank: Frequent Contributor
timestamp: February 23, 2023, 09:50:53 pm
content: I used the JLCPCB ??28 4 layer process and their striplinecalculator says that a 50 Ohm microstrip on layer 1 is 11.55 milwide when Layer 2 is GND. That process is not even impedancecontrolled, 5 boards for $5 or so. I put a test structure, consistingof a 12 mil microstrip with SMA card edge launchers on asynthesizer board that I had do do anyway and checked it witha 18 GHz 54754A time domain reflectometer. The microstrip wasright on spot, perhaps half a pixel below the 50 Ohm line in the TDRwhich may be the missing half mil, but really does not need anexplanation.SMA launchers with fat center pins created for 1.6mm 2-layerboards do not work properly. It takes either the good ones madeby Rosenberger with thin center pins or GND cutouts on layer 2 & 3with enough vias from layer 2 to 4.IIRC, eps-r was 4.2, cannot check that from here.Gerhard

author: ejeffrey
author_rank: Super Contributor
timestamp: February 23, 2023, 11:11:29 pm
content: The directionality of microstrip directional couplers is pretty crappy because the even and odd modes see different dielectric constant. It's better to use stripline if possible.

author: ahbushnell
author_rank: Frequent Contributor
timestamp: February 23, 2023, 11:43:13 pm
content: Hi,Use materials designed for impedance control. Rodgers is an excellent source.https://www.rogerscorp.com/advanced-electronics-solutions/ro4000-series-laminatesFR4 is designed to be low cost and not for impedance control.Good luckAndy

author: Uky
author_rank: Regular Contributor
timestamp: February 26, 2023, 12:24:07 pm
content: IMHO the use of FR-4 for RF depends on the frequency it is to be used for.I have successfully designed and implemented directional couplers on FR-4 on VHF and UHF frequencies up to 880 MHz provided that coupling gapsare not to narrow due to manufacturing tolerances and also by requiering a specific brand and version of resin vs fiber glass mix.It was some time ago, but then a specific ISOLA part number was specified together with the board manufacturer. It is also important thatif the coupler is instantiated as stripline (internal between two planes) on a multi-layer board that the pre-preg is not too old since the compressibility of it deteriorates with timedue to ageing which also affects the performance.As the frequency increases, the dielectric losses increases and so the dimensions must be kept as small as possible. VHF, no problems. UHF, be careful,above 1GHz, think twice if the structure is complex. If it is: Consider dedicated RF-laminates.If you stay on FR-4, also consider the tolerances of the finalized design.

author: JohnG
author_rank: Frequent Contributor
timestamp: February 26, 2023, 02:31:05 pm
content: FR-408 might meet your needs. It is sort of a compromise between "standard" FR-4 and more expensive RF materials. Slightly lower permittivity than regular FR-4, but provides typical numbers from 0.1 GHz to 10 GHz and they are reasonably tight.https://www.isola-group.com/wp-content/uploads/data-sheets/fr408-laminate-and-prepreg.pdf?t=1244069582I am not an RF expert, but I have used this material for high speed power electronics.John

author: nctnico
author_rank: Super Contributor
timestamp: February 27, 2023, 01:26:56 pm
content: In my experience 4.5 is a good number to work with when the dielectric constant isn't specified for FR4.Another thing to consider is variation in the etching process. The thinner the traces, the bigger the effect of variations in the etching process. I've seen 0.1mm traces ending up from 0.07mm to 0.11 mm. It may seem beneficial to use the thinnest dielectric so traces can be narrow but for accurate impedance matching it is better to have wider traces. Say in the 1mm ballpark. But if accuracy really matters, then other materials are better. I highly recommend doing simulations using packages like Sonnet (AFAIK there is a free light version).