2 layer controlled impedance on a budget - Page 1
Forum section: electronics / general

author: tszaboo
author_rank: Super Contributor
timestamp: June 29, 2025, 09:29:54 am
content: So I've been doing some RF tinkering at home, for frequencies up to ~6GHz. For this I've ordered some controlled impedance PCBs from JLCPCB but it was always 4 or 6 layer boards. 6 layer usually wen I needed to open up the GND below pads on the top layer, to get 50 Ohm. And my designs were (shielded) coplanar waveguide.I don't really use the 4 or 6 layers, I often times end up with 5 GND layers. The next design I'm making is strapline, and 2 layers are just fine.So who sells controlled impedance boards for 2 layer?How I learned to stop worrying and love the random FR4 core?

author: nctnico
author_rank: Super Contributor
timestamp: June 30, 2025, 04:11:31 pm
content: Controlled impedance does not exist. It is just a marketing term for stackups which have thin dielectrics between some of the layers so you can route high density digital circuits which kind of meet impedance specification albeit with a large tolerance.If you have a two layer board, what helps is to make the board thinner. Like 1mm or 0.8mm so the traces can be thinner. OTOH, you don't want traces to become too thin because the etching tolerances start to cause a serious error. This is also why the so called controlled impedance stackup are not so suitable for doing RF stuff as the traces become very thin. For RF stuff, I typically like to use widths from 0.8mm to 1.5mm.

author: tszaboo
author_rank: Super Contributor
timestamp: June 30, 2025, 05:45:50 pm
content: For me controlled impedance means that the manufacturer is going to use a stack up that is defined. The core, prepeg is coming from a specific manufacturer, or a range of compatible ones. The plating thickness is defined. Er doesn't have variations between ordering the same board twice.At work I just send the stackup to the fab, and they make the board based on that.This time I would like to build a Wilkinson power divider. That has a variety of impedances on a single board. At home, to try a few things.For Er or 4-ish, I've calculated 2.7mm for the lowest, 50 Ohm trace. So I see why two layer boards are typically not used for RF, or digital. My issue is that I don't even see an option to have defined stackup for 2 layer boards from China. It's just whatever, be happy you get a PCB.For RF, at work (or home), I like to get the trace width to 0.6mm. That way any 0402 component placed on it is going to have the same pad size as the trace width. Usually this becomes a coplanar waveguide. That places the ground on the "other side of the 0402" and reduces the influence of any traces around.I just measured and matched an antenna today at work, and got 94-98% efficiency in the entire bluetooth range, I was quite happy about it.Some of these controlled impedance boards indeed have their prepegs that are too thin, which makes the track width very thin. I just punched in the numbers for a 100 Ohm trace into the calculator for a stackup, and it's 0.09mm, impossible to make.I've also checked Rogers materials, seems to be that the prices are not suitable for a hobbi. 250EUR for a single board. If I need to re-spin it 3 times to get everything right...

author: thm_w
author_rank: Super Contributor
timestamp: June 30, 2025, 09:38:01 pm
content: Hans uses plain FR4 for all of the demos he's done but only measured up to ~4GHz from what I remember:https://www.youtube.com/watch?v=fxOD7g_L3gkJLC it looks like options are: 6 layer, PTFE 2 layer, and Rogers 2 layer from least to most expensive ($35 to $100).If you are really cheap and want to screw around, use plain 2 layer and make 3 variations on the design with calculated width then +/- 15% or whatever width. Lot of hassle though.

author: nctnico
author_rank: Super Contributor
timestamp: June 30, 2025, 09:55:28 pm
content: Quote from: tszaboo on June 30, 2025, 05:45:50 pmFor FR4 Er ranges from 4.3 to 4.7 or so. I've found 4.5 is a good value to use. Even at the extremes, the difference is small enough not to matter. Tolerances in resistor / component values and loss in FR4 will have a bigger influence on the circuit performance.

author: wraper
author_rank: Unknown
timestamp: June 30, 2025, 10:26:43 pm
content: In the past AllPCB let you chose particular PCB material for which you could find a datasheet with actual spec, but seems it's no longer the case. Most of the cheap services use whatever they have in stock. Also chosing different options, such as solder mask color, or whatever of their internal thing may result in orders going to different factories with different materials.

author: tszaboo
author_rank: Super Contributor
timestamp: June 30, 2025, 11:40:08 pm
content: Quote from: thm_w on June 30, 2025, 09:38:01 pmI've watched Hans' video after I decided to make one. With JLC, you can choose stackup even wit 4 layer boards, for now this is probably the cheapest option I found for the defined stackup. Plus they have an impedance calculator on their page.Quote from: nctnico on June 30, 2025, 09:55:28 pmLike, when I'm making an antenna on FR4, the length of the antenna will depend on the Er. Originally I make the antenna longer and cut it to length until it resonates at the right frequency. Then match it. Large variation in the Er will mean that the antenna will resonate at a different frequency. If you have an antenna design that has 100MHz bandwidth at 2.4G that Er will matter quite a lot. It's too late to calculate it, but I think you get the idea. I kind of agree with you for digital signals, where you get a bit extra ringing maybe, who cares.Quote from: wraper on June 30, 2025, 10:26:43 pmExactly the issue. If I need to fix something, and order a new one, it's a coin toss if I get the same material. It might be that me fixing it will make things worse on the new FR4.

author: ftg
author_rank: Frequent Contributor
timestamp: July 01, 2025, 10:59:41 am
content: Quote from: wraper on June 30, 2025, 10:26:43 pmI just checked and it seems to allow selecting the material, with leaded HASL and ENIG, but Leadfree HASL is "please contact customer support".

author: tooki
author_rank: Super Contributor
timestamp: July 01, 2025, 11:15:22 am
content: Quote from: nctnico on June 30, 2025, 04:11:31 pmProper controlled-impedance PCB service means not only using defined board specs and trace specifications, but that the manufacturingprocessis designed to give you certainty of impedance compliance, in that the manufacturer also adds impedance test traces to the panel (outside of your PCBs), which are then measured and the results included in the PCB delivery. They may include images and measurements of cross-sections of the test traces.

author: wraper
author_rank: Unknown
timestamp: July 01, 2025, 11:56:30 am
content: Quote from: ftg on July 01, 2025, 10:59:41 amAh, I didn't go through the price calculation. I just recalled it was there and there was none to select on a quick glance, didn't order anything from Allpcb for years.QuoteShows the price for me.

author: tszaboo
author_rank: Super Contributor
timestamp: July 01, 2025, 12:35:03 pm
content: Quote from: tooki on July 01, 2025, 11:15:22 amSome board houses will send you a small, epoxy encased cross section of the PCB. So the plating thickness, layer distance and whatnot can be verified with a microscope. I remember seeing the supply chain manager collecting these and building small towers of them on his desk.I don't think it was ever actually verified, we didn't have the positioning table for that.

author: tszaboo
author_rank: Super Contributor
timestamp: July 01, 2025, 01:45:46 pm
content: Thanks for the tips, I made some search to see what are the options.AllPCBSeems like 1 oz (please just start calling this 17um) is "contact customer support. for HASL lead free. 35um is standard.An order with 100x100mm (all the rest is calculated at this size) is 24USD + 6 USD shipping. There might be some discounts.JLCPCB4 layer board with JLC04161H-3313 or JLC04161H-7628 stackup is 6 EUR+ 6 EUR shipping. I think once per month you get shipping discount, resulting 8 EUR total, plus some payment fees.2 layer board is not possible with specified stackup.Impedance calculator:https://jlcpcb.com/pcb-impedance-calculatorPCBWayAdvanced PCB with Shengyi S1141 is 128 USD (yeah no)Regular PCB with the option selected as S1000H as base material 5 USD , shipping 6 USDhttps://www.pcbway.com/blog/PCB_Manufacturing_Information/Reasons_to_Choose_SYTECH_S1000H_750db11c.htmlPCBgogo (I have no experience with them)Same, S1000H can be selected, 5 USD for boards, 14 dollar shippingElecrowDoesn't specify it on the order page, but their wiki said they use this FR4:https://www.elecrow.com/wiki/image/3/34/PCB_material_FR-4_info.pdfI wrote to the customer service to confirm that this is the only FR4 they use, or I can specify to use this. Unfortunately the Er is only specified to 100MHz.update: it's not, custom quote is needed.Price is 4.9USD + 6 USD shipping, They have discounts often.Let's take a look at European suppliersEurocircuits:Regular PCB will use a defined FR4 material: About 60 EURDefined impedance pool (Isola base material): 150 EURRF pool (Isola or Rogers material): 170 EURMulti-CBThey seem to use different FR4s, when impedance control is enabled on the online calculator, the price jumps to 115 EUR.

author: wraper
author_rank: Unknown
timestamp: July 01, 2025, 02:30:51 pm
content: Quote from: tszaboo on July 01, 2025, 01:45:46 pmBoth are the same company hiding behind multiple storefronts.

author: tszaboo
author_rank: Super Contributor
timestamp: July 02, 2025, 11:38:32 am
content: Quote from: wraper on July 01, 2025, 02:30:51 pmThanks, that makes sense.Elecrow just emailed me that they are using multiple FR4s, and special quote is needed for fixed stack-up.For now best option looks like JLC's 4 layer board is the easiest/cheapest 2 layer board. You have the choice of 2 stickups. By skipping layer 2, layer 2 and 3 you get 3 different heights. And 1.2mm or 1mm can be selected without extra surcharge. Pretty amazing you can order PCBs now for less than a price of a pizza.

author: asmi
author_rank: Super Contributor
timestamp: July 02, 2025, 02:24:52 pm
content: Quote from: nctnico on June 30, 2025, 04:11:31 pmBullshit. It does exist as a guarantee that traces which follows certain specifications, will end up having a well defined impedance with agreed upon tolerance (which can be as tight as 3% if you're ready to pay for that - maybe even tighter are possible, but 3% is what I've heard about myself), and if not - these boards will be considered failed, and manufacturer will be at fault for not fulfilling his obligations. Manufacturer does have some control over final impedance by selecting specific materials (not all prepregs are the same, especially after they are pressed upon into a stackup) - which is why "talk to your PCB manufacturer" is the most relevant advice when you need your PCB to meet strict specifications - because nobody knows their manufacturing process better than them, so they will always tell you what kind of trace specs to use in order to achieve target parameters.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: July 02, 2025, 03:38:11 pm
content: One way to limit the effects of the "weave" of the glass fibers in a PCB is to route tracks under some (mostly arbitrary) angle. This can limit errors due to one wire of a diff pair being "on top of" a bundle of glass, while the other is "in between the gaps". There have been a bunch of papers written on this, but it was never very relevant for me.

author: asmi
author_rank: Super Contributor
timestamp: July 02, 2025, 04:25:18 pm
content: Quote from: Doctorandus_P on July 02, 2025, 03:38:11 pmThat is why there is a tolerance for impedance. Typical value is 10%, 5% are also available in some fabs as a premium option for those who need it (or if they got more money than they know what to do with), I've heard of 3% for ultra high end process, but I never needed anything better than 10% for my boards so far, so I don't have any practical experience with tighter tolerances.

author: ejeffrey
author_rank: Super Contributor
timestamp: July 04, 2025, 04:25:23 am
content: Quote from: nctnico on June 30, 2025, 04:11:31 pmWhat? No!!!Controlled impedance means that you and the boardhouse agree on a geometry that they promise will hit your impedance targets with their process. They should be producing test structures on the edge of the panel and testing then to make sure the process is in spec.On a recent project we had single ended microstrip on the outer layers and differential microstrip and stripline on the outer and inner layers.

author: nctnico
author_rank: Super Contributor
timestamp: July 04, 2025, 11:35:48 pm
content: Quote from: ejeffrey on July 04, 2025, 04:25:23 amWell, in the end it is all about trace width control. Having test traces outside the board gives some indication that the widths aren't way off but it requires very even etching. But again, this is mostly relevant for high density digital boards with very thin dielectrics and traces less than 100um wide. On such a board a 10um variance gives you an error of a few percent (several Ohms). As I wrote before, in RF designs you'll typically find traces which are much wider so etching variation does not contribute significantly to impedance errors. For a 1.5mm wide trace, a 10um variation results in an error less than 0.5%. And we're also talking about FR4 here with all it's imperfections where it comes to RF use. So better design a circuit to deal with variations (including moisture, temperature and aging) compared to needing tight manufacturing tolerances.

author: Kasper
author_rank: Frequent Contributor
timestamp: July 07, 2025, 04:05:51 am
content: Quote from: tszaboo on June 30, 2025, 05:45:50 pmI had similiar problem with a trace to a bluetooth chip antenna. I cut out layer 2 in that area and used layer 3 as the reference plane so I could make the trace wider. Didn't get to test thoroughly or tune it but bluetooth did at the far end of my house.

author: tszaboo
author_rank: Super Contributor
timestamp: July 07, 2025, 12:45:40 pm
content: If we are already discussing low cost RF:https://a.aliexpress.com/_EywgSxYI've just ordered a pair of these solderless connectors. I still have to make a PCB for them. The benefits of these types is that the connection point is tiny, so there are less considerations for a microstrip (or other) transitions. And technically these are reusable.I've seen these for 20+ EUR in the past, these are 5. My plan is to test them on a board, and see how well they work compared to a name brand ones. And maybe order a couple.

author: tszaboo
author_rank: Super Contributor
timestamp: August 19, 2025, 10:11:29 am
content: I decided that 2 layer was a bit too much hassle and made my board 4 layer.The design is a so-called rat race coupler. It's a power divider, for a specific frequency, which plays with stripline lengths to divide the incoming signal. It's designed for 2.45 GHz.The schematic is this:I made a simulation using the PCB's substrate. I also created a touchstone model for the SMA connector that I'm using.The simulation is a lot more clear when the connector model is ideal. These are cheap 20 cent connectors that I'm using.Here is the picture of the board. One consideration: Why didn't I leave the RF trace without soldermask? You can see ti on the board, JLC will plate un covered traces with HASL, which probably hurts more than the soldermask.And now the measurement of the board:It matches the simulation quite well. The frequency of it, according to the S11 (not shown) of it is 2.425 GHz, where the design was for 2.45GHz. This is well within the tolerance of the technology, the overall result is quite good. The ideal insertion loss of this RF structure is -3dB, the actual is measured to be -4.4dB. One culprit is the cheap connectors, I'm losing about 0.6dB at this frequency because of that. The other is because of the stackup, the 72 Ohm sections are only 0.18mm wide, there is some losses because of that.

author: tszaboo
author_rank: Super Contributor
timestamp: August 19, 2025, 10:40:06 am
content: It just occurred to me that I didn't take the length of the micrstrip T sections into account when making the layout, so the circular trace on the PCB is 4x0.38mm shorter.6L, the length of that trace is 103.2mm ,and the error is 1.52mm, which would account for the frequency difference...It's also worth posting how an ideal ratrace looks like: