Impedence control on FR4 pcb - Page 1
Forum section: electronics / general

author: ppTRN
author_rank: Regular Contributor
timestamp: November 21, 2022, 07:49:37 am
content: Hi, I am working on a project in witch I have a GSM and a GPS antenna, both traces must be matched at 50. I will manufacture the board by JLCPCB, is a 2 layer board, 1mm thick and the traces to the antenna connector have a solid ground plane below and a good clearence around them. Using SaturnPcbToolkit it turns out that I should use a trace width of 2mm! I personally find that weird since i never saw such thick traces to an antenna connector. Do you have any suggestions about this design?PS: what about a matching circuit for the antenna? do you usually include a "R-L-R" circuit or you just connect the antenna connector to the ic pin?Thank you very much.

author: redkitedesign
author_rank: Regular Contributor
timestamp: November 21, 2022, 08:20:21 am
content: I've never done PCB-Antennae myself, but I expect most boards to have more then 2 layers. Thus the distance between the trace and the ground plane will be much less, and the width smaller.I'm not really surprised by the width your getting, although I didn't bother doing a calculation myself. You can try another impedance calculator, there are a gazillion out there, all slightly different.I doubt if you can get reasonable impedance control on a 2 layer JLPCB board, but I've never tried, all my designs that needed impedance control where too complex for a 2 layer board.And on 4-layer boards you can get manufacturer specified geometries for specific impedances, which should work as the manufacturer should have checked it with his PCB-processing.

author: lutkeveld
author_rank: Regular Contributor
timestamp: November 21, 2022, 08:22:35 am
content: That, and is your base copper 9um? Standard PCB technology is often 1 oz (35um)

author: ppTRN
author_rank: Regular Contributor
timestamp: November 21, 2022, 08:30:19 am
content: Thank you for the fast responses. I will take a look to other calulators and compare the resoults. About the geometry of the traces, for such a whide trace i chose to lay down a poligon, resoulting in the immage attached. Should i draw smoother angles or is this acceptable?I found that the base copper thickness has little to no effect in this calculation, i think due to the relatively huge 1mm distance from the trace to the plane, so between 9um and 35um the difference is less than 0.1, so i am neglecting that.ps: in case you wander, the IC is a SIM808.Have a nice day.

author: Tofi
author_rank: Newbie
timestamp: November 21, 2022, 08:36:05 am
content: You first need to contact JLCPCB and ask them for the 2-Layer stack-up for the 1.0mm PCB thickness since it is not mentioned on their website. You would then use the conductor height they provide in the Saturn Calculator. You also need to enter the correct Base Copper Weight and Plating Thickness (typically 35um for standard PCBs on JLCPCB).You would also need to specify which type of transmission line you're using (micro-strip, coplanar.. etc). Check your GPS and GSM modules datasheets for layout recommendations. Once you have that information, make sure to select it in the Saturn Calculator as well.As for controlled impedance stack-ups, I believe JLCPCB and probably most PCB manufacturers only support controlled impedance on 4-Layer+ stack-ups.

author: ppTRN
author_rank: Regular Contributor
timestamp: November 21, 2022, 08:41:28 am
content: Hi, I already contacted jlcpcb and unfortunately they offer no support for 2 layer impedence calculator. About CopperWeight and PlateTickness, they are totally neglectible so I am not even bothering. The transmission line that I am using is a microstrip.Regards

author: Tofi
author_rank: Newbie
timestamp: November 21, 2022, 08:49:32 am
content: They don't have an impedance calculator for 2-Layer boards but they will provide the layer stack-up from which you'll get the correct Conductor Height which actually does make a noticeable difference on the total impedance. I've attached two images with 0.5 and 0.6mm Conductor Heights and you could clearly see the difference.

author: ppTRN
author_rank: Regular Contributor
timestamp: November 21, 2022, 08:59:35 am
content: You were right! I asked them and the correct Conductor Height is 0.91mm and not 1mm. It does change the impedence value, to 44with the 2mm trace width, so i need to adjust that. Thank you very much. Do you have any suggestions about the trace geometry?thanks again

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 21, 2022, 09:06:21 am
content: Why not put the connector directly adjacent to the pads (including pouring ground around, between the nearby GND pads from the module(s), and the connector, with additional vias as well just in case)? With a trace length of nearly zero, the impedance is practically irrelevant.The best solution is no solution at all!Tim

author: Tofi
author_rank: Newbie
timestamp: November 21, 2022, 09:09:43 am
content: No worries!If you want to use a smaller trace width then I'd recommend you use a coplanar configuration and set the appropriate Conductor Gap on your design rules.Check the datasheet of your GSM and GPS modules for the recommended layout and matching network. You would typically find reference designs that you could use as a starting point for your layout.Also look for Hardware Design Document for your modules, they typically have all the information you would typically need.

author: ppTRN
author_rank: Regular Contributor
timestamp: November 21, 2022, 09:17:01 am
content: I surely will. Have a nice day.