JLCPCB impedance calculator - wildly wrong? - Page 1
Forum section: electronics / projects

author: davegravy
author_rank: Regular Contributor
timestamp: October 30, 2024, 11:07:32 pm
content: I used theJLCPCB calculatorto determine coplanar waveguide for a 50 ohm impedance trace on their JLC04161H-7628 stackup. This gave me 13mil trace width for 13.4mil gap.Then I sawthis articlewhere the author determines to use 13mil trace width and 6mil gap (for the same stackup), less than half the gap.I tried some online calculators usingJLC's published parametersand they line up with Rob's results.I've read advice that one should trust the manufacturer over calculators, but since Rob measured his, and since this is JLCPCB (low cost) I'm not so sure. I don't have access to measurement equipment else I'd build some coupons, so I'm trying to make the most educated guess I can.I realize Rob wasn't varying the trace design, he was varying the pad transition, but is it unreasonable to assume he would have commented if there was unreasonable loss from the trace (present in all the tests)?

author: radar_macgyver
author_rank: Frequent Contributor
timestamp: October 31, 2024, 12:28:34 am
content: Note that the linked article states that the trace width and gap were from another project that targeted the OSHPark stackup and that the author felt the JLC one was 'close enough'.I've used the JLC0416H-7628 stackup on a couple of boards for which I used a 13.6 mil trace width, with 20 mil gap. This design was from Genesys TLINE, and the same was true for the one built into Altium Designer. I could verify that the traces had a good match out to 3 GHz.For a 6 mil gap, TLINE shows a trace width of 11.3 mil, while JLC's calculator has 10.4 mil. TLINE does not add the effects of the soldermask, so that may explain the discrepancy. Are the online calculators computing agroundedcoplanar waveguide? Several exist for CPW without a ground plane. GCPW is a weird combination of stripline and CPW.

author: HwAoRrDk
author_rank: Super Contributor
timestamp: October 31, 2024, 09:43:42 am
content: I have in the past compared the results from JLCPCB's calculator and Saturn PCB Toolkit, and they were near enough the same - only rounding differences.

author: tszaboo
author_rank: Super Contributor
timestamp: October 31, 2024, 10:02:28 am
content: https://github.com/tszaboo/RF_SPLITTER_V2/tree/mainI made an RF splitter some time ago. Used their calculator to set up the trace width. You will find the stackup, and VNA measurements in the project folder. They are PNG pictures, you don't need Altium to view those. VSWR is ~1.25 up to 4GHz. It depends what you are trying to do, for me 0.05dB loss is acceptable.My trace width is 0.6mm and gap is 0.175mm. Which is half a banana and 3/16th of a pound in imperial.There are multiple correct width and gap values for CPW.

author: Randy222
author_rank: Frequent Contributor
timestamp: October 31, 2024, 02:17:10 pm
content: There's about 1mil tools to use, paid for and free.What does KiCAD --> Calculator Tools --> High Speed --> Transmission Lines say?Try taking a design into Sonnet Lite amd analyze it, does Sonnet show results that has expectations from the other trace tools?

author: davegravy
author_rank: Regular Contributor
timestamp: October 31, 2024, 08:15:29 pm
content: Quote from: Randy222 on October 31, 2024, 02:17:10 pmI've tried a few of them, per my first post.Quote from: Randy222 on October 31, 2024, 02:17:10 pmGives results similar to the others I've tried, ie calculates a much smaller gap than JLCPCB does.I'll try Sonnet.