JLPCB - Gerber Format/Precision? - Page 1
Forum section: electronics / general

author: Uky
author_rank: Regular Contributor
timestamp: February 17, 2025, 08:39:04 pm
content: I was going to submit a small job to JLPCB but it seems the site has changedsince last time.The suggested layer names are there, but the required (or accepted) unit of measure andprecision was nowhere to be found.I have for years used (RS274X) metric units (mm) with various number of leading/trailing precision.Not wanting to run into problems, I have been looking for JLPCB's format requirementsother than file name conventions.A link?Someone?

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: February 17, 2025, 08:55:02 pm
content: Just upload it and look at the preview

author: SiliconWizard
author_rank: Super Contributor
timestamp: February 18, 2025, 12:41:25 am
content: I use 4.6 (mm) for all my PCBs. JLCPCB takes it with no issues. I see little reason to use less than 4.6 these days.

author: Uky
author_rank: Regular Contributor
timestamp: February 24, 2025, 02:47:04 pm
content: My tool recommends using one trailing digit more than the design itselfso metric "4.3" it was and JLPCB accepted it w/o any problem.

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: February 24, 2025, 04:11:37 pm
content: Ask them on their chat.The buggers have a habit of changing things.I used their recommended file extensions for years then I suddenly got a pcb back with solder resist layers reversed !They had changed recommended file extensions.I had to go into my gerber files and change the extensions to fit their new way of doing things.

author: Uky
author_rank: Regular Contributor
timestamp: February 24, 2025, 09:39:21 pm
content: The extension naming conventions had not changed since last time.And judging from their pre-viewer, all layers were correct.My system (Cadence) produces artwork files based upon classes and subclasses definitionsset up when starting a new board based on a default template (that can be changed).Default extension is "ART" but can be changed to anything. There are also .IL- scripts written that willrename the layer according to GKO, GTO, etc or whatever JLPCB requires but since I seldomorder PCB's for my own personal use I can live with this extra work. I always use aseparate gerber viewer anyway (view-mate) to verify that the layers and their content(s)are named correctly regardless of who will manufacture the boards.the professional customers I am work for uses other sourcesfor their boards, none of which requires naming conventions like JLPCB.Thank G*d for that...

author: tycz
author_rank: Regular Contributor
timestamp: February 25, 2025, 10:31:03 pm
content: Quote from: SiliconWizard on February 18, 2025, 12:41:25 amI think that's supported by the cam software only because more digits after the decimal is required for imperial gerbers. 4.4 in metric is roughly equivalent to 2.6 in imperial.As an aside, somebody submitted a bug report to me that drill files generated by PCB Elegance don't show up properly in Ucamco's gerber viewer. It turns out that it relies on some non-standard (not in their own standard!) Altium addition that specifies the number format within the NC drill file. If it doesn't find this, it just assumes it's 3.3 without any way to input this manually. This seemed a bit silly, but then I looked up the capabilities of the most precise PCB manufactures I could find, and the best tolerance seems to be +/- 8um. That's not changed much in the past couple of decades either. 3.3 (metric) is only a problem when you need boards that are over a metre long.Quote from: nigelwright7557 on February 24, 2025, 04:11:37 pmI never use these cryptic three letter file extensions for gerbers. They are another Altium/Protel invention from the 8.3 dos file name days. Too confusing and I can never remember the order of the inner layers (do they increase or decrease from to bottom?). All the Chinese factories I've dealt with (including JLC) have accepted my gerbers with plain English file names and a .ger/.gbr extension without any complaint or problem.

author: HwAoRrDk
author_rank: Super Contributor
timestamp: February 26, 2025, 03:16:03 am
content: Quote from: tycz on February 25, 2025, 10:31:03 pmMe neither. I just name all my files with a .gbr extension. Have done for years.However, that's because my design software produces Gerber files that contain metadata attributes that includes info that specifies what layer each file is. There is a 'FileFunction' attribute defined in the standard specifically for this purpose.If you open your Gerber files in a text editor and they contain a line like the following, you're golden:%TF.FileFunction,Copper,L1,Top*%I believe if such a line is present, JLCPCB's CAM software ignores anything else. Although I still include the layer name in the filename for my own sake.

author: ahsrabrifat
author_rank: Regular Contributor
timestamp: March 02, 2025, 05:41:28 am
content: Quote from: Uky on February 17, 2025, 08:39:04 pmJLCPCB recommends using the Gerber RS-274X format for PCB design submissions. This format inherently supports metric units (mm), aligning with your current practice.You can find some information in their docs.https://jlcpcb.com/help/article/how-to-generate-gerber-files-in-different-softwarehttps://jlcpcb.com/help/catalog/180-PCB-Files-PreparationIt's advisable to use standard precision settings that are commonly accepted in the industry. Here is an elaborated blog regarding gerber file generation. All things like Configuration Parameters, Aperture Definitions, XY Coordinates, Draw and Flash Commands have been discussed in detail. Hope you will find it helpful.https://www.allpcb.com/blog/pcb-design/what-are-gerber-files.html

author: Uky
author_rank: Regular Contributor
timestamp: March 02, 2025, 09:06:24 pm
content: Used 274X, metric format 4.3JLPCB accepted it and the boards arrived only a few days later.