Good examples of assembly documentation for contract manufacturer - Page 1
Forum section: electronics / general

author: abquke
author_rank: Regular Contributor
timestamp: September 06, 2022, 11:25:24 pm
content: So I'm getting prepared to have some boards assembled by a CM for the first time. Up until now, I've never really used the assembly layers/outputs, so can anybody point to some good examples of things that will be of use to the CM and help things go smoothly?

author: Mangozac
author_rank: Frequent Contributor
timestamp: September 07, 2022, 07:09:42 am
content: You would be best to ask the CM for such documents, as different companies will have different preferences.

author: MarkR42
author_rank: Regular Contributor
timestamp: September 07, 2022, 09:13:02 am
content: Of course you will need to send your CM the PCB files (Gerbers) if they are making the PCBs.You will also need to send them a BOM in a format they can understand to buy the right parts (assuming you're not sending the parts)I have generally sent them additionally the following, my CMs did not have a "standard" fixed format,* A pick-n-place position file - with, ideallly, only the components you actually want them to assemble (ignore anything hand-placed later, or any non-BOM items such as test connectors, testpoints, those are just confusing)* A nice human-readable picture with the designators labelled on every component - especially useful if they are too small / close to add the designators on the silk-screen* If you have one, a high resolution photograph of the correctly assembled board (e.g. if you have a hand-assembled prototype).* Alternatively an annotated screenshot from EDA tool.Here are some examples that I sent my CM. They built them correctly. This is a simple, but very small and well packed board that doesn't have any space for component designators.I was trying to make it very difficult for them to do it wrong.

author: SMTech
author_rank: Frequent Contributor
timestamp: September 07, 2022, 11:43:39 am
content: Quote from: MarkR42 on September 07, 2022, 09:13:02 amBOM - make sure it is correct, has complete part numbers (but maybe hash out any part of the part number that specifies its packaging so they can find the stock more easily.Master Sheet - Put your purchasing rules and build notes in a covering document. This could include things like "All resistors specified at 1% or above can be sourced at your discretion, anything below 1% must be our specified part unless otherwise agreed. All Caps 10% or above must match dielectric and voltage ... etc. We have supported pricing on the following lines with this distributor... We find it good practice to work inside the customer BOM in a spreadsheet, so please not HTML (Proteus I'm looking at you) nor PDF.Human readable designators (and clear orientation marks!). Yes the dream is always to have an assembly layer in your gerber set that includes any handy information that they might have to query if you don't supply it. Don't assume the person running SMT or a soldering iron, knows about electronics or wants to spend 20 minutes tracking down a datasheet to identify pin1, they know their process. Annotated images are another solution but seeing as it is capability right there in CAD why not.If you have no-fits, it can be useful to list them as a reassurance. Nobodies process is exactly the same, I typically merge BOM data with pick and place data using a tool called SMT-Maestro or my own script, it needs to be clear which is the authoritative document if the pick and place file also contains component data.Pick and place - our preference is for it to include Fiducial locations as Essemtec ePlace expects that and adding it manually is possible but slower and potentially less accurate. I'd leave in test points, if needs be I can appropriate those as fiducial or badmarks.Gerbers - an assembler is likely to need a copy, Stencil manufacturer may prefer to ignore/check your paste layer by looking at the copper layers too. Also some printers and placement machines can import gerber data with pick and place data for various purposes including setup, alignment, inspection or dispensing.

author: Gribo
author_rank: Frequent Contributor
timestamp: September 08, 2022, 01:16:27 pm
content: Specify all the meta data and special requirements - material: FR4, Rogers etc. Layer stack-up - # of layers, core or prepreg, Dimensions, target IPC specification in the assembly document.For good example, check TI or Analog devices reference boards. You want to minimize the number of questions the assembly house and PCB manufacturer have.

author: Feynman
author_rank: Regular Contributor
timestamp: September 11, 2022, 09:47:15 am
content: Quote from: Mangozac on September 07, 2022, 07:09:42 amI agree. That is probably the first and best thing you can do.Your CM can tell you what information he needs on a BOM, for example. They might even have a template for you.Or they can tell you what needs to be on your assembly drawing. Many CMs will have internal guidelines for assembly drawings (e. g. what colors to use, how to mark Pin 1, etc.) and will somehow convert your assembly drawing to their own guidelines. So it may be a good idea to create your assembly drawing as close to the CM's guidelines as possible in the first place. Since that's their every-day business chances are that the CM's guidelines for assembly drawings are well thought through and you don't have to re-invent the wheel.They can also tell you what additional files they need:- Many CMs love to have a STEP model of your assembled PCB, because the can see at first sight what the challenges of that particular board might be (overhanging parts, special packages, ...)- What to put in your XY-file (and how).- Some CMs like to have "all in one"-data like IPC-2581, because it is easier for them to generate their internal production data.- ...Creating high quality production data can be considered as an art of its own, that already starts in your library.For additional information you can look for conference talks of CMs, for example:(more focused on assembly)https://www.altium.com/live-conference/altiumlive-2017-has-come-close/sessions/creating-documentation-successful-pcb-manufacturing(more focused on PCB production)

author: exmadscientist
author_rank: Frequent Contributor
timestamp: September 11, 2022, 11:00:56 am
content: Quote from: MarkR42 on September 07, 2022, 09:13:02 amThis one is a trap. I have universally gotten the best results when I includeallcomponents in BOMs, pick-and-place files, et cetera, and then mark the parts I don't want as DNP, usually by a column in the BOM (and then sort those to the end). (That means there will be two lines on a BOM for, say, your 0-ohm jumpers: one for the 37 of them you want placed, and one for the 26 you don't.) This way I don't get questions back about "where's R2?" and have to tell them not to place it, wasting a day for the round trip. (Somehow it always works out to waste at least a whole day.) This way they can just see, very clearly, that, yep, there's a spot for R2, and, nope, they're not supposed to put anything there.

author: Feynman
author_rank: Regular Contributor
timestamp: September 11, 2022, 11:29:02 am
content: Yes, I can confirm this: Every CM I ever worked with preferred to have ALL components in assembly related documents (BOM, assembly drawing, pick&place file, ...) and to indicate clearly which of them are "DNI". Unfortunately, the native approach of some ECAD tools is to leave the DNI parts out. It is also a good idea to indicate the mounting technology ("SMT", "THT", "Press-Fit", "BGA", ...).But all that may differ from CM to CM, of course.