Why and when YOU should be back annotating - Page 1
Forum section: electronics / general

author: VK3DRB
author_rank: Super Contributor
timestamp: December 06, 2018, 12:20:00 pm
content: Hi. I thought I would create this specific discussion, because I have heard engineers say "never back annotate!". I am sharing some tips based on my experience with back annotating.1. What is back annotating.Back annotating allows a designer to set an organised physical location pattern on a PCB layout for designators. Normally you annotate the schematic and then import the design onto your layout. Back annotating imports the logically placed sequential annotations from a PCB layout back onto the schematic.2. Why back annotate?To make life easier for debug technicians and manufacturing staff, as well as the engineer who designed the layout in the first place. In other words, you can find components or test points on the phsyical PCB with ease rather than spending ages trying to find, for example, R23 whichshouldbe near R22 or R24. (And oh, R23 does exist at the other end of the board, but someone hid the designator, just to make your life difficult!)Not back annotating may be a "It's someone else's problem" attitude from some arrogant engineers. Or it is simply due to ignorance on part of the engineer, or the project manager or management who are pushing to get the board out on an unrealistic deadline. Or it is laziness (I have seen a lot of that over the years).3. What to back annotateBack annotate components and test pointsat the appropriate times.4. When to back annotateBack annotate components just prior to the first BOM being released to another department, prior to your detailed design documents are written, or prior to the first external review. If you back annotate after this, your documentation will become almost meaningless. For example, R23 is no longer R23 but R57. You make the call, but make sure all the relevant stakeholders are in agreement. Then lock the component designators in. If you later then add or remover components just annotate them, but leave the rest alone.Most professional PCBs require test points, especially if there is in-circuit testing, or other requirements for manufacturing, testing and debug. Sometimes boundary scan and even AOI can reduce them. I generally aim for 100% test point coverage. Prior to the final design being released to manufacturing (ie: prior to test fixtures being built), the test points can be back annotated. Doing this does NOT affect the BOM. This is very beneficial step. (For non-flying probe ICT, avoid at almost all costs moving test points after the design is released.)Which back annotation algorithm should I use?Whatever is appropriate, depending upon layout. You might want to experiment with each that is available, and choose the one which provides the best solution. There is no hard and fast rule, but for test points particularly, X then Y may be better than than Y then X, or vice versa. Generally try to get Test Point 1 near the datum. With Altium, I think the algorithns are a bit simplistic. Clustering based upon connections might be a better approach.In summaryBack annotation might not impress the chicks, but it might help you win friends in the industry.Anyone else with comments, arguments or would like share ideas about back annotating, go for it!cheers,Dave

author: In Vacuo Veritas
author_rank: Frequent Contributor
timestamp: December 06, 2018, 06:19:15 pm
content: With the advent of cheap ubiquitous computing power and super dense layouts, who cares about back annotating? If someone needs to find R121, just type it in the search box. No one is going to search for a 0201 or 01005 part on the board because someone said it's on grid B3 on the PCB, since there's no silkscreen anymore either...

author: krish2487
author_rank: Frequent Contributor
timestamp: December 07, 2018, 01:14:26 pm
content: 1. Because it is logical to annotate components based on geographical location.2. Because the requisite document may not be available during debugging a board.3. Because you may have a physical printed copy (instead of a digital one) where there is no search bar4. It makes sense when generating physical documentation to handover to PCB turnkey services where they fab and test the boards. (They do charge you for the time they take to hunt down the components)5. If a third party or person tries to debug/service/repair the board then it makes their life easier. They wont have to spend hours find R23 on the diagonal opposite end of a board on the other side from where R22 is.Just my 2 cents.I think the biggest idea to do so - its simply logical and a good practice. Gives a rather consistent approach towards a product design no. If someone cant be bothered to ensure that they take care of small deails, I would not feel confident in their ability to work.Quote from: In Vacuo Veritas onYesterdayat 05:19:15 am

author: Bassman59
author_rank: Super Contributor
timestamp: December 07, 2018, 04:19:12 pm
content: Quote from: VK3DRB on December 06, 2018, 12:20:00 pmWho are those engineers, so I know to not hire them?There is no penalty to performing this geographic re-annotation, and there are all of the significant benefits you listed.Just do it!

author: Bassman59
author_rank: Super Contributor
timestamp: December 07, 2018, 04:19:59 pm
content: Quote from: In Vacuo Veritas on December 06, 2018, 06:19:15 pmThere's a search box on my printed assembly drawing and my printed schematic? AMAZING.

author: Neilm
author_rank: Super Contributor
timestamp: December 07, 2018, 08:10:29 pm
content: I have used OrCad and one thing I have found is if you enter stuff in the constraint manager and don't back annotate, then update the schematic and re-import the netlist you can end up messing up the settings you have in the constraints manager.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 08, 2018, 03:05:33 am
content: Quote from: Bassman59 on December 07, 2018, 04:19:12 pmFWIW --One penalty is the reorganization of hierarchical designs.It is very difficult to keep designators straight while changing the parts within a repeated channel, the number of channels, etc. Outright impossible if pushing a sheet to a different level in the hierarchy.You could spend an entire day matching up the Was-Is list, with a yield of exactly zero productive work. (I speak from experience.)Much easier to push it through, damn the consequences, let hell figure it out.Assemblers and testers have to deal with random data anyway, so it's not going to be a big deal for them. Convenient maybe, but necessary, absolutely not.On that note, I do like to make a print of test point locations -- this isn't automatic in Altium so requires some effort (a bit under an hour). To support a proto build and test session, it's absolutely worth it.Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 08, 2018, 03:07:37 am
content: Quote from: Bassman59 on December 07, 2018, 04:19:59 pmWhy would you print a document with, say, a thousand parts on it, dumping all that useful metadata down the /dev/null?Altium "Smart PDF" for example has properties/fields on components, and complete bookmarks for parts, pins and nets, including cross references.If your problem is not having something handy, don't blame the printer, blame the lack of, say, a tablet computer to access these rich documents on!Tim

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: December 09, 2018, 09:36:42 am
content: I dissagree that annotation should start from physical location. Annotation should be done, in my humble opinion, based on functional blocks - perhaps even starting with a new number as you get to a new block (eg, R10, R11, R12, C10, L10 are for the feedback network of a filter, then jump to R20, R21, L20, C20 for another filter, skipping the numbers between)Since on the practical board, a building block will be layout out close to each other (in the filter example, half of your filters' resistors aren't going to be on the other end of the PCB), and so you get the physical location aspect for free. And on top of that, you can tell by a designator what circuit it is part of easily, without having to look up every part.

author: nctnico
author_rank: Super Contributor
timestamp: December 09, 2018, 06:17:17 pm
content: Quote from: TheUnnamedNewbie on December 09, 2018, 09:36:42 amI agree. If you keep component designators grouped (number ranges) then they will also be grouped on the circuit board. However changing component designators in a schematic will make it harder to change component values. Like change R2 in version 1.0.1 from the 11th of November in 10k Ohm which is now R22 in version1.0.2...

author: ehughes
author_rank: Frequent Contributor
timestamp: January 04, 2019, 02:09:36 pm
content: I have found that grouping of designators happens naturally as parts are grouped/placed by function. Back annotation is rarely needed. Oddball designators usually pop up when you add parts to the schematic towards the end of a layout because of changing requirements, etc. I generally re annotate to clean this up.

author: In Vacuo Veritas
author_rank: Frequent Contributor
timestamp: January 04, 2019, 09:27:56 pm
content: NOTE: This message has been deleted by the forum moderator Simon for being against the forum rules and/or at the discretion of the moderator as being in the best interests of the forum community and the nature of the thread.If you believe this to be in error, please contact the moderator involved.An optional additional explanation is:

author: Mattylad
author_rank: Regular Contributor
timestamp: January 06, 2019, 12:37:06 am
content: If you make a change to the circuit in a PCB, add a component, rename something etc. then it absolutely must be back annotated.The schematic and PCB must match, to not do so is asking for trouble.Even as an end user, coming across a mismatched schematic because the designer has not back annotated his PCB design to the schematic has cause many hours of wasted time and confusion.I can feel the pain Neilm talks about, I have had upset engineers call me up asking for help because they never back annotated then updated the PCB after a schematic change and had the box ticked that matched the attributes - which removed all the attributes they had added in the PCB.While I do not know how to manage back annotation in multiple instance hierarchical schematics (Altium style), if there is a way I would still do it even if it meant a bit of work for me.

author: james_s
author_rank: Super Contributor
timestamp: January 06, 2019, 12:43:58 am
content: Quote from: TheUnnamedNewbie on December 09, 2018, 09:36:42 amThat's how I've always done it, and it's the way I find easiest for troubleshooting as well. If I'm troubleshooting something, I'm often looking at the board and often with no schematic at all. If the annotations are grouped by function it is much easier to identify at a glance parts relating to a specific portion of the circuit. I wouldn't say that I *never* back-annotate, but I rarely find it useful to do so.

author: free_electron
author_rank: Super Contributor
timestamp: January 06, 2019, 05:07:46 pm
content: if a schematic is properly drawn there is no need for back annotation ....if you cram everything on one sheet you end up with spaghetti. if sub blocks have their own sheet and boundaries are set per sheet then parts will be annotated per functional group.

author: mrpackethead
author_rank: Super Contributor
timestamp: January 06, 2019, 06:54:53 pm
content: For the most part, i'm removing annotations from most of the PCB's i design. They just dont' provide any useful function any longer forme or my companyA pnp machine doe'snt need them, and when humans need them, they can just look up teh docs, on any number of screens that are available. This may vary for you and your situations, you need to do what is right for you.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: January 24, 2019, 02:24:11 am
content: Quote from: Bassman59 on December 07, 2018, 04:19:59 pmYou foul dead tree carcasses with ugly smudges?how quaint.