Changing Reference Designators on SCH without Disturbing Existing PCB Layout? - Page 1
Forum section: electronics / general

author: TimNJ
author_rank: Super Contributor
timestamp: November 18, 2023, 02:06:01 pm
content: Greetings,Supposing I have a PCB that’s already laid out and essentially final, and I want to go back and change only the reference designators of a number of parts, what’s the best way to do this?I want all of the components on the PCB to stay exactly where they are, and only the silkscreen reference designators to change.In my 5+ years of using Altium, you would think I would’ve ran into this situation before. But, when I try simply swapping ref des (e.g. R1 -> R2; R2 -> R1) or changing a ref des to a brand new name (e.g. R1 -> R99), then update PCB from schematic, the PCB gets totally messed up. PCB becomes a rat’s nest of connections. For a pair of ref des swapped on the schematic, I would need to exchange the XY positions of R1 and R2 on the PCB to fix it. For a new ref des, the old component (R1) is deleted from the board and a new component (R99) is placed outside the board outline.I just want the ref designator silkscreen text to change. What do I do?As far as I can tell, the Unique IDs are all locked, so I thought this would be enough. But apparently I am wrong.Using AD14.Thanks,Tim

author: Psi
author_rank: Super Contributor
timestamp: November 18, 2023, 02:15:37 pm
content: Before changing anything, confirm thatA) When you go to the SCH and update the PCB from Schematic it says there's nothing to change / no changesB) When you go to the PCB and check project component links everything is linked with nothing unmatched.Sometimes in older versions of altium I have noticed it can get confused if you do A-B and B-A together and then try to update PCB.So, instead, you introduce a temp name, eg do A-C the update, then B-A and update, then C-B and update.

author: TimNJ
author_rank: Super Contributor
timestamp: November 18, 2023, 03:50:32 pm
content: Quote from: Psi on November 18, 2023, 02:15:37 pmThank you. I’ll have to check component links from the PCB side.I’ve also tried A->C and then C->B, but if C is a new ref des to the project, it removes A from the PCB and plops down C as a new component, outside the board outline.I ultimately want to rename all ref designators, which I tried to do via annotations. Cleared all and had it automatically annotate the schematic. Then pushed to the PCB, but same issue as I originally noted. It’s almost like the Unique ID is also being swapped from A->B and vice versa? Then I Ctrl-Z’d on the schematic and PCB to revert to original designators, then tried to re-sync SCH to PCB to confirm alignment. This was a royal mistake apparently. Could not get them to sync even though visually all of the ref des on schematic and PCB were indeed matched. Had to recover from local version history.But anyway, usually the problem exists between keyboard and the chair…so if there’s fatal error I’m making, I’d be curious to know.

author: PlainName
author_rank: Super Contributor
timestamp: November 18, 2023, 05:47:08 pm
content: Had similar with Circuit Studio:https://www.eevblog.com/forum/circuit-studio/re-annotate/

author: TimNJ
author_rank: Super Contributor
timestamp: November 19, 2023, 04:52:14 am
content: Quote from: PlainName on November 18, 2023, 05:47:08 pmThank you. A lot of good ideas there to try/consider.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 19, 2023, 08:43:21 am
content: Yeah sounds like the links aren't right. Always check links (C, K) before pushing updates.Without links, it's inferring them directly from designators, so of course, if you swap them around, it doesn't know anything better to do, and you get what you asked for, but not what you thought you were doing.Links are scrambled by placing, copy-pasting / pushing, even choosing a new Design Item ID (library reference part) (but not Update From Libraries, maybe, at least if there's no change seemingly..?), and you need to re-link them before changing designators. (Curiously, it can say links are off, even though the values still match on both sides. Unless that's a quirk of the design I'm testing just at this instant?) Most common pitfall (after skipping links entirely) is doing too many changes at once (i.e. one or more of these plus designator change) and things get scrambled again.And yeah, it's a scuffed system.. it's designed to improve on a "traditional" method (say, purely matching designators in a netlist transfer mechanism) I think, but it still requires manual oversight. Basically it's replacing Designators with another, even more fragile, and less visible, system of designators. And it fails silently -- you can keep on working while letting it guess what you mean, until such time as you push it too far and the seemingly-functional facade falls face down.My regular incantations / paranoia are:C, K (Project / Component Links)D, I (Design / Import Changes)T, G, A (Tools / Polygon Pours / Repour All; I think I custom-configured this bind but whatever works to repour them)T, D, R (Tools / Design Rule Check, Run)Poly auto-repour isn't bad (at least since... AD15 or so?), but it's quickly bothersome in larger designs, and I've long been in the habit of manual repour so I don't use it. Likewise design rules, I have online checking disabled, I'm good enough to eyeball most of them, and then clean up rules later to suit what I've actually built and adjust what still doesn't match after that.Tim

author: TimNJ
author_rank: Super Contributor
timestamp: November 20, 2023, 05:01:08 pm
content: Quote from: T3sl4co1l on November 19, 2023, 08:43:21 amThanks! It was indeed the links, which I frankly do not understand the meaning of. There are separated Unique IDs on the PCB and schematic side? And those IDs need to be linked?Without exhausting too much brain power thinking about it, hitting "C, K" is easy enough, and I'll definitely add that to the list.Polygon pours certainly terrify me. I almost never repour out of fear that the order will get messed up. I usually do not find it worth it to "back calculate" the correct pour order to get an output which matches how it currently looks. Maybe for the more complicated board I'm working on, I'll spend the time...

author: thm_w
author_rank: Super Contributor
timestamp: November 20, 2023, 09:40:25 pm
content: Quote from: TimNJ on November 20, 2023, 05:01:08 pmWhen you place a component on the schematic it generates an ID, when you initially push it to the PCB it copies the same ID.https://www.altium.com/documentation/altium-circuitmaker/component-linksQuoteI would figure this out on a simple design where it is much easier to do. It will come back to bite you at some point.Setting up a pour order is not so difficult.https://www.altium.com/documentation/altium-designer/pcb-dlg-polygonmanagerformpolygon-pour-manager-ad?version=22

author: JohnG
author_rank: Frequent Contributor
timestamp: November 21, 2023, 02:08:20 am
content: Quote from: TimNJ on November 20, 2023, 05:01:08 pmIf you really want to be absolutely terrified by polygon pours, wait until you are forced into a position where you need to repour them, and watch many, many, many hours of work go down the drain. BTDT.I suggest learning to use the polygon manager to reorder polygons and then either repour automatically or do it manually, and often, i.e. like every time you change some polygons. Then you will get used to it working, and you are likely to find that once you are used to it, you spend a lot less time tweaking a lot fewer polygons, and you will be comfortable changing existing polygons without fear of blowing up your design through a polygon misstep.Just my $0.02, the value of which is approaching subatomic particles...John

author: TimNJ
author_rank: Super Contributor
timestamp: November 21, 2023, 03:38:47 am
content: When I said they terrify me, that’s of course due to my own laziness and not using the polygon manager properly. Current project has 200 polygons and it will probably take me like 4 hours to get them all in the right order. I wish there was a way to take a snapshot of the current polygons and automatically convert that into the corresponding required pour order.

author: JohnG
author_rank: Frequent Contributor
timestamp: November 21, 2023, 04:05:15 am
content: FWIW, the first time I got stuck with such a situation, I had a little over half the number of polygons, maybe 120 or so, and it did take a few hours to get them in the right order. After that, by redoing the polygons and using pour order, I was able to reduce the number of polygons to < 30. Since that time, I have found it much easier to keep the number of polygons down because I no longer need to keep fixing things by drawing more and more polygons. Instead, I have found that I can very often get the same thing by editing existing polygons and repouring. Faster, much easier to manage and I have never looked back.If you start on a new board, it might be easier. In my case, I was handed a board with problems from an employee who had left, and needed to update it. I couldn't make head or tail out of it because it was a mess of polygons overlapping, and I ended up repouring the polygons. At first, I thought I had made a huge mistake by doing so, but it turned out to be one of the best things I ever did. It made every layout since go much smoother.John