Multi Channel Design - Anyone had any experience - Page 1
Forum section: electronics / general

author: snoopy
author_rank: Frequent Contributor
timestamp: August 06, 2017, 03:23:18 am
content: Has anyone layed out a multi-channel design and then flattened the designators by back annotating to the schematic and then tried to add components to the schematic and keep getting messages of duplicate designators etc ?Still to this day I am having nightmares which makes you wonder why they added this feature in the first place if it is so difficult to use

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 06, 2017, 06:20:31 am
content: I prefer to avoid back annotation if possible, for exactly this reason.If you must, then add the part to the schematic, update the PCB to add the component, then rename the new component and back-annotate.All the designators are stored in the .Annotation file. Needless to say, if components or UIDs get confused, things will get out of sync. It's plain text, so if worse comes to worse, you can edit it manually, but it should sort itself out after resetting component links and updating the design.Tim

author: snoopy
author_rank: Frequent Contributor
timestamp: August 07, 2017, 03:10:58 am
content: I just realized I have a situation where some of the component links are broken and for some reason the brain dead thing does not give you the option of linking by unique ID which would solve the problemApparently if you back annotate to many times this can happen

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 07, 2017, 05:45:17 am
content: The links ARE by UID...The single biggest thing that can screw with UIDs is copying a schematic file. The UIDs remain the same, so they get doubled up. You need to reset them on the schematic (T, V, R).And yeah, that's the other big problem: if UID AND designator get out of sync, you're screwed and have to match them manually. (You can match them on the link dialog, or copy and paste UIDs between components and parts.)Tim

author: snoopy
author_rank: Frequent Contributor
timestamp: August 07, 2017, 01:10:06 pm
content: Quote from: T3sl4co1l on August 07, 2017, 05:45:17 amHi TimHere is the problem in a nutshell with one of many examples of duplicate designators after I run the compiler.Code:Logical Designator Physical DesignatorBC110 --> ???? (Should be BC25 because of the same unique id)BC90 --> BC110How to get BC110 on the schematic to link with BC25 by matching up the unique ids and then push back to the schematic so these errors no longer appear ?RegardsDavid

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 07, 2017, 03:49:56 pm
content: Go to PCB view, select Project / Component Links. Find BC110 in the SCH list, BC25 in the PCB list, and hit the ">" button. (Or, if these have already been linked with other parts, find them in the right-side pairs list and press the "<" button, then do the above.)Tim

author: snoopy
author_rank: Frequent Contributor
timestamp: August 08, 2017, 01:39:21 am
content: Quote from: T3sl4co1l on August 07, 2017, 03:49:56 pmHi TimI did all of that and pushed it back to the schematic but it does not work ! Still get the duplicate designatorscheers

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 08, 2017, 07:21:53 am
content: Huh, so is that a schematic compile warning?Because the compiler doesn't take account of the annotation file. If you have e.g. R10 in a channel that's numbered $ComponentPrefix$ChannelIndex$ComponentIndex (so its instances will be named "R110", "R210", etc.), and you have R110 elsewhere in the schematic, then the schematic annotation won't detect any issues (because there is only one part with logical name "R110"), but the compiler will emit a warning, because there are multiple physical parts (R110 by name, and "R110" from channel 1, "R210" from channel 2, etc.).That is an issue if you are doing simulations (the compiled designators are used for simulation). It doesn't matter on the PCB, because the PCB does use the annotation file.At least, I think that's what it does. Again, good reasons to avoid using confusing names and back annotation...Tim

author: snoopy
author_rank: Frequent Contributor
timestamp: August 08, 2017, 02:16:40 pm
content: Quote from: T3sl4co1l on August 08, 2017, 07:21:53 amIt makes it awkward to add new components when it is in a pickle like this. I have tried everything anyone can suggest but nothing seems to be able to fix it except I have found a convoluted way of fixing it which I will document here to help anyone else.Run the compiler and click on one of the duplicate errors. You will see details in the dialog box below the messages. It will look something like this:-BC110BC110 (C90)Double click on the one without the associated physical designator in brackets because this is the component that has lost its physical designator. Now double click on the component and copy its UID to the clipboard. Now find the UID in the .annotation file. Below this entry is the physical designator that it should be linked to (for example BC52) but for some reason Altium is to brain dead to offer component linking by UIDNow replace the logical designator (BC110) with the physical designator BC52. Recompile and note the error disappears. Also cross probe the component on the schematic to make sure it matches up with the correct part on the board.Now repeat for all of the other duplicate errorsI'm sure there must be some hidden undocumented feature that makes this is easy but I could not find it ! It seems to be an issue with multi channel design implementation.Moral of the story is don't back annotate a multi channel design unless you are well and truly sure it is finished and you do not want to change anything !!cheersdavid

author: ludzinc
author_rank: Unknown
timestamp: August 08, 2017, 09:13:15 pm
content: Can be tricky to get right.Here's the reminder I write for myself:http://ludzinc.blogspot.com.au/2014/08/altium-multichannel.html?m=1

author: snoopy
author_rank: Frequent Contributor
timestamp: August 09, 2017, 02:25:36 am
content: Quote from: ludzinc on August 08, 2017, 09:13:15 pmGood docoOn your example can you try adding a resistor on the top level schematic and then run the annotator ? What is the annotation for the new resistor ? When I tried to do it on my own designs it would designate the resistor as R2 instead of R5 as it should be as though it does not understand the new re-annotated parts !! Therefore when you run the compiler you get duplicate designators errorPerhaps they have changed it in version 17 because I haven't been able to test it because of these duplicate component errors which I am working through at the moment !!