Two designators on the one component - WTF !!

[snoopy]

This driving me nuts but I don't think I am the only one with this issue.

After re-annotating a PCB and pushing the annotation back to the PCB (Update Schematics) the components in the schematic have two designators on each component. The smaller greyed out designator in parenthesis match the PCB but the normal designator that gets printed out, are all over the shop and have nothing to do with the physical designators on the boards. I have found a few others who have had the same problems but nothing is working for me to get the main designators to match the physical PCB designators. I really don't want a schematic drawing not to match the PCB drawing. That is totally brain dead !!

Here are some links I have looked at to try and solve this problem but nothing is working. What is the deal with this concept ?

http://www.dutchforce.com/~eforum/index.php?s=2403b817fbd03ab1a68bf2413a2835c5&showtopic=32521

https://gruending.net/2011/01/altium-designer-backwards-annotation-hell/

http://ludzinc.blogspot.com.au/2014/08/altium-multichannel.html

[Psi]

you could try  'annotate the schematic' from the tools menu.
It relabels all your designators so they are consecutive R1 R2 R3 etc.. and so numbers close together are physically close together.

It might fix your issue (or it might make it worse hehe )

[snoopy]

I think it is something to do with the ability to edit the PCB designators from the schematic according to this short video.



But I can't see how it helps my situation.

[T3sl4co1l]

Funny, it's 4 years later and my opinion is still the same (ref DutchForce thread).

The second (Grundig) link sounds good, but, in addition I would suspect mismatches with component links (open PCB file -- Project/Component Links).  As far as I know, forwards and backwards annotation should always give the correct results, including renaming component designators.  Because they are supposed to be matched by UID, rather than designator.  If those aren't matched correctly, then you'll get the shit being fucked up with.

I've seen the same problem, from time to time, in Multisim/Ultiboard; I don't know how they keep those things straight, if there's a hidden UID or if it painstakingly tracks manual changes, or matches parts by netlist, or what.  Sometimes you can rename components and the ECO will be simple, other times it says, "oh shit no son, you done fucked everything up, delete that old shit here's some replacements".

I imagine other tools (KiCAD, Eagle, Diptrace, ) have similar problems.  Seems like one of those things that either has no reasonable solution, or that never ever gets programmed right, from the start.

Tim

[snoopy]

Funny, it's 4 years later and my opinion is still the same (ref DutchForce thread).

The second (Grundig) link sounds good, but, in addition I would suspect mismatches with component links (open PCB file -- Project/Component Links).  As far as I know, forwards and backwards annotation should always give the correct results, including renaming component designators.  Because they are supposed to be matched by UID, rather than designator.  If those aren't matched correctly, then you'll get the shit being fucked up with.

I've seen the same problem, from time to time, in Multisim/Ultiboard; I don't know how they keep those things straight, if there's a hidden UID or if it painstakingly tracks manual changes, or matches parts by netlist, or what.  Sometimes you can rename components and the ECO will be simple, other times it says, "oh shit no son, you done fucked everything up, delete that old shit here's some replacements".

I imagine other tools (KiCAD, Eagle, Diptrace, ) have similar problems.  Seems like one of those things that either has no reasonable solution, or that never ever gets programmed right, from the start.

Tim

All of the components on the schematic match up with the pcb so there are no errors on update and the component links are all correct.

Here is what I see on the schematic for example. The designator in parenthesis is what matches up with the PCB designator but the actual designator (in blue) on the schematic could be anything. The problem is the blue designator is what gets printed out.

I assume there is some method in their madeess but I can't see it myself yet.

cheers

[snoopy]

OK I think I may have egg on my fdace on this 

I just checked the print preview and guess what ? It is the greyed out parenthesised (physical) designators on the schematic which get printed out and not the logcal designators in blue 

cheers

[DerekG]

I imagine other tools (KiCAD, Eagle, Diptrace, ) have similar problems.  Seems like one of those things that either has no reasonable solution, or that never ever gets programmed right, from the start.

Tim

DipTrace have sorted it out just fine. You have the choice to update from the Schematic by either the Component itself or the Reference designator.

If you accidentally choose the wrong one, a single "undo" will take you back to where you were.

[Rufus]

This driving me nuts but I don't think I am the only one with this issue.

It is showing you current and new designators (or current and old?) and will until you next compile the project.

[Araho]

As far as I know, the greyed out designators are the old designators. This is so that you can see what changes were made when you run Tools -> Annotate Schematics. ( To prove this, add any component, say a resistor. It will be designated as R?. Then run Annotate schematics, and you will see that what was previosly R? is now R1, with (R?) in grey behind it.)

When you compile your project, the greyed out portion disappears. (I tested this just now.)

The PCB is not changed until you do a Design -> Update PCB Document or Design -> Import Changes From [...].


This all sums up to one thing: Compile your project BEFORE updating the PCB. Makes everything easier.

[free_electron]

The greyed out ones are the old designators pre-annotation.
those will not be printed , they are for visual reference only.
They disappear after compilation or after a design update to pcb at which point integrity check is done

altium does not use the designators to perform the link between schematic and pcb. The links are made using the GUID of the components. whenever you place a part it is assigned a project wide unique id. ( 6 character alphanumerical code ). that is how the linking works.

never ,i repeat: NEVER , mess with those UId's

you can change designators without problems , Altium will be able to track what happened.

the best way to do an annotation is to first
- reset duplicates
then
- annotate all

it will leave the annotated parts alone and only update duplicates and new ones.

[snoopy]

Maybe part of the problem is that I am using some multi channel design and the roles of the smaller greyish designators are different.

Having said that I have re-annotated the board in the PCB editor and pushed the changes back to the schematic. Also the extra step as outlined by ludzinc was needed to flatten the designators ( http://ludzinc.blogspot.com.au/2014/08/altium-multichannel.html ). Now everything is syncronized but the smallish greyed out (physical) designators are the ones that match the PCB and get printed out which is what you would expect. Now the normal blue-ish larger (logical) designators usually don't match on my schematic. So I can live with that. Even the print preview shows the physical PCB deignators and not the logical ones. OK so far so good except I would like the larger blue-ish designators to match the pcb designators. Is there a command to do that ? What am I missing here ? The Altium doco is not really clear in this respect.

Similar problem here http://www.dutchforce.com/~eforum/index.php?s=2403b817fbd03ab1a68bf2413a2835c5&showtopic=32521

Anyway here is a another problem. When I go to add new components and re-annotate on the schematic the compiler shows an error because it says those designators are already in use !! Found another dude with a similar problem  http://www.edaboard.com/thread180776.html

When you see a shadow designator as pictured, you are looking at one of two things: 1. the previous value of that component, which goes away on compile time (Project / Compile PCB Project); 2. when using a multichannel (hierarchical) design, after compilation, this lists the physical designators which that symbol maps to. (In a multichannel design, you can repeat schematics multiple times, so that one symbol can be used for, say, left and right in an amplifier, bits 0-7 in a data bus, etc.)

From what I can make out the solution is to make the larger blueish (logical) designators the same as the smaller greyed (physical) designators the same but how to do this ?

cheers

[snoopy]

I think the key for Multichannel design is that you have to use "Board Level Annotation" and not the standard "Annotate Schematics". In this case the greyed out designators represent the physical pcb designators and the standard blue designators represent the logical designators. The two should not be confused. Seems to be working using the following procedures:-

Reset all of the designators and then re-annoated using Tools -> Board Level Annotation -> Reset All -> Accept Changes

Then go Project -> Compile PCB Project

Push the changes onto the PCB using Design -> Update PCB

Re-annotate PCB using Tools -> Re-Annotate

Push the changes onto the schematic using Design -> Update Schematics

Also to set the print ordering change the ordering using Tools -> Annotate Compiles Sheets

cheers