Annotation in Altium Designer

[nikhil2402]

Hello Everybody,

In my project I have a specific requirement that the components be annotated in a certain manner.

Example : U702 - > here the first digit(7 in this case) would always refer to the page the component is located and the next digits (02 in this case) would refer to the component number in that schematic page. Here this particular component is located in page 7 and is the 2nd component in that page.

Is there a way to do this in Altium?

Thanks
Nikhil

[mairomaster]

I don't know about an automated way to do it, it is quite unique requirement that you have. You might need to do it manually, but it could be quite cumbersome like that, if you have a complicated project.

[robertferanec]

This may be what you are looking for (Tools -> Annotate Schematics -> Designator Index Control -> Start Index):

[mairomaster]

Alright, good idea Robert. I knew about the feature, but didn't really think that you can set up a different starting index for each sheet.

[robertferanec]

I used it once

But don't use it anymore as for complicated boards it's causing problems e.g. many times we want to keep original designators (from reference or previous designs) because then placement can be easily re-used. Also, when we keep updating schematic and PCB, continuous changes in reference designators could delay the design process and could possibly cause mistakes (you have to be sure the designators were correctly assigned to already placed components - and I try to eliminate this kind of unnecessary erros)

[nikhil2402]

Hello Everybody,

Thanks for the above suggestion Robert and Mariomaster. Robert I think the trick you suggested is what I was looking for. Its working as expected for my project.

Robert you said that you dont use this anymore. I am curious know what method you use for annotating schematics then ?

[robertferanec]

No special method
Every new component is marked with "?" and then only the components with "?" are annotated. Once a reference designator is assigned to a component, we don't change it.

[abarnai]

Hi robertferanec , this is another big 'flaw' in Altium Designer the way I see it, if you cannot change the reference designators to any arbitrary values in a design, by importing the information from an outside source file. (What it was, and what you want it to be for each component.) Or can you? If you could, that would make my day...

Theoretically you could do it using Delphi scripting, but Altium R&D doesn't seem to have updated the scripting API since Altium 6 as far as I could find out. You can do scripting, I tried it myself, it just doesn't work. We do have this requirement most of the time a board is hand-assembled and the way I attempted it is that I use a PADS Layout version to come up with the changes, then I copy-paste the table in sections to PCB List reference designators and then match up schematics to PCB in Altium. Sometimes it works, especially if there are not a lot of parts...

If I want it to work for sure, I do it in PADS Layout, but then it is a nightmare to match up the schematics... Luckily most of these PCBs have OrCAD schematics, and this is not a problem with
OrCAD.

[mairomaster]

I am not exactly sure what you are trying to do, but you can try the following.

Use the schematic filter to select all components in the project with the query 'IsPart'. Then use the schematic list window to copy and paste the whole designator column in excel. In excel you can do whatever you want with the designators, I am sure there are plenty of pluggins/addons/scripts/macros for excel that could be useful for the particular task. After you finish editing them, copy and paste the whole column back into altium (you will need to switch the schematic list to editing mode).

I always use Tools -> Annotate Schematics to work with my designators and find this sufficient, it is reasonably powerful for most of the tasks.

[abarnai]

I just did what you said. I modified all the resistors in Excel, added 100+ to the reference designators just to test, selected all components in the design with IsPart with the SCH filter.
When I select the ref des column in the SCH list, with all Ref Des selected, the paste will not work. It will switch over to the schematics editor panel by itself, even though SCH list was selected, and will paste a partial column into the schematics. As you see when I paste to Notepad it will work fine, from Excel. So Altium truncates the clipboard contents to whatever seems to fit in memory in their way of handling the clipboard and then pastes it into the SCH editor as a partial column, even though the SCH list is selected. Note that the SCH List is in the Edit mode, still it will not be edited.

Does it work for you any differently? (I am using Altium version 13.3) See screenshots.

[abarnai]

mairomaster Why am I trying to do this? Because our boards are laid out such that the components are in clusters of functionality, not necessarily laid out in a linear geometric pattern Altium
wants to annotate the parts.It makes troubleshooting / reading the schematics way easier.

[mairomaster]

Hmm it works perfectly with me. It might be because of the older version of Altium, I am using 16.1.

[abarnai]

I have been hesitant to try 16, because I dislike some of their changes plus I don't trust them necessarily that the newer version is necessarily any better, based on some experience. I will send my boss the Excel file and the project zip file and ask him to do it in 16.1 that he has and I will watch or do it myself. I will let you know.

[robertferanec]

abarnai, please let us know then if it worked with AD16

[abarnai]

robertferanec It works with AD16. There is a catch: You have to use Ctrl +V instead of ->Paste from the menu. They never fixed that. Probably it is something it picks up from Windows. Also, they do not truncate the list at a few dozen parts as they do with older AD13 and AD14. At least they changed to the right data type in their program so now it can hold a few hundred string types instead of a couple of dozen like before.