Altium MultiChannel

Multi-Channel Rules

Just recently I was reading this post on the EEVBlog forum and thought "Ah ha!  I've done this before." Should be easy.  Famous last words.

So after spending a ridiculous amount of time workign out what the missing step was, I thought I'd better capture it for the next time I want to use it.

WHY MULTI-CHANNEL

You use a multi-channel design in Altium when you have multiples of an identical sub-circuit.  QAll you need to do is lay out the one channel, and then you can duplicate the layout by 'Copy Room Formats".  This has saved me a ton of time in the past.

THE PROBLEM

Altium uses a complex naming convention:

Where the use of $Component$RoomName results in very long strings for component names:

So I prefer to use $Component$ChannelAlpha

Which results in a more human readable format like below:

Nifty!

As an aside, to set up a multichannel design in Altium, it's simply a case of having a top level schematic call a  low level schematic - like below.  I wont go into detail here because Altium's documentation on this topic is quite good!

You will notice in the sub-sheet R1 show that subsequent channels will use R1A etc as the numbering format (the water mark text).

However, if you prefer a more tradition number convention, you can go to your PCB design, select Re-Annotate and get a more traditional number scheme.

Again, Altiums's own documentation details this.  It even goes on the mention that you can push these changes to your schematic, and if you are not using a multi-channel design, it's fine.

BUT:  For a standard multi-channel design, it doesn't work.  Grrr!

The ECO is generated and it looks like the change is pushed to the schematic, but it doesn't 'stick'.  And this drove me nuts as I remembered that I got it to work once in the past, and I double checked by opening my old design and it confirmed that it could be done.

I'll spare you the pain of how I *finally* worked it out the missing step, instead I'll just jump to the chase:

In your schematic, select Tools - Annotate Compiled Sheets.  This gives each sheet a unique number in Altium and this is required to make the back annotation work.

In the PCB, push the changes to the schematic (Design - Update Schematics), return to your schematic, Recompile it (right click on the project name, select Recompile) and you're done.  Your multichannel schematic now shows the designators labelled as per your PCB.

WOOT!

Anyway, here's hoping anyone finds this useful.  At the very least, it's now written down here for me for the next time I forget!