Electronics > Altium Designer

Do "Device Sheets" help with PCB planning - or is this a schematic-only concept?

(1/3) > >>

I've been asked to design some equipment where there are 3 indentical channels (each channel itself has mutiple connectors plus analog inputs and outputs and its own dedicated RS232 interface).

I'd like to use the "Device Sheet" concept, as it seems an ideal use-case.

I was wondering what (if any) difference my organising the schematics this way would make to PCB layout.

Basically, once I've laid out 1 channel the other two channels would have the same layout. Note though all channels go onto 1 PCB and share a power rail.

Is there any way that, once I've laid out 1 channel (one Device Sheet Instance), I can import and lay out the tracks etc for the other 2 channels whilst 'leveraging' the 1st channel's layout?

Yes, you can duplicate layouts like this, but device sheets are not required.  This is basically the one situation where rooms are worth using, and it works with regular sheet symbols in regular multichannel designs.  Device sheets are more for reusing schematic sheets across multiple designs.  I imagine they *can* be used here, but don't HAVE to be. 

When you have three instances of the device sheet and allow Altium to automatically generate class and rooms you can lay out one of the channels in its room, and then copy the routing and component placement from that room to the others.  This is kind of clunky, and has some traps, but it's meant to do exactly what you're looking for here.  Make sure to lay out the first room in isolation, as any tracks that are contained by the room--not necessarily just the ones related to that room's circuitry--can be captured and duplicated to the other rooms depending on your settings.  Duplicating changes made in one room to the others can be tricky once the board is mostly laid out, as sometimes it can be hard to avoid capturing some tracks or vias you don't want. 

It's worth noting--since this isn't really clear from the docs, IIRC--that this works whether you use the 'repeat' syntax for one sheet symbol or you use multiple separate sheet symbols to get your three channels.  As long as they all use the same base sheet, they should be recognized as part of the same channel class and it should all work. 

I would definitely recommend playing around with this in a sample project before getting into the real one--or at least, try the room copying tools out before you get too far in laying out the board for real.  There are a few quirks to it, and to using rooms in general.

Thanks for that advice: I now realise I have to understand rooms also.

I'm using Altium 22, and I've been following this walkthrough http://valhalla.altium.com/Learning-Guides/TU0112%20Creating%20a%20Multi-channel%20Design.pdf

I now have a collections of rooms populated with components, and I've laid out one room.

When I now try

* Design|Rooms|Copy Room Formats
* Click on source room
* Click on destination room
This is successful, which is great.

Today I noticed this:

I have a single child sheet (one channel, a 'front panel' containing just connectors). Above that, on the parent sheet, I use REPEAT(FRONT, 1, 3).

Now, the channels are meant to be fully isolated (they will run from physically separate and floating power sources). I do not want any connections between the channels - but I would like them all on the same PCB.

Normally I would expect Altium to show 3 "greyed out" channels as tabs along the bottom of the schematic editor (alongside the actual editable schematic) as expected for a multi-channel design. But noting happens in this case...

I then added an (unwanted) port to the child schematic, and to the parent - 'lo & behold', suddenly the 3 extra tabs appear. As soon as I remove the port, the 3 channels again disappear.


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version