Altium Library SOM

[maxpayne]

What is the best way to make library for a  SOM ? (Like, Rasp Pi CM4, Coral SOM etc.)

These normally have different types of block inside (like power, I2C, HDMI, USB etc.) and it’s convenient to use individual blocks in separate schematic sheets and in hierarchical design, if I do so, they don’t make single designator for one SOM. Also, some of the SOM contains 2 or sometimes more than 2 connectors for interfacing with the main board.

[thm_w]

You can use a multi-part component if you want to split up the individual blocks under one designator.

https://resources.altium.com/p/your-altium-library-multiple-part-symbols-ease-your-design-time
https://www.altium.com/documentation/altium-designer/creating-schematic-symbol

[maxpayne]

You can use a multi-part component if you want to split up the individual blocks under one designator.

https://resources.altium.com/p/your-altium-library-multiple-part-symbols-ease-your-design-time
https://www.altium.com/documentation/altium-designer/creating-schematic-symbol

What about if I place muli-part component across several schematic sheets ? the designator then does not remain the same ...

[thm_w]

You can change the designator to be the same (U1A, U1B, etc.).

Though there may be some setting causing this, I don't recall what the regular behavior is. I think it depends on if you copy the part or place a new part, etc.

[maxpayne]

I can do that (U1A, U1B...) if all blocks are in the same schematic sheet.

But I need the blocks to be placed in different different sheets according to function. then the designator does not behave similar way.

At the footprint side, I want one connector (for example) consisting of blocks placed in several schematic sheets.

[ajb]

Having

I can do that (U1A, U1B...) if all blocks are in the same schematic sheet.

In Tools > Annotation > Annotate Schematics, make sure "Complete Existing Packages" is set to "Whole Project". 

In general, though, I would argue that you should keep the SOM footprint/symbol separate from the footprint(s)/symbol(s) for the connector(s).  There are several reasons for this, but the big one is that Altium can't produce multiple BOM entries or placements for a single part.  So you would need to add separate BOM/placement entries somehow for the SOM and however many connectors it needs. 

Instead, consider making a footprint for the SOM itself that has an overall outline with reference geometry for where the connectors should be placed on the PCB (preferably references you can snap the connectors to).  Once the SOM footprint and matching connectors are placed, optionally union them in the PCB to make them a little easier to handle.  This means your BOM and placement entries for the SOM and connector(s) will be generated automatically, and makes it easier to manage the connectors and their footprints separately from the SOM footprint*.

This doesn't (easily) allow you to use multi part schematic symbols for logical connectivity blocks--but you can place the SOM connectors on one sheet, and then use harnesses to bring out the various sets of HDMI/I2C/USB/whatever signals out of that sheet to wherever you need them.  This is significantly more flexible anyway, since you don't need to overhaul the SOM schematic symbol to use different sets of pin functions.  If you want to show what signals are on what positions on the SOM, you can include that information in the schematic symbol.  In fact, you could create the SOM symbol with pin labels (but no pins) that you can drop your connector symbols right next to, such that the connector pins line up with the signal names. 

* Consider that if you want to switch from, say, PTH headers to SMT, you can do that by just replacing the headers, with no need to edit the SOM.  Similar if you need to edit the footprints for any reason: you can just edit the connector footprints, and don't ALSO have to edit any SOM footprints where those connectors are embedded. 

[maxpayne]

Having

I can do that (U1A, U1B...) if all blocks are in the same schematic sheet.

In Tools > Annotation > Annotate Schematics, make sure "Complete Existing Packages" is set to "Whole Project". 

In general, though, I would argue that you should keep the SOM footprint/symbol separate from the footprint(s)/symbol(s) for the connector(s).  There are several reasons for this, but the big one is that Altium can't produce multiple BOM entries or placements for a single part.  So you would need to add separate BOM/placement entries somehow for the SOM and however many connectors it needs. 

Instead, consider making a footprint for the SOM itself that has an overall outline with reference geometry for where the connectors should be placed on the PCB (preferably references you can snap the connectors to).  Once the SOM footprint and matching connectors are placed, optionally union them in the PCB to make them a little easier to handle.  This means your BOM and placement entries for the SOM and connector(s) will be generated automatically, and makes it easier to manage the connectors and their footprints separately from the SOM footprint*.

This doesn't (easily) allow you to use multi part schematic symbols for logical connectivity blocks--but you can place the SOM connectors on one sheet, and then use harnesses to bring out the various sets of HDMI/I2C/USB/whatever signals out of that sheet to wherever you need them.  This is significantly more flexible anyway, since you don't need to overhaul the SOM schematic symbol to use different sets of pin functions.  If you want to show what signals are on what positions on the SOM, you can include that information in the schematic symbol.  In fact, you could create the SOM symbol with pin labels (but no pins) that you can drop your connector symbols right next to, such that the connector pins line up with the signal names. 

* Consider that if you want to switch from, say, PTH headers to SMT, you can do that by just replacing the headers, with no need to edit the SOM.  Similar if you need to edit the footprints for any reason: you can just edit the connector footprints, and don't ALSO have to edit any SOM footprints where those connectors are embedded.

please check the schematic. Is this what you mean ?

https://github.com/mfolejewski/MirkoPC/tree/main/REV1.1

[ajb]

Not really sure what I'm looking for.  Sheet 5?  I see separate symbols for the CM4 and mezzanine connectors like I mentioned.  You've defined all the pins as part of the CM4 symbol not as part of the connectors, which is fine, although different from my suggestion.  I see you've used harnesses, but if you have all of the pins in the symbol grouped by functionality, why not put the harness connectors right up against the symbol?  You could save yourself from placing all of those net labels.

[maxpayne]

This is not really my design. Found it in internet and it looks similar what you suggested. Specially page 3, 4 and 5.

I will try to make a CM4 library as per your guidance and see how it goes.

Really appreciate your suggestion.