Slick method to populate multiple BOM parts from single Altium SCH parts

[jmarkwolf]

Many times I'll have large multi-pin connectors in a design.

Such connectors have terminals, mating connectors, back shell parts, nuts/bolts, etc, etc.

Till now, I've just included a schematic symbol for these parts, sometimes taking up a whole page.

Anyone have a slick method for getting all these parts "properly" represented in the BOM without adding a schematic symbol for each and every terminal, mate, back shell, nut/bolt?

[julianhigginson]

One option is to create a part number for a parts "kit" (like a subassembly, really but not actually assembled so much as gathered) and put in one BOM only part to call that kit.

however.

If you are going to think about your product being an assembly of parts and subassemblies, then does the actual PCB Assembly you are describing with the BOM require those extra mechanical parts? Does that make sense in production? or should the PCBA level assembly only contain the basic bits soldered to the board in the PCB Assembly process...  then you should have another BOM that uses that PCBA, and the extra connector bits, case parts, screws, firmware programming, calibrating process, etc to make the finished product?

[ajb]

I believe the official answer is that there's no way to get more than one BOM component out of one sch component.  This came up before (either here or on Altium Live) when someone was asking about footprints for plug-in modules requiring multiple separate connectors. 

If the goal is just to get them into the BOM, using snippets or saving and reusing one sheet per connector assembly (perhaps inserting as a repeated subsheet if necessary) may be helpful.  If you also need them to appear in the PCB as a 3D model, then do as above but also include one component that places a 3D model of the fully assembled connector on the PCB?

If you are using Excel templates for your BOMs, you could include a macro that expands a single line for the connector assembly into lines for all of the required pieces, but that's a pretty ugly solution. 

What sort of connectors are these?  Generally it makes most sense that the PCBA BOM only contains parts that are fitted as part of the PCB assembly process.  If you're trying to use Altium to manage higher-level BOMs, it's probably best to do so as a separate project.  Or maybe it's time to start looking at a real ERP system. 

[jmarkwolf]

I neglected to mention that my inquiry related to schematic-only, non-PCB designs, with discrete wire connections to large twist-lock mil-spec Amphenol connectors, and discrete components such as large toroid inductors and large 100W resistors, etc.

I suppose I could add additional parameters to all the parts, and create a custom BOM template with columns for these added parameters.

Thanks for helping me think out loud.

[julianhigginson]

wow. that sounds like a very interesting wiring design job!

I'm not a fan of AD for wiring drawing purposes... but I don't have anything better to suggest that's practical for you.
I miss having a mechanical engineer with solidworks license as a coworker. Best wiring loom and cabling drawings I've ever seen.

But, you can still use a schematic component to call out a connector kit for everything related to a connector.

You end up with one part in the schematic giving one part in the wiring loom assembly BOM, (and hopefully one bag in stores to pick) but you know that part kit has another BOM that tells you what that kit part is made up of.  And if you use the same connector in multiple designs with the same accessory parts, then the kit is always the same so can be reused. (and if it's ever edited, for instance a part is EOL'd/replaced then its edited for all your assemblies that use it)

I'd be especially wary of using special parameters in parts:
1) depending on what you do with part updates from libs, you can easily clobber that info.
2) it's easy to overlook parameter info unless you make the parameters all shown - then it's all over the schematic page again and you could have just done it with separate parts in the schematic using ultra tiny icons.
3) it won't be easy to get "parameter parts" in one schematic part to show up inline in the BOM. You can probably do it with a python script and pandas, but the temptation will be when the python script has issues or doesn't behave right one day just to manually edit the bom output to make it work, and that is the worst idea ever.

Seriously though. Subassemblies. They are useful. They can be properly managed. They will make your design efforts more robust and less prone to human error.

[julianhigginson]

I guess if you really want to keep all your work in altium, you could do a separate schematic sheet for all the extra connector bits related to a connector, then put a sheet entry referencing that sheet next to a connector every time you use the connector.

That would let you keep subassemblies out of your production system and manage it all yourself.... But I still think it'd be easier and better to just start using subassemblies.