KiCAD 6.0 symbol development question

RE: KiCAD 6.0 symbol development question

shabaz — Thu, 08 Sep 2022 13:13:31 GMT

Hi Sean,

It's a nice opportunity if you like, to build a symbol (even if you don't need it and find an existing one) because lots of people here can let you know if you're going the right way about it. I did the same thing, I let people here comment on if I was doing things right or wrong when I was learning KiCad.

You'll also get a nicer symbol than any possible existing one on the Internet. For instance, you might want your relay module symbol to look like this:

A quick way is to find any vaguely similar symbol in KiCad, and make a copy of it, and then copy-paste and edit things like the connections and the shapes. That way, there's very little learning curve, other than copy-paste and double-clicking on things to rename or edit them.

I don't know if my video will suit everyone (some people will prefer documentation with screenshots etc), but these sections cover symbols and footprints, but you only need the first link, if you are happy to use any existing SIL header pin footprint in KiCAD (but eventually it's best to learn how to do footprints too).

08:29 - Component Symbol Editor

15:33 - Component Footprint Editor

It's a short 8-minute video portion for symbols, because the copy-paste method keeps the learning curve low as mentioned (I too was learning KiCad so I didn't want to overload myself).

Incidentally, it's also possible to split up the symbol like this:

It's not much more complicated to do that, however, if you're learning, then it is better to just do the single symbol for now, and get practice making symbols, and revisit such split symbols later.

RE: KiCAD 6.0 symbol development question

colporteur — Thu, 08 Sep 2022 12:20:03 GMT

Thanks for the response folks. I am surprised that there isn't more CAD support for modules such as this. It could be one more attractant to making a sale. Then there is the understanding that many of the modules are cheap knockoffs and investing in support is not their market place. If one does it and then it gets shared extensively why invest in it. I might have gotten lost in the Sparkfun market place resources for makers to think it was possible.

The posted responses made me miss being at work. Only briefly, trust me retirement is so much better! Discussions such as this would have taken place during scheduled breaks in the lunch room huddled over a napkin drawing.

A few comments did leave me with follow-up questions. I tend to gravitate towards finding a way to do something rather than developing my own from scratch. This relay is one example but I can think of others. Using discrete components to build from ground zero is time consuming and labour intensive. Purchasing pin ready just wire up modules seems ideal.

I have a bag of the relay components. I have had them for some time. I purchased them with a project thought but never got around to moving the thought to actually making it. When I planned to use them on the next project I notice the self contained module and thought here is a solution. With a single row socket, this relay module could plug into my motherboard. Driver ccts and EMF collapse diodes all done for me. Also I see relays as common failure points. I try to avoid them if I can. A relay module become a plug and place repair.

Grabbing a resources (i.e. symbol with footprint in this case for KiCAD) to insert into the design rather than DIY again seems ideal. I lack the experience and confidence to create the module support resources. I'm trembling over the constructing just the schematic and getting it working. Symbol and foot print build becomes one more task on the road to getting the project done. Pre-made seems so much more easier.

I also thought the maker community would be all over having a collection of modules. Like resources that are popping up for 3D printing. Creating and making available little snippets of their work to be incorporated into others work. I think I lack the understanding for intellectual property. I tend to have an open-source mind set. Dropping a module symbol on a drawing that has a bald-engineer logo seems fitting for credit.

RE: KiCAD 6.0 symbol development question

michaelkellett — Thu, 08 Sep 2022 09:31:33 GMT

I hardly ever use library symbols (schematic or footprints) in my PCB CAD system.

I might start off with a library symbol which I then modifiy but the CAD system also makes it easy to make new ones.

There are reasons for this:

For complex parts like processors I make different schematic symbols for different projects so that the schematic can truly represent the design intent in a useful graphical way.

So if I have an FPGA connected to an ADC using maybe 10 of the FPGA's 256 pins I'll make a schematic part with only those FPGA pins actually connected to the ADC and put that next to the ADC on the analogue sheet of the design. It's a little bit more work at the start but potentially a huge saving in communicating the design to other people.

You'll see a lot of schematics which are just a lot of blocks with names attached to pins, these are very difficult to understand.

There is no chance at all that a standard schematic library part will match my design.

Standard footprints can work (and for example the IPCC librarires offered by CAD vendors may be good) but conventions and practice regarding solder paste, silk screen etc will vary according to customer preference and production methods.

I have seen so many bad library parts that I would never use one without careful checking, so it often need little extra time to design them to be just right for the job.

RE: KiCAD 6.0 symbol development question

Andrew J — Thu, 08 Sep 2022 08:46:52 GMT

It may, on the face of it, seem complicated to create a symbol and a footprint but it’s actually not at all complicated in Kicad. I actually take the same approach as baldengineer mentions. It’s worth the practice and I would make a guess that it might take you an hour to create a symbol and footprint for that part given it’s the first time. Subsequently it might take you around 10-15mins. The problem with downloading the component representations is that you (a) have to find them; and (b) carefully verify them because there’s a reasonable chance they aren’t right. You could easily spend more time doing that, than just DIY.

Shabaz made a comprehensive YouTube video walking through Kicad 6.0.

RE: KiCAD 6.0 symbol development question

Jan Cumps — Thu, 08 Sep 2022 08:16:22 GMT

Design companies typically have a librarian (or team) that is responsible for all symbols and footprints. They only (are alowed to) use footprints from libraries vetted by that librarian.

It's a business role to own this aspect of electronic design.

RE: KiCAD 6.0 symbol development question

baldengineer — Thu, 08 Sep 2022 03:04:44 GMT

Also, for stuff like this, I have custom libraries named "My Symbols" in Schematic and "My Footprints."

For parts with standard footprints, you usually only need to create the schematic symbol. So my schematic symbol library is significantly larger than the footprint library...

RE: KiCAD 6.0 symbol development question

baldengineer — Thu, 08 Sep 2022 03:01:53 GMT

For any of these "modules", I would rarely expect an eCAD program to have a library footprint for them.

That said, personally, I have never seen this module before. And I'm going to guess others haven't either. This reason is probably why there isn't an easy "just download this" option.

However, it isn't that difficult to do in KiCad.

You could either a) create a Symbol and a Footprint pair or b) just use a standard header pinout.

For something like this, I would go with option B). I would add a "Conn_01x09" in the schematic and use net-labels to identify the pins. For the footprint, I would use Connector_PinHeader_2.54mm:PinHeader_1x09_P2.54mm_Vertical.Then in PCB, I would draw a square polygon on the F.Mask (or one of the User) layer as an output of the module's PCB.

Granted, if I planned to use this module on more than one PCB, I would make a custom footprint for it. But, I would probably still continue to use the generic connector in the schematic.

RE: KiCAD 6.0 symbol development question

fmilburn — Thu, 08 Sep 2022 02:57:14 GMT

Having to develop schematic symbols and footprints is not uncommon, especially for inexpensive modules made in China. Schematic symbols can be developed pretty quickly once you get the hang of it, footprints may take a bit longer. It is worth checking downloaded footprints if from an unknown source as they aren't always correct.