This is a bit of an odd posting since it's about something I've done but is also here to help me explain why I did it and thus perhaps encourage some discussion around the topic within the Kicad community...
Recently (as you will know if you follow this blog anywhere it is syndicated) I have started playing with Kicad for the development of some hardware projects I've had a desire for. In addition, some of you may be aware that I used to work for a hardware/software consultancy called Simtec, and there I got to play for a while with an EDA tool called Mentor Designview. Mentor was an expensive, slow, clunky, old-school EDA tool, but I grew to understand and like the workflow.
I spent time looking at gEDA and Eagle when I wanted to get back into hardware hacking for my own ends; but neither did I really click with. On the other hand, a mere 10 minutes with Kicad and I knew I had found the tool I wanted to work with long-term.
I designed the beer'o'meter project (a flow meter for the pub we are somehow intimately involved with) and then started on my first personal surface-mount project -- SamDAC which is a DAC designed to work with our HiFi in our study at home.
As I worked on the SamDAC project, I realised that I was missing a very particular thing from Mentor, something which I had low-level been annoyed by while looking at other EDA tools -- Kicad lacks a mechanism to mark a wire as being linked to somewhere else on the same sheet. Almost all of the EDA tools I've looked at seem to lack this nicety, and honestly I miss it greatly, so I figured it was time to see if I could successfully hack on Kicad.
Kicad is written in C++, and it has been mumble mumble years since I last did
any C++, either for personal hacking or professionally, so it took a little
while for that part of my brain to kick back in enough for me to grok the
codebase. Kicad is not a small project, taking around ten minutes to build on
my not-inconsiderable computer. And while it beavered away building, I spent
time looking around the source code, particularly the schematic editor
To skip ahead a bit, after a couple of days of hacking around, I had a proof-of-concept for the intra-sheet links which I had been missing from my days with Mentor, and some ERC (electrical rules checking) to go alongside that to help produce schematics without unwanted "sharp corners".
In total, I added:
- an "intra-sheet link" schematic element, including:
- the schematic element itself
- loading and saving of the element (which required a bump in schematic file format versioning)
- UI for adding intra-sheet links to your schematic
- netlist build support to ensure that the links found their way into the internal netlist content.
- an ERC tickybox "Strict wiring checks" and behind that I hid:
- checks for wires with dangling ends (dangles are bad)
- junctions which have no point in being present (pointless junctions are confusing to readers)
- checks that intra-sheet links exist in groups of two or more on any given net, since individual links are pointless.
All of this is meant to allow schematic capture engineers to more clearly state their intentions regarding what they are drawing. The intra-sheet link could be thought of like a no-connect element, except instead of saying "this explicitly goes nowhere" we're saying "this explicitly goes somewhere else on this sheet, you can go look for it".
Obviously, people who dislike (or simply don't want to use) such intra-sheet link elements can just disable that ERC tickybox and not be bothered by them in the least (well except for the toolbar button and menu item I suppose).
Whether this work gets accepted into Kicad, or festers and dies on the vine, it was good fun developing it and I'd like to illustrate how it could help you, and why I wrote it in the first place:
A contrived story
Note, while this story is meant to be taken seriously, it is somewhat contrived, the examples are likely electrical madness, but please just think about the purpose of the checks etc.
To help to illustrate the feature and why it exists, I'd like to tell you a somewhat contrived story about Fred. Fred is a schematic capture engineer and his main job is to review schematics generated by his colleagues. Fred and his colleagues work with Kicad (hurrah) but of late they've been having a few issues with being able to cleanly review schematics.
Fred's colleagues are not the neatest of engineers. In particular they tend to be quite lazy when it comes to running busses, which are not (for example) address and data busses, around their designs and they tend to simply have wires which end in mid-space and pick up somewhere else on the sheet. All this is perfectly reasonable of course, and Kicad handles it with aplomb. Sadly it seems quite error prone for Fred's workplace.
As an example, Fred's colleague Ben has been designing the power supply for a
particular board. As with most power supplies, plenty of capacitors are needed
to stabilise the regulators and smooth the output. In the example below,
the intent is that all of the capacitors are on the
Sadly there's a missing junction and/or slightly misplaced label in the upper
section which means that C2 and C3 simply don't join to the
FOO net. This
could easily be missed, but the ERC can't spot it at all since there's more
than one thing on each net, so the pins of the capacitors are connected to
Fred is very sad that this kind of problem can sometimes escape notice by the
schematic designer Ben, Fred himself, and the layout engineer, resulting in
boards which simply do not work. Fred takes it upon himself to request that
the strict wiring checks ERC is made mandatory for all designs, and that the
design engineers be required to use intra-sheet link symbols when they have
signals which wander off to other parts of the sheet like
FOO does in the
example. Without any further schematic changes, strict wiring checks enabled
gives the following points of ERC concern for Ben to think about:
As you can see, the ERC is pointing at the wire ends and the warnings are simply that the wires are dangling and that this is not acceptable. This warning is very like the pin-not-connected warnings which can be silenced with an explicit no-connect schematic element. Ben, being a well behaved and gentle soul, obeys the design edicts from Fred and seeks out the intra-sheet link symbols, clearing off the ERC markers and then adding intra-sheet links to his design:
This silences the dangling end ERC check, which is good, however it results in another ERC warning:
This time, the warning for Ben to deal with is that the intra-sheet links are pointless. Each exists without a companion to link to because of the net name hiccough in the top section. It takes Ben a moment to realise that the mistake which has been made is that a junction is missing in the top section. He adds the junction and bingo the ERC is clean once more:
Now, this might not seem like much gain for so much effort, but Ben can now be
more confident that the
FOO net is properly linked across his design and Fred
can know, when he looks at the top part of the design, that Ben intended for
the FOO net to go somewhere else on the sheet and he can look for it.
Why do this at all?
Okay, dropping out of our story now, let's discuss why these ERC checks are worthwhile and why the intra-sheet link schematic element is needed.
Note: This bit is here to remind me of why I did the work, and to hopefully explain a little more about why I think it's worth adding to Kicad...
Designers are (one assumes) human beings. As humans we (and I count myself here too) are prone to mistakes. Sadly mistakes are often subtle and could easily be thought of as deliberate if the right thought processes are not followed carefully when reviewing. Anyone who has ever done code review, proofread a document, or performed any such activity, will be quite familiar with the problems which can be introduced by a syntactically and semantically valid construct which simply turns out to be wrong in the greater context.
When drawing designs, I often end up with bits of wire sticking out of schematic sections which are not yet complete. Sadly if I sleep between design sessions, I often lose track of whether such a dangling wire is meant to be attached to more stuff, or is simply left because the net is picked up elsewhere on the sheet. With intra-sheet link elements available, if I had intended the latter, I'd have just dropped such an element on the end of the wire before I stopped for the day.
Also, when drawing designs, I sometimes forget to label a wire, especially if it has just passed through a filter or current-limiting resistor or similar. As such, even with intra-sheet link elements to show me when I mean for a net to go bimbling off across the sheet, I can sometimes end up with unnamed nets whose capacitors end up not used for anything useful. This is where the ERC comes in.
By having the ERC complain if a wire dangles -- the design engineer won't forget to add links (or check more explicitly if the wire is meant to be attached to something else). By having junctions which don't actually link anything warned about, the engineer can't just slap a junction blob down on the end of a wire to silence that warning, since that doesn't mean anything to a reviewer later down the line. By having the ERC warn if a net has exactly one intra-sheet link attached to it, missing net names and errors such as that shown in my contrived example above can be spotted and corrected.
Ultimately this entire piece of work is about ensuring that the intent of the design engineer is captured clearly in the schematic. If the design engineer meant to leave that wire dangling because it's joining to another bit of wire elsewhere on the sheet, they can put the intra-sheet links in to show this. The associated ERC checks are there purely to ensure that the validation of this intent is not bypassed accidentally, or deliberately, in order to make the use of this more worthwhile and to increase the usefulness of the ERC on designs where signals jump around on sheets where wiring them up directly would just create a mess.