I did this to learn how to work with KiCad without having to care too much about how the design was actually made.
I’ve never worked with a CAD tool before so I have limited knowledge in how to work with ERC and what to expect from it.
I’ve got a couple of questions:
Are my power ports created correctly?
Am I using the PWR_FLAGs correctly?
How do you work with PWR_FLAGs? I don’t like to see them in my plotted schematics pdf.
Is it possible to mark R5 in some way so that KiCad agrees that U1, Pin20 is driven?
(I guess then I could place my power flags at J1 instead of at C10, if the same goes for FB1, L1 and L2)
Should it really be an ERC warning that I’ve disabled ”Show pin numbers” of J3 and J4 in my schematic?
Is there a way to save the exclusions of the ERCs without having the small cyan error marker always shown in the schematic?
Is there a more correct way to setup the pins of my components so that I wouldn’t get the 7 warnings? (While still being able to run a meaningful ERC if I use the same components elsewhere. I.e. not just trying to make it pass)
Mostly related to question 3-7; is this roughly what to expect of ERC in the other major CAD tools out there? Or is this an area where KiCad could improve and catch up?
How do you work with ERC? Is it too much work to setup all the rules to avoid warnings so you only use ERC to check for unconnected components/pins/wires?
I want to be careful in telling you that I find the schematic ERC to be not so worthwhile, at least for me. For example I commonly power one or more chips through resistors. If the chip power input pin is not directly connected to a power rail then that flags an error. Also some logic ICs might have several outputs and I will not use all of them. That means that I need to customize the symbol for the project, showing that the unused logic outputs are not connected. ERC will return an error if that is not done. I guess that these checks are worthwhile for some people and situations, but not so much for me. Until I get bitten by a stupid error.
At the moment there is no real solution to “bridge” filter components (ferrite beads, inductors, resistors) for ERC purposes.
I know of at least 3 partial solutions / workarounds.
Add a PWR_FLAG on the other side of the filter component.
Do not use “Power Input” pin types for your schematic symbols.
Just ignore ERC for these, or disable some of the ERC messages. (Try right clicking on them).
You’ve also set the pin types of your MOSfets wrong. They are set to “bidirectonal”, which is mostly used for logic IC’s, microcontrollers, databuses of memory chips etc. I had a look at one of the default MOSfets in KiCad, and it had it’s pins set to passive.
Overall I do find ERC useful, as it does catch a bunch of real errors, but it is very incomplete. There is no “spice like” behaviour behind it. It’s just a handful of relatively simple rules. I do not know how KiCad’s ERC compares to the ERC of other programs. I do like the “No Connect” flags though. This encourages you to think about any unconnected pins, so you do not leave pins open accidentally.
Thanks to @BobZ and @paulvdh for your general thoughts on ERC. And thanks Paul for checking my MOSFETs.
Perhaps one could add a feature request which is roughly:
Right click on a component > Add ERC transparency > Select between which pins the transparency should be.
This way all kinds of symbols could be used as filter components. Beads (1->2), resistors(1->2), common mode filters(1->3, 2->4), diodes (2->1) etc.
Then show these components and their pin configurations in the ERC exceptions window.
Many of those symbols from external sources don’t have the pin type set correctly for KiCad’s ERC. I don’t think I have seen pin type Unspecified for symbols in KiCad’s library, which is what prompted me to ask. You probably need to go through the pins and judge whether the type is correct based on the FAQ.
