First Schematic - Looking for Pointers

I just built a good part of my first schematic and I want to know if I am on the right track. It is supposed to be just a power distribution board where I would connect components to. Some of the components are shown on the sheet so want some feedback on whether or not I am doing this right? Thanks in advance.

Your PCB will contain only connectors and tracks?
If so, you should have only that at schematic as all elements from schematic will go to PCB design.

I have no big experience with KiCad (one PCB). I don’t know if you can left some elements out of PCB outline and pass DRC without complains. I would never do it that way. For me schematic (in PCB design software) is the schematic of PCB and not surrounding elements. If I would like to show that surroundings I would use for it graphic lines and not element symbols (or may be elements without footprints connected to them if it is possible).

For just switching things from input to outputs and not much discrete logic/circuitry going on I wouldn’t bother with wires, as they are hard to follow and do not make your schematic easy to understand.
Use local labels if on one page or global labels if you have several pages. GND for example is a global label automatically.
There also are hierarchical labels for more complex designs, involving more sheets connecting to each other.

Also there are buses for stuff that goes parallel that you can use.



Two pointers:

  1. Remove the 4-way junction. Do not do this:

  2. Although it may seem abstract at first, remove J3A and J3B. Then, change the Footprint of the relay to whatever your intent is.

The way that I interpret this part of the schematic is that the relay is to be remote located some distance away from the PCB. And, this is fine for a paper schematic; however KiCad is an EDA tool and this is going to have trickle down effects when laying out the PCB using PcbNew.

Is there any reason why the relay can not be mounted to this PCB?

Is there any reason why the switch and fuses can not be mounted onto the PCB?

Here are some other concepts to take a look at:

It is common practice to include some form of ground return path symbol instead of drawing “wires” all over the schematic. In the example above, I left one ground symbol with the text “GND”, but in my schematics I leave the text invisible as I find the text to be redundant.

Note: I do not appear to have the same relay symbol that you have. In my opinion, the relay should be drawn as in your schematic.

Your design seems to indicate that battery power will be applied to 3 seperate connectors. Just like a household wall outlet, the connector with power should be a female connector that is not easily shorted or inadvertently touched by a person.

When laying out the PCB, the Footprint for the battery can be the Footprint of a two-pin connector that can be soldered to the board. Or, it could even simply be a Footprint that is two plated through holes where wires can be soldered to the board.

The reason for doing it this way in KiCad is that this method allows for both ERC and DRC compliance during the design.

And, as @Joan_Sparky mentioned, labels can significantly reduce the “wires” in a schematic.


Thank you all for your replies. From my other post came this schematic and what I am trying to do is just build a simple pass-thru power distribution board. The relay, switch, fuses etc are going to be located off-board but I wanted to include them in this screenshot so that you could get an idea of what I am trying to do. I have included a couple of pictures of a similar type of board as what I am trying to build, mine on a much smaller scale. It is just a board with connectors and traces.

A trick that you can take advantage of in this sort of layout is to prepend a ‘#’ symbol to the ref des of ‘off board’ components eg your relay and off board connectors. For example, #J1A etc . This will allow you to draw your schematic with the off board components still visible but they won’t be included in the layout. I have found this helpful when, for instance you are keeping track of a display connector.


Thanks John.
I just want to clarify that the components were only added into the schematic to aid in explaining to everyone on the forum what I am trying to accomplish. The pictures I posted is what I am really after and maybe KiCAD is just not going to work? I thought this would be fairly easy to build as it is basically 7 or so lines that I need to take and run to various connectors. The problem is I am running on a timeline and this timeline is getting near the end so I may have to figure another way around it. Not sure what that will be. Maybe I will just have to build my own boards again but I was hoping for the professional looking boards for this project.

You did not really post a question. At what stage are you stuck?

Are you stuck at getting your schematic converted to pcb_new?

  • Did you already assign footprints to your symbols?
  • Did you update the pcb from schematic?

Actually I did post a question and got some really good answers but I am still wondering “Am I on the right track?” By the sounds of the comments, I would say no. Everyone has been very helpful but I am looking for guidance on what I can do to my schematic to make it better for what I want to do. I have attached pictures of what I am looking for in the end, and a schematic which outlines what my connections are along with the components I am going to connect them to. At this point, I just need to get from A to B so I can get this going to a PCB. Then I create the gerber and send it off to get done. At this point I am almost willing to pay someone to do it. I am not whining, just a little frustrated and I apologize if I sound otherwise.

@bwilliams60 I keep waiting for you to notice/fix the error relating to F4.

And, the way the relay is currently wired up, it won’t actually do anything.

I am not sure what “error” you are looking for with F4? Right now it is not connected to anything.
Here is the corrected relay. Thanks for pointing that out. I was looking at my old diagram and following numbers from a previous relay. The relay will be grounded through a module and then B+ is provided by the relay to the module.

See that little “Ladybug” icon? Click it and find out if you do or do not end up with an ERC error at that location (you will have to agree to annotate first). If you don’t want to see that ERC error, place a “No Connection” flag on the pin.

You have been given helpful advice by some very knowledgeable forum members here; and, as far as I can tell, have only made one change to your schematic with that advice.

Myself, I am currently working with a test project to determine how @John_Pateman’s trick actually works out. However, I have already told you that you can use the Symbol for the battery, but use the Footprint for the connector, and this will pass ERC in Eeschema, and DRC in PcbNew later on in the design process.

And, certainly you should know by now that the green squares along wire traces means a unconnected end? I see at least 3 of them in your schematic.


First off, I want to thank everyone especially SPRIG for the much needed constructive criticism. I have gone in and made some changes to my schematic, taken out components, fixed ladybugs, connected fuse block a little differently, finished connections and installed some flags. What do I need to do now to have this ready for turning it into a PCB? Can I get rid of more connections somehow?

I am a teacher by trade and I teach a lot of electrical in Motive Power. It is good to see the other side of the coin where schematics are concerned and the work that goes into them. You guys are good teachers and I thank you for your time. Much appreciated

@bwilliams60 This seems to be a pretty good KiCad EDA schematic for your board layout.

From earlier:

A paper schematic may very well include everything shown in your first uploaded image.

I have seen many schematics that look exactly like this new one you have drawn. As you have noticed, there is now no additional information to figure out what “lies beyond”; but that is not the purpose of KiCad as an EDA design tool.

Your next step is to determine the Footprints for the connectors that will be mounted to the board.

You can do this with CvPcb (Assign Footprints Menu Item) or in Eeschema to edit each symbols Footprint property.

The step after that is to open PcbNew and select the menu “Tools/Update PCB from Schematic”. After that, I expect you just went down the rabbit hole and have a whole bunch more questions swirling about in your mind.

1 Like

LOL, yes there will always be questions. I am going to make some revisions to this schematic and see if it still passes your qualifications and then I will get ready to look at footprints. I am sure you have done many of these so may I ask for some further assistance? I am curious what connectors would be best suited for the following?

Battery input 12V 20A
Relay 12V 20A
Rest 5V 1A

I am thinking that Molex connectors would serve this purpose well. I am hoping to come in at 90 degrees to each connector to keep a low profile. Thanks again for your help.

@bwilliams60 I would suggest adding notes to the schematic to explain what is expected to “lie beyond” to elevate the schematic from just a first step to getting a board done to documenting the design intent. Put notes next to the connectors, maybe even a table for the relay describing how the connector pinout translates to the relay pinout.

Also, I would add local labels to your wires. I’d probably label them by the output connectors, and then maybe label the switched 12V to the fuses and the fused 12V to the relay. This will do two things. First, it will make understanding what the pinouts of all the connectors are (similar to the examples above, but also have your existing wires making the connections to help guide the eye along the path), but because the net names are also visible when laying out the board it makes it easier to select the proper netclass (for trace width, clearance, etc.) for different design considerations. It will also help routing related nets together when the nets are sensibly named.

Then think about footprints. :wink:

P.S. You may have noticed that no one seems to be giving exactly the same information. Drawing a schematic is sort of like writing an essay. Everyone has their own unique writing style.


Is there a specific way to do this so that it does not interfere with the schematic? Hit T and type away and locate it next to the pins?

Same question

Yes, use the “T” tool button on the right tool bar. You can also use the blue dotted square tool button right above the test button to place graphical lines. (Yes, the icon looks like a square/rectangle, but the tool only puts down lines. The style is (currently) locked at blue dashed.) These tools are specifically only for making non-electrical notes.

The notes for the connectors (at least in my mind for my schematic drawing style) would consist of describing the part (or parts with the fuses) that connect to the connector. Therefor I’d probably put the notes where you had the off-board connectors in your first uploaded schematic. Think of these notes like comments in programming code.

Use the right toolbar button that has the black letter “A” above a green line.

For both the label and the text tool, select the tool button then click anywhere in the schematic window. Type your text (the text tool supports multi-line text blocks). When you close the text entry window you can then place the text or label where you want on the schematic. Play around with the rotate (keyboard shortcut “r”) to see how that effects your text.

Note that with the label, because it is considered an electrically relevant part, there is a connection point (the small green square). This connection point must be on a wire of the net that you are naming. Unlike adding a pin or another wire to the same place you won’t get (and won’t need) a connection dot, but that is a good thing because the connection dot may partially obscure the first letter of the label depending on the text size you choose. Extending the analogy above, you can think of the net labels like variable names in programming code.

How am I looking now? I added in my fault switches and rewired it a bit to suit my needs a little better. What else do I need to do?

By the way, I know as much about programming as I do about KiCAD. Well, maybe a little more but not much :slight_smile:

Is there a way to save each version of schematic that you draw?