How can I design a readable and understandable schematic?

Question

After reading all of your feedback on my flight controller schematic I posted two days ago in Model rocket flight controller schematic review, I redid the entire schematic and tried my best to make it readable and easy to understand, so that others can more effective look over it and check for errors/mistakes.

The main goal was to make connections clearer, and not so split.

Is my second version better, in terms of readability?

And what are things to improve? (mainly on the "aesthetic" side; not for the functional side of things)

This is the first version:

And this is the new, second version:

Answer 1

It's definitely an improvement but, nothing beats having main flow from left to right unambiguously connected on one sheet: -

And, you can improve the above by moving TX and RX on the MCU to the left side and physically making a connection to where they are on the USB/UART chip. It's all about main signal flows and not breaking it up. I can see what the design does now.

Answer 2

An old post on this forum by Jonk outlines good practices for drawing schematics.
Your second schematic is OK, meaning it is readable with some difficulty, however, it needs some cleanup.

Some thoughts on what I see:

• Schematic symbols and reference designators can be found in IEEE Std 315. It's best to use the standards. If your region has a different standard for drafting, use it.

• When depicting transistors, use the proper symbol instead of a box. When others look at your schematic proper symbols are instantly recognizable. Don't make viewers do extra work parsing symbols. Modern schematic tools allow homogeneous and hetrogeneous parts.

• The common symbol has "GND" along with it. This extraneous text adds to clutter. There are times to show labels with common symbols if you have multiple commons. Also, this looks like Altium with the non-standard common symbol with four horizontal lines (it should have three horizontal lines). For that reason, I use a triangle symbol in Altium and hide the "GND" text. The first schematic has ground symbols pointing upwards which is bad practice. You fixed that in the second schematic.

• Q5 & Q6 has crowding with junction dots touching Q5 & Q6 which looks like there should be a pin on Q5 & Q6. This adds confusion. Also the PyroContinuityn nets split the resistor symbols (R8 & R9) from the labels. There is no need to do this as you have ample space to route the net around the resistors.

• Be consistent in your labeling. Most of your symbols have the reference designation over the value (good). R8 & R9, and other parts, have the value over the reference designation. The reference designation and vale should line up. C15, C16, & Q6 are good examples of being sloppy. A schematic is also a work of art.

• No need to include the omega symbol for the resistor values. It clutters up the schematic.

• My personal preference is to have reference information horizontal. LED1 & LED2 are examples of vertical text which I don't like.

• My personal preference is to use upper case text except for design notes. Easier to read when printed. I also use a mono-spaced font with no ambiguities (i.e., 1 l I are distinct). However, Altium doesn't handle non-default fonts well when using the built-in PDF printer (solution is to use a third party PDF printer).

• My personal preference is to use as few pages as possible. Having a one page schematic as you do is wonderful. On more complicated schematics I'll group functionality per page. Example: core schematic on page 1, power supplies on page 2. Unfortunately, Altium schematic editor gets very slow when there are lots of parts/pins on a single page. My cure is to work on small parts of the design on a separate worksheet page, then move (copy/paste) the section to the final page. Other approaches to the program slowness are to have a 20+ page schematic which makes it hard to follow.

• Be careful about color selection. Some colors don't have good contrast when printed.

• Check for connection errors like CN1-1 going to +VBAT. It looks like you are missing a junction dot. The design rules may show this as an error when you transfer the design to PCB.

Answer 3

This is already much better. I would put all the power related circuits together (VBAT, 5V, power LED etc), and the USB circuit together with the UART circuit. Either connected or, at least next to each other (but then it will be obvious that you will want to connect them). But it's already OK.

Now it depends what you intend to do with the schematic. And according to what you want to do, you may want to make a second schematic, in another way.

Here the schematic is useful to understand how the circuit functions, how pins receive signals and what signals do etc. That's fine for the theoretical concept. Now, when the schematic is to serve as a preliminary to board design, or to be used later to compare the PCB with the schematic to debug something, then you are going to face problems, maybe making mistakes, because the pins are not in their right physical order. It sometimes makes the schematic easier to draw and to read to invert the pin orders or to reset the pins in a random order. But when you use your schematic to remember what your board is doing, to compare it with the real PCB design, check the datasheet (where pins can also be put in random orders in some circuit examples, but not in the same random order as yours), then you will run into troubles and lose time.

A second schematic where pins are in their original order and where everything is connected could be useful prior to design the PCB. It will help you place and rotate the components already in a rational way, visually closer to the real PCB while still having all the informations about the circuitry. It's not possible to make a schematic identical to the PCB, because you always rotate or move something to reduce trace lengths and so on, but at least, you can have intuitive similarities. When, 5 years later, you will look at your PCB and at the schematic next to each other, you will remember what does what easily, and won't lose half an hour scratching your head.