Feedback on small schematic project

[PsySc0rpi0n]

Hello.
I’m going to be working with a LiLyGo device and whle I’m wating on the device to get to my hands, I decided to take a sneak peak on their github where I found some schematics in PDF format.

So, to help burning time while I don’t get the device, I decided to create KiCAD files for the schematic they have on their github.

The PDF I followed is this one:

Xinyuan-LilyGO/T-SIM7600X/blob/master/schematic/T54_SIM7600_20201012.pdf

I tried to stay as close as possible to the design they have, including creating all symbols to match pin labeling and positioning, etc.
Only thing I didn’t follow, and when I noticed was not feasible to change and start over, was the size of the sheets, so I had to resize some components and change a little bit the positioning of components in the schematic in some cases.

I would love to have some feedback on my humble attempt to mimic their schematic and what can I do to improve and eventually fix errors I may have done in the process.

Sheet 1

Sheet 2

Sheet 3

Sheet 4

I have a zip file with the project. If anyone wants them, I can send them. I don’t know if I can send zip files here to the forum!

[jmk]

Hi @PsySc0rpi0n

You seem to have done a great job of mimicking the original. Unfortunately, the purpose and workflow of that original is virtually impossible to understand.
I would liken the original to someone asking me what was the picture on a jig-saw puzzle if that puzzle had been dumped out of its box and onto a table without assembly.
The four pages and 29 rectangles of symbols will take hours of effort to try to understand the design.

If you changed the sheet size to A3, removed all the boxes and connected all symbols together this circuit would then be readable and able to be understood.

A schematic is best presented like a page of a book. Left to right and top to bottom, so the reader doesn’t have to waste time and effort hunting through the pages and boxes to find out what goes where and why.

[PsySc0rpi0n]

Indeed. I totally agree.
I even end up creating 2 issues on their github asking if some of the power input symbols were typos or not, because I couldn’t find a match in the entire circuit for one or two of them. But I got no response so far. I’m not an expert in electronics so I might have missed the point of some of those power inputs

My goal was also to get some insight of how we are supposed to organise, let’s call them, functioning blocks of electronics of a major circuit for readability purposes, but when circuits gets a bit bigger, as you said, it may become actually harder to track things.

Anyway, thank you for the feedback.

[bask185]

You call this “small” ? it is bloody massive .

I am huge fan of hierarchial sheet in combination with busses. The general idea is that I can see all core components and connectors in a single page. Especially fo such massive schematics as you show

This is one of my relative larger schematics

Found another relative (relative to what I make) large one

Kind regards,

Bas

[jmk]

@bask185 's schematic works as he has an overall “map of the camp” with defined paths (the reader can follow) from one part of the circuit to another.

I didn’t consider the “small project” that massive. Hence, the suggestion that the whole lot would probably fit on an A3 sheet.

[paulvdh]

@jmk

Unfortunately, the purpose and workflow of that original is virtually impossible to understand.

Same here. I have been looking a bit at two pages of power regulators, and I can’t figure out which are the inputs and the outputs. Apparently there is a battery too somewhere in there. I have always had a big dislike of the many unconnected puzzle boxes.

This is a relatively big / complex schematic, There are much bigger schematics of course but this is getting there. I find that with A4 sheets, you have to cut circuits into too small pieces and it often becomes illegible.

You can’t dump everything on a big sheet and connect it either. You have to find some balance. Putting all power related stuff on a single A3 sheet is a good idea. Combine it with (roughly) signal flow from left to right, and Voltages from top to bottom. And put emphasis on important parts. If the battery is the main power supply for the circuit, then show it as a big battery in the circuit itself, and put all derived voltages from the battery on the right side of it. If there is a battery charger circuit (with input connectors?) then put that on the left side of the battery.

Similar for microcontrollers. It often is the main part of the functionality of a circuit. Put it central on the page, Try to put sensors on the left side, and outputs on the right side. Try to connect most of the things directly to the microcontroller with wires, but labels are OK too. But make a conscious decision of what makes the most sense in each instance.

There are some open wire ends. Always scan your schematic for the small green open squares:

Jut today an ERC test has been added to KiCad-nightly:

Post-V8 New Features and Development News

New ERC check for wires with unconnected endpoints. [image]

You also do not have to make this construction:

In KiCad local and global labels always connect to each other if they are on the same page. So you can use local labels on the same page, and if you want some of those labels to go global, just put a global label with the same name on that page.

[jmk]

@paulvdh

Try to put sensors on the left side, and outputs on the right side.

And for @PsySc0rpi0n: place all the bypass capacitors where they are needed, not on a separate page. This way you have half a chance of remembering to place them in the right places on the PCB, instead of having to alter that PCB later because you forgot the bypass caps.

[paulvdh]

@jmk

And for @PsySc0rpi0n: place all the bypass capacitors where they are needed, not on a separate page.

My own preference is to put bypass capacitors on a row on the power supply page.

The bypass capacitors are important, but they do not modify the function of the schematic in any way. (They just prevent your project from working at all if you omit them )

Also, the schematic should be drawn according to logical function, not to how currents flow though the PCB. Putting them on the schematic close to the IC’s often makes it difficult to connect signal wires to the IC, and I find those much more important to show clearly on the schematic. I know some disagree with this. You can expect to find both methods out in the wild.

Below a screenshot of the power of a (simple) project. No weird boxes, just a bit of whitespace between sections (which makes maintenance a lot easier). Important things have big fat texts, and I also put some small miscellaneous stuff on this power supply sheet, because the project has just two sheets. There was plenty of room left on this sheet, and it keeps the main sheet free from the clutter.

[PsySc0rpi0n]

Thanks for all the replies and suggestions.
As I’m not very experienced in designing electronic circuits anywhere near this size, of course that many of the suggestions are new to me. The only one not new is the last one about having the decoupling caps all together in a single sheet near the components where they really need to physically be.

The screenshot above also shows new parts to me. Not sure if the come in default libraries of if they are custom made, but they look fancy!

About the comment about regarding local and global labels, well, what I did was more with the intent of trying to make it look like the original rather than to give it any sort of functionallity. In fact, I am not even sure about the goal of the same parts in the original schematic! Not sure if they really meant to be local and global labels or something else!

[paulvdh]

Those spark gaps are self designed. I was mostly experimenting a bit with custom pads and I don’t know how effective they are. Below a screenshot of their PCB footprint. The purple is a cutout in the solder mask and the tips are 0.27mm apart. Looking at them now, I could have made them a lot smaller.

I’m not really sure if footprints like this would be worth committing to KiCad’s default libraries.

[retiredfeline]

I had one glance at the “graphical netlist” “small project” over breakfast and it was cereal out.

[PsySc0rpi0n]

Forgot to mention that the 2 wires that were unconencted were due to dragging items. For some reason the connections got lost. I redo them. Thanks for pointing out.

Regarding the labels, in the original schematic. Did you take a look at them? I mean, with respect to your comment about the construction I have? Are those labels needed in the first palce? I didn’t understand that very well.

[Paul.Blitz]

(A very simple circuit, all actually on a single A3 sheet:)

1. An audio Distribution Amplifier:

Nothing clever. Duplicated for stereo. Input buffer amp (with the option to change gain at build time), and load of unity gain output drivers. The output resistors never get fitted (just the link), but added them “just in case”.

To my eyes, it’s easy to see the flow of the audio, from left to right. If I’d used “little boxes” this would have been FAR less obvious.

2. The power supply bit:

5 volts power in by one of 3 possibilities (solder in the one you want!), input caps (and power LED!), a choice of two 5v-12-0-12v converters (similar function, slightly different pinout, fit what you have in stock when you build it!), and output caps. Yes, some people would maybe prefer to put the 100n caps with the op-amps, I just decided it was cleaner this way. Besides I know why I put them there! I could have used more 100n caps, but they just were not needed.

We use several of these at a community radio station, they sound good, no hum, no artefacts from the DC:DC converters.

This is audio stuff, so the ground plane is not at all critical, it just fills in all the gaps on both sides of the PCB - although, because those DC:DC converters are isolating, I have 2 grounds, one for the incoming part of the power, one for all the audio stuff.

Size is just under the 100mm x 100mm for cheap PCBs at Chinese places, the indents in the edge are for mounting pillars in the plastic box! No mounting holes needed on the PCB, as it’s held in by the 3 screws on the panel phono (=RCA) sockets. And I left space around the (relatively bulky) sockets at the bottom, just to make it easier to get to stuff once built.

(yes, it’s not as complex at what many of you guys design, and it’s probably my own simplest board too, but thought it nicely showed how much better it was to have a schematic with a nice flow to it)

[Vaibhav_Khatri]

Hello
The schematics link you have given is kind of difficult to follow, they should have opted for a system level block diagram approach (don’t know if OrCAD provides that), you have also done a good job of simplifying most of the schematics but you should try using Hierarchical sheets. Their are so many nets to follow which jump from one page to other why not use Buses, using these two with improved symbol (like grouping similar kinds of pins together such as power/gnd, GPIOs, communication line, etc. and breaking up symbols with larger number of pins by using multi-unit symbols). I think once you make these improvements your schematic will look a whole lot better.

Thanks.

[jmk]

@Paul.Blitz

That is my idea of a schematic. A pleasure to read

@Paul.Blitz

some people would maybe prefer to put the 100n caps with the op-amps

Personally, I do as you. My earlier comment was really aimed at the not so experienced. Many a time I’ve seen good PCB layouts torn up because there was no room to place the bypass caps, as they had been forgotten until too late to fit.

My personal method for footprint placement, my time tested method, is:
“Must be in certain places” footprints and holes first. ICs with bypass caps next. Any other critical footprints for the ICs next. Transistors, Resistors, Capacitors and Connectors last.

[craigarno]

I agree with most of the comments here for “good practice”.

I’ll add that I find it easier to keep larger functional associations together if a larger sheet, like A3 (297 × 420 mm), or in my case B-size (11 × 17) schematics. Of course, this means I had to buy a B-size printer for my A and B size schematics. But design reviews go a lot better if everyone can easily read and understand the design. For those with less experience, B-Size pages can be fan folded and 3-hole punched for an 8.5 x 11 notebook. This has the added advantage that they retain their landscape orientation while in the notebook, and are still easy to use.

Some might argue, with a 4K 85" screen why do you need paper? Paper is useful if you need to view several pages at the same time. Just lay them out on the conference table in the review… unless of course you’re working remotely from different parts of the world.

[bask185]

some people would maybe prefer to put the 100n caps with the op-amps

I prefer this as well. For one reason alone,
1). I am a hierarchial sheet user. I re-use schematics and boards, so having all decoupling C on a special page cannot ever work for me.

I have more less significant reasons.
2). The reference numbers would be completely different. My pages have 3 digit numbers, I find it logical to have a C9xx close to an U9xx. With the same reference ranges, it also makes it easy for identifying which C should be placed where (though they are interchangable)

3). Placing the cap near the IC where it belongs, explicetly shows readers that the cap is not forgotton. And it also shows it’s purpose. A typical rookie mistake would be forgetting about these. And if I see some power sheet with 13 100nF caps, how do I tell that every C is acounted for?

Kind regards

Bas