Help/advice/guidance translating schematics onto a pcb

[djmiggymigz]

Looking for some help getting over the initial learning curve of reading and translating a schematic onto a breadboard/blank pcb. Very specifically I'm trying to breadboard the DIYRE cloudbooster. I just bought and built the diy kit and looking at the schematic (https://cdn.shopify.com/s/files/1/0698/2265/files/MB2_1.0_Schematic.pdf?v=1642446351) it seems to be simple! Already ordered what parts I don't already have.

I already know I need to learn about how parallel/series components are actually laid out. I have at least a decent understanding of the theory behind it but how it looks and is organized on a PCB is where I get lost.

How did you do it? When building your first project based solely on a schematic, what did that look like? Breadboard first? Try, try, try maybe burn a few components but eventually you get there? As a rather newbie, building something solely from the schematic is very intimidating but I gotta start somewhere! Any help/thoughts/questions are appreciated!

 

[djmiggymigz]

Here's a pdf of the schematic I'm looking at in case the link doesn't work!

 

[djmiggymigz]

Also, side thought: what software do yall use to design and print custom pcb's? Maybe even just tinkering around in there would help me understand how things get laid out! I'm thinking/hoping something like blender but for PCB's exists. Googling now!

 

[djmiggymigz]

Talking to myself right now lol but: on KiCad now and this seems highly helpful! Draw out and copy the schematic, look at how it lays it out on a pcb!

 

[ruffrecords]

For a relatively simple circuit like the cloud lifter, your physical layout can be very similar to the schematic. You will notice that most of the components are vertical on the schematic apart from the semiconductors and a couple of capacitors. I would encourage you first to try building this circuit on Vero board which works pretty well if you layout the components as they are in the schematic.

Before you get into full blown CAD programs like Kicad I would suggest you look at Fritzing which will help you layout a Vero board design and then progress to PCB design (although, looking at the latest version, it looks like Vero board support has been dropped and replaced by protoboard support???)

Edit: Turns out Vero board or, as they call it, strip board, is still supported - phew!

Cheers

Ian

 

[djmiggymigz]

Okay awesome thanks for the reply. I'll give that a look as well! At what point do PCB layout start to not resemble the schematic layout? Is it just a matter of how much is going on and kind of the most economic/easiest way to lay it out?

To give a little context, the goal I'm working toward is building a 312 clone from scratch (with the addition of a trim before the output similar to 1073's. I have several schematic including the original from API and they look deceivingly simple! Really not much going on considering the value of the hardware however, I need to start somewhere simpler for sure.

 

[fragletrollet]

I'd consider EasyEDA as well, for both schematic drawing, PCB layout and even part selection/placement and PCB manufacturing integrated.

Free, and less intimidating than say Eagle.

 

[Whoops]

Looking for some help getting over the initial learning curve of reading and translating a schematic onto a breadboard/blank pcb.

There a lot of videos on Youtube where you can learn to do that,
nowdays I find youtube the best learning resource that exists.

Here are just 2 videos, but there's a lot of videos on youtube:

 

[Whoops]

Also, side thought: what software do yall use to design and print custom pcb's?

A lot of people use and like KiCAD.

In the past Ive used Eagle and that was popular, but I always found Eagle to be too outdated in it's user interface and not user friendly

 

[ruffrecords]

Okay awesome thanks for the reply. I'll give that a look as well! At what point do PCB layout start to not resemble the schematic layout? Is it just a matter of how much is going on and kind of the most economic/easiest way to lay it out?

Schematic layout is (should) be driven by the need to convey how the circuit operates - things like inputs on the left, outputs on the right, ground at the bottom and supplies at the top. None of these is relevant for PCB design. For example, some of the additional things a PCB needs to to are:

1. Be mounted somehow
2. Have input, output and power connectors plus controls in positions determined by things like how it fits in the enclosure, and the desired physical postion of the controls
3. Be designed for ease of assembly. This often means lining up passive components in rows (which is preferable for automated component insertion)
4. Take care of ensuring that power and ground reach the right places with minimum voltage drop.

To give a little context, the goal I'm working toward is building a 312 clone from scratch (with the addition of a trim before the output similar to 1073's. I have several schematic including the original from API and they look deceivingly simple! Really not much going on considering the value of the hardware however, I need to start somewhere simpler for sure.

Well, first the 312 uses an edge connector and a very specific size of PCB (two items not included on the schematic). It also has controls that need to be in very specific places in order to properly mate with the front panel.

Cheers

Ian

 

[TLK]

Many years ago where I worked, I had a seat license for a very expensive piece of software for PCB design called Protel. After years away from any PC board design, I recently designed a fairly simple electronic device that I sell using KiCad. KiCad is a good piece of software that will do everything you need. It does have a but of a learning curve, but it's a short one and there is plenty of KiCad help available with many YouTube videos. For those here that like to design PC boards, the place to get them manufactured at a minimal cost is JLCPCB.COM in China. I doubt you will beat the prices and quality is firat class. I recently re-ordered 10 pcs of a double sided thru hole board they previously manufacturered for me. Time from placing the re-order on line to finished boards arriving at my door was 7 days !

 

[blue_luke]

As usual Ruffrecords gives good advices.
I have been making PCB using Protel in DOS 3.0!! 40 years or so?
Now I am retired and I still do electronic designs and builds mostly for fun.
Electronic is still a passion for me.
So now I use KiCad https://www.kicad.org/ which is very potent and free, and it generates all the files needed by the pcb fabs, but most software works somehow on the same principle:
- draw the schematic
- specify all the required footprints
- generate the netlist and the component list
- import the netlist in the pcb design tool and at this point it is very important that you have no errors. To insure this run the "rule" check tool and go back to the component list and the connection list. Check especially for network that in your head are all the same but are different on the schematic.
To give you an example, GND, Gnd, Ground and GND1, GND2, are all different things,
Same with Vcc +V Vpos +15v etc are different so if you want these connected there should be a point on the schematic where the intended connections are made otherwise you will get error messages like "power source not connected","Power pins not connected" etc...

As Ian suggested, first place the connectors, switches, potentiometers etc... where they will go on the front/rear panel AND DO NOT FORGET THE MOUNTING HOLES ! I still do this mistakes!
Usually, I print the top layout and the silkscreen on the same sheet and I check if the main components like transformers, pot switches connectors etc how they will "look" on the board especially any mounting holes for connectors if any, the size of the holes for the pins etc...
It gives you also a good idea of the final dimensions. A 2X4 inches pcb projects a certain image in your head but there is nothing like seeing it in front of you!

Once you import the components they usually get placed all close together, I usually separate them by sections, say move a quad op-amp, you will note that the "ratnest" follows it, so now move all the other parts that are related to this chip and move that cluster somewhere NOT on the board.
Do the same for all other sections like regulators, power stages etc...
Then at this point you can consider moving these sections on the PCB.
The name of the game is to keep all the tracks short.
Use always at least 2 layer or more pcb , the cost of two layer stock is trivial and sometimes even less expensive than single sided board!
The reason for this is that each pad will be more sturdy because of the internal plating that acts as a small rivet so it reduce very much the tendency for a pad to lift from the board when repairing or removing components.
Make all traces on one side vertical, and on the other horizontal and then stick to it, using vias to go from one side to the other.
There is no rule as to which side, just decide on any reason you may have.

There is much more to it but your little project is a good first try but be aware that just the layout, especially using high impedance and high gain devices, will have an effect on noise, distortion, bandwidth, stability etc...

Luc

 

[Cqwet Dbdfte]

Here's a pdf of the schematic I'm looking at in case the link doesn't work!

17 parts on a PCB should be a super easy first project. Most of the time is to learn the program.
With SMT part only 11 parts possible with dual resistor and semiconductor packages.
The PNP is obsolete, SMT (dual) alternatives a plenty.
A postage stamp PCB size possible.
0805 size parts not too hard without a microscope.
Maybe like this...?

 

[djmiggymigz]

Wow thanks to everyone for the replies and advice!!

Progress report: I fully dived into and hyperfixated on KiCad. Got the schematic drawn out, figured out how to import some footprint that I needed as well as matching footprints to the components I've already bought. Then went on to PCB design and ordered 5 of them last night! Admittedly, I probably should have posted the draft here before ordering them but I was excited and it was cheap enough that I'm willing to send it and find out!

It was certainly a challenge at first to route all the tracks without intersections (which can't even happen), and then,, I figured out that you can lay tracks on both the front and the back!! Game changer. Then, I measured a few manufactured pcb's I have around and found that the tracks I was working with were incredibly tiny lol. So I blew my tracks to 1mm (I think at first they were literally like 0.06 mm). Then, had to redo the tracks since they no longer fit as I had them. Also found a very helpful github that automatically imported all the manufacturing constraints for JLC (I double checked and edited a few parameters).

Next breakthrough, I figured out how to add the ground plane inbetween all tracks and components. This brought the realization that any leads routed to ground were now fine where they were whereas before adding the ground plane, KiCad was wanting me to add tracks connecting all the grounded pins.

Also, another note is I'm designing this to fit inside a procraft case. So in terms of size and thus layout, that's the logic behind that. Major shoutout to DIYRE. This really isn't my work. I copied their schematic (which is listed under creative commons) and also did my best to copy their layout for the PCB. Stepping stones towards doing it all myself!

Going to attach screenshots here. Let me know what yall think! I hid the ground plane so that the tracks and component layout could be seen more clearly but its there as you can see in the 3D view. Blue is bottom, red is top tracks. I'm afraid that someones going to call out a mistake that's going to result in it not working lol but that's part of the process I suppose. Like @ruffrecords tagline says, gotta make mistakes!

 

[djmiggymigz]

I'm going to be trying to wrap this up before moving on because a) the learning process but also b) I dont want to start the next thign and never finish this lol. BUT, I already found some very helpful githubs that had the schematic and pcb templates for 500 series modules! So once I wrap this up I think I'm diving STRAIGHT into the 312 build because I'm so excited on it/this.

 

[Cqwet Dbdfte]

You have 2 layers, use them.

 

[djmiggymigz]

You have 2 layers, use them.

As in the top and bottom? I have tracks layed out on both the bottom and the top! Unless you're talking about something I haven't learned/found yet, already done! I was so excited when I figured out I could lay tracks on both the top and bottom lol

 

[Cqwet Dbdfte]

As in the top and bottom? I have tracks layed out on both the bottom and the top! Unless you're talking about something I haven't learned/found yet, already done! I was so excited when I figured out I could lay tracks on both the top and bottom lol

You have not made a single layer-to-layer jump with a via, to shorten the traces.
Traces are too close to pads.
Don't lay out your parts like an Excel spread sheet, put them like a signal flow. The schematic is a good guide.
Put input bypass caps (NPO/C0G types) close to the FET gates. Those FETs could be responding to RF.
Do not be afraid to rotate the parts to shorten traces.
Stitch top and bottom ground fills together with vias (name them the same as your ground net).
My example does not include any connectors, just 0.1" pitch pads, or any specific mechanical considerations.

 

[djmiggymigz]

Ok thank you for the direction. I don't actually know the function of vias at the moment so I'm going to go learn that! Also need to learn about nets, not sure what that's referring to either.

Forgot to hit send so UPDATE: Wow!! This is game changing. Figured out how to use the vias to jump over/under tracks and am shortening a bunch of my traces right now! Thank you again, this is going to be incredibly helpful when routing

 

[MidnightArrakis]

1) The -- acute angles -- that you see here in this image of your PCB-layout are also known as "acid traps"!!! These are a NO-NO!!!



What happens here is.....during the fabrication etching process, the acid that is used to etch the copper off of the laminate is caught inside these -- acute angles -- and ends up ever-so-slightly etching away the copper -- UNDERNEATH -- these angles. Over a period of time, the copper tracks at these points of your PCB may loosen and cause the PCB-track to actually pull-away from the laminate itself. What this means is.....you need to perform all of your track-routing to be be either at a 45-degree or a 90-degree angle.

In addition.....and, I am only assuming that this image may have been taken with the PCB at a slight angle, but.....this image shows that your component copper pad and your N/C Drill hole are -- NOT concentric -- meaning, they're not in perfect alignment with one another. In other words, the "white hole" and the "yellow pad" should be in perfect alignment (or, "concentric") with each other.

2) Your -- track-to-pad -- clearances are "WAY TOO CLOSE" than is necessary:

-- --
>> Don't be afraid to offer at least 15- to 20-mils of clearance between
your tracks and pads, especially on a layout as "loose" as this.

3) R8 is both placed and routed as a -- stub-route -- scenario:


>> The two upper-most yellow pads shown here are the component pads for R8 and the lower-left corner track that connects to another pad and then angles upwards to the upper-left at a 45-degree angle (also creating the "acute angle") is its same net connecting track. Since R8 is placed in the manner in which it is, technically.....it is -- NOT -- directly within the circuit's operation, but instead is "off-to-the-side", so to speak. While doing this may not much matter with a resistor, it -- DOES -- make quite a difference with capacitors!!! I have worked inside many engineering environments where the Electronics Engineers have literally shown me on their test equipment how the placing and routing of a component using a "stub-route" makes a difference in the circuit operation. And, this minute effect is additive as well. Meaning, the more components that are placed and routed using -- stub-routes -- the less the overall circuit behaves as it was designed to do!!!

However, while in your particular layout circumstance, it probably doesn't matter one hoot.....but, -- NOT -- placing and routing components in a --stub-route -- situation is a good habit to learn about and get into as you are learning the "PCB Design" ropes and techniques.

/