Feedback on schematic

[rHermes]

I made a simple circuit which is just a binary counter with a debouncer.


Afterwards I thought this would be a good exercise to try out in KiCad, so here is my first schematic:



I was just wondering if anyone have any feedback on the schematic (and circuit for that matter). Please be as harsh as you want, I have think skin and want to get better

Any feedback is much appreciated!

[Benta]

You'll need a resistor for each of the LEDs.

Apart from that: difficult to read, even for such a simple circuit. Try to arrange the parts in a left-to-right signal flow fashion, and cut down on the labels and use real connections instead.

Use the logic symbols for CD40106. Use the KiCAD library symbol for 74HC163, either standard or IEEE.

The only labels you really need are VDD and VSS, and only once.

Here's an example of my style of making schematics:

[S. Petrukhin]

My grumbling.
1. Two contacts PWR_flag would be good to note + and -.
2. SW_push does not say anything, I would write in their place "reset" and "inc".
3. The Vdd network is more often denoted by a special symbol in the form like T letter.
4. In the old days, when the circuits did not use flying networks and everything was drawn in solid lines, it was accepted Gnd at the bottom, and Vdd at the top. If you don't want oldskool to grumble, try not to flip Gnd and Vdd.
5. You won't need an inverter chip if you change the button scheme - just swap Gnd and Vdd on them.
6. If you write nRESET, it will be clear to everyone and you will not need to increase the node designation for the upper underscore.

[Benta]

6. If you write nRESET, it will be clear to everyone and you will not need to increase the node designation for the upper underscore.

This I decidedly don't like for a lot of reasons, but it's worth discussing. Petrukhin, we should open this in a new thread to avoid confusing the issue (and a beginner).

I'll start the party

[S. Petrukhin]

6. If you write nRESET, it will be clear to everyone and you will not need to increase the node designation for the upper underscore.

This I decidedly don't like for a lot of reasons, but it's worth discussing. Petrukhin, we should open this in a new thread to avoid confusing the issue (and a beginner).

I'll start the party

I have already noticed that you are a supporter of the old school of solid lines. There's nothing wrong with that. For public diagrams, this is even clearer and clearer to other people, but not always, sometimes the lines are very confusing to read the diagram. In industrial design, flying connections are quite convenient because the scheme is "secret" and no one needs to explain it.

Let's scare the newbie with an argument! 

[Benta]

I have already noticed that you are a supporter of the old school of solid lines. There's nothing wrong with that. For public diagrams, this is even clearer and clearer to other people, but not always, sometimes the lines are very confusing to read the diagram. In industrial design, flying connections are quite convenient because the scheme is "secret" and no one needs to explain it.

To me clarity and readability is #1 in a schematic, mainly for my own sake. If I come back to an old design 10 years later, I wan't to know what it does, as I've forgotten all about it in the meantime.
If it's about secrecy, then just burn it or never publish it.

[S. Petrukhin]

I have already noticed that you are a supporter of the old school of solid lines. There's nothing wrong with that. For public diagrams, this is even clearer and clearer to other people, but not always, sometimes the lines are very confusing to read the diagram. In industrial design, flying connections are quite convenient because the scheme is "secret" and no one needs to explain it.

To me clarity and readability is #1 in a schematic, mainly for my own sake. If I come back to an old design 10 years later, I wan't to know what it does, as I've forgotten all about it in the meantime.
If it's about secrecy, then just burn it or never publish it.

Drawing a complex device with solid lines, even with the use of bus, is not so simple and very cumbersome. Flying networks are more understandable for me personally. The diagram is displayed in function blocks, which gives clarity. Yes, they are fraught with the risk of missing the connection when reading the circuit, for example, not seeing all the signal consumers and having to scan the circuit to find out this issue. But only if they are poorly designed and scattered like peas. At the same time, driving your finger along a lot of lines or figuring out the exit from the bus is no less problematic.

[msat]

I've seen the method of using labels quite a bit, so I incorporated that in my most recent design. I'm basically a beginner too, so we might both benefit from each other and others.

BTW, I'm so used to seeing ground and VSS symbols pointing down that it would drive me nuts if I didn't do that. If you're the only one looking at your schematic and it doesn't bother you, then do whatever you want!

I separated and labeled sub-circuits as I felt it was the cleanest and easiest to read. But what someone might consider easy to read, someone else won't. So as I said, do what works for you, but if you're going to routinely share with others, then take a look at professional schematics (you can generally find dev board schematics from all the big MCU brands) and see how they do it.

[rHermes]

Thanks for all the feedback so far!

@Benta: Thanks for the feedback and the example circuit, it’s much appreciated! I have some questions though:

1. I have a resistor for each of the LEDs, R3, separating them from ground.
2. I searched for both in the kicad library, but found neither. I downloaded the lib files from digikey and mouser, and that is what I’ve used. When you say use from library, do you mean this one: https://kicad.github.io/symbols/74xx? Also when you mean use logic symbols, what does that mean? I found the 74LS163 in the library down, but I have the HC variant. Should I just use the LS one and rename it on the schematic?
3. I didn’t quite understand what you meant by using the labels only once. What would that mean in this circuit?

@S. Petrukhin: Thanks for the feedback! Some questions:

1. Do you mean that I should put ‘+’ and ‘-’ in text at the ground and +5VD nodes?
2. Great suggestion
3. Thanks for the tip, will do so!
4. I don’t want oldschool grumble, I’ll follow the convention from now on.
5. Yeah, this is something I’ve been thinking about. I’ve tired the circuit without it, but had problems with bouncing. What I found on the internet talked about using a schmitt trigger for debouncing normally high signals, but I know more about capacitors now, so I’ll give it a try and see if I can make it work without!
6. This one flew right over my head, sorry Mind explaining it a bit more? What is a node designation?

@msat: Thanks for the feedback and the example circuit!

I’ll make sure to follow the ground pointing down convention from now on, my bad  On the example circuit is each of the boxes a sub-circuit in kicad or have you just boxed them in? Great tip on looking up professional schematics from MCU brands!

[S. Petrukhin]

@S. Petrukhin: Thanks for the feedback! Some questions:

1. Do you mean that I should put ‘+’ and ‘-’ in text at the ground and +5VD nodes?
2. Great suggestion
3. Thanks for the tip, will do so!
4. I don’t want oldschool grumble, I’ll follow the convention from now on.
5. Yeah, this is something I’ve been thinking about. I’ve tired the circuit without it, but had problems with bouncing. What I found on the internet talked about using a schmitt trigger for debouncing normally high signals, but I know more about capacitors now, so I’ll give it a try and see if I can make it work without!
6. This one flew right over my head, sorry Mind explaining it a bit more? What is a node designation?

1. You have 2 control points with the same name PWR_FLAG, but these are different signals. PWR_FLAG+ and PWR_FLAG- will be better or Vdd, Gnd which is even more true.
5. Schmitt trigger can be non-inverting. Flipping the signal only confuses the circuit. When you have a complex circuit, it will be difficult for you to understand and remember what makes this CHIP a drawn square, and not a graphical representation of the Schmidt trigger.
6. Look here: https://www.eevblog.com/forum/beginners/signal-naming-styles-in-schematics/

Don't expect KiCad to give you all the tools and libraries. You'll have to draw some yourself. 

[rHermes]

@S. Petrukhin:

1. As far as I can tell in KiCad, you cannot rename the PWR_FLAG text. In the power menu it also seems to be the only component with the property that it tells ERC where power is coming from.
5. Ahh now i get it, instead of representing the circuit that I've made in the real world, I should put a representation of it, which in this case would be a simple schmitt inverter?
6. I read that thread, but I still don't know what: "not need to increase the node designation for the upper underscore" means 

[S. Petrukhin]

@S. Petrukhin:

1. As far as I can tell in KiCad, you cannot rename the PWR_FLAG text. In the power menu it also seems to be the only component with the property that it tells ERC where power is coming from.
5. Ahh now i get it, instead of representing the circuit that I've made in the real world, I should put a representation of it, which in this case would be a simple schmitt inverter?
6. I read that thread, but I still don't know what: "not need to increase the node designation for the upper underscore" means 

1. I don't know all the details of KiCad, I don't use it. Perhaps I didn't really understand which element is designated PWR_FLAG. I usually mark control points in this way.
2. The Schmidt trigger is much more convenient to see as an element, rather than in a box - see attached.
3. This discussion is a good indicator of how opinions may differ, that there are no strict standards on all issues, and that creativity and experience are often required. Even the harsh Soviet standards, which described everything that had to be strictly observed, did not always provide answers to questions. 

Don't be afraid of mistakes - they are useful as a source of experience. And a good source of knowledge, of course, is the work of professionals-to see how the design is made out. They, too, were once newbies, studied and followed the standards, including the tacit, is soaked in the experience of mankind. 

[Benta]

@Benta: Thanks for the feedback and the example circuit, it’s much appreciated! I have some questions though:

1. I have a resistor for each of the LEDs, R3, separating them from ground.
2. I searched for both in the kicad library, but found neither. I downloaded the lib files from digikey and mouser, and that is what I’ve used. When you say use from library, do you mean this one: https://kicad.github.io/symbols/74xx? Also when you mean use logic symbols, what does that mean? I found the 74LS163 in the library down, but I have the HC variant. Should I just use the LS one and rename it on the schematic?
3. I didn’t quite understand what you meant by using the labels only once. What would that mean in this circuit?

1: you have 5 LEDs. Then you need 5 resistors, one per LED.
2: using the standard KiCAD library, you click on the library tool on the right (the one that looks like an opamp). Then you click on the schematic. This will open the library. Whther you choose 74HC163 or 74LS163 is irrelevant, you can rename it later. It's still the same symbol.
3: you misunderstood, my fault for a bad explanation.

[Bud]

Make it one piece schematic, there is absolutely no reason to have 6 pieces with ports which make it hard to read.

[rHermes]

@Benta:

1. Ahhh, yeah I was thinking about this wrong! The voltage over the leds will be the same, but the current might not be and it won't be the 20 mA that I want. Thanks, total brain fart on my side!
2. Ah ok, thanks
3. If you don't mind me asking, what is the correct interpretation of the tip then?

[Benta]

@Benta:
3. If you don't mind me asking, what is the correct interpretation of the tip then?

The problem was, that placing labels all over the place does not improve readability, which is the goal of a schematic (a picture or a graphic is worth a 1000 words).

Your schematic was a sort of "graphic netlist", which is a bit of a hybrid. On a single sheet, make the connections. The labels belong to the outside world, like connecting to a different schematic sheet.

[msat]

On the example circuit is each of the boxes a sub-circuit in kicad or have you just boxed them in?

Yeah, just boxed them in and labeled the function of the subcircuits. I know it's all very simple so it was unnecessary, but I thought it was actually easier to follow along that way, while being cleaner. I have seen more traditional schematics (minimal labels) with subcircuits still boxed in with a quick description.

[Benta]

@rHermes:

Just for fun, I redrew your circuit to my satisfation, using the KiCAD library standard parts (took around 15 min. It's Corona time...).

What immediately stood out after redrawing is that your "debouncer" circuit wont work.

Here it is:

[S. Petrukhin]

@rHermes:

Just for fun, I redraw your circuit to my satisfation, using the KiCAD library standard parts (took around 15 min. It's Corona time...).

What immediately stood out after redrawing is that your "debouncer" circuit wont work.

Here it is:

You redrawn incorrectly 

[tooki]

@S. Petrukhin: Thanks for the feedback! Some questions:

1. Do you mean that I should put ‘+’ and ‘-’ in text at the ground and +5VD nodes?
2. Great suggestion
3. Thanks for the tip, will do so!
4. I don’t want oldschool grumble, I’ll follow the convention from now on.
5. Yeah, this is something I’ve been thinking about. I’ve tired the circuit without it, but had problems with bouncing. What I found on the internet talked about using a schmitt trigger for debouncing normally high signals, but I know more about capacitors now, so I’ll give it a try and see if I can make it work without!
6. This one flew right over my head, sorry Mind explaining it a bit more? What is a node designation?

1. You have 2 control points with the same name PWR_FLAG, but these are different signals. PWR_FLAG+ and PWR_FLAG- will be better or Vdd, Gnd which is even more true.

PWR_FLAG isn't a net name, it's a special "component" (actually, just a flag on a net) that tells KiCad that the net it's attached to is a power net. (Not that they're the same power net. It's literally just metadata saying "I'm a power net".) Apparently, KiCad uses this in ERC when making sure every component is powered.

[Benta]

You redrawn incorrectly 

You're right, corrected now. Like I said, a 15 min. job.

Jeez! You call me pedantic? Wow! 

[S. Petrukhin]

You redrawn incorrectly 

You're right, corrected now. Like I said, a 15 min. job.

Jeez! You call me pedantic? Wow! 

You are not a native German, and you are not yet imbued with German pedantry. 

[S. Petrukhin]

PWR_FLAG isn't a net name, it's a special "component" (actually, just a flag on a net) that tells KiCad that the net it's attached to is a power net. (Not that they're the same power net. It's literally just metadata saying "I'm a power net".) Apparently, KiCad uses this in ERC when making sure every component is powered.

Thanks. I'll know. I'm just planning to switch to KiCAD this year. 

[tooki]

PWR_FLAG isn't a net name, it's a special "component" (actually, just a flag on a net) that tells KiCad that the net it's attached to is a power net. (Not that they're the same power net. It's literally just metadata saying "I'm a power net".) Apparently, KiCad uses this in ERC when making sure every component is powered.

Thanks. I'll know. I'm just planning to switch to KiCAD this year. 

From what? After getting comfortable in EasyEDA and Altium, I find KiCAD to be needlessly complex and fiddly. (Though not impenetrable like Eagle.)

[S. Petrukhin]

PWR_FLAG isn't a net name, it's a special "component" (actually, just a flag on a net) that tells KiCad that the net it's attached to is a power net. (Not that they're the same power net. It's literally just metadata saying "I'm a power net".) Apparently, KiCad uses this in ERC when making sure every component is powered.

Thanks. I'll know. I'm just planning to switch to KiCAD this year. 

From what? After getting comfortable in EasyEDA and Altium, I find KiCAD to be needlessly complex and fiddly. (Though not impenetrable like Eagle.)

EasyEDA is very similar to KiCad, probably modeled on it and made. But there are already too many glitches and inconvenient moments in it. The last thing I didn't like was hiding the project through some clumsy other site, before it was just enough to choose "share". Direct selection of components from LCSC is very convenient, but increasingly limited and the price is already catching up with Mouser, for example. Altium is very bulky and expensive.

I used KiCad for a long time, but then I used EasyEDA for a long time - I'm drawn back. 

[Benta]

@tooki, Petrukhin, you're really going off topic!
Take this discussion to the KiCAD section, please.

It's not helpful to the OP.

[tooki]

PWR_FLAG isn't a net name, it's a special "component" (actually, just a flag on a net) that tells KiCad that the net it's attached to is a power net. (Not that they're the same power net. It's literally just metadata saying "I'm a power net".) Apparently, KiCad uses this in ERC when making sure every component is powered.

Thanks. I'll know. I'm just planning to switch to KiCAD this year. 

From what? After getting comfortable in EasyEDA and Altium, I find KiCAD to be needlessly complex and fiddly. (Though not impenetrable like Eagle.)

EasyEDA is very similar to KiCad, probably modeled on it and made. But there are already too many glitches and inconvenient moments in it. The last thing I didn't like was hiding the project through some clumsy other site, before it was just enough to choose "share". Direct selection of components from LCSC is very convenient, but increasingly limited and the price is already catching up with Mouser, for example. Altium is very bulky and expensive.

I used KiCad for a long time, but then I used EasyEDA for a long time - I'm drawn back. 

Definitely not. EasyEDA is very clearly modeled after Altium. Some dialogs even copy Altium's layout and oddball wording! EasyEDA is nothing at all like KiCAD. (I use Altium and EasyEDA frequently.)

Altium is costly (if you're not in education), and while it does have a learning curve, it still makes more sense than KiCAD or Eagle.

@tooki, Petrukhin, you're really going off topic!
Take this discussion to the KiCAD section, please.

It's not helpful to the OP.

It happens, and it's not entirely off-topic. (Nor would the KiCAD forum be unambiguously appropriate since it's a comparison of packages.)

[Benta]

It happens, and it's not entirely off-topic. (Nor would the KiCAD forum be unambiguously appropriate since it's a comparison of packages.)

Seriously? Your bickering about different EDA packages is on topic? Just because there's no general EDA forum on this site, you hijack a thread like this to to ride your hobby horse?

No.
Bad style.

[rHermes]

@rHermes:

Just for fun, I redrew your circuit to my satisfation, using the KiCAD library standard parts (took around 15 min. It's Corona time...).

What immediately stood out after redrawing is that your "debouncer" circuit wont work.

Here it is:

Thanks for the redrawing, but I see something that doesn't look quite right, you are pulling CEP and CET to ground, which will disable the counter.

Also, the debouncer circuit did work, what is it that shouldn't work?

[Benta]

Sorry, my mistake. like I said it was a 15 min. job, so I didn't bother to consult the datasheet. My purpose was more to show how a schematic could look using KiCAD.

EDIT: spent a couple of minutes correcting the schematic. Attached the .PDF as well as the .sch file for you to play with

[tooki]

It happens, and it's not entirely off-topic. (Nor would the KiCAD forum be unambiguously appropriate since it's a comparison of packages.)

Seriously? Your bickering about different EDA packages is on topic? Just because there's no general EDA forum on this site, you hijack a thread like this to to ride your hobby horse?

No.
Bad style.

Discussion ≠ bickering. And your complaints have now equaled the number of posts (excluding my responses to your complaints) that I had written on the topic. A discussion of what is and isn’t on-topic is even less on-topic than the EDA discussion. So you’re helping... how? Or just flexing your nuts trying to boss people around? (Which won’t succeed with me, mmkay? At least not with the tone you took when doing so.)

[Benta]

So you’re helping... how? Or just flexing your nuts trying to boss people around? (Which won’t succeed with me, mmkay? At least not with the tone you took when doing so.)

I've tried to help the OP, who's a newbie in schematic drawing/artwork, and hasn't got the full grip of EDA and KiCAD yet. I've even replicated his circuit in KiCad (with a couple of errors which have been fixed).

Where's your help?

I've reported your boorish/Trumpish response to the moderator.

[Bud]

Sorry, my mistake. like I said it was a 15 min. job, so I didn't bother to consult the datasheet. My purpose was more to show how a schematic could look using KiCAD.

EDIT: spent a couple of minutes correcting the schematic. Attached the .PDF as well as the .sch file for you to play with

Ground the unused logic inputs, it is a general practice to not leave them unconnected.

[S. Petrukhin]

So you’re helping... how? Or just flexing your nuts trying to boss people around? (Which won’t succeed with me, mmkay? At least not with the tone you took when doing so.)

I've tried to help the OP, who's a newbie in schematic drawing/artwork, and hasn't got the full grip of EDA and KiCAD yet. I've even replicated his circuit in KiCad (with a couple of errors which have been fixed).

Where's your help?

I've reported your boorish/Trumpish response to the moderator.

Herr Benta, stop grumbling. 

[wizard69]

Understand that the comments I'm abut to make come form somebody that has read more schematics and wiing diagrams than you could iaigne over the years.    These are both of the Electronics engineering mindset and the controls engineering mind set seen in automation so might not reflect what is normal here.

I made a simple circuit which is just a binary counter with a debouncer.


Afterwards I thought this would be a good exercise to try out in KiCad, so here is my first schematic:

I have to agree with others here.   Whenever possible use standard drawing elements and minimize the use of tags/labels/whatever you want to call them.   Simple schematics like this should have a minimal of tags/abels.

As for those labels there is a fine line between too many and not enough.   In general you want your schematic to flow from left to right and when that becomes an issue make use of labels.   The problem with labels is that it isn't always easy to find the other end so to speak.   It helps to make such labels large and distinctive.

I was just wondering if anyone have any feedback on the schematic (and circuit for that matter). Please be as harsh as you want, I have think skin and want to get better

Any feedback is much appreciated!

Some other thoughts that might ruffle a few feathers:

• It helps to distinguish human interface elements from others. In this regard don't tag a pushbutton switch to be used by humans with an SW prefix.    Use PB instead.   PB short for pushbutton of course.   It is a good habit to get into in m mind if you graduate to machine control you may have a hundred (possibly many more) ""switches"" of various types 
• Make use of large and thick fonts, for data entered on to the schematic.    This will save you a lot of grief as you age.   Further you can't expect that everybody that will read your schematic will have amazing eyesight.  This is perhaps one of the things that I run into the most using schematics from many sources. There is another factor that must be considered and that is reproduction capability.   I know his might shock a few people but paper still works well in the field and often those printouts are not to the original scale.   I'm talking about most text on a schematic.
• Make use of colors!    You have to be careful here as color blindness is real, however colors can really help separate out drawing elements if you don't have that issue.   However like many things you can go overboard, so have a plan.
• Create a column of numbers and a row of letters (or vs versa), to allow referencing coordinates on the schematic.    This seems to be more common in the industrial controls world but it can really help with communications with others.   The perfect example here is the ability to simply say that tag you can't find is at coordinates 5H.    This is done in some form or another world wide with industrial controls and I've seen this on conventional electronics type schematics also.   Now you may say that it isn't needed on a personal project and you are likely right but often this is incorporated into the template that sets up the border.   An example from the net: https://www.google.com/url?sa=i&url=http%3A%2F%2Feon.sdsu.edu%2F~johnston%2FEng_Graphics_Essentials_5th_Ed%2Ffiles%2Fege%2Fintro%2Fintro_page6.htm&psig=AOvVaw0-g_mJYNEwD1eWU4gsAfm1&ust=1610525361257000&source=images&cd=vfe&ved=0CAIQjRxqFwoTCPibp_b4le4CFQAAAAAdAAAAABAD   Hopefully that works.
• Sometimes you really need a short description beyond what would make sense for an item tag.   Many CAD solutions don't handle this well as ideally the short description becomes part of the element specified and would move with it.   Usually this is of benefit with I/O points.   Probably not applicable to this drawing but something that you should be aware of.