My First Schematic - Critique please!

Go To Last Post
24 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi All,

 

So I decided to jump in off the back of my previous post and have a go at doing my first schematic - and perhaps overly ambitious.

Goal:

Isolated USB<>UART adapter with TX inverted and shifted to 12V without need for additional power over that supplied by the USB BUS.

 

I've tried as best I can to follow some of the great advice here: Rules and guidelines for drawing good schematics

So (rightly or wrongly) I have copied and edited some of the IC symbol layouts to fit.

Alternative thought was to drop the LTC1751-5V, throw 5V through the ADuM's isolated DC-DC converter and then use an LDO to get a 3.3V source on the isolated side and chuck a BSS138 (or similar) to handle the 3.3V > 5V pre ADuM for the RX.
 

Would love to get some feedback, both in terms of style and technical (of which I'm sure there's many - USB ESD seemed to be a huge minefield of research..)

 

Thanks all.

 

Last Edited: Mon. Feb 22, 2021 - 02:32 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

As drawn, haven't you shorted USB D+ and D- together?

 

If so, I don't think you will see much USB traffic on the bus!

 

JC

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Looks very neat. Is Q1 really wired up that way?

John Samperi

Ampertronics Pty. Ltd.

https://www.ampertronics.com.au

* Electronic Design * Custom Products * Contract Assembly

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ah... Not a great start ! 

I replaced the IC with the one from the library and clearly missed the orientation and pinout change. *facepalm*

Thank you!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

 

JC in post #2 is trying to tell you that you have not connected the USB protection device correctly. Should be like this...

 

 

As C4 is large, I suspect that is a polarized item and should be drawn as such (like C8).

 

And JS was telling you that you have the collector and emitter of Q1 connected ass about. The emitter goes to ground.

 

And (sorry to be a pest), you should label the connector functions and the supply lines with their voltages. I did not check datasheets for the devices so don't know where your 12 volts come from.

 

And... I would probably put the fuse at the USB connector instead of after the connections to the USB protection device.

 

Ross McKenzie ValuSoft Melbourne Australia

Last Edited: Mon. Feb 22, 2021 - 04:10 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

What program are you using to create the schematic?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

bobioknight wrote:

What program are you using to create the schematic?

It says KiCad on the drawing.

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

As above; the transistor is upside down (should be emitter to ground, collector to the output), and the USB connector is shorting the signal: inputs should be on pins 1 and 3, outputs on 6 and 4.

 

Those voltage regulators U4 and U5 might be clearer if they were both drawn the same orientation.Do yo really need two? Possibly not...

 

But that said, a lot better than most first attempts we see. Nice one.

 

Neil

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hai All

 

barnacle wrote:
Those voltage regulators U4 and U5 might be clearer if they were both drawn the same orientation.Do yo really need two? Possibly not...

 

Yes,Since the ADuM5401 was isolated protection then only 1 DC-DC converter.

 

Nice schematic

 

Regards

JSB

 

.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

barnacle wrote:
As above; the transistor is upside down (should be emitter to ground, collector to the output)

Might have to disagree with that one - OPs intention I think is to buffer the (now isolated) TX output from FTDI chip. We don't want any signal inverting here. Perhaps an emitter-follower was the intention.

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0


That is pretty excellent.  A few tidbits (other than a few electrical mishaps):

 

avoid drawing 4-way connections...they can cause grave issues if not noticed, smeared, faded, or illuminated.  If your technician overlooks a 4-way, it can be a long hello to figure out why something isn't working.

Draw 3-way connections (T-connections) & maintain your sanity.

 

At least add places for pullup resistors on your switches---you will be GLAD you did.

 

U2 pin20 lacks a cap, as does its net going onwards to U3 

 

Add a led on the secondary...to u4, maybe to pgood (check if pgood is a open drain to turn on led/resistor, or other arragnement)....so you can see it has secondary enabled juice.

 

I'd slightly prefer the 3 LED's to point to the right or downward (especially since their source of current is emanating from their left)....current flowing to the right or down towards gnd when possible.

Seeing the current going through the leds towards the right feels better, but is below the bottom of the barrel in importance.

 

It's doubtful your caps C5/8/9 are polarized in 2021. 

 

this looks like an intentional connection to the pin:

 

This appears slightly less so (did you pause there to answer the phone & got distracted)

 

 

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

N.Winterbottom wrote:
OPs intention I think is to buffer the (now isolated) TX output from FTDI chip. We don't want any signal inverting here.

 

I may have misread his original intent, but:

 

Whiterat wrote:

Isolated USB<>UART adapter with TX inverted and shifted to 12V without need for additional power over that supplied by the USB BUS.

 

Neil

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Wow, thank you so much for all the feedback !

Despite my several faux pas it really is very encouraging to read laugh

 

So I've made a number of small changes:

 

1. Replaced U1 with USB6B1 (easier symbol to place)
2. Corrected Q1 orientation (indeed, it should be operating as a NOT gate!)
3. Rotated U4 to match U5
4. Added 0R pulldown resistors to switches for "just in case"
5. Replaced a number of tied grounds to individual or smaller groups
6. Added cap for U1
7. Rotated LED array
8. Having (re)read the ADuM datasheet, added parallel caps.
9. Tidied up pin connections that looked unintentional

 

TBD:
Labeling!

 

The reason for the 2 charge pumps on the isolated side is the LTC1263 (12V) required 5V input and I am stepping down 5V input on the AdUM5401 to 3.3V due to RX operating at 3.3V.

So I'm using the LTC1751-5 to get from 3.3V to 5V to feed the LTC1263.

(I really like the idea of inductorless charge pumps)

 

It would possibly (probably) be more efficient to do 5V-5V through the ADuM, add a 5V-3.3V LDO and shift RX up to 5V before passing through the ADuM. Thoughts?

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Whiterat wrote:

Isolated USB<>UART adapter with TX inverted and shifted to 12V without need for additional power over that supplied by the USB BUS.

So are you converting to RS232 levels ?

If so; what's wrong with the old fashioned MAX232 or perhaps a modern equivalent  ?

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

 

This looks great!  You are obviously taking the time to  do neat work...many can't spend more than 5 minutes at it  & won't bother to show any wired connections.

 

I think you meant to leave you switches alone and add pullup resistors...maybe.  Then your 3 switches can produce BOTH high level &  low levels.  Maybe you had other intentions.

 

Tie your spare UDM input & make a solder pad on the isolated side...then you have something for the future when you whish you had an isolated output pin...it is 100x easier to do now, rather than with a drill & hammer.

 

 

 

 

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

Last Edited: Mon. Feb 22, 2021 - 11:21 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

N.Winterbottom wrote:

So are you converting to RS232 levels ?

If so; what's wrong with the old fashioned MAX232 or perhaps a modern equivalent  ?

Ish. It's not strictly RS232 - just similar, and only for TX not RX. It's operating at 0-12V rather than -/+12V in RS232.

With regard to MAX232 or similar transceivers, unfortunately a lot of the charge pumps have a typical output of ~10V and the other end I'm connecting to has a hefty voltage divider before a darlington pair.

 

 

avrcandies wrote:

This looks great!  You are obviously taking the time to  do neat work...many can't spend more than 5 minutes at it  & won't bother to show any wired connections.

 

I think you meant to leave you switches alone and add pullup resistors...maybe.  Then your 3 switches can produce BOTH high level &  low levels.  Maybe you had other intentions.

 

Tie your spare UDM input & make a solder pad on the isolated side...then you have something for the future when you whish you had an isolated output pin...it is 100x easier to do now, rather than with a drill & hammer.

 

Thank you! I frequently draw network diagrams and I think it is a partially transferable skill in this regard!

I've seen several schematics where people separate each IC out and whilst I'm not against it, it does lose the flow/readability (for me at least)

 

Ahh sorry, I get you. They're pulled to VCC @10K on the device at the other end so seemed a little redundant to pull them high again. But otherwise 100%, floating pins = bad.

Great advice with regard to the spare isolated input, I hadn't thought of that! 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Did you change the part for the USB protection? The symbol and pinout differ from the original; I just wanted to be sure that was what you intended (noting that it needed re-pinning anyway).

 

Neil

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I did indeed !

Changing a part to fit the diagram rather than the diagram to fit the part may seem like a lazy approach, but these chips are much of a muchness anyway.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Whiterat wrote:
Changing a part to fit the diagram rather than the diagram to fit the part may seem like a lazy approach,

Hardly - Seems like extra work to me; plus; in my experience that's exactly where the errors creep in.

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

There's minimal difference between the two (USBLC6 vs USB6B1) - but I do accept your point that even seemingly minor changes have an element of risk involved.

 

Given the layout of the built in USBLC6 symbol, would it have been better practice simply to create a new symbol for USBLC6 that resembled USB6B1 more closely for ease ?

I just couldn't see a good way to place the built in symbol without causing quite a mess sad

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Rotate the symbol 90 degrees clockwise. A pins go to 1, B pins to 3; outputs from 6 and 4 respectively. The power rail connections leave to the sides and turn up and down respectively.

 

Just needs a little across, up (down), across, down (up) to get the inputs in the right place.

 

Certainly the symbol could have been better drawn.

 

Neil

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Went for a half and half approach (and added a polyfuse)

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Wonderful editing.   U1 pin 2 could be brought to the left, if you like.   Time to make a board!

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

avrcandies wrote:
Time to make a board!

 

Then we can all jump in and criticise your board! <rubs hands in anticipation>

 

Neil