Isolated fixed low voltage power supply and serial interface

[kehribar]

Hi All.

I designed an isolated fixed low voltage power supply and serial interface board. Design idea is coming from Dave's uSupply board: http://eevblog.com/files/uSupplyUSBrevB.pdf He used optocoupler whereas I used a dedicated isolator IC. You can find the eagle based schematic and layout files attached.

Sometimes i need to send ADC results to the PC for further analysis but also I don't want to inject noise to my measurement system from PC ground. Isolated serial link is perfect for this. Also i used a very low noise LDO - LT1763 - which can be used to supply power to host circuit. Lastly, 1V65 supply can be used in single supply opamp based circuits.

I guess this will be a very usefull little tool which helps people to prototype their low noise measurement circuits.

What do you say? Comments are welcomed.

Best,
ihsan.

[Dave]

You should put component values (resistors and caps) on the schematic. You also might want to omit the text (email address?) on the bottom copper layer. It just reduces the effective isolation distance. Put it somewhere else, or make it a silkscreen instead.
Other than that, it looks great.

[David_AVD]

Rotating the USB chip 90° CCW would make for a neater (shorter) traces in that area?

[mariush]

I don't understand why use the op-amp to get 1.65v and why you'd use such a weird regulator (with difficult to solder footprint).

A simple generic 1117-33 in to252/to-263/dpak form

for example
http://www.digikey.com/product-detail/en/NCP1117DT33G/NCP1117DT33GOS-ND/1483318
http://www.digikey.com/product-detail/en/LM1117DT-3.3%2FNOPB/LM1117DT-3.3%2FNOPB-ND/363583

would work just the same and be easier to heatsink with just some copper pad under it. It's not like you won't waste just as much power as heat with that LT1763 getting 3.3v out of 5v, yet you just make it harder to solder it on the board.
The 1.65v could be done with a plain 1117 adjustable in to-261 form :
http://www.digikey.com/product-detail/en/LM1117IMPX-ADJ%2FNOPB/LM1117IMPX-ADJ%2FNOPBCT-ND/3440162
http://www.digikey.com/product-detail/en/SPX1117M3-L/1016-1235-5-ND/2411167

Basically , rather than using 3 separate parts with capacitors and resistors, you reuse same component, reduce bom, get better prices etc.

later edit:

move the traces for rx,tx,rs all the way to the side, move the 3.3v regulator just a bit more to the center with the heatsink tab kinda where those 4 capacitors are, and  your input and output capacitors by the insulation gap, away from heat. you'll have a larger area to act as a heatsink.

I'd probably put the rx,tx,rs, gnd, 3.3v on the far right side, aligned to a side and maybe with a 2row 10pin header (but 1 row, 5 pin is also ok) so that you could use commercially available cables (0.1" / 2.54mm spacing), or to just press fit it into a breadboard without blocking the whole breadboard.
Some space further to the right corner , put the gnd , 1.65v , 3 v .. again aligned at 0.1" (2.54mm, for breadboard) ... basically make it as if the holes are a DIP14 or something like that, with the middle pins missing.

Even if you don't care about breadboard, if the pins are all on one side it would be better because the pcb won't flip on the desk due to cable weight and it would use less desk space (the cables for serial won't get on the outside of the board, don't know if I explain it properly)

[David_AVD]

What is the 1.65V for anyway?  The only thing I saw connected to that was an LED which is unlikely to work at that voltage anyway unless it's red.

[mariush]

I've edited a bit my post above in the meantime.

David, I think he wants it for biasing opamps : http://www.analog.com/library/analogdialogue/archives/35-02/avoiding/index.html

later edit... one more thing.

It looks like you're powering the isolator from the usb-serial ic , that's ... weird but ok I guess.

One potential problem I see is that it seems ftdi's absolute maximum input voltage is 5.5v which is really small. You could get this high even on computers.
I have a chinese usb charger on my desk that outputs 5.7v at low load, and I guess it could be quite possible for someone to just want a 3.3v power source for a microcontroller without caring about the serial stuff.
The ftdi would work just fine at 3.3v bypassing it's 3.3v regulator so I don't see what's the hard of using a standalone 1117-33 to regulate the voltage before it goes to the serial and isolators, and a regulator like this would tolerate higher voltage.

[Dave]

I found another one, and this one is sneaky.
Tie one of the CBUS pins on the FTDI to ground. Why? These chips sometimes unexpectedly go into suspend mode, for no good reason. The way to prevent this is by setting one of the CBUS pins to function as #KEEPAWAKE input and tying it to GND.
Read all about this in the errata technical note.

[codeboy2k]

The idea looks sound, surely if it's useful to you then it's great that you open source it and it can become useful to others too..

I'd follow mariush's advice and just use a variable voltage regulator for the 1.65 volts, not an op-amp.  You could pull out the 5V from the CUI DC/DC converter, you might one day want that off-board too.

@Begin(Rant)

Also, I wish people would stop drawing schematics like you did... that's not a schematic.  It's just a bunch of parts with named nets, and we have to hunt all over it to see the connections.  Your schematic is small so it's not that hard to follow, but other people do this too on much bigger drawings.

I see so many schematics on the net like this...it's not necessarily your fault, perhaps you are following the status quo.. but I think that people are abusing the ability to name nets by drawing it this way.

All circuits have a logical flow of electrons; the schematic should convey this.  It should not match the physical layout; the PCB editor is good at doing that. 
I hate parts that are made of just square boxes with their pins in numerical order around the box from 1-8 and 8-16 like a DIP package.  In the part editor, the  pins can be re-ordered, the  power and ground can be top and bottom, the inputs can be on the left, the outputs on the right.. they can be split into multiple boxes if needed...

The schematic tools help to do this, and the circuit flow is much more easily visualized.

@End(Rant)

(rant markup courtesy of Scribe from my Vax/VMS days)

[kehribar]

You should put component values (resistors and caps) on the schematic. You also might want to omit the text (email address?) on the bottom copper layer. It just reduces the effective isolation distance. Put it somewhere else, or make it a silkscreen instead.
Other than that, it looks great.

Hi,

You are right, i should better move my mail address to bottom silkscreen. No need to ruin the isolation

Also, yes I should add the component values on the schematic. I know the values by heart but since this is a public release, i should behave accordingly.

Best,
ihsan.

[kehribar]

To all "why 1v65 rail and why you used an opamp to generate this?" questions,

I will be using this voltage for single supply opamp biasing applications. For example Dave's uCurrent uses an opamp based voltage rail splitter and many other portable circuits uses the same approach. I wanted to emulate that as much as possible. You wouldn't use a voltage regulator in your portable circuit to generate virtual ground in general.

Also,

Driving an LED with 1v65 might not be good idea. Thanks for the warning. I should better be looking at V_forward of the indicator LED.

ihsan.

[kehribar]

I've edited a bit my post above in the meantime.

David, I think he wants it for biasing opamps : http://www.analog.com/library/analogdialogue/archives/35-02/avoiding/index.html

later edit... one more thing.

It looks like you're powering the isolator from the usb-serial ic , that's ... weird but ok I guess.

One potential problem I see is that it seems ftdi's absolute maximum input voltage is 5.5v which is really small. You could get this high even on computers.
I have a chinese usb charger on my desk that outputs 5.7v at low load, and I guess it could be quite possible for someone to just want a 3.3v power source for a microcontroller without caring about the serial stuff.
The ftdi would work just fine at 3.3v bypassing it's 3.3v regulator so I don't see what's the hard of using a standalone 1117-33 to regulate the voltage before it goes to the serial and isolators, and a regulator like this would tolerate higher voltage.

I don't want people to use this with a wall wart USB plug. This is a design choice. But thanks a lot for indicating your concern! Also if someone needs a simple USB based power supply they can use something like this: http://www.seeedstudio.com/depot/5v33v-breadboard-power-supply-p-566.html

For the regulator part:

FT230x has its own voltage regulator output and I didn't want to put an another regulator IC to prevent redundancy.

Also,

Pre-uno Arduino boards were using FT232's 3V3 regulator output to its 3V3 pinheader. It can't provide much current but many circuits worked perfectly with this output.

ihsan.

[kehribar]

Rotating the USB chip 90° CCW would make for a neater (shorter) traces in that area?

Thanks for the warning! I'll give it a try

Best
ihsan.

[kehribar]

I don't understand why use the op-amp to get 1.65v and why you'd use such a weird regulator (with difficult to solder footprint).

A simple generic 1117-33 in to252/to-263/dpak form

for example
http://www.digikey.com/product-detail/en/NCP1117DT33G/NCP1117DT33GOS-ND/1483318
http://www.digikey.com/product-detail/en/LM1117DT-3.3%2FNOPB/LM1117DT-3.3%2FNOPB-ND/363583

would work just the same and be easier to heatsink with just some copper pad under it. It's not like you won't waste just as much power as heat with that LT1763 getting 3.3v out of 5v, yet you just make it harder to solder it on the board.
The 1.65v could be done with a plain 1117 adjustable in to-261 form :
http://www.digikey.com/product-detail/en/LM1117IMPX-ADJ%2FNOPB/LM1117IMPX-ADJ%2FNOPBCT-ND/3440162
http://www.digikey.com/product-detail/en/SPX1117M3-L/1016-1235-5-ND/2411167

Basically , rather than using 3 separate parts with capacitors and resistors, you reuse same component, reduce bom, get better prices etc.

later edit:

move the traces for rx,tx,rs all the way to the side, move the 3.3v regulator just a bit more to the center with the heatsink tab kinda where those 4 capacitors are, and  your input and output capacitors by the insulation gap, away from heat. you'll have a larger area to act as a heatsink.

I'd probably put the rx,tx,rs, gnd, 3.3v on the far right side, aligned to a side and maybe with a 2row 10pin header (but 1 row, 5 pin is also ok) so that you could use commercially available cables (0.1" / 2.54mm spacing), or to just press fit it into a breadboard without blocking the whole breadboard.
Some space further to the right corner , put the gnd , 1.65v , 3 v .. again aligned at 0.1" (2.54mm, for breadboard) ... basically make it as if the holes are a DIP14 or something like that, with the middle pins missing.

Even if you don't care about breadboard, if the pins are all on one side it would be better because the pcb won't flip on the desk due to cable weight and it would use less desk space (the cables for serial won't get on the outside of the board, don't know if I explain it properly)

Hi,

LT1763 was chosen because of its very low noise characteristic. http://cds.linear.com/docs/en/datasheet/1763fg.pdf Datasheet indicates 20uV RMS noise. And out of curiosity, why do you say LT1763 has a "difficult to solder footprint" ? It has an SOIC8 footprint. Am i missing something?

And also the heatsink,

I don't think that I will prototype any circuit with this device that will require intensive heatsink for the voltage regulator. But again, thanks for your consideration!

For the pinheader alignment, I want to create 'shield like' measurement circits. With this approach two headers lies at two different sides and they can share the weight of the "shield"more easily.

Best,
ihsan.

[kehribar]

I found another one, and this one is sneaky.
Tie one of the CBUS pins on the FTDI to ground. Why? These chips sometimes unexpectedly go into suspend mode, for no good reason. The way to prevent this is by setting one of the CBUS pins to function as #KEEPAWAKE input and tying it to GND.
Read all about this in the errata technical note.

Thanks for the warning!!

Best,
ihsan.

[kehribar]

The idea looks sound, surely if it's useful to you then it's great that you open source it and it can become useful to others too..

I'd follow mariush's advice and just use a variable voltage regulator for the 1.65 volts, not an op-amp.  You could pull out the 5V from the CUI DC/DC converter, you might one day want that off-board too.

@Begin(Rant)

Also, I wish people would stop drawing schematics like you did... that's not a schematic.  It's just a bunch of parts with named nets, and we have to hunt all over it to see the connections.  Your schematic is small so it's not that hard to follow, but other people do this too on much bigger drawings.

I see so many schematics on the net like this...it's not necessarily your fault, perhaps you are following the status quo.. but I think that people are abusing the ability to name nets by drawing it this way.

All circuits have a logical flow of electrons; the schematic should convey this.  It should not match the physical layout; the PCB editor is good at doing that. 
I hate parts that are made of just square boxes with their pins in numerical order around the box from 1-8 and 8-16 like a DIP package.  In the part editor, the  pins can be re-ordered, the  power and ground can be top and bottom, the inputs can be on the left, the outputs on the right.. they can be split into multiple boxes if needed...

The schematic tools help to do this, and the circuit flow is much more easily visualized.

@End(Rant)

(rant markup courtesy of Scribe from my Vax/VMS days)

As i said before the idea comes from the Dave's uSupply. This is something like subset of his circuit with couple of modifications

For your rant,

I hear your point but I prefer this way. It's easier to follow for me

Best,
ihsan.

[ve7xen]

I don't understand why use the op-amp to get 1.65v and why you'd use such a weird regulator (with difficult to solder footprint).

I can think of a couple reasons why you might use an opamp here instead of a series regulator:

- push-pull output, since his intended use as (presumably) a virtual ground may need to sink current
- proportional output voltage tracks Vcc

It's not really any extra cost nor extra parts (might be one less BOM line in fact, since the resistors will be the same value), and given this is a reference voltage, not a power supply, the opamp makes more sense to me.

Driving an LED with 1v65 might not be good idea. Thanks for the warning. I should better be looking at V_forward of the indicator LED.

If you feel the need for an indicator LED, I'd just use an NPN in the cathode. It's a couple more parts, but will work with any LED. 1.65V is iffy even for low Vf LEDs.

For the pinheader alignment, I want to create 'shield like' measurement circits. With this approach two headers lies at two different sides and they can share the weight of the "shield"more easily.

I would design this so you at least have the option of using a breadboard without taking up too much breadboard space. Maybe move the output header to the 'top right' as shown and the serial to the right edge, then you can plug the board into the top right corner of a breadboard and not lose much space. The serial pins can be on the top or top right angle style to not interfere with plugging into the breadboard.

[mariush]

LT1763 was chosen because of its very low noise characteristic. http://cds.linear.com/docs/en/datasheet/1763fg.pdf Datasheet indicates 20uV RMS noise. And out of curiosity, why do you say LT1763 has a "difficult to solder footprint" ? It has an SOIC8 footprint. Am i missing something?
[..]
I don't think that I will prototype any circuit with this device that will require intensive heatsink for the voltage regulator. But again, thanks for your consideration!

The LT1763 is available in DFN - 12-Lead Plastic DFN (4mm × 3mm) - or S8 8-Lead Plastic Small Outline (Narrow .150 Inch)

I could only find it on Digikey and reputable stores in the first footprint.

The isolated power supply  can only do about 0.4A at around 5v, and it will be noisy. Probably LT1763 would filter that to some extent, but does it really matter that much?

Anyway, LT1763 is still a linear voltage regulator. If you get 5v in , 3.3v out, at 0.4a you have 0.7 watts to dissipate as heat. Go to page 18 in your datasheet and see the math done for s8 and 0.71 watts dissipation.... and keep in mind that's done for 2500mm² of copper on the pcb or about a square of 5 cm and it will still be very hot.
Granted, you won't use 0.4 amps all the time but the point is you still need pcb space for heatsink purposes and you have to be careful with surface mounted ceramic capacitors and how their capacitance changes when the pcb heats up (see page 16 in datasheet) and how load regulation varies with the temperature and so on.

A regulator in DPAK or to252 etc have larger footprint through which they can dissipate heat, so they'll dissipate heat faster and won't heat as much but I agree they probably won't do as low as 20uV.
 

[kehribar]

LT1763 was chosen because of its very low noise characteristic. http://cds.linear.com/docs/en/datasheet/1763fg.pdf Datasheet indicates 20uV RMS noise. And out of curiosity, why do you say LT1763 has a "difficult to solder footprint" ? It has an SOIC8 footprint. Am i missing something?
[..]
I don't think that I will prototype any circuit with this device that will require intensive heatsink for the voltage regulator. But again, thanks for your consideration!

The LT1763 is available in DFN - 12-Lead Plastic DFN (4mm × 3mm) - or S8 8-Lead Plastic Small Outline (Narrow .150 Inch)

I could only find it on Digikey and reputable stores in the first footprint.

The isolated power supply  can only do about 0.4A at around 5v, and it will be noisy. Probably LT1763 would filter that to some extent, but does it really matter that much?

Anyway, LT1763 is still a linear voltage regulator. If you get 5v in , 3.3v out, at 0.4a you have 0.7 watts to dissipate as heat. Go to page 18 in your datasheet and see the math done for s8 and 0.71 watts dissipation.... and keep in mind that's done for 2500mm² of copper on the pcb or about a square of 5 cm and it will still be very hot.
Granted, you won't use 0.4 amps all the time but the point is you still need pcb space for heatsink purposes and you have to be careful with surface mounted ceramic capacitors and how their capacitance changes when the pcb heats up (see page 16 in datasheet) and how load regulation varies with the temperature and so on.

A regulator in DPAK or to252 etc have larger footprint through which they can dissipate heat, so they'll dissipate heat faster and won't heat as much but I agree they probably won't do as low as 20uV.

Hi,

I can find the SOIC8 version of the LT1763-33 from this link: http://www.digikey.com/product-detail/en/LT1763CS8-3.3%23PBF/LT1763CS8-3.3%23PBF-ND/891881

Thanks for indicating very useful parts from the datasheet! I don't think that i change my mind from this regulator since I _really_ don't expect to see more than 100 mA with the prototypes I'm working on with this device. Also , even though wheter my layout will help me to achive that level or not, 20uV noise level is an absolute plus for me.

By the way,

To all you people; thanks a lot for your great contributions and sharing your ideas/comments! I'm getting to like this place

Best,
ihsan.

[kehribar]

Hi All,

Please take look at the updated version of the layout and schematic

What do you think now?

Best,
ihsan.

[kehribar]

Any comments about the new design that I've post before?

[Legit-Design]

If you are proud of it, then build it up and tell us how it performs?

[kehribar]

If you are proud of it, then build it up and tell us how it performs?

Who said I wasn't proud of my design? Nevermind ...

Best,
ihsan.