Linear lab power supply

[JuanGg]

Like that? Or to the output ground?

(My resistor numbers don't mach yours R20 = R10)

[xavier60]

It's the other 10K, between the inverting input and ground.

[JuanGg]

I see, sorry. My mistake

[xavier60]

You should also add the CC LED. It can be very useful.  A CV LED also if there is space.

[xavier60]

As with my layout, there is an undesirable length of track between the shunt and the ground star point. Can you calculate the track resistance?
Try to make the track wider , also the tracks that interconnect the shunt resistors.

[xavier60]

The compromise I made with mine was to put the star point half way along the ground track. I also have 0.8mm solid copper wire soldered along its length. I measure the total resistance at about 1.5mΩ putting about 0.75mΩ in series with the shunt.
My star point is actually a single connection between the  control circuit's ground print and the  ground track.

[JuanGg]

I'll move things around as per your suggestions. Time for next version. Regarding CC and CV LEDs, I could measure this with the Arduino and show it on the displays (maybe on the mA one, as I will only be using 3 out 4 digits). I also have to think about measuring voltage and current as well. The Arduino has a 12 bit 10bit ADC with an internal reference if 1.1 V.   For measuring voltage, a simple resistor divider, and for current, maybe tapping off something at the input of the CC op amp.
I can calibrate errors in software.

    Juan

[xavier60]

I'll move things around as per your suggestions. Time for next version. Regarding CC and CV LEDs, I could measure this with the Arduino and show it on the displays (maybe on the mA one, as I will only be using 3 out 4 digits). I also have to think about measuring voltage and current as well. The Arduino has a 12 bit ADC with an internal reference if 1.1 V.   For measuring voltage, a simple resistor divider, and for current, maybe tapping off something at the input of the CC op amp.
I can calibrate errors in software.

    Juan

With my previous bench supply project, I put CC and CV LEDS on the regulator board as well as having the PIC monitor the CC op-amp.
With its layout, the shunt got positioned off the PCB and allowed the main current paths to run parallel from left to right. It is the floating type design with everything is referenced to the + output.
Amplifying the shunt voltage could be tricky. With my bench supply, I had split control rails. So I was able to use auto-zeroing op-amps, mainly because it's important to have low input offset and drift for the shunt amplifier. It wouldn't have been easy for me to correct errors in the code because I have only 10 bits.
You will need an op-amp that is rail to rail, input and output.
I got some OPA2192's to replace the TLC072 CC/CV op-amp in my bench supply, mainly to reduce offset error also.
The specs say "Rail-to-Rail Input and Output".  Its other specs would be an over kill for your application though, its high speed and high output current.

[JuanGg]

LM358 op amp is rail to rail. I am running out of space on the board if I want to get it manufactured (prices go right up out of the 100 x 100 mm size) I see what I can fit. I'll have to mount the shunt resistors vertically, and the regulators as well. This is where I'm at:

    Juan

[Kleinstein]

The LM358 is not rail to rail, it is an single supply OP only.  For the circuit likely used, this is not a problem, as there is no need to go close to the positive supply. The OPA2192 would be rail to rail - however it is still relatively expensive. The OPA2171 would be a cheaper, though less precise alternative.

For making the  board smaller one could change the non critical resistors and capacitors (e.g. at the regulators) to SMD form factor.  This can safe quite a bit of space. Size 0805 is not that difficult to solder by hand. For manual placement and soldering, there is no big penalty for mixing THT and SMT. If available I even tend to prefer THT chips and SMD passives (expect electrolytic).

[JuanGg]

The LM358 is not rail to rail, it is an single supply OP only.  For the circuit likely used, this is not a problem, as there is no need to go close to the positive supply. The OPA2192 would be rail to rail - however it is still relatively expensive. The OPA2171 would be a cheaper, though less precise alternative.

For making the  board smaller one could change the non critical resistors and capacitors (e.g. at the regulators) to SMD form factor.  This can safe quite a bit of space. Size 0805 is not that difficult to solder by hand. For manual placement and soldering, there is no big penalty for mixing THT and SMT. If available I even tend to prefer THT chips and SMD passives (expect electrolytic).

Right, I got confused with another datasheet (LMV358). LM358 comon mode voltage range does include ground. Pinouts seem standard, so I could change which op-amp I use later on. It seems I can fit everything on the space I have (and THT resistors are handy for jumping traces). The TLC072 op amps only came on smd.
    Juan

[Kleinstein]

For jumping traces SMD resistors in 1206 size also work.  If just for a single private used circuit one can even solder 0805 parts to the slightly larger 1206 taps.  It's extra mechanical stress to the parts, but should be OK for resistors, if no too much solder is used.

The OP pinout is pretty standard with most types.  One trap for the young players here is the LT1013 - in SMD (SO8) it has a different pinout.

[xavier60]

LM358 op amp is rail to rail. I am running out of space on the board if I want to get it manufactured (prices go right up out of the 100 x 100 mm size) I see what I can fit. I'll have to mount the shunt resistors vertically, and the regulators as well. This is where I'm at:

    Juan

The layout is looking more tidy.
Some space can be saved by using narrower tracks around the driver transistors.
I had to use adapters for the OP2192 op-amps, https://i.ebayimg.com/images/g/0XkAAOSwtfhYqoh0/s-l300.jpg
I solder 0.5mm wire  into the holes so I can put them into a standard DIP socket.
I tried an OP2192 in the current power supply project. It worked no differently to the TLC072 as expected.
With both types, I have seen the inputs of the CC op-amp go down to -0.4V with no problem.

[JuanGg]

The layout is looking more tidy.
Some space can be saved by using narrower tracks around the driver transistors.
I had to use adapters for the OP2192 op-amps, https://i.ebayimg.com/images/g/0XkAAOSwtfhYqoh0/s-l300.jpg
I solder 0.5mm wire  into the holes so I can put them into a standard DIP socket.
I tried an OP2192 in the current power supply project. It worked no differently to the TLC072 as expected.
With both types, I have seen the inputs of the CC op-amp go down to -0.4V with no problem.

And the tydiness goes down the drain... I have added the micro, PWM filtering, connectors... The only thing missing is the current measuring. I have half of a LM358 left. I didn't terminate it in case it could be used for that. I have attached my current schematics as well.
I bought those adpters to, I'll maybe change the SOIC outline for a DIP one just in case.
This is taking some effort, and I hope it works out. Do I go ahead and prototype the CV part on perfboard, or will it work for sure on a manufactured PCB?

    Juan

[Kleinstein]

The PWM filter is rather low impedance with 1 K and 1 µF.  Even with the LM358 one can use larger resistors like 10 K or 22 K.  If one has an OP, one could also use a proper 2nd or  3rd order active filter to get less residual ripple.

The CV part is not that complicated. The main uncertainty is in some resistor or capacitor values.  So one could include the CV part on the board. If for some odd reason it would not work as expected one could still keep it unpopulated and add the CV part separate.

[JuanGg]

The PWM filter is rather low impedance with 1 K and 1 µF.  Even with the LM358 one can use larger resistors like 10 K or 22 K.  If one has an OP, one could also use a proper 2nd or  3rd order active filter to get less residual ripple.

The CV part is not that complicated. The main uncertainty is in some resistor or capacitor values.  So one could include the CV part on the board. If for some odd reason it would not work as expected one could still keep it unpopulated and add the CV part separate.

I still have some space left on the board, so I could use a more complex filter. I have to do some reading on that. I just did it that way on my electronic load and it worked fine.

I definitely prefer getting the PCB made and then change a couple values or cut a couple traces than making a full prototype first. I just want to make sure I don't make any stupid mistakes.

    Juan

[xavier60]

The layout is looking more tidy.
Some space can be saved by using narrower tracks around the driver transistors.
I had to use adapters for the OP2192 op-amps, https://i.ebayimg.com/images/g/0XkAAOSwtfhYqoh0/s-l300.jpg
I solder 0.5mm wire  into the holes so I can put them into a standard DIP socket.
I tried an OP2192 in the current power supply project. It worked no differently to the TLC072 as expected.
With both types, I have seen the inputs of the CC op-amp go down to -0.4V with no problem.

And the tydiness goes down the drain... I have added the micro, PWM filtering, connectors... The only thing missing is the current measuring. I have half of a LM358 left. I didn't terminate it in case it could be used for that. I have attached my current schematics as well.
I bought those adpters to, I'll maybe change the SOIC outline for a DIP one just in case.
This is taking some effort, and I hope it works out. Do I go ahead and prototype the CV part on perfboard, or will it work for sure on a manufactured PCB?

    Juan

Although I have done a lot of testing here, I would prefer that you test the CV loop at least  before committing it to a PCB.
I still need to test with a larger group of TIP35C's which I don't expect to see for a week or so.

[JuanGg]

  Although I have done a lot of testing here, I would prefer that you test the CV loop at least  before committing it to a PCB.
I still need to test with a larger group of TIP35C's which I don't expect to see for a week or so.

Thanks again for doing so. I'll do just that, although I won't be able to until next week or so.
    Juan

[JuanGg]

Regarding PCB grounding, should I add a groundplane or keep the star grounding as is? I have been doing some reading on the subject and there are different views.
   Juan

P.d: happy 2019!

[Kleinstein]

For a linear lab supply the star ground (or similar) is usually more suitable than a ground plane - especially a bad ground-plane can be a real pain.

[JuanGg]

With my current layout, digital ground return looks like below. That can't be any good. As I have clearly separated analog and digital sections, should I separate grounds in any way? Also, no current should flow between the output ground and the regulator's ground, should I move the star point?
Or maybe I should have separate digital and analog groundplanes, joined under the traces going from one section to the other?
8 V reg is only for analog, while 5V one is only digital, I should separate those too.

Thank you.
    Juan

[xavier60]

Unless someone has a better idea, I would link AUX reg ground to Digital ground to main star point.
The 12V regulator should be placed on the left so that fan current has the shortest path in and out.
Regulator input bypass capacitors can inject some ripple current into ground rails.
One input bypass capacitor that is carefully placed is sometimes best.
Are you panning to temporarily power the AUX regulators from the main unregulated rail at all?

[JuanGg]

Unless someone has a better idea, I would link AUX reg ground to Digital ground to main star point.
The 12V regulator should be placed on the left so that fan current has the shortest path in and out.
Regulator input bypass capacitors can inject some ripple current into ground rails.
One input bypass capacitor that is carefully placed is sometimes best.
Are you panning to temporarily power the AUX regulators from the main unregulated rail at all?

Ok, so all digital grounds tied together, and then to star point. Each analog ground to star point. Fan connector and transistor is as close as it can be to the 12 V reg. I am not planning on powering the aux regulators from the main unregulated supply, as I have all transformers and rectifiers set up.
I will make a couple changes and include a single input bypass cap. BTW, will the op-amp need a bypass cap?

    Juan

[xavier60]

I have to be certain that we are not misunderstanding each other. Ill see If I can make a sketch.
 I don't bother with bypass capacitors for op-amps because my PCBs are usually small. It's difficult to say at what power track length an op-amp will suddenly need a capacitor.
But when a capacitor is added, a HF loop is formed and needs to be broken with resistor or choke in series with the supply rail.  You can make provision for the parts and fit them if necessary.

[xavier60]

Ideally the the digital to analog ground path should not carry any currents but it's difficult to avoid.
The return current path current for the 8V is low and doesn't fluctuate much at all.
Even a possible HF loop isn't really a big problem because the 100nF capacitor would filter a lot of it out at the CV op-amp.