Some EE opinions please

[Incoherent]

Originally Posted by Groth

Hah, looks like you're designing a plate of spaghetti! What software are you doing the schematics with? They look great.

Generally looks good to me. What sort of the currents are you running through your heater? Might be better to move your current sensing shunt off board.

If you don't do the digital ins and outs yet, how about leaving yourself solder pads or a header that gives access to +5/ground/p-port lines. That way you could attach a daughter card later.

It's free software from ExpressPCB. Quite OK, you can link the schematic to the PCB layout. I'm still learning that part.

The heater current will max out at about 8-10amps, probably a little high to be on board but I am a little worried about connection resistance buggering up the readings. What do you think? The currents around this circuit are very low (10-100µA area), probably a prime candidate for a bit of inductive crosstalk. Any thoughts on reducing this if I did keep it on board. It is all effectively DC of course.

You are right regarding digital i/o, it'd be a bit silly to not give myself at least the future possibility.
I am debating now whether to optocouple the digital side. The added circuit complexity does not appeal.

Been looking at precision resistors, they are not cheap (~$3 each here in Sweden) for 0.1% <5PPM/*C metal film. I'm wondering whether your frypan sorting technique will be applicable here if I used the far cheaper 1% 50PPM/*C ones.

Originally Posted by Groth

... If you can, pick a low power single supply amp and run it off your Vref (may require a beefier voltage follower); that way the ADC inputs are guaranteed be to be with bounds.

Been thinking, actually theres no real reason why I can't use a 5v reference, If I am reading the MAX186 spec sheet properly, that way I can power the INA122s from Vcc.

[Groth]

Originally Posted by Incoherent

The heater current will max out at about 8-10amps, probably a little high to be on board but I am a little worried about connection resistance buggering up the readings. What do you think? The currents around this circuit are very low (10-100µA area), probably a prime candidate for a bit of inductive crosstalk. Any thoughts on reducing this if I did keep it on board. It is all effectively DC of course.

With the currents from the sense shunt to the amp so low, connection resistance isn't a big issue there (mV signals, µV connection drops). As long as you use twisted pair from the shunt to the board (to avoid differential noise), just let the in-amps reject any common mode noise that shows up.

You are right regarding digital i/o, it'd be a bit silly to not give myself at least the future possibility.
I am debating now whether to optocouple the digital side. The added circuit complexity does not appeal.

Give your self the expansion possibility, and put aside digital thoughts for another day.

Been looking at precision resistors, they are not cheap (~$3 each here in Sweden) for 0.1% <5PPM/*C metal film. I'm wondering whether your frypan sorting technique will be applicable here if I used the far cheaper 1% 50PPM/*C ones.

I think you'll do fine without the precision ones. The thermistors will all want to be calibrated anyway, so the 80K's don't need to be precision. The juctions of R13/R15 and R11/R12 can simply be measured - no need for precision. R9 would be cool to have precise, but there's no point in having it more precise than R10...

Go cheap.

Been thinking, actually theres no real reason why I can't use a 5v reference, If I am reading the MAX186 spec sheet properly, that way I can power the INA122s from Vcc.

I didn't read the datasheet closely, so :shrug: Check to see how the ADC inputs respond to voltages higher than Vref. Most have a limit to how much over-voltage current they'll sink, be sure the caps on the inputs won't supply more that that.

[Incoherent]

Originally Posted by Groth

With the currents from the sense shunt to the amp so low, connection resistance isn't a big issue there (mV signals, µV connection drops). As long as you use twisted pair from the shunt to the board (to avoid differential noise), just let the in-amps reject any common mode noise that shows up.

This I'll do.

Originally Posted by Groth

Go cheap.

Indeed. At this point thanks to Maxims fantastic samples policy, it's definitely looking to be pretty cheap. The thermistors are going to be the biggest cost.

Originally Posted by Groth

I didn't read the datasheet closely, so :shrug: Check to see how the ADC inputs respond to voltages higher than Vref. Most have a limit to how much over-voltage current they'll sink, be sure the caps on the inputs won't supply more that that.

Originally Posted by MAX186 Datasheet

Analog Input Range and Input Protection
Internal protection diodes, which clamp the analog input to VDD and VSS, allow the channel input pins to swing from VSS - 0.3V to VDD + 0.3V without damage. However, for accurate conversions near full scale, the inputs must not exceed VDD by more than 50mV, or be lower than VSS by 50mV.
If the analog input exceeds 50mV beyond the supplies, do not forward bias the protection diodes of off-channels over two milliamperes, as excessive current will degrade the conversion accuracy of the on-channel.
The full-scale input voltage depends on the voltage at VREF. See Tables 1a and 1b.

As I read this I think I'll be OK if I feed up to Vdd. I gain nothing resolution-wise from a 5V reference I realise, except a little bit of noise sensitivity.

Is the U5/U6 -ve input going to need an input bias current path? The voltage follower o/p is low impedence but would I need an e.g. 40K to ground (I'm switching the 80k-ers to 40k, better linearity in the 20-60 deg range.)

BTW, Thanks for all your input Groth, it has helped/is helping immensely. Re-learning stuff as I go.

[Groth]

Originally Posted by Incoherent

Originally Posted by MAX186 Datasheet

Cute.
Uh yep, sounds okay. Use the +5.

Is the U5/U6 -ve input going to need an input bias current path? The voltage follower o/p is low impedence but would I need an e.g. 40K to ground (I'm switching the 80k-ers to 40k, better linearity in the 20-60 deg range.)

The low impedance of the follower is current path aplenty.

Thanks for all your input Groth

No problem. When you get the board laid out, you're gonna post it right? We want to mooch!

[Incoherent]

...mooch!

Mooch?

[Groth]

Originally Posted by Incoherent

It's free software from ExpressPCB.

Not a bad little program. It's a lot easier to bung up a tolerable schematic with it than with the SPICE programs I have. And their PCB layout is easy and straitforward. It ain't very powerful, but the learning curve is much nicer than with the hardcore PCB programs I've failed to master.

It's a shame the output is so crippled; they certainly want the software used only with their services. Are you planning to have them make your board? Got to be a way to hack the output...

[Incoherent]

I'll be totally honest, I didn't realise it was a propriatory format, was just happy it was so user friendly. In any case, for me it's a great help just to get the layout, so I can do it manually.
I might use them. The little miniboard for $51 for three boards is not cheap but in the long run (actually in the short run too) it would save a hell of a lot of hassle. That way anyone else interested could perhaps benefit as well. We'll see.
Been thinking about incorporating a radiator fan speed controller into the circuit. As it stands I have a spare amp so I could take a feed from one of the INA122s and feed a fan driver. I am certain that I am able to see quite strong water temperature dependency on WB performance just with the crap thermometer I have now, I'd like to explore this and a bit of water temperature regulation could be useful.

Attaching a near final schematic for general perusal.
The fan driver is incomplete, I'll add a bit of proportionality and hysteresis later. But you get the idea.

[Groth]

Nice to see I'm not the only one who grabbed the schematic.

Looks good. I like how you've used the control/data lines, should make the interface program easier. Let not forget the vital green LED!

If the time constant for your system is large enough, you could get away with just the simple on/off thermostat fan control you have shown, though I wouldn't mind seeing a PWM controller attached to your newly tasked error amplifier.

What sort of plans have you for the digitals ins and outs?

[Incoherent]

Originally Posted by Groth

Nice to see I'm not the only one who grabbed the schematic.

Looks good. I like how you've used the control/data lines, should make the interface program easier. Let not forget the vital green LED!

If the time constant for your system is large enough, you could get away with just the simple on/off thermostat fan control you have shown, though I wouldn't mind seeing a PWM controller attached to your newly tasked error amplifier.

What sort of plans have you for the digitals ins and outs?

Re control/data lines, I really can't take any credit for this, it's a carbon copy of the original circuit this is based on.
Vital green LED indeed. A side effect is that it keeps a 10mA load on the 317, but the blinky lights factor is of paramount importance.
PWM. I'd like to do that but I'm wondering if that might be a bit noisy. ?
No real plans for the digital side, just a nice to have thing. Perhaps for switching the heater power level or multiple pumps.

[Groth]

Audible noisy or electrical noisy? For electrical it wouldn't be a big deal, assuming you have J4-4 be your PWM signal and have the power transistor and, more importantly, the fan's ground off board.

[Incoherent]

Originally Posted by Groth

Audible noisy or electrical noisy? For electrical it wouldn't be a big deal, assuming you have J4-4 be your PWM signal and have the power transistor and, more importantly, the fan's ground off board.

Electrical. OK, suggest a good PWM circuit. Emphasis on noise reduction and simplicity.
Wouldn't I need some common ground connection? Oh. Not with an optocoupler.?

[Groth]

I guess you could use an opto, but not really necessary. I'm assuming you're going to have everything with a common ground, just without the fan's current return through your board. Given the small but real /trace/connection/wire resistance, you don't want the pulses of fan current to induce noise in your board's ground.

As for the circuit, a linear ramp sawtooth wave is easy to make with a 555 timer. Then run that into a comparator along with the output of your error amp (variable gain on that would be cool), voila PWM.

[DeadEye]

Looks like you both have been busy lately. I like how it has progressed since our last chat.
I have been very tied up with work recently, so hadnt been about much myself. I will go sit back on the sideline and give any comments/input as required but it all seems to be in hand.

BTW, I use the Ranger2 PCB program for my circuits and layouts, it gives every type of output that I would want including photoplot and gerber files for hole drilling etc.

Later guys.

[Incoherent]

Guys.

Regarding grounding of the analog side of things, do you think that a ground plane is a good idea. I am planning to seperate digital and analog grounds, connecting them only at the ADC. Tips? Suggestions?

[Groth]

Separate digital and analog ground is probably unnecessary, since the internal ADC convertion clock (1.7 MHz) is much higher that your comms clock (~1-10 KHz) and your sample rate (10 Hz?). If you really want 'em separate, use the p-port ground as your digital ground and your power connector solely analog.

Plane: yeah, cool if you can. I'd try to lay everything out as a single sided board (easier to home make) and then use the other side as a ground plane.

What sort of through-hole to surface-mount ratio are you going to have?

[Incoherent]

Originally Posted by Groth

Separate digital and analog ground is probably unnecessary, since the internal ADC convertion clock (1.7 MHz) is much higher that your comms clock (~1-10 KHz) and your sample rate (10 Hz?). If you really want 'em separate, use the p-port ground as your digital ground and your power connector solely analog.

Plane: yeah, cool if you can. I'd try to lay everything out as a single sided board (easier to home make) and then use the other side as a ground plane.

What sort of through-hole to surface-mount ratio are you going to have?

Well, as it is evolving the board will be two sided. I will probably use the ExpressPCB service. I can see that there is no way I am going to be able to lay this out by hand and keep a decently small board.
As it is so far I am managing to keep the bulk of the analog stuf on on side with a few power and digital lines on the other. This means there is a fair bit of room for a ground plane.

The only surface mount stuff are the opamps and the instrumentation amps.

Have a gander at the current unfinished but nearing completion state of things. Right click and save target. Circuit and pcb. You need the ExpressPCB software to view it and feel free to be critical.

Not pretty, I am not giving up my day job. I decided to try the layout for size before seeing if I could incorporate a PWM generator in the available "miniboard" space. It will probably work, I will at least put the traces in.

[Groth]

Uh, both of those links are schematics, no PCB layout.

I did eventually find a layout: damn fine start, though it's a shame not to have the schematic that's linked to the PCB. Too bad the program doesn't include templates for mounting resistors/diodes vertically - could save you a bunch of space.

You like the through-hole, eh? If it was mainly surface mount and most of the complex artwork was on one side, I could've etched it for you...

[Incoherent]

Originally Posted by Groth

Uh, both of those links are schematics, no PCB layout.

I did eventually find a layout: damn fine start, though it's a shame not to have the schematic that's linked to the PCB. Too bad the program doesn't include templates for mounting resistors/diodes vertically - could save you a bunch of space.

You like the through-hole, eh? If it was mainly surface mount and most of the complex artwork was on one side, I could've etched it for you...

Sorry about the mixup, was in a hurry.
The relevant files are DAQ_xx3.xxx. The PCB should be linked to the schematic.

I am leaning heavily towards getting it etched for me. There's a catch though, $51 for three boards. $44 shipping to Sweden. I am not feeling rich.


I do not have much/any experience with surface mount stuff. Is it easier to hand solder? I don't have any special SMD tongs or anything.

[Groth]

Most surface mount part are easy, I prefer them cause I don't like drilling holes. For resistors/caps (0805 is my size of choice), I grab them with plain old forceps (I'm grounded, of course), position them, and touch one end with a fine tipped iron that has a tiny blob of solder on it. Assuming I didn't twitch at the wrong time, the other end gets a similar blob of solder.

IC's are only a bit tougher. Grab one lead with the forceps, position the part, and tack down a corner lead. Then tack down the opposite corner. If you use a decent amount of rosin flux, you can then sweep a heavily tinned iron across the leads, soldering an entire side at once (the flux plus the solder surface tension will prevent bridging; if you do get bridging desolder braid clears it right up).

Well... the SOIC ones easy at least. If you get into TSSOP or QSOP it's more fun.

44 for shipping? That's absurd.

PCB is looking good. I'm impressed that you've needed so few vias. I think you could clear up some of the loopy paths by swapping which amp in the quad packages is doing what. Same with parallel port.

Your analog (power connector) and digital (p-port) ground: keep 'em separate. Star ground > ground loops. Same with the shunt inputs, don't tie it into board ground.

By the by, the tons of through hole stuff doesn't mean I can't make the board. It mostly means drilling your own holes. Oh, and no plated vias in home boards; components could need soldering both top and bottom.

[Incoherent]

Originally Posted by Groth

Your analog (power connector) and digital (p-port) ground: keep 'em separate. Star ground > ground loops. Same with the shunt inputs, don't tie it into board ground.

Do you mean totally seperate analog and digital grounds? i.e. connect only the DGND pin of the ADC only to the parallel port ground? No connection to the AGND pin or power supply ground at all? Anywhere? Should the Flipflop and the digital IO's be connected to P-port ground? but at the same time they need a power ground.
Or should there be a single connection for the digital circuitry as per the datasheet...

But they suggest a star ground.
Sorry, I get confused all the time about this.


PCB, schematic.
Damn, back when I was supposed to know all this I was drunk. I do remember hating to manually insert little via rivets so I avoided them like the plague. It carries through still perhaps.
Hmm, so surface mount is easy eh? I'll have a look at that I think.

Been thinking about the PWM circuit. The comment about the time constant triggered a flurry of calculation which led to a bit of a tiff with the Differential Calculus. I came out of it OK I think. T@t=e^(-t/c*m*(C/W))*(DTi-((C/W)*W)+(C/W)*W is my thought for the day.
Anyway, this comparator fan control circuit is a PWM circuit in a way. The triangle wave generator is the water itself and the fan. Just a really low frequency and a bit of PFM as well.
A bit of friday night irrelevance.

[Groth]

Yeah, they thinkin' the same thing I am, just different scales/justifications. The reason behind not connecting the board ground with the parallel port ground is induction, loop = antenna. In the meantime, the parallel port signals are noisy (no reason for the mobo maker to use filter caps on the outputs, in their normal task it doesn't matter). Beyond the loops thing, letting the the signal current return to ground via the parallel port keeps the local ground cleaner.

The latch doesn't need a similar treatment. It's not bothered by noise, and any noise it introduces when activated isn't important since you aren't going to be doing AD conversion at the same time you're setting the latch.

Then again, do I really know and understand the things I think I know and understand? :shrug:

Vias: I've never done the rivet thing, it sounds frightening. Speaking vias, you could kill a number of the ones west ot ADC if you move the Vref line to underneath the ADC (it's DC so it won't be an issue) and remove the reduntant ground connections.

The parallel port has its inputs at the north end and outputs at the south, while you have the digital-in connector to the south and the -out to the north. You could eliminate a couple vias and shorten a lot of traces there.

Ground for U7 and it neighbors is a problem. All the return current from there passes under the ADC; any noise C3 bypasses to ground will travel directly under the ADC.

Diff-Eq, ewww. I went to class three times, don't expect me to decypher that. You should patent that combined PWM/FM concept.

[Incoherent]

The beginnings of another attempt. PCB5 and schematic5.

This really is time consuming. I can't figure a way to get the digital stuff through any other way so I'm leaving it. I've moved some things arround a bit.
The via's to the west of the ADC are for some decoupling if I find I need it.

[Groth]

Wow, you did make a bunch of changes. Looks damn good. I like the idea of the spare holes for decoupling.

I played with it a bit, to see if the digital lines could be unkinked any. I swapped the functions of J5 and J6 and switched around which pin goes to which parallel port bit. The only thing that might cause a problem (if you're not writing your own software) is the way I switched a couple pins from the 'control' output byte. Easy enought to switch 'em back...

While I was playing I also removes a redundant power trace, ran grounds to U1 and U2, and switched around which output of U2 went to which ADC input.

I got a little carried away, but I really like puzzles.

[Incoherent]

Oh, you've been busy. Thanks heaps for that, I like your treatment of the ADC west components, much better than what I had.
If possible I would like to not have to change the program. The intention is to use the ISEE program here , it seems to give me what I want (a time stamped data log file) and some limited calibration possibilities. Most calibration will be done offline, in Excel but there is a very simple control language that in the ISEE program that I'm going to try and use as well. Could also be used to control the fan actually.
This means that I do not want to change the IO distribution too much, my programming ability is close to zero and I don't want the time for me to learn to be another implementation delay.
I am rerouting the digital spagetti a bit though, inspired by your treatment of it.

Edit: Looking closer at your version I suddenly realised what you've been driving at. Brilliant. Simple and obvious on reflection. Another one of what you are full of Groth.
But I will keep the ADC steering signals the same as the original, otherwise your suggestions are the bees knees.

[Incoherent]

OK, near final version is done.
PCB and Schematic 6_g.

The digital stuff has is as you suggested Groth, the only difference being I have reset the ADC control lines to where they were. Not sure if your suggestion was actually correct in this respect, what does p-port pin 17 actually do? Anway, I am happy that the software will work, it's just a matter of assigning channel numbers.
Things added are some through holes for if I later need filter resistors on the inputs and on the ADC Vdd. A matter of trace cutting.
Some verification to clear up the slight remaining confusion. Should I leave the DGND unconnected to the AGND?
Is it worth spreading the ground around the place?