Cool, questions, i like questions
ruzki wrote:Ned !
You may could tell us some more about the PCB design ?
I personally would like to know how such dense PCB design is done ? How many Layer´s did you use ?
How does your mixed signal grounding looks like ?
So the PCB is only 2 layers. I was thinking about 4, and it m,ight still be the way to go but i thought i'd try 2. There arent many tracks on the bottom layer except for power and ground. Just a few little bits like the silly USB coms lines and some some jumpering. The design isnt very complicated, its pretty simple, so the components could generally be laid out so that they all connected via the top layer.
Ground wise, as you can see, the only things on PGND is the injectors and the low side drivers. They are all placed physicaly close to the PGND pins so that section of PCB could get poured with a PGND ground plane on top and bottom layer for a nice solid connection. The rest of the board is all SGND
DonTZ125 wrote:Hi, Ned.
Very nice! I do have a few questions / comments:
1. I don't understand the point of R83, and the comment about removing either R13 or R83. I can understand a 12v pull-up on a logic input, so long as the series resistor is sufficient to allow the shunt diodes to break down the voltage, but I don't understand having both a 12v and 5v pull-ups. Removing R13 leaves the input broken; do you mean R12?
2.Having pull-up / bias resistors on ADCs makes them useless for 0-5v inputs. While this doesn't much matter for a DIY design built for your purpose, if this ever becomes a device for the masses, I would suggest that solder jumpers should be included.
3. That USB6B1 is a chunky beast; have you considered the much teenier NUP4201MR6? It does the job and takes up less real estate. (I assume this is why you went with the FT230-XQ, not the more common FT232RL.
a. What are the red symbols between the USB socket and the USB6B1?
b. Why a big honkin' USB-B socket? A micro-B socket is easier to fit in, AND
can be had in IP67.
4.I like the way you've handled the USB / RS232 combo. I don't recall ever seeing an AND gate for that purpose.
5. As with the pull-up / bias resistors in #2, the shunt resistors in the VR circuits should use solder jumpers. From discussions on the forum for the "EMS That Shall Not Be Named" (Voldesquirt?), adding the shunt resistor to a MAX9926 input when it isn't needed can actually cause issues.
6.You might consider switching your Tach pull-up to 12v, allowing the circuit to directly drive a lot of tachs.
7. The power supply. Ummm ... I assume the multiple caps is an artifact of your opinion of tants?
a. Instead of the LTC4411, consider a 3A SOT23 P-channel Mosfet at the 12v input pin, installed with the body diode pointing towards the power supply and the gate grounded. This gives battery-reverse protection with near-zero Vf.
b. Why do you have a 6.8v Zener, vs 5.6v?
c. How are you going to see the fuse light?
d. Why the heavy filtering on the VRef?
multi part questions and some good ideas in there, i like it! I also like that you obviously really looked at the PCB and not just glanced at it, appreciated!
1. So because this project was done mainly for me, not for the general public, my documentation is super super shit. Let me explain what happens there. Fred had a big hissy fit about measuring 12V battery being one of the most important things in this world, and he hated that the voldesquirt measured the 12V on its input feed, and he was dead keen on being able to measure the battery voltage seperately, so for the sake of one extra track and one resistor, i gave him that option. If you populate R83 and remove R1, as well as remove R13, then SPARE3 will become the battery V input and gets rerouted to the same BattV pin on the micro and spare3_adc gets left unconnected.
You dont actually need to remove R13 if you dont want to, the protection circuit will take care of it, but its best to remove it. R12 can stay, it will just draw 3mA but thats ok. You really just need to move the 3K9 from R1 to R83 to move the battery sense pin.
Does that make more sense?
2. guessing you mean having the 2K49 resistors from 5V to the input are no good for things like a MAP sensor? i understand, but things like a MAP sensor that have an actual driven output SHOULD have enough output current to completely negate a 2K49 pullup. Thats only 2mA afterall. I agree that its a part thats not needed, and in a perfect world not wanted, but its also not worth putting a solder blob on the board for it because it should operate fine with it.
The other thing is that a machine cant place solder blobs, unless its on the bottom side of the board during wave soldering and then you need an extra step (peel able solder mask) if you want solder blobs to be open by default. You make a valid point though because it wouldnt work with another TPS for example. Actually, even that you could make work by only using the bottom bin and the wiper on the TPS. Signal size would go down but it would still operate fine.
3. that USB6B1 sure is big! and there is a simple reason why i picked it... i already had the footprint etc for it haha. I have 2 units i use, the USB6B1 (nice and bit and simple and easy) and the ESD7383, which is tiny and little and awesome but 'impossible' to hand solder. It's a BGA and i can fit 7 of them in the same space as your NUP4201MR6 suggestion
but thats a volid suggestion, and i probably should actually have changed to a smaller device really...
I actually picked the FT230 for the same reason, had the footprint so used it as thats the part i normally use. Its harder to solder, but actually easier than the micro if you ask me... It's also 1/2 the price...
3a. the squiggles are markers in altium to say those are differential tracks, so i can use the differential track router. It lets me route both tracks at once through the same places and keep track and gap constraints etc etc.
3b. simple reason, if i trip over the cord, i am less likely to ruin a USB B port, but will 100% rip the little micro USB socket off the board. It's just a robustness thing really. People like fred have complained to no end and say they dont even have that cable anymore, but i still use them every day on a bunch of hear i have here. It really is the right choice if you ask me. I never tried to make this board small, so it wasnt an issue.
4. the NAD gate is on the 'top' schematic where all the green blocks interconnect. Not sure if that works yet because i think the MAX chip shutdown pins are set so it Hi-Zs the output and i didnt put on pullups so that may require some work still... but its nice being able to use either setup and there being no code changes for using different serial ports etc
5. yeah, a solder blob wouldnt be a bad idea, but i just wanted to stay away from that for this revision because again, a machine cant place a solder blob.
6. i was thinking about having 2 pullups. One to 12V and 1 to 5V, that way you could choose. You could also put an inductor in place of the resistor to the 12V that way and actually create a big spiking high voltage to drive an old school tacho thats normally fed from the -ve of the coil... but figured an external circuit works well and keeps the high voltage noise out the ECU case.
7. multiple caps is because ceramics just arent perfect, but adding lots of physically big, lower value caps, you get a good end result, so thats why that is.
7a. the ideal diode isnt there for reverse polarity, its there purely to not back-feed 5V from the USB into the regulator when the reg isnt powered. A lot of regs wont like that.
7b. The problem with clamping diodes is that they start conducting too early, and a 5V6 will likely conduct at well below 5V and wanted to avoid that.
7c. put a light pipe in the case if you want, but basically you're not, but i like having at least a power LED on a board and 1 to a micro pin because just that is enough to test a lot of stuff with.
7d. the heavy filtering is just to get the micro noise and other switching noise out of the ADC. The Jaguar board uses a complete second reg for this purpose, but i opted for a few little passives.
I never set off making this board small. It was made with big components where i could so it was easy to manufacture and make it not massive. This board could shrink down to a lot lot lot smaller if i really tried...