MrOnion's OnionBoard - GP IO/Power PCB (requires CPU board)

[Compassion]

MrOnion,

I'm interested in the outcome of your OnionBoard project as I've got two TA cards, and a pair of first run BrickRPM chips, and would like to have a chance at getting a chance at one of the runs if possible.

For my project, I'm looking at getting started on ECU integration for my AJ16 (a relatively modern EFI 6 cylinder with COP, CAS, and a 60-2 trigger wheel engine transplant sometime in June/July and could end up implementing the setup on a second car. My build thread is linked here.

I have some background in Electrical Engineering and I'm in the middle of completing my degree in the subject.

I could see about going down the DIY HW route for an interim solution, but breadboard prototyping still lacks the benefits of PCBs with ground planes. Either way, I'm hoping to be in touch.

[MrOnion]

Thank you Andy and Fred for taking a look.

1. You need current limiting resistors on the outputs of the TC442x drivers just as Fred mentioned. I used 100 ohm resistors on my Jaguar board.

Agreed. I moved the driver chips along with load and pulldown resistors lower so I made some space from them. They are now in vertical position and enough space for a 3w if desired.

100ohm sounds good. In ravager schematics they are 150ohm and in the notes.md they are mentioned as 200ohm. So probably depends on your current needs? What wattage are you using, 2w?

2. For your 12v power feed to the voltage select jumper for the TC442x drivers, it would be better to branch that off from the MOV rather from the decouple capacitor to the regulator. If you want to decouple the 12v input to the drivers, place another pair of capacitors closer to the driver supply line (the 5v/12v jumperable line) and the driver ground.

2. also reminds me of this: You should take your 5V to the ignitor drivers directly from the supply, not from the tail end after the other stuff has its share. Star power, if you like. Much like star grounding.

Ok, That was something I was not so certain about so traced it to the point after some filtering. Added two 0805 size caps to the supply line of the drivers. big enough? Also the 5V to the drivers is now taken straight from the reg leg.

3. Try to keep the positive voltage runs primarily on the top side of the board by the regulator instead of on the bottom with the ground plane. It looks like you have plenty of room to re-route the 5v traces on the top side. With a two sided PCB, I try to run the low power 5v and the signal traces on the same side when possible and the ground on the opposite side. Also try to run the 5v supply traces at 90 degrees from the signal traces to help with noise reduction on the signal traces if you route them on the ground plane side of the PCB.

Sin confessed . I tried to use this approach and also read about gridding the power and ground traces. But ended up just running a single trace around the board. The power rail is now connected only to the schottky pairs of the A/D circuits and nothing else so not that critical?

Might make a run for it though and as Fred mentioned branch first.

4. Another idea for the voltage regulator and the 5v capacitors, slide the regulator closer to the VR inputs and move the output capacitors up to below the PolyFuses to keep the 5v supply lines away from the VR inputs.

Unsure how 4. would work, even after asking Andy However this reminds me that you have 5V between the inputs of the VR traces down the bottom. If that could be reworked to keep the trace away. If you're using VR and the pull ups are not installed, then that trace would be isolated. You could keep it as is and put a solder bridge where it joins the main wire like I showed you the other night. IE, just a thin cut through the trace near the 5V rail.

I could run the 5V rail on top side near the VR traces or put the VR traces on top side. Want to keep the 5V caps near the CPU power connector. About the 5V line between the VR traces does it solve the problem if I run it on the opposite side of the board? The pull-ups could be surface mount also and just connect it though a via to the VR trace. Just use through hole for the shunts.

5. You will want to use a mica insulator between the regulator heat sink and the board to keep from burning the board in the event that one of the 5v accessories is shorted or tries to draw 0.5A for any amount of time before the PolyFuse opens the circuit. This will also act as a electrical isolator between the traces and the heat sink if you route any 5v traces under the heatsink (but I don't recommend this routing).

Not sure that I agree with 5. I'd tend to put some copper under it instead and use the board to sink more heat away.

I'll try to keep the heatsink area clean so it can be used anyway possible. My idea is to use a simple heatsink as pictured on the board. But if that causes trouble I still can make a L-shaped profile and attach it to the side of the metal casing for more heat dissipation.

6. I agree with Fred on the A/D grounds, don't separate them.

Sure. Thanks for clearing that up.

Another thought regarding the voltage regulator and the capacitors for the regulator circuit, why not use SMD components to:
1. save space and,
2. allow for more ground plane/heat sink area

Valid point. My approach is effected by the fact I was first going to make quick prototypes of supply, input and output boards separately. Just to get something to start from. So I checked the parts I have available or easy to get and make a simple through hole single side power supply board. Then I ended up joining the input and output boards together and after that was like "fuck it" and lets put all this crap on single board.

I might go the SMD way later if this thing needs more space and maybe some rerouting of the traces.

One additional thought about routing traces...
I generally route supply voltage first, then signal traces and finally let the CAD program fill in the ground plane at the end.

With that said I normally route the traces manually (by hand) instead of using an auto-router...

Good tip. I did not use the auto router either. Don't trust it and might need more work fixing it up and placing "restricted areas" because of "no no no, don't run the trace there you bastard!"

I'm interested in the outcome of your OnionBoard project as I've got two TA cards, and a pair of first run BrickRPM chips, and would like to have a chance at getting a chance at one of the runs if possible.

Sure thing. I might order them soonish as I get the final changes done. Seeed has the minimum order of 5pcs but 10pcs isn't costing the much more if needed. Of course it would be nice to test this sucker first in real life before distributing too many of them. Onion warranty. It will either be ok or bring tears to your eyes

The board is designed a 4-cyl in mind running sequential + COP but could be used with more cylinders. Because there are only six timer ports (Port T) available for inj + ign I'm running wasted spark ignition at first. I'm using the two acc fets for fuel pump relay and leaving the other available for future like pwm boost solenoid etc. I'm running a separate H-bridge board for idle and if I don't get that running smoothly then I might use the other fet for simple PWM idle solenoid.

Are you planning to run the 6-cyls seq, semi-seq or batch?

I'll post a new pic of the board when I get my changes done. But now I need to go to the garage and do some engine building + wrestle a twisted passenger door back to the car...

[Fred]

100ohm sounds good. In ravager schematics they are 150ohm and in the notes.md they are mentioned as 200ohm. So probably depends on your current needs? What wattage are you using, 2w?

Have a read here: viewtopic.php?p=29853#p29853

If you're setting it up for 5V use, I'd go 100, for 12V use, I'd go 150, 150 is OK for 5V use, 100 is too higher dissipation in a short circuit at 12V, 200 is too low a current, period. Hence 150 :-)

Added two 0805 size caps to the supply line of the drivers. big enough?

Depends on the values and properties! :-) more the merrier, but it's getting tight, and it no longer shares the supply with most of the critical stuff. From the latest picture you showed me, how about routing the end of that trace down right to the left hand reg leg?

The power rail is now connected only to the schottky pairs of the A/D circuits and nothing else so not that critical?

My amateur opinion is that it'll be fine like that.

About the 5V line between the VR traces does it solve the problem if I run it on the opposite side of the board? The pull-ups could be surface mount also and just connect it though a via to the VR trace. Just use through hole for the shunts.

Sounds like it could be a good thing. Try it, you can always git reset --hard HEAD^ afterward. Keen to see a screeny of that change.

Are you planning to run the 6-cyls seq, semi-seq or batch?

Excuse me answering on her behalf: semi sequential and wasted spark, for a start, at least.

Fred.

[Compassion]

Mr Onion,
I'm figuring I will need to start with semi-sequential and wasted spark to start with. Without the original ECU, or FreeEMS control of triggering the dumb electrically controlled distributor that can be retrofit, I'm left with needing to have the COP functioning for spark at the same time as fuel.

Later on I might run a dual TA card setup for fully sequential spark and one TA card for fully sequential fuel, or just wait for further development for the other ports to become available.

[wheeler_express]

Mr Onion, when you get the companion boards done, I would like to buy a couple if you have extras please.

[MrOnion]

Thanks for the interest in this project!

Had some time again to work on this thing. Heres a list what I have done since last version. Thanks to all reviewers!

- Changed through hole pull-up resistors on the brick circuit to 0805 smd near the headers.
- Added smd resistors and wire pads that can be used to feed 5V into the brick board to make a 2.5V divider for hall sensor (check jaguar scheme for more info).
- Switch A/D + BRV circuits schottky pairs powered from beginning of 5V rail on top layer. Tried to make the ground plane more consistent.
- Ignitor drivers 5V is now fed straight from regulator leg.
- Ignitor 5/12V jumper header changed from pin header to solder bridge on the bottom layer.
- Fet and ignitor load and pulldown resistors swapped the other way around (N00b failure and created a voltage divider).
- Fet ground plane and source vias on the last fet moved a little to the left. More isolation when sliding the board into a case with side slots.
- Changed larger 1206 load resistors to A/D channels.
- Through-hole load resistors added after mosfet driver channels.
- Renamed the pinheaded connectors to make more sense.
- Several grounding wire pads with thermals added to the cpu ground plane.
- Ground loop monitors moved to right to shorten 5V rail and load/run ground trace.
- Thicker signal traces
- Added ground pins for sensor connector. One for each input. Moved the driver connector to make space.
- Some minor fixes to traces

I decided to make one "home etch" prototype of the board to make an actual test run with it. Just to be sure it works and no more flaws are present that are hard to see from schematic or the board image. Then I feel more confident to go into "production" with this thing. This means I order 5-10 pcs of these as a test batch for myself and possible test users.

Here is a new image to look at. The vias are larger and have thermals in this version so don't be alarmed. They are just for making home made vias easier .



Hopefully I get one done soon and install in my project car.

[Fred]

From chat, the rest is done to or better than my suggestions, good work! :-)

(12:23:09) Fred: getting picky now:
(12:24:13) Fred: if you mirror the topology of the ground lift sensors, you could shorten the 5V bus, if you do that, you could raise the whole lot up a bit closer to the FETs, and expand the ground plane there, or will that not work with the 3 pin diodes?
(12:24:42) Fred: they can be rotated, i think?
(12:25:36) Fred: in fact, you could move that circuit to the right a bunch too, and shorten the bus even more and expand the ground even more

(15:47:52) Fred: just noticed that you're trying to economise on vias, sharing the ground point for the load/run with the right gnd monitor
(15:47:53) Fred: and
(15:48:06) Fred: your board edge spacing, i guess the FET ground is the limit?
(15:49:05) Fred: if so, you could push the bus and right edge of ground right a few mm and WAY shorten the trace to the load/run sw
(16:04:44) Fred: ie, new via bottom right corner of ground plane post widening it :-)
(16:04:56) Fred: tell me to sod off, if you want

[wheeler_express]

The pin out on the ravage.pdf (column 6 at the top) shows PT2, 3 and 4 for both an ignitor and an injector. Has this changed and which is correct?

[Fred]

viewtopic.php?f=54&t=1084 < in short. Longer from someone else. Very busy for next few days.

[MrOnion]

Ok, first prototype etch done. Made this just before the trip to sweden to meet Fred.



The vias where a little too small so I made a new one yesterday. Added more isolation between the groundplane and 5v rail + more copper on the vias for easier soldering. Also shortened the exposure time a little on the UV. Our laser printer makes too light transparencies so it makes the surface a bit matte. Could print two on top of each other or use a toner spray...

This is only a prototype so it does not need to be perfect. Anyway soldered most of the parts to the board and will probably test it during the weekend. Decided to make a breakout board for my ms2 daughterboard to make the first test with . If it burns, bummer... .