For discussion of Speeduino compatible boards designed / built by other members of the forum and for guidance around making such a board
By fram
#41212
Hi

First PCB design? Automatic placement? Automatic router?
I just check the gerber files, and sorry to say but it's a bit messy... :?

I think you should start again from scratch, with board outline, and placement of the STM32 daughter card, first.
Then, from your schematic, start a good placement, the noisy parts (mainly transistors for INJ and ING and the stepper driver) close to the main connector.
Analog inputs, far away from the noisy parts if you can. Try to be as logic as possible according to your pcb area and your schematic. Same thing with power supplies. Be logic how to place and distribute the power.

You need a full ground plan, on top and bottom, with a lot of vias top/bottom for EMC issue.
Bluetooth module is in the middle of the board, with antenna close to the pcb and ground plan: will not work.

Please do not send this design in production, you're going to have a lot of issues.
I add two screen shots as examples of bad routing design/crapy autorouter.

Spend more time on the placement before starting to route and come back in a few days with a better design! ;)
Attachments
b.JPG
b.JPG (204.65 KiB) Viewed 8818 times
a.JPG
a.JPG (66.84 KiB) Viewed 8818 times
By Tjeerd
#41214
Hi Fram

Thanks for the review! Board has been produced and build actually (see photos). It works quite nicely for now. No jumping RPM or anything from EMC issues when the stepper PWM and injectors are running. Also stable analog inputs, but there is a lot of analog and digital filtering going on on these analog inputs so i will check with a scope if there really is no issue.
fram wrote: Thu Feb 27, 2020 8:42 pm First PCB design? Automatic placement? Automatic router?
I just check the gerber files, and sorry to say but it's a bit messy... :?
Yes it is not very polished i agree, I will check the point you show in the pictures. I got a bit annoyed after placing components in the correct location and routing multiple nights to get it to work on a two layer PCB. In the end I used the push and shove function of KiCAD a bit more than i liked. That ended in making the board look funny and auto routed indeed.

Also the track width of power tracks must be sufficient to carry the intended currents. Taking up quite some space. The last important thing is the planes around the transistors for cooling. I may add some via's to also have some cooling on the back of the board if i run into problems with heat.

The schematic is not very nice as it is partly imported from eagle for version 0.1 of the board, need some clean-up on PCB and schematic i agree!
fram wrote: Thu Feb 27, 2020 8:42 pm I think you should start again from scratch, with board outline, and placement of the STM32 daughter card, first.
Then, from your schematic, start a good placement, the noisy parts (mainly transistors for INJ and ING and the stepper driver) close to the main connector.
Well. That is exactly as i started ;-). All injector drivers and stepper drivers (ignition as well) are <30mm from the main connector. then all filter capacitors and resistors for analog inputs close to their respective ports on the 2x 44 pin headers of the CPU board.
fram wrote: Thu Feb 27, 2020 8:42 pm Analog inputs, far away from the noisy parts if you can. Try to be as logic as possible according to your pcb area and your schematic. Same thing with power supplies. Be logic how to place and distribute the power.
All analog filtering is done close to the input pin of the CPU board, if possible. But most are all the way to the back of the board and therefore need to cross the high power switching units at some point. That is the drawback of using only one combined connector for power and signals (I would like to have separate connectors).
fram wrote: Thu Feb 27, 2020 8:42 pm You need a full ground plan, on top and bottom, with a lot of vias top/bottom for EMC issue.
Placed a ground plane on the bottom and a VCC plane on top. As i recon the VCC is also just low impedance plane to get rid of any EMC induced high frequency currents as is a ground plane. It even has ceramic capacitor coupling to the ground plane making it essentially a ground plane for high frequencies. I could very well be wrong on that. You have any Thoughts on that? It would be beneficial to have top and bottom ground planes and via's. Then the planes would actually be al over the board and can not be separated by any traces.
fram wrote: Thu Feb 27, 2020 8:42 pm Bluetooth module is in the middle of the board, with antenna close to the pcb and ground plan: will not work.
That module is placed even worse because it is sandwiched between two PCBs ;-). I should find a more appropriate place but that is some extra work. I tried it this way to see how well (or bad) it works in practice before i try and place it such that the antenna can radiate.
fram wrote: Thu Feb 27, 2020 8:42 pm Please do not send this design in production, you're going to have a lot of issues.
I add two screen shots as examples of bad routing design/crapy autorouter.
Board is already been produced and DRC checked before sending. DRC check is set to >0.3mm spacing and the board house can produce to 0.25mm spacing reliably. Yes i did a lot of back and forth placing and routing. there are multiple traces that could be places much nicer. But that would not effect the functionality i ques?
fram wrote: Thu Feb 27, 2020 8:42 pm Spend more time on the placement before starting to route and come back in a few days with a better design! ;)
I spend quite some time to place and route this board actually :-D. But i will see how it works when running an engine and to see if any EMC issues arise. Thanks for the review i will do some more checks ;-).

By the way i don't know if you noticed but the two 44 pin headers are the daughter board headers not the ECU header itself. The ECU header is the 4 rows of pins on the edge of the board.
By fram
#41218
Board is already been produced and DRC checked before sending. DRC check is set to >0.3mm spacing and the board house can produce to 0.25mm spacing reliably. Yes i did a lot of back and forth placing and routing. there are multiple traces that could be places much nicer. But that would not effect the functionality i ques?
Agree your pcb supplier can produce 0.25mm spacing, same for your DRC.
But you need to have different rules into your design for:
static and no critical signal
analog signals
digital signals
Noisy signals
High current, high voltage signals or power supplies
etc...

And if you have enough space into the pcb for 0.5mm space track to track instead of 0.25mm, go ahead for 0.5mm!
The PCB supplier capability is one thing, your design rules is another! you need to have both in mind for your design!
;)
#41221
You can't rely on DRC checks to guarantee good design. Simple things like not having angles of less than 90 degrees to avoid acid traps and solder paste issues. You have a multitude of tracks coming off pads at acute angles where it just isn't necessary.
By Tjeerd
#41223
fram wrote: Fri Feb 28, 2020 8:45 am
Agree your pcb supplier can produce 0.25mm spacing, same for your DRC.
But you need to have different rules into your design for:
static and no critical signal
analog signals
digital signals
Noisy signals
High current, high voltage signals or power supplies
etc...

And if you have enough space into the pcb for 0.5mm space track to track instead of 0.25mm, go ahead for 0.5mm!
The PCB supplier capability is one thing, your design rules is another! you need to have both in mind for your design!
;)
Yes if i had no trouble getting the board routed with that many signals i would chosen 0.5mm spacing. I will try another round with version 0.4 if i fixed all the other issues with this board on the schematic part. I did try to route all analog and trigger/small signal signals not to be close to switching current carrying traces to reduce EMI. At least not for very long traces.
By Tjeerd
#41224
JHolland wrote: Fri Feb 28, 2020 12:40 pm You can't rely on DRC checks to guarantee good design. Simple things like not having angles of less than 90 degrees to avoid acid traps and solder paste issues. You have a multitude of tracks coming off pads at acute angles where it just isn't necessary.
True, but its a tool to check if you did make mistakes on the spacing part at least. Isn't under etching (because of acid traps) not a bigger problem for very small traces? Less of an issue with bigger traces. (but if preventable better to prevent it any ways ). Next design i will try and better my life :-D.

Hi, I am trying to assign Signed values to the x-a[…]

Vr Conditioner Noise when cranking

New version 202305 don't fix the issue. Now after[…]

blitzbox

I've finally figured out why MAP and Lambda weren'[…]

Hello, I bring news!! Let me tell you that after […]

Still can't find what you're looking for?