I have finally gotten the courage to ditch breadboards for my first professional PCB. This is a rectification module for converting power from my 3d printed wind turbine into something actually useful. The microcontroller is just in case I get bored and I wanted to add in a weather module for extra flair. I’d also like my traces viewed (like if they are in the right pins.) if possible because I’ve messed up on those way too much. I tend to be quite unorthodox in my trace/component placement (Fritzing’s trace alignment is kinda bad.) but I’d just need it work.
Thanks all,
Bread guy :DD
Components:
KBP206 Rectifiers 2X
1000UF 35v Capacitor (Stabilization)
5v 1.5A Voltage regulator
Female 4 pin USB A port
Raspberry Pi Pico W
Dht 11 (I had this laying around…)
0.96 Inch Oled display
Which illustrates my point that pictures are basically useless. The sketch allows running DRC (routing->Design Rules Check (DRC) which flags a bunch of errors:
I’m not immediately sure what this one is about, it may indicate a part error as it appears to be complaining about an apparently valid connection. Yep, the svg has a teminalID defined in the svg, but the fzp file is not correctly defined causing the errors reported.
it looks like I changed the moduleId so you should be able to just load the new part then do a delete minus on all the existing parts, and then drag the new part in to the sketch and move the wires to connect to the new part (in all three views.)
Also I’m running an old beta version of fritzing and none of these errors popped up ://. Also other than these any other issues like if the traces are at the right pins or if there are any other things drc caught?
Yes. The first overlap shorts many of the I/O pins on the micro and that will likely be a problem. The too close ones may or may not be an issue and the board house may or may not flag it as an error (the cheap ones I usually use just do whatever the gerbers say and leave it up to you!) The rectifier one is probably a non issue as the copper is correct just the part is wrong.
there is a hole hidden by the silkscreen layer that is too close there and likely truncating the trace at least somewhat and may short to whatever is filling that hole (I assume one of the USB pins) the black areas are not supposed to have traces in them because they may interfere with the USB operation. You look to have enough space to run the trace up on the other side of the micro pins if you move the traces a bit to the left which will avoid the keepout area.
same with this one it will likely short the input voltage to ground although there is likely a little clearance there, it is dangerously low. bringing the trace out parallel to the pin for a bit would fix this.
OK, here is a fixed version that passes DRC. I substituted my corrected rectifier to get that out of the way, but the case is a little too large according to the data sheet. Then I moved some of the traces around to clear the various DRC errors. The bridge rectifiers are on odd pin spacing so the traces don’t exactly line up.
the path circled in red can be simplified like this (the line circled in green is a new change that I just noticed was possible to simplify the routing even further.) All the same pins on components appear to light yellow indicating the two routes are identical electrically. The same applies to the positive side unless I am missing something (which is entirely possible .)
I see. Probably just me it probably was the way some traces converged that lead me to believe something was up. It should be working the same way. I changed some stuff around kinda felt like it but SHOULD BE IT. (I don’t wanna nag pcbway again.) ECU Unit fixed.fzz (184.0 KB)
(Reached Chat limit .)
Lemme know if its ok this way.
Over all looks fine. I however made some more changes. I screwed up with the rectifier part, it actually has 2 parts in the .fzpz and I’m not sure how Fritzing will react to that. Since I was modifying the part anyway I chose to check it and fix it up (which was lucky because the hole sizes were marginally too small! A 0.035in hole where the pin is 0.034in wide at max tolerance, I replaced with 0.038 holes (which as a bonus will accept 0.1in headers if you choose to make them plug in.) Corrected the size of silkscreen to match the real part then substituted the new part in to the sketch. Then I changed the grid size to 0.05in, because the rectifier pitch is 0.15in with the 0.05 in grid the traces will align with the pads which looks neater.
first move all traces possible to the bottom layer (anywhere there isn’t a collision with the top layer.) The reason for this is that with solder joints potentially under components and thus not visible, they can (but usually won’t) not get soldered correctly. Joints on the bottom of the board are easier to examine if there are problems. In this case I moved the two traces outlined in green here from top layer to bottom layer as there are no conflicts.
then set the grid size from the default 0.1in to 0.05in to allow the rectifier pins to be aligned straight for neatness (makes no practical difference except appearance.)
then align the new part connectors (which are on 0.15 boundaries the original part was on 0.14in boundaries but the tolerance is 0.160in to 0.140in and thus the center at 0.15in is the preferred value and happens to align well with the 0.1in grid.) The smaller grid size also allows tighter corners (which doesn’t matter much in this case as there is lots of room.) The traces circled in blue were moved to bottom layer, and in the case of the regulator simplified to reduce the length of the traces. It likely isn’t important in this case, but is in a high current situation where trace resistance matters, so it is a good habit to get in to.
and here is the new rectifier part (I will probably post it in the thread I posted the original as well) which is technically in the temp parts bin associated with the sketch, but is here for convenience too.
.)
.)
