[info] 72 pin 1123038-2 connector board

[Rhinoman]

There are some bad solder joints there - the solder hasn't flowed through the conductors so the wire is only soldered on the outside edges, you may just need to reflow those joints. I would think that the problem was caused by the wires not being properly 'tinned' first.

[AndreyB]

Has the trace fractured at the pad? it is a thin trace and it is not thickened before it joins to reduce stress.

I believe we can make connector-side holes smaller, and use checkmate pattern for wire side?

Now looking at the PCB file connector side is not too tight, the wire side is a problem due to huge copper diameter. Let's just make all wire side copper rectangular 1.4x1.9mm would that allow twice thicker wires? See my screenshot with a few pads modified to that shape.

At the moment I have intermittent continuity between 2A points. I am 101% sure there was no continuity recently and injector was not clicking and car was not running right.

[kb1gtt]

I do not see a problem. Perhaps a hair line fracture somewhere, which does not show on the picture. I don't think there is a difference between circuit pad vs rectangular pad.

You can find a hair line fracture by continuity / beep testing the trace. At some point the trace will not conduct. You can grab the wire with one side of the probe, then get a sewing needle, thumb tack, or some kind of sharp bit of metal on the other probe and poke through the mask until you find a point that does not beep any more.

To me it looks like that bare spot next to the circular pad is perhaps a bit thinner than the rest of the trace. Is that perhaps a hair line crack?

[AndreyB]

I don't think there is a difference between circuit pad vs rectangular pad.

My thinking was that I want the traces to be three times wider. I was assuming that the traces are so tiny (and while I do not know what's the exact problem with current size, I know from experience to be concerned about current tiny size) because of the lack of space between current wiring side pads. My suggestion is to change the shape of the pads in order to get more gaps between pads in order to make traces three times wider.

Should we make traces three times wider?

[kb1gtt]

Wider traces is better.

Currently I use the hole diameter plus some thing like 16 mills for the copper. Square or round does not change this. It's based on having enough copper such that holes do not miss the copper. We do not want any crescent shaped copper. That's 8 mills per side which can be 12mills at a 45 degree angle. I attempt to bump that up to 12mills, but often I'll consider 8 mills good enough. I forget what I did on that board. I think I bumped that down to 8 mills as it was tight.

The traces are thinner than my normal because some need to get through the narrow gaps.

[AndreyB]

At the moment
connector pads:
drill 1.2mm/47mil
outsize 1.6mm/63mil
ring (each side) 0.2mm/8mil

wire pads:
drill 1.2mm/47mil
outsize 1.9mm/75mil

ring (each side) 0.35mm/14mil

current track size 0.152mm/6mil

Using same outside 1.6mm/63mil would lower each wire pad side to 0.2mm/8mil would give us 0.4mm = ~16mil of extra gap between pads. If we triple the width of tracks to 0.45mm/18mil we would also have a bit extra clearance between pads and tracks.

Still wonder if square pads would help us by providing more solderable copper surface?

[kb1gtt]

For this board I violated some of my normal design limits, and we seem to be getting burnt from it. I usually design with a goal of 12 mill gaps, and 12 mill traces as my minimum specs, which allows multiple low cost PCB MFG's to build the board. Then I violate these specs only when required, like on the MAX9926 which requires 7 mill clearance. In this case we pushed the limits to what OSHPark can do with a 6 mil clearance, and 6 mil trace. When I put it to 12 mill clearance and 12 mill ringlets, It looks like this.

Capture.PNG (15.66 KiB) Viewed 14172 times

Note there are to many traces between the gaps and it violates the clearance rules, which I have currently set. These traces are on the harness connector, not the generic KICAD connector. I see I currently have a ringlet of 15 mills, or 7.9 mill copper width.

I also got buggered by using the KICAD provided modules without looking at them to closely. KICAD had about a 30 mill ringlet, which is crazy. I just changed the board to a 12 mill ringlet which is shown above. Even at the 12 mill ringlet, a 12 mill clearance is not sufficient. I can decrease the clearance, but we run the risk of similar quality issues that we got with the R0.2 of this board.

By switching to a 6 mill clearance I was able to get you an 8 mill trace. This is the OSH park minimum clearance and slightly larger trace. I'm not crazy about this board, as I don't like pushing the MFG limits.

[AndreyB]

8mil is still very scary, I need more confidence in this connector. So let's focus on the "2" area which is the most problematic.

idea#1: reduce drill size on connector side? do we know the official connector terminal size? I measure 0.68mm by 0.68mm that would theoretically require a 0.962mm/38mill drill, 1mm drill for safery? Does this look like enough gaps? I know a 1.1mm drill would work for sure, with current 1.2mm there is a lot of room around terminals. That would get us 4 or 8 mills of extra gap between holes.

Idea#2: would a different pattern on the wiring side help with routing? For example if we flip 2A with 2C on the wiring side, we can place both A and C traces to the left of everything on the top layer. Once we flip 2R and 2P on the wiring side we can place both traces to the right of everything on the top layer - just like that we've resolved two of these "two traces between holes" situations. That would leave us only with 2K trace, do we want to route it around everything with a couple of vias? Would thicker traces with vias be better than thin traces without vias?

bad idea#3: different width traces - at least use thick traces were we can. I think with #1&#2 we would not need that

worst idea#4: 4 layer board. that would bankrupt me but I need a reliable connector board, I cannot afford to worry about it at the track.

[stefanst]

[...]I believe we can make connector-side holes smaller, and use checkmate pattern for wire side?[...]

I just checked the datasheet. There's no spec for the through-holes, but the pins on the connector are 0.64mm square. So a 1.00mm, or even 0.90mm hole would be perfectly sufficient. That should give us some more space for traces.

[kb1gtt]

I recall that on the Frankenso connector we enlarged the holes to make it easier to install the connector before soldering. AKA slightly bent pins is a real pain. However this connector has less pins. So we could try a smaller hole.

How about we only make these problem pins 1.0mm. Then the others we leave at a larger diameter.

[kb1gtt]

As luck has it, this board was also my attempt to use the auto-router. I would have been much better off doing this by hand as I normally do.

[AndreyB]

How about we only make these problem pins 1.0mm. Then the others we leave at a larger diameter.

That's a great idea! Like this.

So with some drills lowered to 1.0mm we are now at 12mill traces (up from 6 mill originally), that's progress.

Q1: How concerned are you about the 2A<>2D double-trace? What do you think about flipping 2 wiring side pads in order to avoid at least some of these two-traces-between-holes situation?

Q2: I _really_ need reliability here. Can we move 2Q trace away from 2P hole? 3B away from 3A? 4P from 4O? What I am saying yes we cannot move all traces further away, can we please at least move the ones we can easily move?

Q3: 3C trace can be moved to the left I believe to avoid the double-trace.

Q4: 4Z<>4AC triple-trace, please move 4AE trace to have two double-traces instead of 3+1

[kb1gtt]

The more you make me look at this the more I think I need to just start over. This was an attempt to use the auto-router to speed up the design cycle, but as you have noted, those 3X traces was not needed at all. As well I don't like how it routed things in general. Any how I guess it is what it is.

Committed, let me know if you see other things.

[AndreyB]

Committed, let me know if you see other things.

Progress

Q1: Move wiring pad 2R to the right - this way 2R trace goes on the right side of 2P, we avoid a double-trace between 2M and 2P

Q2: Move wiring pad 4C to the left - this way 4C trace goes to the left of 4B, we avoid 4B<>4E double-trace

Will look more with fresh brain tomorrow. Thank you for the progress!

[AndreyB]

Q3: trace 4W can go to the back, avoid 4X<>4AA double-trace

[AndreyB]

Q4: move traces a bit between 3J and 3M to increase gaps, same the single top trace between 3M and 3P, same trace 3B too close to pad 3A. I think if we temporary increase rule gaps DRC would show all the nasty spots and we can see how many could be improved?

[kb1gtt]

Hmmm, do you mean like this? Committed.

I also don't like how the connector hides the traces on the top layer. I would prefer if all of 3rd row was on the top layer such you minimize hidden traces. If it's on the bottom layer, then you can see what has gone wrong. I do not like traces under the connector. But it's a bunch of work to change it.

[AndreyB]

Q4b: trace 3B too close to pad 3A

Q3: trace 4W can go to the back, avoid 4X<>4AA double-trace

[kb1gtt]

I saw something shinny and got distracted.... Squirrel......

Have all the questions been addressed? Are there more items?

[AndreyB]

rev 0.3 ordered in 2oz version - traces are now 12 mill (twice the size), gaps are now 10 mill - that was achieved by reducing few connector holes to 1mm and moving two connector pads just a hair. Maybe very small connector bending would be needed.

[AndreyB]

Connector slides right into the board without any bending.

[stefanst]

Nice! I do like this better than the previous version.

How tight is the fit of the pins in the holes?

[AndreyB]

You can zoom on the image above and it would show details. Here's a crop where couple of holes are smaller - still, no pin bending was needed probably because we still have some (little) clearance.

[stefanst]

Hmmm. Looks like we have two "4AC"s.

[AndreyB]

6) silkscreen, connector side: 4AC instead of 4AG