Not able to route signal out from 0.4mm WLP

Hi,
I’m using Kicad 6.0.0 rc1.
I’ve MAX17262 in my project am not able to route out signal Alter pin with minimum trace width of 4mils(since PCB Manufacturer recommended min trace width is 3mils)


lead-free 0.4mm pitch, 1.5mm x 1.5mm, 9-pin wafer-level
package (WLP).
I’ve attached the image FYR

The faint circles around the pads are the pad clearances. They either come from the netclass or from the footprint itself. With the current setting it is simply impossible for a trace to fit there.

1 Like

If you absolutely can not reduce clearances or trace width then you have to drop a via right where the pad is. Just know that you may have trouble with soldering that part that way and it may need a bit more paste for that center pin since via will wick it away.

1 Like

If the manufacturer really requires such a huge clearance/trace width (If it is not a setup mistake) then it is quite unlikely they have vias this small. Meaning the most likely solution is to either ditch the bga part (replace it with an equivalent in an easier to handle package) or change to a more capable fab (more expensive)

3mils = 0,0762mm, very narrow.

1 Like

from the evaluationkit, it seems they use a very tiny track for the center pad and the pad clearance is lesser than your.

max17262-evalkit-zoom

2 Likes

Which means big bugs fab and p&p!

Edit:

According to max’s 9WLP specs there are only 0.19 mm gap between landing pads (0.21mm diameter) which means a fab house capable of 3mil tracks and clearances. Doable at a cost.

I found a footprint from snapeda and copper to copper space between pads seems to be ~0.15mm (diameter 0.25mm). It would mean 0.05mm trace/space. With smaller pads (0.21 like in jos’s calculation, but I got a different number when the space is devided by 3) you would have enough space for 2/2mil.

Real via-in-pad is also an expensive option. You can’t do this with even 0.2mm via hole, 0.15 could be acceptable.

Maybe the best (cheapest) option is something like PCBWay’s “Advanced PCB” with 2/2mil trace/space - or just move to another chip package.

2/2 mil definitely will work.
3/3 could work but depends if the fab plays along.

3/3 is already in premium service, 2/2 is going to be expensive. Via in pad with filling might be a better way

2/2 or 3/3 does not make a difference for pcbway.
Not even for automotive grade boards.
May be a dollar, two or so. That’s it.

For such things, there is via-in-pad with conductive or non-conductive fill and cap technology.
What is this?

  1. Your center pad will have a small via in it. This might be through-board, or blind, depending on cost sensitivity.
  2. The plated via hole will be plugged with a resin system so it will not steal solder from the pad. For normal signal pads, non-conducting is cheaper and just fine. For lower current power pads same story.
    3, After setting, the surface is ground and foil caps bonded or plated over the resin so your BGA solder works.
  3. You will route trace(s) out from that pad on other layer(s).

It’s interesting to follow the costs of special technologies. Maybe some day we are in a situation where a board with microvias and via in pad cost 2$. Until them it’s easily 10x as much.

If someone asks here question which leads to an answer recommending a special technology, there’s a good change that it’s cost sensitive and some other alternative should be found. Those who already know what they need rarely ask in this kind of forum.