2
\$\begingroup\$

I have a PCB layout as shown. My question is can I route the PCB between the copper pads? The purple colour is solder mask. From what I know solder mask is the green stuff on a PCB which covers the copper, determines where the copper is actually exposed. So once copper is removed on the board, it is coate with a solder mask which is then removed at certain places. Is it okay to route between these red copper balls?

enter image description here

\$\endgroup\$
  • 3
    \$\begingroup\$ Routing a BGA chip as (what seems to be) your first PCB is going to be a trial by fire. \$\endgroup\$ – scld Jan 15 '16 at 14:53
  • \$\begingroup\$ It is ony a 64 pin BGA. WIll it be very hard to do? \$\endgroup\$ – red car Jan 15 '16 at 15:01
  • 3
    \$\begingroup\$ No, it won't be hard, relatively. Good design rules should allow you to create a functional BGA fanout. But your hesitation, even on what soldermask actually is, makes it seem like this is one of your first few PCB designs. I don't want to discourage you but a BGA does not lend itself to rework/rewiring/hacking if something is amiss. Are there other variants of this IC that have leads? What part are you making? If I asked a carpenter if it was easy to make a chair, they'd say yes, but I'd personally end up with a crappy table. \$\endgroup\$ – scld Jan 15 '16 at 15:28
  • \$\begingroup\$ Yes , it does. I think I will use the other part instead \$\endgroup\$ – red car Jan 15 '16 at 15:35
  • \$\begingroup\$ I think that's the best way to go (unless you really need the space). Depending on what you're doing with the chip, you may be able to remove a few layers in the final board by going with the leaded option. \$\endgroup\$ – scld Jan 15 '16 at 15:39
4
\$\begingroup\$

Looks like you have a 0.5mm-pitch BGA. You may even have to use via-in-pad and 6 layers to get this to work. Below is a suggested 6-layer layout from Lattice that does not require via-in-pad.

enter image description here

\$\endgroup\$
2
\$\begingroup\$

With the solder mask as shown, you should not route between pads on the top layer. The reason is that if the solder mask relief for a pad also exposes a track connected to a different net, then there's a high risk of the solder ball bridging between the pad and the track and causing a short circuit.

For a 1-mm pitch BGA it's usually possible (with a high quality pcb shop) to reduce the solder mask reliefs enough to allow routing at least one 4 or 5 mil track between pads.

As the comments and other answers have said, if this is a 0.5-mm-pitch BGA, you'll very likely need to use higher-cost processes, such as multi-layer board, narrow tracks, via-in-pad, etc. to route into this device.

\$\endgroup\$
0
\$\begingroup\$

It all depends on your chosen design rules.

Your PCB manufacturer will have several sets of rules for the minimum width for your pads and tracks, and the minimum spacing between tracks and other features. They will have a cheap set of rules, with large dimensions, that are easy to achieve. They will also have a premium set of rules, with tighter dimensions that they will need to work harder to maintain (more careful alignment and control of etching conditions). The thickness of copper can also affect these distances, thicker copper means more undercutting. The last time I looked, 4 thou was expensive, 8 thou was easy. YMMV.

Decide how much you want to spend on their process, and get the correct figures for minimum track and gap widths. Then measure the distance between the pads and see whether the numbers add up. Or put these figures into your layout program DRC (Design Rule Checker), route a track between the pads, and see whether it's allowed.

\$\endgroup\$
  • \$\begingroup\$ These are 0.25mm balls. Can I route it on a 2 layer board? \$\endgroup\$ – red car Jan 15 '16 at 14:38
  • \$\begingroup\$ No, i don't think you can do it in 2-layer board. You have to put lot of vias beneath the BGA package and bypass caps. \$\endgroup\$ – ammar.cma Jan 15 '16 at 15:03

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.