5
\$\begingroup\$

I am new to PCB design. I am creating a 4 layer PCB with the following layer stack:

Signal (1) - GND (2) - Vcc (3) - Signal (4)

Now, I'll need Vcc and GND on both the signal planes. This means I'll need blind vias from 1-2, 1-3, 2-4, 3-4 but the PCB manufacturer I chose said that they cannot do blind vias like that - it has to be 1-2, 3-4 and such. Now I am stuck and have no idea how I shall route Vcc and GND. Please help.

\$\endgroup\$
  • 5
    \$\begingroup\$ Why do you need blind vias? Some manufacturers can produce them at an increased cost but because of the cost most PCBs I have seen, and everyone I have designed, have avoided them entirely. All my vias are on all layers. This reduces your maximum tracking density slightly but has never been an issue for me. \$\endgroup\$ – Warren Hill Sep 13 '17 at 5:47
  • \$\begingroup\$ Hi Warren, the reason is when I am using through hole via, I am making it hard putting components on the other side of the PCB. And particularly in Altium, its too hard to move tracks and components as they keep disconnecting. Too hard to move the vias and manage space to put other components on the other side.. So blind via definitely saves PCB space and make it compact. \$\endgroup\$ – Rakesh Mehta Sep 13 '17 at 7:02
  • 5
    \$\begingroup\$ In Altium turn on push and shove routing, and do all your component placement BEFORE you start routing. Placement is everything in PCB design, get this right and the thing usually mostly routes itself, get it wrong and you have a nightmare. I have used blind and HDI microvia, but that put the cost of 5 prototype boards up to £2,500 for the bare boards, for that product it didn't matter, but simple vias are to be preferred when possible. 0.2/0.5 finished is doable without much cost premium by most better board houses. \$\endgroup\$ – Dan Mills Sep 13 '17 at 10:34
10
\$\begingroup\$

Usually you just use normal vias that go all the way through. This usually isn't a problem unless you need to worry about stubs (RF, though back-drilling is an option) or you're shooting for very high density where the through vias will get in the way.

\$\endgroup\$
10
\$\begingroup\$

No, you do not need any blind vias.

Not unless you have some very dense tracking, and if you're just starting in PCB design you do not want to be doing that.

The vast majority of PCBs use vias all the way through. If you don't need a ground or VCC on both sides of the board, then just ignore the unwanted one, it doesn't take up much space.

FWIW, you probably don't need a VCC plane either. You lose a whole layer that you could otherwise use for tracking signals. Just route the VCC as a signal, in wider tracks suitable for the current of course.

With 3 layers for tracking signal and supply, that makes it easier to do what's really important, which is to leave your ground plane whole. Don't be tempted to squeeze a last track through on the ground plane layer. Not if you're just starting PCB design. When you have more experience, you'll know under what limited circumstances you can break this rule. When you have even more experience, you'll set things up so you don't need to.

\$\endgroup\$
  • \$\begingroup\$ Thank you for all the suggestions. It seems I should really remove the blind vias and use through holes.. I know that I don't need the GND plane but I am a little confused and not very much confident with polygon pours on the signal layers.. But I'll try.. Thank you again \$\endgroup\$ – Rakesh Mehta Sep 13 '17 at 7:14
  • 3
    \$\begingroup\$ @RakeshMehta Don't do polygon pours. Do use a ground plane. Don't use a VCC plane. \$\endgroup\$ – Neil_UK Sep 13 '17 at 7:43
  • \$\begingroup\$ Hi @Neil_UK, so how do I route VCC to both of the signal layers? Will not that increase resistance in the Vcc rail if I route Vcc though Vias? \$\endgroup\$ – Rakesh Mehta Sep 13 '17 at 8:51
  • 2
    \$\begingroup\$ While it's true that a via has non-zero resistance, and a track has more resistance than a plane, the magnitudes are so small that it's totally irrelevant, unless you are running serious power, so several amps to power FETs for instance. Once your supply tracks are wide enough that you're only dropping a few mV across them, then that's enough. I would recommend the following layup. 1 components and a few tracks, 2 ground, 3 Manhattan EW and 4 Manhattan NS, and a few components if required. That gives you an organised tracking, and you can use 3-4 blind vias if you want to improve density. \$\endgroup\$ – Neil_UK Sep 13 '17 at 9:20

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.