Join our Ask Me Anything about via design where you can ask us questions on:
• Blind, buried and microvias
• Stitching vias
• Via stub length and backdrilling
• And much more!
Question submission window: Through August 21st
Why is back drilling still used in PCB design even though blind and buried vias are available? Discuss the scenarios where back drilling might be preferred over these via types.
1 Like
This pretty much comes down to cost and space. The simple and least expensive approach is to laminate all the layers in one press cycle – “Single Lam” – then back drill to break unwanted connections between layers which can replicate a blind/buried via. Problem is everything starts as a through hole which takes up a lot of space. True blind and buried vias can’t go all they through the board due to circuitry running either above or below them. Also laser vias have limited depth and rarely connect more than two layers. All this requires the use of sub-assemblies and sequential/multiple lamination cycles which substantially drives up the number of process steps and cost.
1 Like
How many microvias can you reliably stack on top of eachother for a class 2 or class 3 PCB these days?
1 Like
Hi
Thanks for your great idea
- Could you please show a demonstration about how vias are manufactured?
I know that some PCB fabrication companies can not manufacture buried or blind vias; why the fabrication of them is difficult? - May increasing the number of the stitching vias have a disadvantage? I think that more stitching vias is better because (a) it can help in shielding HF EM waves, (b) it can make the HF voltage difference between the GND layers and also copper pouring part less so that it decreases the RE or RS problems and (c) it can provide better current return path (with smaller loop area)
- is it recommended to add current return vias every where the current changes the layers? I mean, is adding a via between the reference planes to provide a lower inductance path for the return current really important?
- about the above question, what if the current for the signal is flowing in the power planes (with two different voltage values), in this case no vias can be added in between the two reference planes … So is it why we should locate a GND layer close to every signal layer in our stack-up (to be able to provide a via for current return)?
- To have a low inductance via, is it better to implement a big-diameter via or just increasing the number of small-diameter vias? Is there any formula for that?
- How vias change the impedance matching? How should the designers consider the via impedance in the calculations? for example what is the formula for calculating the characteristic impedance of one via pair (imagine a via close to its current return via)?; i think it probably has to be a formula similar to the formula of the characteristic impedance of the microstrip line because in high frequencies (that the impedance matching maters more), because of the proximity effect in differential currents the current will flow in the close faces of the two vias …
- Generally, what considerations should the designers take to ensure that the SI/PI/EMC will remain OK?
Thanks
1 Like
Do laser vias and/or controlled depth drilling require extra laminations?
Is there any reason to prefer backdrilling over controlled-depth if the fab can do controlled-depth? (Are there even sensible ways to do backdrilling without being able to do controlled-depth drilling?)
1 Like
4 is pretty easy. Can do 5 but that’s starting to push it a bit. It’s not the number of Vias but the number of press cycles the material can withstand. Testing some new materials that are designed to handle more cycles so expect the number to increase fairly soon.
1 Like
You should register for our next virtual tour: Facility Tour | Sierra Circuits
This question involves more than will fit here. There are so many things that make up this topic. I would refer you to PCB Handbook by Coombs.
Of course there is a limit for anything, so if your vias were so close they started to overlap, you’ve gone too far. But assuming they don’t interfere with anything else (components, traces, etc.) then the general rule is the more the merrier.
Yes, it is.
I’m not sure I understand.
Again, there’s more than one factor you need to consider to answer this. If you have room for a larger via that’s good. Also vias are usually pretty small already so it’s hard to make them smaller and still drill them successfully, and are there any thermal issues that can capitalize on multiple vias? All things being equal I would opt for a few smaller ones over one large one.
1 Like
Sierra Circuits provides a tool for calculating via impedance. Try it here: Via Impedance Calculator | Sierra Circuits
Plan. Plan stackup. Plan layers. Plan impedances. Plan trace widths. Plan routing. Plan vias. Plan component placement.
This is a basic explanation but the difficult part of building boards with blind and buried vias is getting everything to line up/register after multiple lamination cycles as the material shrinks during each cycle. For example, the center core of a 12”X 18” panel with 2 sequential laminations is usually stretched/scaled around + 20 mils in the 12” axis and +30 mils in the 18” axis to end up being nominal after all the shrinkage. If you have a design with 3 mil line & space and 5 mil laser vias this is a lot to compensate for. A fabricator needs a software system to predict material movement, an X-ray drill to confirm the movement and drill alignment targets based on internal fiducials tied to internal movement, Vision and Laser drilling systems that can align to these targets and Laser Direct Imaging that aligns and scales each panel using targets tied to the internal movement. Aside from the original prediction all of this gets repeated for each lamination cycle. The equipment is expensive and requires a lot of engineering support to make it all work and not all shops have the resources.
1 Like
If there are only laser vias on the outer layers then no extra lamination cycles are needed. Same for controlled depth unless it’s used in a sub-assembly where additional cycles are required. Controlled depth is a term that usually relates to creating new connections between layers much like a laser via while back-drilling is a term for breaking connections in an existing plated through holes. From a process standpoint they are virtually the same – it’s just a matter of controlling the drill machine’s Z axis travel to a selected depth.
(1) For a crude through-hole via, you can just drill straight through. There are still instructions that talk about putting a sacrificial layer under a huge stack of PCBs so that you don’t even have to worry about how deep to drill. For blind and buried vias, you have to do something more carefully. @steve.carney can better explain what you have to be careful about, including which parts you should be careful about even if you don’t strictly need to, but the simplest-thing-that-could-possibly-work is a much higher bar for blind and buried vias.
(2) Many online resources (and presumably plenty of engineers) talk about blind and buried vias as also implying much smaller (diameter) holes (more delicate, and harder to plate), and often implying denser routing (more chances to mess up, more difficult to etch) and sometimes implying (more expensive to buy) laser drills. Strictly speaking, that isn’t true, but … from a commercial perspective, it might be that almost no large customers will pay for blind/buried vias unless they also want the other advanced stuff.
Is doubling or quadrupling the number of vias likely to affect cost in 2024?
@s_akbarivash
I think you were asking about signals that start out referencing a 5V power plane, and transition to referencing a 3V power plane, or a ground plane.
Yes, there should still be vias nearby for the return current to flow through, but they might be carrying +3V or +5V instead of ground, and they should probably lead to a capacitor instead of being sufficient on their own.
And … Try not to do that. Apparently, it is like adding extra gearsets to a drivechain. In theory, it should work. In practice, no gear is 100% efficient, and if you add a bunch when you don’t need to, theory and practice may start to get farther apart.
Yes, that is part of why reference planes should normally be ground. There are other reasons too, but the ones I know about also mostly boil down to Keep It Simple.