I have a four layer stack with Top Inner1 Inner2 Bottom
Is there a way to span a via from Bottom to Inner1 without connecting it to inner2 ? The software we used before had an option to add an annular copper free area around the via on specific layers to prevent these from being connected.
If the inner layers are power planes and not the same net then you can tell it to remove pads on those layers. Otherwise you can control this by using an Area, in a similar manner to the other system.
I have a four layer stack with Top Inner1 Inner2 Bottom
Is there a way to span a via from Bottom to Inner1 without connecting it to inner2 ?
You say you are going from "Bottom" to "Inner1" which implied to me a blind via through three layers of a four layer board.
This is an unusual stack up for a blind via PCB if the drill is mechanically drilled.
On a four layer board utilising blind vias a suitable stack up would be a blind via through "Bottom" and "Inner2" and the PCB would be built using two double sided pieces of laminate and a single bonding process.
If the board is using laser microvias then it's not unusual to laser drill down through two layers to meet the third layer and a stop pad, however in this case the PCB fabricator would usually require a pad on the intermediate layer (Inner2) as the laser drilling process "counts" the pads as it burns down through the layers.
Thank you both for the answers but this is not what I wanted to hear (-; With an advanced PCB solution, it must be possible to get off the beaten track and to create solutions which do not apply standard layer stacks !
I can imagine several situations, where it does not make sense to reserve two of four layers for power and ground.
I now solved that with some boolean operations in our CAM solution. I wanted to attach an image of what I finally made and what I would expect from Pulsonix, but uploading an image result in a "server 500" error. Therefore I uploaded the file here: www.xecro.com/upload/2015-01-06_09h03_33.png
If you want to connect from Bottom to Inner1 (passing through Inner2), I don't see the problem.
You need a hole though inner 2 though.
And no - you don't have to reserve an entire inner layer as a power plane. Some of my designs use inner places for power and signals (or multiple power pours).
When the crossing plane is not part of the net of the 2 "sandwiching" planes, a connection isn't made.
Are you asking that there should be NO pad on the non-connecting plane?
That's totally possible with a custom pad stackup. (I've actually done it before on a board supporting high voltages).
So -- I maybe I don't understand the problem you're having.
Is this a blind via from Bottom to Inner1 with no hole appearing on Top? This is what I took the requirement to be as the original question said the via span required was from Bottom to Inner 1. My answer was based on the assumption that the design intent was a blind via.
If the via is a normal via, not a blind via, and appears through the whole board, then as has been said, it's easy to remove a connection to an inner layer plane by adding an area on that layer, or if it's a via on a different net from the plane, to remove "non-functional" pads in Pulsonix.
The PCB fabricator will usually remove all non-functional pads in the CAM editing stage. The barrel of a through hole via will plate all the way from the top to the bottom layer - there's no requirement to have a copper pad on the inner layers. "Non-functional" pads on the inner layers may be needed for vias for some board designs but not in the majority of cases.
To remove non-functional pads on an inner layer, Edit Technology > Layers and select the particular layer, press Edit and you will find in the bottom right corner "Suppress Unconnected Lands" where you can toggle Pads and Vias independently of each other.
Posted - 03 Jan 2015 : 12:02:20
