|Ask the Experts|
November 6, 2020
Removal of Non-functional Pads from Inner Layers
Should we remove non-functional pads from inner layers. In some cases, it may be necessary to free up space between rows of pads to route additional trace data. I've read articles that favor both options. What is you opinion?
|Expert Panel Responses|
Non-functional copper, is generally used to balance plating. On inner layers, with non-functional copper, this would be a very sophisticated lay up, as it sounds as if there are embedded via's and high-density features.
With that assumption, replacing non-functional copper, with functioning copper features is a 1:1 trade-off. These non-functional features are used to "thieve" amperage and/or plating away from sensitive areas. By putting functional copper in these area's, you are balancing the design, to be less dependent on non-functional copper.
Capital Equipment Operations Manager
Specialty Coating Systems
An interesting question to be sure. Fabricators normally do prefer it, because it makes drilling easier. Copper is a tough, stringy metal, and in general it's a pain to drill through.
On the other hand, removal of all unused pads on thick, high layer count PWBs may result in long distances between points where the PTH copper is "tied" into the hole wall. This can result in somewhat reduced reliability (I've seen examples of this).
Selective removal is one option that may provide the routing flexibility needed, and easy fabrication, while maintaining a few tie points along the depth of high-aspect-ratio vias. One approach might be to leave lands on selected plane layers, even if unattached. The plane layers are not used for signal routing so the presence of pads will not impede routing.
This is a very interesting question. What we find is that,from a reliability point of view, based on thermal cycle evaluations, removing non-functional pads increases the reliability of the PWBs to some degree. It is thought that having non-functional pad "in" will cause the drill to work harder as it drills through the extra copper offered by non-functional pads and increase the temperature internally, aging the material in the barrel of the hole.
Having non-functional pad in is thought to have a tendency to provide stress risers that focus the strain into the barrel of the PTH. What ever the case what we find repeatedly is that non-functional pads "in" reduces thermal cycle to failure by 10% to 20%.
What I suggest that you do is remove most of the non-fictional pads in the central zone of the PWB. Leave in one or two non-functional pad in the top or bottom third of the stack up. This will give you the most reliable construction. You can always test the two different constructions to prove my contentions, using thermal cycling methods.
PWB Interconnect Solutions
Non-functional pads should be removed if this is a signal via.Non-functional pads do not improve reliability from a barrel fatigue perspective and can greatly reduce manufacturability in the drilling process (dulls the drill bit).
IF the via is used for assembly, such as a through-hole solder joint, then non-functional pads can prevent hole wall pull away.
CEO & Managing Partner
Eliminating non-functional pads is a great way to gain some real estate on all types of PCB's, but this practice should be used with caution on flex and rigid-flex printed circuit boards.
Copper plating generally does not bond to flexible materials in the plated through hole as well as it bonds to rigid materials. This is especially true on controlled impedance flex and rigid flex where thicker flex dielectrics are incorporated into the material stack up.
All pads, both functional and non-functional, provide points dispersed along the plated barrel for the plating to adhere to. If all non-functional pads are removed causing the gap between functional pads becomes too great, the plating may start to separate from the hole wall.
I would recommend leaving at least some of the non-functional pads in place on flex and rigid flex boards and attempt to keep then evenly dispersed along the plated through hole wall to avoid possible plating separation.
Senior Applications Engineer
Flexible Circuit Technologies
The additional copper the non functional pads represent can reduce low pressure areas in high layer count boards. There is some evidence that they may also decrease thermal cycle failures in some designs. The trade off is the reduced hit count during drilling and the loss of real estate on the board.Roxanne V. Jones, PJC Technologies, USA
From the manufacturing side, we prefer to see them removed on ground planes. The risk of electrical shorts is greatly reduced. I would suggest leaving them on and only removing them selectively when spacing dictates... keeping in mind that the spacing to the hole is still a factor. Then allow the manufacture to remove them as needed.
No one seems to have commented on one important aspect of the question - pads are being removed to allow additional trace routing. Remember the pad is there to provide a connection to the via.Mike McMaster
The size of the pad then is a good reflection of where you can except the drill to be relative to the layer in the finished board. The spacing between the pad and the trace then represents the minimum possible drill to copper spacing.
Removing the pads to make room for the traces means you are potentially moving the traces closer to the drilled hole and increasing the risk of shorts. Removing non-functional pads is therefore recommended after routing, not before.
It has been an old question. For high-speed PCBs, multi-layer PCBs are inevitable development trend and through via manufacturing is the first problem.Dora Yang, PCBCart
Non-functional pad features great improvement to PTH copper in the process of manufacturing PCB via wall and plays an effective role in stopping via copper from falling and dealing with quality problems such as via wall crack.
Of course, NFP features some variables and performs badly on insertion loss in some circumstances.
Visit https://www.pcbcart.com/article/content/non-functional-Pads-in-high-speed-PCB.html, and I believe this article can give you accurate answers.
With the assumption the original question was only pertaining to thru hole pads, not vias, you may consider instead of removing non-functional pads you decrease their diameter on inner signal layers.C. Herring, NASA-JSC
As a 15+ circuit designer, I can add that there are major advantages to having the non-functional pads removed. First is what we refer to as 'via damage' - in a multilayer PCB board the through-hole via is a multilayer constraint and especially under high-density BGAs the ground and power planes are very much needed for providing low impedance to the IC for decoupling.
When a PTH via passes and assuming a different net than the plane, quite large circular cutout appears on that plane - for clearance. The result of many vias placed under the BGA is a compromised plane. Simply omitting the non-functional pad allows for lesser damage to the internal planes because the cutout can be made smaller, therefore the impedance is reduced and its high-frequency decoupling is improved.
Second, the proper way to protect the via is by plugging it! PTH usually are plugged with epoxy. It's not a significant cost driver and if the board is known to get hot during operation or if generally high reliability is required - via plugging is the better way to go. Lastly, for high-speed signals, you really don't want the reflections coming off the via as the impedance of the via change as the cross-section is non-uniform. Although an extreme case, we recently had an 80GHz signal going on through-hole vias on a custom RF PCB we designed. Just imagine the reflections that may worsen due to the non-functional pads.
|Submit A Comment|
Comments are reviewed prior to posting. You must include your full name to have your comments posted. We will not post your email address.
Free Newsletter Subscription
Circuitnet is built for professionals who bear the responsibility of looking ahead, imagining the future, and preparing for it.
Insert Your Email Address