Electronics Assembly Knowledge, Vision & Wisdom
Ask the Experts
Removal of Non-functional Pads from Inner Layers
Should we remove non-functional pads from inner layers. It may be necessary to free up space between rows of pads to route additional trace data.
Ask the Experts

View the Expert comments below.
,{url:'http://www.circuitinsight.com/videos/experts_final.mp4'}], clip:{autoBuffering:true, autoPlay:true, scaling:'scale' } }).ipad();

Arranged via association with Circuitnet..
See the Expert Panel | Submit A Questions | Join the Panel
Ask the Experts Question
Ask the Experts
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?
S.S.
Expert's 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. 
image
Rodney Miller
Capital Equipment Operations Manager
Specialty Coating Systems
Rodney is currently Operations manager at SCS coatings, Global Leader in Parylene and Liquid Coating equipment. Rodney applies his BS in Computer Integrated Manufacturing from Purdue University, along with 20+ years of Electronic manufacturing and Equipment Assembly, to direct the Equipment business at SCS Coatings. "We provide unique, value added coating equipment solutions for our customers". Including conformal, spin and Parylene coating expertise.
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.
image
Fritz Byle
Process Engineer
Astronautics
Fritz's career in electronics manufacturing has included diverse engineering roles including PWB fabrication, thick film print & fire, SMT and wave/selective solder process engineering, and electronics materials development and marketing. Fritz's educational background is in mechanical engineering with an emphasis on materials science. Design of Experiments (DoE) techniques have been an area of independent study. Fritz has published over a dozen papers at various industry conferences.
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 stackup. This will give you the most reliable construction. You can always test the two different constructions to prove my contentions, using thermal cycling methods.
image
Paul Reid
Program Coordinator
PWB Interconnect Solutions
Paul Reid has over 35 years experience in bare board fabrication, quality and reliability. Working for PWB Interconnect Solutions, which does thermal cycle evaluations (IST) of representative coupons, Paul provides failure and root cause analysis of how PWBs fail. His area of expertise includes how circuit board's copper interconnections and material fails in assembly, rework and in the field, as a result of thermal cycling.
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.
image
Dr. Craig D. Hillman
CEO & Managing Partner
DfR Solutions
Dr. Hillman's specialties include best practices in Design for Reliability, strategies for transitioning to Pb-free, supplier qualification, passive component technology and printed board failure mechanisms.
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.
image
Mark Finstad
Senior Applications Engineer
Flexible Circuit Technologies
Mark Finstad has over 30 years in the flex circuit industry in both design and manufacturing. He is a regular speaker at IPC APEX (Professional development courses) and PCB West (flex circuit design courses). He is also vice chair of IPC-2223 and active member of IPC-6013. Finstad has extensive experience with both domestic and off-shore manufacturing.
Reader Comment
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.  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.
Roxanne V. Jones, PJC Technologies, USA
Reader Comment
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. 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.
Mike McMaster
Reader Comment
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. 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.
Dora Yang, PCBCart
Reader Comment
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
Submit A Comment

Comments are reviewed prior to posting. Please avoid discussion of pricing or recommendations for specific products. You must include your full name to have your comments posted. We will not post your email address.

Your Name


Company


E-mail


Country


Comments


Authentication

Please type the number displayed into the box. If you receive an error, you may need to refresh the page and resubmit the information.



Related Programs
bullet RF Capacitor Material for Use in Printed Circuit Board
bullet BGA Components and Coplanarity
bullet The Effects of PCB Fabrication on High-Frequency Electrical Performance
bullet Electronics Manufacturing by Inkjet Printing
bullet HASL vs. Immersion Gold
bullet Opening Eyes on Fiber Weave and CAF
bullet Study of Various PCBA Surface Finishes
bullet Advances in Conductive Inks Across Multiple Applications
bullet Long Term Thermal Reliability of Printed Circuit Board Materials
bullet Flexible Circuit Materials for High Temperature Applications
More Related Programs
About | Advertising | Contact | Directory | Directory Search | Directory Submit | Privacy | Programs | Program Search | Sponsorship | Subscribe | Terms

Circuit Insight
6 Liberty Square #2040, Boston MA 02109 USA

Jeff Ferry, Publisher | Ken Cavallaro, Editor/Business Manager

Copyright © Circuitnet LLC. All rights reserved.
A Circuitnet Media Publication