Bob Vanech wrote:- > The original question was in respect to larger internal pads in > their designs and why, since we have never seen or done that ourselves. > I was just interested in the rational that went into making that design > requirement for possible implementation into our product line if like > requirements occur. > > After all is said and done, the message is: Whatever set of design > parameters are generated, communicate with your fabricator NOW to reduce > problems later. Hi Bob, I commend your last para and hope all on the forum are of like mind. On the original question, if you want to know why larger pads on internal layers are a good idea, read on and please forgive me if this is too simplistic. Basically the main problem with inner layers is the registration of the drilling to the inner layer pattern. The extra tolerances which have to be considered are:- Photo-Tool stability 0.1 mil per inch Laminate movement 0.25 mil per inch Layer to Layer alignment 2 mil Core to Core alignment 2 mil Tooling hole accuracy for drilling 2 mil Drilling machine tolerance 1 mil The registration of the outer layers is affected by the first and the last but not those in between and so the tolerance has to be greater for internal layers. It follows that the pad sizes must be greater for inner layers than for external layers. The main reason is not breakout. The most important reason is to make sure the clearance between the plated holes and any adjacent copper is not reduced below the minimum specified which I would say should be not less than 7 mils. If the inner layers are designed with 2 mil land and 7 mil space, the fabricator will need to increase the space to around (say)14 mil to achieve an acceptable yield on a large production panel. A prototype or pre-production batch could be manufactured with less clearance on a smaller panel and achieve acceptable yield, but it would be more expensive to produce in production quantities. The alternative is to make the minimum land 9 mils and the space 7 mils to ensure that there is no possibility of breakout. This is much better than making the minimum land 2 mils and the spacing 14 mils for obvious reasons. It is just a question of how to achieve the end result without causing undue restrictions on the track density. Making the lands bigger is a neat solution although the reason may not be obvious. I had a design where landless holes were within 6 mils of adjacent ground planes on inner layers, and on finished pwb's manufactured by another less dilligent supplier showed a spacing of 1 mil after micro- sectioning. The customer said they had been receiving pwb's without any problems but when the evidence was presented, the decision was to give us the business. I don't know how many potential field failures there were but suspect many, and probably a high dropout in assembly. There was a lot of flack initially, not least from my sales department who could not see why we should reject a design that another major manufacturer was making. These are the pressures that fabricators are under but there is only one right answer. To all designers out there, please don't forget the hole is a copper land and the clearances must make allowance for the registration variations. Putting lands of suitable size on all holes will make the design much better and the unconnected pads can always be deleted later by the fabricator. I hope this is clear but if there is any question about this please let me know. -- Paul Gould Teknacron Circuits Ltd [log in to unmask] Isle of Wight,UK