Hi Paul-
I don't believe your graphics show a condition where resin is starved. I believe the graphic with the non-functional pads NOT removed just shows "telegraphing" of internal features to outer layers: The resin appears to have compacted between the non-functional pads, forcing even more resin in towards the via stacks. This can result in problems with trying to make the outer layers and/or silk screening and solder pasting, but not internal voids.
If you were to add metal fills on every layer between the vias, then your pictures will look very different: There will be LESS total metal where the via stacks are, so if you leave out the non-functional pads you will get "sags" at the via locations, not "posts", as you show. The main reason fabricators like to remove non-functional pads is to improve yields due to inner layer etch resolution problems. On dense designs, layers with non-functional pads often have planes/pours/fills or traces immediately adjacent to where the pad would have been.
On the other hand, if you don't have a high level of metal loading and are using thick conductors and thick prepregs then your pictures are accurate.
I think we might be able to agree to recommending that for most circumstances the amount of copper on inner layers which intersects a vertical line (like a "phantom" drill) going through a board should be close to the same no matter where you put that line or you may get a lot of "telegraphing" to the outer layers. This copper level can be balanced by a combination of increasing or decreasing copper loading on internal layers or removing non-functional pads on inner layers.
Wayne
From: Paul Reid [mailto:[log in to unmask]]
Sent: Friday, January 18, 2013 10:55 AM
To: TechNet E-Mail Forum; Wayne Thayer
Subject: RE: [TN] PCB design/build question about via construction
I always assume that the hole size is small due to HDI. It can be an advantage to put "non-functional pads in" larger hole sizes.
What I am saying is that with non-functional pad out there is no resin starvation in the PTH. With non-functional pads in there can be resin starvation between the non-functional pads and a "telegraphing" of the internal image to the outer layers. Of course this depends on the percent resin, glass style and the thickness of the copper foil. There may be a condition of "glass lock' or glass crush with some constructions.
What we find is that, generally, on small hole sizes, there is an improvement in thermal cycles to failure with non-functional pads out.
I have included two graphics in this email. I don't know if the email will be forwarded with the graphics in or not.
[cid:[log in to unmask]]
[cid:[log in to unmask]]
Sincerely,
Paul Reid
Program Coordinator
PWB Interconnect Solutions Inc.
235 Stafford Rd., West, Unit 103
Nepean, Ontario Canada, K2H 9C1
613 596 4244 ext. 229
Skype paul_reid_pwb
[log in to unmask]<mailto:[log in to unmask]>
-----Original Message-----
From: TechNet [mailto:[log in to unmask]] On Behalf Of Wayne Thayer
Sent: January 18, 2013 9:15 AM
To: [log in to unmask]<mailto:[log in to unmask]>
Subject: Re: [TN] PCB design/build question about via construction
I disagree. And if you review the TechNet archives, as recommended previously, I think you will see general agreement with the following:
Resin-poor is due to too much volume and not enough resin. If you add more copper, then there is less volume, so the resin can fill it. If you have thin prepregs and thick copper, then there is a higher probability of having resin starvation if you leave out the copper. If you put the copper in, it will squish the resin out into the adjacent void and provide higher resin concentration in the electrical isolation area where you need it.
Leaving the pads in gives better seals as noted above, but can make etching more difficult, especially on plane layers with small backoff. If it's not a "stressed" design (thin prepregs) then I leave the decision to the board fab house.
Wayne Thayer
-----Original Message-----
From: TechNet [mailto:[log in to unmask]] On Behalf Of Paul Reid
Sent: Friday, January 18, 2013 8:54 AM
To: [log in to unmask]<mailto:[log in to unmask]>
Subject: Re: [TN] PCB design/build question about via construction
I vote on non-functional pads out. You get an area that is resin poor if you have a stack of non-functional pads. The stack of pancakes, as it were, "telegraphs" the image of the pads to the outer layers. The resin in the stack is depleted because there is copper on every layer.
What we suggest is to leave three or four non-functional pads in but not in the center zone of the board.
Sincerely,
Paul Reid
Program Coordinator
PWB Interconnect Solutions Inc.
235 Stafford Rd., West, Unit 103
Nepean, Ontario Canada, K2H 9C1
613 596 4244 ext. 229
Skype paul_reid_pwb
[log in to unmask]<mailto:[log in to unmask]>
-----Original Message-----
From: TechNet [mailto:[log in to unmask]] On Behalf Of David Bealer
Sent: January 17, 2013 4:13 PM
To: [log in to unmask]<mailto:[log in to unmask]>
Subject: [TN] PCB design/build question about via construction
On an internal copper plane(pour) where a via intersects the plane but doesn't connect, should we remove the pad on that plane for that via? I would think that it would add some measure of structural support for the via if we left it in place. Am I wrong?
Thanks,
David Bealer
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]<mailto:[log in to unmask]> ______________________________________________________________________
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]<mailto:[log in to unmask]> ______________________________________________________________________
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]<mailto:[log in to unmask]>
______________________________________________________________________
______________________________________________________________________
This email has been scanned by the Symantec Email Security.cloud service.
For more information please contact helpdesk at x2960 or [log in to unmask]
______________________________________________________________________
|
