Sorry, must disagree with you, on this one as both ex-fab and
ex-assembler guy, or, at least, qualify your remarks.
In particular, it is essential when the inner layers have more than 35
um copper to have "dummy pads" or when there may be high voltage or high
impedance tracks in proximity to the hole barrels, even respecting the
design rules. Furthermore, although dummy pads take up inner layer real
estate there is no risk, with most CAD systems, of a track-to-pad
violation. With the tolerance of positioning the inner layer and the
hole drilling position, plus the ingress of metallising solution into
the surface micrometres of the hole barrel, this cannot always be
guaranteed without the pads. Finally, my practical experience has shown
that the "loose" lamination without pads is much more prone to produce
conductive anodic filaments than the "tight" build-up with pads.
My recommendation each time is to have inner layer "dummy pads". Their
diameter should be such that, with the accumulation of tolerances, the
"crown" will always be intact after drilling. Under any of the
circumstances outlined at the beginning of the last paragraph, this
recommendation becomes quasi-mandatory.
Finally, for your thoughts: I know of no CAD autorouter or design rules
system that modifies the design rules so that the spacing from the
nominal hole barrel to a track takes into account the mechanical
tolerances of the hole diameter, position and layer position. This means
that the general spacing rules must be set more generous than would
otherwise be necessary, resulting in more practical loss of real estate
than with dummy pads. The only way round this dilemma would be to do the
autorouting with copper inner pads and then to remove them subsequently.
Brian
Genny Gibbard wrote:
>
> Fascinating stuff. We had a board vendor at one point that wanted us to put
> pads on all the layers of a PTH. I thought the reason given was to help the
> hole plating process. Our standard block for multilayer boards
> automatically puts pads on all layers and if not a ground via, it also
> clears the ground plane away around it on all layers. I've never heard of
> any of the problems mentioned over the last few days.
> It's kind of funny, the amount of things I hear about on this forum that
> question things or dispute things that we've never really paid much
> attention to in our own layouts makes me fascinated that this co. has gotten
> as much product out the door working as it has over the last dozen years. I
> guess Murphy's law isn't always on duty.
>
> -----Original Message-----
> From: Hinners Hans M Civ WRALC/LUGE [mailto:[log in to unmask]]
> Sent: January 17, 2002 4:03 PM
> To: [log in to unmask]
> Subject: Re: [TN] Remove unused "dead" pads on internal layers
>
> Hi All,
>
> Now that I think of it we always stuck our nonfunctional pads in places we
> didn't have to drill. But I'm on the list to learn - thanks to Warren,
> Werner.
>
> Roger, this sounds very weird - granted I've only been in the industry since
> '98. There are very good reasons to use nonfunctional pads. Now I know not
> to use them in PTHs (& Route areas I imagine). I wonder if people are
> making this more difficult than it has to be - we've always used decent
> sized dots so they wouldn't pop off of the core from rough handling or
> processing. We kept them far enough away from traces to avoid etch problems
> - we're not talking about something that has to have a critical feature
> size. They may have been struggling with metallic contamination but
> non-functional pads should be a fixable problem - no?
>
> If they were truly having problems with non-functional pads then they must
> have had the same trouble with the functional pads? Houston . . . . we've
> had a problem.
>
> Hans
>
> Integrity First - Service Before Self - Excellence in All We Do
> ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
> Hans M. Hinners
> Electronics Engineer
> Warner Robins - Air Logistics Center (WR-ALC/LUGE)
> 226 Cochran Street
> Robins AFB GA 31098-1622
>
> mailto:[log in to unmask]
>
> Com: (478) 926 - 5224
> Fax: (478) 926 - 4911
> DSN Prefix: 468
>
> -----Original Message-----
> From: Roger M. Stoops [mailto:[log in to unmask]]
> Sent: Wednesday, January 16, 2002 2:10 PM
> To: [log in to unmask]
> Subject: Re: [TN] Remove unused "dead" pads on internal layers
>
> I have been following this thread with interest. When I asked a pcb vendor
> about having non-functional pads in the inner layers, they said it was not
> a good idea, that the unattached pads/lands would move around, or "float,"
> and cause potential mfg problems, such as shorts to other copper.
> Question: Is there any truth to this statement, or is this just an old
> husband's tale?
> TIA,
> Roger M. Stoops, C.I.D., PCB Designer
> [log in to unmask]
>
> Trimble
> Engineering and Construction Division
> 5475 Kellenburger Rd.
> Dayton, OH 45424-1099 USA
> Ph: +01 937.233.8921 or +01 937.233.4574 ext 288
> Fax: +01 937.233.7511
>
> "<Peter
> George To: [log in to unmask]
> Duncan>" cc:
> Sent by: Subject: Re: [TN] Remove unused
> "dead" pads on internal layers
> TechNet
> <[log in to unmask]
> ORG>
>
> 01/15/02
> 09:09 PM
> Please
> respond to
> "TechNet
> E-Mail
> Forum.";
> Please
> respond to
> peter.duncan
>
> Hi,
>
> Actually these "unused" pads are replicates of the hole "rules" created for
> the surface layers. Most routing packages, or routers, seem to do this by
> default for each layer to save manual replication where traces, etc are to
> be connected. (At least PADS, Alegro and Mentor do). On the grounds that
> it's always easier to destroy than to build, it's easier to delete pad data
> than to create it, so it's put in by default as there's a good chance it
> will be needed.
>
> I still say you should consider hole barrel strength/support issues before
> just deleting them - e.g. they can constrain the "resin recession" and hole
> wall pull-away that have been recent threads on this forum. Think of the
> "unused" pads as 'wall ties' holding the copper at frequent intervals to
> the hole wall. Copper bulging or pull-away in the event of recession or
> whatever is reduced.
>
> Peter Duncan
>
> Hinners Hans M Civ
> WRALC/LUGE To: [log in to unmask]
> <Hans.Hinners@ROBI cc: (bcc: DUNCAN
> Peter/Asst Prin Engr/ST
> NS.AF.MIL> Aero/ST Group)
> Sent by: TechNet Subject: Re: [TN] Remove
> unused "dead" pads on
> <[log in to unmask]> internal layers
>
> 01/15/02 09:40 PM
> Please respond to
> "TechNet E-Mail
> Forum."; Please
> respond to Hinners
> Hans M Civ
> WRALC/LUGE
>
> Hi Patrick,
>
> As others have said, I don't think the class of board matters for "unused"
> pads. It all depends on what your procurement documentation states, are
> you
> building to drawing or is there a clause that says process improvements
> that
> do not affect functionality are permissible.
>
> "Are they really unused pads?"
>
> They may be electrically nonfunctioning but they are there for a reason -
> better lamination quality (avoiding low pressure areas or excessive prepreg
> flow), better hole wall quality, better plating quality (esp. for any
> isolated traces), reduced loading of your etch solution or better thermal
> loading during assembly.
>
> Hans
>
> Integrity First - Service Before Self - Excellence in All We Do
> ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
> Hans M. Hinners
> Electronics Engineer
> Warner Robins - Air Logistics Center (WR-ALC/LUGE)
> 226 Cochran Street
> Robins AFB GA 31098-1622
>
> mailto:[log in to unmask]
>
> Com: (478) 926 - 5224
> Fax: (478) 926 - 4911
> DSN Prefix: 468
>
> -----Original Message-----
> From: Patrick Lam [mailto:[log in to unmask]]
> Sent: Friday, January 11, 2002 5:12 PM
> To: [log in to unmask]
> Subject: [TN] Remove unused "dead" pads on internal layers
>
> Hi TechNetters,
>
> For class 3 boards, is it acceptable to have unused pads removed on
> interanal
> layers.
>
> Thanks,
> Pat
>
> ----------------------------------------------------------------------------
> -----
> Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
> To unsubscribe, send a message to [log in to unmask] with following text in
> the BODY (NOT the subject field): SIGNOFF Technet
> To temporarily halt delivery of Technet send e-mail to [log in to unmask]: SET
> Technet NOMAIL
> To receive ONE mailing per day of all the posts: send e-mail to
> [log in to unmask]: SET Technet Digest
> Search previous postings at: www.ipc.org > On-Line Resources & Databases >
> E-mail Archives
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
> information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700
> ext.5315
> ----------------------------------------------------------------------------
> -----
>
> ----------------------------------------------------------------------------
> -----
> Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
> To unsubscribe, send a message to [log in to unmask] with following text in
> the BODY (NOT the subject field): SIGNOFF Technet
> To temporarily halt delivery of Technet send e-mail to [log in to unmask]: SET
> Technet NOMAIL
> To receive ONE mailing per day of all the posts: send e-mail to
> [log in to unmask]: SET Technet Digest
> Search previous postings at: www.ipc.org > On-Line Resources & Databases >
> E-mail Archives
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
> information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700
> ext.5315
> ----------------------------------------------------------------------------
> -----
>
> ---------------------------------------------------------------------------------
> Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
> To unsubscribe, send a message to [log in to unmask] with following text in
> the BODY (NOT the subject field): SIGNOFF Technet
> To temporarily halt delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL
> To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
> Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
> information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
> ---------------------------------------------------------------------------------
---------------------------------------------------------------------------------
Technet Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF Technet
To temporarily halt delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------
|
