Via pads in mid-layers

[David]

Thanks to all who answered - it seems there is nothing significant to be
gained by removing the inner layer pads myself.

mvh.,

David



On Tue, 15 Mar 2005 22:06:12 +0100, Helmut Sennewald wrote:

"David" <david.nospam@westcontrol.removethis.com> schrieb im Newsbeitrag
newsan.2005.03.15.14.14.44.767000@westcontrol.removethis.com...
In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via?

Hello David,
our PCB manufacturer removes the unconnected pads in the inner layers,
because there is no advantage for them in the process.

For higer density cards, reducing or removing the anular ring in
inner layers (or > even the top or bottom layers, if there is no
connection) would free a lot of routing space.

No, you can't route closer when you remove the unused pads.
You must be aware that the drill size is about 4mil more than the
finished hole size and there are also tolerances of the drill position.

Summary: You don't get any clearance advantage when you remove these pads.

Best Regards,
Helmut

 

[David]

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via? For higher
density cards, reducing or removing the anular ring in inner layers (or
even the top or bottom layers, if there is no connection) would free a lot
of routing space.

David

 

[Uwe Bonnes]

David <david.nospam@westcontrol.removethis.com> wrote:

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via? For higher
density cards, reducing or removing the anular ring in inner layers (or
even the top or bottom layers, if there is no connection) would free a lot
of routing space.

The anular ring in the inner layers and the space around it gives the needed
alignment accuracy for the board manufacture. A smaller/no ring needs
higher accuracy meaning a higher price. Talk to the choosen manufacturer if
the premium is worth the freed routing space.
--
Uwe Bonnes bon@elektron.ikp.physik.tu-darmstadt.de

Institut fuer Kernphysik Schlossgartenstrasse 9 64289 Darmstadt
--------- Tel. 06151 162516 -------- Fax. 06151 164321 ----------

 

[nospam]

David <david.nospam@westcontrol.removethis.com> wrote:

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via? For higher
density cards, reducing or removing the anular ring in inner layers (or
even the top or bottom layers, if there is no connection) would free a lot
of routing space.

It won't free a 'lot' of space. You still have to leave clearance around
the hole and the hole size you specified is the finished plated size so the
hole is bigger than you think.

There is also a slight problem that without a pad there is more possibility
of a crevice being left between layers when the board is laminated and when
plating holes there is a possibility the crevice will be plated creating an
internal short. The closer you have tracks to the holes the more likely
this is.

Pads on outer layers provide an anchor for the through hole plating. Plated
holes are barely bonded to the inside of the hole, they are held in place
mechanically by their shape. Without pads there is the possibility of
getting resist down the holes which means they may be partially plated
and/or partially etched, if the problem goes deep enough you may loose
connections to inner layers.

 

[Helmut Sennewald]

"David" <david.nospam@westcontrol.removethis.com> schrieb im Newsbeitrag
newsan.2005.03.15.14.14.44.767000@westcontrol.removethis.com...

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via?

Hello David,
our PCB manufacturer removes the unconnected pads in the inner layers,
because there is no advantage for them in the process.

For higer density cards, reducing or removing the anular ring in
inner layers (or > even the top or bottom layers, if there is no
connection) would free a lot of routing space.

No, you can't route closer when you remove the unused pads.
You must be aware that the drill size is about 4mil more than the
finished hole size and there are also tolerances of the drill position.

Summary: You don't get any clearance advantage when you remove these pads.

Best Regards,
Helmut

 

[Helmut Sennewald]

"Gary Crowell / VCP" <vcp@cableone.net> schrieb im Newsbeitrag
news:bkan311ntegeac3o87e40d5urfu0a18t2s@4ax.com...

On Tue, 15 Mar 2005 15:14:45 +0100, David
david.nospam@westcontrol.removethis.com> wrote:

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via? For higher
density cards, reducing or removing the anular ring in inner layers (or
even the top or bottom layers, if there is no connection) would free a lot
of routing space.

David

Reiterating what some of the other folks have said...

1. It doesn't give you any routing space, unless you had a greatly
oversized pad to start with, because you have to allow clearance for
the (oversize) drill and drill tolerance.

2. The fab folks like to remove unconnected inner-layer pads because
it simplifies their optical inspection and processes, and thus
improves the fab yield a tiny bit. (And its just a quick one-button
click on the CAM system to do it.)

3. You *don't* want to remove pads if you have thick inner-layer
copper (e.g., 2 oz copper power planes), and/or thin dielectric (2-3
mil). Removing the pads can lead to 'resin starvation' in that area,
resulting in voids and shorts between planes. (And I've got the
burned boards to prove it.)

4. Some folks want the pads to stay because it supposedly helps to
'anchor' the barrel of the via. (Other folks say 'taint so; take your
pick.)

5. If you are way up there in the regions where signal integrity is
an issue, removing pads can affect (improve) the capacitance and
inductance of the via, but you have to do 3D field modeling to make
any use of that.

6. If, for whatever reason, you have decided that you want the pads
to stay, you must explicity say so in the fab instructions. Some
fabricators will routinely remove them if not told differently.
Likewise, if you want them removed, you also should say so, or just
remove them yourself.

Gary Crowell CID
Micron Technology

Hello Gary,
your comment in point 3. sounds new to me. It seems I should
ask my board manufacturer about that.
There is one thing about inner pads I have in mind. They told me
that unconnected pads may not hold good enough on the core material
during drilling. They also automatically create tear drops when an
inner pad is conencted.

Thanks for your comments. I will keep it in my library.

Best Regards,
Helmut

 

[Brad Velander]

Helmut,
The comment about the inner pad on a core not adhering very
well during drilling, that would have to be only for a buried
via. One that is drilled while the core is still not laminated
within the stackup. If it is a regular via through the stackup,
it would of course be completely supported top and bottom between
pieces of laminate, can't get more secure than that!
Gary's point 3 is valid but at the extremes. Just think, you
have a heavy plane area and then a large void area, what will
fill and bond between the two void areas while the other Cu plane
areas are setting the final thickness between the two laminate
layers. The prepreg epoxy will flow into that area but possibly
not quite enough to fully, completely, fill and bond it 100%.
Same for very thin prepregs that will have trouble filling the
gap to start with.

--
Sincerely,
Brad Velander

"Helmut Sennewald" <helmutsennewald@t-online.de> wrote in message
news:d1glik$f53$00$1@news.t-online.com...

Hello Gary,
your comment in point 3. sounds new to me. It seems I should
ask my board manufacturer about that.
There is one thing about inner pads I have in mind. They told
me
that unconnected pads may not hold good enough on the core
material
during drilling. They also automatically create tear drops when
an
inner pad is conencted.

Thanks for your comments. I will keep it in my library.

Best Regards,
Helmut

 

[Gary Crowell / VCP]

On Tue, 15 Mar 2005 15:14:45 +0100, David
<david.nospam@westcontrol.removethis.com> wrote:

In a multi-layer pcb, if I have a via going from the top layer to the
bottom layer, is it necessary to have a full pad on the inner layers, or
just on the layers where there is a connection to the via? For higher
density cards, reducing or removing the anular ring in inner layers (or
even the top or bottom layers, if there is no connection) would free a lot
of routing space.

David

Reiterating what some of the other folks have said...

1. It doesn't give you any routing space, unless you had a greatly
oversized pad to start with, because you have to allow clearance for
the (oversize) drill and drill tolerance.

2. The fab folks like to remove unconnected inner-layer pads because
it simplifies their optical inspection and processes, and thus
improves the fab yield a tiny bit. (And its just a quick one-button
click on the CAM system to do it.)

3. You *don't* want to remove pads if you have thick inner-layer
copper (e.g., 2 oz copper power planes), and/or thin dielectric (2-3
mil). Removing the pads can lead to 'resin starvation' in that area,
resulting in voids and shorts between planes. (And I've got the
burned boards to prove it.)

4. Some folks want the pads to stay because it supposedly helps to
'anchor' the barrel of the via. (Other folks say 'taint so; take your
pick.)

5. If you are way up there in the regions where signal integrity is
an issue, removing pads can affect (improve) the capacitance and
inductance of the via, but you have to do 3D field modeling to make
any use of that.

6. If, for whatever reason, you have decided that you want the pads
to stay, you must explicity say so in the fab instructions. Some
fabricators will routinely remove them if not told differently.
Likewise, if you want them removed, you also should say so, or just
remove them yourself.

Gary Crowell CID
Micron Technology