Speccing 4-layer boards

[Spehro Pefhany]

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.


Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
speff@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com

 

[John Larkin]

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany
<speffSNIP@interlogDOTyou.knowwhat> wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.

FR-4 has Er around 4.6, and 1 oz copper is 1.4 mils, so I use those
numbers and impedances seem to come out close. It seems to me that the
cheapie multilayer houses (in the back of EE Times and such) often
prefer 12 mil dielectrics on the outer layers, about 30 for the inner,
which is sort of silly but will give you 75 ohms microstrip with an 8
mil trace. Could get lossy with such skinny traces.

Probably calling out 20+20+20 with a few mils tolerance on the
dielectrics is safe for multisourcing. Lots of board houses will tweak
your art to a target impedance, but I don't like board houses messing
with my dimensions.

I'm just finishing up a board right now. 2 layers, 0.062 FR-4, 0.72
square inches total. It's a tiny 50 MHz oscillator. The reference
designators are 50 mils high, which means most nobody can screen them
legibly, so I guess I'll skip the silkscreen step. Last week we did a
board that must be about 0.1 square inch.


John

 

[keith]

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.

Specify the impedance you want and let them guarantee it, or tell you what
you need to do for *them* to guarantee it.

--
Keith

 

[Rich Grise]

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.

They have no clue. I speak from experience here - I had to spec a PCB
that could handle insane amounts of current, and couldn't get the guy
at the board house to give me a catalog, or list of options, or menu,
or anything - he said, "put your spec on the drawing, and we'll do it."

So, look up the constants on FR4, design your thing, scale it such that
they can do it with sane tolerances, spec it and order it.

They call out copper thickness by "ounces", and everything else is
limited only by the resolution of the artwork, and the thickness
of the FR4 - the only thing you can realistically nail down a board
vendor on is tolerance of thickness, and _possibly_ a list of options.
(for thickness of the interlayer FR4). Everything else is fair game.

Good Luck!
Rich

 

[Mac]

On Sun, 06 Mar 2005 20:54:09 -0800, John Larkin wrote:

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany
speffSNIP@interlogDOTyou.knowwhat> wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.



FR-4 has Er around 4.6, and 1 oz copper is 1.4 mils, so I use those

When I worked at a large company making SBC's, we used 4.2 for the
FR4 dielectric. It doesn't make a huge difference, but where did you get
4.6?

numbers and impedances seem to come out close. It seems to me that the
cheapie multilayer houses (in the back of EE Times and such) often
prefer 12 mil dielectrics on the outer layers, about 30 for the inner,
which is sort of silly but will give you 75 ohms microstrip with an 8
mil trace. Could get lossy with such skinny traces.

I think choosing a dielectric thickness for 75 Ohms and 8 mils trace
widths is reasonable. We did 5 mil traces standard and 4 mil quite often,
especially for video, since it needs 75 Ohms. (Most of the traces were at
a slightly lower impedance, and therefore wider) I never measured the
loss, but the video seemed to work fine. We usually did the boards with
"controlled impedance," meaning that the board house was supposed to
guarantee the impedance to within 10%, but we had to pick realistic
geometries to give them something they could work with. I usually just
tried to make it so the traces were a little bit wider than they needed to
be to get the target impedance with the given stackup (Because it is easy
for them to make the traces narrower, but not so easy to make them wider
if there isn't enough clearance.) This might be a good strategy in
the current situation as well.

regards,
Mac

 

[nospam]

keith <krw@att.bizzzz> wrote:

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.

Specify the impedance you want and let them guarantee it, or tell you what
you need to do for *them* to guarantee it.

Which will probably exclude 3/4 of all board houses and cost significantly
more - not much flexibility in sourcing.

 

[Ken Smith]

In article <jqmn21l5i2o5vuot65jgcmn0o8kvkll1gg@4ax.com>,
John Larkin <jjSNIPlarkin@highTHISlandPLEASEtechnology.XXX> wrote:
[...]

Probably calling out 20+20+20 with a few mils tolerance on the
dielectrics is safe for multisourcing. Lots of board houses will tweak
your art to a target impedance, but I don't like board houses messing
with my dimensions.

I you keep all the controlled impedances on one side, they do tend to
track each other.

I'm just finishing up a board right now. 2 layers, 0.062 FR-4, 0.72
square inches total. It's a tiny 50 MHz oscillator. The reference
designators are 50 mils high, which means most nobody can screen them
legibly, so I guess I'll skip the silkscreen step. Last week we did a
board that must be about 0.1 square inch.

How about, making your Screen do this:


Mark 100/N ticks along the edges of the PCB. Mark the values from 0 to
100 on the ticks. You then can make your schematic match the PCB using 4
digit reference designators.
--
--
kensmith@rahul.net forging knowledge

 

[John Larkin]

On Mon, 07 Mar 2005 06:39:08 GMT, Mac <foo@bar.net> wrote:

On Sun, 06 Mar 2005 20:54:09 -0800, John Larkin wrote:

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany
speffSNIP@interlogDOTyou.knowwhat> wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.



FR-4 has Er around 4.6, and 1 oz copper is 1.4 mils, so I use those

When I worked at a large company making SBC's, we used 4.2 for the
FR4 dielectric. It doesn't make a huge difference, but where did you get
4.6?

That seems to work most of the time. Appcad also uses 4.6, so that's
convenient. We commonly make TDR measurement of trace impedances, to
pretty good accuracy, and 4.6 seems about right.

Oh, I can TDR boards for anybody who's curious about actual
impedances.

numbers and impedances seem to come out close. It seems to me that the
cheapie multilayer houses (in the back of EE Times and such) often
prefer 12 mil dielectrics on the outer layers, about 30 for the inner,
which is sort of silly but will give you 75 ohms microstrip with an 8
mil trace. Could get lossy with such skinny traces.


I think choosing a dielectric thickness for 75 Ohms and 8 mils trace
widths is reasonable. We did 5 mil traces standard and 4 mil quite often,
especially for video, since it needs 75 Ohms. (Most of the traces were at
a slightly lower impedance, and therefore wider) I never measured the
loss, but the video seemed to work fine.

A reasonable-length (couple of inches maybe) 50 or 75 ohm trace on FR4
will be pretty much lossless up to hundreds of MHz, so most people
don't have to worry about this much.

John

 

[Mac]

On Mon, 07 Mar 2005 08:23:59 -0800, John Larkin wrote:

On Mon, 07 Mar 2005 06:39:08 GMT, Mac <foo@bar.net> wrote:

On Sun, 06 Mar 2005 20:54:09 -0800, John Larkin wrote:

[snip]
FR-4 has Er around 4.6, and 1 oz copper is 1.4 mils, so I use those

When I worked at a large company making SBC's, we used 4.2 for the FR4
dielectric. It doesn't make a huge difference, but where did you get
4.6?


That seems to work most of the time. Appcad also uses 4.6, so that's
convenient. We commonly make TDR measurement of trace impedances, to
pretty good accuracy, and 4.6 seems about right.

[snip]
We did 5 mil traces standard and 4 mil quite often, especially for
video, since it needs 75 Ohms. (Most of the traces
were at a slightly lower impedance, and therefore wider) I never
measured the loss, but the video seemed to work fine.

A reasonable-length (couple of inches maybe) 50 or 75 ohm trace on FR4
will be pretty much lossless up to hundreds of MHz, so most people don't
have to worry about this much.

John

Thanks! Maybe I'll use 4.6 from now on. ;-)

--Mac

 

[Greg Neff]

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany
<speffSNIP@interlogDOTyou.knowwhat> wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.


Best regards,
Spehro Pefhany

Press your PCB manufacturer for more detailed information. 'FR4' is a
generic designation these days. Ask them for the manufacturer and
part number of the material, and the standard core thicknesses. For
example, our 'FR4' is really Nelco N4000-2.

For information on some available materials see:

http://www.parknelco.com/


================================

Greg Neff
VP Engineering
*Microsym* Computers Inc.
greg@guesswhichwordgoeshere.com

 

[Spehro Pefhany]

On Sun, 06 Mar 2005 20:54:09 -0800, the renowned John Larkin
<jjSNIPlarkin@highTHISlandPLEASEtechnology.XXX> wrote:

On Sun, 06 Mar 2005 22:48:33 -0500, Spehro Pefhany
speffSNIP@interlogDOTyou.knowwhat> wrote:

Trying to finish up some FR4 microstrip boards, the PCB maker tells me
that they can make them with various thicknesses and to ask for what I
want, but the trace widths in the gerbers depend on my assumptions for
the Er, dielectric thickness (and copper thickness).

What *should* I be asking for to get maximum flexibility in sourcing?
Looking for 75 ohms with signal/gnd/pwr/signal layers.



FR-4 has Er around 4.6, and 1 oz copper is 1.4 mils, so I use those
numbers and impedances seem to come out close. It seems to me that the
cheapie multilayer houses (in the back of EE Times and such) often
prefer 12 mil dielectrics on the outer layers, about 30 for the inner,
which is sort of silly but will give you 75 ohms microstrip with an 8
mil trace. Could get lossy with such skinny traces.

That's about what I got from googling for information 12 mils with Er
4.6 (though some suggest 4.2), from which I get about a 9.1-9.2 mil
trace width).

Probably calling out 20+20+20 with a few mils tolerance on the
dielectrics is safe for multisourcing.

Which yields about a 16 mil trace width. Quite a difference. 8-(

Lots of board houses will tweak
your art to a target impedance, but I don't like board houses messing
with my dimensions.

Yes.

I'm just finishing up a board right now. 2 layers, 0.062 FR-4, 0.72
square inches total. It's a tiny 50 MHz oscillator. The reference
designators are 50 mils high, which means most nobody can screen them
legibly, so I guess I'll skip the silkscreen step.

With 10 mil line widths it should be legible at 0.05" high, even
though it's a bit less than is usually recommended. They should only
care about the line width.

Last week we did a board that must be about 0.1 square inch.

John

I was just looking at a design that uses three or four boards like
that in a tiny awful box assembly to fit mechanically in a very tight
electro-mechanical assembly. The PCB house will supply them in panels,
with internal routed slots and with V-groove, so they are pretty easy
to handle until they are depanelized.

Thanks for the suggestions!


Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
speff@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com