Speccing 4-layer boards

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

Reply to
John Larkin
Loading thread data ...

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
 Click to see the full signature
Reply to
Spehro Pefhany

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

--
  Keith
Reply to
keith

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).

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

Yes.

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.

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
 Click to see the full signature
Reply to
Spehro Pefhany

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?

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

Reply to
Mac

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.

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

Reply to
John Larkin

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

Reply to
nospam

In article , John Larkin wrote: [...]

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

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
Reply to
Ken Smith

[snip]
[snip]

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

--Mac

Reply to
Mac

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:

formatting link

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

Greg Neff VP Engineering

*Microsym* Computers Inc. snipped-for-privacy@guesswhichwordgoeshere.com
Reply to
Greg Neff

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.