I am starting layout on a new project using Eagle 7.5 So far, we have only used 2 layers and this will be the first 4 layer board. I had in mind to use one of the internal layers as ground and the other for power routing with signal planes on surface layers. No BGAs but lots of fine pitch (mostly leaded) SMTs. No buried vias, vias through all layers.
Any pointers would be appreciated - TIA
On Fri, 1 Apr 2016 10:54:37 -0400, "Oppie" Gave us:
If it is all populated on the top side, you could move the ground plane to the bottom and it will act as an electrostatic containment shield for the circuit (to a degree). But then you would have vias that traverse all layers.
Our usual stackup would be
1 parts and traces 2 ground plane 3 power pours, maybe some traces 4 traces, bottom parts if really neededWe use PADS for layout. It allows official plane layers, but we don't use them; we just make copper pours on regular routing layers. That's a lot more flexible. If we want to do goofy cutouts, or mix power pours with some traces, it's easier.
-- John Larkin Highland Technology, Inc lunatic fringe electronics
Ditto, this is pretty much standard practice.
For copper weight: We either use:
1oz 1oz 1oz 1ozor
1oz 2oz 2oz 1ozCheers
Thanks, I'm making progress in setting up a configuration script. Like most engineering, so many ways to go horribly wrong. Trying to think out as much as possible in advance.
What designations do you use for your Gerber layers?
For our 2-layer designs, we use a different file extension for each of the layers. Most of these came, recommended by CadSoft: .cmp top component traces .sol bottom side traces (cary-over from through hole) .plc silkscreen top .pls silkscreen bottom .stc stop mask top .sts stop mask bottom .pho solder paste top .crs solder paste bottom .bdl board dimensions .tdoc document top .inspect incoming inspection print .drd drill data (excellon)
For the two new layers, will probably use .ly2 and .ly3 unless there is a better recommendation.
planes seem to be a silly left over from when doing a reverse of the pads saved a bit of work
-Lasse
It's probably wronger than wrong but the few 4-layer boards I've done have been ground pours on top & bottom, with all the signal traces in the middle. Cuts & jumps become a pain, but since I'm usually trying to pack things in tightly, the room for traces makes up for it.
-- Tim Wescott Wescott Design Services http://www.wescottdesign.com
if it works it isn't "wrong", but I'd call it odd :) with SMD everything but ground would need a via taking up lots of space
if you put ground and power inside only those need vias and everything else can be routed with very few vias
-Lasse
You can use those or anything else, just include the descriptions in a readme.txt file so the board house has a reference.
Cheers
Here's a 4-layer board.
-- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
Found a bunch of things better explained in the help file than in the user manual... This is Eagle 7.5 and in the Eagledata\doc\ folder, is the user manual in pdf form. In Eagledata\doc\Help Files\ is the help file in .docx form. I got so accustomed to help files in chm format that were difficult to view in total, that I had overlooked this. Opened it in Word and exported to a PDF to mark up.
Getting there... Thanks for all comments and have a good weekend - Oppie
Why? In an effort to get some shielding?
On an early instrument, (front panel with pcb 1/2 inch behind it.) I made the back of the pcb ground and had the components facing the front panel.. With an idea towards shielding. Didn't do much and made it a PITA to service.
George H.
With surface-mount parts, you can do a lot of the routing on layer 1 without vias, which really helps density, especially for analog circuits.
L2 ground can be a solid ground plane, whereas L1 can't... the parts and pads get in the way. The L2 ground is a nice close low-inductance common ground, and is a good heat spreader, with the minimum thickness of FR4 between parts and ground.
We do a lot of 6 and 8 layers lately. BGAs need a lot of layers to get the traces out. I tried to do my high-voltage board in 4, but couldn't make it work. Inner-layer traces need much smaller voltage clearances.
I have a friend who is doing a board with 0.3 mm ball pitch and 2 mil traces. He's looking for somebody to assemble it.
-- John Larkin Highland Technology, Inc picosecond timing precision measurement jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
It's odd - and makes the circuit difficult to probe - but there's one strong argument for power planes on top and bottom of a four layer board and it's that microstrip transmission lines are dispersive and (buried) striplines aren't.
You've got to be shipping GHz signals around for it to matter ...
-- Bill Sloman, sydney
That's nice, thanks. I do mostly 2 layers, I do the signal first, and it's always a pain routing power around.
George H.
Huh, How can that be? It's the fiber glass that causes the dispersion, No? I can believe the buried stripline shows less dispersion... It's more symmetric.
George H.
ve
ther
lots
l
the
pack
trong argument for power planes on top and bottom of a four layer board and it's that microstrip transmission lines are dispersive and (buried) stripl ines aren't.
You don't have to use FR4 epoxy-resin bonded glass fibre for your substrate . Rogers do a bunch of less-dispersive materials, and if you were worried a bout dispersion, you'd use them. I've done so for stuff where we wanted sub
-nanosecond transition times, though it was probably an over-kill - the tra nsition times weren't all that sub-nanosecond.
Apparently having air as half your dielectric and even a non-dispersive sub strate as the other half makes microstrip intrinsically dispersive.
Buried microstrip can be non-dispersive, if you make it right, or so I was told, why back when I had an immediate interest.
-- Bill Sloman, sydney
They are both dispersive, but microstrip has some (most) propagation in fiberglass and some in air, which makes it slightly worse.
But for a given impedance, a microstrip trace will be wider, and only one side has dreckky "black copper" adhesion treatment, so microstrip can be better as regards losses.
-- John Larkin Highland Technology, Inc lunatic fringe electronics
Of course you can use what you like but...
I have found that following the "altium standard" is best.
Gerber viewers can associate the file extensions automatically, and so do the online/automatic checkers used by prototype PCB companies. A high-quality, high-price place will follow the readme.txt and do what you ask anyway. Budget/hobbyist/maker places will not.
Here is an unusually honest explanation of this from one such supplier:
---------------------------------------------------------------------- Readme.txt & special instructions
Get the hell out of here. We are an automated conduit to cheap local Chinese fabs. We don't read squat, and at these prices you'd be insane to think we do! Nobody at the board house even speaks English! You need a much more expensive board house if you need this level of service."
----------------------------------------------------------------------
But they can still provide *excellent* prototype boards for next to nothing prices. Just don't expect them to do much except throw your gerbers at their automated front end and post what comes out.
For example I follow something like this (but worked it out myself before seeing this page).
-- John Devereux
With fast stuff, it becomes impossible to route power and ground on a
2-layer board; you need planes and pours. We almost never use 2-layer boards in products, but we often go 2-layer for test fixtures and breakout boards.I accumulate a bunch of ideas from various people and occasionally lay out a conglomerate 4-layer proto board that we can shear up into tiles and let people play with.
-- John Larkin Highland Technology, Inc lunatic fringe electronics
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.