New to PCB's

I have a question about 4 layer boards... If there is such a thing as a typical layout, would it consist of signals & hardware on the top layers, signals on the bottom layer, an internal power plane with all

3.3 volt connections to this plane via vias (sorry), and the other internal layera ground plane with all grounds (from the two outer layers) connected through vias?

Does this make sense, or do people normally route signals through the two internal layers.

Thanks much, Tom

Reply to
Blip
Loading thread data ...

Unless it's an RF stripline or microstrip design that's pretty much how it looks like. If it gets tight you can cram the decoupling caps on the other side. Just keep the variety of parts on that bottom side low, like only 0.1uF caps and 100k pull-ups.

Hint: If you've never done that have a professional layouter do the first round and watch him/her carefully.

--
Regards, Joerg

http://www.analogconsultants.com/
Reply to
Joerg

Thanks Joerge -- I'm a hobbyist/hacker with this stuff - don't know anywhere to go watch this; however, I'd be glad to watch some kind of video of this if anyone's aware of any out there (probably should have googled this first before I replied).

Best, Tom

Reply to
Blip

If it's absolutely positively guaranteed that the board will always be built by hand then put whatever the heck you want on the back.

Some space-sensitive boards in high-end systems don't make much distinction between the 'top' and 'bottom' layers, as long as they can cram everything they need onto the board. Fabrication costs go up sharply, though.

--
Tim Wescott
Wescott Design Services
 Click to see the full signature
Reply to
Tim Wescott

Personally, I've never had much use for power planes. Using one of the internal layers as a ground plane is a big win, but I use the other internal plane as a routing layer. Route your power with thicker tracks, be careful about your bypass capacitors and routing from the caps to the package pins, and use polygon pours to give you a mini-plane (on any suitable layer) if you need it.

If you've got a higher speed board (> 50 MHz), or particularly high current parts, you need to think more carefully - but for most boards, dedicating a whole plane to 3.3V is a waste (IMHO, of course).

Reply to
David Brown

There are times when it makes sense to put components on the bottom side also. In my case, they were an RF comms module and a GPS module. You have to be careful about putting surface mount components on the bottom side as it can complicate automated assembly. Since my boards are hand-soldered, that's not been a big problem.

Also, make your boards large enough so that you don't have to crowd things too much. 20% extra room really makes the layout go faster!.

Mark Borgerson

Reply to
Mark Borgerson

The major disadvantage of routing on internal layers is that it can be very difficult to cut traces or add jumper wires to the nets routed on the internal layer.

There is also a potential disadvantage to power and ground on internal layers: you can end up drilling out a lot of holes to find the short circuit! In my case, I forgot that the prototype quick-turn service plates ALL holes so that only one drill or mask step is required. Some mounting holes that were specified as unplated ended up shorting power and ground planes. Luckily, I had only 4 holes set up that way--- on a component I had cut and pasted from another designer's layout.

I've modified the part pad stack so that the inner layers are set back from the holes (a good practice in any case, if you plan to use metal mounting screws).

Mark Borgerson

Reply to
Mark Borgerson

These are all general points about multi-layer cards, which apply no matter what you do with the inner layers. Basically, if you expect to be doing significant amounts of trial-and-error on your pcb tracks, you should either take it into account when doing the layout (if you think a track might not be right, route it through a 0-ohm resistor to make it easy to test and "cut"), or stick to a two-sided pcb with a larger area (to make it easier to route, and easier to modify after production).

Reply to
David Brown

Another old trick is to order the first 10-20 boards in the form of two double layer boards. Put a sheet of woven glass fiber cloth (the kind used in fiberglass) between the two boards as a spacer and solder a thin wire through every via. If everything tests out, order the next batch in 4-layer. If there is a problem, you can cut and jumper another set of 2-layer boards and assemble them into another pseudo-4-layer board. Order the thinnest standard board material if you do this.

--
Guy Macon
Reply to
Guy Macon

Gentlemen -- I appreciate all of these answers & more importantly the discussion about those answers - for me, this venue, google, & a couple of good books are the fastest way for me to ramp up in a new (to me) technology. Now that I've blown the smoke... I have a few more board-related questions...

1 How is it possible to tell how many layers a board consists of? If you only hace the board in hand? This seems to me a problem...
  1. What can I expect when routing under a 256BGA? These are stoopid questions, but I don't know, not can I find the answers to them. Since I want to route on at least 1 bottom layer, do I have to put vias on every bubble-pin that will route to a lower layer?
  2. Can I route across the top layer between the pads? Can I put vias between the top layer pads?
  3. Last, is there a standard size for SMT caps & resistors? I've gone through the shapes & compared the different classes (ex 1402, 1210) at mouser & it seems that any number of footprints will work in a given situation. Do I go w/ the smallest pad? The cheapest (these are not for big runs)?

Thanks for your time.. Best, Tom

Reply to
Blip

Um, cut it open and look at a cross section under a microscope?

The more pin rows, and the closer the pins, means the smaller design rules you'll need, and the more layers you'll need to route the signals out from the bga. 256 balls means four rows, so if you can route one trace between balls/vias, that's two layers - the top layer is the first two rows, the next two rows via to the bottom. Normally, each additional row is an additional layer, since the existing vias are in the way, preventing you from bringing out two rows. If you can fit two traces between balls/vias, the rules change, etc.

Normally, the vias go between the balls, not under them - unless you're willing to pay extra for via-in-pad. Google for "dog bone bga".

If they fit.

I'd go with the smallest you're comfortable with, that work with the sizes you need (i.e. big caps don't come in small packages). In general, smaller is better for bypass caps, and often cost (to a point). 0603 seems to be the most cost-effective size these days, but

0402 is catching up.

For each standard size (like 0603 or 0402) part, there are usually a couple of land patterns of varying sizes; these have more or less extra copper around the part to ease soldering; use a larger pad for hand soldering and a smaller pad for space-critical reflow soldering, etc.

Another option which I use is to put an 0805 or 1206 land pattern down, but put 0603 parts on it. The larger land allows me to change the part if needed, like for power rail filter caps. It also allows others to use the design even if they're not comfortable with parts as small as I use.

Reply to
DJ Delorie

Gak, 256 balls is 16x16, or eight rows from the edge. That's 6 signal layers (two rows on top, two "outer via" rows, and four more for rows behind vias).

Often the innermost balls are for power/ground, which may save you some routing layers.

A 64-ball BGA is four rows from the edge.

Reply to
DJ Delorie

Shine a bright light through it.

Single layer: duh.

Two layer: With the light, you only see the traces you see on both sides.

Four layer: With the light, you see traces or a plane that are not on either side. Also, without the light you see component leads that appear to have no traces and vias that have zero or one traces.

Six or more layers: Almost certainly one of the layers is a plane, so your only way to tell it from a four layer is usually to look at the edge with a microscope. Sometimes you can tell by counting how many sides a large BGA needs to reach the vias around it; if it needs all four layers but your light shows a plane, it's six or more layers.

BTW, if it's a PC motherboard, they often brag about how many layers they use. Check ads and website.

--
Guy Macon
Reply to
Guy Macon

Often they have a stack-up-strip : Results in a simple staircase of one number per layer. That helps the PCB house get the layers in the right order, and avoids doing one twice!

Depends on your design rules. A good starting point, is the Vendors EVAL PCB. Look at what they did, and the rules they used. Often, you can import their File into your CAD package, and get a head start.

Choose the one easiest to handle! That's probably 0805 : 1206 are trailing off, and 0603 are getting too small to handle manually.

-jg

Reply to
Jim Granville

Look for Xilinx XAPP 157. Altera also has a similar document. Most of what I know about PCB layout is drawn from manufacturer app notes and reference designs.

Reply to
mng

And of course make sure they are large enough to handle the load.

Robert

--
Posted via a free Usenet account from http://www.teranews.com
Reply to
Robert Adsett

I don't know any movie about it since I can't watch YouTube stuff (yet). What helps is to disassemble things and take a look. For example an antenna pre-amplifier or mast amplifier. They are not as dense as other RF gear such as cell phones so they provide a better learning experience. Distribution amps are often soldered shut so a mast amplifier may be better because they are easier to open without destroying them.

--
Regards, Joerg

http://www.analogconsultants.com/
Reply to
Joerg

Yes, then it won't matter. However, having active parts on the back side can become a little nightmare in debugging if the whole thing is mounted in a rigid housing and you can't easily get to the bottom.

That's why I suggested limiting those to bypass caps of the same kind and such. I did that on a board end of last year and the cost increase was quite minimal. I was told that it would have been major if they had to do a full rigging for lots of different parts, basically like twice the cost.

--
Regards, Joerg

http://www.analogconsultants.com/
Reply to
Joerg

s

You'll find plenty of BGA routing info here:

formatting link

Leon

Reply to
Leon
[...]

Often you can take a strong magnifier and look at the side of the board, even if the planes aren't routed to the edges (they shouldn't). Or look into a large non-metallized mounting hole.

Careful with BGA, they need a very precise temperature profile. I avoid them altogether where possible even if some call me a Luddite. This is definitely a topic to discuss with a really seasoned layouter.

Yes and yes. But heed the clearance req's of the fab house. Old rule: The finer the pitch, the less fab houses will do it, meaning more $$.

My layouter has his own libraries for that, he is older than I am and thus knows what works. Don't simply take the ones in the CAD libraries, always vet them with either a fab house, a data sheet or, better, with an experienced layouter.

--
Regards, Joerg

http://www.analogconsultants.com/
Reply to
Joerg

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.