PCB

You're a little off on step 3... from a netlist, a PCB layout program will pull a bunch of footprints from a library that came with the package or that you've drawn and place them arbitrarily. Typically, then, you position them the way you want them, and draw (route) the connecting traces between the pins indicated by the layout program via the netlist. There are PCB tools that contain both auto-placers and auto-routers, although given how quickly you can drag the component footprints around yourself, auto-placers aren't used that much and tend to not be very good. Auto-routers are used commonly, although setting them up correctly can be somewhat time consuming for complex boards. For something like a digital board with reasonably slow edge rates, however, an auto-router can do in 5 minutes what might require many hours of manual routing. (In many cases a good layout person can do a better job than an auto-router, but often auto-routers are good enough -- or can be made good enough with, say, half an hour of tweaking the results manually -- and it's more important to get a board built quickly than make it look nice, minimize the number of vias, etc.)

Finally, note that you can skip steps 1 and 2 if you desire -- PCB packages will let you drop component footprints onto a board and start wiring them up, so if you have no need for a formal schematic, you can potentially save time on some designs by not bothering to enter one. Some PCB packages (e.g., Pulsonix) seem designed to encourage this approach, whereas some others (e.g., PADs) seem designed to discourage it, but they'll all bend to your will given enough bludgeoning.

Thank you very much ! What is "Footprints"?

So far, so good. You'd run design rule checks before generating the netlist. You will likely have to create new schematic entities for parts not in the libraries.

No, there is quite a bit of manual work to get from the netlist to the final layout. You'd want to set constraints on spacing and trace width for an autorouter. You may wish to route manually, in which case the program will typically keep you from creating a layout that does not match the netlist and some of the constraints. You will have to do much of the placement of parts manually. You will have to create the board outline manually. Some of the processes can be iterative (you may find that the parts won't fit on the outline you hoped to use, or you may find that routing is impossible with the placement you have, or you may have to add layers to the board). Footprints can be associated with each component at the schematic stage or at this stage. Generally you'll have to create new footprints for parts that are not in the library.

When you're done the 'layout', you run Design Rule Checks to ensure that the desired rules are not being violated. Then you generally generate Gerber and Excellon files, which the PCB manufacturer can use to generate film and 'drill tapes' (a file of instructions for the drilling machines). Some PCB makers work with the design files directly, which eliminates a step, but it's not a very important step, and would usually be limited to one or two 'softwares'.

Best regards, Spehro Pefhany

"Hi, guys, I am a layman, I want to know the basic process of PCB. I was told that the process is:

1. draw out the schematic of the circuit in the software: Orcad, PADS DxDesigner, or something else.
2. generate the netlist of the schematic
3. the software will generate the PCB layout automatically according to the netlist file
4. the PCB manufacturer will make the PCB according to the layout.

right? Thanks. "

Nope. Between 2 and 3, insert a few steps. No known software will just take a netlist and give you a layout.

You must have all schematic symbols in a "known good" condition, then you have to have all PCB footprints in a "known good" condition. The netlist merely connects the physical parts according to the logical information in the schematic.

Then you have to design the outline of the PCB, what size and shape it has, if there are mounting holes, if they are plated or not, if there are "keep out" areas where you have special conditions apply (like restricted height, etc..). You also need to keep track of any electrical parameters like differential pairs, high voltages, min or max trace lengths, etc...

Then you need to setup the board, number of layers, type of material, thickness, via technology, etc... You also need to set up the CAD to respect minimum trace widths, solder mask clearances, etc.

Big CAD packages let you define all these parameters at the schematic level or the PCB level.

Then you place the parts. Autoplace in CAD software usually refers to the software's ability to place parts in pre-determined areas as opposed to a big pile of parts centered at 0,0. Again, you do all the work.

Even after all this you need to then connect all the netlist in however many layers of PCB you have deemed necessary for the job. By hand. CAD software can sometimes try to guess how to terminate a particular bunch of traces but again, you have to do this and it all depends on the setup. Most of the time it makes unusable traces.

There are autorouters but you can't just click "go" and have it guess everything. You still need to set it up, and they are usually un-intuitive and have a steep, expensive learning curve.

Then ideally, you can have your artwork checked against the PCB manufacturer's design rules, they usually will check things like drill sizes and trace widths.

Of course, you didn't say what you want to do. If it's an 8 pin PIC with a few resistors, you still go through the same steps but it's not that painful. Some lightweight software like Eagle is actually pretty easy to learn, I hear.

Big designs= big headaches = big $$$ for the CAD monkeys like me.

Footprints are the copper patterns that represent a component's physical layout on the board - pins, pads, silkscreen, holes, solder mask, etc.

A footprint is a layout entity that contains all the elements required for the layout of a component. It would generally have the silk screen outline, maybe assembly information, padstacks (which might involve several layers each), and so on. This entity will be replicated for every instance of each component that is associated with that footprint.

For example, you could find one for the 0402 SMT package in the library which comes with the software. It might be okay for your use, or you might have to modify it or create your own, but you only have to do that once for each unique footprint.

Best regards, Spehro Pefhany

PADS isn't bad. You just enter ECO mode and then do whatever you like... add parts, add connections, route traces. It keeps an ECO file of whatever you do. You can use the ECO file to back annotate a schematic if you ever had one, or just delete it. But in reality we always start with a schematic to document whatever the thing is.

We rarely autoroute. If you place things carefully and assign pins intelligently, routing isn't usually hard, and we get much better and prettier boards by hand routing. PADS typically makes such a mess of autorouting that it takes more time to clean it up than it's worth, and if you don't check carefully you can wind up with critical signals making the grand tour of the board.

People can think strategically, autorouters can't.

John

My PCB Design tutorial might be of some help:

Dave :)

Small ones do, too :-)

Eagle is pretty easy to learn and for a beginner it might be the right tool. It's integrated, meaning you can go from schematic to layout and back and forth without a netlist or other hassle. What took me some time was to learn the library editor to generate parts that aren't found in the libraries (for some reason hardly any parts that I use are in there...). The OrCad library editor was easier IMHO.

I think Eagle can do up to 16 layers or so and boards the size of a small kitchen table top. If that ain't a big design I don't know what would be. Much less $$$ than others, which is what convinced me. A huge downside though, at least for me, is the absence of a hierarchical design methodology.

Since I don't do layouts I can't say much. Of course I tried it out a bit. It's quite easy and even the autorouter did a pretty neat job. However, as was already said, you cannot just hit "route", go have coffee or tea and expect a flawless and nice layout to result.

Regards, Joerg

Hello David,

Very nice!

I kind of disagree with the notion about star grounds but that's a whole other topic.

Now if you could convince some of the universities to encourage their students to read your paper we might finally get some competent engineers out of them again.

Regards, Joerg

Thanks.

I know! :->

Trying to keep it to the lowest common denominator.

You'll be pleased to know that several US universities (plus several in other countries) are now including it as either reference material or as a basis for their PCB design subjects.

One major european PCB software package has also included it in their Help system.

Dave :)

gEDA and PCB can be used to make boards up to, um, [does math], oh boy, 0.3 miles square. I don't think anyone's tried that. I just tried some big ones, it handles 333 feet square before my working copy[*] segfaults, probably due to buffer overflow trying to print those numbers. That's with 0.01 mil resolution. The official version stops at 30 inches, but that's a leftover from an old design.

As for layers, it's a compile time constant. I've tested it with up to 50-something layers. The UI gets ugly at that point, but it functions. Default is 8 layers.

Oh, and gEDA and PCB are free (cost and license). So, other packages might have more polish and glitter, but there's no reason to use cost as an excuse to avoid big designs.

[*]

Got it. 21,474,836 mils == 21,474 inches == 1789 feet per side == 1/3 mile. It crashed when I tried 40,000,000 mils, which exceeds the 2^31 range for signed 0.01 mil units. dsub-9 connectors are *really* small on the screen.

Jackie wrote:

The procedure used to be:

(1) Draw out the schematic on a collection of fag packets, old envelopes, and scraps of paper, mostly in lunch and tea breaks, or at home, because all the time at work is spent in "meetings" with customers, the boss, or discussing football or rock music. (2) Give the said collection to the drawing office. (3) A week later, check the print of the beautifully drawn ink-on-paper schematic. Find that they've drawn big round dots wherever one line crosses another. Mark the wrong ones in red felt-tip. The same for all pin numbers, where consistently 0 has been read as 8 and vice-versa. (4) Meanwhile, the boss has taken another copy, marked it "LATEST VERSION" in large green letters, and put it in a filing cabinet. (5) Return the drawing to the drawing office. Mike is off sick, so wait

3 weeks for the corrected drawing to come back. (6) Repeat 3 to 5 until you can stand it no more, and just remember what differences there are between the dreawing and the circuit you wnat. Note that the boss now has 7 different copies of the drawing, all labelled "LATEST VERSION", and all undated. They are filed in no particular order. (7) Get a big sheet of squared draughting film, and 2 big pieces of acetate sheet. Tape them together. (8) Get out the required footprints. Find that you are short of a couple of types. Order them in, and rub down the rest. (9) A week later, when the footprints arrive, lay them out too. (10) Use crepe tape to place the tracks, rubbing down pads as vias where necessary. Find that you haven't left enough room between some components, and have to rip them up, scrape off the footpints, rub down new ones in the changed location, and replace the tracks. (11) Interrupt a colleague and persuade him to stop discussing football, and help you to check the schematic against the layout. Correct errors. Forget the bits the draughtsman got wrong in (5), and 'correct' them too. (12) Send the completed layout to the PCB manufacturer. Because the photography cost is £200, the boss has demanded that you have 50 off made. (13) 6 weeks later (guaranteed 15 working days, but who's to say which days they actually work) the PCBs arrive. (14) Check with a meter. Dead short between power rails- THAT was what the draughtsman got wrong, and what you'd forgotten about in (11). Cut the offending trace with a scalpel, cutting your thumb in the process. (15) Populate the PCB with components. Power up. Observe volume and location of smoke. (16) Find that, while most databooks give the pinout looking from the top, a few critical components have the pinout looking from underneath. These of course are the most expensive and on long delivery times. (17) The prototype now has some components soldered on top and some others on the bottom. But at least it powers up. (18) Start functional testing. Find that this particular manufacturer likes to label his data bus with DB1 as the MOST significant bit. That means that, after assembling the source code (which only takes 25 minutes for the 2k test program), you have to manually reverse all the bits before you program the EPROM. Detail the office whizkid to write a program to do it automatically, and call it a security feature, before the boss finds out. (19) Go on a LONG holiday, after which you put in your notice and get another job.

Paul Burke

Hello DJ,

Pretty impressive. However, in my experience a board of that caliber leads to some problems. Solderability, warping, alignment, just to name a few.

The shareware concept is great. But timely support is also a big issue in the CAD world. Eagle isn't really a huge cost issue either. For the full version each part is under $500 and there are only three: Schematic, layout and auto-router (which many folks like me don't need).

What I really like about it is the fully integrated environment. For a beginner like the OP I believe that would be a key requirement.

Regards, Joerg

Hello David,

Great. Now they just have to require the students to do something practical with it. I have encountered numerous cases where freshly minted engineers could not even solder (!) . To me that's like a tile setter who can't mix mortar.

If it's not Cadsoft Eagle it might be worth a mention on their support forums.

Regards, Joerg

On our list, the concerns were shipping and finding a big enough card cage ;-)

gEDA and PCB aren't shareware. Unlike shareware (which, I think, is/was a trademarked term for a very specific distribution plan), gEDA and PCB are non-prorietary, and don't require payment.

Hmm... our average turnaround on critical bugs is minutes. But yeah, we don't have a large team of developers with lots of time to work on bug fixing. PCB has, er, two people working on it regularly in their spare time. I suspect anyone who was willing to pay for a fix wouldn't have trouble convincing us, though.

I wasn't trying to compare pcb and eagle; each has their strong points. Just pointing out that in the "big projects cost money" argument, there's a zero cost software option available that supports arbitrarily big projects.

NOTE: That's COPPER layers--there's still lots left for silk, soldermask, keepout, etc.

. .

What's the name of that place where you come from? Brobdingnag? Wherever is is, they must have HUGE kitchen tables there.

Ah. A variation on a theme that complements Ken Smith's gem:

and the addendum by George Gonzalez: