I thought I would lay this page out as an FAQ. Then as you ask questions, I can just add the answers here for everyone's benefit. You can of course make your own contributions.
Schematic Design FAQ
Q. How should I lay out my schematic?
A. Usually custom is positive at top, negative (or ground) at bottom.
Signal flow from left to right. So Inputs at left, outputs to the right.
Q. In Protel schematic, are we meant to _physically_ draw a
resistor as a box and then label it as a resistor?
A. No. Only thing you should every draw with wires are wires. Even a box should be drawn using a specific "draw a box" command. I'll call them wires rather than lines, because they have special significance to Protel. It expects wires to join components together to form a net (a node), and will try to do so.
A resistor or capacitor has two "pins", labelled 1 and 2 usually.
That is two ends, on two different nets. The resistor also has other
properties such as an associated footprint which is used by the PCB editor,
and a resistance, which is used to create a BOM (bill of materials) and
prehaps a pspice file.
Q. I can't seem to find any component libraries for basic items like resistors, capacitors and transistors.
A. The standard library is called "device" I think, and the components are within the library. The components you want are RES1 or RES2, CAP and ELECTRO. Used the browse command (button).
Q. When we are designing circuits in Protel, do we have to try an
make it as small as possible while drawing? Or is this something
we have to do after we have made a netlist?
A. When you are drawing a schematic, it doesn't matter what size or shape it is. Not to Protel anyway. Protel is only interested in the logical connections between different components, that is, the netlist. This will be the same regardless of how your circuit is drawn, so long as your circuit is indeed the same. For the benefit of the human reader of your schematics, it makes sense to make them neat, structured, logical, and resonable compact without crowding them.
Now, when you are laying out a PCB, this is no longer true. Although the same circuit may work regardless of how it is layed out, layout can have a large impact on performance. Poor layout can introduce large parasitic L, R, and C. You're circuit may oscillate, even though it is meant to be an amplifier! Also a small layout is preferable to a large one because it is cheaper -- less PCB area and smaller box etc. I'll deal with good PCB layout later.
PCB Design FAQ
Q. DIL? SIL? DIP?
A. Dual In Line. Single In Line. Dual In-line Package.
Q. What is a "Thou"? Is a "Thou" the same as a "mil"?
A. A "Thou" is one thousandth of an Inch, 0.001". A "mil" is the same quantity, a milli-inch. I prefer the term thou because it is less likely to be confused with millimetres.
Since there are 25.4mm to the inch, 1mm = 39thou. All components originally used imperial measurements, so the thou is a good unit to work with. For example the pins on a normal DIL package are 100thou apart.
If you haven't seen it used before, a single quote ' is an abbreviation
for feet, and a double quote " stands for inches. So I could write
my height as 5'10".
If you are working in metric, just use millimetres for everything. eg, I am about 1800mm high. DON'T use cm!
Q. What size grid should I use? How close can my tracks
A. Short answer - 12 thou tracks on a 25 thou grid, alternatively 10 thou tracks on a 10 thou grid.
Long answer. Well the old capabilities of most PCB manufacturers (last century!) was 12 thou tracks with 12 thou clearanaces (gap between tracks). These are called 12/12 design rules. If you use 12 thou tracks on a 25 thou grid then you have a guaranteed 13thou gap between adjacent tracks. You can run one track between the pads of a DIP and meet the clearance rule if you use 62 thou diameter pads, or at least 62 thou wide anyway.
Almost everyone can manufacture to 10/10 rules these days. Some can do 8/8, even 6/6, but you will start to pay for the priveledge. Stick to 12/12 rules unless you have a reason not to.
With 10/10 rules you can run two 10thou tracks between 50thou wide DIP pads on a 5thou grid. 10/10 rules are pretty much a necessity if you want to do a SMD layout.
Q. What clearances and trackwidths should I use?
A. Well there are some tables to guide you dependant on what voltages and currents will be on those tracks. But as a guide, on a standard (1 Oz. Cu) PCB, a 0.010" track will carry 0.8A with a 10 degree C rise. Plenty for you. But remember to use thicker tracks anyway for power supply traces etc, just in case you short them.
Q. Which way should I run my tracks on a double sided board?
A. Usually tracks on the solder-side are run horizontally, and vertically on the component side.
Q. What drill sizes should I use?
A. Usually only a couple of drill sizes are needed. A guide to drill sizes can be found on the useful tables page. Try to limit the number of drills you use to eight, this avoids extra hassles for the PCB production line people.
Q. How do I get footprints for resistors, capacitors and diodes?
A. In schematic, double click on the component so that you are editing its attributes. Here you can change its designator (eg R4), part type (eg 100k) and footprint (eg axial0.4). These attributes are exported along with the netlist, so that PCB knows what footprints to use, and what labels to attach to them.
The footprints you will commonly need are
0.25W resistors axial0.4 (Axial explains the way the leads leave the body of the component)
small signal or 1A diodes diode0.4 (The 0.4 is 0.4", the spacing of the holes)
capacitors rad0.1 or rad0.2 (Rad stands for radial - the way the leads exit the body - radially)
electros rb.2/4 (Radial Bipolar, 0.2" lead spacing, 0.4" case diameter)
ICs dip8, dip14
All the most common footprints are in a library called advpcb.lib. You can add this to the list of searched libraries by using add/remove libraries command.
If you don't import a netlist, you can still place footprints of your choosing by simply placing a part. You choose a footprint from the library.
Q. What do you mean by this: Minimum via size 40 thou outer,
25 thou inner.
A. A via is a plated through hole (PTH), placed on the PCB purely to connect two tracks on different layers. For you, this is the top and bottom layers, component side and solder side. Since there is no component leg going through the hole, just the copper plating, we could make the hole any size we wanted. But we keep it above a minimum hole size, so that the drill isn't to tiny, fragile, expensive etc. It also allows them to drill a stack of PCBs at once (say upto about 5 deep). For BEC, this is 25 thou (0.6mm). Then you need a certain thickness of copper pad around the hole, to ensure they can cope with a small misalignment, amonst other things. The ring doesn't have to be big, since we aren't soldering to it. The 40 thou (1mm) is the diameter of the via "pad". This only allows 8 thou (0.2mm) of copper ring, which is pushing the 10/10 rules a bit, when you look at it. I'd be working with 45thou dia, with a 25 thou hole.
If you are doing a single sided layout, then you don't even need to know what a via is.
BEC Manufacturing does a lot of the departments PCB manufacturing work. If you know you will be using their service, then read and conform to their technical capabilities and design tips.
If you would like to understand better how PCBs are made, then read the manufacturing page on BEC's website. The Green CirKit Reference Stack® is a comprehensive source of information on PCB prototyping, drilling, electroplating, etching, and laminating.
School of ITEE / Geoff Walker / firstname.lastname@example.org