Do’s and don’ts in schematic symbol creation

Article By : Paul Rako

It's important for other engineers to be able to read your schematic at a glance.

Drawing schematic symbols should be understandable, first and foremost. Make sure you have a package that makes symbol creation easy, since you will have to re-draw every single part, as well as create the new parts you use. The tens of thousands of included symbols your CAD package brags about are simply a starting point for you to redraw them all.

Good schematics have a predictable flow. This flow requires inputs to be on the left and top, while outputs are on the right and bottom. This is not cast in concrete, but it's pretty important if you want other engineers to be able to read your schematic at a glance. I can scream at you, “Make it does difference what<img alt="?” That syntactic, it kind of parses, but if I flow from left to right, “What difference does it make?” then you can understand it in a moment. With semiconductor companies making so much money, and providing so much support, sometimes their tendency to be stuck inside the part makes the schematic flow disappear. To this day, some companies draw their schematic symbol to mimic the pin-out of the part rather than the signal flow (Figure 1).

[EDN schematic fig1 (cr)]
Figure 1: Schematic symbols imitate the pin-out of the part rather than the signal flow.

The hex inverter U1 is not very useful. It combines six parts into one symbol. There are both inputs and outputs on both left and right. The pins are longer than they need to be. The symbol for U2 is a little better. Here, the inputs are on the left and outputs are on the right. Old guys like me don’t like coloured backgrounds since six generations of a black-and-white copy turn the yellow into black and you can’t read anything. I created U3 as a heterogeneous part. It has the six parts, as well as a 7th part that shows power and ground. Resistor pack RP1 is stupid, you don’t want to tangle up your schematic when the resistors should be at various places on the sheet. RP2 shows how a heterogeneous part can do this.

Some semiconductor companies adopted that ANSI symbol for logic, obviously invented by linear minds that need to parse, as opposed the graphical minds of analog engineers (Figure 2).

[EDN schematic fig2 (cr)]
Figure 2: The ANSI/IEEE logic symbol convention is disliked by many engineers and worse than useless. Showing the exact logic symbol is better than useless. What is useless is the way the part comes in your CAD package. Better is when you break the part into its two halves. Better yet is putting the power separate so you don’t clutter the signal flow. What an analog guy wants is a little drawing inside the part that shows what the heck it does.

For multi-part packages, like many logic gates, the schematic symbols need to be broken apart, since you rarely use them all in one place in your schematic. The same applies to dual or quad op amps. The part symbol could have a DeMorgan equivalent view (Figure 3). I respect engineers than can look at Boolean expressions and understand how a circuit works, but I have always preferred a graphical representation, where I can imagine the bits sitting inside a D-latch, or the pin a multiplexor asserting with a given input.

[EDN schematic fig3 (cr)]
Figure 3: OrCAD 9 would allow the DeMorgan equivalent view of a NAND gate back in 1995. Altium/CircuitStudio lets you assign different “modes” to a part to do the same thing. This can be handy if you want to make an op-amp symbol with a mode that has the minus pin above the plus pin. With no equivalent symbol, if you flip the part vertically, it also puts plus power on the bottom and ground on the top. By invoking the DeMorgan equivalent you drew, you can swap input pins while keeping power and ground where they should be. Another way to solve this is to make a heterogeneous part with separate power (U6). Now you can vertically flip the amp to put the minus pin on the top.

Schematic programs of a certain age came about in a period when a PCB was about 40 14-pin logic ICs, a decoupling capacitor for each, and an edge-card connector. In 1985, DOS OrCAD could not even draw a triangle. That was their milleu; that was what they needed to worry about. Many of these companies felt there is only one power on a PCB and that was VCC (the two “Cs” standing for “common collector” since all those logic gates feed power to collectors of many transistors). So, you had VCC and ground. The programmers at the CAD companies thought there was no need to even show the power pins on the ICs. They just invented “zero length” pins, and then the layout program would connect all the pins with the same name. Programmers think engineers are silly for using a schematic when it all comes down to a netlist.

Speaking of ground, “common” or “return” is more accurate, unless your circuit connects to the earth ground pin of your wall socket (Figure 4). I admit it is only a personal preference, but I like American-style power and resistor symbols, circles around transistors and MOSFETs with a clear indication of N- or P-channel type.

[EDN schematic fig4 (cr)]
Figure 4: Circuit connection to the earth ground pin of wall socket.

I had a professor that would flunk you if you showed the earth ground symbol on a car radio schematic. The chasis of the car is a different symbol, despite Altium calling it Earth, and what you should be using for most PCBs are the triangles, meaning common or return. A personal preference is using the arrow for power, and I have never met an engineer that likes the European conventions for resistors like R1 and R2, and even the Altium symbol R3 for a pot makes no sense unless it has three pins, or the footprint shorts two pins together. I also prefer circles on transistors, short pins, the letter N or P to make clear the type of MOSFET, and the gate pins drawn to help show that, as well as the P-channel type being flipped so that source is on the top, where the more positive power goes. I give Altium/CircuitStudio credit for showing the body diode.

The problem with invisible power and ground pins in a modern design is you will always get burned when the layout package connects them wrongly. Always. It’s a huge problem since you might have the power on planes, so reworking the PCB, even for a prototype, is very difficult. For this reason, many of us draw the power pins explicitly. There are three approaches for multi-part packages like a quad op-amp (Figure 5). You can have the power pins on every part. Secondly, can only put power pins on one part and make sure to place all the spares. Third, you can make a quad op amp as a five-part heterogeneous package, with each of the four op-amps as a part, and then the power and ground pins as a separate part. The advantage to this is you can then put the power and ground part with all the decoupling capacitors. The disadvantage is you might forget to place that part and then same disaster, only you have no power to the part, instead of the wrong power. One trick is to make the power pins the first part in the package, so that shows up first when you go to place it. You should be plopping down all the parts anyway so you can bias unused parts so they don’t oscillate.

[EDN schematic fig5 (cr)]
Figure 5: Don’t use zero-length pins for power and ground. Instead, draw the power pins, on every part if you want (U1). Otherwise, you can only draw the power pins on one part of the package, but be sure to place all the parts so you remember to connect power (U2). With U3, you make a package with a separate “part” that has power and ground. That has the advantage of letting you flip the op-amps to put the minus pin either above or below the plus as the circuit dictates.

Next: Careful imprinting scheme

Leave a comment