CAD Schematic pin arrangement approach

Question

I was looking for related questions here, and the closest one I could find was this one: Industry Practices for Schematic Design?

However, it does not address my specific question, so here goes: I am not an EE and am just trying to learn Eagle so I can break my reliance on ExpressPCB, which I have found to be okay for simple projects, but being stuck with their proprietary format, tool, and fab no longer appeals to me.

In my past, limited experience with making schematics, I lay out the pins in numerical order, which is typically pin 1 to (N/2) from top to bottom on the left, then pin (N/2+1) to N from bottom to top on the right.

While that's fine and all, I'm now laying out a board for the MCP73123 to test a LiFePO4 charger (because of my other post here) and noticed that in Microchip's datasheet, they lay out their schematic like this:

Personally, I would think this is the way to do it, since CAD/CAE tools know what the correct pin assignments are anyway, and this looks a heck of a lot cleaner in the schematic since related pins are within close proximity of each other.

So my question is simply, do you experienced PCB designers typically do this, or do you go with the numerical-order approach? What do you consider to be the pros / cons of each approach. Also, is there another methodology?

Answer 1

This is a no-brainer, use the functional layout approach. There are a lot of bad schematics out there, including professional ones, so you will see pin order schematic layout sometimes. However, it is a bad idea.

Pin-order symbols is mostly laziness on the part of someone defining the part in the CAD system. Slapping everything down in the pin order is easier than digging out the full names and functions of each pin. Of course this isn't usually the stated reason. The most common excuse is that it aids in debugging. However, a little thought reveals that is not so.

When you are debugging a new board, you have both the board and schematic in front of you. Think about the usual work flow. Which is more common: "I want to look at the clock line, which pin is that?", or "I want to look at pin 5, which function is that?"?. Clearly the answer is the former, by a lot. Yes, occasionally early in the debugging process you may want to go around a IC and look at the signal on every pin, but that is usually once, if at all. There are cases where pin-order helps, like for some repair work, but for every one of those there are multiple cases when function order is better. Functional pin depiction is actually better for debugging than pin-order depiction. Don't get taken in by the excuses for not spending time on the symbol definition once.

Then there is the other considerable issue of schematic clarity. Here there is no contest at all. Pin order obfuscates the circuit and either forces a lot of air wires or forces other blocks to be put in inconvenient places.

For more on good schematic practises, see my more lengthy writeup on the subject.

Answer 2

Olin and I have "agreed to disagree" on this topic. While I wholeheartedly endorse his approach for fixed-function ICs where each pin has a well-defined function and direction, I don't think it makes sense to try to enforce this approach for general-purpose chips such as microcontrollers and FPGAs, where pretty much every pin can be defined as an input or an output depending on the specific application.

Since I don't want to create a unique schematic symbol for the part for each application, the pins need to be organized in some arbitrary order on the symbol. It makes sense to group the pins for each "port" or "bank" together, and since they're usually grouped that way on the physical device anyway, I argue that using the physical pin order on the schematic makes more sense than any other arbitrary order.

For one thing, it helps you do some pre-planning with regard to the layout while you're doing the functional pin assignments, since the grouping of components and connections on the schematic corresponds more closely to the physical layout, at least in a general sense.

And it really does help with debugging (probing) the physical prototype. With high pin count devices, it really helps you keep your bearings if you can see the same pattern of, say, power and ground connections on both the schematic and the layout near the pin you're trying to probe. I don't know about you, but I tend to lose count when trying to find a particular pin on one side of an 84-pin fine-pitch QFP.

However, these comments do not apply to really high pin count devices in BGAs. For one thing, you're not generally trying to probe them directly, and for another thing, the schematic symbol is probably broken up into multiple sections. For these devices, purely functional grouping on the symbol makes sense again.

Answer 3

The schematic exists to:

• Help you design the circuit
• Help you debug the circuit
• Help other people understand the circuit

You should do whatever you need to do to satisfy those requirements. Personally, I have laid out chips every kind of way depending on my needs for that particular circuit.

I have laid out the pins for microcontrollers in pin order, matching the real device. (And FakeName now probably thinks that's how I always lay out my symbols). I sometimes arrange create a different schematic symbol for a device for every application, because that's what makes my job easier in those cases. I sometimes arrange small devices in pin order, sometimes in function order.

If you're going to lay out a microcontroller in function order, when what function order?

This is the same PIC32 drawn different ways. The first in some generic function order, the second in an order for a specific circuit. As you can see, the left hand symbol is about as useless as a pin order symbol. So if you choose the function order route, be prepared to draw a different symbol for each circuit.

I almost always draw connectors to match the arrangement of connections on the actual connector. This really helps stop me wiring up the connector backwards (which I seem to do a lot). I even try to draw in details of the connector, so that when I'm debugging, I can easily correlate the connector on the board with the symbol.

Whatever you do, do it because you find it helpful. Do it whatever way helps prevent you making mistakes. And whatever way helps you to debug the board. Don't listen to anyone else tell you there's only one way to do it. Don't be ashamed to do it your way.

Whatever way you choose, it may never fully satisfy you. I find that some parts are best drawn in function order for the design of the circuit, but when it comes to debugging, I wish I had another version of the symbol in pin order, and I end up opening up the datasheet, searching for the pin information, and reading through the large number of functions for that pin, trying to remember which one I used. Or I have to look right around the symbol several times trying to find pin 139.

If the schematic must be read by other people too, you should take bear them in mind when you choose your method.