Pins in real position or grouped by function in schematic symbol?

[ElektroQuark]

Designing a schematic symbol of a microcontroller with many pins.
How to draw pins? Like real IC or grouped by function, port, etc?
Or doesn't matter at all?

[free_electron]

in such an order that your schematic has the least amount of crossing possible

[tautech]

I like to do a symbol with an in/out flow. That is inputs grouped, outputs grouped.
Often in comes down to what will make you schematic look nice and easy to connect.

[8086]

in such an order that your schematic has the least amount of crossing possible

This is how I go about it usually. Group by function and keep functional groups logical and separate.

[T3sl4co1l]

I usually do MCUs by pinout, but bigger devices (large MCUs, CPLDs, and most any FPGAs) are not only better to draw symbolically, but the larger ones are impossible to draw by pinout on a single page.

Small functions (e.g., regulators, op-amps, controllers, etc.) I usually draw symbolically, while MSI functions (bus latches, decoders, etc.) I draw about as often symbolically as physically (by pinout).  Multipart components (op-amps, logic gates, etc.) always by symbolic parts.

Tim

[c4757p]

in such an order that your schematic has the least amount of crossing possible

This.


It's a schematic, not a PCB layout.

[tszaboo]

in such an order that your schematic has the least amount of crossing possible

This.


It's a schematic, not a PCB layout.

I think it really depends on the MCU. If you are using a nice (say) 48 pin cortex M3 the pins are usually nicely grouped anyway, and you can go with the order. If you are using ie an old infineon, where they used the roulette table and dices to decide the order of the pins, you are better off using multiple symbols and order the pins, since the manufacturer was unable to do so.

[ElektroQuark]

in such an order that your schematic has the least amount of crossing possible

So you have to modify the schematic symbol for each project.

[AndyC_772]

On larger devices, I tend to group them together by function. With smaller devices I might start out with the pins arranged as per the physical pinout, but I'll happily move them around if it's likely to make the resulting schematic easier to read.

With few exceptions, power and ground pins get separated out into another symbol. This keeps them well out of the way and keeps the signal flow uncluttered. They're *always* made visible and *always* explicitly connected to the correct power rail.

Many years ago I was working as a design engineer for a major networking company. They had a parts library which was centrally managed, and it was the job of a small team of component librarians to actually draw up symbols for any new parts the engineers wanted to use.

We had to submit the component's data sheet, get commercial approval to use the part (please allow several weeks), then wait for the symbol to be drawn up for us. Only then could it go on the schematic.

They had a rule for symbols: inputs go on the left, and outputs on the right. Just like we were taught at school, when the most complex device has about four pins.

So, you want to use a device with a crystal oscillator in it? Fine, XI is on the left, and XO on the right. Hmm, yes, that's clear and uncluttered.

An FPGA? No problem. The JTAG input pins are on the left, TDO is on the right, and all the bidirectional I/O pins are top or bottom. 

[nctnico]

Designing a schematic symbol of a microcontroller with many pins.
How to draw pins? Like real IC or grouped by function, port, etc?
Or doesn't matter at all?

I prefer to have the pins as they are on the physical device if the pins are accessible for probing. If the schematic symbol is the same as the physical package it is much easier to find the right pin to probe. Ground and power traces are usually easy to recognise so probing a pin 4 pins from 'that' power pin is easier than having to count from the beginning or end of a side of a chip.

[gxti]

in such an order that your schematic has the least amount of crossing possible

This.


It's a schematic, not a PCB layout.

Wouldn't that be an argument in favor of making it a physical mapping? If your schematic wires don't cross then neither would the physical wires, after all. This is why I've switched to keeping the pins on MCUs in physical order other than power pins, because it's easy to see at a glance where I can connect something without needing to jump over 6 wires.

As for everything else, I'll stick to the physical pin order if it's convenient, otherwise move things around.

[T3sl4co1l]

A schematic with PCB mapping would also allow wires to cross over components, and have multiple layers.

I've seen it before 

[Niklas]

It depends on the type of device and your preferences about how to draw a schematic. Put everything on a single sheet and draw all the wires or split it up into several sheets and use net name tags.

Usually I tend to make voltage regulators and switching regulators with inputs to the left, outputs to the right and GND down. That kind of device is usually connected with wires but for more complex devices, like microcontrollers, I use flags with net names. Microcontrollers will get their ports and functions (supply, oscillators etc) grouped by function on the left or right side. Power supply on top or bottom.

[David_AVD]

I almost never leave the pins in their "real" positions, especially for micros.

[HackedFridgeMagnet]

Obviously talking about MCUs here.
I was grouping by function until recently and now I have changed approaches and am now using physical mapping.
Assuming a flexible MCU, one where I can assign pins to lots of things, when assigning gpios into functional groups I can choose nearby pins, and when it comes to laying out the board as gxti said if you can minimise crossover on the schematic then you can do it on the pcb.