As we do design review we find some very common problems in schematic designs we are sent for review. Therefore we thought we would save you some money by point out these common problems.
Audience
Back in the college dark ages the public speaking class instructor told us to always know your audience. The same is true when doing a schematic design, so who is the audience for the schematic design?
When I was younger I figured the audience was the PCB layout tool, that is the schematic's only purpose was to make a PCB. I also viewed firmware as the only purpose was to meet product requirements. As I have aged and had to go back to those designs and firmware I realized that audience is the next engineer that will look at it. Which might be you in a few months/years.
For myself looking at a design, firmware or software I did 3 months ago it might as well be something that another engineer did. That is my projects change so rapidly that 3 months seems like a different life time ago.
What this means is that the work-product you produce as an engineer is more about documenting the design intent, than it is about actually making it work. For young engineers this seems crazy, that is you will spend more time documenting what and why you did something than you will actually doing it. However the reality is that 6 months from now having that documentation will save you more time and head aches than the cost to produce it.
When this is applied to schematic designs it means your design should be a work of art that another engineer could pick up and say "I know exactly what he was doing here."
Revision Control
Most people doing one off designs never think about revision control on schematic designs however it is a very common problem. I have seen people order the wrong boards, review old designs etc.
The schematic and hardware design is just as important to your product as the firmware as such you should follow the same revision control and data backup philosophy as you would on source code. We recommend that you use git or other version management system for version control. We have seen people use directories and store files locally, this works for versioning but if your hard drive crashes you could loose the designs.
We have seen people try to use dropbox for versioning. This usually ends poorly because unless you do different directories for each revision you will eventually overwrite an old revision.
People often ask when should I change revision number. Anytime you send out, email or print a design it should have a revision number. If you email a zip file this is an act of publishing the design and it needs a revision number, and new revision number if any changes happen there after. If you have any questions about this ask a software developer as their release cycles are much faster than hardware and have lived this problem enough where they have solved it, so follow the rules they have set up and learn from them.
At the end of the day git is easy to use, free, and it works and is built into most CAD packages like Altium, so why risk not using it?
Lack of Manufacture Part Numbers

Above is an example of an IC from a schematic design. If you give this schematic to someone to review they can not determine if the pin out of the part or anything else is correct as they have no idea what part the designer intended to use.
By adding the manufacture's part number the design review can determine the fit and function of the circuit.
Reference Equations
In designs we often have a voltage dividers or resistors to set various parameters. For example a voltage divider to set the output voltage of a regulator.
When we have such settings we are doing in the design it is helpful to put the equation into the schematic such that the next person understands the design intent.

In the above schematic we have a voltage divider to set output voltage but have no idea if it is correct.
Simply adding the feedback voltage is a huge help.

Adding the intended output voltage is even better.

Adding the calculation is even better.
Power Supply Currents
As we saw above adding the output voltage and equations are very helpful. On power supplies it is also good to add the output current.

Adding the current output and other parameters settings the reviewer now has much better idea of what the design intent was.
Unconnected Pins
In our power supply above pins 1,3,15 have no connection is this and error or was this the intent? By adding an 'x' (no DRC in Altium) on the pins it in forms the next engineer that it was intentionally left unconnected.

Critical Component Parameters
You will notice that all the inductors and capacitors in the above examples have the voltage and/or current limits noted for each part. For example we know that L4 at 6.4A rating should large enough to hand the 3A output of the power supply, and that the capacitors have enough voltage tolerance for the net.
This should also be done on Zeners and other symbols for example:

It is easy to see that D7 and D8 TVS didoes are 3.3V rated, also the part number is visible so next engineer can verify.

In the above schematic we know the nets are RS485 and are protected in what appears to be back to back avalanche diodes, but we have no idea if the voltage rating of the diodes are correct or even what part number they are.
Custom Schematic Symbols and Footprints
Often in a design we will use a module, for example a step stick module like this one.

So design engineers will often just put down on the schematic two 100mil pitch connectors for the module and wire up. They often view that they are in a hurry to get design out and do not want to take the time to make a custom symbol and footprint for the module. This is always short sighted and costs them money in the long run.
When you create a custom symbol and footprint you can do things like add the 3D model and label pins on schematic as to their function. So now your design review process can review the symbol and footprint and know it is good all time forward. Without doing this each schematic review and hardware design review must go back to the modules datasheet and verify every pin on the module and connector placement on the PCB. Then even things like generating the step model for the mechanical engineers becomes a large problem without the custom footprint with 3D model. In the end that quick route on the schematic design ends up costing more than doing it right the first time.
Of course the above step stick is a minor example, but imagine a processor module with 300 pins. Here if you do not create a custom symbol and footprint every design review the reviewer needs to get SOM datasheet and go through the connections pin by pin and verify it is wired up correctly. A couple of times through this process and your engineers will be happy to create custom symbols and footprints.
Be Specific on Part Numbers

This appears to be using a BSS138 transistor. The gate threshold on a BSS138 from different vendors are different. For example:



If you look at these numbers you might determine they are less than 1.5V max. However if you look closer the current that transistor conducts for 1.5V is vastly different. So if you designed transistor for 1mA and 1.8V Vgs then it may only work with the last transistor.
To be more specific assume we need 50mA through transistor, then this transistor needs at least a Vgs of 2V.


This one needs ~2.2V. Both transistors are BSS138 but only one may work in your circuit. If this is the case you should specify the part number and ideally the critical parameters for the part.
Mixed IO Voltages
If you are doing a design with mixed IO voltages then it is a good idea to indicate each net as to the IO voltage. This can be done by appending the voltage to a net name, or better in programs like Altium you can change the color of the trace/wire for that net.
This is very helpful for accidently connecting wrong IO voltages together.
Capacitors
Today most ICs are sold based on the real estate the circuit takes on a PCB. Therefore power supply chips often try to reduce the number of capacitors they require.

The above design has only two capacitors, often designers copy this reference schematic and assume the design will work. If they read further they find out that the reference design only works in specific cases and usually you need more capacitance than the reference design has, and/or very low ESR capacitors which get expensive.

Generally all switching supplies should have some bulk capacitors and smaller decoupling capacitors on input and output with low ESR, like ceramic 100nF that is often used for decoupling in designs. Adding more capacitors to the design generally does not hurt the design and lowers the noise on switching supplies. If you are cost and/or size limited then you can tweak capacitors to design tolerances after it works, but make it work first.
Off Board Connections
Off board connections are usually problems that engineer waste at least one board spin on getting correct. Here are few common problems.
Note if connectors are exposed to user then at some point the user will connect the connector the wrong way.
Reverse Polarity Protection
When power comes into a board the board really should have some sort of reverse polarity protection.

This design uses a P-FET for reverse polarity protection. It also has a fuse for current limiting. However the design does not include any voltage or current ratings for the reviewer to determine if the connector, FET, and fuse are designed with tolerances.
Current Limits
Here common ways to limit current are fuses, poly-fuses, and simple resistors.
ESD Protection
Generally if the connector is inside the box without user access you might not need ESD protection but if it is exposed to user then you need ESD protection.

The above circuit uses a ESD chip designed specifically for USB.
EMI and Noise Reduction
For EMI it is always a good idea to place a decoupling capacitor on all power pins as close to a connector as you can. This helps reduce any noise coming in from the wires.
If you have switching power supplies and worried about EMI emissions then also consider a common mode choke to limit emissions.
Note that most problems with switching power supplies and noise is either the lack of capacitors, or poor PCB layout, if you have this problem we can help.
For noise if a pin is an analog input consider putting a LC or RC filter on the pin to prevent any high frequency noise from coming into board.