Naming (C1, C2, R1, R2…) components on PCB

I want to label all the components on my board C1, C2, R1, R2, IC1, IC2, etc.

I am trying to think about the best naming convention for everything. On one hand, I want to group together all the components by the IC or function that they are attached to. So in this way, I would group all the resistor and capacitors attached to IC1 together such that IC1 has C1, C2, R1, R2, R3 and then IC2 would have C2, C3, R4, R5, R6.

On the other hand, I want to group together components by value so that when building the board it will be easier to just drop in R2, R3, and R4, which are all 270 ohm but are spread across different ICs and functional modules.

Is there a standard convention on how to go about naming components on a board?

-
This has been converted to wiki as a question that has many different valid solutions but is worth discussing. –  Kortuk Jul 21 '12 at 3:57

Trying to get cute with component designators will be more trouble than it's worth. Ultimately it comes down to the basic problem that component usage is multi-dimensional and no linear naming scheme is going describe that well.

Sometimes I've seen people use 3 digit designators with the first digit identifying the schematic sheet. That's only one parameter, and doesn't help at all for finding the component on the board. It's also a hassle to maintain as you move components between sheets.

Even worse, very rarely I've seen people try to use numbering to identify which subcircuit something belongs to. For example, R1xx might be for the power supply, R2xx with the microcontroller, etc. This is even harder to maintain than the page scheme and less useful. OK, so R105 is probably part of the power supply. Now what? That gives me a rough idea of one of the many dimensions but does nothing for the others. Then there will be a large number of in-between cases where are part could be thought of as belonging to two or more subcircuits. This becomes a mess quickly and takes more effort and attention to maintain than it ever saves. Forgettaboutit, keep it simple.

As for trying to number them by value, that makes even less sense. That's what the BOM is for anyway. Having sequential numbers for each BOM line doesn't solve any problem I have ever encountered.

Let your software pick whatever numbers it wants to initially. As you edit the schematic, there may be gaps and things move around. Don't worry about it. When the schematic is all done or you're going to export it for others to look at, you can run a renumber utility if your software has that. That usually starts the numbering for each component type at 1 and goes up sequentially. They will probably be in some rough order by placement on the schematic, but don't count on that. Once you realize that component designator numbers are arbitrary labels, life becomes simpler.

No scheme is going to give you much information about part usage just from the number, so you need to make a cross reference listing anyway. I use Eagle and have created the INDEX ULP for that purpose. It makes a alphabetic list of all component designators and gives their schematic and board coordinates.

-
I don't agree that the 3 digit designators are useless. I've been designing PCBs for more than 10 years and at some point I felt the need to have a way to easily know to which subcircuit each component belongs. On simple circuits this may not be relevant but when you have complex circuits it makes sense and it saves a lot of time when troubleshooting or testing. –  Bruno Ferreira Jul 20 '12 at 12:22
+1 - I think you're the only one who mentioned re-annotation afterwards. –  Joel B Jul 20 '12 at 14:29

One convention is to use a multi-sheet (flat or hierarchical) schematic and on each sheet have a portion of the overall design (e.g. power supply, MCU, I/O interfaces, FPGA, etc)
Then you use a across and down (or down and across) numbering system on each sheet, but prefix the number with the sheet number. For example R10, R11, R12 on sheet 3 become R310, R311, R312. On sheet 2 they would be R211, R211, R212.
This way you can recognise what subsystem the component is part of by the first digit.

Many PCB software tools have the option to annotate automatically in this way.

-

I like the designators assigned by physical layout on the PCB. This way when looking for R56 you can tell you are getting close when you see R54.

But this is also the hardest because it involves back annotating to the schematic. Then the purchasing BOM needs to be redone because the original BOM was created using the schematic. Now all the designators have changed.

All in all, it's a pain.

-
@FedericoRusso, even if you don't like it, this method is common enough that Altium provides an automatic tool to re-number this way. Of course it also automatically back-annotates the schematic, which allows you to automatically regenerate a BOM reflecting the new designators. –  The Photon Jul 20 '12 at 16:00
The BOM for purchasing doesn't need the reference designators, I just part numbers and quantities. After back annotation I regenerate the BOM for production. –  Brian Carlton Jul 20 '12 at 17:40
@FedericoRusso, any reason why you think this is bad? I personally prefer this approach, especially because modern tools support back-annotation and automatic BOM generation. –  ajs410 Jul 20 '12 at 18:39
@ajs410 - well, he says himself that it's a pain. And the EDA software may do the back-annotation it's you who'll have to do the renumbering. (I don't know why my first comment, saying this is a bad way of doing it, was deleted.) –  Federico Russo Jul 21 '12 at 7:45
@FedericoRusso As The Photon says above, Altium renumbers for you and back-annotates to the schematic. It's really quite painless. –  ajs410 Jul 25 '12 at 14:35

Using consecutive numbers for the same resistor value doesn't make much sense. Like you say they will be spread across the board, so how is this going to help with populating the board? Also components are automatically numbered as you place them, so you would have to override that number for each part; it's unlikely that you place all resistors with the same values at the same time.

I usually start with the power supply, and then the main IC, like a microcontroller. So capacitors around my voltage regulator will be C1, C2 and the like, continuing with C5, C6,... for the decoupling capacitors of the uC. If you place them in that order C4 and C5 may end up in each other's vicinity on the PCB too. Most of the time it isn't worth the trouble to change that.

If you have a more complex board where you can distinctly separate different function blocks you may use a new numbering for each block. You'll want to draw an outline around each block, or place them on different sheets. The first function block may have capacitors C101, C102,..., while for the next function block you'll find C201, C202,.... This only requires you to change the next number once for each new block you draw in your schematic.

-

A commonly-found system in stereo audio systems is to use three digit refdes's, with the first digit denoting the channel. This practice makes troubleshooting a lot simpler. Most audio problems will only affect one channel. So the repair technician can quickly run through the voltages of the circuit and look for values that differ between channels. If Q214 has 15V on the collector and Q114 has 5V, there problem is in that stage or a previous stage.

A similar practice is useful whenever there are other duplicated circuits. When you make the repair technician's job easier, you make your own job easier.

-

I don't thing there is a standard naming convention for that.

What I do is to divide the circuit in functional blocks and have a different hundreds digit for each block.

So, for example:

Power supply block will have R101, R102, C101, C102, U101, ...

MCU block will have U201, C201, C202, ...

This way it is easy to know where each component belongs.

Regarding grouping by values I don't think is a good idea because in order to do that you cannot group by functional blocks.

-

The method I prefer to see uses blocks #'s of REF DES assigned to each functional module or logical block on the schematic.

Reason

• They do not need to be all used up in contiguous blocks.

• More convenient for troubleshooting, and functional theory of operation.

• There is no benefit in automated assy, so don't care

• In manual assy, as long as it is easy to locate and blocks on schematic tend to be located physically close.

• ease of adding components without breaking the RefDes sequential scheme...

• Numbers assigned are designer's choice, i.e. arbitrary and and logic depends on ease of interpretation.

hmm last second I see my answer is same as Bruno's... Over 4 decades of reading schematics, I find the worst to read are automotive ones on hundreds of pages that are "logical" and functional but not as good as Tektronics for Instrument design and Hitachi for peripheral desig. Maxtor also had excellent documentation on disk drives.

As long as you consider the person who has to support your design after you move on, and don't create a schematic that is hard to find parts , leaving them to feel like it is a Where's Waldo or where's Goldbug baby-book, I would consider any convention is fine. Just make it error free without duplicates or missing parts unless intended.

-
Yeah, automotive "schematics" are usually more wiring diagrams and it's often difficult to follow a signal to see where it really goes. –  Olin Lathrop Jul 20 '12 at 18:00