8
\$\begingroup\$

Let's say I have diode or a polarized capacitor in my circuit.

How do PCB manufacturers know how to orient the part on the PCB?

When I create the part in Altium for example, I just make up which pin is pin 1 and which pin is pin 2. As long as the schematic matches the PCB, it won't throw an error at me.

In other words, is there something that relates the pins on the schematic and the pads on the PCB to the real-life leads of the component?

I have not seen on diode datasheets where it says "pin 1 should be the cathode, pin 2 should be the anode", unless it does say that and I am dumb.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ Some datasheets have pin numbers on the footprint. There are also silkscreen conventions. You can put a bar in the silkscreen for a diode to indicate polarity. Or if it is a bigger part you can draw a little diode symbol in the silkscreen. I have certainly had backwards diodes on first runs before. \$\endgroup\$
    – user57037
    Commented Nov 10, 2021 at 17:53
  • \$\begingroup\$ related: "Whats the standard for denoting the orientation of an LED on a PCB?" \$\endgroup\$
    – davidcary
    Commented Nov 10, 2021 at 23:18

2 Answers 2

Reset to default
12
\$\begingroup\$

In other words, is there something that relates the pins on the schematic and the pads on the PCB to the real-life leads of the component?

None, just like there is no standard of whether the anode and cathode in a diode symbol or footprint should be pin 1 or pin 2. It's all up to you to use the appropriate footprint with the schematic symbol you use.

The component in the tape can be any which way and you have to look at the datasheet or the markings on the component sitting physically in the tape reel to know.

You sort it out with 2-way human communication (i.e. notes to the assembler. A diagram is best and clear silkscreen markings are even better.) and the guy sets up the pick and place machine does it.

I've had instances where the guy ignored diagrams accompanying my notes and assumed the silksreen "dots" (not dots as much as little random linear ticks which were artifacts of the footprints in the library I was using) floating around different components on the board were indicators for pin 1. All the ICs came backwards. The IC footprints being used in that case did not have clear pin 1 markings on the silkscreen other than the fact it was always to the top-left when the was read upright RefDes which was why I included a diagram. The diodes in that case were not part of the diagram but not a problem either because I went through their footprints and manually sure all the footprints used had a white polarity line or the actual diode symbol for their silkscreen. After all, I was going to be the one debugging and reworking the board and I needed to know what the polarity was by looking at the board. I assume the guy setting up the pick and place just looked at how the diode sat in the reel since the SMD packaging also had a white polarity line. I doubt he went to the datasheet for every single diode and looked at the packaging information.

This is a much bigger problem for some components like SMD photodiodes which, due to requiring an unobstructed face, cannot have polarity markings on the component. The only way to know which is anode and cathode is to look at which pin is bigger and smaller, but to know which is which you need to go to the datasheet. In that case you really do have to go to the datasheet and look at the packaging information to see which way they come in the reel. It's a major pain. I would probably send a snapshot of every diode datasheet page containing that info as part of the notes.

\$\endgroup\$
9
  • 1
    \$\begingroup\$ Yeah, I have also had components placed backwards on PCBs before - I guess it comes down to having clear symbols on the silkscreen and good manufacturing notes. What did your notes to the manufacturer usually look like? place the positive terminal of the component on the side with the "+"? \$\endgroup\$
    – RGB Engineer
    Commented Nov 10, 2021 at 4:39
  • 1
    \$\begingroup\$ @RGBEngineer Actually, it was worse than that. I remember now. It wasn't text notes. It was actually a diagram of the board printed from the Gerber and all the ICs on the board with pin 1 labelled. The IC footprints being used had pin1 always to the top left of the RefDes when read upright but that's not obvious so I included a diagram. For that one, the diodes were not part of the diagram because I made sure the silkscreen contained a white polarity line or the actual diode symbol. There were no issues with the diodes. The human manually went through and sets up the machine for each component \$\endgroup\$
    – DKNguyen
    Commented Nov 10, 2021 at 4:42
  • 1
    \$\begingroup\$ This might be a much bigger problem for some components like SMD photodiodes which, due to requiring an unobstructed face, cannot have polarity markings on the component. In that case you really do have to go to the datasheet and look at the packaging information to see which way they come in the reel. \$\endgroup\$
    – DKNguyen
    Commented Nov 10, 2021 at 4:51
  • 2
    \$\begingroup\$ @RGBEngineer God that was a shit show. Had to send all the boards back and some sucker on their end had to manually desolder and flip all the ICs around and I'm pretty sure the high failure rates on that run were because not all the components survived the desoldering. \$\endgroup\$
    – DKNguyen
    Commented Nov 10, 2021 at 5:03
  • 1
    \$\begingroup\$ @RussellMcMahon And make sure the guy you go over the instructions with is the same guy who is going to be using them. In my story, I did go over the instructions but apparently it wasn't the same guy who was doing the work. \$\endgroup\$
    – DKNguyen
    Commented Nov 10, 2021 at 14:14
7
\$\begingroup\$

I have not seen on diode datasheets where it says "pin 1 should be the cathode, pin 2 should be the anode"

It is because you are looking in the wrong place. The datasheets define the pin function of the specific part. The orientation (called "zero orientation") of the pins in the footprint is defined by IPC-7351 (IPC-7351B). Specifically in your case:

SOD Diodes – Pin 1 (Cathode) on Left

Aluminum Electrolytic Capacitors – Pin 1 (Positive) on Left

The above applies both to SMD components and Through-hole axial and radial packages. Moreover, it also applies to non-polarized components (resistors, inductors), as far as land pattern numbering is concerned. Maybe it does not make much sense, but it does bring a bit of an order into the CAD chaos.

How do PCB manufacturers know how to orient the part on the PCB?

When you send your files to manufacturing house you usually include component positioning file, which specifies component coordinates and rotation relative to zero orientation. So, if your footprints conform to IPC-7351 standard then manufacturers know exactly how to orient the part on the PCB. If still in doubt they can also consult silkscreen markings, which coincidentally defined by the same standard.

\$\endgroup\$
2

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.