The LED in question is described as 0805 dimensionally. However, the footprint in the PDF is different from that described as being suitable for a resistor. For example, the gap between the anode and cathode is a recommended 1.1mm while that between resistor electrodes is typically 0.65mm

Can I put these LEDs onto 0805 resistor footprints?

  • 1
    \$\begingroup\$ 1.1 is the same as 1.1. Is there a typo here? \$\endgroup\$
    – caveman
    Jan 26, 2015 at 14:16
  • \$\begingroup\$ Yes - corrected \$\endgroup\$ Jan 26, 2015 at 14:23
  • 8
    \$\begingroup\$ If you do decided to just use the resistor pad, consider making a copy of the footprint and adding a diode direction indicator. If you don't you have a 90% chance your assembler will put it in backwards. \$\endgroup\$ Jan 26, 2015 at 15:38
  • 3
    \$\begingroup\$ I love that everyone agrees that the chance is higher than 50% despite there being only two ways to populate it. \$\endgroup\$
    – ACD
    Jan 26, 2015 at 15:57

3 Answers 3


Yes, you can place your 0805 LED onto a 0805 resistor pad. The LED has the exact same pad size as a 0805 resistor so it will fit on the pads fine. Recommended pads are useful but when you're using a part with an established pad size like 0805, it's unnecessary to match it exactly. I've had parts with established pad sizes have recommended patterns slightly different in one dimension or another. I've never had issues ignoring the recommended pattern and using the generic 0805 pattern.

I assume Passerby was talking about if you were hand soldering parts(?). Your manufacturer should have no problem putting the LED on a 0805 pad. There's definitely no harm in taking 3 minutes to make new pads for the LED, but I find it a little unnecessary to say you need to take all those steps if you don't.

edit - somehardwareguy has it right in the comments though. You'll want to add an indicator in there so the manufacturer knows which side is which.

  • \$\begingroup\$ I just did it the hard way - created a new package footprint \$\endgroup\$ Jan 26, 2015 at 15:59
  • \$\begingroup\$ Ah ok, well I guess in the future you now know you don't need to. It probably worked out well in this case anyway, since you needed to add a direction indicator, and it's usually easier to add that to the pad layout instead of adding it on the silk layer. \$\endgroup\$
    – I. Wolfe
    Jan 26, 2015 at 16:04

What is the correct size footprint for an 0805 chip resistor? Anyone? If we all fire up our favourite PCB design softwares I bet we'll all come back with a slightly difference answer. I realise I might be wandering off topic a bit, but if helps to answer questions from other people later on then it's worth writing.

There is in existence the IPC-7351 standard. It's really boring [Check it out!] but it does give explicit naming conventions and, the reason for the answer, PCB land patterns. That said, I didn't get very far into the document before my brain shut down, so I don't have any quotable sizes from the horse's PDF. However, my PCB software (Proteus) comes with the full IPC library as well as it's own. See the following:

IPC 0805 footprints

Yes, that's three footprints for 0805 chip resistors, and one for an 0805 LED. They all differ slightly, and they're all IPC. The turquoise is silk-screen graphics and the black outlines are the "occupancy" boundaries. Red is of course the pads, but I haven't shown solder mask or paste outlines. From top to bottom:

  1. RESC2012X50 - 0805 @ 0.5mm high. Pads 1.45 x 0.94 mm, centres 2.0mm (gap 1.06mm);
  2. RESC2012X60 - 0805 @ 0.6mm high. Pads 1.39 x 0.94 mm, centres 2.0mm (gap 1.06mm);
  3. RESC2012X70 - 0805 @ 0.7mm high. Pads 1.39 x 1.04 mm, centres 1.9mm (gap 0.86mm);
  4. LEDC2012X120 - 0805 @ 1.2mm high. Pads 0.99 x 0.94 mm, centres 1.8mm (gap 0.86mm).

Now have a flick through some datasheets for 0805 resistors (or any other 0805 component) from different manufacturers and see how many fit one of the above specs exactly. Very few, if any.

So what's my point? I suppose it's "do whatever's easiest for you". But excercise some common sense: What's the difference between a resistor and an LED - polarity! Yes, you can use a resistor footprint, but you'll have to mark the cathode. You could just add your own graphic if you want, but don't forget some poor bugger has to make this board and he'll have no idea what your circuit does or which way round things go unless you tell him. So long as you use common practices (marking cathode not anode) I'm sure it will be fine.

At the end of the day you should ALWAYS read the component datasheet. You might end up with a power LED that has a third pin, electrically isolated from anode and cathode, just for removing heat. If you fail to include a copper pour and some breathing space around the LED because you didn't read the instructions it might cry, and water and electricity don't mix.

  • \$\begingroup\$ I think you allude to it, but there isn't "one true measurement" for an (e.g.) 0805 package. If I recall correctly, IPC specifies 3 different land dimensions for all the standard parts (chip passives through ICs). They're somewhat annoyingly named, "Least", "Most", and "Nominal", and whose letters are all consecutive (LMN), but in a mixed order from smallest to biggest (132). \$\endgroup\$
    – Nick T
    Jan 26, 2015 at 20:25

Recommended is not absolute. Adjust how much solder or solder paste you use, and test for shorts. Of course, it's just easier to use the recommended footprint.

  • \$\begingroup\$ I can't do that because it will be manufactured elsewhere. I guess I will have to lay out a new package footprints. \$\endgroup\$ Jan 26, 2015 at 14:42
  • \$\begingroup\$ If you have someone making the boards and machine placing the parts I doubt it would be an issue. Really comes down to what point of the design process you're in. If you've already paid for a stencil, just go ahead and place the LEDs on the 0805 pads. If you're still designing the board and just didn't want to make new pads, make the pads to match the LED recommended specs. It doesn't take long so might as well do it right. \$\endgroup\$
    – I. Wolfe
    Jan 26, 2015 at 14:49
  • \$\begingroup\$ I have always used a "generic" 0805 footprint for all my 0805 components. Never had a problem with any of them. \$\endgroup\$
    – Majenko
    Jan 26, 2015 at 15:08

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.