Standard package footprints

Question

I'm looking for footprint dimensions for the standard packages like 0402, 0603, 0805, etc.

I did a quick search on Google, but I got many different results and I got confused.

Is there something very common to use both for resistors and MLCC capacitors? I don't want the pads to turn out too big or too small.

score 4 · Accepted Answer · answered Mar 26 '17 at 13:04

4

Each manufacturer is going to have their own recommendations for land patterns. However, IPC-7351 is a more generic standard that covers SMD component sizes and footprints. There are usually three versions of every footprint: Low density (level A), medium density (level B), and high density (level C) designed for low, medium, and high density boards ("density" referring to how tightly together the components are placed). When I lay out a board, I determine how many components are needed and how tightly packed they will need to be based on the dimensions of the board, and I will pick one density level. I will then use the footprints for that level.

IPC has a land pattern calculator that can help you determine how large or small to make your pads for surface mount components based on the physical dimensions of the component itself (provided by the manufacturer) and the desired density level. The above link will download a ZIP file containing the installation files. If you a tool such as Altium Designer to design your board, it has this calculator built-in and you can generate footprints by entering the component dimensions.

answered Mar 26 '17 at 13:04

DerStrom8

21,042
8
61
95

I use Altium Designer and I use its built-in IPC footprint wizard for other type of components like ICs. I didn't think it before, I'll give it a try. I haven't mentioned my assembly process which is "reflow" by hot air and might a little "hand soldering" would be necessary to make some changes due to R&D. In my recently prototype I choosed very restricted pads for 0402, I didn't expect that it would be that tiny. I can't remember where I found these rules. Although, it doesn't seem that bad and the assembly carried out successfully. – MrBit Mar 26 '17 at 21:03
However, as long as I can see in all these documents I understand that there are different "standars" depending on component type. I think this might be due to high of the component, which, for example, in MLCCs is greater than resistors therefore more solder paste is needed. But, after all, I'd expect to find something common. – MrBit Mar 26 '17 at 21:18
1

You actually bring up another excellent point -- the footprints will vary depending on whether you want to reflow or wave solder (or hand solder) the parts. I think IPC has different standards for these as well. I definitely recommend reading through the IPC document I posted in my answer. It's very long, I know, but it has a lot of information that will be very useful – DerStrom8 Mar 26 '17 at 22:52
Regarding Altium's IPC Footprint Wizard, indeed, looks pretty good but it bothers me little that I have to choose the dimension of Bandwidth Range (T) of the package. This means I will have to make dedicated footprint for each standard component. – MrBit Mar 27 '17 at 16:55
Not necessarily true, just plan for the worst case and a single footprint will work for just about every component that uses that package – DerStrom8 Mar 27 '17 at 17:06
That's what I intend to do. Although, I can't predict the worst case but I'll add some more solder area in the pads. – MrBit Mar 27 '17 at 17:16
Do you think that this is ok to use with Altium's IPC Footprint Wizard? http://www.tortai-tech.com/upload/download/2011102023233369053.pdf – MrBit Mar 27 '17 at 17:50

score 1 · Answer 2 · answered Mar 26 '17 at 12:52

Either find a representative part to design your pads to, or back to first principles and design the pads to that. The numbers in the package sizes you quote (there are others that use metric) are in units of 10 mils. So "0805" means the package is 80 x 50 mils. The metric ones are in tenths of mm. "4321" would therefore mean 4.3 x 2.1 mm.

The optimum package size depends on how the part will be soldered and if you really need every last mil of room. Most of the time, I add about 20 mils to pads lengthwise. That allows for manual soldering, and gives a little room for holding the tip of a scope probe on the pad. Generally for stand-alone parts like these two-terminal ones you are asking about, I leave about 5 mils extra for the width, and maybe 5-10 mils extra length on the inside end of pads.

score 0 · Answer 3 · answered Mar 26 '17 at 11:12

Accurate dimensions depend on stuff like solder paste, pcb finish a so on. But on the other hand they don't matter that much. Take something and see how it works in assembly. Biggest risk is that after prototypes they will ask to make some changes, usually very minor.

score 0 · Answer 4 · answered Mar 26 '17 at 12:14

Some manufacturers will specify recommended land patterns, and since they are standard sizes, these will usually work for most or all other parts with the same package size. E.g. a 0603 cap will solder fine on a footprint for a 0603 resistor. There is some amount of tolerance and you can probably adjust if needed, but you most likely wont need to if you use standard footprints. This document gives footprints for standard sizes.

Standard package footprints

4 Answers4

Linked