PCB Pad Size

[grimmn]

So I'm currently working on designing my first PCB that I'm actually planning on getting made and I was just wondering what criteria you all use for sizing drill holes and solder pads?

[lewis]

Drill holes are normally about 0.05-0.1mm larger in diameter than the pin going through the hole, but for easier insertion and soldering you can make them 0.2-0.4mm larger. 0.8mm works well for almost all through hole resistors below 1watt, all DIP IC pins, 1N4148s, TO92 transistors and the like. Use 1.0mm for header pins, TO220 packages, 1N4001, etc. and 1.3mm for terminal block connectors.

Rule of thumb with pads is make them as large as you possibly can (within reason). Ensure adequate spacing between adjacent pads - 8-10 thou is good - but otherwise make them as big as you can. Same goes for tracks, make them as fat as possible at all times. Rounded finger pads are good for DIP ICs because they give you more surface area for solder contact while still allowing you to easily route a track between pins.

Bigger pads also give better adhesion to the board substrate, so if you have any large and heavy components (big psu caps) it's a good idea to give them extra big pads to ensure the mass and leverage of the component doesn't break the pad off the board when your board is chucked about.

I usually specify drill size in mm but work with thou for pad/track sizes.

[Psi]

If your board includes any QFNs and you will be assembling them yourself it's a good idea to edit the qfn footprint and expand/move the pads lengthwise a little. That way there's more exposed pad extending beyond the package and this makes drag soldering easier.

The same thing goes for SMT resistors/caps. If you plan to hand-solder then you want a good amount of extra pad beyond the component.
Use the bigger "low density" footprints if there's an option. The "high density" footprints are for pick-n-place / reflow and have little room around the package.

[Falcon69]

If you are doing SMD components, some manufactures have a pad layout sizing on their data sheet for that component. If they don't have a pad layout for that, then you can look at a similar component, (i.e. sot-23) from another manufacture, and they may have the size on their data sheet.

Most, PCB drawing programs already have the standard pad layouts and more for components that you can use, but always double check the datasheet of the component you are buying.

[Psi]

When using footprints from other components always check the pad numbering at least twice.

Its very common to make mistakes here and have your pads numbered 1 2 3 but the IC is actually 3 2 1  etc..
Its a real PITA when you find out after the PCB is made.

Also, watch out when viewing the PCB design from one side and working on the other side.
 If you're looking at your PCB design from the top, and checking the bottom layer footprint numbering, it's very easy to forget you're looking at a mirror image of the bottom layer.  If you just match up a datasheet picture to the screen you will get it wrong.

[Kremmen]

When using footprints from other components always check the pad numbering at least twice.

Its very common to make mistakes here and have your pads numbered 1 2 3 but the IC is actually 3 2 1  etc..
Its a real PITA when you find out after the PCB is made.

Also, watch out when viewing the PCB design from one side and working on the other side.
 If you're looking at your PCB design from the top, and checking the bottom layer footprint numbering, it's very easy to forget you're looking at a mirror image of the bottom layer.  If you just match up a datasheet picture to the screen you will get it wrong.

So true. Been there, paid the price. Now i _never_ insert an ad hoc component on a PCB, period. Every single one comes from a trusted library every time. The downside is that i have had to create all the libraries i really trust, but that is OK. I will want to include the vendor part numbers and datasheet links to the components anyway.
So after checking, double checking and triple checking the library components when they are created, there is no need to further adjust anything while designing the actual PCB. In fact it is a definite no-no. If a component turns out to be not suitable for any reason, it must be replaced in the schematic with another library component. If one does not exist it must be created in the library using the regular workflow for that. Once created, checked and provided with the proper metadata, it can replace the problem component and the change propagated to the PCB layout. That keeps every step aligned and updated, and you don't need to worry if your mirror images are the right way up

[grimmn]

Tons of useful info here. Thanks a bunch. Time to get back to creating my libraries.