Eagle pad size recommendation

[substitute]

Hello,
I got back some PCBs that I designed using Eagle, the component pads are a little small and I find them difficult to solder.  I understand how to change the pad sizes, I just don't know what to change them to.  For instance, Gustav's PCBs have always been very easy to work with.

Here's a link to the component library I used.
http://gaussmarkov.net/wordpress/tools/software/eagle/eagle-2-libraries/

Opening up a 1/4 watt resistor (for example) in the editor, the drill size is 0.02755906 which is fine, and the pad size is set to auto.  It seems like that amounts to the pad being 0.046 diameter.  If I change it to 0.05 it's a slight increase.

So my question is, what's a nice comfy pad diameter for components like 1/4 watt resistors, panansonic chicklet caps, etc?

Thanks!

 

[gar381]

Hi substitute

I just use the stock pad sizes in the rcl.lib 
for most resistors and caps.
I have use this .lib for years with much success. 

Best

GARY

 

[PRR]

> pad being 0.046 diameter

For hand/eye soldering??

I think classic DIP pads are small. They on 0.1" centers, small gap between, twice as long as wide. Maybe 0.075" * 0.15"?

Big enough to find without nose-scratch.

That's 10X the area of your default.

For discrete parts with more than 0.1" lead spacing, I really like 0.2" diameter (or 0.15" * 0.3").

This will increase overall board size requirement, true. But you have to build it before you can use it. You don't have sharp-eyed young women or programmed robots to do it.

 

[john12ax7]

If you are hand building, bigger is better. As a rough guide, add 10 mil to the diameter of the part for drill size and at least 40 mil on top of that for the pad.

So a part with 25 mil leads, use 35 mil hole and a 75 mil pad.

Samuel Groner had a nice write up for common part sizes.

 

[substitute]

Thanks everyone.  I also found this...

http://www.pcb-3d.com/knowledge-base/pth-dimensions

It sure is a pain toggling back and forth between mils, inches, and millimeters.  If only Jimmy Carter had issued a metric system executive order...

To clarify, these PCBs are for effects pedals, they're relatively simple circuits in 1590bb enclosures.  So, on one hand, there's not tons of space but the layouts aren't super dense.

Thanks again!

 

[PRR]

> a pain toggling back and forth between mils, inches, and...

Inches and Mils are the same, only 1,000X smaller. Swap the comma and dot. 10 Mil is 0.010 Inch.

Those French units.... but ya know, an awful lot of "odd metric dimensions" turn out to be even-inch numbers, because inch-based US makers dominated the field in early days.

"Maximum Lead Diameter + 0.25mm"

0.25mm is 0.010 Inch (or 10 Mil). Your abacus may say it should be 0.254mm, but we don't need 3-digit accuracy here, it's just a pad.

All those "2.54mm" lead spacings on chips and connectors ARE 0.1 Inch (here we need the 3rd digit because across a 100-pin connector it would add-up).

Those "Level A B C" specs are for EXPERTS. And are stated to be Minimum. If I threw baseballs all day, I could sink a 4 inch hole most of the time. If I pitch only a wee bit between other life activities, I want a hole a foot or a yard wide.

One thought is: don't make pads, make ditches. Save all copper except the little bit needed to separate "pads", which may be half the size of the parts. At 9V-50V, ditch width is about your etching precision, not voltage.

 

[substitute]

PRR, how you can convey so much wisdom and wit in seven lines about solder pad sizes is beyond me. 

I emailed Gustav directly, his pad sizes are about 2.4mm for such components for future reference.