I am trying to use a couple of resistors in my project but I am unsure of what is the correct footprint to use. Looking online there seemed to be a standard “R1” resistor footprint for older versions which is what I want. I am using Kicad 4.0.2. Can someone briefly explain what the different types of resistor footprints are used for?
Thanks in advance!
The surface mount resistors have two footprint options because reflow soldering uses paste on the pad beneath the resistor end caps and hand soldering requires a larger pad to allow the iron tip to touch the pad to use reeled solder
Make your own according to data sheet.
Kicad 0402 size is not good for example.
Way to big.
The pads do protrude enough on datasheet defined 0402 pads.
Examples :
KOA 0402.
Murata 0402 GRM15 series
IEC sizes (imperial).
Don’t get confused as there are metric sized marked packages for them as well and naturally they’re not unique but somehow managed to become offset - a 0201 imperial equals a metric 0603. So be sure what you have in front of you.
Usually the metric size has got an ‘m’ in the front of the 4 digit number.
It’s also good to check what kind of track you can put through the pads (as you might need that very often while layouting). My personal pad spaces can do the following:
Sorry I don’t know why people are talking about SMT resistors!
R1 was a vertical through-hole style, look in “Resistors_ThroughHole”. But there doesn’t seem to be a 0.1" pitch footprint, the nearest is 5mm (0.2"). I guess you need to create your own.
He’s posted a screenshot with ‘SMD’ in there… all of them 
KOA datasheet defined versus Kicad
Both 0402 Resistors
I would not recommend the Kicad version unless you like to have an extra big PCB = $$$
Yeah, the KiCADs Courtyard is definitely generous or taking very old placement machines into account 
As for the pads… depends on the vendor really.
Are you sure KOA Speer does suggest pads that are smaller than the device?
Have a link please? Thx!
Not omly KOA but Muarata also etc etc
http://www.koaspeer.com/pdfs/Appendix_E.pdf
tombstoning comes from too big pads so the solder gets powerful enough to raise the component
“When the pad is too large relative to the component, the pulling force applied by the toe
fillet will increase making the component easier to stand up right.”
double checked
exactly as i made my RK731E footprint
Kicad versus Murata GRM15 for 0402 ceramic cap is not funny either
Hm… 0402, EIA notion, right?
If the yellow outline represents 1x0.5 mm^2, then the pads are too thin imho, unless I do read the document wrong? See also the pink colored area for MLCC:
0.5 x 85% would be 0.425… 0.3 is 60% of 0.5, that’s way below the advisable minimum value, no?
Anyhow, if they work for you then that’s good.
The right tool for standard footprint generation according to IPC-7351 is PCB Libraries Library Expert: https://www.pcblibraries.com/products/compare/
There is a free “Lite” version and it can export to KiCad.
RK73H1ETTP1001F
RK73 series not KQT
IPC is nice but manufacturers recommended footprint (when available) is how I pray
each to his own religion, because thats what it is
