I have been updating some projects to 5.1.0 with the new 0603 resistor footprints, either standard or handsolder. These now have rounded rectangular pads.
Before I was routing 0.5mm tracks through them. Now I find 0.3mm usually just works, but sometimes, presumably with rounding errors, I have to go down to 0.29mm.
Was this really intended?
When I first look at KiCad (just before 4.0.7 released) I noticed that 0603 resistor footprint has very large gap betwean pads (1mm). I thought it is genius as I will be able to go under it with two 0,2mm tracks with 0,2mm clearance.
For me it is important as my PCBs are two layer with bottom full GND. As I don’t go at bottom with signal tracks I need a possibility of crossing some signals and I sometimes added 0R resistors just for it. I have never before thought about makeing pad gap under 0603 so big.
I was happy with it till I asked my contract manufacturer and they didn’t accepted so big gap as being out of production tolerances.
I looked for other firm footprints and they have smaller gaps for 0603 resistors. If you look at resistor pictures you will also notice that they have different sizes of contacts. As I don’t wont to say to contract manufacturer: “I don’t accept any other resistors then VISHAY” I designed my R0603 with smaller gap. My contract manufacturer said 0,85 is maximum, but I designed 0,9mm with hope that when I will need I will use 7mils track with 7 mils gap to put two tracks under R0603.
When I sow rounded corners I said I like it. It is not important at inside of R but at outside the corners frequently were for me the problem to have enough space for tracks.
1 Like
The footprints are now IPC 7351B compatible from the fillet sizes but already include the pad shapes as suggested by IPC7351C
The resistor sizes come also from IPC where we could find them. But we researched a lot and looked at how real resistors compare to that definition. For 0805 this was a full on discussion over at github with wayne. (It seems these resistors are produced quite differently debending on manufacturer which means one footprint to rule them all might not really be fitting if you have high yield requirements or if you want to achieve something special like getting a trace through the gab.)
1 Like
The pad to pad spacing seems to be 0.7mm now.
The old 1mm caused be some pain, super fussy about placement and to be honest any crossing track near the pad depended on the resist to avoid shorting to the resistor end cap.
I would not go for 0.9mm either for the same reason. 0.8mm should be fine.
It is hard to interpret the data sheets. The nominal insulated span of a Panasonic 0603 is 1mm, but the tolerances are large and there is no guidance on how these are correlated. A very unlikely worst case could mean almost no gap at all.
With 0,9 I have designed one PCB.
I didn’t remember what gap I left when changing pads to rounded. I’ve checked - I left 0.8 
I will try my own footprint with 0.81mm, so that a 0.4mm track will pass through reliably
My decision was to have round such values - so I would use 0.8. But clearance I would define to be 0.1999.
I have checked (4.0.7) that it worked well.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.