passive footprints

[Simon]

I once copied my 1206 and 0805 footprints from a resister datasheet. But i found that some 0805 components sometimes pull to one end so go open circuit. i think maybe my footprints are a bit out. So i went on the hunt again and looked at a sample of datasheets where I found a varying range of sizes with some datasheets giving multiple sizes for various density levels of boards.

So is it just me or are the basic passive footprints more a case of anything goes?

[wraper]

But i found that some 0805 components sometimes pull to one end so go open circuit.

You mean tombstoning? It could be there is too big gap in between of the pads, too much solder paste applied, crappy reflow profile. Also sometimes you can stumble on some stupid components which are just prone to tombstoning. For example I have a reel of such 0603 caps and had 0805 ferrite beads. Replacing with different part solved the issue. I suggest you post a pic with those footprints so we can see if there is anything wrong with them.

[rx8pilot]

Passive footprints are subjective in most applications. I have about 4 variations per common size depending on the needs of the design. Some considerations are component density, ease of hand-assembly, impedance control, reliability, and perhaps a few others.



Typet purly on my fone.

[DannyTheGhost]

But i found that some 0805 components sometimes pull to one end so go open circuit.

You mean tombstoning? It could be there is too big gap in between of the pads, too much solder paste applied, crappy reflow profile. Also sometimes you can stumble on some stupid components which are just prone to tombstoning. For example I have a reel of such 0603 caps and had 0805 ferrite beads. Replacing with different part solved the issue. I suggest you post a pic with those footprints so we can see if there is anything wrong with them.

Also, another reason for tombstoning is asymmetrical traces going to the pads. Traces also act like heatsinks, so during reflowing with bad amount of luck one pad will not be hot enough to melt solder during reflow

[Kasper]

Another cause of tombstoning can be uneven heat sinking. If one pad has a big track and the other pad has a small track then one may heat faster than the other.

When solder turns to liquid, surface tension pulls the component towards it. If that happens at different times for different pads then components can tombstone.

Try to have even amounts of copper connected to each pad. When that is not feasible, thermal relief connections should help.

[wraper]

But i found that some 0805 components sometimes pull to one end so go open circuit.

You mean tombstoning? It could be there is too big gap in between of the pads, too much solder paste applied, crappy reflow profile. Also sometimes you can stumble on some stupid components which are just prone to tombstoning. For example I have a reel of such 0603 caps and had 0805 ferrite beads. Replacing with different part solved the issue. I suggest you post a pic with those footprints so we can see if there is anything wrong with them.

Also, another reason for tombstoning is asymmetrical traces going to the pads. Traces also act like heatsinks, so during reflowing with bad amount of luck one pad will not be hot enough to melt solder during reflow

Forgot to mention that. But it's usually not that paste is not melting (you'll notice that). But that it's melting on one pad with delay relative to other pad.
EDIT: and if it's a crappy reflow oven, you don't even need any of those issues mentioned earlier for tombstoning to happen. Uneven heating by oven itself is already enough.

[Simon]

Ah, yes, it seems that it might be that the board is unevenly heating. I think the caps in question (I will have to check tomorrow at work) are bypass caps that go from a solid ground plane to the positive of a chip. I think the pads are that far apart that the positive pad heated first and that cap terminal pulls to the centre of that pad pulling it off the ground pad.

My new layout uses a pad that is more centred under the parts terminal so it will tend to move less i hope. The cap does not tombstone.

I am using a little Chinese re-flow oven and it does struggle to heat.

[rx8pilot]

Uneven paste deposition is a major contribution to tombstoning. Are you using a stencil or a hand-operated syringe for the paste?

Typet purly on my fone.

[Dubbie]

I went from having to rework every single board I reflowed to practically zero rework after I built my stencil holder. It made an incredible difference to the quality of my paste job. I got the idea from someone here on the forum. It’s made of thick aluminium machined very precisely after machining and lapping everything perfectly flat.

[Simon]

I am using a stencil. I think the uneven heating is the problem. Presumably my new footprint will help? If the terminals are already centred on the pads presumably the part won't pull to one side due to capillary action centring it as it is already centred.

[Bud]

I have done several thousand pads with a syringe, my boards had utmost uneven paste deposition you can imagine, that has never caused tombstones. What causes tombstones is too quick heating. Simply extending the initial heating phase  took care of that. Strictly speaking, it was uneven heating,caused by insufficiently long preheating ramp.

[Simon]

But i do not have tombstoning, simply that the part is pulled to one pad. It does not stand up on one end. I preheat to 125C for some minutes to get everything as hot as i can without damaging it and then go for solder temperature. The ovens built in profile does not work as it is "too fast" for the oven to work so i manually control the temperature.

[rx8pilot]

But i do not have tombstoning, simply that the part is pulled to one pad. It does not stand up on one end. I preheat to 125C for some minutes to get everything as hot as i can without damaging it and then go for solder temperature. The ovens built in profile does not work as it is "too fast" for the oven to work so i manually control the temperature.

Do you have any pics? I have personally never seen that and I have placed millions of SMT components by hand and machine, stencils and syringes, ovens and hot air guns.
Now I am curious.....

[Simon]

I can take some tomorrow. The part simply move to the positive pad so far that it comes off the pad on the ground plane.

[Kasper]

I too would like to see that.

My guess is your pads are too far apart.

[Kasper]

I went from having to rework every single board I reflowed to practically zero rework after I built my stencil holder. It made an incredible difference to the quality of my paste job. I got the idea from someone here on the forum. It’s made of thick aluminium machined very precisely after machining and lapping everything perfectly flat.

Nice job. Thanks for sharing.

[Simon]

I too would like to see that.

My guess is your pads are too far apart.

That is what i thought but I found footprints in datasheets that range from as far apart as mine to much closer so i have closed the gap anyway as it allows for denser layouts

[T3sl4co1l]

Following manufacturer footprints (if given) is a crap shoot.  They have various priorities, which may not be the same as yours.

Following IPC recommendations is the most universal.  Any assembly house should be able to succeed with those.  Go download IPC-7351, whichever version you can find, and read through it.  You can use calculator tools as well.  Can also look at SM-782, but it's superseded by 7351, and gives annoyingly small pad gap figures for most parts.

Finally, do a sanity check on the final dimensions, and adjust accordingly:

Will the pad gap REALLY be as awful as the worst-case dimensions imply?  Or will that be wasted pad and paste area and potentially lead to shorts under the component?
Does the component actually have any side fillet at all (e.g., chip resistors typically have top, end and bottom, but not side, metallization)?
Do you even care?  Chip caps and multilayer inductors/FBs normally have wraparound metallization, but a large side fillet takes up a huge amount of space, and may make the part more prone to cracking.
For leaded parts, are the pads narrow enough to allow soldermask inbetween, or will that be optimized out by the fab -- or worse yet, left in, and the too-thin webs flake off during soldering?
(FWIW, for 0.5 and 0.65mm pitch components, it's almost always perfectly fine to use pad width equal to half the pitch, give or take a little fudge.  This leaves enough space between pads for two solder mask expansion plus one solder mask minimum web width.  0.8+ mm pitch you have more room to play with, and you can take more consideration of pin width and side fillet.  Some 0.8mm pitch AVRs with wide pins come to mind.)

And as mentioned, pad heatsinking ratio is important.  Thermal relief is not a problem even for power components -- copper is quite conductive, calculate the electrical and thermal resistance yourself!

If you've done all this and your parts are still shifting or tombstoning, check the reflow process, definitely.  That's probably the bigger elephant to begin with though.

By the way, tombstoning, as such, is very rare for larger (0805+) components.  Gravity dominates and the part tends to stay flat.  The nearest thing you'd expect, then, is shifting lengthwise, lack of wetting, or head-on-pillow failures.  Basically still tombstoning, just without as much vertical element.

Tim

[Simon]

Thinking about it it is more a case that the part tips ever so slightly and the solder for some reason goes to the furthest point on the pad and nowhere near the part so i figured that bringing the pads in would bring the outside edge closer the the part and hopefully the solder is less likely to not end up on the part. I'll take pictures tomorrow as I've not looked at the boards in a while (been switched to another project) .

[Simon]

OK, i have some snaps. It's actually the other way around, they have pulled to the ground plane. I guess the ground planes sucked up all the heat.

[Dubbie]

Those pads look way too far apart. You should rely on surface tension to pull each contact pad to the center of its pcb pad. There shouldn’t be a tug of war between two pads because you will be the loser!

[Simon]

Well so much for manufacturer datasheets

[DerekG]

Yes, the pads are clearly too far apart.

Also, the tracks to the ground plane are far too wide. They suck up the heat, delaying the solder on that side from fully melting in unison with the other solder pads on the board.

As a guide the tracks should leave the back-side of the pad furthest from the resistor itself. For 0805 resistors the thickness of the track should normally not exceed 24mils (thou). Never connect the entire pad to a copper plane.

[Psi]

You definitely need some thermal relief on those pads. (google image search 'thermal relief pad' if you're not sure)

But you might get away with keeping the same gap if you reduce the size of the pads to stop the component moving around so much during reflow

etc,  A and B have the same gap but A will cause the part to tombstone a lot more than B
This is because a part will sometimes tombstone after it has first slid off a pad (ie when surface tension stops holding it down on one side it will start to lift up).
The B option gives much less room to slide around and slip off a pad.
Keep in mind that the B style will only help reduce movement based tombstoning, it wont help temperature related tombstoning. You will still need to add thermal relief.

[wraper]

OK, i have some snaps. It's actually the other way around, they have pulled to the ground plane. I guess the ground planes sucked up all the heat.

Those footprints are junk. You need much smaller gaps in between of the pads, pad size itself is OK as is. Also you certainly need thermal relief as already said.