Hi everyone! It’s my first time ordering PCB assembly and the manufacturer contacted me today about errors in my design that caused a lot of tombstoning. They claim I chose too big pads for the too small components and that’s causing issues in the assembly. They’re asking me 300 EUR to rework it, or they’ll send it as is, with errors.
I don’t understand, really, I used 0201 footprints and I ordered 0201 components for the assembly, I used KiCad for the design and I sent KiCad files to the manufacturer. Do 0201 footprints have pads that are too big for 0201 components? What should I do? Should I pay up the 300 EUR and get my boards reworked, should I refuse and ask for refund? Is it my fault? Is it their fault? I’m fine with sharing my PCB design here if it helps. I really need advice on this, I’m a beginner in this field and I’m feeling miserable at the moment.
what usually causes tombstoning is imbalance in “thermal impedance” between both pads. Be it a large plane on one side or large track on the other… Such things draw heat away unevenly and thus one pad will become “wet” before the other and surface tension will cause tombstoning.
what 0201 pads did you use as there are two variants
R_0201_0602Metric
R_0201_0603Metric_Pad064x040mm_HandSolder
if you use #2 and also had imbalances in traces to either pad this could cause it
As to whether €300 is worth it… is it how many cards, how much did you already spend? can you work with 0201? they might be banking on you not being able to work with 0201.
How many tombstoned parts? any pictures? if you have pictures could you post and also provide a screenshot of the associated pcb design
I used R_0201_0602Metric, I hand soldered them before ordering the assembly and then decided to order SMT. I’ve paid 870 EUR for the assembly, and I’m fine with paying an extra 300 EUR, I just want to make sure it’s me who made a mistake and not them just asking for more money.
Unfortunately they didn’t send my any pictures and didn’t share any details about the tombstoning. This is my PCB:
Holy smokes. 0402s are a real challenge for hand soldering, and I did not know that anyone could hand solder 0201s. I have not tried because even the 0402s often get lost in the drop of solder on the tip of the iron.
Thanks for explaining that. I would guess that the smaller sizes are generally worse for tombstoning (??). Is ROHS compliant solder worse than leaded solder?
Not using thermal relief may be the cause here, if the solder on one pad liquifies earlier it can “pull up” the component by surface tension. You should absolutely insist on pictures.
I’d say this one may be the most at-risk of a temperature difference at reflow:
Exactly, looking over the layout, there are quite a few resistors who have pads on copper zones and then tracks on the other - the component would tombstone and pivot on the pad with the track.
Unfortunately, I would say DFM oversight compounded this
Smaller is definitely more prone due to lower mass. I am not to sure about SAC306 vs 60/40 and I would rather not find out
May I ask why did you used 0201 instead of 0402? I don’t see any benefit from 0201. They don’t save much space when the track width and via diameter are “largish”; even one via takes more space than a 0201 pad.
I have not checked the design but I imagine an 0201 chip standing on end and fitting inside the PTH. I recently worked on a design which included some 0201s. I made every effort to avoid those. I am the elephant who does not want to step on a mouse.
Do you mean that a resistor is vertically (assuming the board lays horizontally) between the top and bottom layers in a NPTH? It’s possible but painful to solder. I don’t know if there’s any technique which can guarantee some reasonable success rate without unpredictable amount of manual work. I have done it with 0402.
Yes. But not as an intentional assembly; just as something that could happen. Of course the 0201 chip is much shorter than the common 1.6 mm pcb thickness.
EDIT: Whether the hole is plated or not is not my point. Obviously there is less space in a PTH/via.
Smaller footprints are more difficult to handle and process parameters must be optimized for good yields.
One of the thumb rules is that the amount of copper, (and the direction of tracks) must be balanced for these small components. If one of the pads has one copper track leaving it, and the other pad has two tracks, then this can already cause a difference in the way the pads heat, and this leads to tombstoning.
If one pad heats quicker, then the solder melts earlier on that pad, and the bigger the difference between the pads, the more time there is for tomb stoning to occur. If you look carefully at youtube (or similar) of SMT reflow, then you can see the flux doing it’s work when the solder melts and the solder gradually adheres to more of the pad and the footprint. And more adherence equals more pull from the solder. And if this happens on one pad before the solder on the other pad melts, you get tomb stoning.
Your PCB has not taken factors like this into account, and it’s neither of the manufacturer, nor of KiCad’s library. If you are able to rework the 0201 (Imperial or metric?) components yourself then it will be interesting to make notes of which footprints are most likely to tombstone, and which solder reliable
Heat dissipation isn’t the only thing affected by asymmetrical connections. The value of mask clearance is an absolute value unless you use solder mask defined. The smaller the component the larger the clearance relative to the pad. So, if one pad is on a copper fill with solid connection, it will be effectually x percentage larger than the other pad (calculate yourself). The same with thick traces. Asymmetric trace connections – even if the amount of copper is the same but traces go to different directions – affect smaller components more.
This may be the reason for the errors because “They claim I chose too big pads for the too small components”. Maybe you didn’t choose the pad size, maybe it came with the mask clearance.
0201 is useful if space is at premium and the traces and vias can be smaller, too. The normal ~0.17 mm / 0.6 mm trace/via of cheap manufacturing isn’t small enough, they are often more critical for saving space than moving to 0201 from 0402.
I still mainly use 9603 as i like resistors to be marked. 0402 and smaller are anonymous.
On my boards smaller vias of 0.6/0.3 save far more space than the KiCad default of 0.8/0.4. I have used 0402 components copying a reference design, but find that the courtyards don’t shrink as quickly as the part itself.
I agree with comments above that the lack of thermal relief to zones is the root cause on this board
I have another similar but more complex project with a lot more components and I couldn’t use 0402 components there (too little space), this one is a stripped down version of that and I didn’t touch the footprints when I cloned it (probably a mistake). For this other project I had to use 0.090mm traces.
Thanks for everyone’s valuable comments and suggestions, you helped me learn a lot! This is the first board I’ve ever designed and I considered it a miracle that it actually worked on the first try (I’m a software developer and I have about zero electronics background), I knew it must have a lot of design issues and plenty of bad practices, but it’s always fun to learn. I applied your suggestions to my new design and I’m going to order new PCBs to try them out. Thanks again for your help and suggestions!
It’s no a mistake, it’s a feature.
If you’re willing to work with 0201 (I’m not) then starting with some small / simple and relatively cheap PCB’s is a good way to get some experience with it and fine tune the PCB for manufacturing.
bingo the 1st PCB I pushed out with Kicad with ridiculously trivial and it was more to guage what was needed to produce something in Kicad (until then I had used kicad as a space claimer to influence bigger designs)
how many cards, how much did you already spend? can you work with 0201? they might be banking on you not being able to work with 0201.
