Placing 0603 or 0402 between TH connector pins.

[Psi]

I need to put passives between some connector pins on the underside of the PCB. Pitch is X 3mm Y 4mm.
Currently they're 0603 but I could drop them all down to 0402 to get more clearance to the through hole pads.
I changed one to 0402 in the image just to get a better idea of size.
It's pretty much avoiding accidental bridges between the components and connector pins when soldering verses general increased reliability of 0602 over 0402 due to size.
The PCB will be assembled by PCBA service.

What's your opinion?

[Someone]

A customer accessible/functional connector will have massive forces compared to what a skilled assembler or tech would do. I wouldn't put any ceramics within several mm.

[Psi]

A customer accessible/functional connector will have massive forces compared to what a skilled assembler or tech would do. I wouldn't put any ceramics within several mm.

It will be installed once and left, so I'm not worried about connector insert/remove stress.
The pins are all a solid part of a plastic connector assembly, so don't expect much bending twisting between pins.
This is a very small product, basically just a connector and PCB of the same size.

[PGPG]

The PCB will be assembled by PCBA service.

Your pads (specially for 0402) looks for me being too long. My 0402 footprint (used since 15+ years) has 1.4mm distance between pad further ends.
I was told years ago that too long pads can shift element on one of them and then make it stand-up. Specially if it is soldered by being shifted through hot curtain and it enters it lengthwise, which makes the tin on one pad liquefy faster. Maybe all such problems are long gone...

[Psi]

The PCB will be assembled by PCBA service.

Your pads (specially for 0402) looks for me being too long. My 0402 footprint (used since 15+ years) has 1.4mm distance between pad further ends.
I was told years ago that too long pads can shift element on one of them and then make it stand-up. Specially if it is soldered by being shifted through hot curtain and it enters it lengthwise, which makes the tin on one pad liquefy faster. Maybe all such problems are long gone...

Thanks I will double check the IPC size for 0402 and check that footprint. It was a random 0402 I had in the library, so it could be wrong.

[wraper]

A customer accessible/functional connector will have massive forces compared to what a skilled assembler or tech would do. I wouldn't put any ceramics within several mm.

It does not even need to be functional. Simple presence of that connector will create quite a bit of stress. Simply look on some PCBs with longer 2 row pin header at the edge, especially with a thinner substrate. PCB will be warped to some extent. Raspberry Pi is a good example, every single one I've seen was warped. This is a very bad idea even without considering assembly. Look how the side with no header connector is completely straight.

[Psi]

A customer accessible/functional connector will have massive forces compared to what a skilled assembler or tech would do. I wouldn't put any ceramics within several mm.

It does not even need to be functional. Simple presence of that connector will create quite a bit of stress. Simply look on some PCBs with longer 2 row pin header at the edge, especially with a thinner substrate. PCB will be warped to some extent. Raspberry Pi is a good example, every single one I've seen was warped. This is a very bad idea even without considering assembly.

The pitch between pads is 4mm. There's plenty of room in there.
But your warnings are accepted.

But what's more risky here, 0402 or 0603.  That is the question.

I can make the PCB thicker if needed to reduce bending, 2.4mm etc. But i really dont think this will be an issue.

[Psi]

wraper, That's a pretty thin PCB .  Is that 1mm or 0.8mm

This is pretty small PCB 38mm x 36mm and a large amount of it is the 4mm pitch connector in the middle of the PCB taking up 1/2 the PCB area. It's so small/solid I just cant see it bending/flexing in the connector area.

[booscrawl]

Might be a problem for wave soldering.

[Jeroen3]

This will be difficult to solder by selective or wave.
This will also add additional challenge to manual soldering possibly getting higher defect rate.

Avoid if possible.

[JPortici]

A customer accessible/functional connector will have massive forces compared to what a skilled assembler or tech would do. I wouldn't put any ceramics within several mm.

It will be installed once and left, so I'm not worried about connector insert/remove stress.
The pins are all a solid part of a plastic connector assembly, so don't expect much bending twisting between pins.
This is a very small product, basically just a connector and PCB of the same size.

i've seen this done on some ECUs. Under the connector they would place hundreds of passives for input noise filtering

[wraper]

wraper, That's a pretty thin PCB .  Is that 1mm or 0.8mm

This is pretty small PCB 38mm x 36mm and a large amount of it is the 4mm pitch connector in the middle of the PCB taking up 1/2 the PCB area. It's so small/solid I just cant see it bending/flexing in the connector area.

1.2mm

[thm_w]

But what's more risky here, 0402 or 0603.  That is the question.

Larger is riskier, more displacement across its body, specifically for caps, less for resistors.

https://www.digikey.com/Site/Global/Layouts/DownloadPdf.ashx?pdfUrl=48437FD6C5394475AFC63F2AB6F3E378
https://www.mouser.com/pdfDocs/TechTopic-FlexCrackMitigation.pdf
https://product.tdk.com/en/techlibrary/solutionguide/mlcc_flex-crack.html

[Doctorandus_P]

Apart from (insertion / long connector bending) stresses. there is also manufacturability. And that depends on the way the PCB is going to be manufactured. To be sure, it is probably better to ask your manufacturer

[jovelyngentallan02]

The package size is probably not the main issue here .... the assembly process is. If the SMD parts are reflowed first and the connector is subsequently hand- or selectively soldered, 0603 should be practical at a 4 mm pitch, provided there is adequate solder-mask clearance between the pads.

If the connector will be wave soldered, however, bottom-side components between its pins could create bridging, shadowing or component-retention problems. PCBWay’s compact PCB layout guide similarly recommends maintaining manufacturable solder-mask dams and sufficient pad spacing to improve assembly yield.

Between the two sizes, I would retain 0603 for resistors unless clearance requires otherwise. For ceramic capacitors, 0402 has less body length over which PCB strain can act, although placing any MLCC near a large connector still presents some flex-cracking risk. Soft-termination capacitors may be worth considering if reliability is critical.

The best approach is to send the proposed layout to the PCBA supplier and ask which soldering process they will use and whether the clearances pass their DFM review. If they approve the 0603 layout, I see little advantage in changing everything to 0402.

[Psi]

Thanks, i think i will stick with 0603 and see how things go.

[asmi]

I learnt the hard way - no ceramic caps anywhere near parts of PCB where user-accessible connectors or buttons are located. Those caps LOVE to fail to short, and then good luck figuring out which one of 50 caps between a rail and ground failed. Resistors typically fail to open circuit, which is usually less dangerous. As for size, in my experience larger size caps fail more often than 0402 or 0201 (never seen that one fail). I suspect the reason is that larger caps have larger distance between terminals and so require smaller bend to fail.

[booscrawl]

Those caps LOVE to fail to short

Even X7R? Even AEC-Q100? Even X2/Y2?

[free_electron]

Those caps LOVE to fail to short

Even X7R? Even AEC-Q100? Even X2/Y2?

oh yeah ... for anything safety critical you need to use floating electrode caps. in automotive : any unprotected rail (not current limited) needs to exclusively use floating electrode caps. (this is not the same as soft-termination on the package !. floating electrode caps use a third plate internally that is not electrically connected. https://www.digikey.com/en/product-highlight/k/kemet/high-volt-floating-electrode-mlcc-cap

they are also called "series element capacitors) . kind of dpeends ont he manufacturer, but all the big boys make em.

Ceramic caps cannot be placed anywhere in regions that qill experience board flex ( like connectors or board edges ). Depanelisation of pcb's is the be done exclusvely using route and retain tabs and endmill cutten. absolutely no v-score or mouse bites in automotive !. Not only board stress is a problem with mousebites but also local delamination risk that can be a point for moisture ingress and dendrite or CAF growth. Board need to have guard rings on all layers to block that.

[free_electron]

Thanks, i think i will stick with 0603 and see how things go.

you'll have to glue them . wave soldering would dislodge them.

and you can't do selective wave like a drag-wave or fountain if you have parts there. they need a clearance of 2.5 to 3mm around the pin for the nozzle.
 
fountain : https://kurtzersa.com/products/electronics-production/soldering-machines/selective-systems
drag wave : https://packaged-media.redd.it/cvu4tr3bs1dd1/pb/m2-res_1280p.mp4?m=DASHPlaylist.mpd&var=sgpssan&v=1&e=1787612400&s=a6eba2499786576a7b1589c2abff6116f0a27356

[booscrawl]

There are flat-ish plastic shrouds some fab houses build to cover SMT parts that have to go through the wave. Either Teflon or some other high-temperature plastic is used. I forget the term at present.

[free_electron]

There are flat-ish plastic shrouds some fab houses build to cover SMT parts that have to go through the wave. Either Teflon or some other high-temperature plastic is used. I forget the term at present.

That's called a pallet , but that requires minimum 5mm clearance. They need space on the underside so the wave can touch properly. The surface tension of the wave prevents it from reaching anything closer than that. And you still need to glue parts. gluiing anything below 0805 is tricky . The glue dispenser simply can't make small enough dots. 0603 requires specialistic nozzles. It also requires an additional curing step. Not many assemblers offer this.
Sending SMT devices through a wave also requires careful attention to the direction of travel in the wave and the orientation of the parts to prevent shadowing (starvation of solder) and bridging (when the wave breaks contact with the pad) . you will have to adapt your footprints ( typically elongating the pads and widening any exit pad. for example on an So8 package the two pins where the wave exits need to be widened to trap excess solder as the wave breaks contact )



you can see the first and last pads have been widened on the ics to catch the wave entry and exits and prevent blobbing . all the passives use the same orientation to prevent shadowing and let the wave bind properly .

this stuff requires careful planning.

[nctnico]

I need to put passives between some connector pins on the underside of the PCB. Pitch is X 3mm Y 4mm.
Currently they're 0603 but I could drop them all down to 0402 to get more clearance to the through hole pads.
I changed one to 0402 in the image just to get a better idea of size.
It's pretty much avoiding accidental bridges between the components and connector pins when soldering verses general increased reliability of 0602 over 0402 due to size.
The PCB will be assembled by PCBA service.

What's your opinion?

I would place these components away from the connector. The reason is accessibility for selective or manual soldering.

[Accu-Sembly]

As an assembler, I would risk selective soldering the connector at the 0402 size, but I probably would charge for manual soldering or masking with the 0603.

That said, the best option for me is not to have parts between the pins at all.

[Psi]

As an assembler, I would risk selective soldering the connector at the 0402 size, but I probably would charge for manual soldering or masking with the 0603.

That said, the best option for me is not to have parts between the pins at all.

Thanks.
Paying extra for manual soldering might actually be ok if it's the only way.

I learnt the hard way - no ceramic caps anywhere near parts of PCB where user-accessible connectors or buttons are located. Those caps LOVE to fail to short, and then good luck figuring out which one of 50 caps between a rail and ground failed. Resistors typically fail to open circuit, which is usually less dangerous. As for size, in my experience larger size caps fail more often than 0402 or 0201 (never seen that one fail). I suspect the reason is that larger caps have larger distance between terminals and so require smaller bend to fail.

Most of them are resistors but if I can move the caps away from that area I will. Just for peace of mind.
In my limited experience of caps failing due to board flex it has always been caps that have a large capacitance for their physical size.
Like 0603 22uF 25V   or 0402 10uF 10V.  Whenever the layer thickness is being pushed to the thinnest possible to fit the capacity within the package.
I guess when the layers are super thin the risk of a short between layers is way higher.