Double-sided assembly

[asmi]

Hi guys,

I've just received my very first 4-layer board which contains components on both sides:




So I'm wondering how shall I go about assembling it. I have reflow oven (T-962 with some modifications to make it to actually do what it's supposed to), so I see three options:
1. First assemble front side with lead-free paste (because BGA balls are made from it), then assemble back side using regular leaded paste - this will allow reflowing at lower temperatures so it makes sure that LF solder stays solid and holds top components in place. But top side contains some plastic parts (mainly I'm concerned with connectors) so I'd rather not heat them up second time if I can help it.
2. Assemble both sides with LF paste. First is to assemble the back side, then - front side, hoping that surface tension of molten solder with hold parts on the bottom in place. Not sure if it will actually happen though.
3. First assemble back side using LF paste, then - top one but using leaded paste. Again, same idea as #1 - leaded paste reflows at lower temperatures, so it ensures bottom components will stay in place. The concern here is that BGA balls are made from LF solder, so they obviously won't melt, and the question is would leaded solder-to-LF solder bond be good enough to provide good electrical as well as mechanical connection.

Please post any thoughts on this - I will be assembling the board on the next weekend, so I have enough time to discuss all options, pick the best one and plan this whole thing. The board contains over 200 parts in total, most of which are 0402 capacitors and resistors, so it's going to be an interesting endeavor in and of itself - the most complicated boards I've assembled so far contained just about 60 parts
Thanks for your time reading this wall of text, and I'm looking forward to hear your thoughts on this.

[Grayfox]

I am a nub and have no experience with SMD soldering.

But I would use the oven for the top layer since it has the most parts then wrap the PCB in some foil and make a small cutout where the bottom parts are and then use a heat gun.
I reflowed a Fat PS3s CPU using this method to get it working, might work in this case, but might not be safe.

[Ian.M]

I see you've only got ceramic bodied passives on the bottom.  They'll tolerate two reflow passes without any issues.  Use thermal curing epoxy sold for SMD assembly. That way, all potentially heat sensitive parts only get one reflow pass and you can use the same solder paste both sides.

After silk-screening the paste, dot the center of all the bottom footprints with the glue before placing the parts, reflow normally,  assemble the top side normally without any glue, (though the DC jack, USB connector, JTAG header and expansion ports could probably benefit from a couple of dots each if you want to reinforce them), and reflow again supported by the corner holes (which could be as simple as a screw & nut through each), so there isn't anything pressing on the bottom components.  Some of the bottom passives are probably too small to easily glue-dot, but surface tension will hold those in place during the second reflow as long as nothing's touching them.

If you don't have a syringe driver, the glue's probably a bit to viscous to be able to dot with easily even through a cut-down large bore needle, so squeeze a small blob out onto a watch-glass or similar and use a toothpick.

Plan B (without glue):
Do all the 'fly-speck' sized passives on the bottom by normal reflow, do the top normally, relying on surface tension to keep the bottom passives in place then hand-solder the remaining larger bottom passives.

[rs20]

I happened to come across the pictures of your finished board on another thread -- very impressive indeed! Well done!

Is there any chance you could please share the KiCad and/or gerber files for it? I'm sure I (and maybe others) could learn a lot by seeing some of the approaches you used to deal with such high pin-count parts and BGA routing.

[asmi]

Sure - you can download KiCAD project with gerbers, as well as assembly PDF file here. This PDF has been generated by Python script from pick-and-place file and gerbers, and helped a lot during assembly.
Routing this was actually kind of fun - you have to think ahead to make sure you don't block yourself before all pins are broken out. Kinda like playing chess As you can see, this is a second revision of the board, as I made a number of mistakes in the first one (good thing I've discovered them before I've started assembly - so I only wasted money on PCB). The technique I came up with is to create a package pinout diagram in Excel, and mark pins as I route them so that I always knew which pins are already in use - with FPGAs you have a great deal of flexibility when it comes to pinout in a sense that you can reassign pins to fuctions in order to facilitate routing, but you have to watch out for the fact that different I/O banks can (and do in my case) have different logic voltage levels, as well as dedicated pins with fixed functions (power/ground, JTAG, configuration, etc.). I also didn't want to go with 6 layers as they are much more expensive to manufacture, which is why I had to settle on some compromises - not breaking out all FPGA balls, putting few signal traces on the power layer as well as having some "jumper-traces" on the top layer under BGA (which is not a recommended practice, but I had no choice). Desperately waiting for new Spartan-7 chips to become available, as they come in FBGA-196 package specifically designed to be broken out on 4 layer boards.
In general, routing big BGAs may seem intimidating at first, but once you get into the routine so to speak, it's not that hard. Just think ahead, break out inner balls first (to lessen the chance of cornering yourself), break out whatever component traces are going to first so that you will know in which order traces need to come from FPGA, then break out FPGA balls you want to connect them to making sure that the "bus" have same traces order as component you're connecting them to, and then connect them adjusting trace width if you need it (for example for controlled-impedance traces, or power lines which need to be thicker). Also since these boards cost non-trivial amount of money to manufacture, don't rush it, check, double-check and triple-check all packages' pinouts (unless you used them before and know for sure they are correct, I've messed this up more times than I'm willing to confess ), if you need traces with controlled impedance (as I do here for HyperRAM chips) - make sure you reach out to the fab you going to use to find out the layers stackup so that you can calculate traces' width from that information. Do backups often and be prepared to go few versions back it case you realize that you've cornered yourself (and trust me, you will do that few times until you get some experience). Use 3D view to check that there is enough clearance between components (especially connectors as they tend to have parts of them protruding beyond the footprint), also think about how you're going to assemble the board when you decide where to place components on the board, place noisy magnetics and power parts away from sensitive analog and high-speed traces. Another thing - even though KiCAD's DRC is a royal pain in the behind in KiCAD, make sure you run it and fix all errors which are actual errors (it often issues false alarms like complaining that package pins are too close to each other - nothin' you can do about that!, or some other nonsense like that), also this DRC tool seem to ignore copper pour-to-pour clearances so make sure you manually check that.

And since this thread is about assembly, I ended up using leaded paste for both sides. Assembled bottom side first, then used some bolts and nuts to make standoffs so that I can assemble top side. During top side reflow even big 1210 components stayed in place just fine, not to mention smaller parts. I've purchased a very affordable stereo microscope from AmScope (SE-410-XYZ, $200+S/H, here), also excellent (even if quite expensive, but it was totally worth it) vacuum pickup tool with set of tips for small components from Zephyrtronics ($493 for the tool and tips + S/H, here), and I was reflowing in cheap Chinese T-962 oven (with some minor hardware "upgrades" and community firmware). These tools made assembly a breeze, and I hope will serve me well in the future projects.

[suicidaleggroll]

FWIW - I have designed/assembled many boards like this, and I typically use paste on the top with an oven/hot plate, and then just manually solder the components on the bottom.  You don't have a lot of components on the bottom, and chances are many of them are the same value since they're decoupling the FPGA power lines, so it would probably take less time to do this than to paste, place, flow a second time for the bottom components.

[asmi]

Quote from: suicidaleggroll on Today at 12:34:23 AM

FWIW - I have designed/assembled many boards like this, and I typically use paste on the top with an oven/hot plate, and then just manually solder the components on the bottom.  You don't have a lot of components on the bottom, and chances are many of them are the same value since they're decoupling the FPGA power lines, so it would probably take less time to do this than to paste, place, flow a second time for the bottom components.

I tried that with one of boards (since I got 11 of them anyway), and manual soldering ~50 0402 capacitors & resistors took over 3 hrs under stereo microscope, while placing & reflowing took about 45 minutes. Also manual soldering was very annoying because some of 0402's were so close that I couldn't touch one part with iron without touching adjacent part.
So for anything more than a few parts I would strongly advise reflowing. And the result IMHO looks much more "professional" and more aesthetically pleasing Also I ordered stencil with both sides on the same sheet of steel (this is a no-cost option in all fabs I ever used), and then just cut it in half with scissors. I 3D printed a little holders to make putting on solder paste easier:

(This photo shows first revision of the board which turned out to be unusable due many mistakes I made in layout).

[suicidaleggroll]

I tried that with one of boards (since I got 11 of them anyway), and manual soldering ~50 0402 capacitors & resistors took over 3 hrs under stereo microscope

That's over 3.5 minutes PER passive, that's an insanely long amount of time.  You should be able to do it in <20 seconds each, which would bring the total time to around 15 minutes.  3 hours is crazy for less than 50 passives (I only count ~33 0402s), I can't even comprehend how it would take that long with a stereo microscope.

You should be doing it in 3 phases.
1) Go through and tin one pad per passive on the board, for all footprints.  This should take <2 seconds per part.
2) Under the microscope, grab a component with tweezers, hold it in place, and tap the pre-tinned pad to reflow it and tack the part in place, do this for all parts.  This should take <15 seconds per part.
3) Under the microscope, go back through with solder and the iron and solder the second half of each component.  This should take <5 seconds per part.

If every one of your components was a different part number, that would increase the time quite a bit, but still nowhere near 4 minutes each.  Since they're all decoupling the FPGA power lines I imagine you only have 5-6 different part numbers for your ~33 0402s though.

I recently assembled a batch of boards this way.  They each have over 220 SMD parts on the bottom (109 0402s), and it only took a bit over an hour per board.

[mikeselectricstuff]

Do the side with the small stuff first, no need for glue dots - the surface tension of the solder will hold them on during the second pass.
 

[asmi]

That's over 3.5 minutes PER passive, that's an insanely long amount of time.  You should be able to do it in <20 seconds each, which would bring the total time to around 15 minutes.  3 hours is crazy for less than 50 passives (I only count ~33 0402s), I can't even comprehend how it would take that long with a stereo microscope.

You should be doing it in 3 phases.
1) Go through and tin one pad per passive on the board, for all footprints.  This should take <2 seconds per part.
2) Under the microscope, grab a component with tweezers, hold it in place, and tap the pre-tinned pad to reflow it and tack the part in place, do this for all parts.  This should take <15 seconds per part.
3) Under the microscope, go back through with solder and the iron and solder the second half of each component.  This should take <5 seconds per part.

If every one of your components was a different part number, that would increase the time quite a bit, but still nowhere near 4 minutes each.  Since they're all decoupling the FPGA power lines I imagine you only have 5-6 different part numbers for your ~33 0402s though.

I recently assembled a batch of boards this way.  They each have over 220 SMD parts on the bottom (109 0402s), and it only took a bit over an hour per board.

Wow! I'm just not that good at this I guess maybe in the future I will become...
One big problem with 0402 parts for me is that microscope's field of view is not very large, so I only see a portion of the board, so I grab parts from the tape that is on the side outside of microscope's FOV. I have pretty good vision so I can do that OK, but it takes time - especially if parts start flying away from bad grapple I'm think about 3D printing some kind of rail where I can insert the tape and this will make extracting parts easier, but now as I have a very good pickup tool, it's just easier to pick and place parts and reflow them (I can't use the tool to hold part for hand soldering as tip material is not heat-resistant, and these tips are $33 each).

[nanofrog]

Why not hold the part with a pair of tweezers after placement?

[asmi]

Why not hold the part with a pair of tweezers after placement?

Insufficient amount of hands I often wish I had three hands - one for iron, another one for pickup tool (to extract parts from the tape) and third one for tweezers As it is, switching tools all the time kills efficiency (which I don't really care about as it's a hobby project) and is just annoying (this is a big problem because I don't have angry client shouting in my ear so I have to maintain motivation)
Things are different when you do stuff just for fun.

[nanofrog]

Insufficient amount of hands I often wish I had three hands - one for iron, another one for pickup tool (to extract parts from the tape) and third one for tweezers As it is, switching tools all the time kills efficiency (which I don't really care about as it's a hobby project) and is just annoying (this is a big problem because I don't have angry client shouting in my ear so I have to maintain motivation)
Things are different when you do stuff just for fun.

There's some clever DIY solutions for that. 

Segmented CNC hose makes excellent 3rd hands.  Loc-Line will yield better search results (photo examples), but there's notably less expensive equivalents from China that will do the job quite well from eBay and the like. There's posts on this here in the forum as well, and worth exploring IMHO. 

Here's one photo example:



BTW it's possible to attach other tools, such as clamps, tweezers, and hemostats. I found regular inexpensive 3rd hand devices are great for cannibalizing parts; namely the segmented joints as they make great tool holders that allow you to change them as needed (hacksaw & epoxy are your friends to attach the joints to the CNC hose).

Here's another idea (particularly if the board is lying flat on the bench):



With a little modification, this basic idea makes a great probe holder too. 

[mikeselectricstuff]

So for anything more than a few parts I would strongly advise reflowing. And the result IMHO looks much more "professional" and more aesthetically pleasing

+1
It also allows much faster placement, using a foot-operated vacuum pen - much quicker than tweezers as you can pick parts direct from tape, and they will have a consistent orientation

[jmelson]

You don't need to do 2 different solders.  Practically all my boards have parts on both sides.  One of them even has a big regulator chip on the back.  I stencil, place and reflow the back side, then stencil, place and reflow the front.  The only trick is to make sure the whole board is below liquidus temperature before picking it up.  I've NEVER had a part fall off the back of the board, and I've done well over 1000 boards this way.

Jon