What are the ideal footprint values for handsoldering a 0.5pitch IC?

Hi! I’d like to optimize my footprint for a 0.5mm pitched IC, so that I can hand solder it.

My consideration is this …
pad width: 0.3mm
soldermask clearance: 0.00mm
soldermask bridge width: 0.2mm

what do you think?

I haven’t found special pad sizes are needed to hand-solder SMD components.

1 Like

Well, I essentially want to avoid solder bridges. I make the pads, longer, thinner, oval, move them further aways from the pins. But I would like to know how other people choose values for width of solder mask bridges and solder mask clearance to have the
best results.

To avoid solder bridges, get the right solder flux. I use 2331zx water-soluble flux and bridges seldom form and, when they do, they’re easily removed. Then wash the board with distilled water, dry it, and you’re done.

If you must play with the pads, the thing that’s mostly done is to extend them outward to make it easier to apply the soldering iron. This can be helpful with QFN packages but isn’t really needed for gull-wing packages.

In my experience, it’s worth the effort to adjust pad width, and the soldermask parameters, to get a sliver of soldermask between pads. Be careful that you stay within the design rules for the fab house that makes your boards, though. (I don’t know if many board fabricators will accept your 0.0mm clearance.) For the soldermask, some of them will adjust the parameters to meet their minimums and either not tell you, or send you a note after the boards are done saying that soldermask clearance was increased to 0.08mm (or whatever their standard is)

If you can truly hand-solder 0.5mm pitch, you have my greatest admiration!!

I tried doing 0.65mm entirely by hand (the LTC4011 in TSSOP-20) and it became a half-day project. I had better luck doing that package in my poor-man’s excuse for a reflow oven, and clearing out any bridges with a soldering iron and solder wick. (See Pad Holes Under SMT for Heat Sinking and other questions) After a little practice, if I laid down solder paste under a toolmaker’s microscope with a toothpick, I could reflow solder the TSSOP without any bridges.

But I am not brave enough to attempt 0.5mm pitch!

Dale

Hi devbisme! Yes, flux is necessary. But why not optimize the footprint to prevent
even better any solder bridges? To move the pads further outward is maybe
even for gull-wings an improvement, at least in that sense, that the pads
should better range from the base metal of the pin to the front, but not behind
the pins. Because if solder bridges happen, you can hardly see them if they
take place behind the pins.

You can adjust the pads however you like. I just have never seen the need. Solder flux prevents the issues you are trying to avoid. Even with no mask between the pins, I don’t get bridges (at least, not any that are hard to remove).

Also, I would never move pads outward so far that the pins don’t fully contact them. I have never, ever, ever had a solder bridge behind the pads.

And if you ever go to production, then you have to change all your hand-solderable footprints which means your routing may have to change. Who needs that mess?

And just so you don’t think I have super-duper equipment, I use a 1/16" or 1/8" iron tip, common 0.031" 63/37 leaded solder, 2331zx flux, and a 2.5x magnifying visor.

1 Like

Well, if you are hand soldering a 0.5 pitched IC with just an iron and 2.5x magnifier, then you have my admiration :-), a 2.5x magnifier is like nothing? I’m just an amateur, with poor technique. I get even solder bridges with solder mask between the pads. So I’m trying to compensate my lack of skills by footprint design (as I’d like to discuss here), and of course some tools (as an 60x microscope, gel flux, stencil, etc.). But my goal is to make it dummy proof, not only for me, but for other users too.

@dchisholm No I can hardly hand-solder it, that is why I write this thread :slight_smile:
As written, I use some tools, also a stencil. But that is not enough for me, I want the footprint as good as possible.
You wrote “a sliver of Solder Mask between the pads”. Yes of course I want that but the problem is,
there is a min. width of Solder Mask Bridges, and it is 0.1, which is still troublesome (0.1 may lift up),
so 0.2 is better. But there is hardly any room for 0.2 Solder Mask Finger on a 0.5mm pitched IC, if
Solder Mask Clearance isn’t shrinked down to the bare minimum. You say fabhouses may accept 0.00 and adjust the value to the minimum needs. Yes, I will try that.

If I understood you right, practically I may end up with something like this:
Pad width: 0.25mm
Solder Mask Clearance: ?.??mm (fabhouse adjusts it, maybe to 0.075mm)
Solder Mask Bridges: ?.?? (depending on Solder Mask Clearance maybe 0.1mm)

The pads + solder also anchor the device to the pcb board… by modifying the contact interface in that area you are in uncharted country and probably working against the intention of the original design there (which has been developed + tested by countless engineers).
If this is for hobby fine, for production… no way I would be signing of on that.

If you have problems with bridges during reflow you need to:

  • check the solderpaste you use
  • check the solder stencil thickness and area ratios
  • check your process

I have bridges sometimes too, but I know that I use crappy paste and that my stencil has got too big a holes in it for some of the footprints to work properly… but I’m sure with my 4th attempt I’ll be mostly fine.

Sometimes the device leads are not flat, a common problem when parts have been separated from their trays and wrapped in conductive foam.

Let’s take a concrete example. Here is my footprint of an 0.5mm pitched IC.
The pad width is 0.3mm which is the minimum value of my fabhouse.
As far as I understand it, my fabhouse has a minimum value for
solder mask clearance of 0.08mm. So, with these values
there is are no solder mask bridges possible anymore!
What to do?

Adjust the amount of solder flux via the paste stencil and don’t worry about not having solder mask on the pcb material between the pads?
The solder mask coating is there to not have copper suck away solder from the pads… you don’t really need it between pads. The solder will wet/cling to the copper and pins, not to the pcb material.

If you get/got bridges get better paste (=finer, better fluxes, fresh) and adjust the amount of paste disposed to be less by tinkering with the stencil design (paste ratio values, stencil thickness, squeegee movement, stencil positioning/moving, etc…)

1 Like

Im not so sure about that. Personally I have the worst experience without SMB (solder mask bridges)… and the best experiences with SMBs. So I want them even on a 0.5mm pitched IC :slight_smile: