Stencils, hand assembly versus PNP

[Simon]

I have made some boards recently and was a little dismayed at the amount of extra solder i managed to get on TQFP parts and the bridging I ended up with. I am also due to redo a design with VQFN on it where much trouble was had on the first version.

So other than pick the thinnest stencil how can I try to correct my over pasting in prototyping without affecting manufacture? I can obviously pick the thinnest stencil available which is usually 100µm versus the usual 120-127µm but that does not take much off.

If I go for reducing the apertures this will surely affect the PnP manufacturer. Do PnP assemblers make stencils based on the paste layer or do they just run their own figures on the pad sizes?

[Simon]

I guess I can have an additional layer on a footprint that is used as an alternate stencil?

[SiliconWizard]

Do I understand it right if I got that you mean you have excess solder when "hand assembling" the boards, which I further assume is done with solder paste/stencil and a reflow oven?

[Simon]

Correct.

[Simon]

For example the 64 pin 7x7mm TQFP in Kicad has stencil apertures the same size as the pad. I thought usually some clearance was given? what i can do is use the back solder past layer to set custom hand assembly apertures

[langwadt]

For example the 64 pin 7x7mm TQFP in Kicad has stencil apertures the same size as the pad. I thought usually some clearance was given? what i can do is use the back solder past layer to set custom hand assembly apertures

in the board setup you can globally set the solder paste clearance and ratio to make the stencil opening different from the pads

[SiliconWizard]

If you have experience with the footprints/solder mask you used, and they work well for automated assembly... AND if you only have to make a few prototypes by hand, I would personally not bother and do manual touch-up on the assembled proto boards instead of changing anything. Now if it's a significant number of boards to rework, that may be annoying, but doable. TQFP parts are not hard to touch-up. Even assembly plants do manual touch-ups on occasion on customer's boards, especially when the components on them are too expensive to just discard. It's not a shame to do it.

[Simon]

VQFN is a problem

[Pseudobyte]

4 mil stainless stencils are pretty standard and the goto for most operations. The unfortunate thing is that having the right stencil is only part of the solution. There is alot that goes into hand stenciling, and it isn't as simple as grab a credit card and smear some paste around as some people like to make it out to be.

The setup is everything.
need a rigid flat surface
need board stock the same thickness as your pcb to jig up your board
need the stencil to be supported very well along the edges of your pcb
need the stencil to be held taught and able to be adjusted in x,y https://www.pcbunlimited.com/products/prototype-stencil-printer?taxon_id=2
need a decent squeegee http://www.stencilsunlimited.com/aluminum-handle-with-90a-square-edge-squeegee-p-420.html

got to run ill explain more later

[SiliconWizard]

4 mil stainless stencils are pretty standard and the goto for most operations. The unfortunate thing is that having the right stencil is only part of the solution. There is alot that goes into hand stenciling,

Yup, I would suspect it to be the main problem. It's pretty hard to hand stencil properly for fine-pitch stuff if you don't have the right tools. The stencil should lie extremely flat against the PCB, which is always hard to do manually (I don't know what kind of tools the OP has though.)

[Simon]

I use a couple of PCB's either side of the one i am pasting selotaped down with the stencil taped down. And yes a credit card.

My point is that I accept that my process will be different from mass manufacture which is why i am trying to have two options. In any case I think the Kicad footprints should have some settings other than 100% paste. I can't set a global setting as some parts have such tiny pads that 100% is desirable really each part needs doing individually.

[Pseudobyte]

If I go for reducing the apertures this will surely affect the PnP manufacturer. Do PnP assemblers make stencils based on the paste layer or do they just run their own figures on the pad sizes?

Most CMs will use the data that you provide. They also may decide to tweak apertures. Common things are adding window panes to large pads, changing circular apertures on BGAs to squares circumscribed by the pad to prevent bridging.

In my experience working at a CM we have never modified the paste of a TQFP. The finer the pitch the more critical your pasting method and registration become.

Out of curiosity what ball size paste are you using, this also can be a large factor with fine pitch parts.

[Simon]

I can't remember the ball size but it's the smallest you can without trying too hard.

[Simon]

The stencil printers seem expensive. As I work for a company that can manufacture i could look at making my own. So essentially the stencil are pulled tight and pressed down on the PCB?

[asmi]

Of all packages I hate QFNs the most as despite my best efforts I still get a bridge every so often (especially with newer 0.4 mm pitch QFNs). I will take a reasonable-pitch BGA over QFN any time.
Things I've done to reduce changes of bridges in QFNs:
1. Use 0.1 mm electropolished stencils.
2. Use stencil printer that works with double-sized boards with proper steel squeegee. Credit cards are way too soft for paste printing.
3. Use framed stencils instead of frameless - this allows for a very tight fit to a board and reduces solder paste getting under the stencil.
4. Use PCB fab that reliably manufactures thin solder stops between pins.

Like I said, despite all of that I still get a bridge every so often, but they are much less often now than it used to be. The biggest difference was moving from frameless stencils and ad-hoc bodged-together holders to proper printer and framed stencils. It also made process much faster if I needed to process several boards/panels in a row - once you set things up for a board type, printing paste takes literally few seconds. The printer is ZB3040H, I got it on Aliexpress for about 580 CAD including shipping (shipping is expensive because it's heavy!), but it's totally worth it!

[Pseudobyte]

The stencil printers seem expensive. As I work for a company that can manufacture i could look at making my own. So essentially the stencil are pulled tight and pressed down on the PCB?

When you buy framed stencils that is the benefit you are paying for. They take a screen material and stretch it across a frame.

Some frameless stencil printers have the ability to put your foil stencil in tension which is also good.

The thing you are really trying to avoid is the stencil bending up, allowing paste to bleed together, deposit unevenly, or deposit too much paste. Paste bleed tends to show up after reflow as bridging or solder balls. Bridging is obviously a defect, solder balls are not great either and are considered a process indicator.

Think about how springy the steel foil is. Now imagine you placed that foil at the edge of a table. Now imagine you dragged a steel squeegee across the top surface of the table. You eventually start to deform the steel at the edge. In the photo below you can actually see the outline and features of the panel. This stencil has seen some action. This happens to all stencils but much faster in foil stencils that are not framed.

[jonroger]

You could use a solder paste that has less solder and more flux.

[T3sl4co1l]

Let me guess, every time you make a pass, spreading paste, it seems to disappear, so you come back to apply more and so on?

Yeah, it's slumping down, because the stencil isn't sitting flat.  And the result is a terribly blobby mess?

I did a few boards earlier this year, 6 boards, ~200 components/board, framed stencil, went pretty well.  First time doing it, and only one or two boards got pasted poorly.

Ordered a loose stencil for another board some months ago, turned out terrible.  Tried just laying the stencil on the board and going with it.  Nuh uh.  Useless without support.  Needs at least a support frame (the same height as the board being pasted).  Otherwise it ends up bowing up and making a mess.

Tim

[Simon]

Useless without support.  Needs at least a support frame (the same height as the board being pasted).  Otherwise it ends up bowing up and making a mess.

Tim

Yea I need to make something to tension the stencil and then hold the PCB in place.

[nctnico]

Of all packages I hate QFNs the most as despite my best efforts I still get a bridge every so often (especially with newer 0.4 mm pitch QFNs). I will take a reasonable-pitch BGA over QFN any time.
Things I've done to reduce changes of bridges in QFNs:
1. Use 0.1 mm electropolished stencils.
2. Use stencil printer that works with double-sized boards with proper steel squeegee. Credit cards are way too soft for paste printing.
3. Use framed stencils instead of frameless - this allows for a very tight fit to a board and reduces solder paste getting under the stencil.
4. Use PCB fab that reliably manufactures thin solder stops between pins.

Like I said, despite all of that I still get a bridge every so often, but they are much less often now than it used to be. The biggest difference was moving from frameless stencils and ad-hoc bodged-together holders to proper printer and framed stencils. It also made process much faster if I needed to process several boards/panels in a row - once you set things up for a board type, printing paste takes literally few seconds. The printer is ZB3040H, I got it on Aliexpress for about 580 CAD including shipping (shipping is expensive because it's heavy!), but it's totally worth it!

This starts to add up to a serious amount of money. Given time & cost it would make more sense to have an assembler deal with it.

About the fine pitch QFNs: one of the assemblers I work with has told me to keep a distance of at least .2mm between pads to avoid bridging. This likely means you need to change the footprint to have narrower pads but production wise it is better.