Hello, new poster here. I am relatively inexperienced. Hopefully this is the correct category. I am at my third iteration of a narrow and long PCB. 25mm x 200mm that contains several through hole push buttons and through hole rotary encoders. I have them manufactured by JCLPCB.
Space is at a premium on this narrow board (Isn’t it always) and I am forced to run traces (0.25mm) underneath the rotary encoders to make it all fit.
However, the metal backing of the encoders damages the solder mask after a while and cause short circuits. I fixed this problem by applying capton tape to the PCB before mounting the rotary encoders but this is labor intensive.
I have been reluctant to place the fine traces on the back of the board because I glue a plastic backing plate directly against the back of the PCB and this backing plate forms the device mounting surface. It seemed unwise to expose the fine traces to mechanical stresses through the glue bond.
Does anyone have a suggestion on how I can protect the traces from the rotary encoders or am I stuck with the capton tape?
Well, a 4-layer board will give you room to leave a top-layer keep-out or ground-plane area under the encoder, and the same flexibility on the bottom layer, with traces on the inside (also a low-emi/esd approach).
If the board cannot be changed, the kapton tape is a decent solution. I have even used peel-and-stick notepad reinforcing rings, or dots, from the office suppy store – no cutting of tape so much faster.
Alternately, solder the encoders on with an air gap – you could slip a temporary shim under the encoder before soldering the encoder pins. If you are looking at production volumes, a new pcb would be a good way to go.
Hello thanks for your reply. Of course! I completely failed to think of that option to have an extra layer. I am old enough to have drawn circuit boards by hand with a thick ink. The luxury of multiple layers is just insane to me. Double sided is already unbelievable.
Yes I definitely will go through another iteration and board design. With 4 layers I can also protect the much thicker GND traces on the back. Now it’s a matter of weighing cost versus spending time putting capton tape down and pricking all the though holes.
I am looking at production runs of several hundred so it’s worth doing it right.
If the component is through hole and it doesn’t matter if it’s raised a bit, you can add silkscreen ink under it. But 4 layers may indeed be better solution.
If you go to 4 layer. You should be able to use one layer for a full ground plane. So it won’t matter if it get scratched a little bit (as long as the external metal stuff doing the scratching can be connected to ground without any issue.
Also, if you have high current trace, the internal layer are not very good at dissipating heat, so they are not very good for high current trace.
Finally adding a big rectangle of silkscreen, is a way to add an extra layer of protection. It’s not very thick, but silkscreen+solder mask will be more resistant then just solder. And with JLCPCB for the same price you can have silkscreen on top and on bottom
Are these switches and encoders soldered by hand?
That would already be a fair amount of time.
Maybe by rotating the switches you could use a single piece of kapton tape over the PCB, or even consider a different brand of switch that does not have a metal backsidde.
Also, in these modern times, 0.25mm (250micrometer) wide tracks are not considered “fine traces” anymore, but quite generous for nearly any PCB manufacturer.
6/6mil (track/spacing) is considered quite standard and that translates to 153micrometer.
4/4mil can be the same price and is 102micron. Although in general it’s not recommended to go to the limit of what PCB manufacturers quote, but 180um for the 6/6mil and 120um for the 4/4mil process is quite reasonable.
4-layer PCB’s are often made on a production line with tighter tolerances, and 4/4mil may be standard. It’s not only the extra layers that make it more expensive, it’s also the inherent tighter tolerances used for the process.
For current handling capability it’s also no problem. A 100um wide track can already handle 450mA. In practice this means that the PCB manufacturing process dictates the limit for all PCB tracks except power distribution.
Also consider PCB quantity.
I am experimenting a bit with websites of european PCB manufacturers. They tend to be expensive for low quantities, but that is due to setup costs, which are not listed separately, but divided over the number of PCB’s ordered.
With Eurocircuits for example, you can have 1000 PCB’s of 25*200mm for EUR 1.7 each for a dual layer, and EUR2.65 each for a 4 layer.
Edit: For PCBway, it’s 75ct and about 1USD each for either two or 4 layer PCB’s respectively. So quantity does suppress costs per piece quite a lot.
You can also turn it around and put the kapton on the underside of the encoders.
If you put a tube vertically in a vice, then you can drop the axle of the encoder into the tube, put on some kapton, and cut it with scissors. That should be quite quick.
Or find other sticky things. For example the strengthening rings for paper in ring binders or other small stickers. Even if they fall of after years, there will still be a gap left with the thickness of the sticker.
One more idea:
Create a sticker. It has the shape of the board.
It has cutouts for the THT pins, and for SMD.
The THT cutouts are shaped similar to what @BlackCoffee showed, that is one cutout for a row of pins.
The sticker can have any color and design.
I have ordered thousends of stickers at wirmachendruck in germany. Good quality at low price.
You can chose from different material. I prefer 70 or 140mic laminated heavy duty outdoor.
I have not used them for the mentioned purpose, but maybe it it worth considering or giving it a try.
Requires hand soldering of course.
Flipping the board is a good idea! With the through hole solution I can indeed flip the board and have the ground side face the components. But this also means that the side with 0.25mm traces faces down. That side needs to be glued to a special back panel but I guess that is not that different from a 4 layered PCB.
Those are glued together too. Makes me wonder though if the glue holds better if I omit the solder mask.
That is a great idea but in my optimism I hope to make hundreds if not more of these things. I already found it difficult to align the Capton tape properly on the PCB
If I am forced down that route then I will 3D print make a jig with needles for all the holes so I can prick the tape in one go.
