How to minimise trace fracturing in PCB design - multiple thin traces or one thick?

Question

Designing a board with strict and inconvienient requirements. Currently the boards are breaking frequently - the aim is simply to reduce this frequency as much as possible.. The board is a 100mm square but only supported with standoffs in each corner.

On the board are 20 throughhole 4 pin sensors. Effectively they are analogous to DIP switches.

The PCB experiences a lot of vibration as well as intermittent force (perhaps up to 100N point load) randomly, suddenly applied on a random sensor. Board is FR4 1.6mm. The environment is also humid and moderately corrosive.

I would love to redesign/support the board etc etc to be supported better, not loaded heavily, with a backing plate etc - but this is not an option.

Unsurprisingly, the board traces breaks frequently under this flexing. This generally causes unreliable performance. Electronically the board is simple slow digital signals so noise etc is not a concern.

I'm unsure as to how best to prevent/mitigate the traces breaking. I could either route multiple narrow traces for the same signal, thus my thinking being that stress is more likely to break one and the crack not propagate through to the others, or one wide trace.

I'm also thinking curved traces might be worth a thought and I'm interested in how best to connect the trace to throughhole connection to minimise risk of fracture. Also interested in if using extensive ground planes may help and if the most critical traces should be routed on top or bottom of PCB - so that they are either predominantly in compression (top) or tension (bottom). I have read around flexible PCB design but not got much conclusive information and am unsure if a rigid PCB that flexes is a significantly different case.

Thanks

Answer 1

Tricks we have used with some success: Make your feedthru holes big enough to insert a small piece of bus wire and solder top and bottom. Also solder top and bottom on your sensors if possible. We have seen lots of breakage between traces and the plated through holes and this is pretty effective, especially if you use 2-sided boards. Multi-layer boards are prone to cracking between trace and plating on the plated through hole, so stick with two-sided if you can.

If you must use multi-layer, be sure and watch the heat on your joints. Overheating can stress the joint because the board material expands at a different rate than the copper. The idea is to prevent cracking at the outset.

Trim component leads before you solder; Trimming them afterwards can stress and start a crack which will propagate.

No sharp corners on the traces. Cracking often begins on the corner where a trace runs into a pad outer radius. Fan out the trace to where it matches the pad tangentially.

For long parts like through hole resistors, mount them parallel to the expected flexure so that the leads are not getting stretched and compressed.

If you have leaded parts that mount flush, leave some space so that they are not sitting directly on the board.

Of course, you are probably already mounting your heaviest parts nearest to the mounting holes where they have the most support.

Good luck!

Answer 2

Answers to questions:

Compression vs. Tension

This is only applicable when there is continuous flex on a board. In your case, you describe a strong, intermittent force. When that force begins, your board will flex one way. When the force ends, your board will not immediately come back to its original shape, it will release the stored energy and flex back in the opposite direction before the oscillations damp down. So any trace you have on the board will both compress and stretch.

Meanders

When stretching, the copper will be deformed but is largely fixed to the rigid FR4. This limits the benefit achieved by meandering traces over the board.

Suggestions:

Component placement

The amount of flex will be directly proportional to the torque on your board. This is minimized by moving the components as close to the supporting struts as possible. Try to keep things away from the middle of the board. I would also remove as much copper from the middle of the board as possible.

Wiring

We used to call them printed wiring boards. :) In your case, it might make sense to go back to jumper wires. Rather than having copper traces affixed to the board and likely to break, you could solder jumper wires across the board for signal lines.

Power should still be provided using power planes but your signal lines could be soldered between through-holes located close to the edge of the board and close to the component lines. These wires should be tacked down using a glue in the middle of the line. Usually you would tack them every 1" but with your scenario, one tack in the center will reduce the stress on the solder points. Pick the thinnest wire you can get away with for your signal.

Answer 3

There are several things you can do. Apply as many of these as you can:

• Thicker PCB. Your boardhouse should have several options.
• Heavier copper. Instead of 1oz. go for 2oz. or 3oz.
• Wider traces
• Larger annular rings around through holes
• Add space between components and the board.
• Place something behind components that take force. Non-conductive foam, for example.

Answer 4

I would love to redesign/support the board etc etc to be supported better, not loaded heavily, with a backing plate etc - but this is not an option.

Ideally you would add additional supports in the middle of the card. Equally you would want the high mass components near the edge of the card.

However... you have stated a redesign is not an option. This means options like

1. Thicker PCB ( I only use 3mm thick cards in the environment I work in, high Vib)
2. Thicker tracks
3. Heavier weight copper

ie all the things to stiffen the card, are not possible

If these are not possible the only real option is the equivalent of Anti-Vibration mounting on whatever you screw the board downto. Can you place rubber washers down to help mechanically isolate the card?