Best way to design a PCB for frequent component switching?

Question

I'm getting a PCB made with an OpAmp circuit on it that will need some tuning. We aren't sure what resistance and capacitance values we'll need to use for the integrator circuit. These will need to be calculated, tried, tested and tuned after the PCB is made.

I know we will be changing those components out frequently until we get the response that we want.

Is there an easy and robust way to swap out these components as we iterate?

It is a wearable so for testing purposes the solution should be rigid and compact-ish. Right now I am thinking through hole components and just de-solder and solder different values. I was thinking of variable resistor but the values for this circuit could vary from 10kOhm - 10MOhm.
The frequencies carried by the resistors will be in the range of 500 – 1000 Hz.

Answer 1

Nothing directly to do with design, but specify a superior PCB laminate (typically high-Tg) and invest in good soldering tools, including a tweezer type de-soldering tool if you feel flush.

Avoid lead-free solder for your prototypes if you can and use only eutectic Sn63Pb37 solder. Don't spare the liquid flux and use gentle means of cleaning solder from pads such as high-quality fresh de-soldering braid.

Use fairly large SMT parts where possible (0805 is good) and, if your library has several options for pad size, pick the larger ones. Avoid really narrow traces where possible- they'll be more robust against a slipped tool.

Use 0Ω resistors, pull-ups or pull-downs instead of direct connections where you might conceivably want to access a pin or change the state of a line. Add test points and test connectors liberally to prototypes. Bringing out a 0/5V serial port connected to an MCU can be a tremendous time saver if your only other UI is a single blinking LED.

10 years ago I would have suggested socketing the op-amps but that’s of limited usefulness if you have insufficient space or can’t get the op-amps you want in THT.

Answer 2

If you have enough space, just use 3 potentiometers (or other variable resistances) : one 100k max, one 1M max, one 10M max in "parallel", with a jumper to select which potentimeter to use.

^{simulate this circuit – Schematic created using CircuitLab} (nb : I used switches because there are no jumper symbols in circuit lab).

Close one jumper depending on which range you want to experiment with. If you plan on changing frequently the range, you might use a selector instead of the 3 jumpers.

R0 is only needed if you need to make sure that the resistance is never smaller than 10k. If you don't care if by mistake the resistance is 0, then no need for R0.

If you want to know the value of the resistance, open the corresponding switch, and measure the resistance of R1 or R2 or R3 with the multi-meter (it is an open circuit now, so you can measure in circuit without disturbances)

Answer 3

For your prototype you can use a machined-contact DIP socket and 'fly-wire' it to your board to bring the components out.

This type of socket will accept 1/8W resistors and caps with 0.300" lead spacing. Through hole components will plug right in.

Come to think of it, it might make more sense to put the entire circuit (op-amp and passives) on a breadboard and hot-wire that to your target board. Then problems with parasitics and noise pickup will be reduced since the op-amp and its components will be near each other.

Answer 4

The traditional way was to use DIP headers holding the components and a DIP socket on the PCB.

Nowadays, there are much smaller board-to-board connectors that could be used to implement the same concept with SMD components on a tiny daughtercard.

Answer 5

If you can afford a prototype board that is different from production, just stick a pot on there, like Sandro said. Once you have it right, measure it, and put a fixed resistor in that place for production. Just be careful that you're not actually measuring the parallel combination of what you want and something else!

If you must have a single design, or if you can't squeeze a pot in there anyway, then I would go ahead and use the production design with surface-mount single-value parts, and hot-air replace them by hand.

Tweezers and flux are your friends! Likewise for a small-nozzle hot-air gun that can barely waft enough air to heat things up but not blow them around.

I've never had good luck with de-soldering through-hole parts. Seems I can never get that last bit of solder out that insists on holding on. Surface-mount is plumb easy! Just:

1. Put some flux on it.
2. Heat it up until the tweezers can move it.
3. Pick it up.
4. Let the pads cool.
5. Put a dab of new solder paste on them.
6. Push the new part into the paste.
7. Heat it again.
8. When the new part jumps into position (surface tension of solder), let it cool again.
   • If it wants to stand up on one end ("tombstone"), you might need to hold it down with the tweezers. This is usually caused by different amounts of solder on each pad, so that the surface tension of one overwhelms the other. If you hold it down, you'll still have different amounts of solder to deal with next time, but at least both ends will be connected.
9. Use a meter to check for the proper connections and no bridges.

Answer 6

If the frequencies in question is low, you can use a regular 2.54 mm pin header (female) and push the legs of THT resistors and capacitors in them.

Answer 7

If you asked me to do it, I’d do it a bit differently. First, the opamp-based circuit would be replaced by an MCU or FPGA with ADC on the input side and a DAC on the output. The initial setup would be transparent, ie. “no change” to the signal.

Then you can modify the transfer function digitally. The transfer function can be parametrized by opamp specifications and by the passive network values. So you could be changing virtual resistances and capacitances, and the digital part would emulate it in real time.

Then when you’re done tuning, put the parts you calculated back into the original circuit and it should work the same if you were careful.

If you want to keep it analog, you need a PCB layout specific to the tuning process. It would be what one calls a tuning jig. You’d put some convenient sockets for through-hole resistors and capacitors. Then once the tuning is done, you’d measure the parts on an LCR meter. And then, for the production version, you’d use “same” values but SMT.

Depending on how close you need to be to the original tune, the SMT parts may need to be selected using a batch process with a parts feeder, a probe, and an LCR meter under computer control.

Through-hole parts may have parasitics not present on SMT parts. That will matter at sufficiently high frequencies. In any case, you can measure those parasitics and replicate them with SMT parts.

Answer 8

1. You can allow multiple parallel pads to add SMD and not have to change them often unless you overshot the target.

2. You can have jumper traces that may be cut to increase R.

3. I'm guessing you should only need one variable R or C if RC=T.

4. Ceramic disc C's can be tuned with a blade to reduce a few %.

5. Design by specs is better with simulated tolerances.

Answer 9

While not a direct answer to OP's question about the best way to make it easier to replace a component multiple times, this answer provides a means to obviate that need.

Our power supply design team frequently needs to tweak some resistance values during testing to get the loop response desired, set the current and overvoltage limits correctly, etc.

They do all the appropriate analysis, modeling, simulation, etc to come up with the component value.

Let's say after all that a 5 K resistor is needed. They will build the board with a (say) 5.1 K resistor in place, and provide a place to put another resistor in parallel (say 500 K in this case). But instead of that parallel resistor, a pot will be installed so that the appropriate parameter (overvoltage trip point, for instance) can be adjusted.

Once that is established, the pot is measured and a fixed value resistor installed in its place. With this technique you only have to rework that site on the board one time.

Answer 10

Nothing beats 0.1" headers for practicality.

It is possible to solder 0805, 1206 or MELF components on the pins of a 0.1" header. The dimensions fit just right. You can solder a range of resistors on the header, then cut it to separate them. Then it's plug and play.

Using female headers for the components provides a space on the side of the header to stick a label. With male headers, it's also possible to fold the label over the component and cover it, then there's enough space to write a value. Then I cut the header strip and the label at the same time. It doesn't take long.

If it is too high for your application, you can use 90° headers, so the plugged module sits on top of the board, accessible from the side.

You could even have them pre-fabricated and labeled, by mounting the components on flex PCB with silkscreen label, and 0.1" spaced pads on the side for the header. Then cut it into slices.