What are the advantages of through-hole PCBs over wire wrapping?
I can see many advantages of wire wrap (though I've never used it, so I might be mistaken):
- due to wire shape, unwanted capacitances are kept much smaller in wire wrap (compared to e.g. a 2-layer PCB),
- it should be about as labor-intensive to wire wrap through-hole components as it is to solder them (TTBOMK you can't reflow through-hole components, so you need to spend some time per pin),
- no need for explicitly making multi-layer PCBs: the problems of routing, possibly stacking layers (for >2 layer ones), coating vias, etc. just go away.
The only advantage of through-hole PCBs I can see is that they're more durable mechanically and thinner.
Am I missing something obvious?
"it should be about as labor-intensive to wire wrap through-hole components as it is to solder them"
Mass production uses wave soldering. You simply insert all the parts into the board, soak the board into molten solder, and pull it out. bingo, the full board is soldered within seconds. You can't wrap all the wires within seconds."due to wire shape, unwanted capacitances are kept much smaller in wire wrap (compared to e.g. a 2-layer PCB),"
Due to physical construction, unwanted inductances are much higher compared to a PCB. Even for advanced wire-wrap boards with ground planes (people used them in the late 80s during wirewrap's last days), it's still difficult to match a PCB's performance. A typical 4-layer board's signal layer is 0.1 mm above the ground plane, a wire-wrap board it's typically 5 mm, causing a 40x increase of loop area."no need for explicitly making multi-layer PCBs: the problems of routing, possibly stacking layers (for >2 layer ones), coating vias, etc. just go away."
One huge motivation to use a multi-layer PCB in modern designs is not even extra layers for the signals, but to have solid power and ground planes that contain nothing but solid copper. A copper pour on a multi-layer PCB naturally forms microstrips, the simplest kind of microwave transmission line, which is required to support high-speed digital signal transmission. Likewise, the capacitance between the signal layer and a ground plane is a feature, not a bug. Because of its planar circuit nature of a PCB, characteristic impedance is tightly controlled and extremely reproducible. Overlapping wires over a ground plane do not have a consistent characteristic impedance.Even in lumped circuits and analog designs when controlled impedance does not matter, a solid ground plane is often still important to minimize loop area and parasitic inductance. Modern power MOSFET's switching speed is reaching 100 volts per nanosecond.
Standard wire-wrap construction is ill-suited above 10 MHz. Even back in the late 80s when electronics is made of really slow through-hole parts by modern standard, wire-wrap already started to show serious signal integrity problems.
---
But... Believe it or not. All of these problems I listed have been solved already in the 80s by combining the best of both world. The final next-gen invention was called "Multi-Wire" circuit board. It looks like a normal PCB but its inner layer uses insulated wires for connections, allowing overlapping traces. The ground planes and outer layers are similar to PCB. Reportedly,
IT can convert a multi-layer PCB design with 12 signal layers to a six-layer board with just two signal (wiring) layers.
But it was an highly expensive technology, and did not see much uses outside niche high-end applications. Today Hitachi is one of the few companies that still offer this service.https://www.swtest.org/swtw_library/2013proc/PDF/SWTW13-22.pdf
> Likewise, the capacitance between the signal layer and a ground plane is a feature, not a bug.
Do you mean that it being consistent and predictable is a feature, or that it being high enough is a feature? (IOW, would consistent lower capacitances be better?)
@robryk@qoto.org Both can be features under the correct circumstances. Between a signal and ground layer, the consistent capacitance creates a well-controlled characteristic impedance, since a transmission line is defined by Z = sqrt(L/C). Impedance can further be tuned just by adding and removing coppers just by modifying the design files.
Between a supply voltage and ground layer, the capacitance also creates a nearly ideal parallel-plate capacitor with negligible parasitic inductance, good for noise suppression up to many gigahertz, and useful for reducing electromagnetic interference, even 100 picofarad helps at several GHz, sometimes you just need a little bit of it to pass radiation testing.
But it's still pretty low. To make the capacitance as high as possible there's a special PCB manufacturing process called Buried Capacitance, also a niche technology invented in the late 80s, can create a circuit board with power and ground planes with a 0.05 mm spacing, separately by a special material with high dielectric constant, boosting the capacitance by 10x. This also allows you to remove most bypass capacitors from the board, freeing up more routing spaces.
@niconiconi