Using arc trace routing instead of 45 degree trace routing
Most modern CAD software for PCB design offers arc trace routing or a form of conversion between 45/90 degree angel trace routing and arc trace routing. Despite this, the overwhelming majority of commercial-grade PCBs seem to still be using 45/90 degree traces.
A similar question has been asked before. The consensus there is that CAD software is easier to design that way. That question was asked in 2010 and the situation has changed since then, so I do not think that answer is sufficient anymore.
Are there downsides or upsides to using arc traces in PCB designs as opposed to 45/90 degree angle traces? Are there situations where one or the other is preferred? Is there a reason for the popularity of the 45 degree routing style besides it being the default option in CAD?
3 answers
You are accessing this answer with a direct link, so it's being shown above all other answers regardless of its score. You can return to the normal view.
Olin has a great answer, I just wanted to add some of my personal experience. I only started laying out PCBs three years ago, and I use KiCad. KiCad got curved traces support in test version 5.99 over two years ago, and I immediately started using that build because I was fixated on the aesthetics of curved traces. Using the curved traces took away the push and shove routing option, and I persisted still. In hindsight, I spent too much time to get a layout done that could've been routed in a fraction of the time with push and shove.
I also spent a month evaluating TopoR version 7, another layout software that boasts organic traces and a powerful, feature-rich auto router. They've done a great job with that software, but by the time I've set up all the constraints, and ran the algorithm for a few hours, the board could've been already done by hand using standard 45 degree traces. This is, however, on a relatively simple, non-HDI, no impedance control - all the things that could benefit from the advanced constraints and guided routing. I've done a bunch of testing, and while I really liked the smooth, organic traces, it just wasn't practical for my use case.
After all that, I am in a place where I don't use curved traces at all, and I don't see them becoming mainstream.
0 comment threads
The best route is a straight connection between the two points being connected. Of course that's not always possible due to other objects being in the way, or to be able to route other connections.
I think most auto-routing software uses 45° bends because that's a reasonable tradeoff between electrically good enough and keeping the software simple. I use Eagle, and that's what its auto-router does even when a direct path between points is available.
45° corners are shallow enough so that there isn't much inductance due to the corner, nor possibility to trap chemicals. Remember that inductance goes with the square of the number of turns. 45° is half the "turns" of 90°, so ¼ the inductance due to the bend. Since even 90° isn't a problem in most cases, 45° is "good enough" for the vast majority. The increase over a straight line isn't that much.
Routers are one of the few remaining pieces of software that take significant time on a human scale, even on today's computers. It can take over 10 minutes to route a decent size board on a reasonably modern machine. Therefore algorithm efficiency is still important. I'm not privy to the internals of any auto-router, but it's easy to imagine that having only 7 possible directions to go from any existing end simplifies things considerably compared to being able to head off in any direction, let alone in a curve.
The fixed grid architecture of most existing routers isn't well suited to arbitrary angles and curves. The overall grid size goes up with the square of the fineness, and of course the algorithm has more grids to look at, so gets slower too.
0 comment threads
The 45° routing makes it easier to route multiple parallel traces across the PCB - I would say that's the main reason why they are so popular. Whereas 90° turns of multiple parallel traces next to each other is a big no-no, since that may lead to crosstalk. And routing multiple parallel traces as arcs will perhaps take up a lot of extra board space needlessly.
Regarding arc traces, they have their place, namely when designing a RF path or PCB antenna. These layouts are often sensitive in all manner of ways:
There's various best practices such as placing all series inductors in a RF filter/matching network at 90° angles in relation to each other to avoid coupling. And matching network components should also be placed as close to each other as possible, to avoid parasitic capacitance. And so on - best practice design rules like that will in turn mean that the trace will end up in whatever shape that makes it easiest to draw the shortest possible RF path between components while avoiding sharp turns or vias.
0 comment threads
0 comment threads