I understand that right angle pcb traces should be avoided because it can cause problems during manufacturing.
But what about right angle through a via? Will this have any negative effects?
I have a multi layer board and I don't have that much space. I have come across a point where the only place I can place a via is right next to the pad I want to connect to, and my trace is coming from directly above.
"because it can cause problems during manufacturing"
If right angle traces come loose you have to go to another PCB manufacturer. Quality PCBs don't have this problem anymore.
On HF boards right angles are avoided because of radiation they cause (reference, p.14). Otherwise the only reason seems to be aesthetical. You can safely part from your via on the other side of the board any direction you want.
If yours is an HF board, keep in mind that vias cause extra inductance and capacitance, and cause reflections because they change the characteristic impedance.
The reason for avoiding right angles is that it causes a discontinuity in a trace routed for signal integrity.
This is caused by two distinct physical phenomia.
1: The wavefront interacts with itself after a small delay in the same way as an inductor or capacitor does (H or E fields respectivly)
2: The right angle corner contains more copper, so has a different impedance.
As with any signal (trace trace or not), if there is a sudden change in it's impedance of it's medium you create a resonant circuit.
This is relevant at ANY signal frequency. It is the speed of the edges that matter.
For a sine wave this is not such a problem unless your signal frequency is at a really high frequency. But for for a digital signal, for any edge you get a series of harmonics of the rise & fall time combined with the duty cycle. This creates an 'infinate' series of harmonics (in reality more than 100 or so is so small, it's below noise) We see these harmonics as ringing because of the filter effect of the trace's mismatched impedance.
Remember this does not matter if it's a 1kHz or 1GHz signal, the only difference will be the size and number of harmonics, not their location.
Of course you get related harmonics of the signal itself, and because the rise and fall time can never be less than half the period of the signal they are closely related (for periodic signal), hence popular confusion.
Now, if any of these harmonics are at a location of the resonance frequency of our discontinuity we get emissions, or even worse, ringing so bad that our signals become corrupted.
You can avoid (2) by making the corners the same width all the way round. Imagine a narrow strip of paper folded at 45 degrees, you don't get a corner, you get a chamfer.
You can avoid (1) by avoiding right angles, however for most signals and circuit sensitivities this is not really an issue.
Now back to the question:
For vias we have a problem. The via introduces a discontinuity if we like it or not because of it's annular ring(s). That means reason (2) becomes irrelivant for vias and (almost) impossible to avoid. The effect of the annular right will be far worse than the bump in the traces width.
And (1) does not apply to vias as normally the via will route a signal to another layer through a plane. The field lines will not go through the plane so the effect is eliminated, however, the signal going through the plane also creates a discontinuity of it's own, which will be far greater change in impedance unless carefully designed.
Conclusion:
Don't worry about right anges in vias unless you are dealing with very high frequencies, but do worry about vias for fast edges or high frequencies (especially both).
