If I have an obtuse trace, will the complementary acute angle cause issues?
It's not going to matter much which one of the choices you use.

Generally it's good to avoid corners less than 90&deg;.  Note you don't seem to have a problem with the small 90&deg; corners at left where a thinner trace leaves a fatter pad.  Down to 90&deg; is going to happen.  Don't worry about it.

There are two issues here, acid traps and inductance.  In some bad PCB processes, chemicals can get trapped inside sharp corners of the copper.  This isn't going to be a problem if you use a competent board house.

A conducting path going around a corner has more conductance due to it acting like a coil.  You can think of a 90&deg; bend as a &frac14; winding.  Unless you have high frequency signals, this too is a minor issue.  However, it's usually no big deal to use two 45&deg; bends instead of one 90&deg; bend, as you do in the red traces in the bottom of your pictures.

Remember that when hand-routing, you're not stuck with multiples of 45&deg;.  What I'd do for the case you show is to have the trace go straight from the via to the left-bottom corner of the pad.  There is no reason for a bend part way like you show.

It may also be that in your bottom layout that the trace is too close to the left pad.  Did you run a DRC check?  It seems odd that all your traces are fatter than the minimum distance between traces.  You expect power traces to be fatter, but signal traces are usually the minimum.

Here is a example of what I'm talking about:



This resulted from a combination of hand-routing and auto-routing.  Note the various traces leaving pads at corners.  This guarantees greater than 90&deg; angle.  There is also two 90&deg; Ts at the top, and other places where traces leave the edges of pads.  That's OK, but try to avoid less than 90&deg; angles.

The red trace going around also illustrates turning a 90&deg; corner by using two 45&deg; corners (near top right).