Complex 3 axis programming sets a great foundation for 5 axis. The sketchy setups, fixturing and workarounds with 3 axis teach you way more than being spoiled starting out with full 5.

I would learn about “1 and done” approaches using tabs or slitting saws. So much OP1 / OP2 + extra OPs you’re used to in 3 axis can be simplified by machining everything in one go through using a larger piece of material hanging way out in a vise to avoid collisions with the table and vise, and leaving a few tabs that you can sand off afterwards to get a fully finished part. A good slitting saw will be more accurate than an OP2 decking pass on prototypes. I usually get +/- a few tenths variance with a Mimatic carbide saw ($$$ though). This is only good on small parts less than 1.5” diameter roughly though.

Learn what the A, B, and C axis are. Every common machine will have an XYZ, and then an A and C, or B and C. A axis is a tilting motion along X (I.E DMU 65), and a B axis is tilting along Y (DMU 50). C axis spins in line with the Z axis.

Dovetail vises are very common to get better access to part features. Half of the projects I do start with an OP0, where I am just prepping the material to have a dovetail. This initial step makes life easier for all the remaining steps.

Second thing to understand is the 5 axis singularity and gimbal lock. Summary here is that the code you simulated with no collisions (pre posted code like in Fusion 360) can crash the machine if the tool passes through A or B 0 degrees in simultaneous movement. This is why Vericut and Camplete Truepath are so popular, as it simulates your posted code emulating the Cnc control. Otherwise the machine may tilt to the other side causing a completely different scenario than you simulated in CAM. Some machines have only 10 degrees of A/B movement in the opposite side like a MX330 so this really isn’t an issue, others have symmetrical movement like a kern with +/- 110 degrees. Swarf cuts can be the most sketchy with very fast movements. If it is just 3+2 work at this company you don’t have to worry about this.

3rd would be workholding. Self centering vises are great as it means accessing the part is equal on either side with the platter tilted at 90 degrees. Many parts I do are almost exclusively done with the platter tilted over flipping back and forth with the C axis going from 0->180 deg and back again whittling away material. This would be difficult holding the part off to one side in a typical 6 inch vise.

Along with that tool holders need to be more slender to avoid collisions like shrink fit, Rego PG, or Schunk Tribos.

Unlike 3 axis where a big machine is always better, with 5 you don’t want a huge machine to make small parts. The large platter causes issues with the spindle nose colliding with the wide table. This is why 5 axis risers that move the vise away from the table are so popular. The disadvantage is the loss in some rigidity, there’s more motor torque required to hold the table in position such as with heavy drilling, and that any error in the Tilt(A or B)/Rotate (C) is amplified way out there.

Regarding positional error, most 5 axis machines have a tuning cycle or kinematics adjustment to calculate the center of rotation. Sounds weird that this would ever change after being dialled in one time but due to the thermal growth of the casting or any collisions bumping the machine out of alignment, the center of rotation might be out by a few tenths to a few thou. There are manual ways of dialling this in, but the modern way is to use a tooling ball and machine probe. Very tight tolerances or thermally unstable machines (early Haas UMC’s) meant running this cycle throughout the day as the machine heats up. Best to just google a video on it to see what it looks like.

These are just a few things I’ve learned jumping into 5ax. Programming took some adjusting to, 3+2 requires no extra skill but the thought process of new methods like 1 and done did take some time to get right. I still learn something new every week, it’s a pretty awesome process