Boedeker has some very useful machining guidelines:
https://boedeker.com/Technical-Resources/Technical-Library/Plastic-Machining-Guidelines
Also, Quadrant Plastics and Eppinger both have guidelines and recommendations. I have been involved with machining of plastics and composites for 4 years now at Lehigh Valley Plastics. Some are very pleasant to work with (acetals, PVC's, unfilled nylon) and behave very nicely.
Nylon is hygroscopic and will change sizes depending on how wet it is. It can also be very abrasive especially if glass filled. But it is very strong and wear resistant.
Acetals (think Delrin but there are many different types) are very nice to work with, hold sizes well and are very stable. Slippery and makes for a decent bearing.
PVC is easy to work as well, holds sizes well.
UHMW's are easy to work with but difficult to get good finishes and hold tight tolerances. Especially on larger parts. Super slippery. Excellent bearing material. Nothing sticks to it.
Teflons are similar to UHMW's.
PEEK's are extremely tough, can be difficult to work with but excellent surface finishes and very tight tolerances are possible. Diamond tooling is preferred. No stringy chips, machines a bit like cast iron.
Polycarbonates (Lexan) and Acrylics (Plexiglass) are more brittle and tend to chip out easily. Especially when drilling.
There are so many others that they don't spring to mind at the time.
Rule #1: Heat is the enemy of plastics!!!
Thermal expansion is a problem and coupled with the fact that plastics don't dissipate heat like metal presents some unique challenges.
use a water based coolant whenever possible.
Look for tooling designed to cut aluminum.
Use positive tooling on a lathe. negative tooling doesn't work well. Except maybe on PEEK.
I use 600SFM with carbides as my base line and adjust from there based on behavior at the machine.
For feedrates start with .01 IPR and adjust as needed.
For drilling I usually use 150 to 200 SFM due to rule #1. Peck a lot, get the chips out or they will bind and create friction and therefore heat and melting and burning WILL happen. Chiploads are similar to those used in drilling metals.
For milling with carbide start with a baseline of 600 SFM and .003 to .007 IPT to start. For HSS tooling maybe try 200-300 SFM. Light depths of cuts with fuller radial engagement is preferred especially on routers.
Just because it is plastic is no excuse for a poor setup so like all materials consider cleanliness and rigidity. If working in a chuck or vise get a good grip.
I can't stress this enough: HEAT IS THE ENEMY OF PLASTICS!!!! KEEP YOUR TOOLING SHARP!!!
I hope this helps.
Benz