Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
Part of the problem with extruded is not just the internal stress (as mentioned previously) but that it uses a different recipe to actually lower the melting point (this is why they use extruded for thermal forming and it flame polishes better). The combination of the low melting point with higher internal stress makes it almost impossible to cut perfectly, without VERY material specific tooling (think “extrude acrylic cutter” not “plastic cutter”) or other equipment (air, vortex coolers, etc). Otherwise you are always either shattering the stressed material or partially melting it.
Keep in mind for the following that this is a tiny soft media tool. I’m intentionally trying to keep this vague due to bias issues and I don’t want anyone trying to use these numbers for anything other than the plastic comparison. To give you an idea I ran the same tooling from the same batch in some extruded and cast acrylic for testing. My test increased by 0.000125" (0.0032mm) chipload at each step. The extruded had a “tolerant” cut at one step 0.002" (0.051mm) chipload. The worst part of this is that, in our experience, even the same material from the same supplier might not run at that chipload again. This is due to the changes in processing of the plastic even with the same recipe. The cast material had a range of good cuts from 0.00275”-0.00325” (0.067mm - 0.083mm) (6 steps).
The geometry is where you can potentially get much better results in the material but cutter price starts to climb with extremely specific cutters. You can get a lot closer with plastic or soft media cutters as they have higher rake, different helix angles (lower for less “pull on the material, higher for more sear), more flute volume (places to hold chips in the flute), and relief to keep as little of the tool from touching the material. All of those things cost you in other areas though (tool strength, chip clearing, more stress to material, machine time, etc). So it’s always a fight between the economy of scale and the best tool for the application.
Yeah, coated tools in general I don’t like to recommend for plastics. It depends on the plastic, but you are always going to be dealing with a thicker edge slamming into the material (you coat the WHOLE tool). The advantage is less wear and possibly a smoother surface depending on the grinding wheels and coating used.
Are you sure this is PVC? Most of the stuff I looked at on their site is melamine, PET, or acrylic. The ultra high gloss is listed as “foil” on melamine.
Liam already got most of this. Basically a bigger upcut cutter for profile with a high speed clean up (not personally a fan of compressions but they are an option with pros/cons). There are a couple other specifics for multi material with deflection limited machining I’ll add though.
Won’t comment too much on the specialist tooling as again I’m bias. But it is possible with very high grades of carbide to make cutters that are both more aggressive and last. The blanks and processing material are more expensive though in addition to increased grinding time.
The first problem is that you have to find a feed and speed range that’s at least cutting both. Most likely it won’t be ideal for at least one though. Switching in this case to more aggressive tooling can help as they are both soft media. That will reduce the cutting force and get a “thinner” edge giving you a wider range at the cost of tool strength.
Even after accounting for that though you have 2 different materials with 2 different strengths changing the deflection. So once you are cutting anything but matching material(s) it will deflect more or less than before based on the strength of the different materials. That will end up slicing a very small amount off either the conventional or the climb side of the cut. This can leave a very poor cut or in the case of some plastics, melt it.
You can reduce the above effect by limiting deflection (shallower pass, less chipload) but you need to still keep it inside of the material range which is already limited by 2 different materials. In an ideal world we would cut it in a single pass keeping the load on the tool and machine the same throughout the cut. But we all have to deal with the limits of the tooling, machine, and materials.
Hope that’s useful. If there’s anything I can help with or expand on let me know.
