I use carbide and tool life is very good. HSS should be sufficient but I've spent the extra on carbide and have made 4-5 sets of DLG molds with the same tools.

All of the cutting speed / cutter / pass info is based on your individual machine and what it can handle.

Mine is happy roughing with 1/2 ballmills (2 flute) at 60-80ipm and 25% stepovers and 25% depth with a 3.25hp router.

Finish passes are usually done with 1/4" tools (2 flute again) at 80-100ipm and 10-25% stopovers. Sometimes I use 1/8" tools and run a little over 100ipm. If I am using 4 flute tools, I typically run a bit faster.

It's important to get your CV and acceleration settings properly configured first or you'll lose steps even at lower speeds when cornering sharply, say at a resin channel edge.

FWIW, mine is a homebuilt rack and pinion CNC with 425oz/in steppers and a Hitachi 3.25hp plunge router, G540 drive and Mach3.

Sorry for taking so long,
PC got lightning damage, so i've had to improv.

So this is a mixed part 2.
Steps that I have taken to the point of completion.
1. Create mold layout and plan ahead to create different borders or containments for the different cuts that you will be making.
2. Create rough cuts and undercut them by 0.25mm or more.
3. I use the biggest cutter to cut most of the material. (I use 8mm roughing bit with chip breaker solid carbide only)
4. Calculating the speed and chip rates is easy if you get cnc cookbooks g-wizard as a starters guide.
5. Generally the fastest and most efficient cut is just before the tool breaks, DO NOT TRY THIS AS IT IS BAD FOR YOUR MACHINE, YOUR CUTTER, YOUR WALLET.
6. I use the borders to contain the cuts as this reduces the cutting time.
7. My final cut is done with a 0.3mm stepover and it is important to pic the correct tool for areas like the leading edge, here you can use ball nose or corner radius bits.
8. One thin I have learnt with less complex cnc programs is that parallel finishing is the best, and in more complex programs there are some features that allow nicer finishing methods.
You really only need what RhinoCAM can offer.

If there are any more questions let me know I will answer what I can but I'm no expert.

Oh, and I will only use Solid Carbide and coated if needed.
I've used SC Bits 35X more than HSS and still have not blunted any, I tend to break them first.....

Orrin

I prefer the cuts to be perpendicular or 45* to the span of a wing or length of a fuse mold. Cuts that are parallel to the span are more difficult to sand and polish accurately

Ww,

You are 100% correct thanks for bringing that up.

Orrin

I also like a small positive protrusion milled around the LE of wings and around fuse molds. This allows one to polish the mold cavity without rounding out the seaming corners. Once the cavity is polishing you block the protrusion off leaving a nice sharp corner. This will make for tighter nicer looking seams.