Long and delicate endmills

[Moded1952 (Lucas)]

@jwr

When using modeling board, cutting objects which are 30-40mm in height and might have tight corners where only a 1mm endmill can reach is challenging. And there are often steep walls where you have to reach >20mm deep, so tapered endmills won’t often work.

I too have encountered this problem but the answer for me at least wasn’t to use crazy long endmills (the 883 Pro is very unsuited to that), it was to reduce the depth an endmill would have to reach.

A couple of alternatives to super-long endmills:

• Layers: Instead of cutting a 40mm-high object in a single setup, cut one 20mm slice, then another 20mm slice, then join the two slices together with some kind of bond or adhesive. This would be particularly suitable if you’re carving something like terrain.
• Multi-sided machining: Cut one side of your workpiece down to 20mm depth, then flip it over and cut 20mm from the other side. This would be good if you’re dealing with something like figures.

I’m not exactly clear on what it is you’re making, are you able to elaborate?

@jwr

But then I started thinking and realized that I have no idea how to approach feeds and speeds for such an endmill. It has a 25mm long part of the shaft where the diameter is only 0.95mm! Do I go with max spindle speed and feed very slowly (150-200mm/min)? Or do I try to scale everything down? Will the cutting forces be lower if I also slow down the spindle?

Haven’t used them so keep that in mind but I’d look for directions from a manufacturer of similar endmills (or buy an endmill from a manufacturer that supplies feeds and speeds).

For example the DIXI Polytool 7239 looks pretty close and they supply feeds and speeds on page 165 of their catalog.

For a 1mm endmill in plastic (assuming that’s what “modelling board” is), they recommend:

• 240-260mm/min surface speed (38k RPM)
• 0.1mm axial engagement
• 1mm radial engagement
• 10-15µm feed per tooth (so 380mm/min with a single-flute at 38k RPM, or 240mm/min at 24k RPM)

But I’d consider what you’re doing to be really experimental. These endmills aren’t intended to be used for our class of machine, they’re made for rigid high-precision machines with high-speed spindles.

And the one thing I can absolutely say with 100% confidence despite never having used one of these is check your spindle and collet runout. Figure out which collet you’d use and buy a precision dowel pin with the same diameter and as close a length as you can to the endmill you want to use. Measure the runout at the tip with a dial indicator. With these delicate endmills, runout is super important. 0.1mm of runout might not cause too much trouble with a bigger endmill but with these tiny ones it’s the difference between cutting and just slamming head on into the stock.

If your runout is too high, you might need to look into high-precision collets or techniques like clocking.

@jwr

At 30€/piece, I’d rather not do too much wild experimenting, so I’m looking for any advice from people who worked with long, thin and delicate endmills.

I don’t think you’re going to have much luck, the only micromachining I’m aware of using Carbide 3D’s machines is @wmoy milling graphite and the folks using it for PCBs. Both of those cases use V-bits.