Facemilling Titanium

[Squidmaster23]

We've been having some trouble getting a decent surface finish with facemilling titanium. Our parts are 5.45" long by .470" wide and the total amount of thickness we take off each part is around 30-40 thou with the finish pass being around 1 to 5 thou. I've been using a Maritool 3 flute 45 degree shell mill with some Sumitomo inserts but I'm still struggling with it. I've tried speeds and feeds from both HSM and Gwizard with no luck.

Do you guys recommend any particular tools for facemilling titanium?

 

[Finegrain]

Since the part is so narrow, I think I would rather use a corner-radius endmill.

Regards.

Mike

 

[EnginCycles]

If your part is that narrow why are you using a face mill? Use a 0.500" 5 flute with a 0.030" corner radius and it will be done. I use SGS with excellent success. The next issue will be how you are holding the part and obviously the machine. A 2" mill is big if the machine is not stiff enough.

 

[Booze Daily]

I generally don't like to use a facemill unless the part is wide enough to get 2 inserts in the cut at a time.
Otherwise you're just banging one insert thru at a time.

 

[gregormarwick]

A method of facing narrow parts that works very well is to offset the facemill to one side so that the cutting diameter just overlaps the edge of the part. That directs the cutting forces along the length rather than across the width and gives much better engagement. The result is a much better surface finish.

 

[Finegrain]

If your part is that narrow why are you using a face mill? Use a 0.500" 5 flute with a 0.030" corner radius and it will be done. I use SGS with excellent success. The next issue will be how you are holding the part and obviously the machine. A 2" mill is big if the machine is not stiff enough.

Eh, maybe a 5/8" . 1/2" with 2x .030" corner radii won't clear a .470" wide path.

Regards.

Mike

 

[Rick Finsta]

I'd use the CR endmill and climb cut down each side longways with like 1.5-2X the corner radius overlap in the center to make sure I don't push a ridge and to minimize the burr that the chamfer tool has to deal.

I also really like the SGS 5 flutes. Great surface finish and hard to kill.

 

[EnginCycles]

Eh, maybe a 5/8" . 1/2" with 2x .030" corner radii won't clear a .470" wide path.

Regards.

Mike

One thing I like is when you go both directions it removes the heavy burr left with a single pass. Probably going to chamfer it but if it is a first op you can ditch the chamfer with both directions. If you are going to handle the part after facing this is also a welcome thing. The 5/8" is probably the better option but I use it so rarely I would rather stick with the tool in the machine.

 

[DouglasJRizzo]

I have to agree. On a narrow part, a good, coated carbide end mill with radius ends would be my choice.
If you want to keep the shell mill, offset it to one side by about 40% and leave more material for the finish pass.

 

[OCTANE WORKHOLD]

Agree with the other suggestions to use an endmill with a corner radius for a narrow facing operation.

If turning the part on it's side is an option, using the periphery of an endmill will leave a great finish.

Whenever using a facemill, it is best to mill from thick to thin.
This video from Sandvik illustrates this well.
Tips film: Golden rules - thick to thin milling machining - YouTube

 

[mhajicek]

As said above, solid carbide bull. If surface finish and flatness matters more than cycle time I'll take narrow stepovers, like 10%, and dynamic milling parameters.