Broken bit

[MillAlien]

I'm milling a house marker plaque from walnut - I ran a roughing pass using a 1/2" ball nose and started the finishing pass using a 1/8" shank tapered ball nose. Snapped the bit at the collet using a 1/8" collet.

It looks like the tool was furrowing just before it snapped.

It's an Amana 46295-K tool and the tool data was imported into VCarve from the Amana library. (One thing I noticed is that the tool is described as having a 1/4" shank in the library, but Amana's data sheet and the tool itself tells me it's 1/8" shank. That threw me off at first, I thought I was using the wrong collet, but it's clearly not a 1/4" shank tool.)

The parameters are per the defaults - pass depth 0.12", stepover 0.0156", 18,000 RPM, 80"/min feed rate and 40"/min plunge rate.

The new tool's on order and I'd rather not repeat the same mistake twice.

I selected the 46295 after simulating about a dozen options and choosing that one because it was good balance of finished quality and toolpath time.

What should I adjust?

[martin54]

What size tbn are you using for finish, has to be 1/32 at the minimum if it's tapered & that's a big jump from a 1/2" roughing bit. Post a couple of pictures. Do you really need to go that small to get the level of detail required?

Just to add for a 3d finish pass the tool doc in the tool database isn't taken into account. Finish pass is one pass at full depth

[SteveNelson46]

For projects like this I usually use a .25" end mill for the roughing pass with a 30% stepover and a .25" depth of cut per pass and a .03" machining allowance. For the finishing toolpath I use a .125" tapered ball nose with a boundary offset of .063". You also need to check the chipload of the bits you use. 18000 rpm seems a little fast for 80 ipm.

[Pete Cyr]

I would use a 1/4" shank , 1/8" tapered ball nose at 12k rpm, 200ipm with a 9% stepover

[sharkcutup]

At least that bit got a taste of wood before it broke. I have had a brand New 1/4" shank 1/16" diameter (Amana 46290) bit break on a Z-Zero Set to touch plate. The machine decided to continue on after it made contact and bit snapped. Never got the chance to carve/taste wood!

Sharkcutup

[MillAlien]

What size tbn are you using for finish, has to be 1/32 at the minimum if it's tapered & that's a big jump from a 1/2" roughing bit. Post a couple of pictures. Do you really need to go that small to get the level of detail required?

Just to add for a 3d finish pass the tool doc in the tool database isn't taken into account. Finish pass is one pass at full depth

I'm using the 1° straight angle ball tip, 1/8 Dia x 1/16 Radius x 1-1/2 x 1/8 Shank.

I did not know that the tool doc isn't used for the finish pass.

[MillAlien]

I would use a 1/4" shank , 1/8" tapered ball nose at 12k rpm, 200ipm with a 9% stepover

Yep - that's the tool I'm using and I was thinking my stepover (12.5%) was too much.

But, 200 IPM?

[MillAlien]

What size tbn are you using for finish, has to be 1/32 at the minimum if it's tapered & that's a big jump from a 1/2" roughing bit. Post a couple of pictures. Do you really need to go that small to get the level of detail required?

Just to add for a 3d finish pass the tool doc in the tool database isn't taken into account. Finish pass is one pass at full depth

I get a chip load of 0.0022" @ 12k rpm @ 80"/min and 0.0015" at 18k rpm. Amana's spec for that tool is IPM 80-100" and 0.0015-0.0025" chip load.

[Rcnewcomb]

But, 200 IPM?

You have a decent machine. It should be able to handle 200 ipm for 3D finishing.

[MillAlien]

But, 200 IPM?

You have a decent machine. It should be able to handle 200 ipm for 3D finishing.

Okey doke.

I've melded all of the above comments and suggestions into a new path to my toolpaths that ought to work.

Thanks everybody!

[Pete Cyr]

I would use a 1/4" shank , 1/8" tapered ball nose at 12k rpm, 200ipm with a 9% stepover

Yep - that's the tool I'm using and I was thinking my stepover (12.5%) was too much.

But, 200 IPM?

You listed a tool with a 1/8” shank......I listed a 1/4” shank