Killing 3/32" endmills?

[saturnnights]

Okay, I've just started using some 3/32" carbide, 4-flute, square end, plunge-cutting endmills that I had here - never used one of this size before...
Anyway, I don't know what's going on, but they start to plunge and either snap before the plunge is finished or after the plunge, when the cut starts to move laterally, they snap.
It's weird because I have the same end mills in 1/8" and can cut the same piece and pattern without trouble. I can also drop a 1/16", 2-flute without issue either.
Now the weird thing is that when I look at the hole, it looks like the mill just didn't cut - like it's dull, but they're brand-new. They feel sharp to the touch too.
More specs: Taig CNC; 6,700rpm; soft brass; 0.0625" plunge; 4ipm feed rate.

Any ideas? I've just killed two end mills and don't want to try another until somebody gives me some advice. Is 6,700rpm too fast??? Too slow?? Weird thing is that I was just cutting with a 1/16", 2-flute end mill and it was eating the metal like candy. The only other thing I can imagine is that 4-flutes is too much for a 3/32" cutter to clear the chips, but the chips are more like dust - something I haven't seen before. I slowed this down to 4ipm to let it have an easy time of it and that didn't help - I usually run at 8ipm or so with my other cutters.

Thanks,
Mark

[HuFlungDung]

I would suppose that there is just not enough clearance in the flutes for the chips to come up the flutes. A two flute can usually be made to do a decent job of 'drilling' a hole while plunging. Still the chips can occassionally weld into the flutes if lubrication is interrupted (in aluminum) and plug the tool. In deep slotting, it might be good practice to allow the tool to rapid up to clear itself before beginning the lateral movement.

The center cutting 4 flutes, IMO, are suitable for ramping in, not so good on the vertical plunge. A zigzag ramp, or a helical ramp or a boundary ramp are more desirable from a tool life point of view.

[widgitmaster]

When we ran small endmills at our last shop, they programmed them to either spiral feed down into the stock or ramp feed, ramping is done when either x or y axis is moving durng the z-axis feed. Also, the RPM looked a little slow!
What grade of Carbide ar thos endmills, C2 C4 C6? C6 being the toughest grade!

Eric

[WhiteTiger]

I've used 4 flute cc minis in all 3 diameters, and one thing I've noted is that they have to be specified for aluminum in those itty bitty sizes. Every time I've gotten mixed up and used one with rake and relief angles ground for steel, they do exactly what you describe when cutting aluminum.

That "dust" chip description sure rang a bell

Might be something else as your specific problem, but my own booboo history has always been wrong rake and relief angles when this sort of thing happens with the minis.



Tiger

[saturnnights]

Originally Posted by widgitmaster When we ran small endmills at our last shop, they programmed them to either spiral feed down into the stock or ramp feed, ramping is done when either x or y axis is moving durng the z-axis feed. Also, the RPM looked a little slow! What grade of Carbide ar thos endmills, C2 C4 C6? C6 being the toughest grade! Eric

I don't know the grade - they are 30-degree helix made by Fastcarb Tool. I will try to ramp feed one tomorrow and see what happens. I was curious about this after I posted, so I put the same piece of stock back into the vise, installed a 2-flute, 1/16" end mill, reprogrammed SheetCam with the new diameter, but kept the feed and z plunge and everything else the same and ran it. The 1/16" did a fantastic job, even if it took over 75 minutes :-(

Oh well, maybe I need to try some 2-flute end mills in the 3/32"...

Thanks,
Mark

[saturnnights]

Originally Posted by WhiteTiger I've used 4 flute cc minis in all 3 diameters, and one thing I've noted is that they have to be specified for aluminum in those itty bitty sizes. Every time I've gotten mixed up and used one with rake and relief angles ground for steel, they do exactly what you describe when cutting aluminum. That "dust" chip description sure rang a bell Might be something else as your specific problem, but my own booboo history has always been wrong rake and relief angles when this sort of thing happens with the minis.

They're 30-degree helix - not sure what that's intended to cut? Probably not soft brass? Shoot...

Mark

[HuFlungDung]

Sorry, I missed that you said the material was brass. A high helix is not likely to be the answer, because brass has a tendency to cause the tool to 'hog in', overload itself and wreck something.

For the best cut while drilling (plunging) the brass or bronze alloys, the tool flute should have no helix at all. If you have a tiny wheel on a Dremel, you can get the wheel inside the flute at the sharp edge at the cutting end, and grind it flat, with a flat face parallel to the axis of the tool. This flat does not need to be extremely wide, probably .020" wide would be sufficent. It should be accurately flat, and should not round over the edge. Even presented to the work at a 90 degree angle, an edge will still take a chip if it has clearance underneath.

[Rich Carlstedt]

Did you buy them on eBay
I bought some carbide endmills and they were snapping like popcorn
I believe that sometimes they unload the poor carbide on ebay.
when i used the same size cutter from MSC, it took the load no problem !
On 4 flute plunges, I never go deeper than 1/2 the cutter diameter.
A 2 flute will go 3 diameters, but those 4's cannot clear out the chips.
rich
I run down to 3/64 (.045 )too on carbide .

[saturnnights]

Originally Posted by Rich Carlstedt Did you buy them on eBay I bought some carbide endmills and they were snapping like popcorn I believe that sometimes they unload the poor carbide on ebay. when i used the same size cutter from MSC, it took the load no problem ! On 4 flute plunges, I never go deeper than 1/2 the cutter diameter. A 2 flute will go 3 diameters, but those 4's cannot clear out the chips. rich I run down to 3/64 (.045 )too on carbide .

Yeah, they're Ebay, but supposedly made in USA. The Chinese imports I have from Ebay seem to work okay too. I don't know, it just seems like maybe this entire lot is bad? I wrote the seller and am waiting to see what he says. I may try another one today and only plunge 1/2 of the diamter and see what happens, but there's just something else going on here because of the "squeal" these make when they touch and start to plunge - just doesn't sound right. I have some ball nose ones from another vendor that I may try, just to see if they work and sound differently.

Mark

[saturnnights]

Originally Posted by HuFlungDung Sorry, I missed that you said the material was brass. A high helix is not likely to be the answer, because brass has a tendency to cause the tool to 'hog in', overload itself and wreck something. For the best cut while drilling (plunging) the brass or bronze alloys, the tool flute should have no helix at all. If you have a tiny wheel on a Dremel, you can get the wheel inside the flute at the sharp edge at the cutting end, and grind it flat, with a flat face parallel to the axis of the tool. This flat does not need to be extremely wide, probably .020" wide would be sufficent. It should be accurately flat, and should not round over the edge. Even presented to the work at a 90 degree angle, an edge will still take a chip if it has clearance underneath.

Does the helix refer to the number of spirals/turns per unit length, or are they referring to the faces of the spirals themselves? I guess I don't understand this all very well

[Caprirs]

The helix is the angle of the flutes relative to the axis of the cutter. On a high helix end mill, the flutes have to go around the cutter more revolutions than a standard end mill. High helix is analogous to a finer pitch screw thread. The advantage of the high helix is usually better surface finish. The disadvantage is that the chips have to travel farther up the flutes to be ejected from the cutting zone. So high helix are not good at deep slotting in aluminum but leave a lovely finish when profiling steel.

I agree that the 4 flute is probably loading up and cannot clear the chips.

[JRoque]

Hi. Didn't read every post here so I might be missing something. How's your runout? Are you using the same collet for that particular tool? For that small of a tool, I'd spin it as fast as I can and make shallow cuts.

JR