Coated Carbide 4Flute Endmill, 3Flute Slot Drill, or 2Flute Slot Drill?

[weaston]

My preference has been to generally use a 4flute coated carbide endmill for almost all my machining and only use a 2flute slot drill when slotting or if shavings could be a problem. I never really used a 3flute slot drill.

In my new company, they only really have 3flute slot drills and use 4flutes only for finishing aluminium jobs. I think the idea is to reduce tool inventory, as they can use the 3flute slot drill for all types of operations.

Can anyone give me their opinions and preferences.

Thanks.

[cdlenterprises]

3 flutes give you the best of all worlds. They generally have enough flute clearance to cut the softer metals. 3 flutes also allow you to still maintain a decent feedrate and can give you better harmonics than a 2 or 4 flute because it they will tend to have a flute in the cut at all times (depending on depth of cut, etc.) The downside is that they're a little tricky to measure for cutter comp.....

[weaston]

3 flutes give you the best of all worlds.

I suspected that this was the reasoning behind our company using 3flute tools. .[/QUOTE] give you better harmonics than a 2 or 4 flute because it they will tend to have a flute in the cut at all times [/QUOTE] Sorry for my lack of understanding but could you perhaps explain this concept a little further, in particular the phrase "better harmonics". I assume you are trying to say the the 3flute tool is better 'balanced' during machining than the 2 or 4 flute variety.

Thanks

[holbieone]

the amount of flute engagement has to do with the angle of the helix

the grater the angle the more engagement you have

always having the tool engaged in the stock will keep it from relaxing in between flutes

3 fluted tools or odd fluted tools tend to cancel out some of the vibrations

data flute makes a really nice 3 flute end mill

[kalmah]

My preference has been to generally use a 4flute coated carbide endmill for almost all my machining and only use a 2flute slot drill when slotting or if shavings could be a problem. I never really used a 3flute slot drill.

In my new company, they only really have 3flute slot drills and use 4flutes only for finishing aluminium jobs. I think the idea is to reduce tool inventory, as they can use the 3flute slot drill for all types of operations.

Can anyone give me their opinions and preferences.

Thanks.

- 4 flutes with special design for roughing, slotting is very good when slotting material difficult to cut (steel, stainless steel, superalloy). You can have a very good productivity.
The main problem is the shouldering:
4 flutes produces easily chatter when you use roughing parameters. Either you use a special mill with differential pitch in order to avoid chattering, or you have a very rigid structure.
Other solution:
Use low ae (radial depth of cut) with high cutting speed and feedrate.

- 3 flutes should be used for little diameter (diam 2...8mm) in slotting and shouldering of material difficult to cut (steel, stainless steel, superalloy, titanium). There is just a special case: It's the method drilling/slotting. These special mill (Nachi, NS tool) have 3 flutes whatever the diameter. Here is an exemple
http://www.nachi-fujikoshi.co.jp/eng...eo/geoslot.ram

- 2 flute should be only used for very little diameters (diameter 0.05... 2mm) for steel, stainless steel, titanium. 2 flutes is very good in slotting of material such plastics, aluminium, cooper whatever the diameter.

Reason:
- Aluminium, Plastic,...produce low cutting forces and the most important is the place for chip evacuation => 2-3 flutes maxi
- Steel, stainless steel, ... produce high cutting force. The most important is the flute resistance and it's not the case with 2flutes end mills (for diameter 3mm or more).

[jmagnuson]

To sum it all up. If you have large chips (i.e. aluminum), you want less flutes when hogging it out so chips don't get caught in front of the post-ceding flute. More flutes are better when the material makes small chips (i.e. cast iron) so you can get a higher material removal rate when increasing rpm (increased heat) or travel feed rate (increased spindle load) will produce problems.

[Integrex]

I would recommend to use 4 flute for everything is possible.

Centrecutting tool is not an issue, 4 flute cutter with Ramp or helical entry motions on all toolpathing. id usually recomment 2 to 3 degree entry angle

feed fast with light cuts to avoid heat build up (heat should be ejected with chip if you do everything right)

also trocoidial toolpath motion will give incredible chip evactuation

[newguy81]

My tool salesman got me hooked on 3-flute by Duramill, they call theirs "WhisperCut" . Big time tool life and feed rate. Only drawback is the corner is not a true 90. Dosen't matter much on the parts we run, and our Integrex smokes with'em.