Surfacing - is a 2 flute really the only true option?

[MILLRUNNER]

A friend of mine experienced in surfacing was telling me that 2 flute endmills are the only ones that really cut all the way down to the center. I was looking at some 3 and 4 flute ball endmills, and sure enough, I see the relief. Can a 3 or 4 flute be used in the rough surfacing (or any op for that matter) at all, and how do I know the limits for speeds and feeds because of the small section of flute that is essentially not cutting?

[Müřlıń®]

On 3-d surfacing there is alot of downward ramping motion so a 2 flute has the best chip clearance.....yes I use only 2-fl for 3-d surfacing...

[betts]

Your friend needs a different end mill vendor.  If you look at a 3-flute ball there is one flute that goes past center.  A 4-flute ball has two relieved and two meeting at center like a two flute.  That being said if you MUST spend a lot of cut time using the tip, as murlin said you will probably have more success with a two flute.

 

And yes basically you have zero SFM at the tip of a ball end mill so depending on material and rough or finish cut you may need to make adjustments to what you would otherwise do.

 

HTH

[Müřlıń®]

Everyone has their own style of machining...

 

For those who like to run mostly waterlines and horizontals, a 3 or 4 flute works just fine depending on the shape of your geometry.

 

I like to do a lot of scallop machining and most of the parts I do are complex with a lot of features so scallop does a lot of ramping down.

 

To keep the number of tools needed to a minimum, I will choose a tool that will work on all my tool paths.

[jeff]

...yes I use only 2-fl for 3-d surfacing...

Even in steel?

I've never tried it, maybe I should.

[?Mark]

3 FL bull nose is great too....depending on what kind of surfaces you're cutting

[Müřlıń®]

Even in steel?

I've never tried it, maybe I should.

Used 2 fl on High Nickle die steel for years...

 

But we are talking ball cutters here...

[Matthew Hajicek - Singularity]

Bull cutters are great for surfacing, especially in the up/down direction.  I've used 3" indexable cutters to surface a slope on a three axis setup, and I was able to get good finish with a pretty large stepover.  You're never cutting with the center and it acts like a noticeably larger ball.  The zero SFM at the center is why five axis programmers will tilt the tool when possible so as to never cut with the center; sometimes you can do it with four axis or even three axis setups too, if you have options on how to orient your part.

[gaijin_2007]

Mitsubishi have a 3 flute ball nose tools with all 3 flutes to center (some of the other Japanese manufacturers do too IIRC).

http://www.mitsubishicarbide.com/application/files/2614/4643/8971/b059g.pdf

 

Most 3 flutes have 1 tooth to center and 2 that are relieved.

For 4 flutes they are generally 2 to center and 2 relived.

 

I asked Mitsubishi to consider making a 6 flute ball with 3 to center and 3 relieved (still waiting, haha).

 

 

 

I've used 3" indexable cutters to surface a slope on a three axis setup, and I was able to get good finish with a pretty large stepover.  You're never cutting with the center and it acts like a noticeably larger ball.

 

The zero SFM is only a problem with ball cutters.

For bull nose (and square) tools tilting the tool gives the effect of a much larger radius on the bottom of the tool.

This is called Sturtz milling or P-Milling.

Figure 13 in the image below shows it quite well.

While the image shows the tool being tilted if you machine a slope in a 3-axis setup then you are getting the same effect

 

[AMCNitro]

I only use a ball nose if I have a feature that requires it, for surfacing I rather use a bull nose or even flat sometimes.  For roughing you're going to go a lot faster with a bull or flat, the ball nose hates to be buried, you're using a lot more surface area when you rough with a ball.

Ive never done any 5 axis(dream of mine...sigh...) but I've heard that if you must use a ball nose and have 5 axis you should tilt the cutter as to not use the tip.

[crazy^millman]

 

Ive never done any 5 axis(dream of mine...sigh...) but I've heard that if you must use a ball nose and have 5 axis you should tilt the cutter as to not use the tip.

 

Yes I like to give anyway from a 5 to 30 deg kick when surfacing using a ball endmill. You would no problem doing 5 Axis Programming.

[AMCNitro]

Yes I like to give anyway from a 5 to 30 deg kick when surfacing using a ball endmill. You would no problem doing 5 Axis Programming.

Yes, but first I have to get near a 5 axis machine...   Thanks for the compliment Ron!

[Matthew Hajicek - Singularity]

I like figure 10.  Two depth cuts in one pass!

[dstryr]

Helical makes a 3flute ball with all 3 flutes ground to center. Works very well in the aluminum I've cut.

[dstryr]

Has anyone tried a PCD ball endmill from Harvey tool for dedicated finishing in alumium?

http://www.harveytool.com/prod/Browse-Our-Products/Application-Specific-Designs/Diamond-Tooling_190/PCD-Diamond-End-Mills---Ball_99.aspx