Speed and feed ball end mills?

[FP1]

A little help with speeds and feeds for ball endmills. What do some of you recommend for speeds and feeds for a 1/2 diameter solid carbide 2 flute ball end mill roughing 1018 cold rolled steel. DOC, RPM, Feed rate? What is a good rule of thumb for this.

[MLS]

Personally I would try to avoid roughing with a ballnose if at all possible simply because the surface speed of the tip of the ball varies so much relative to the tangent of the ball at the flute.

 

That might not help you much though...

[Mike S @ S4A]

exactly - Q: could you do your initial ruffing with a bullnose? (asking blind w/o seeing the part...)

[Jack Neelands™]

What is it that you are cutting if we may be so bold as to inquire...slot?...how wide, deep and long....standard length ballnose will cut a basic slot that is 12 inches long at 1600 to 1800 rpm with max .05 depth of cut on a ramp at 45 to 60 inches a minute...depending on your setup and the length of the slot...ball noses dont like to plunge and have a habit of blowing up

 

3D geometry roughing maybe?

 

the tip of the ball nose is considered a dead Zone for cutting and from what you have there in your sig...you have multi axis....can you tilt the tool on angle so that you can avoid the bottom of the tool somewhat?....

 

Is the cutter a variable ball nose(makes a difference when cutting side cuts)

[ReDEyZZ]

What is the application?

 

a slot? if so how deep?

 

surfacing?

 

 

A 4 flute may work better in that material, but if all you have is a 2 flute.....

generally 200-300 sfm depending on the make.

 

For slotting go around .006" per rev at around a .100" depth of cut.

 

Ball end mills need a lighter cut once you get past the full radius generally.

 

If it is surfacing , you can prolly get up to 400-500 sfm if the chip load is light.

 

Like others said..rough as much as you can with a reg endmill if possible.

[FP1]

Well its just a shallow concave surface on the top of a flat block, kind of like the egg shape lens from a pair of eyeglasses. Thats why I was thinking of a ball end mill to rough it out. Its about 1-1/2 wide x 2-1/2 long x .5 deep cavity. Has to be done on a 3-axis vmc for now.

[Jack Neelands™]

Rough pocket ..... .05 stepover....05 depth of cut...50 inches a minute 1600 rpm .... .02 material left .....then surface finish .02 stepover(semi)...leave .005 stock for finish pass......depending on the finish you need use another ball nose ...4 flute would be better.... .0025 stepover 1800 rpm @60 inches a min

 

HTH

 

*The thread you started indicates that you are not familiar with cutting steel so these are safe values for you to work with.*

 

Please note that HSM requires PROPER TOOLING and PROGRAMMING APPLICATIONS and must be adhered to, this post does not infer what other's use or apply to their machines presently at this time.

[FP1]

Thanks for a starting point Jack. Thats all I was really looking for. I am actually familiar with speed and feed calculations for many materials including some of the exotics in 2D applications. I just don't have much hands on cutting experience using ball end mills and surface tool paths. I have only done it 3 or 4 times, one piece each time. Do you still think it would be better to rough out the shape I described with a smaller bull nose end mill? What diameter would you try?

[Jack Neelands™]

If you can get in there with a 3/8 endmill with a .02 rad on it that would work much better...you still have to ramp the tool into the metal with the roughing program ...make sure that all your rads will clean up...just in case they are smaller than .25