I am coming up with:
27ipm
2 flute .5 carbide endmill
6061-T6
3640rpm
.050 DOC

this feed (27IPM) seems very slow to me.

Opinions/suggestions ?

Thanks
Ken

Ken,
The basic feed rate for endmills is the feed per tooth, expressed as inches per tooth. There are many factors to consider, cutting tool material, the material to be cut and it's hardness, the depth and width of the cut, the type of cutter, finish desired, rigidity of the set up, the machine itself. There is no formula to resolve these factors.
However there are guidlines to follow, as a cardinal principle, always use the maximum feedrate that conditions will permit, avoid using a feedrate that is less than .001 inch per tooth because this will result in a decrease in tool life. A 1/2 inch endmill using a depth of cut of .050 in aluminum varies from .002 to .005 inch per tooth, depending on the condition of the material.
More often than not, using formulas from the refernce books just don't reflect the real world. Many times the recommended rpm far exceeds the capability of the machine itself. Using a simple shop floor rule of thumb:
RPM x #of flutes x IPT (inch per tooth) = IPM (inch per minute)
So if the most you can get out of your machine is 3500 rpm, using a two flute endmill and starting with .003 inch per tooth, you would end up with 3500 x 2 x .003 = 21 inches per minute feedrate.
The biggest detriment to heavier feedrates with softer materials is the ability of the tool to effectively eject the chip. It only takes a millisec for the material to weld itself to the tool and we all know what happens next. That funny noise that causes heads to turn.
caitolly

Thanks for the information caitolly, seems that the settings may not be that far off. Perhaps I can decrease the machining time by increasing the DOC, would you think .075 DOC out of reason for a commercial machine?
This is not a production run so 1 hour or two it does not matter, this information is just for optimizing machining time.

Thanks
Ken

Ken,
If you setup is pretty solid and your machine is also, you could probably go as deep as .250 using the same feedrate. Depth of cut has the least effect on tool life, you should always use the heaviest depth of cut possible. After the depth of cut is about ten times the feedrate, it has no significant effect on tool life.

I have only been at this about a year and a half, and this feed /speed/DOC still seems a mystery to me.

For this job .050 seems on the conservative side so I will increase and see how it goes.

Thanks again
Ken

Ken,

In my experience, when hogging aluminum a deeper cut can bite you if:

The cut is a full-width cut and the chips don't evacuate and, instead, pile up around the end mill. What happens is, the coolant can't get to where the action is and you can wind up with a molten mess clogging your flutes and breaking the tool. It sounds counter-intuitive, but shallower cuts at supercharged speeds and feeds often result in more parts and fewer problems.

Where did you get those speeds and feeds?


Mike

Hi Mike,
I got the chip load from your efforts and my CAM software calculated the rest, which are essentially identical to your ME Consultant 2.0 calculations.

There does not seem to be a great deal of guidelines/suggestions for light cuts and fast feeds.

Thanks

Ken

Ken,

When I run ME Consultant and calculate a .500 2 flute carbide end mill, .500 wide x .050 deep cut in 6061 wrought aluminum, I get 6723 RPM at 36.5 IPM (880 SFM at .0027 IPT).

Have you modified some of the machining data in the ME.dat file? If not, could you send me a screenshot so I can figure out why we're getting different numbers?


Mike

For roughing at a shallow depth like that, your chipload could likely be .010" to .020" per flute. The finer feedrates are for achieving a desired finish and minimum tool deflection.

Ken,
I would suggest that the other gentlemen are on target also, there are just so many variables it's difficult to offer guidence without actually standing there with you.
What kind of machine are you using anyway??
caitolly

The machine makes a difference, at work we push 1/2" 3flute carbide 6500rpm 60ipm through anything, theres small 1/4" wide sections of 1" thick we push it strait through, doesnt sound the greatest but it does it without asking questions, otherwize taking 1/4" passes and 1/2" passes in some parts. This is on a Haas VF-3 and I think series 2000 aluminum(Im not completely sure, I think thats what boss said) The stock was cut too long and plunged that 1/2" EM at 40ipm, that made a LOT of noise but it held up.

I am told you want to get full chip load(meaning cut as fast as rated) with carbides, but the depth could be the limiting factor to the machine.

Jon

I've found that 3 flute end mills are the best choice for slotting, whether in aluminum or steel. Sounds like yours are making some major chips!

Mike -
Our different results are explained in that I have a 4000rpm limit which put the IPM at 21 with the same DOC and cut width as you entered, when I bumped it to 7500RPM I came up with the same specs as you did.

caitolly -
Lots of variables, I agree, and I am learning it's not all science, who is that says that? :)
My machine is a Haas toolroom mill.

JFettig -
I think I will be a wee bit more conservative :D

Thanks guys
Ken