Removing aluminum stock fast or drill vs end mill...

[zaebis]

With my little benchtop CNC mill I have to be patient while separating my part from its stock. So I was thinking if I could drill a bunch of holes (drilling cycles with drillbits) to remove chunks of material before zipping through with endmill. I am under the impression that drilling is more efficient than endmilling for removing the same amount of material.

Also my endmill will not have to engage at full surface and will be cutting at 25-60% contact with material so I will feed it fater.

Or may be for circular pokets it would make sense to predrill and then interpolate the rest with a boring tool.

Again the onjective is to remove chunks fast and then finish with endmill(s) going faster.

Am I on a right track to reduce the cutting cycle?

[Lexx0001]

If the size of the drill bit is a significant portion of the pocket, it might be worthwhile, especially if there are a lot of pockets to mill. Otherwise it would seem that there would be a lot of time going from one hole to another. That's just my 2¢.

Bill K.

[vision-cnc]

It has been my experience that milling is faster than drilling even though theory says otherwise. Here is why. Chips chips and more chips. When you drill you get chips wrapped around the bit or have to use a peck cycle. Both consume feed time to either stop and remove the angel hair or peck drill. The only exception I have found is small cavities and that is simply to reduce the lateral load on the cutter. I only have a 7-1/2K spindle, now if I had a 12K spindle things would be different.

[kling8]

I've found the fastest ways to remove metal is saw, drill, then mill, so I would drill the holes to speed up your time. I have done this on many parts. Depending on application.

[Geof]

Originally Posted by zaebis With my little benchtop CNC mill I have to be patient while separating my part from its stock. So I was thinking if I could drill a bunch of holes (drilling cycles with drillbits) to remove chunks of material before zipping through with endmill....... .....am I on a right track to reduce the cutting cycle?

You might reduce the time, although that is questionable, you will also probably degrade the appearance. As the milling cutter goes through the drill holes the deflection varies so you finish up with humps and hollows matching the hole locations. This means you may have to take a finishing pass to get things smooth and if you have removed the part from the stock that is going to be difficult.

[rigo430]

From what I've heard the fastest way to remove a large amount of material the quickest in some of the harder steel's drill roughing is the fastest way and they even make special cutters to do it. On softer metals end mills maybe faster due to constant cutting if you use the right cutters.

[vision-cnc]

Geof has a valid point. When you drill then mill you get deflections that need to be addressed, usually with multiple finish passes. The other point if we want to get down to the small points. Imagine a a block that has just been drilled full of holes for fast stock removal. Assuming you are using a standard drill, not a rigid spade type, then you will have a block with holes that resembles a shower drain. Okay, now imagine the milling cutter moving through this area. Odds are at some point the cutter is going to be in full contact (in the web between holes) just as if no drilling had been done. Therefore you have to set your feed and speed for worst case scenario. So you are still milling at the same rate as if you had not drilled. If not then you hear those awful sounds. "Tick" for 1/4" and under endmills. "Snick" for up to 3/8" endmills. "Snap" for up to 1/2" endmills, and "Wooom" for 1" and bigger endmills. Use lots of coolant. I have a cool video of a ramp milling operation where we were rolling along and I said "let me turn the coolant off so you can see the cutter better to the guy filming. It was a 1/2" ISCAR (I$CAR). Yup "Snap". If I can find it I will put it up here. My friend edited out the words that fell out of my mouth so I will be able to post it here.

[crabbass]

I believe "plunge milling" is only faster, or applicable to deep cavities where a conventional (radial) milling tool would have to be mounted with a high diameter to length ratio. I have never used a benchtop cnc, but I can imagine they are not the most rigid things. However, the spindle bearings in most machines can usually tolerate a larger axial load than they can a radial load. If your machine or setup simply isn't rigid enough to perform the end milling operation at optimal speed/feed/doc, plunge milling might work for you. When I say plunge milling, I am referring to using the endmill in a drilling cycle, but decreasing the step over to less than 1/2 of the endmills diameter, therefore you wouldn't have to rough mill the pocket afterward, just finish.