Hmmm... Endmills deflecting?

[Driftwood]

Hello all...

I found something strange when I was running some pockets in aluminum. I had to do 2 pockets, more or less 1" square with a 1/16" radius in the corners, so I ran it with 1/4" carbide endmill followed by a 1/8". One pocket was .1" deep, the other .03"

Well, when I looked at the finished pocket, the 1/8" endmill cut several thou lower than the 1/4", hard to say how much, but I'd say 4 or 5 thou. When I reran the 1/4" endmill, it cleaned up the excess, but I'm having trouble understand why it left it in the first place. Any ideas?

I ran both tools at full depth. The 1/4" was 5000 rpm and 20 ipm and left .005" on the wall for the 1/8" endmill to clean up. The 1/8" ran at 5000 rpm and 10 imp.

So any thoughts?


And while I've got your attention, here's something I've always wondered: Do you use 4 flutes when slotting or plunging or do you find them to be particularly bad for this?

[StealthDumpKits]

I'm not a machinist, but were you climb milling or conventional? When was the last time you checked the X & Y backlash?

[pastera]

How is your backlash in Z? This could easily answer the issue of the 1/4" riding higher than the 1/8" EM.

I use a 2 flute for slotting/pocketing but I am also running on what should be considered a toy (SEIG X1). With a 1/2" 2-flute EM I can slot 0.025" deep as fast as I turn the handles. With a 4-flute, same brand/size, it jumps around and chatters like crazy under the same conditions.

Aaron

[StealthDumpKits]

...looks like two problems. Might be tool offsets related.

[Driftwood]

Well, I'm running on a CNC mill.

I checked the offsets and they were fine. I'm not really sure how to check the backlash, anyone suggest how?

Assuming its not the backlash (and I don't think it is), I'm leaning more towards the endmills deflecting or something... does that make any sense at those speeds and feeds?

[widgitmaster]

Its the Long Endmill that seperates the man from the machinist!
In theory they look simple to use, but rarely behave as you would expect at full depth of cut! They flex, chatter, and snap without warning!
The problems are a lot more obvious than the solutions, and it takes a while to learn just how much they can be pushed before problems show up!

I have had brand new high grade long 4-fl endmills with 4 totally different fluts! The grinding wheel was breaking down as it sharpend the primary flutes, an left each flute with slightly more metal than the last! That was the endmill from hell!

As for milling deep pockets, sometimes you have to re-run the program to do the pocket walls several times, just to get the taper out. Then you can see the results improve.

[kalmah]

Originally Posted by Driftwood Hello all... I found something strange when I was running some pockets in aluminum. I had to do 2 pockets, more or less 1" square with a 1/16" radius in the corners, so I ran it with 1/4" carbide endmill followed by a 1/8". One pocket was .1" deep, the other .03" Well, when I looked at the finished pocket, the 1/8" endmill cut several thou lower than the 1/4", hard to say how much, but I'd say 4 or 5 thou. When I reran the 1/4" endmill, it cleaned up the excess, but I'm having trouble understand why it left it in the first place. Any ideas? I ran both tools at full depth. The 1/4" was 5000 rpm and 20 ipm and left .005" on the wall for the 1/8" endmill to clean up. The 1/8" ran at 5000 rpm and 10 imp. So any thoughts? And while I've got your attention, here's something I've always wondered: Do you use 4 flutes when slotting or plunging or do you find them to be particularly bad for this?

For slotting aluminium, 2 flute is the best !! It works too for shouldering. DUring maching of aluminium, the most important things is the place for the chip, that's why a lot carbide tool manufacturer have 2-3 flute end mill for aluminium.

[dertsap]

Originally Posted by Driftwood Hello all... And while I've got your attention, here's something I've always wondered: Do you use 4 flutes when slotting or plunging or do you find them to be particularly bad for this?

four flutes not designed to plunge , ramp in if anything
, it is not uncommon to remove some material with a spring pass but it sounds like youve got a pretty heavy taper , it may be worth adding a spring pass to cleanup the extra

[big_mak]

Ive gotta ask, `What is the floor thickness at the bottom of the pocketÉ

Can your machine go any faster RPMÉ

Where I work, we`d just use the .125 endmill for the entire pocket, that way you don`t have to worry about blending two cutters. Or else we`d run the second cutter 0.002 inches higher that the first.

As far as deep pockets go, for finishing the walls, I`d use a long reach endmill with relief ground after the cutting length. Say if you are gonna take .25 inch deep cuts, relieve the cutter so the flute are a max of 0.3 insches long. This will reduce your area of contact, and should help keep your walls nice and square.

[HuFlungDung]

The toolholder, the spindle rigidity, the diameter of the endmill, the length of the endmill, the feedrate, these factors all contribute to how much the tool leans in the cut. Endmills will bend back in heavy cutting and this pushes the corners of the flutes down into the work to some degree. So a small amount should be left on the floor of the pocket for a light finish pass wherein this effect is minimized and you get the true accuracy out of the tool height setting.

Also, the method used to set the tool length offset can have an effect on how accurately all the tools are set relative to one another.

[Precise1]

Good advice so far, here comes mine... Slotting 2, maybe 3 flute if it is designed for the material. Avoid 4 flute like the plague !!
Your endmill depth issue sounds material deformation roughing with the 1/4 inch/pushing z upwards (how heavy/rigid is the machine?). Thats the main reason to see .004-.005" step that is removed after rerunning the 1/4" em, other than the part lifting up a bit which I have dealt with often enough...