speeds and feeds again

[mofosheee]

Hello
When cutting a pocket, I am experiencing excessive chatter focused in the mill head that I believe this is due to improper feeds.  Thinking that too fast = bad,  I decrease feed and am not observing the reduction in chatter that I expected.  Online readings lead me to believe that perhaps my feed rate is too slow.  Being a big chicken, I am hesitant to just ramp up feed and cut away.   The variables as follows........

Using Cambam and HSM adviser,  inputting; 7075 T-6 Al
2 flute, .375" carbide end mill with 2.125" stick out @ 3500 rpm
going .025" per pass to a depth of -0.960"  using default cross and step over

HSM is outputting 15 ipm feed rate.  I am using a plunge rate of 5 ipm.

When loaded into Mach3 I have an initial feed rate of 50% which equates to 7.5 ipm.  My intent was to ramp up feed rate as cutting progressed but the chatter caused me to back off and stop.   Am i going too slow?

Thank you

Jerry

[lloydsp]

Chatter is usually a sign of bit flex or work movement. 

Although that's not an unusual stickout for a 3/8" diameter cutter, 2-flute cutters have a lot less "meat" in the center than 4-flute types, and therefore are more flexible.  Moreover, each cutter has its own inherent resonant frequency.  It is anchored rigidly at one end, and free to vibrate at the other, forming something much like an harmonica reed.

Often, minor chatter can be alleviated by changing (up or down) the spindle speed, so that the tooth-rate doesn't correspond to the resonance of the cutter.

LLoyd

[Bubba]

Based on.003" per tooth chip load you should be able to cut @21 ipm.. Try it, but keep your hand on the feed override to adjust as necessary.

[mofosheee]

Thanks Bubba

Speaking of "meat", I have a 4 flute rougher the same size that I'll try tomorrow.   Considering the dimensions I probably should have started off with one in the first place

Conventional for roughing?
Climb for finishing?

Jerry

[lloydsp]

Jerry, that's the conventional wisdom about roughing and finishing.

With any flex of the bit, or play in the spindle, and with some aluminum alloys (or other metals that tend to 'hog') you might have to make the last roughing cut in climb, too.  That's because in conventional, it will be cutting deeper than you expect.  Of course, in climb you normally would take light cuts.

Climb and conventional were originally made such a big deal of because of play in the leadscrews/nuts of manual machines.  Too deep a climb cut would result in the whole bed being pulled to the opposite limit of lash in the screw, causing damage to the finish.

This still holds true on manual machines, or 'single-nut' CNC machines.

LLoyd

[klystron]

hello lloyd

[lloydsp]

Good morning, Yves!
Lloyd

[Bubba]

In your case I don't think the.375" carbide tool is deflecting much. The overall machine rigidness and tightness have more impact on your finish than cutter deflection. Everything above .250" is nothing to be concerned about as long as the feed and speed in relation to the depth of cut and kind of material is machined. I would stay with 2fl cutter, because of its geometry(usually higher rake) is is better for chips removal. As Lloyd suggested, keep everything short and make this a common practice.. I do! Always, as long it is possible keep everything close to the machine column,Quill short, etc..

[Garyhlucas]

As Bubba said "keep it short". A cutter half as long is 4 times stiffer. A cutter that is twice as big in diameter is four times stiffer too.

On small machines spindle power is often the limiting factor. When I firts built my CNC mill I used a Sherline spindle and then found out it's continuous rating was just 60 watts! Now I have an 1800 watt tread mill motor on an R8 minimill spindle. What a difference. 

If your spindle is 120 vac consider getting a Kill-A-Watt device. It shows true power and can really teach you how to optimize what you are doing.

[mofosheee]

I changed to a rougher and the resonance went down greatly.  Tool stick out was always keep to minimums.   As Bubba stated he didn't think deflection with the original 2 flute / .375 wouldn't be significant.  Either did I,  but it is what it is.............

Considering that the pocket has been roughed out and for my finishing pass,  would someone please comment on my thoughts of increasing the cut depth increment from .025  to a greater value?

Thanks again to all who responded.

Jerry

[Bubba]

 would someone please comment on my thoughts of increasing the cut depth increment from .025  to a greater value?
****************
its all depend on how rigid the machine/ setup is. I know on some machines .25" depth cutting steel is not a problem,but you case maybe different. I say try it, to start keep the feed override slide down to about 25% of the programmed feed rate, and then bump it up till you like how it does. Only you be able to tell because you are the one who is running it. I can only speculate knowing nothing about your machine.. Good luck.    

[lloydsp]

Mo,
Often, I'll use a "high spiral" cutter, and finish at full-depth.  I don't like the thread-like finish marks that a spiral or stepped finish can produce.

When I do such, it's usually at a much smaller feed rate than called out for the cutter, and always in climb.

LLoyd