[skray775]

I would go to a 2 flute. The 4 flute is going to have a hard time evacuating the chips without re-cutting them
and clogging.

.06 should be fine if you ramp down into the material.

[brow318]

Any suggestion on ramp setting? Cut2D allows me to set a length of the ramp or plunge. Right now I have it set to .125".

[SCzEngrgGroup]

Personally, I always prefer going deeper and slower - you'll get a higher MRR. For a 1/4" tool (HSS is fine for this), I'd be cutting 0.125"/pass, 5000 RPM, 20 IPM. You DEFINITELY want to be using a 2-flute, not a 4-flute (I never use 4-flutes on aluminum). For finishing, take off 0.010" at 35 IPM, at full depth. Flood coolant will no doubt help, but should not be required for this fairly easy cut.

You absolutely want to ramp, rather than plunge, wherever you can. I'd recommend at least a 45 degree ramp - i.e. - the "distance" at least equal to, if not greater than, the depth.

Regards,
Ray L.

[tbaker2500]

I can't quite tell from the picture- did the tool break?
What do you mean by the x0y0 got out of sync?

61ipm is was to fast. I'd suggest going into "advanced" mode in G-wizard, and look at tool deflection. If your tool is deflecting more than 1thou, you're in trouble. It marks that in orange. Make sure you enter the tool stick out for this to work.

Ramp in .125" is fine. For DOC, reduce as needed until g-wizard say's you are in the clear for deflection. I'd also recommend using setting 2, instead of the default 3, for how aggressive the cut is.

4 flutes is going to have a harder time clearing the chips out, and they can weld to the cutter, making it dull and causing it to break. But if you go slow enough and use flood coolant, it should work fine at that DOC.

[LSM]

Well what happened is you melted the aluminum that loaded the tool up and it stopped cutting. 1/4 inch stock with a 1/4 inch em needs flood coolant the spindle speeds for aluminum tends to melt it if you don't run flood cooling.
You aren't really profiling with those cuts more of a slot cutting operation, so need to use a chip load for full cutter engagement .
A 1/4 inch cuter will only take so much side load about 0.001 maybe .002 chip load is all it will take. in that size you can get carbide for about the same price as HSS and it's a bit stiffer.
A good starting point would the the manufactures recommended chip loads for the tool smaller diameter smaller max load

[zero_divide]

I second what Himmy said.
You should be using a 2 fute carbide or HSS endmill.
With flood coolant i notmally go 5000rpm 24 ipm, 1/8 deep full slot.

Without coolant all bets are off, but i would suggest 3000rpm and 16 ipm same doc.

Good luck.

[kevinro]

On the setting for the ramp, there are many valid ways of thinking about it. I tend to have my students stick with 4 x depth of cut as a rule of thumb. They have very good outcomes with that with that.

Sent from my GT-P5113 using Tapatalk HD