Machining Deep Profiles

[Babba]

I'm trying to improve the finish on some deep profiles I need to machine & as they are taking 30mins+ each I need a little advice from experience rather than set about experimenting blindly & losing a lot of time + needing a larger scrap box.

I'm starting with a 70mm X 70mm X 25mm 6062 alloy blank & need to profile this the full 25mm depth in a complex curved shaped (like say an egg) but with straight sides.

I'm using a 10mm carbide 2 flute cutter (still sharp after 1yrs+ service doing similar) spinning at 3500rpm.

I'm taking 2mm deep passes at 102mm p/m. The final pass of 1mm is also cutting into the whole side of the profile by 0.25mm.

After experimenting I've managed to lose the horizontal ridges that showed each step down but I'm now getting vertical ridges which I'm assuming is caused by flexing of the machine and/or the tool.

I'd like to use a 12mm+ cutter but can't source one as economical as my 10mm (£8ea). (Due to an inside radius 12mm is the max)

Is there any aspect which I can concentrate on to minimise these vertical ridges??? They will easily sand/stone out but I'm really looking forward to a finished part straight off the machine.

[Gregory B]

To get a better finish Try a 0.2mm or a 0.1mm step over with a 0.2 mm depth of cut at 350mm per min or 400mm per min with a 6mm dia ball end 3 flute cutter, this is what I use.
Greg

[neilw20]

Seven roughing down to 0.5mm from the bottom 3.5 depth of cut leaving 0.25mm makes 7 passes. Use air or preferably coolant, so chips don't get recycled. You should be able to rough at least up to 150mm/min or even 200.
Take one pass all around taking off another 0.15mm leaving 0.1mm for the finish cut. Final pass at Z-25.1 or -25.2 at 30mm/min
If there are any sharp corners in the profile make sure you don't just stop moving in X then start moving in Y. Going around corners you need to keep a constant chip load so that the cutter keeps bending/deflecting the same amount, so the path around a sharp corner is an arc. If moving into a corner and backing out pause for about 1 second before backing out. The bending of the cutter has to catch up. If your 2 flute cutter is really thick and stiff in the middle you could even use 5mm DOC. 1/2 diam of cutter should be OK.
Plenty of Speed, Reasonable Feed, Flood coolant. The chips getting recycled is what will do the most damage. 3500 rpm x 0.025 chip x 2 flutes = 175.
Go for 250 if the vibration is OK. Keep the HEAD LOW, Gibs firm, Short Cutter. 3500rpm or more.
Once machine/cutter deflection equals chipload is when the chatter sets in as the cutting becomes unstable. Also you should be climb milling. If not climb milling you are guaranteed a S#!T finish. Cutting away from you the waste part should be on the left and the finished part on the right for a clockwise rotating cutter. That makes each chip cut from full load at the front of cut to nothing at the side of the cut and any swarf get eaten on the waste side.