Types of technics you guys use for milling deep cavities

[X-L Engineering Corp]

Types of technics you guys use for milling deep cavities in Alum,

Largest cutter 1/4 going 1.5 deep

3/16 going 1.750 deep

smallest 1/8 going .900 deep

 

Thanks for any suggestions

 

Ted

[mkd]

ramp entry followed by small (<10%dia) radial stepovers?

[crazy^millman]

That is not all that deep should be okay with Optirough or Rest Rough.

[Rotary Ninja]

That 3/16" depth is going to suck. The others aren't so bad. I always rough with the biggest tool I can and work my way down. For the finish pass I lower the RPM on long tools. Conventional passes sometimes help with taper.

 

After I get everything roughed in and am ready to finish I usually will try to get any vertical walls finished to the top of the stock left on the floor of my pockets. Then I finish the floor from the center out.

[Bob W.]

I have have had great luck taking a high feed approach when the cutters get long and skinny like that. I will do a .025" step down with standard or faster feed rates and it keeps chatter down. Dynamic style toolpaths are great for this as well because they don't overload the tool and set off chatter. With the 1/4" tool I would start with a Dynamic area milling toolpath with a 50% stepover and .025" depth cut. I would helix in and feed at 100 ipm @ 10k rpm. This would be after going as deep as you can with a standard length cutter and normal parameters. I would then finish with a ramped contour. This is how I would approach the part but it usually takes some experimenting to find out what works best.

 

I like to finish the floors first, leaving .03" to the walls, then finish the walls all the way down to the floor.

[djstedman]

I find having a relieved shank and only leaving about .05 to .100 length of flute reduces tool pressure and chatter a lot.

 

Once the tool is relieved ramp down about .025 / .030 and adjust surface footage down till you find the right balance between speed and surface finish.

 

This has worked for me doing slots and pockets as deep as 10 times diameter, though sometimes they take longer than I would like.. would be nice if engineers would always make inside corner radii as large as possible - seems the aerospace ones love to choose pretty arbitrary sizes with no thought on if its possible to make the parts or not.. makes things challenging though and challenging keeps things interesting..

[Chris Rizzo]

Ramping and 3-flute cutters.

[X-L Engineering Corp]

I'm tying pocket toolpaths @ 50% depth of cut this seems to be faster than the dynamic toolpaths then I always ramp mill to finish the walls but never more than .025 on the depth. I'm going to run this in a Robo-Drill with 24k.

[Müřlıń®]

Ramping and 3-flute cutters.

 

+1

[MWR15]

Depending on the shape of the area you are milling you may need to turn on the trochodial motion option.