What's new
What's new

Deep pocket finishing

tcncj

Cast Iron
Joined
Dec 15, 2016
Hello
I need some advice on "deep pocket" milling in 6061.
The part got 50mm walls. We rough everything out with a long neck roughing endmill.
But what about the finish passes?
I can't use an endmill bigger than 14mm because of the corners (8mm radius). I don't want to use a 16mm one because it will chatter in corners.
Two tooling reps don't have a carbide endmill long enough to do the finish pass in one z height.

What I could do is finishing in multiple z depths but it will leaves lines I guess? No experience with it. Normally our parts aren't this high.
One tooling rep recommends a HSS-E-PM endmill for finishing in one pass. But how good will the HSS endmill hold up? Again no experience with HSS, since we always run carbide.

Any advice on this is appreciated :)
 

AD Design

Stainless
Joined
Jun 27, 2012
Location
Tennessee USA
HSS cutter will work just fine on 6061 provided the cutter is sharp and you get chips off the cutter and out of the pocket. Re-cutting chips, especially those that cling to the cutter for another revolution, can leave marks on the pocket wall and affect accuracy. Use a good coolant suitable for aluminum, about anything is better than running dry. Rough pass and remove chips, finish cut will produce fine needles. Use proper f/s and HSS will hold up well. We used to use tapered HSS to cut the draft on medium sized CorningWare molds made from Waspaloy with good results. Rough out whatever diameter cutter you wish and leave the corners for appropriate sized cutter if that speeds the cycle time.
 

tcncj

Cast Iron
Joined
Dec 15, 2016
50mm height parts is for us not daily work.
I understand there are always people who do different work and have far more experience.
So what's your advice? ;)
 

Hazzert

Stainless
Joined
Dec 21, 2014
50mm height parts is for us not daily work.
I understand there are always people who do different work and have far more experience.
So what's your advice? ;)

He has to go ask his spreadsheet...

I would try a ramp down contour pass. It will provide a wiping action when it gets to the bottom of the contour and will effectively take a spring pass.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
I would go with the z-steps and a quick ramp-in near the corner entry. That way any entry/exit step will be less noticeable. Make the lengths of cut in equal z-steps so that tool pressure will be as close as possible to the same on every pass. Lines should not be an issue this way as long as your machine is in good shape and your cutter is straight and sharp.
 

tcncj

Cast Iron
Joined
Dec 15, 2016
He has to go ask his spreadsheet...

I would try a ramp down contour pass. It will provide a wiping action when it gets to the bottom of the contour and will effectively take a spring pass.

Just tried it in my cad/cam package and should work!
I will let you know how it turns out
 

tcncj

Cast Iron
Joined
Dec 15, 2016
The ramping works but it does leave lines...not a big issue though. But I expected an almost perfect finish.
Ramping overlaps so that shouldn't be the issue.
Cutter is new
 

Finegrain

Diamond
Joined
Sep 6, 2007
Location
Seattle, Washington
I always see lines when I ramp or step, with a square-end endmill.

Might try ramping with a bullnose endmill, then finish the very bottom with a square-end endmill.

Regards.

Mike
 

Finegrain

Diamond
Joined
Sep 6, 2007
Location
Seattle, Washington
Oh :o.

Then my next possibly useless advise is to try a brand new YG-1 Alu Power 2" LOC x 1/2" (or metric equivalent) endmill, and don't go too slow, or the tool will chatter.

Regards.

Mike
 

Mechanola

Stainless
Joined
Mar 21, 2011
Location
Äsch
Shit part. A two-parts assembly would be smarter, doweled and secured by screws. Then perfectly sharp edges and corners can be had and the smoothest thinkable bottom surface. Really now.
 

DethloffMfg

Cast Iron
Joined
Sep 22, 2018
Location
Portland, OR
Oh :o.

Then my next possibly useless advise is to try a brand new YG-1 Alu Power 2" LOC x 1/2" (or metric equivalent) endmill, and don't go too slow, or the tool will chatter.

Regards.

Mike

The Alupower I've been playing with leaves a beautiful finish, especially floor finish. But man they are not rigid tools, I have to take at least 2-3 passes at 20ipm to get .020" off with a .25"x1.25" end mill.
 
Joined
May 3, 2016
Location
Findlay, Ohio USA
I have a customer making carburetors out of 6061. It has a pocket around 2” deep that has quite a bit of material that needs removed probably 10-20 cubes (just a guess) he has made over 1,000 with one (as in one single tool) of these

Helical 3 flute high balanced coolant through end mil

As you see they are very expensive but they are worth it. As a tool salesmen I don’t like it!:D I don’t sell him 1/2” endmills any more. Previously they were using Yg-1 AluPower then Helical 45 degree helix aluminum specific end mills but now this is king!

That said those cutters leave an awesome finish on the sidewall & floor!
 
Last edited:








 
Top