Got a rectangular pocket, 6061 aluminum, need 0.25R corners. I can drill them to begin with, pocket with a 3/4 end mill, but then I have some rest machining to do and the drilled finish isn't great. I tried a long 3/8, chattered like a mad woman. As does a long 1/2 when it hits the corner. I tried a reduced shank 3/8 (3/4 LOC), same result. Tried climbing and conventional. Also tried plunging the corner at the end. Any tricks for this?
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
How to make 0.25R corners 2.5 inches deep in a pocket?
- Thread starter swarf_rat
- Start date
- Replies 41
- Views 9,455
Zahnrad Kopf
Diamond
- Joined
- Apr 5, 2010
- Location
- Tropic of Milwaukee
Manipulate the feeds in the corners if your CAM will allow you too. ( PowerMILL does ) If not, you can trochoid the corners. Also, you can leave rest stock and helical bore the corners in small step downs. There's a billion ways, but those three pop to mind immediately.
Krovvax
Hot Rolled
- Joined
- Mar 5, 2012
- Location
- Quebec, Canada
maybe reaming the hole instead of drilling in 6061 reaming is not a long task and will give you way better finish.
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
What kind of endmill are you using? Buy a 35* Helix tool. This isn't that bad...I do some pockets with a .250 radii 3.5" deep in 6061. You need a 1/2 tool , 5/8 flute, necked 2.5" and finish in .500 dp steps.
Reaming the bore would improve the finish of the radius itself. I am using HSM paths, as soon as a 1/2 tool hits the 1/4 radius hanging out 2.5 inches it begins to sing. No feed seems to make it better. The rest material is actually pretty thin at the junction of the 3/4 HSM pocketing and the 1/2 bore. I tried using a 1/2 and arcing through a larger radius (0.26) but it was unstable enough to mark up the corner radius. The necked 3/8 was even less stable. I can't helical bore a 1/2 hole with much bigger than a 3/8 mill. I don't have a necked 1/2, of course that would be a lot stiffer than the 3/8. If others are doing this clearly I just need to keep trying.
zero_divide
Stainless
- Joined
- Feb 2, 2012
- Location
- Toronto
Rough them out, leave some material. Everywhere.
Leave maybe 5 thou per side.
Get that half inch endmill and at slower spindle speed , but heavy feed plunge it into the corners.
Then come back and finish the wall MAKING SURE you keep a small arc in the corner.
I am using niagara's 3 flute hihelix endmills and this seemed to work.
Leave maybe 5 thou per side.
Get that half inch endmill and at slower spindle speed , but heavy feed plunge it into the corners.
Then come back and finish the wall MAKING SURE you keep a small arc in the corner.
I am using niagara's 3 flute hihelix endmills and this seemed to work.
Tolk
Plastic
- Joined
- Aug 9, 2013
- Location
- Georgia USA
I'd go with the reamer plan. If your tolerance allows give yourself an extra half a thousandth or so on the radius so the endmill is just cutting air on the corners
Greg White
Titanium
- Joined
- Jan 22, 2007
- Location
- Pinckney Mi.
Slow down, get outa HSM, it should work fine wit a 1/2 enmil.
Send in to a mold shop.
Gw
Send in to a mold shop.
Gw
allloutmx
Titanium
- Joined
- Mar 6, 2013
- Location
- Rochester, NY
i would do as dstryr and zero divide suggest, but would add, if they call it a .25 radius and they give you .005-.01 tolerance on the radius, i would manipulate the geometry of the part so that the 1/2" cutter doesnt go 1:1 in the corner. you want to cut it bigger than the cutter radius if possible.
jamesu229
Hot Rolled
- Joined
- Feb 20, 2011
- Location
- Grant Alabama USA
I would use a long reach 4 flute endmill, with a reduced neck. 1/2' loc, and use the tolerance on the radius to keep it from chattering.
Parkerbender
Stainless
- Joined
- Dec 19, 2009
- Location
- Kansas City Mo, USA
Yeah, we have had to put some .125 radii down holes in that 2.5" range... that was not time effective, but basically got away with that by making the rest of the part, then coming back to the corner and taking a billion pecks... two things to remember, firstly rpm isn't always your friend in things like this, and secondly (at least what I've learned) don't be afraid to just waste time pecking, if you are getting paid enough to do so. It seems sometimes you can do stupid and crazy things, as peck count approaches infinity. if you are making one of these and getting a good chunk of chip, if you finish that corner to .265-.27, then come back at it just a couple thou over on the radius at .05" pecks, probably like 4800-5200 rpm (see if you can find a friend with that blue swarf thing maybe, I have been interested if that program would help this specific problem a lot...) and about 6 ipm, just clean up the .300-.325" on either side of the corner, blending into the wall... probably looking at 5 minutes tops, but it would work! I'd use a .5"dia long 4-fluter to clean it up, 2.5" deep on a .5 endmill isn't really even very scary, .125" pecks should be just about as safe and boring...
If these are production parts and you have dozens (or hundreds... Gasp!) of these corners to make, god help you... make a broach maybe?
-Parker
If these are production parts and you have dozens (or hundreds... Gasp!) of these corners to make, god help you... make a broach maybe?
-Parker
John Welden
Diamond
- Joined
- Mar 21, 2009
- Location
- Seattle
I don't see what the big deal is. Just cut it.
706jim
Titanium
- Joined
- Jun 14, 2006
- Location
- Thunder Bay Canada
Yes, there are several ways of making this 1/4" radius but once again it begs the question: "Why?"
I will (once again) state that I believe there should be more interaction between designers and machinists.
It is only too easy to pop a 1/4" fillet into a solid cad model without the designer appreciating that it will create problems later in the manufacturing process. While in some cases, the 1/4" radius may actually be necessary for some purpose, it may well just be decorative. Would not a 0.255 or 0.27 radius achieve the same result while allowing a standard 1/2' cutter to be used?
I don't know the solution to this common dilemna but wish that there could be more interaction between the two camps for just this type of situation.
I will (once again) state that I believe there should be more interaction between designers and machinists.
It is only too easy to pop a 1/4" fillet into a solid cad model without the designer appreciating that it will create problems later in the manufacturing process. While in some cases, the 1/4" radius may actually be necessary for some purpose, it may well just be decorative. Would not a 0.255 or 0.27 radius achieve the same result while allowing a standard 1/2' cutter to be used?
I don't know the solution to this common dilemna but wish that there could be more interaction between the two camps for just this type of situation.
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
The helix of your tool makes a huge difference in long reach. Go to MA Ford or Helical Solutions and get a 35* necked 1/2 em. Like I said I'm running production right now on my horizontal with a 1/2 em 2.250 and its a piece of cake. Now the side with the 3.5" depth and 1/4 radius has been tricky. Just gotta drop the rpm and slow the feed in the corner.
gorrilla
Stainless
- Joined
- May 2, 2007
Anybody tried a boring head in this situation? It would create the same situation as the short length of cut EM, in that you aren't "seeing" that long cut which is likely where your harmonics for the chatter are coming from. The tool would only "see" whatever feed you put on it as the depth of cut. Should cut smooth as your mill is capable of, and in aluminum, it won't take long.
I did just cut it. Looks like shit. I'm not happy with shit. Now what?
I only have one to make. But I've made two now and I'm running out of aluminum that size. I have never had much luck making a radius x with a 2x diameter end mill no matter what the depth, but certainly with a DOC at 5x the diameter, there are problems. Doesn't sound good, doesn't look good. It doesn't take much force to deflect 2.5 inches stickout on a 1/2 end mill.
I'm the engineer, the radius isn't there out of whim. It really should be 3/8, but I gave that up early on. I tried arcing a larger radius by 0.005, thinking that would keep it from engaging 90 degrees, also pulling off the floor a few thousands. Still no joy, the EM is deflecting more than that as it approaches the corner I guess, still leaves marks around the radius. I don't know how far I need to be away, if had a thousand to do I would experiment more. The 12mm EM is a good idea, don't have one that length on hand (nor do my normal suppliers). Maybe pecking with the reduced shank EM would work - I tried pecking with the long .5, it gets a ways and then its rubbing on the wall too much and goes unstable. I haven't tried lowering the RPM a lot, may give that a go. These are 38 deg EMs I am using.
allloutmx
Titanium
- Joined
- Mar 6, 2013
- Location
- Rochester, NY
Have you tried the pocket re machining function? You could generate your corner rads and cut with a 3/16 relieved at a small step down...or even interpolate the radius. Or you still might be going too fast with the 1/2
JP Machining
Stainless
- Joined
- Jul 15, 2006
- Location
- Wisconsin
7/16" reduced neck variable flute, pocket remachining method
706jim
Titanium
- Joined
- Jun 14, 2006
- Location
- Thunder Bay Canada
Ok, I'll stop grumbling about the engineering. Like you, I was usually the guy who specified the geometry.
You've received a number of suggestions so here is one more:
Conventional mill the final finishing pass. I found that long end mills will literally "climb into" the part with considerable deflection whereas in conventional milling, the cutter will bend but otherwise "stays put".
It's unfortuate that you are running out of material, but maybe you could try this suggestion on a bit of scrap metal just to see if it helps.
