need tooling ideas for 12 in deep pocket on cnc mill

SDConcepts · Oct 15, 2017

need to cut a 12 in deep pocket in 6061 aluminum. and in actuality its a stepped pocket. first step is 7 inches. second step is another 5.0 inches. I don't even know where to start to look for tooling for this. thankfully its aluminum. I've got a prox mill for aluminum that will go about 4-5 inches deep, but what to use after that?

the second step of the pocket is 3 holes two 3" holes and one 2inch hole. i'm sure I can get a spade drill to pop those in if I had to. still would like some info on long reach mill tooling.

thanks

DMF_TomB · Oct 15, 2017

SDConcepts said:
need to cut a 12 in deep pocket in 6061 aluminum. and in actuality its a stepped pocket. first step is 7 inches. second step is another 5.0 inches. I don't even know where to start to look for tooling for this. thankfully its aluminum. I've got a prox mill for aluminum that will go about 4-5 inches deep, but what to use after that?

the second step of the pocket is 3 holes two 3" holes and one 2inch hole. i'm sure I can get a spade drill to pop those in if I had to. still would like some info on long reach mill tooling.

thanks

what would be the problem ?

Milland · Oct 15, 2017

Knowing what machine you'll be using, its condition, and what budget you have for tooling would be helpful. Also what your programming strategy will be - shallow radial/lots of Z, or traditional hogging? Surface finish and accuracy requirements matter too.

If you can swing the cost, look at vibration damping extensions, like from Kennametal.

DMF_TomB · Oct 15, 2017

as helical mill picture shows you can easily buy a carbide insert mill that goes on tool holder thats smaller dia for clearance. i everyday mill deeper than 12 to 18"
.
obviously the longer the tool the more tool deflection is a problem

DMF_TomB · Oct 15, 2017

many horizontal mills the majority of tools are over 12" long just to be able to reach the center of the table (pallet) it actually would be rare and unusual to have any tools less than 9" long

SDConcepts · Oct 15, 2017

currently my plan is to run this on a has vf3. yes I realize chips will be a problem. its a one off. I don't think surface finish is critical I think this pocket is just for lightening the object. I will find out more on Monday. cat40 taper. I could get a 1.5" dia tool in there. obviously cheaper is better. currently my plan is to do .150-.250 deep step downs in z will clearing chips as best as I can. if I can I've got some 1.5 dia insert drills that will get my about 4-5 inches deep and plan on poking a bunch of holes in it first.

dstryr · Oct 15, 2017

12" deep? I hope you meant to say you were going to go .015-.025 deep with a 12" long 1.5" tool in a VF3?
What are the pocket dimensions? Blind?

Matt@RFR · Oct 16, 2017

dstryr said:
12" deep? I hope you meant to say you were going to go .015-.025 deep with a 12" long 1.5" tool in a VF3?
What are the pocket dimensions? Blind?

Exactly. And a HSM toolpath will be essential. No sharp corners, ever! Without much thought, I'd start at maybe 5000 RPM, .015 IPT, .020 DOC and about 75% WOC. A Ripper type face mill on an extended arbor will work ok.

Kaszub · Oct 16, 2017

Does the Vf3 have enough travel in Z axis to do this. I just run into a problem on my DMG 1035 where after having a part sitting on table and tool in spindle only had 1/8 clearance between them.

Kaszub · Oct 16, 2017

Found a pic. Pain in the ass job, thank god it was only one pic.

ToolHIT · Oct 16, 2017

If you are looking to do it economically then a spade drill would be the cheapest and most effective way to remove material to begin with. From there if you can fit a 2" Facemill in the bore then I'd use a 2" Diameter Facemill in a CAT40 Anti-Vibratory Shell Mill Arbor and interpolate down to size (a 2" Pro-X Mill would be a great option as it is very free cutting and would keep tool pressure down).

If the 2" Mill doesn't fit the bore then a 1.5" Threaded Arbor Facemill (these have a M16 Thread, Korloy offers it in their Pro X Mill) with a Solid Carbide ISO Milling Bar would give you the reach and rigidity you need to interpolate down at the 12" Depth. Attached is a picture of the Milling Bars

Hopefully this helps.

DMF_TomB · Oct 16, 2017

if tool holder dia needs to be less than cutter dia you will have a hard time with anything less than 2" dia at 12 deep. actually 3" dia is more practical dia to length ratio
.
the 20" long tool shown is a 1.75 dia end mill but tool holder is tapered. much over 6" DOC the tool holder will rub on the part. and such a long tool will vibrate if pushed too hard

HuFlungDung · Oct 16, 2017

I'd be somewhat concerned about unseating the tool in the taper. At least on my '96 VF3, there isn't really a hell of a lot of retention pressure available from the retention system, it's pretty easy to unseat the toolholder out of the socket with a 12" long pry bar. Sometimes I wish there were a mechanical clamping system like the old NMTB socket had, but front mounted so you could apply positive clamp pressure with a bolted on ring. Yes, it would not be tool change friendly, but that is beside the point if you're just trying to get 'er done.

dandrummerman21 · Oct 16, 2017

HuFlungDung said:
Sometimes I wish there were a mechanical clamping system like the old NMTB socket had, but front mounted so you could apply positive clamp pressure with a bolted on ring. Yes, it would not be tool change friendly, but that is beside the point if you're just trying to get 'er done.

Make 2 special keys with a split "ring" welded to it which goes halfway around the flange (inside the v groove), that you can bolt onto the spindle after putting in the tool. Will kinda "toe clamp" the tool into the spindle...

I mean, i think its only an M6 bolt in there, but a couple of M6 bolts might help? I would probably rather change the bellevilles or simply get a better machine. But hey, why not.

Anyway, I have the same question as above, can you actually get a 12" tool above a 12" tall part? I guess you could mill it to first depth and manually insert a tool into the spindle with it already in the pocket to get to full depth. don't go rapiding home afterwards if you gotta do that! I've done that. Not pretty....

Search

Largest Manufacturing Technology Community on the Web

Search

need tooling ideas for 12 in deep pocket on cnc mill

SDConcepts

Stainless

DMF_TomB

Diamond

Attachments

Milland

Diamond

DMF_TomB

Diamond

DMF_TomB

Diamond

SDConcepts

Stainless

dstryr

Diamond

Matt@RFR

Titanium

Kaszub

Hot Rolled

Kaszub

Hot Rolled

ToolHIT

Plastic

DMF_TomB

Diamond

Attachments

HuFlungDung

Diamond

dandrummerman21

Stainless

Similar threads