hi I just joined this site but I've been visiting for a while and now I need some advice.

I've just gotten this project handed to me that requires some very long VERY thin end mills. I am running a fadal VMC4020 and I need to know where I can get some 4"x1/8" carbide end mills. and some 4"x1/16" carbide end mills.

any suggestions would be very helpful.

PTcutter :banana:

Are you looking for endmills or saws???

OR

Is it 1/16 and 1/8 endmills, 4.00" long??

the second sorry I can see how that could be confusing.

I am searching for a 1/8"dia. and a 1/16" dia. at LEAST 4" long

Off hand, I don't know anybody who makes carbide ones 4.0 long and keep them in stock. However, I do have endmills like that for some of my parts, but there are custom ground. Check out Destiny Tool (http://www.destinytool.com/main.html) and give them a call for you need. They have a good price (and can be coated too) and delivery.

HTH :cheers:

thanks a lot I will check it out

What is the job and what are you trying to cut?

Is there draft on the walls? if so, custom grind a cutter to suit the job, otherwise you will pay big bucks for long carbide like that.

Not that it really matters much, but unless you are cutting something like styrofoam, I can't see how a 4" long 1/8 or 1/16 cutter will last or be accurate in any other material.

But I'd like to hear the rest of this story to see how things went. Great learning experience.

Not that it really matters much, but unless you are cutting something like styrofoam, I can't see how a 4" long 1/8 or 1/16 cutter will last or be accurate in any other material.

Oh, you'd be surprised.... :banana:

:cheers: :cheers:

Please, surprise me, cause I know that I've still a lot to learn.

I would hope that the Fadal has a speed head on it, because I don't think the 4020's come with anyting more than a 15,000 rpm spindle.

For most, speed will kill the tool in this case. Not saying that you can't run that tool at those speeds, but it will take more than just a "good cutter". At 4" long, most shops don't have the 'stuff' to make it run that. However, it will work, and the end result for the speed and feed will be well within the range of the Fadal. The most important aspect of this will be the TIR.

the job is an aluminium cavaty to be used as a prototype, the walls have a draft but it is so slight there is just enough room to do any work on it. the reason I need the smaller cutters is that there is detail work that has to be done in the bottom of the cavaty. the cavaty is aprox. 2.5" deep if not a little deeper and only 3"x2.5" wide/tall.

As for the cutters lasting, we have 3 or 4 small cutters that we have been using quite often and they have lasted quite a while and they have been sorely abused, as long as we don't take too deep a cut we should be ok. the other problem is that the cutters have to be ball nosed.

and the part about the grinding one to size almost made me choke on laughter. not that it isn't a good idea but the only cutters we have in stock that are more than 3.5" long are 1.5" in diameter! it would be just a little bit of grinding there!

Psychomill:

i almost never do that kind of work. sooo could you give me an example of using that long and thin of and end mill in alum./steel feeds/speeds you used. and what exactly is neccessary to get that. I would assume some sort of messuring tool to get the TIR very low??? what else???

I would have expected you to buy a 3/16 blank, and possible bring it down to the taper size you need. Thus a little more rigid than a straight cutter.

BTW, why not just make a carbon and burn it? Take no time at all...just a guess, not and edm specialist.

the cavaty is aprox. 2.5" deep if not a little deeper and only 3"x2.5" wide/tall.

At 2-1/2, it won't be that bad depending on what the actual feature is. I have a part with a slot at .150 deep on the floor next to a wall at 3.300 tall. An 1/8 em cuts it thats 5.0 OAL.

I would assume some sort of messuring tool to get the TIR very low??? what else???

Just indicate the tool like you would a drill/reamer. But, do it at two points. One at the holder end of the tool shank, one at the cutting end. An ER style holder will work best for small shank/dia tools. I use Bullseye and VC holders from Lyndex/Nikken (http://www.lyndex.com/) mostly. These holders are deadly accurate. Your spindle condition will affect your speed as well. If you have some runout or vibrations, you won't be able to run the higher speeds. You can still do it, just slow down.

I would have expected you to buy a 3/16 blank, and possible bring it down to the taper size you need. Thus a little more rigid than a straight cutter.

Tool design is important. Number one: avoid long LOCs. Just because the feature is 2-1/2 down, doesn't mean you need a 2-1/2 LOC em. Use "necked back tooling". To see what I mean, check out Dataflute, Destiny Tool (http://www.destinytool.com/main.html) , GW Schultz (https://www.gwschultz.com/) , Hanita (http://www.hanita.com/) etc. Even SGS and Niagara makes them. If you can get away with a little more shank dia, do so and get one custom ground. The 1/8 I'm using has 3/16 LOC, necked back to 2.70 (theres a step at the top of this wall), then into a 3/16 shank. Get as much shank as you can in there and keep the LOC short. For aluminum, use a 45 deg helix. The standard type helix is a little tougher, but it will more than likely "walk" on you. The helix will help it to keep engaged.

The best way I've found to do the machining is plunge mill the roughing, then profile or "slot". Keep the DOC short (20-30% of dia), axial to 50% or under. This isn't set in stone, just a starting point. You can get away with more, or have to go less depending on the situation. The 1/8 I'm using cuts between 6000 to 8500 rpm. But don't be surprised if you end up at 3000 rpm or less. You play with these things long enough, you'll get a feel for the running conditions. I can't give you exact speeds and feeds since the variables can change greatly. This type of machining has more curve balls than "how fast can I cut 304 with a 1" Carb hogger". Use your tolerance as well. Cut slightly big if you can and still be in print.

Why not EDM? For the most part, the feature is a small amount of detail. Maybe only a few of them at short depths. I can cut them faster on the machine in the same set up than having to unload the part, stage them at the EDM, set up the EDM and run. Thats if you have an EDM. If not, you have to pack, ship to an outside source, wait for them to run, ship back, unpack, check, etc, etc. It's a lot of added lead time.

1/16" gets a little trickier but the rules apply similarly. I have a 1/16 that reaches 1.80 dp, and just ran a 1/32 (actually ground to .029) that reaches .850 ( and sticks out from the holder at 1.35 on a 3/32 shank).

:cheers: :cheers:

That sounds like some pretty sound advice psycomill.

And I am truly impressed at your capabilities, I never would have even tried cutting what you described......like I said, still lots to learn.

Well, maybe I would have tried, but I probably would have been welding, or buying a few carbides before getting back to my favorite forum for help.

Just to clarify something when you say "necked back" are you referring to clearing the shank of the carbide above the flute? I've done that on many occasion and it really does make all the difference in the world.

Just to clarify something when you say "necked back" are you referring to clearing the shank of the carbide above the flute? I've done that on many occasion and it really does make all the difference in the world.

Exactly. Most people have been doing it for years on long LOC tools to get that " extra 1/2 inch " of cut length and just step down the finish. The principle is the same here. Except you take a stub LOC tool with a long OAL and relieve the shank behind the flute for the desired depth. This makes for an extremely strong tool capable of reaching great depths. I've been doing that and having these ground for more years than I can remember until the toolmakers started making and marketing them.

:cheers:

well this is a little more response than I expected to get. I was just hoping for something like "look here,_______." or "this is a good place ______"

so I have to say I'm really happy with this thanx a lot psychomill, and everyone else.

YA :banana: For the great response