What's new
What's new

Long reach 1/4 endmill in 6061

Clonekid54

Plastic
Joined
Feb 20, 2017
I've got a "very" deep feature to make in 6061 Al. The minimum corner radius is .125" and this thing is 3.8" or so down there. Machine is VMC and tool is held in er32 collet/ 40 taper. I purchased some 6" reduced neck 1/4" endmills for the job. 2 flute and for aluminum and all that. Having some problems with chatter. Stickout from the collet is 4". I test ran some slots and .003 DOC at 12k rpm and 154ipm seemed to be doing "ok" (still crappy for my taste) going in conventional. Climb cut started digging in the corners. Anyone have any pointers for running this long length/diameter ratio stuff? I'm roughing out with a larger endmill but I just need to get the smaller diameter one to run a bit better.
 
Carbide cutters are more rigid. If those are not available in the full length, one could possibly braze a carbide extension to a shorter one.
 
lilerob1 hit it on the SFM issue. The other issue is you're banging into a corner thats the same radius as your cutter. Thats a lot of engagement. If you can find a cutter a little smaller on diameter, that would help as well.
 
154 ipm is way too fast
I would see about getting some 6mmm tools so the part has a corner radius to swing in the corners.
Drill close to the corner with a ~.244 drill

Also I would use multiple tools to get down there first.
first tool with 1" flute length
second tool with short flutes necked 2.125
third tool with 3.375
fourth tool with your 4" reach

How many parts to do?
How wide is the overall pocket?
 
I cannot say I have had success in this area, but the closest I have come is starting with a shorter end mill and going as far as I can with as small a remainder as possible, then only finishing with the longer end mill. I would probably also try drilling the corners. I think if there is a 7/32 end mill that long it is worth while trying, especially if the accel decel is making it seem to dwell in the corner
 
Another option is to tilt the part 2-5° on a sine plate and use a ball end mill and a surfacing routine to get the engagement down to just a tiny fraction of a plunge or straight cut. Will be slower and you still may have some minor issues at the very corner of the floor depending on what radius is allowed there.
 
all sfm and feed rules go right in the can on long reach. You have to figure out what your combo likes, and thats machine, holder, cutting tool, and part- yep the part can induce chatter too if its thin wall/ fragile.

all I can say is try slower than you could ever imagine and see what it does. work up from there.
 
Drill the corners before pocketing?

Yes, this, and if you feel it would be OK with your customer, predrill at the nominal corner location but cheat a bit high on the drill size, maybe a 6.5mm or "F" drill.

Now having said that, drilling 1/4" x 4" deep is no picnic either :willy_nilly:. Might need to do it in steps.

Have you mentioned this to the customer? Sometimes they don't really care that much what the corner radius is and would be OK with either a larger radius or a dogbone corner that gives the same clearance but allows larger tools.

Regards.
 
Let me begin by describing the part. It's basically a box with an angled lid from front to back. On the inside of the front face there's some reliefs about .125"ish deep with .125 corners. The only way I've seen to reach this is by setting the box on the front face and coming in from the back. The clearance there is 4.6" or so. (I misspoke in my first post, it's deeper than I remembered)

So the actual feature I need to do is a profile cut with some .125 corners at a .125 depth 4.6" down inside. Corner drilling won't help me as much because the point on the drill will go to deep and not give me enough clearance in the corners, there's only about .08 wall thickness to the outside face. What I came up with this morning is using a 4 flute on my finish pass at 385sfm and .015 chip load, .01 DOC and only finishing in the corners using trochoidal pocketing. I'm using a larger endmill for the main passes. It gives me a decent finish, not the best but acceptable. I may play with some other options that were suggested to try out something a little faster. I tried all different feeds and speeds this morning and a few different DOC and WOC. 2 flutes were giving me a pretty rough finish no matter what speed I ran it at. The 4 flute seemed to do decent enough. I should be ok with the 4 flute cause it's just a finish pass and shouldn't have to worry about chips clogging it up. I'll just have to get a green wheel and relieve the shank a little cause it was just a regular extra long length one that was laying around.

There's only 3 of these I have to make so no large production runs. I only work on prototypes so I'm always doing these one off things.
 
I do shit like this all the time in prototypes and usually cheat by using a 5 axis machine and a tiny ball em to 3d the corners with it tilted over using a long tool extension.
:)

Glad to hear your 4 flute is working...
 
5 axis would be pretty sweet to cheat with, but I don't have to do to many parts that would need something like that. Never programmed one either, it'd be fun to learn though.

Thanks for all the help everyone! Lots of excellent ideas! That's what I love about this line of work, always about 100 ways to skin the cat!
 
This also might be a case where you go back to the designer and point out if they made the corners 1/2" radius it would be much easier/cheaper. If it's a box, chances are that radius dimension is pretty arbitrary and the designer just doesn't know. There's that CAD thing where you radius the vertical corners and the bottom of the edges at the same time with the same number, not realizing that you should design for a bullnose end mill which has a different bottom corner radius than the diameter.
 
Let me begin by describing the part. It's basically a box with an angled lid from front to back. On the inside of the front face there's some reliefs about .125"ish deep with .125 corners. The only way I've seen to reach this is by setting the box on the front face and coming in from the back. The clearance there is 4.6" or so. (I misspoke in my first post, it's deeper than I remembered)

So the actual feature I need to do is a profile cut with some .125 corners at a .125 depth 4.6" down inside. Corner drilling won't help me as much because the point on the drill will go to deep and not give me enough clearance in the corners, there's only about .08 wall thickness to the outside face. What I came up with this morning is using a 4 flute on my finish pass at 385sfm and .015 chip load, .01 DOC and only finishing in the corners using trochoidal pocketing. I'm using a larger endmill for the main passes. It gives me a decent finish, not the best but acceptable. I may play with some other options that were suggested to try out something a little faster. I tried all different feeds and speeds this morning and a few different DOC and WOC. 2 flutes were giving me a pretty rough finish no matter what speed I ran it at. The 4 flute seemed to do decent enough. I should be ok with the 4 flute cause it's just a finish pass and shouldn't have to worry about chips clogging it up. I'll just have to get a green wheel and relieve the shank a little cause it was just a regular extra long length one that was laying around.

There's only 3 of these I have to make so no large production runs. I only work on prototypes so I'm always doing these one off things.

Even high speed toolpaths don't help much if the endmill radius matches the corner radius. The instant the tool hits the corner, the chipload skyrockets from .015" to .196 per flute (1/4 of the tool circumference) and the rpm doesn't even come into consideration at that instant. So it is essential to use a slightly smaller diameter tool, probably a 6mm would be good, but anything to prevent the tool radius matching the feature radius.

I'd probably cheat if I had to use the 1/4" tool by creating a mask surface to put in that corner with a .275" radius and see if anybody noticed.
 








 
Back
Top