-
02-21-2021, 07:32 PM #21
-
moonlight machine liked this post
-
-
02-21-2021, 11:20 PM #22
if you have a significant amount of material to use, use a roughing endmill, and remove the last .005-.01 with a 1" dia HSS endmill, it'll save you money and the finish will be the same.
-
02-22-2021, 01:02 AM #23
I agree, I was going to suggest a 1” inserted cutter such as a Korloy (Ripper) Endmill. I run those as hard as I can, even swung out 4 inches.
1 INCH RIPPER MILL
Sent from my iPhone using Tapatalk
-
-
02-22-2021, 07:03 AM #24
What is the reason to choose the 4" long of the end mill. Is it surface finish and squareness expectations?
You might consider the cost of one-time use tooling compared to just sending the job out.
Using an end mill end and then hand finishing the last by hand.
Using a fly cutter.
Way back when I worked in a die shop we bought end mills with with having centers at both ends, and with having a recess the cutting end where that center was. That recess made them not good for deep pocketing because one had to only go deep perhaps 1/16 to 1/4 max or they would end bind. They would be resharpened between center so would remain dead true to the shank.
-
02-22-2021, 08:47 AM #25
-
mhajicek liked this post
-
-
02-22-2021, 12:23 PM #26
OK you don't have much aluminum experience which is fine.
HOWEVER, if you are doing 4" LOC ROUGHING with a 4" LOC cutter, you're gonna have some serious chatter in my view.
Heres how I would approach this. Buy a reduced shank 3/4" dia cutter that can cut 4" deep. Itll prob be 200 if you buy from Helical Solutions. Use that tool to rough. Then come in with your 4" LOC end mill and finish the profiling. No need to rough up an expensive tool like that when you could just use it for finishing. Also less likely to deal with chatter when you have a solid carbide shank of the reduced neck cutter. Take it from someone with experience doing ultra deep pockets in aluminum with small internal corners. Reduced neck is the way. It is known.
-
02-22-2021, 12:46 PM #27
You can probably use that same cutter to finish. Do small stepdowns with skim cuts and you'll get a pretty nice finish. I've got a 5/8" Helical relieved that sticks out 4" that does this on 17-4 H900 and Ti grade 5. I run Helical's recommended parameters, which for a long reach tool like this are higher RPM and smaller radial engagement.
-
02-22-2021, 01:15 PM #28
All endmills will have runout. Never seen one that does not top to bottom.
One tenth runout of the holder in the spindle can be very different 6 inches out.
Same deal with making the endmill even with a new 1/2 to one million dollar cnc as you have to clamp them somehow.
At four inches full the endmill even if one inch diameter carbide is going to bend or flex under any load.
Hence the necked down approach.
In production use I've seen the deep wall endmill ground with a reverse taper so as to make a flat wall with the deflection or bend comped into the grind.
This crazy stuff only for people with very large runs and endless pocketbooks.
Bob
-
02-22-2021, 03:33 PM #29
Well it's not something I'm going to worry about, I'm sure the better brands of endmills that I use (YG/Niagara/Kyocera) are more than acceptable. Especially (in my case) as their going into side lock holders, ER16 and ER32 collets of questionable origin and some off brand CAT40 holders. And then into a 10+ year old Fadal spindle, and a 30+ year old Makino spindle.
----------------------------------------
On the other hand I do care about the shape of ball endmills and their concentricity in the holder. Some prototype parts I have to make have 3D contour tolerances of +/-.003-.005.
So the ball end gets checked for shape and position. A good proportion aren't accurate balls. Some you tell by looking at the tip that opposing radiuses aren't tangential, etc. The ones that look good with a radius gage and visual inspection get run thru a piece of RenShape and then checked on a comparator.
Cos' I was wasting so much time trying to find correctly shaped ball end mills I ended up using Dapra ball inserts in a Dapra holder. I check those in the spindle to make sure the collets,toolholder,insert are concentric.
That's something else the OP should worry about
-
-
02-22-2021, 04:52 PM #30
I normally don't mention brands but someone mentioned Niagra and I think they are very good
here is their spec sheet:
https://www.niagaracutter.com/solid-carbide-tolerances
-
02-22-2021, 04:53 PM #31
I normally don't mention brands but someone mentioned Niagra and I think they are very good
here is their spec sheet:
Niagara Cutter
-
02-22-2021, 04:53 PM #32
I normally don't mention brands but someone mentioned Niagra and I think they are very good
here is their spec sheet:
Niagara Cutter
-
02-22-2021, 05:34 PM #33
I greatly appreciate all the responses. We ended up getting a reduced shank .75" diameter endmill from gorilla mill with a long reach. We are going to rough and finish with it.
We are a 2 man shop and I am relatively new to the trade and am learning as I go. My dad (my boss) has been in the trade for over 40 years and he really knows his shit whether it is milling or lathe work, but I like to get opinions from other people as well.
Thanks,
Chris
3/4" Diameter Square End (4FGMNRI) | Gorilla Mill
-
02-22-2021, 06:36 PM #34
if you have size to play with milling long-sided you might be skillful and lucky...0r not.
But with square and size both critical, it can be a bugger..good that you have your Dad.
Let us know how it goes
Buck
-
02-22-2021, 07:56 PM #35
I think it was 'Psychomill' that posted several years ago, that they worked out the proper radial cut and feedrate so the cutter wanted to dig itself in the right amount so that it cut a straight surface and didn't chatter. And I don't think there was any 'science' involved, just a ton of experimenting.
At least, that's what *I* got from the post(s). And it's entirely possible I just 'didn't get it'.
It seems reasonable, depending on ... a bunch of things maybe.
I did a prototype model of a 'handheld device' quite awhile back. I bought a stupid expensive 1" carbide endmill for it, about 3" long I think. Might be 4. I think I made the finish passes full depth, and it came out looking just fine. But even though the part was aluminum, I wasn't running it anywhere near the RPM that might be considered normal. Probably more like 200 SFM, which is pretty wimpy even for HSS. It was friends of mine that offered to lend me a relieved 3/4" that they do this with fairly often.
As suggested by someone else, a proper long reach short flute tool would be better. Much stiffer without the flutes running full length. But sometimes harder to find, and it's not too difficult to 'relieve' the flutes on a normal cutter on a bench grinder with plain Al oxide wheels. But it looks ugly, so don't let your picky customers see it.
-
mhajicek liked this post
Bookmarks