Thread: Endmill flutes concentric with the shank

Originally Posted by cgrim3

Yes we will be side cutting with all 4 inches of flute length. I was going to buy carbide since it is so much stiffer than hss (less chatter problems with carbide) but hss would probably work okay. I would imagine you would want the most flutes possible to make the endmill more stout. What feeds and speeds and radial step over for carbide? CAM calculated it to be 1000 ft/min, 125 in/min feed, .011 feed per tooth. Maybe a bit fast for an endmill this length? Don't want to produce any chatter or harmonics

I haven’t needed to run extraordinarily long endmills for many years (I always find a work around any more), but when I did, I always found very low rpms and high chip load to work much better.


Sent from my iPhone using Tapatalk

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.

Originally Posted by triumph406

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.

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

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.

Originally Posted by Gobo

A variable pitch end mill will help reduce chatter.

^^this
These help so much when you have long flute engagement.

Originally Posted by cgrim3

Our machine is a box way daewoo 3016 dmv 3 axis mill, 8000rpm spindle. The machine is mostly used for stainless and titanium. Its a pretty rigid machine and the pioneer tool holders we have runout less than a tenth. We were already awarded the job...we included 400 dollars in the quote for pricing on the endmill. I found garr has a 1" diameter variable helix 4 inch loc for about 340 dollars give or take, uncoated or 20 dollars more for ticn coating. The hardest part will be dialing in the speeds and feeds and radial doc so it doesn't chatter.

Garr part numbers for the endmill we are looking at is 42360 & 42364

We are not used to running aluminum. 95 percent of our work is 316 stainless and titanium

Also, we are not machining any pockets. It's just side milling with the cutter on the outside of the part.


We looked into endmills with a reduced shank but decided to go with a 4" loc endmill. We will revisit the reduced shank endmills and see what we can come up with

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.

Originally Posted by metalmadness

Heres how I would approach this. Buy a reduced shank 3/4" dia cutter that can cut 4" deep.

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.

Originally Posted by cgrim3

.... He said the flutes on some cheaper brands were not nearly as concentric with the shank and the flutes had a bit of runout (assuming your holder is running out <.0001 in the spindle).
...My question is have any of you guys bought long endmills, or any endmill, that had runout or concentricity problems?
Chris

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

Originally Posted by CarbideBob

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

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

Originally Posted by triumph406

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

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

Originally Posted by triumph406

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

I normally don't mention brands but someone mentioned Niagra and I think they are very good
here is their spec sheet:
Niagara Cutter

Originally Posted by triumph406

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, tool holder, insert are concentric.

That's something else the OP should worry about

I normally don't mention brands but someone mentioned Niagra and I think they are very good
here is their spec sheet:
Niagara Cutter

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

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

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.