End Mill or Shell Mill, what's better??

[jspangler]

Hi

Just wondering if there were any benefits to using Shell mills over regular end mills.

The reason i ask, is that i just picked up some regular type inserted end mills from US SHop tools. They have great prices, and the Tungalloy style i picked allows me to use 4 sides of the insert, vs. 2 for the iscar. The one downfall is that for the sizes i picked to replace my iscars, the new tools have less teeth

( Iscar 1" = 2 Flute, USST 1" = 1 Tooth, etc. ) they say this is due to the size of the insert.

 

Whatever, All I know is that I've had to drop my feed rate ( figured by using Cimco Feed and Speed) Alot!!

 

Anyway, the shell mills they offer (that use the same inserts as my new end mills) offer a lot more teeth per cutter which should equal more feed, right??

What are the benefits or disadvantages to using these?? I am cutting .375 1018 steel header flanges - Contouring, and pocketing. I drill entry holes or enter with a lead in, so there is no ramping or helixing involved.

 

Thanks

John

[chris m]

John

 

I am confused

 

First you make a query about "regular" endmills; do you mean "regular" solid carbide endmills or inserted endmills?

 

Then you are saying that you can get a facemill-style inserted cutter that holds more inserts than a endmill-style cutter of the same size. And you are [correctly] stating that more teeth at the same RPM would yield more feed. That part I understand.

 

But...

 

then you make a statement about 1" cutters; are you looking for a 1" facemill? I've never seen one that small; do they make them? If so I would think that the inserts must be very small.

 

More info please

 

C

 

[ 10-28-2002, 12:18 PM: Message edited by: chris m ]

[McRae]

The Definitive Post on the Subject.

 

How much money did you cost yourself by buying cheap? Studies show that cutting tool costs are in the order of 3-4% of the total hourly operating cost of a CNC Machine (Seco and Sandvik Literature). Think about this for a minute. If you spend 5 hours doing a job instead of 1 hour, just to save $3.00 on an insert, then you just gave your customer 4 hours of Free Machining... (for which you could have invoiced someone else for that time!)

 

Send Back that US SHOP CRAP and get a hold of the Iscar Guy again, Partner with him, or the Sandvik Guy, or the Kennametal Gal, or one of the Japeneese Cutting Tool People and work closely with those who understand what they sell. Catalogues are for buying "Soap, Dope and Rope" not engineered tooling!

 

Sorry for the "Mayette Style" answer but see the real deal below.

 

Cutting Tool Selection.

 

Material Removal Rate (MRR) is the measure of what you really need to ask yourself. This includes the

 

Cutter Body (Diameter, No of Teeth, Spindle Speed, Width of Cut),

Insert Grade/Geometry (SFM, Feed per Tooth, Depth of Cut),

Setup Style (Horizontal/Vertical - for determining if Recutting Chips is a problem),

 

MRR = RPM * FPT * No of Teeth * DOC * WOC

 

Thinking of all these parameters, see if there is an advantage to using 4 corners on a reduced MRR setup. Oh and BTW - Let me know your address so I can attend the Auction when you go out of Business.

 

[ 10-28-2002, 12:39 PM: Message edited by: Andrew McRae ]

[Guest CNC Apps Guy 1]

quote:

---

Sorry for the "Mayette Style" answer but see the real deal below.

---

Uh, it's Meyette.

 

Sometimes you just gotta tell it like it is and not sugar-coat it to make the point. Good job Andrew.

 

To add to Andrews statement, tooling is the positively LAST place you should go cheap. Think about this for a second. A part I just finished programming originally took 3 hours of machining time, not including setup or anything else, just in the machine cutting. I was asked to reduce the cost (read make it faster). I did some investigation and found that a $250 custom tool, (oooohhhhh, dare I say that word? custom?) and a custom diameter end mill that cost $30 ea. would cut one section of the program from 45 minutes to 5 minutes and another section from 45 minutes to 10. Do we need to do the math? I think we get the picture. You don't always need to get custom tools made but you definitely need to make wise decisions regarding tooling.

 

JM2C

 

[ 10-28-2002, 01:57 PM: Message edited by: James Meyette ]

[chris m]

quote:

---

Let me know your address so I can attend the Auction when you go out of Business

---

WOW!

 

Andrew; I think we need to change your handle to "Hannibal" as you are always looking to devour the rest of us.

 

I gotta say John; that chopping the feed to save $20 on inserts is probably not the way to go.

 

C

[jspangler]

Hi

OK, you're right. I've been going through my programs to repost using these new "CHEAP" cutters, and DAMN, just backplotting them shows about 20 minutes additional machining time due to the slow xxxx feed rates. It was my mistake for not checking the number of teeth per cutter BEFORE I placed the order, and one i will not make again.

 

But...

the inserts i'm using ( let's forget the fact that there is just not enough of them) easily cut as good as the Iscar 950's i was using, and allow me to run coolant, and cost less than half. Also they DO have 4 cutting sides as opposed to only having 2. That's why i was asking about using the Shell mill to increase the number of teeth. In their catalog they offer a 2" dia, shell mill that will hold 5 inserts.

 

I think what i will dois this - Replace the 1.25 3 flute from iscar, to not slow my programs down to the point of non profit, return these cutters in exchange for a larger shell mill type 5 flute and use these cheaper inserts for fast rough cutting?

 

Well, hopefully this keeps someone else

from making the same mistake.

 

Thanks

 

John

[Hugh.Venables]

John, it's not just the number of cutting edges you have to consider. It's the relationship between the number of tips and the diameter of the cutter. To put it more simply, look at the circumferential distance between tips. A 1" cutter with 3 tips will have a better removal rate than a 2" with 5 tips, for the same depth and width of cut.

 

Of course, as the tips get closer together there gets to be less chip space between them. Generally, solid tools can have tips closer together and still have more chip space.

 

Like Chris, I was a little confused with your first post. Isn't a shell mill an end mill with a removable shank?

 

Hugh Venables.

[Hugh.Venables]

John, it's not just the number of cutting edges you have to consider. It's the relationship between the number of tips and the diameter of the cutter. To put it more simply, look at the circumferential distance between tips. A 1" cutter with 3 tips will have a better removal rate than a 2" with 5 tips, for the same depth and width of cut.

 

Of course, as the tips get closer together there gets to be less chip space between them. Generally, solid tools can have tips closer together and still have more chip space.

 

Like Chris, I was a little confused with your first post. Isn't a shell mill an end mill with a removable shank?

 

Hugh Venables.

[jspangler]

Hi

I guess, but the shell mills come in a lot larger diameters. I read here once that you want to use the largest dia. cutter possible. Am i missing some general rule of selecting these utting tools. Obviuosly, I understan that you need to fit the cutter into whatever size pocket or radius on the contour that you are cutting, but other than that, how is a 1" 3 flute, better than a 2" 3 flute?

 

Thanks

 

John

 

PS I went out and picked up a new copy of the original Iscar cutter I was trying to replace.

 

Thanks Again

[Hugh.Venables]

John, take your 1" 3 flute and your 2" 3 flute and work out the speed and feed. For the same cutting speed and feed per tooth, you should find that the table feed for the 1" will be twice what it is for the 2". This simply because the 2" cutter rotates through twice the distance at the circumference between tips than the 1". Twice the table feed for the same depth and width of cut will translate into twice the material removal. It is the distance between tips around the circumference that you need to consider. A 1" 3 flute will work out the same as a 2" 6 flute.

Hugh Venables.

[Hugh.Venables]

John, take your 1" 3 flute and your 2" 3 flute and work out the speed and feed. For the same cutting speed and feed per tooth, you should find that the table feed for the 1" will be twice what it is for the 2". This simply because the 2" cutter rotates through twice the distance at the circumference between tips than the 1". Twice the table feed for the same depth and width of cut will translate into twice the material removal. It is the distance between tips around the circumference that you need to consider. A 1" 3 flute will work out the same as a 2" 6 flute.

Hugh Venables.

[Hugh.Venables]

Sorry about the duplicated posts guys. having a little server trouble I think. Or maybe a little bit of computer illiteracy.........

Hugh Venables.

 

[ 10-29-2002, 12:08 AM: Message edited by: Hugh.Venables ]

[chris m]

quote:

---

how is a 1" 3 flute, better than a 2" 3 flute?

---

RPM, my good man. As Hugh stated [i think] in his posts:

 

1) 1" 3 flute 400 SFM .006 IPT = 1528 RPM and 27.5 IPM

 

2) 2" 3 flute 400 SFM .006 IPT = 764 RPM and 13.8 IPM

 

1" good

 

2" bad

 

To clear up something; are you talking about FACEmills or SHELLmills? They are different animals and this may be causing confusion.

 

quote:

---

I read here once that you want to use the largest dia. cutter possible. Am i missing some general rule of selecting these cutting tools.

---

Not really but a big cutter with the same amount of flutes as a smaller cutter will not help unless:

 

1) there is not enough clearance in the smaller cutter to evacuate your chips

 

2) you are milling a surface that the larger cutter allows you to take in one pass [MUCH better cosmetics] where the smaller cutter will not.

 

Any time you go for a bigger inserted cutter without the above issues involved, always go for more teeth!

 

I'm with Andrew; I'd bring in the local rep from Iscar, KM, Sandvik, or whoever you like and have him work the problem with you. The only reason those guys are employed by the cutting tool companies is to give you good solutions that will keep you coming back.

 

C

 

[ 10-29-2002, 06:55 AM: Message edited by: chris m ]

[chad fisher]

I have done header flanges before and other type of plate work in 1018 steel with the iscars.

your running probably hole diameters in the range of 1 3/4 and up. We would use iscars ic328 inserts in the e90a body style of cutter running at 700sfm with .007 ipt with 3 flutes this equaled too 3565 @ f74.8 with depth of cut around .125 deep. But you must run it dry! other wise you get into all of this thermal cracking of the inserts "now it gets over my head"

Hope this might help.

[jspangler]

Hi

Ok, now it makes sense. One more thing, since I'm running the Iscar 950's I should be able to run at least the speeds you're running, but my insert life is too short at those rates. I am running a .125 DOC, but I am not doing multi passes, so there are sections in my flange, on the contour, where the cutter is cutting less than .2, then parts where its about 75% engaged.

I am also running without coolant.

 

How long do your inserts last at those speeds. I have had longer life with the 950's than the 328's, using 2 and 3 flute e90a style cutters.

 

Would it be possible to see one of you files to see how you are running your pocketing and contouring ops.

 

Again, thanks for all the tips and criticisms.

 

Thanks

 

John

[McRae]

John,

 

Here are my questions...

 

1) Material (this will help with specifying what Insert Grade)

 

2) DOC - WOC (or post file of what you want to do)

 

3) Machine style, and Spindle ( IE Vertical CAT 50)

 

4) Machine Horsepower, Max Feedrates, etc...

 

Anything else that you think may help. I love this stuff!

 

IC950 is a decent hard carbide for high temperature milling - Needs to Run Dry!. IC328 is a Tough Carbide that likes to run slow with Heavy Feed (And it Loves Coolant!)

[chris m]

Andrew and others

 

From what I understand here; this is the situation:

 

1) Material: 1018 [sh*t steel]

 

2) DOC: .125 WOC: Varied from .200 to approx .750 due to variations in part profile

 

3) Machine style, and Spindle: unknown but I'm guessing 40 Taper VMC

 

4) Machine Horsepower, Max Feedrates: unknown but probably not a huge factor in this equation

 

My opinion:

 

John, I think you may need to try to even out the radial DOC to get good consistent tool life in this application. Feed that is appropriate for a 20% radial DOC is too heavy for .70% DOC and, inversely, feed for the heavy cut is too light to really make chips fly on the light sections. Would it be possible to re-program to get a little more consistency?

 

Assuming that the stock isn't flame-cut or anything I think I would start out with a 1" 3 flute endmill assuming you're using 11mm inserts with Sandvik 4040 inserts at around .125 axial DOC and no more than .300 radial DOC with about 800 SFM and .004 IPT which yields 3056 RPM and 36.7 IPM.

 

I would think that the feed could go up from there without much trouble; anybody else?

 

[ 10-29-2002, 12:26 PM: Message edited by: chris m ]

[McRae]

I am thinking of a Highfeed style approach to this problem. If we are milling across a face that has openings, then we can insert feed changes as required - higher feeds in areas of lighter radial DOC. If this is an open face (no shoulders to come up against) then we would modify the lead angle by selecting either a 15 degree tool or something along these lines to prevent part edge frittering or burring.

 

HP and Spindle information would be important if we want to use one of Iscar's Mill 2000 or Tangmill cutters. These things will draw power like crazy. As well, as we increase the lead angle of the tool, the length of the cutting edge increases drawing more power from the spindle.

 

I am working up a drawing to illustrate some of Hugh V's suggestions and can only point out that Hugh is missing Radial Chip Thinning in his assertion, there are apparent reductions when you run the following numbers

 

SFM=600

*FPT=.007

NoTeeth=3

 

1"

F=2292RPM * .007 * 3=48 ipm

 

2"

F=1146RPM * .007 * 3=24 ipm

 

For the same full engagement and given the same depth of cut (.150") the cutters would have the same MRR. (I think that this is this what you are saying Hugh, please elaborate)

 

But now lets look and take a radial engagement of .25" and see the effects.

 

In order to maintain the same actual (Hm=average) chip thickness, use the following

 

FPT=Hm(SQRT(Dia.Cutter/Width))

 

For the 1" at .25 width

FPT=.007(SQRT(1/.25))

FPT=.014

 

For the 2" at .25 width

FPT=.007(SQRT(2/.25))

FPT=.0197

 

Now lets use the modified values in the feed formula

 

1"

F=2292RPM * .014 * 3=96.26 ipm

 

2"

F=1146RPM * .0197 * 3=65.32 ipm

 

With the same Depth of Cut, the MRR is greater for the 1"

 

Hugh wins...

[jspangler]

Hi

OK, The material is 1018 .375 bars ( not flame cut or lasered), and the machine is a Haas VF-2 20 HP, 40 taper. I am using mainly 1" 2 flute, and 1.25" 3 flute IC950 Iscar's, with no coolant. I'm running the 3 flute at 2300rpm, and 45 IPM, the 1" varies depending on the op. Never deeper than .14. I am using the shortest holders possible, with the shortest possible extension of the tool. I would really like to be able to use the HSM option, but my first attempt was a disaster, and I've steered clear since then.

 

More help please

 

Thanks

 

John

[McRae]

Post a process model and we will see more of the specifics.

 

Thanks,

[Tony]

"1018"

I don't think you even need inserts

in the cutter!

[McRae]

We have tried to coat our cutter bodies with 1018 material using this same technique! Blue looking colour smudges are a nice effect!

[Hugh.Venables]

Thank you Andrew for a very informative post. I feel obliged to admit that the reason I didn't consider radial chip thinning is because I never have. My excuse is that all our work here is prototyping and one offs but I'm not sure it's a very good excuse. Your adjustment formula is very interesting and certainly reduced the margin by which I "won". If the two cutters hadn't been such extremes, I wouldn't have "won" at all. The benefit of using a larger cutter for a smaller WOC is clearly demonstrated and the closest thing to an answer to John's original question.

Hugh Venables.

[Jack Mitchell]

quote:

---

I think we need to change your handle to "Hannibal" as you are always looking to devour the rest of us.

---

I actually met this man a few weeks ago; he mentioned my aftershave before he came through reception to meet me. - funny thing is, I fed him lunch just to make sure that I didn't end up on the menu.

 

By the way, lamb chops extra rare is the only way to eat these babies.

 

You guys are killing me!

 

Regards, Jack

[Jack Mitchell]

John,

 

I just ordered the 390 - 2" Facemill with seven inserts.

 

Give me teeth or give me death - hold the Chianti and Fava beans.

 

Regards, Jack