Shoulder Milling

Upnorth4 · Dec 20, 2019

I am machining an aluminum block. Due to the radius on the corners I am trying to machine 5 sides in one setup.
First attempt was with a long (4" long) 1/4" high helix endmill. I roughed it out in .250 DOC passed and all was great. I had the finish pass to cut full DOC (2.5") contour (fusion toolpaths, .010" WOC .002" chip load. All looked good until the endmill dug in and broke rounding the 3rd corner....

I am open to any ideas, I don't really want to try the long endmill again $$, I was too cheap to go with a large diameter long endmill as the cost seems exponential.

I am considering going with an insert endmill (I have APKT 1003 inserts that run well on aluminum).

Surface finish may not be critical, at first these were to be anodized but now I may powder coat the exterior.

Would this be a reasonable endmill? 5/8" 90 Degree End Mill OAL 7-7/8” APKT Insert

The aluminum is cast, but T5 hardened, not gummy at all and high helix endmills and WD-40 got smooth finishes on the cap ( the cap in the picture was etched harshly (trying out finishes)

ripperj · Dec 21, 2019

This is not really the place to discuss that mill.
2.5” at .010 is a lot of cutting force for a very light machine

Sent from my iPhone using Tapatalk Pro

D.D.Machine · Dec 21, 2019

I have never found insert mills to be good for this kinda part .. the shanks are steel and only about 1/5 th as ridged as carbide ,,, look up YG-1 Alu-power endmills ,, you want non coated and I think they make some 2 1/2" long ones in 1/2" dia ... for the lid run a stub alu-power.

you well need to play with the speed and feed to find a sweet spot were the tool does not chatter. Slow RPM and a med feed rate of like .002 or .003 per tooth should work good. other trick is wrap the od of the part with a chunk of rubber from a inner tube for ID work and for od work ,,, pack the inside with "DARK" brown sugar and bake it at about 300 deg for a half hour ,,, when your done cutting the OD put in a pan of hot water tell the sugar goes away.

"If the ID is small fill it full of ear plugs"
it well keep the part from singing like a bell

Use of WD40 is a no/no on a part like this ,, you need coolant flow or a mister to keep from re-cutting the chips.

Ebay has a lot of the YG-1 alu-power end mills listed and the price is good if you shop around on them ..

DMF_TomB · Dec 21, 2019

.25 dia at 4.0 long thats 16x length to dia
compared to .5 long thats 8x more
8x8x8 = 512 times more deflection for same cutting forces
.
where you could take certain depth and width of cut you would need to reduce 1/512
lucky if you could take .001 width of cut

michiganbuck · Dec 21, 2019

Nice looking part but a ,250 end mill of any kind is a huge waste of effort and time.

QT:[ I was too cheap to go with a large diameter long endmill as the cost seems exponential.]
*For a one up anything that works is OK.. but broken cutters and damaged parts are costly.

Yes a 5/8 real end mill would do better

Upnorth4 · Dec 21, 2019

D.D.Machine said:
other trick is wrap the od of the part with a chunk of rubber from a inner tube for ID work and for od work ,,, pack the inside with "DARK" brown sugar and bake it at about 300 deg for a half hour ,,, when your done cutting the OD put in a pan of hot water tell the sugar goes away.

"If the ID is small fill it full of ear plugs"
it well keep the part from singing like a bell

Use of WD40 is a no/no on a part like this ,, you need coolant flow or a mister to keep from re-cutting the chips.

The WD-40 I am using is sent out of a mister, lots of air to clear the chips.

Interesting tip about the sugar, I have wrapped parts with rubber hose before to stop chatter. At a shop I once worked in we had rubber bungs made up for sleeves that we were turning. This part is rather stout, the vibration came from the endmill that had a ridiculous dia to length ratio.

I found a 5/16" Alu power with just the length I need for $65 on ebay. I figure the diameter will also have an exponential effect on rigidity.

wheels17 · Dec 21, 2019

I don't think you are getting the importance of diameter. Stiffness is related to the moment of inertia. For a solid rod, I = PI x .25 x R^4. So, setting the moment of inertia of the .25 endmill to 1, a 5/16 endmill only takes you to 2.44, where michiganbuck's 5/8 endmill would go to 39.

michiganbuck · Dec 21, 2019

I have set two bar stocks and C Clamp (or two) on the sides of such work if having a hollow midsection for ID.
And a wedge inside for OD.

Yes just enough pressure so not to distort the part.

Mike1974 · Dec 21, 2019

michiganbuck said:
Nice looking part but a ,250 end mill of any kind is a huge waste of effort and time.

QT:[ I was too cheap to go with a large diameter long endmill as the cost seems exponential.]
*For a one up anything that works is OK.. but broken cutters and damaged parts are costly.

Yes a 5/8 real end mill would do better

Really? Hell, that is a BIG cutter where I work... but I digress

I've used a 1/4" endmill with approximately the same length (4.0")... it will work, but you have to think of your speeds (rpm/sfm) appropiately--- something like 100sfm, instead of 300-44... same thing with feed, can't do .002-.003" per tooth, need to be more like .0003-.0004"* per tooth

*don't quote me please, just throwing out examples-'

like we normally use a 1/2" endmill at 1000 sfm and .006" per flute, BUT, when I have to hang it out 2 1/4" from the holder, I go down to something around 3-400sfm and .003" per tooth....

706jim · Dec 21, 2019

1/4" endmill 4" long.

Yikes!

I once used a 1/4" two inch long 4 flute HSS to cut a slot. Only cutter I had that would reach. It deflected enough when climb milling to cut the far side of the slot.

If you want to go 4" deep you will need something stiffer for sure.

michiganbuck · Dec 21, 2019

Guess a long end mill with a bearing at the far end and then a box jig for the bearing to follow in would be good for a production part.. still 1/4" diameter would be chancy.

Upnorth4 · Dec 21, 2019

wheels17 said:
I don't think you are getting the importance of diameter. Stiffness is related to the moment of inertia. For a solid rod, I = PI x .25 x R^4. So, setting the moment of inertia of the .25 endmill to 1, a 5/16 endmill only takes you to 2.44, where michiganbuck's 5/8 endmill would go to 39.

That was a typo, I was looking at a 5/8” endmill on eBay but have since found a 3/4” from a supplier in FLA for $80, much cheaper than I first thought.

CarbideBob · Dec 21, 2019

For various reasons 5/8 end mills in a four flute are a sweet spot for material removal.
This is why you see it used so often in demos.
No indexable cutter can make perfect 90s unless it sits at zero/zero rake and you do not want that. There is always a crown or a cave.
It's rotating geometry problem and is best at only one specific cutter dia for any standard insert design. Note that with the same callout letters and numbers this dia may be different between insert makers.

3/4 is good but is it a steel or Al endmill?
You are going to step this? One could consider high speed paths and go in and knock the corners off first, then profile if you have a endmill with the length.
Bob

D.D.Machine · Dec 21, 2019

cheap and good normally do not go hand in hand ....... cheap carbide I have found looses teeth faster than a crack head

Most of the cheap carbide I have seen seems to use crap for the tool blanks and there is only a few company's like YG-1 that buys so large of suppy of the blanks they can get good carbide to start with ,,,

Upnorth4 · Dec 21, 2019

CarbideBob said:
For various reasons 5/8 end mills in a four flute are a sweet spot for material removal.
This is why you see it used so often in demos.
No indexable cutter can make perfect 90s unless it sits at zero/zero rake and you do not want that. There is always a crown or a cave.
It's rotating geometry problem and is best at only one specific cutter dia for any standard insert design. Note that with the same callout letters and numbers this dia may be different between insert makers.

3/4 is good but is it a steel or Al endmill?
You are going to step this? One could consider high speed paths and go in and knock the corners off first, then profile if you have a endmill with the length.
Bob

This is the endmill I am looking at:
5/8 3 Flute Single End T15 Powdered Metal TiCN Long End Mill

I will step down to rough off the sides of the block and then do a counter pass at full depth to hopefully get a good finish on the sides.

If there is a better "harmonic" with 5/8" than ill go with that over the 3/4". These have a good reputation for good finishes on aluminium.

ripperj · Dec 21, 2019

The OPs mill is no longer mentioned, but unless I mixing up my threads , it originally listed the model.
The mill weighs a couple hundred pounds and has a 1hp motor. I’m not knocking it, and I personally couldn’t care less that it’s discussed here( but it happens to be the rules) , but that mill is not going to do much with a 3/4” end mill.
The machine needs to be taken into account when discussing DOC and endmill suggestions

Sent from my iPhone using Tapatalk Pro

Upnorth4 · Dec 21, 2019

ripperj said:
The OPs mill is no longer mentioned, but unless I mixing up my threads , it originally listed the model.
The mill weighs a couple hundred pounds and has a 1hp motor. I’m not knocking it, and I personally couldn’t care less that it’s discussed here( but it happens to be the rules) , but that mill is not going to do much with a 3/4” end mill.
The machine needs to be taken into account when discussing DOC and endmill suggestions
QUOTE]

Unless there is some rule regardIng minimum WOC per diameter of endmill then a smaller machine CAN use a larger endmill.

The purpose of the larger diameter is to provide the ridgity that the grossly disproportionate 1/4” dia 4” long endmill had.

I have never seen limitations on endmill diameter based on spindle horse power.
Depth of cut, yes. Material removal rate certainly.

I have a 2” face mill that I get great results from, would I shoulder mill 1/2” woc 1/4” deep with it on 1/2 hp spindle? Heck no!

What is your experience with small machines?

Why do I get the feeling you don’t want me to do this?

D.D.Machine · Dec 21, 2019

Upnorth4 said:
This is the endmill I am looking at:
5/8 3 Flute Single End T15 Powdered Metal TiCN Long End Mill

I will step down to rough off the sides of the block and then do a counter pass at full depth to hopefully get a good finish on the sides.

If there is a better "harmonic" with 5/8" than ill go with that over the 3/4". These have a good reputation for good finishes on aluminium.

FYI T15 powdered metal is hi speed steel ,,, "NOT" carbide . Carbide is 5 times more ridged than HSS .

you would be "WAY" better off with a 1/2" carbide than that 5/8" HSS end mill .

Upnorth4 · Dec 21, 2019

D.D.Machine said:
FYI T15 powdered metal is hi speed steel ,,, "NOT" carbide . Carbide is 5 times more ridged than HSS .

you would be "WAY" better off with a 1/2" carbide than that 5/8" HSS end mill .

Despite the better ridgity carbide doesn’t seem to be used with aluminum often. The endmill I linked above has a great reputation for aluminum.

The SFM listings I see for carbide on aluminium (1250) result in high spindle speeds(8000rpm with a 5/8” endmill)

The results for HSS are much much lower. 300sfm yielding a spindle speed of 2000rpm.

Of course these numbers are max “generic” numbers and a lot of “tweaking” with speeds and feeds are up coming.

Also....... Is there any real harm with running much lower surface speeds? I think not.

I have heard that the coatings on carbide fuse to aluminum, chip weld even with good coolant.

Wsurfer · Dec 22, 2019

Upnorth4 said:
Despite the better ridgity carbide doesn’t seem to be used with aluminum often. The endmill I linked above has a great reputation for aluminum.

The SFM listings I see for carbide on aluminium (1250) result in high spindle speeds(8000rpm with a 5/8” endmill)

The results for HSS are much much lower. 300sfm yielding a spindle speed of 2000rpm.

Of course these numbers are max “generic” numbers and a lot of “tweaking” with speeds and feeds are up coming.

Also....... Is there any real harm with running much lower surface speeds? I think not.

I have heard that the coatings on carbide fuse to aluminum, chip weld even with good coolant.

I had a 1500lb mill with 1.5hp spindle. I would definitely go carbide with a long reach cut. Yg-1 are damn sharp which is what you want. Super long high speed steel is going to flex and chatter like crazy unless you relive the shank way back. A large diameter end mill will certainly be way more rigid, but if its more rigid than the mill, its back to chatter town. Probably need very light cuts to avoid violating the model climb milling. The full length finish pass will be tricky. I would use a test piece to dial in the process.

Shoulder Milling

Plastic

Attachments

Stainless

Stainless

Diamond

Diamond

Plastic

Stainless

Diamond

Diamond

Titanium

Diamond

Plastic

Diamond

Stainless

Plastic

Stainless

Plastic

Stainless

Plastic

Cast Iron

Similar threads