Using the Shars 7/8" insert end mill on a BP

Jake2465

Registered
Registered
Joined
Dec 27, 2017
Messages
340
So, I needed to machine out this piece of aluminum for part of the helicopter project. On hand I had an insert end mill that I got from eBay for the sole purpose of giving me some deep hole machining capability. The stick out needed to be 3" so the collet nut would not end up crashing into the top of the part.

Note: rpm was set to 3000 for both tests.

my first attempt was to use the entire depth of cut that the inserts could give me, which was about 0.350. Then I went down to a 0.100 width of cut and tried to run at 12 inches per minute. The results were not great and I was getting a lot of vibration. So I aborted the run and went back to the drawing board.

I knew the problem was that the mill was not liking that much sideload from a tool with that much stick out, so, the answer was to find a way to reduce the side load and increase the axial load (vertical load). I went from a 0.350 depth of cut, down to a 0.035 depth of cut. I increased the width of cut to 100% of tool width. I increased the feed rate to 60ipm.

metal removal with initial settings that gave me problems:
0.350 depth x 0.100 width x 12 feed = 0.42 ci/min

metal removal with modified settings:
0.035 depth x 0.875 width x 60 feed = 1.84 ci/min

The results were much better and although this is not really supposed to be the way to run an end mill, it's working well for my applications and that's all that matters. I had to push the mill to 60ipm to eliminate chatter. Once I did that, then it worked out ok. I used mist coolant and lots of it. The mix was Kool mist 77 with water. Spray mist had to be used because the inserts are not nearly as sharp as an end mill flute and chip weld would have been near-instant. I had my air gun handy and good thing too. It started to chatter when recutting chips, so I had to keep blowing the chips out of the hole every few seconds. Should have brought my snorkel gear along.

information on the end mill:

I got it from eBay from that Shars dealer located in Illinois:

cleardot.gif

I went with this end mill because it had a 3/4" shank, but the diameter of the actual cutter was 7/8". This would eliminate any chance of the tool rubbing on walls.

The only downside is that I found out I had to use their proprietary inserts which were not all bad because their prices were reasonable. I went with these inserts simply because that's what I could find on eBay, although I believe they have some that are actually intended for aluminum:

 

Attachments

  • pic1.jpg
    pic1.jpg
    75.8 KB · Views: 56
  • pic2.jpg
    pic2.jpg
    104.6 KB · Views: 56
Wanted to verify you are doing climb cutting as opposed to conventional milling. Per Jim's recommendation use aluminum specific inserts makes a big difference. APMT you are using is for stainless, so not optimal for aluminum. Usually there is more information as speeds and feeds for a particular cutter head and insert, but what you are doing looks conservative. On the inserts, my read is you can use APKT which are very common but according to the holder information they only say compatible with ZCC inserts which is strange.

FYI, I use the Minicut Wave endmills, something along the lines of the 930PM-2440 has a 4" DOC and typically in aluminum I can do a 1" with a DOC 0.3" or greater at 3200 RPM around 12+ IPM. I use these for rapid material removal and deeper cuts, 3/4-1" size endmills. The wall cuts are also very clean.
 
Wanted to verify you are doing climb cutting as opposed to conventional milling
Yes, that is correct. I am using climb milling.

according to the holder information they only say compatible with ZCC inserts which is strange.
Strange indeed. I ordered other inserts and had to send them back because they would not fit. I ended up just going with those inserts I purchased.

I do need the correct inserts for sure. Normally, I use ALU-Power end mills from YG1 whenever I need to cut aluminum. They have performed very well and I was able to maximize the power my mill could give me and hit around 6 ci^3in/min. It was throwing a little rooster tail of aluminum and that made me happy. I took a swig of sweet tea and chomped on my burger while watching that mill get with the program. Life was good that day.

Anyway, this is my first time dealing with some deep hole stuff. The only tool I had on hand that could do it is said Shars insert mill. But, I believe for Low HP mills, regular carbide end mills cannot be beat in performance with their sharp gound edges and higher helix angles. The only rub is that the end mills that get that large in size start to really cost come coin.
 
I looked up the inserts on the Shars website and I noticed that they were not the 1003 series inserts. I ended up ordering these other inserts from eBay since they explicitly stated that they were 1003.


I hope those work out.
 
They are pricy but I use solid carbide reduced shank end mills from Maritool for deep hole/pocket finish work. Roughing is done with corncob roughing end mills after pre drilling as much as possible. Good chip clearing is esential for finishing.

Sent from my SM-G955U using Tapatalk
 
I was just talking to Jim about insert end mills and I think the consensus was that it's hard to get a knee mill to behave well with those things. Helix geometry is just not optimal. My mill only weighs about 3000lbs and uses the little quick-change 30 taper Erickson holders.

I have had good success with using a big 1.5" indexable end mill as a face mill. Good finishes and such. But, once I try sideloading the tool, the mill starts to complain and I noticed that the quick-change system seems to not be real fond of high amplitude vibration. I've had the big spanner nut start to work itself loose before when I tried running an indexable T-slot cutter for 5/8" T slot nuts. It vibrated like hell and I started to hear a pitch change mid-cut and hit the E-stop. sure enough, the nut loosened up and was thinking about dropping the tool holder out of its quill.

After this thread kicked off, I did go and research some of the end mills. Unfortunately for me, most of them were a bit out of my budget since I do not have any immediate work to perform that can offset the cost. I ended up bidding on this new carbide end mill from eBay and picked it up for about $60 bucks. I figure if I use it for aluminum, then it should last a very long time. This one is from a company in CA called "Promax", model # 109-04846. It is a 3/4" three flute with a 3-1/4" LOC.
 

Attachments

  • end mill.jpg
    end mill.jpg
    638.1 KB · Views: 14
Roughing is done with corncob roughing end mills

How do those run in terms of noise and performance? Also, I have heard others say that odd-numbered flutes tend to vibrate less. I am not sure if that means they vibrate considerably less or marginally less, lol.
 
How do those run in terms of noise and performance? Also, I have heard others say that odd-numbered flutes tend to vibrate less. I am not sure if that means they vibrate considerably less or marginally less, lol.
Roughers are amazingly efficient at removing a lot of material quickly. I can't say I ever recall experiencing any unusual vibration with one.
 
Back
Top