How fast can you push an 3/64 ball endmill

[Delw]

In 6061 aluminum ? The haas is tight as its just a few months old.
.020 depth of cut 12k rpms 4flute.

right now I am at 15.0IPM with a 4flute a few different companies claim 35 IPM and some tell me not more than 5 IPM just curious before I start busting them LOL
I am using Gar endmills I would love to find alum ball endmills that run faster in alum that are small like 1/8" and below so far Garr standard endmills have worked the best.
I havent found one 1/8" endmill that will withstand 100 IPM .150 deep with a step over of .010 . I tried 6 different brands both 2 and 4 flute.
Garr is the only one that doesnt snap at these speeds I know there are others out there. even the Garr people told me the endmills I am using are not for alum but they work.

any suggestions?

I am not complaining about tool salesmen,its just they always tell me yeah yeah yeah, but it ends up wasting my time and money and makes them look like a fool. so I would appreciate it ,if someone who actually uses small endmills(3/16 and smaller) alot on aluminum would reply.

Speed and feed calculaters havent been usefull in real life with ball endmills
Thanks
Delw

[tobyaxis]

Originally Posted by Delw In 6061 aluminum ? The haas is tight as its just a few months old. .020 depth of cut 12k rpms 4flute. right now I am at 15.0IPM with a 4flute a few different companies claim 35 IPM and some tell me not more than 5 IPM just curious before I start busting them LOL I am using Gar endmills I would love to find alum ball endmills that run faster in alum that are small like 1/8" and below so far Garr standard endmills have worked the best. I havent found one 1/8" endmill that will withstand 100 IPM .150 deep with a step over of .010 . I tried 6 different brands both 2 and 4 flute. Garr is the only one that doesnt snap at these speeds I know there are others out there. even the Garr people told me the endmills I am using are not for alum but they work. any suggestions? I am not complaining about tool salesmen,its just they always tell me yeah yeah yeah, but it ends up wasting my time and money and makes them look like a fool. so I would appreciate it ,if someone who actually uses small endmills(3/16 and smaller) alot on aluminum would reply. Speed and feed calculaters havent been usefull in real life with ball endmills Thanks Delw

2 and 4 Flute end mills are weak because of the small core diameter. Try 3 Flute, and 5 Flute end mills. The cores are much stronger and you can increase your feed rate at least 15 to 20%.

Oh and get a Coated End Mills preferably ZrN.

Show that Aluminum who's BOSS.

[tobyaxis]

BTW: here is the Coating PDF from Harvey Tool. You should try some of their end mills.

[BobWarfield]

I know you don't like feeds and speeds calculators, but...

Mine (G-Wizard), says the 1/8" 4 flute can run 0.15" DOC (and assuming a full width slot) at 24 IPM for a solid carbide, and 34 IPM if its coated.

100 IPM would definitely be a problem!

RE ballnoses being a problem, you need a feeds and speeds calculator that will figure the effective diameter based on depth of cut because it changes if you're less than half the cutter diameter deep.

Let's take your 3/64's example:

- 3/64's ballnosed cutter
- 0.020" depth of cut
- Assume solid carbide and full slot width (at least at the cutter's effective diameter when 0.020" down the hole

So the effective diameter for 0.020" DOC is 0.0464", which is pretty darned close to the 3/64's anyway. I make that a 24 IPM cut.

Still not seeing 100 IPM in your future for these operations. On the 1/8", I think the problem is cut depth. Your more than one tool diameter deep, which is hard on those little endmills.

Cheers,

BW

[Delw]

toby thanks for that info. I didnt know they had 3 fluters that small, I might try a 5 also, the 3/64's I am running its coated from garr. on 1/8s I run 2 fluters mostly cause thats all I can find. 4 fluters chatter on me.


bob, I am feeding the 2 flute 1/8 ball at 100 IMP on a 1/2 to full depth cut( full depth meaning the flute length of a standard endmill .500") with step overs being about.010-.015,

on plunge grooves(first cut in x or y) I am going about 27 IPM so the cal is pretty close on that one, I hit 30ipm a few times by accident but they dont last all that long.

Thanks guys.

[Geof]

How fast can you push a 3/64" ball endmill?????

Fast does not come into the picture; the question should be how slow do you need to go with a teenzy ball end mill like that.

[BobWarfield]

Originally Posted by Delw toby thanks for that info. I didnt know they had 3 fluters that small, I might try a 5 also, the 3/64's I am running its coated from garr. on 1/8s I run 2 fluters mostly cause thats all I can find. 4 fluters chatter on me. bob, I am feeding the 2 flute 1/8 ball at 100 IMP on a 1/2 to full depth cut( full depth meaning the flute length of a standard endmill .500") with step overs being about.010-.015, on plunge grooves(first cut in x or y) I am going about 27 IPM so the cal is pretty close on that one, I hit 30ipm a few times by accident but they dont last all that long. Thanks guys.

OK, I was running assuming the full slot scenario, and that one came out pretty close to your 27 IPM.

Now let's look at the 0.010 - 0.015 stepover cuts. Those cuts live to tell about it because of the radial chip thinning of stepovers that are less than 1/2 cutter diameter. If you turn on compensation for that chip thinning, then G-Wizard would say you're good to about 122 IPM on the 0.010 stepover and 99.77 IPM for 0.015 stepover.

And it does like all 12K of that rpm too!

Here's a screenshot of that calculation:



If you haven't ever looked at chip thinning, its a fascinating topic and one of the things that got me started writing G-Wizard.

More info on chip thinning here:

http://www.cnccookbook.com/CCChipThinning.htm

Cheers,

BW

[anemachinebc]

We use a lot of Harvey tools, make small cutters usually .125 and below. They work very good and seem to last a long time. Running alum we only use 3 flute end mills, 2 flutes leave a sh$tty finish, and 4 flutes would load up too easly. Other than that we use primarly Garr and OSG. GW Shultz makes nice cutters as well.

[HuFlungDung]

If the application would permit, look at the Harvey Tool Mold cutters. Look like decently sturdy little ball end tools, if you can work with the angle of the neck.

[Delw]

Originally Posted by BobWarfield OK, I was running assuming the full slot scenario, and that one came out pretty close to your 27 IPM. Now let's look at the 0.010 - 0.015 stepover cuts. Those cuts live to tell about it because of the radial chip thinning of stepovers that are less than 1/2 cutter diameter. If you turn on compensation for that chip thinning, then G-Wizard would say you're good to about 122 IPM on the 0.010 stepover and 99.77 IPM for 0.015 stepover. And it does like all 12K of that rpm too! Here's a screenshot of that calculation: If you haven't ever looked at chip thinning, its a fascinating topic and one of the things that got me started writing G-Wizard. More info on chip thinning here: http://www.cnccookbook.com/CCChipThinning.htm Cheers, BW

I will have to check that one out, never seen anything like that before

Originally Posted by anemachinebc We use a lot of Harvey tools, make small cutters usually .125 and below. They work very good and seem to last a long time. Running alum we only use 3 flute end mills, 2 flutes leave a sh$tty finish, and 4 flutes would load up too easly. Other than that we use primarly Garr and OSG. GW Shultz makes nice cutters as well.

Originally Posted by HuFlungDung If the application would permit, look at the Harvey Tool Mold cutters. Look like decently sturdy little ball end tools, if you can work with the angle of the neck.

Looking into harvey tool, I called them there going to have a tech call me monday. They were pretty cool, I called at closing time and the guy told me all about the stuff for 30 mins then went to hunt down a tech, I told him not to worry about it call monday.
over that time I looked at quite a few endmills, they had a large selection. I just wish there website had bigger text I cant see the stuff LOL.


Delw

[Vogavt]

Originally Posted by Delw I just wish there website had bigger text I cant see the stuff LOL. Delw

Hey Delw,

If you're using IE7, there's a little enhancement in the bottom right-hand corner of the browser. Click where it says "100%" and it will change the size of information. Call it a magnifier! Keep clicking it to see it make changes and cycle through. You can also select the small triangle to the right of it and pick other zoom factors. Enjoy!

Give it a whirl,
Regards,
Vogavt

And to save you the time for looking up Harvey Tools:
http://www.harveytool.com/products/p...y=Mold+Cutters

[tobyaxis]

Originally Posted by Geof How fast can you push a 3/64" ball endmill????? Fast does not come into the picture; the question should be how slow do you need to go with a teenzy ball end mill like that.

Geof is correct on this because if you think about how small the cutter is, and how big the VMC is it is almost impossible unless you have 60,000 RPM.

The Core Diameter of 2 and 4 flute End mills is too small which is why your getting chatter. Your best bet is 3, 5, or 7 Flute because the Cores get Larger while the actual Flutes get Smaller. This means a Smaller Chip Load, but it also means More Chips Per Revolution. Hence a faster Feed can be achieved.

Get one of those Speed Increased Tool Holders and a 3 Flute End Mill. Then you can hit the Feeds you want as long as the Set-Up and Machine can handle it.

Remember to use a High Pressure Coolant Line to clear chips at those increased S&F to help with Tool Life.

The Goal in Machining is to remove as much material as fast as you can with Tool Life and Machine care in mind.

To be honest I have Maxed a 1/32 3 Flute Ball End Mill 8000RPM @ 24 IPM, but it didn't last very long before it wore down and then broke.