A bit confused here.

MC program has the half inch 2 flute endmill speed rate suggested at 12 ipm, but this does not take into account the depth cut I have set at .125..

I am running 2hp Industrial Hobbies mill around 3,200 RPM. What depth cut should a 7/16 or 1/2 two flute endmill Tin Coated and HSS be doing? If the depth cut is .125 what feed rate should I be running at? Or is .125 too conservative for 6061 aluminum.

The part I am cutting is 25" long about .75 deep with pockets and so forth. Right now with 12ipm feed rate at .125 it is taking about 6 hours. Looking to reduce this time without wearing out stuff

Mill 3200 rpm 2hp Industrial hobbies, with Mist (NO FLOOD).
6061 Aluminum x=30" y=6" z=.75" stock

R.

It is hard to suggest feeds for a mill that I'm not running. Just run the spindle as fast as the tool can take, and in aluminum bump up the feed rate until:

a: you run out of power
b: you can't clear the chips out,

discovering optimum speed is quite an art.
Thanks much

At 12 ipm you are feeding to conservativly. Your chip load is only .002, with a 1/2" mill I would run with a chip load of .003-.004 which would put your feed rate at 20-25 ipm. I would reduce the depth of cut to .100 and try it at 20 ipm for a start. According to my software you would be using a little over 1/2 a horsepower to achieve this. Of course I would also use a 3 flute mill in order to run at an even higher feedrate. Hope this is of some help.

roger that I bumped it up to about 20imp now with no problems really. have gotten a couple chipped endmils no idea how that is happening the part is well ancored maybe larger chunks becoming lose during contouring operation.

R

roger that I bumped it up to about 20imp now with no problems really. have gotten a couple chipped endmils no idea how that is happening the part is well ancored maybe larger chunks becoming lose during contouring operation.

R
Are you cutting dry? You really will need coolant to achieve max feed rates and not chip the endmill or gouge the aluminum.

using mist coolant only..

using mist coolant only..

Mist is ok if that's all you got, flood is better as it gets the chips out of the way. A strong stream of air works well for chip removal as well, the idea is to not be recutting the chips. Try a 3 flute end mill, I think you will be impressed.

According to my software you would be using a little over 1/2 a horsepower to achieve this.


Hi,

Do you mind me asking what software you are using?

John

Hi,

Do you mind me asking what software you are using?

John
Millworks, it's a free speed and feed utility that calculates feed, speed, horsepower, amount of material removed per minute, etc. Here's the link
http://lovejoytool.com/free.htm
I use this all the time when I program our VMC, works like a charm for getting you pretty close to where you need to be as far as feed and speed goes.

just wanted to say thanks for the advise on this thread. I know the question was quite open ended, which is never a good thing, which takes some patience to answer. Cheers.

R

Millworks, it's a free speed and feed utility that calculates feed, speed, horsepower, amount of material removed per minute, etc. Here's the link
http://lovejoytool.com/free.htm
I use this all the time when I program our VMC, works like a charm for getting you pretty close to where you need to be as far as feed and speed goes.

Thanks for that; I have an old copy of ME Consultant 2.0 which gives the same numbers as you did other than the power requirements which is 0.284 HP for a full width cut.

Looking back at the first post in this thread I noticed a Tin coated HSS EM was being used. From what I have read on the zone Tin is a bad choice for use with aluminium as the chips stick to it. Ticn coating is better but more difficult to find on HSS.

John

Thanks for that; I have an old copy of ME Consultant 2.0 which gives the same numbers as you did other than the power requirements which is 0.284 HP for a full width cut.

Looking back at the first post in this thread I noticed a Tin coated HSS EM was being used. From what I have read on the zone Tin is a bad choice for use with aluminium as the chips stick to it. Ticn coating is better but more difficult to find on HSS.

John

I was always under the impression that Tin coating provided lubricity, and was a good choice for aluminum. Granted I don't use it hardly at all, so I can't speak from experience.

Thanks for that; I have an old copy of ME Consultant 2.0 which gives the same numbers as you did other than the power requirements which is 0.284 HP for a full width cut.

Looking back at the first post in this thread I noticed a Tin coated HSS EM was being used. From what I have read on the zone Tin is a bad choice for use with aluminium as the chips stick to it. Ticn coating is better but more difficult to find on HSS.

John
Yep, TiN coating is generally a poor choice for aluminum, TiCN is far better. I usually buy the TiCN coated carbide mills, sure they are more expensive up front but they last a really long time when milling aluminum. I'm still running a 5/8 endmill that has to have a 1000 parts on it, still looks brand new and cuts like it too.

I have had good luck buying TiCN coated HSS cutters of the Niagara brand.
I still ONLY use carbide in .5 and smaller cutters.
When I am looking for a less expensive alternative for large dia cutters I will buy TiCN (the are much better than TiN on any metal).

Based on the advise.

I ordered a 1/2" and 1/4" TiCN 3 flute for Aluminum from McMaster. How much faster should I be cutting with these over the two flute.

Saying I am around was around 20ipm with 2 flute .125 depth 2hp, 3200 rpm, mist no flood.

Thanks

Based on the advise.

I ordered a 1/2" and 1/4" TiCN 3 flute for Aluminum from McMaster. How much faster should I be cutting with these over the two flute.

Saying I am around was around 20ipm with 2 flute .125 depth 2hp, 3200 rpm, mist no flood.

Thanks

28 to 38 ipm should be fine for the 1/2" mill, I would decrease your depth of cut to .100 though. As a general rule you can increase your feed by a third when using a 3 flute versus a 2 flute. You will have less chip clearance with a 3 flute tool, so you really should work on getting those chips out of the way, even if it is just an intermitent blast of air from an air gun.

Don't worry about your IPM.
Feed is calculated by the chipload per tooth.
3 Flutes X .004 chip/tooth = .012/rev
3500 RPM X .012/rev = 42 IPM

I think you see how this is going.

If you have questions about chipload, every manufacturer has charts (recomendations) for their cutters.
These charts usually include DOC recomendations and increaser percentages for the different coatings.

Eventually you will know everything and will not need the charts anymore

Once you have your feed numbers is doc governed by spindle power, machine rigidity and tool diameter?

John

"Once you have your feed numbers is doc governed by spindle power, machine rigidity and tool diameter? "

Yes!

I have some 3 flute SC endmills, Recommended feeds and speeds to 1x Dia slotting cuts 10,000rpm and 100"/min. Don't be shy!

Experimenting with your setup, will determine your best DOC for the application

Based on the advise.

I ordered a 1/2" and 1/4" TiCN 3 flute for Aluminum from McMaster. How much faster should I be cutting with these over the two flute.

Saying I am around was around 20ipm with 2 flute .125 depth 2hp, 3200 rpm, mist no flood.

Thanks

I would very much appreciate an update on this thread when you try out your new tooling.:)

John

I would very much appreciate an update on this thread when you try out your new tooling.:)

John


Finally got to use the 3 flute Ti 1/2" Niagra endmill today. Running it at 24ipm, with .15" depth cut, at 3200 rpm with flood on 6061 T6 Aluminum.

It is quite impressive. Firstly the cutting is very quiet, wisper quiet! at most half of the noise level of the 2 flute enco standard mills. It seems to be removing the aluminum with zero effort. And the cut seems cleaner.

wondering now how fast can I go with this!

I am sold on 3 flute endmills, and Niagra right now.

Finally got to use the 3 flute Ti 1/2" Niagra endmill today. Running it at 24ipm, with .15" depth cut, at 3200 rpm with flood on 6061 T6 Aluminum.

It is quite impressive. Firstly the cutting is very quiet, wisper quiet! at most half of the noise level of the 2 flute enco standard mills. It seems to be removing the aluminum with zero effort. And the cut seems cleaner.

wondering now how fast can I go with this!

I am sold on 3 flute endmills, and Niagra right now.

Thank you :)

I est. a feed of up to 33.35 IPM at 3200 RPM with a IPT of .0035 using a 3 flt 1/2 endmill full width of cut .150 depth. That's a 2.5 CIPM removel rate (full width of 1/2 cutter). At a max 84% step over the feed can be increased to 36.39 IPM (so long as not the full width of cutter.) But the CIPM is reduced to 2.3.

So long as this does not slow down the spindle or move the setup.

[For a finish pass I would limit the feed to about 15.36 IPM at 3200 RPM. Of course faster if finish requiment is still met. If there is no bottom/end cutting the finish feed should not be less than 36.2 IPM or more than 86.4 IPM depending on finish requiments. ref 1/2 end mill at 3200 RPM.]

Good call. I checked it is / was TICN

Here is the order from McMaster:

HSS THREE-FLUTE END MILL FOR ALUMINUM, TICN COATED, 1/2" MILL DIA, 1-1/4" LENGTH OF CUT $20.09

Now for the bad news. I have ruined two of these. But besides that have been getting lots of Chip loading.

After about 15 hours have had about 3-4 times it loaded up doing 3200 rpm, .15" depth cut, 24 ipm feed rate. Here is a video of it really loading up badley at 40ipm feed rate.. What a mess.

http://www.terrablades.com/MVI_1149.AVI

Eeeks! You are correct, what a mess.

Ok first full disclosure. I do not pretend to be a professional machinist so take what I say with a grain of salt. There are FAR more qualified people here but I have been down this path and I have gotten things working pretty well here. I started with a Mach controlled HF mill, now we have a nice mach controlled BP clone and are getting ready to get a Haas VF-3...

First, tooling. Throw those enco Ti coated end mills in the trash. I thought the same thing at first too, Hey I can get like 14 different end mills in a box for like $50, woo hoo. Yea, not so much. Learned real fast you get what you pay for when it comes to tooling.

I now use only solid carbide uncoated two flute high helix. It might be over kill but my bits last forever, I never break edges (unless I drop the dang thing, then it is off to the regrinder) and things don't load ever. I only have a mist system and I mix it pretty rich.
The BP only has 5600 max rpm and I have found that I just don't have the cooling or spindle speed to make three flutes work effectively. It seems that the two flute are better at getting the chips out of the helix and reduces the chance of loading especially at our rpms.

If you have a chipped edge than that bit is shot and needs to be reground. Chipped edge doesn't shear metal, it just pushes. I have found this is a sure fire way to start a bit down the loading path. On the FIRST sign of loading STOP. IF you get a little load you can stop and use a scribe or something to pop out the loaded stuff and continue, I like to give it a shot of WD-40. I am sure that this doesn't do anything for more that a sec or two and is probably just a good luck charm.
The video that you posted, wow never loaded one like that. That bit is probably history. You were not cutting anything just smearing around metal.
It looks like you have a flood rigged up. Never cut without it. And I would also mix the cutting fluid richer, can't hurt.

Speed: As fast as your spindle can go. When milling alum my mill has one speed, as fast as it can go.

Feed: I have found that the recommended chip loads and feeds and speeds don't usually work very well for those of us without a mega dollar vmc. I usually start out with something conservative and in the ball park then start upping the speed until things start getting funky, bad finish, loading, machine groaning...

You have a small machine, I have a bigger, small, machine. A big real cnc is a totally different animal. I realize that you want to get stuff made as fast as possible, however loaded bits and ruined work takes a lot more time than slower and cutting correctly.

Anyway just some suggestions. Good luck.

Chad

That is some excellent advice from Chad. When it comes to tooling, never buy the el-cheapo crap. I wasn't able to see your video for some reason, so what is the grade of aluminum you are cutting? If it is something like 3003 series, that is really gummy, and the WD-40 trick is the best for that. I use 3 flute endmills from these guys (http://www.lakeshorecarbide.com/). I cut aluminum on a daily basis, running a .750 diamteter cutter at 8150 rpm, 150 ipm, .300 depth of cut, 85% stepover. I have found the ZrN (ZIRCONIUM NITRIDE ) works best and tool life is exceptional. Check their website, they have speed and feed charts and cutters with other coatings for steel, stainless, etc. and their prices are better than anyone else I have found.