Cyle time help in alum.

[Decomaster]

We are machining some parts out of 6061-T6 that is about 5" X 4" X 2.5" thick using a 3 flute Diamond Back series roughing endmill form Destiny Tool that works awsome, the only problem is we don't have the horse power to make our cycle times faster. We are running the parts with a .75" endmill on a Haas VF-4 with supposedly 30 horse power at 10000 rpm and about 110 ipm. I can only go about a .5" deep on the cut or the machine runs well beyond 100%. The cycle time right now is about 10 minutes and needs to be more like 8, but we just don't have the HP. Does any one now if there might be a better cutter that reduces horse power without losing cycle time? Thank you all very much for your time.

[?Mark]

Not sure about the shape of your part, but if possible try using plunger to take the meat out and then finisher...

Just a suggestion

Kind regards, Mark

[?Mark]

By the way

quote:

---

30 horse power at 10000 rpm

---

on a hass vmc ???

I doubt it

 

Kind regards, Mark

[Mike Whitten CAD/CAM Contractors]

You may need to just slow the RPM down as you are most likely out of the high HP range. I am not familiar with the cutter you are using but I would try a normal (like a YG) 3fl HSS TICN hog mill for aluminum at about 6k-7k. I would think you can get about twice the cubes from this machine than you are getting.

 

Mike

[Decomaster]

I know. That is what I was trying to say. There is no way that the machine is actually putting out 30 horses. Do you have any good ideas on a plunge cutter? We have been looking but no luck.

[Mike Whitten CAD/CAM Contractors]

Use HighFeed with a HSS Hog mill.

[jeff]

We bought an OSG 2 flute Blizzard carbide endmill.

That thing shreds aluminum. about $70 for a 5/8 endmill.

They sy run it at 7500 rpm 205 ipm slotting.

5/8 d.o.c.

Osg reps came in and did tests on it.

We also use Imco 3 flute 3/4 Streakers with .03 corner radius,work just as good,but streakers are almost double the price.

[mrainey]

By my calculations, you're removing just over 40 cubic inches/minute, which should require 10-12 HP at the spindle with 6061.

[?Mark]

quote:

---

Do you have any good ideas on a plunge cutte

---

There is plenty around. Try Iscar PLX plunger (6 flutes), will do face milling also. Step over up to .400" and as deep as you are willing to go

On a 2" you can go S2900 and F120.0 or more.

It's a great way to go only on certain parts, so give a local rep a call if you are not sure

 

Kind regards, Mark

[Chris Rizzo]

I have had good sucess with those destiny diamond back roughers. They do seem like a bit of "horsepower hogs", not sure about their rake angles? I can tell when they start to go though, the loadmeter will go up considerably.

 

gotta get to work.

[Rick McAllister]

Decomaster,

Try reducing your depth of cut to around between .150 and .200 axial, increase your feed to around 400 IPM. Make sure you coolant nozzles are on the tool tip from all sides. Your cycle time will be reduced proportionately to the material romoval rate increase.

[MACHINEMASTERG]

like rick said does the haas have the high speed look ahead lighter depth faster feed ive run our haas in the 400 ipm range no problums

[Jack Mitchell]

+1 to Rick's comment.

The other thing to consider is the beating you're putting this machine tool through.

I always go light axially and heavy on the feed, this way the machine tool should last a lifetime.

 

 

Regards, Jack

[Mike Whitten CAD/CAM Contractors]

You may not be able to convince the Haas to go 400ipm. This is why I believe it is just better to use a good Hog mill and bury it and go to town. You won't run into any servo lag problems either.

 

Mike

[notso]

We had a VF-5 at my old shop that we consitently ran at 125-150% on the load meter. About 5 years of that abuse and no problems as of yet. I can't remember exact speeds & feeds But it seems like we were doing 7000 and about 125ipm full tool width and around .5-.75 doc w/ a 3/4 in minicut endmill. Like I said we ran it like this all the time w/ no probs but it was common for the spindle speed to drop by 1k or more during a long cut like that.

[Charlie Pierson]

Take a look at the AB Tools "Shearhog"

at

www.abtoolsinc.com

 

they say to wind it up and then feed it as fast as you machine will allow

 

works great !!

 

cp

[DavidB]

Hi all,

To rough Al I use Sandvik Al Kordel cutters.They are 3 flute RMR cutters.In your 10,000 RPM machine.

Converting your Yanky sizes to Metric I would run a 20mm Sandvik cutter at 10,000 RPM and at 6500mm/min at 8mm deepth of cut and 8mm step over that works out to 7.9KW = 10.6 Horsepower.

Taking the full width I would use 4mm step down at 10,000 RPM and 7100mmmin that works out to be 4.2KW = 5.63 Horsepower. Assuming you have Ridgig setup and Min overhang!

I have 20000 RPM so I run even faster.

Believe me these cutters work and the sound of swarf hitting the gaurds is heavenly

 

[MetalMarvels]

+1000 to Charlie on the AB Tools - I have one of the 1-1/4 diameter tools and it really blows the chips out in a hogging operation. Only good for non-ferrous though and the inserts are a bit more costly (BTW - if you DO get one of these - they warn you about cutting yourself with the inserts - they MEAN it!!!). I use a Fadal 3016 at about 5500 RPM, DOC of .15, and feed of 100 IPM with only a 75% load. I found that a spiral conventional cut from the center was the quietest on my machine. It is fairly quiet (in comparison with a 1/2-inch MAFORD moving as fast as I can push it). Great tool for owners of low-power equipment (like me).

 

I also needed to watch my setup on cuts - the stream of chips coming off blew the paint off of the doors on my mill - they also get into EVERYTHING in the machine. On top of the tool changer - in the tool changer - on top of everything in sight - they bounce off 2-3 walls sometimes inside the machine. My vintage of 3016 is open-topped - wasn't THAT fun! I now have an enclosed system (made up some 1/4 plex guards for the "roof" of the mill).

[one shot]

I really the Putnam AP series for alum. Blows right through it. 1/2 em .5 dp 6000 prm ( max I have ) .008/rev cuts real clean w/ good tool life.

[Chris Rizzo]

AB seems like a smaller outfit. How are they about service/insert supply, etc? You have to contact the factory for inserts, or do local suppliers carry them?

[MetalMarvels]

I went through my local Shop Tools dealer - I could have had the tools overnite, but settled for shipping via ground since I wasn't in any hurry. The one time I ran out of inserts, I had them the next day. A word of caution - ONLY AB tools has these inserts to the best of my knowledge. They are a specially ground insert apparently designed specifically to rip through aluminum like nobodies business. On the plus side, they have been in business for quite awhile (28 years I think). I always have gone through my local supplier, but I think that you can order direct.

 

I also have one of their 2-1/2 inch shell shear-hogs. Great tool for my low-powered mill and uses the same inserts.

[Psychomill]

AB Tools is a smaller outfit but seems to always carry stock. I've never had a problem with getting stuff, even customs. I've had a lot of custom sizes, lengths, and other configurations done by them using the same inserts. And yes, it does rip and kick a$$! It will run faster than most people are willing to push a machine.

 

Shop Tools is the only tool supplier I know of that carries/distributes them. Thats why Gary can buy them in Colorado Springs/Denver.

 

Cmr, you can buy them direct as well. Check out their online catalog here AB Tools

You can order through this site as well or contact them direct. They're a good bunch of people.

 

You'll definately have fun with one.