What's new
What's new

Best cutting life for cast aluminum tooling plate hogout?

specfab

Titanium
Joined
May 28, 2005
Location
AZ
So, we have a small VMC (Sharp 2414) in place for doing small volume R&D/prototyping work. Our parts often require use of cast aluminum tooling plate, for stability in the finished part. We are currently running a part from 2" thk x ~8" x ~10" cast plate, starts out at about 23 lbs, finished weighs a bit less than 4 lbs. Lots of material being removed with 3/4" 2-flute carbide endmill, typically 1/2"-5/8" DOC, stepover maybe .5-.6 X diameter. Programmed speed 6K RPM. Final depth of pockets is anywhere from 1" to about 1.7".

Cutter life for the end mills seems short, going from nice-looking part without much burr to a pretty ratty-looking burred edge in 2 parts, total time per part maybe a bit over an hour for rough-out, and interim handling and chip management activity. These endmills are Ultra brand, 45 helix for aluminum.

Anyway, looking for suggestions for highly durable endmills, or insert tools to consider for significantly better lifetime. Thanks --
 
math time.. ROUNDED #'s..

So you are removing approx 20lbs.. Taking an hour including chip removal and what not...

Lets say half an hour. That 6-7 cubic inches a minute.. That's a 1hp cut.. At .6 woc, and .6 doc,
that's approximatley 17ipm.. Which gives you .003 per rev...

Is it possible to rub a carbide tool to death in cast tooling plate?

I haven't run them all that much, but I had one of those Destiny tools with that black coating stay in the
machine for over 2 years, that thing still cut like a champ until I ran into a bolt.
 
Thanks for the feedback. We have 10K RPM available. The parts are 1st-time pieces for an instrument development project, which is also a process development project for trying out some novel techniques in both the instrument construction and the machining processes. We want to come out with good parts right at the outset due to time constraints, so we may be a little tentative in making chips. The fact that it is cast plate with some thin tall walls is also a cautionary element...I am not running the machine or writing the programs (that guy works for me); my numbers are visual estimates just from what I observe.

Thanks for the suggestion on rougher and Destiny tools. We'll look into any and all options.
 
Specfab, IMO the art of hogging is to take as big a cut as possible, at the maximum chipload possible, then worry about the spindle speed ......maintaining that DOC & stepover + feed rate as you up the spindle speed, until you max out on either the cutter speed or spindle load.

But, and especially, - when cutting deep pockets chip clearance is vital. Recutting chips will shag out any tool LONG LONG before it's expected life is up, - it doesn't do much for the finishes either ! and personally speaking I still favour the old school method of hosing the coolant in a fast as you can to flush the chips out.

Richer coolant also helps a lot with aluminium.
 
Have you tried any of the Ripper Mills from Curtis? If the pocket size is large enough you can use a 2 FLT 1" tool and ramp into the pockets, the inserts are razor sharp and throw the chips out of the pockets so very little recutting and the inserts are cheap and last for ever. The only down side to the 2 FLT tool is they are a little nosy at lower RPM but get 10K or more and their sweet sounding but you'll need a fully enclosed machine otherwise it will rain chips on your head.
 
Have you tried any of the Ripper Mills from Curtis? If the pocket size is large enough you can use a 2 FLT 1" tool and ramp into the pockets, the inserts are razor sharp and throw the chips out of the pockets so very little recutting and the inserts are cheap and last for ever. The only down side to the 2 FLT tool is they are a little nosy at lower RPM but get 10K or more and their sweet sounding but you'll need a fully enclosed machine otherwise it will rain chips on your head.

Good call Captdave,

FYI inc a vid, 1 INCH RIPPER MILL
 
Cast plate is abrasive but nicer for chip control.
Do not use .5 to .6 stepover or the tool will flank wear early. (one should never use 50% step on any material, it's a tool dynamics bad spot thing)
Get above or below this value then test carbides and tool geometry.
 
Will second Bobw's remarks...

0.5in dia. 3fl Destiny with stealth coating. Been in the machine for year or more. We cut mostly 6061 cast plate or Mic6 as we build instruments for use in research lab environment (mostly microscope add ons) and need the stability and flatness. Run aforementioned cutter at 10K, 30% stepover on offset tool paths at .8-1d depth of cut. With HSM toolpaths, we lower the engagement of 15-20%, same or somewhat higher feedrates. Usually helix into pockets regardless of tool path type. Leave 0.01 for finish bottom and sides using same tool.

Depending on how thick your partitions are, may need to run with less stepdown and machine all pockets at each depth.

If we get into deeper pockets or larger plates, may move to 0.75dia. Destiny, and finish with 0.5in dia. As others have mentioned, getting the chips out is the key. We'll flood the area heavily and use the chip throwing capability of the Destinys or occasionally Lakeshore cutters to get the chips out of the way.

Fred
 
many alloys are abrasive. not hard but abrasive and are hard on tools.
.
take a grinding wheel, you can open the hole up going slow rpm and just drill it out with a twist drill. of course drilling a grinding wheel with a hss twist drill will dull the drill bit quickly.
.
i often use 1.75" dia roughing end mill taking 1.75 doc and 1.5 woc at 20 ipm feed in aluminum. you need hp and ability to get chips out of the way fast enough and got to be able to hold the part securely.
.
they make 4" roughing shell mills too. 1" doc at 3.5 woc is possible often more is possible. again you need hp and ability to hold parts and flush chips out of the way fast enough
 
Will second Bobw's remarks...

0.5in dia. 3fl Destiny with stealth coating. Been in the machine for year or more. We cut mostly 6061 cast plate or Mic6 as we build instruments for use in research lab environment (mostly microscope add ons) and need the stability and flatness. Run aforementioned cutter at 10K, 30% stepover on offset tool paths at .8-1d depth of cut. With HSM toolpaths, we lower the engagement of 15-20%, same or somewhat higher feedrates. Usually helix into pockets regardless of tool path type. Leave 0.01 for finish bottom and sides using same tool.

Depending on how thick your partitions are, may need to run with less stepdown and machine all pockets at each depth.

If we get into deeper pockets or larger plates, may move to 0.75dia. Destiny, and finish with 0.5in dia. As others have mentioned, getting the chips out is the key. We'll flood the area heavily and use the chip throwing capability of the Destinys or occasionally Lakeshore cutters to get the chips out of the way.

Fred

I would agree with all of this. I can't see how you could be losing a quality carbide endmill in 2 parts. The Diamondback with Stealth I currently have loaded has plowed several hundred # of chips, in 6061, 7075, and a little MIC-6, and shows no signs of deterioration.

Assuming your machine can handle it -- 25% stepover, 2xD axial, .006" - .01" chip depending on ability of control to keep up, max RPM. If your spindle bogs, decrease the stepover.

Regards.

Mike
 
Thanks, ever'body -- good info to work with. We'll look at the actual cutting parameters (rather than my guesstimates from the sidelines) and see where we can adjust to improve lifetime, and look at the other cutters suggested. I certainly thought lifetime should be "somewhat" longer.... We are running coolant at 9-10% to help a little with cast material and deep pockets, and we have been trying to improve the coolant nozzle distribution as well, to make sure we are clearing chips out.

Carbide Bob -- thanks for the definitive statement about stepover ratio.

LimySami --"Specfab, IMO the art of hogging is to take as big a cut as possible"... That was something that I still remember from an interview I had with the shop manager at Harvard Astro lab shop, back in mid-80's when I first discovered I didn't know much: "The most important thing is to get rid of the material as fast as possible..." Still sticks in my mind to this day.

Finegrain, Bobw, Freds -- sounds like a winner in the Destiny line.
 
Finegrain, Bobw, Freds -- sounds like a winner in the Destiny line.

I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.
 
I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.

I also use Alu Power for all finishing and little work. I still like the 1/2" and 3/8" Diamondbacks for 2 reasons:

1. Lower spindle load
2. Chips are much more dense -- 1" or 1-1/4" long strings from a non-segmented endmill are way fluffier and fill the pan much more quickly

Regards.

Mike
 
I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.

You probably know there's a simple dodge to making a roughing cutter ;)

Get a cheap diamond tile saw blade, then mark with a sharpie each flute of the EM in say a 1/4'' pitch helix, then grind your own chip breakers in to the flute - a .030 to .040'' deep nick is plenty.

Okay, maybe it's not the real McCoy, but it still works, .......and when you're in a hole or have a load of cutters on the cheap, nothing beats a few $ in the pocket :D
 
Leave 0.01 for finish bottom and sides using same tool.

You're finishing with the Diamondback? Don't the serrations leave an atrocious wall finish?

I use mine for floor finishing all the time, but come in with another tool for the walls.
 
You're finishing with the Diamondback? Don't the serrations leave an atrocious wall finish?

I use mine for floor finishing all the time, but come in with another tool for the walls.

Diamondback? I think somebody else mentioned that. We use Destiny Viper 3fl, Stealth coating for both rough and finish.

Fred
 
I know that this is an old thread but it might be of some value to revive it.....
I’m machining cast aluminum blanks and just thought I would add this:
Check the part for residual sand from the casting process.
I have rough cast blocks I am machining and it has beaten the APKT inserts that I have been using for almost a year.
The casting have entrained sand from the casting process and I suspect that is what caused the inserts to wear rapidly.

I’m not sure what the best way to get rid of the outside layer of these blocks is.
 
I’m not sure what the best way to get rid of the outside layer of these blocks is.

Don't know if this would help, but how about a 30-40% engagement conventional cut? Push the dirty skin generally straight out into space instead of mashing it into the rest of the cut.

Regards.

Mike
 








 
Back
Top