[houdini]

Hello, I am brand new to this site and new to cnc machining.
I just got a job at a local CNC shop and they seem to be having problems with milling a block. I wondered if I might get some input.
The block is A2 14"*16"*6".(x-y-z)
They are using a 1.25" index end mill with only 1 carbide index.(mitsubushi carbide)
pieces in it.
The machines is a Milltronics VM24 I.

they are making a mold for a stamp for a shovel head, It is taking forever, they have tried multiple different end mills and broke them usually with in a hour trying to get a good fast speed.

The mill is running loud and isnt removing a lot of material when trying to get it optimum.

Any tips or suggestions for this block with this machine.
ie different tooling, feeds speeds, you know what I mean.

Currently it is set to .025 depth, cutting at radius except for first cut is 100%. speed is 800, feed is 7in. per min.

mfg (Mitsubushi Carbide)says should be able to due 1200rpm, 3/8 depth of cut, and a far faster feed, is our machine rigidity the down factor here.?

The tool is really long we cut it down but it still is 6" long, but we need to go 6", all the way down on the outsides.

We do 95% Aluminum, so Im assuming thats why they aren't figuring it out quickly.

Heck I dont even know, does A2 come annealed?, I would hope so.

Thanks
CHEERS!

[One of Many]

The A2 should come annealed from your supplier, unless it is being resurrected from some other life history, then I'd at least check it with a file. If a file struggles to cut it, it must be harder than 48Rc, send it out for annealing.

Machining it, I'd consider using a short corncob rougher and hog cut steps over the arc, then finish with a stout radius mill.......lights out if need be.

Look at the feeds and speed cutting data. For the life of me, I cannot comprehend why they wouldn't have a multi-flute cutter. Single flute index on steel? That sounds bizarre!

A2 Data sheet

DC

[houdini]

Have you milled A2 then?
Sorry, lights out if need be?
They tried some rough end mills , is the corn cobb you mention a single end mill or a multi flute indexable tool?

Im too new to this to figure out what the feed and speeds are, they look slow in this tech. sheet?

[One of Many]

Yes, I have milled A2. It is a little tougher than 4130-4340, but still not bad in its natural state. Maybe 20-25Rc?

Lights out is, set it up and run it. Go home, have a beer and kick your feet up. When you return the part should be done. As long as you have a decent cutter, good coolant flow, it should run on its own for several hours at a reasonable pace.

Roughers AKA Corn cobb endmills

The surface feet per minute is listed as 165ft/min for a solid C2 carbide and 400-565 for C5-C6 inserts, Now convert that to RPM based on whatever cutter diameter you intend to use.

Fox Valley Link

The inches per tooth is listed as .003-.008. Use the above link to find the feed rate.

Considering the profile of a shovel, this should all be done for you in the CAM package to create the program path. Whom ever is doing the programming should know this before metal ever meets the machine. The operators duty is to keep a hand on the feed Over Ride knob and keep things under control. That is rather difficult if you don't know what a good cutting process even looks like.

DC

[houdini]

Thanks for you help, this is awesome.
I am brand new at this and they say that the guy that is the main machinist there is good but in my head as soon as I saw him buying a new end mill because he broke the roughers you mentioned and then saw a single flute for steel like you mentioned I was like huh? Thats why Im here.

He cant do lights out because it chews up the carbide inserts every couple hours.
Yesterday the owner ordered 20 inserts to "hopefully" finish the job. CRAZY.

btw they are using GibbsCAM on a Milltronics VM24

[One of Many]

Gibb Scam as I have heard, can have issues with feeds and speed as it selects it. I don't use it, but that seems to be a common complaint.

Regardless, the operator or the programmer should have enough experience to make changes after seeing it run to prevent impending disaster. The color and thickness of the chip(AKA Chip Load), along with sound and vibration of the machine will be a fairly good indicator of running conditions. Some compensation must be given to how well it is being held on to. While there is optimum, there are also limitations that must be gained, unfortunately...via bad experiences. Be that broken cutters, flying parts or just creating cool looking scrap.

It is fairly common that ball nose radius insert cutters are single tooth. Those can be reasonably productive with aluminum at high spindle speeds, but steel is a totally different circumstance. I'd think minimum of a 2 flute, but as a matter of efficient material removal, it's counter productive. A solid 3-4 flute might be a better investment at slower spindle speeds. Other contributors can chime in with greater experience in this regard.

The other concern with ball nose cutters is that where the cutter meets the material, the circumference changes, which affects the mean SFM and feed rate. While the optimum spindle speed and feed rate may be calculated at the cutter diameter, if the cutter is larger than say 1/2-5/8", the spindle RPM can be too slow as it cuts material nearer the center and the feed rate too fast to handle the chip load. Typically the programmed speeds and feeds are modal(do not change once set) unless the programmer takes that into account, or an attentive operator is given the option to make adjustments based on current conditions in the path. Doing a one off die won't really allow for much efficiency improvements on subsequent parts, but in a production environment it becomes key to profitability.

DC

[jetski]

I hard mill after heat treat H-13 which is similar to A-2. When I do my finish pass the steel is 48-52 Rockwell c scale. I use mainly SGS tianamite coated cutters. I have cut H-13 with an Ion nitride coating .008 thick 72 rockwell c with the same cutters. Just got through building a injection mold tool that is H-13 tonight. All except for tap and water holes cut in the hard state.