Max Roughing of aluminum

[DTHOMSON]

We have a part that is 7"x7"x3" aluminum and is taking 50 minutes to rough on an 3yr old Hardinge VMC. I am using Surface High Speed Core Roughing, 1" dia 3 flute Data Flute cutter in a mill chuck, DOC of .5 and .2 stepover. It wants to chatter and the operator cuts the feed to 20ipm at about 3500 rpm to stop it. I would welcome some suggestions on the best way to rough this part. Is HS the way to go? Or do I use a Corn Cob Rougher for deeper cuts per pass? I put it on the FTP site under X4 files and named it High Speed Flange. Thanks in advance.

[cobra95kev]

What is the max RPM you have? 50 or 40 taper?

How long is the endmill?

[DTHOMSON]

Great questions. Max RPM is 12,000. It has a BT40 taper and the length of the cut on the end mill is 3 inches. Thanks.

[Jayson Kramer]

Go after dynamic milling you should be able to move that out in a 3rd of that time with that tool.3" is long but not to bad for a 1". do you need to cut thru?

[Chris Rizzo]

EDIT:

 

just saw you put it on the ftp. Trying it now.

 

K I just uploaded something to try.

 

Put a surface over the top to keep the core roughing out of the hole. Much quicker and smoother to blast that round hole with just a contour ramp. On the core rough, increased doc to .7 , reduced stepover to 10%. increased feed and rpm lots. Your leaving .050 so I turned up your tolerence to reduce code. Set entry to feedrate (not plunge rate). Retracts switched to minimum distance and tweaked the leads a bit.

 

Probably not perfect, but should get you closer and much faster and smoother ( and keep the operators hand out of it )

 

[ 02-25-2010, 01:46 AM: Message edited by: Chris Rizzo (Italian' stylin') ]

[DTHOMSON]

Jay, I have not tried dynamic mill but I will look into it. For HS roughing should I be using a corn cob style cutter or a standard aluminum cutting endmill.

Chris, I appreciate your effors on this. I'll let you know what we find out.

[Chris Rizzo]

Standard should be fine. 3 flute is key though.

[jeff]

Stupid question but, your 1" endmill has a bright finish right?

I haven't seen the part, but try looking at the OSG Blizzard endmills, or the Hanita 3 flute Javelin endmills.

I can run a 1/2 blizzard 8,000 rpm 200IPM taking up to 1/4 width of cut full depth.

[cobra95kev]

Sounds like these guys got you on the right track.

I would use up to 10000 rpms if possible without going to hard on the spindle. We use regular solid carbide here for roughing.

[Dave.L]

quote:

---

It wants to chatter and the operator cuts the feed to 20ipm at about 3500 rpm to stop it.

---

How is the part fixtured? If it's not rigidly clamped you will get chatter at almost any feedrate.

[Zoober]

On our 12K spindles, we use HSM exclusively. No corn cobs, Destiny Vipers and Hanita 4AN kick. Look for variable helix to reduce chatter.

I don't go over 3/4 dia. Full RPM, 600+ IPM.

Look for tool corner radiuses at .06-.12 or so, and utilize chip thining techniques.

I havent seen yout file, but we rough a 6x6x10.5 box, which ends up with 3/8 walls x 5+" deep, in about 16 minutes. Was 6 hrs on old slow mazak, using 1-1/2" corn cobs.

Oh, and all that on a .125 dovetail.

[spade117]

Fixturing is key. I saw the part, just don't have time to play around with it, but from the looks of it, roughing time shouldn't be more than 10 minutes.

[Dave.L]

A few years ago we had some enclosures to make. Simple parts just a bit big. If I remember correct they were around 4" plate x 8 x 8.

 

One of my guys used a 3" Iscar face mill to core these out. 12K and fast. 2 Ops to complete the parts, it took like 5 minutes total.

 

[Elmer Fudd]

The chatter is from the long end mill. Use a standard length cutter to rough the top section then use the longer one to get the deeper sections. Dan

[Dowty123]

We also use Data Flute ALDH-C 1" neck down 6" OAL 4.25 stick out and we run at 8500 at a feed of 180 without any chatter. We're in a shrink fit on a taper 50 tough.

[Dave.L]

quote:

---

The chatter is from the long end mill

---

1 to 3 ratio

 

Not that long at all.

[BenK]

3500rpm at 20ipm is only .0019fpt. For roughing aluminum that is really low. I use Ski-carb endmills from SGS they recommend 1600-2000sfpm at .010fpt. I would look into what the manufacturer recommends and start there, but also remember chip thinning.

[Zoober]

With chip thinning, we get upwards of .04 fpt. Just depends on the geometry of the part and tool.

Pretty rare we are under 300 IPM unless we are drilling .093 dia x 5" deep.

Those iscar Helido's are aluminum eaters.

[Nick Eaton]

I think the chatter problems are because of the type/size of cutter.

I've never been a fan of 1" solid carbide 3 fluters. Even in a super rigid 50 taper system with lots of HP they just don't seem to cut smoothly. Not to mention the expense.....

On a Hardinge 40 taper they are way overkill. You just haven't got enough HP and rigidity to overcome the torque forces at the cutting edge so the whole thing starts vibrating.

5/8 or maybe 3/4 will allow you to achieve maximum material removal rate with this machine at a far lower price. Up front sharp free cutting insert cutters are the other option if you are set on the diameter, Dapra (as mentioned above) and Misubishi are examples.

Your maximum material removal rate will be 4x the HP (continuous) of your machine in cubic inches per min..

You can use any radial and axial engagement you want to suit your cutter.

You should try and use the highest spindle speed which gives peak HP on the torqe curve of the motor, this will allow you to keep a high chipload (.006+ - I prefer to run .01+) and prevent thermal distotion of the part.

As far as programming strategy I like to look at each part/machine system indidually.

Somtimes I'll use short axial broad radial engagement sometimes the other way around, this is usually driven by part geometry and the cutter you select.

Hope this helps

Nick

[DTHOMSON]

I appreciate all the input and the effort by everyone. We have reduced it down to about 20 minutes. I guess I don't completely understand the references to "Chip Thinning". Could someone provide additional info on exactly what this should entail.

 

Nick - I really found your comment about the size of the cutter insightful as I had wondered if this was just too big.

[Zoober]

Here is a link to a decent explanation of most stuff inserts. By Ingersol, but pretty good reference for many terms, including a good explanation of both lead and radial thinning.

 

Liny-Dink

[DTHOMSON]

Zoober -I really appreciate the link. I understood lead thinning, but never saw charts for factoring correct feeds for fadial thinning. Thanks Again!

[Zoober]

Glad to help!