High Feed Insert Cutters

[g huns]

In our quest to go more faster, I started in the area that was our biggest bottleneck, 3D finishing. It was the area I knew the most about. When someone told me we couldn't do it any better, I was able to call BS and show them they were wrong.

 

The next on my list of painfully slow to watch processes is when we rough using insert cutters. The cutter we use most is an old SECO 1-1/4", 3 insert, high feed cutter, the screw on type. I know very little about using such cutters so I deferred to our operator as to how it should run. He gave me 500SFM and a .008" chipload at .035DOC and 70% stepover. So that thing runs 1500RPM and 37IPM, not really "high feed" if you ask me. I thought he was full-o-chit so I dug out the SECO book. I hate that book. After puzzling over their material groups and insert grades for an hour, I came to the conclusion that he's pretty much right, I think.

 

I started googling and saw new SECOs, Mitsubishis, Ingersols, etc just haulin arse. The choices are overwhelming. So my questions is, whadda ya like?

 

I should add, we are roughing mold cavities, P-20, S-7, H-13, to +.030 on machines ranging from a CAT50 Enshu to a couple of ragged out Fadals.

[MIL-TFP-41]

Personally I am a big fan of Mitsubishi's AJX cutter. You should have no problem getting .04 chip per tooth at that depth of cut.

[Beem]

We just started running a Kennametal (formerly Stellram) HFM.  We're using the C7792VXD12 in the 2in size.  It runs faster, deeper cut, and is capable of more than our older Ingersoll ones.  This tool is capable of a lot more than the Ingersoll as well.  We cut mostly H-13 in both hard and soft states.  

 

http://www.kennametal.com/en/products/20478624/57493250/556247/46610642/100048482/100048483/100048492/100035123.html

 

We currently are running it at 1050RPM, 289IPM, .05DOC, with a 75% stepover.  We could push it more, but don't have a need to.

[Goldorak]

we use tungalloy's feed mill here 

 

rarely we feed under 150 ipm even in SS316 or 4140HT 

 

in mild steel we can push it over 300 ipm without problem 

 

[g huns]

What is it that makes these things capable of taking those crazy chiploads?

 

Browsing Kennametal's site, it looks like I could replace my 1-1/4, three flute, at .008"IPT, with a 1-1/4, five flute, at .040"IPT. That's crazy.

[jeff]

Mitsubishi AJX is a good cutter, right now we have a Sandvik HFM (can't remember the model # offhand) and it's a really nice cutter.

 

With m ost high feed mills, you should be upwards of .04 ipt and a light d.o.c.

[jeff]

That's crazy.

 

 

Not really when you think about it, the high feed mills are designed in such a way where the cutting force is directed up in the Z+ (if a 3 axis vmc), making it more rigid.

[Goldorak]

What is it that makes these things capable of taking those crazy chiploads?

 

 

Chip thinning factor  

 

even with a .04 IPT the chip itself still at .005 thick 

[Matthew Hajicek - Singularity]

The screw on type give you more setup flexibility 'cause you can put it on different shanks and extensions, but it will be noticeably less rigid than a one piece cutter body.  Some companies even offer a cutter body with integral CAT-40 or HSK shank for even more rigidity.  More rigidity of course means you can push it harder. 

[Sticky]

Chip thinning factor

 

even with a .04 IPT the chip itself still at .005 thick 

 

That is part of it. Physically the difference is relief angle behind the cutting edge, you need enough clearance so that the non cutting edge doesn't smack the material after the cut.

[gms1]

I used to use the crap out the mits AJX but I switched to iscars medium high feed H600 mills. I can get 6 indexes off 1 insert with those and still feed the same as ajx with more DOC.

 

The reason these tools can offer .040" chiploads is because of the insert geometry. I cannot for the life of me find this really neat picture I had of the process but because of the insert geometry as it enters the material the chip maintains a constant chip engagement. Its not instant engagement for the whole insert like a rectangular insert. Its got a nice gradual lead in built right into the insert shape. The main problem I have with these tools is explaining to people they really need to be engaged in the material (I shoot for 60% engagement all the time). Everyone wants to use them to side mill their 3" tall blocks cause it goes reaaaal fast... silly people.

[jlw™]

I love high feedmills. I really prefer Iscar but Ingersoll has one that is on par.

 

I run an Iscar fast feed and medium feed. I have 1in, 2in, 2.5in and 4in. My favorite little 1in runs .8in woc, 0.02in doc, 500sf to 700sf and 0.02-0.03ipt depending on material. The slowest I run it is 100ipm, normally in the 160ipm range. Next if doc allows I run a 4in medium feed 3in woc 0.035ipt/62ipm at 350sf in 4140, p20 and final fxt1 and t2. It comes in at over 20 cubes.

 

I have an mcam tool database of all I run if you want I'll send it and you can spy some of them to your parts to see if you can win.

[g huns]

I have an mcam tool database of all I run if you want I'll send it and you can spy some of them to your parts to see if you can win.

I appreciate the offer, but I don't use MC.

 

I went back to the Seco book, like a dumbarse, I was looking at the wrong table. Mine can do .040IPT. Took me a couple hours to figure it out. I HATE that book. I feel dumb, not as dumb as the operator who's been running it wrong for 10 years, but still dumb.

 

Maybe next week I'll crank her up and see what happens.

[gms1]

I appreciate the offer, but I don't use MC.

 

I went back to the Seco book, like a dumbarse, I was looking at the wrong table. Mine can do .040IPT. Took me a couple hours to figure it out. I HATE that book. I feel dumb, not as dumb as the operator who's been running it wrong for 10 years, but still dumb.

 

Maybe next week I'll crank her up and see what happens.

 

Lol I don't like their catalog either. The only reason the boss will not order Sandvik is because he hates trying to find anything in there.

[THEE THAINZ™]

Here is some info for you.

b028a AJX Brochure.pdf

[THEE THAINZ™]

I have 2 more brochures but they are too big to down load.

[g huns]

I have 2 more brochures but they are too big to down load.

 

Thanks. That's plenty to chew on.

[SlaveCam]

Sandvik has also some good info on chip thinning: http://www.sandvik.coromant.com/en-us/knowledge/milling/getting_started/general_guidelines/max_chip_thickness The bigger the lead angle, the faster can go.

I love the Pokolm Quadworx high feed milling tool for fast material removal. The lead angle is 80 deg and it can feed 1.5mm (=0.06 inches) per tooth with 0.8mm (=0.03 inches) depth of cut in tool steel (HRC 33).

[jlw™]

It's funny this has come up. We got a few cutter to try recently.

 

We have a 4in Ingersoll, 7 inserts, 0.05ipt, 0.05doc, 3.6woc, 350sf at 116.9ipm. That's 21.042 cubic inches in tool steel. The impressive part... it does it for 4 hours.

[g huns]

With our various Seco cutters, we might make it 45 minutes with a set of inserts but even an hour is pushing it.

 

I think a lot of our problem is the path itself. With our kosher software, and I assume most others, the actual shape of a feedmill isn't accurately defined. The extra stock it leaves behind is sometimes engaged in a conventional cutting direction, or in other less than optimal ways.

[jlw™]

I agree. I find area mill or area surface rough gives the longest life. Then I play the step over to leave minimum "pyramids" where the tool runs around corners. Opti paths make the tool last longer but are geared towards depth of cut instead of width of cut and can literally add hours to a program. I will also use contour/trim a lot to get the exact path I want. Width of cut affects area paths more than depth of cut so my fisrt adjustment is to woc. Usually go up before I go down.

 

I also really like the little 1in Iscar feedmills. No matter what I run them in they last 90 minutes or more.

[g huns]

Feedmills are not new technology. Is defining their shape and calculating the remaining stock left behind still not possible within current software?

[jlw™]

mastercam supports it, not with custom tool but with a tool definition. It will only get close to some, if they are a radiused or compound angle it won't fit. I always do a custom tool then check it in Verify. You can see exactly what stock is left that way.

 

 

I wish that custom tool was more than "for looks" and actually used in more than 2 toolpaths.

[M Horton]

90 mins on same edge? I'm lucky to get 60 mins/ edge in p20. The local iscar rep said 60 mins is doing alright. way to burst my bubble. I've noticed the edges of iscar tend to break don quicker then that of the ajx, but with tice the edges plus n extra insert i can't complain. One questions i have been pondering.. High pressure tsc or air blast?

[crazy^millman]

I always ran air I never ran coolant.