What cutter would be good for this?

[MILLRUNNER]

I work in a tool and die shop and I regularly run a 3 axis vertical CNC mill. We cut alot of tool steels (D2, A2, S7, 01) and whe are having trouble finding a good cutter. An HSS rougher of the highest quality and coating will last, but eventually fail. Carbide face mill cutters do pretty good, but they take forever. I have been given the opportunity to grab some tools, and I want to get the best couple of ones for the job. Right now I am cutting a 1 inch deep depth of cut with a 1" DIA cutter and taking the full with of the cutter. I know a carbide rougher would work well, but what kind? A indexible endmill would be cool, you know the kind with the inserts running up and down the flutes. I am just not sure what would be the best cutter to get. If you have more questions feel free to post them, and I will try to get them answered. Thanks.

[kinglouie V]

for D2 especially I would go with a high end grade of iscar(inserted cutter). runs like nitro and you iscar rep should know how to apply optimum sp&fd. I personally shocked at how fast I was able to get away with running D2. I asked my rep, "are you sure?", to which he replied "cut it!". I never looked back.

 

[Colin Gilchrist]

Millrunner,

 

Your best bet would be to talk with a couple different tooling reps. Tell them what you are cutting and that you are looking for maximum material removal rate.

 

For example, you are using a 1" cutter at 1:1 Depth to Diameter ratio, with 100% radial engagement. What speed and feed are you running?

 

You might be able to get a "high feed" mill that will only be taking a .04-.08 deep cut, but you are running a feedrate of .05-.1 PER REV! So instead of feeding at say 10 IPM, you might be feeding at 250 IPM in the same material.

 

It seems counter intuitive, but it works great. Regardless of the technique, you should be able to get much higher performance out of carbide than high speed steel.

[crazy^millman]

I would strongly recommend highfeed cutters and stay away from the nasty tools as I call these indexable fluted tools. The cause more problems than they are worth. You need some very very strong Iron and need some major chip evacuation for these things to be ok at best. The there is the loading up on inserts, you can not push them that hard and most times only use the bottom couple inserts. Highfeed cutters are better value for the price of the cutter body, life of insert and wear and tear on the machine. It is truly amazing to watch them run the 1st couple times, but once you use them you will never look back. Most people will give you them on a test, I like the Seco, Mits, and Iscar. There are others all pretty good.

 

HTH

[cqualls]

I like the Walter Novex High Performance inserted cutters for ruffing. In P20 you can run 200 ipm at about 1400 rpm. With a 1 1/4 inch diam. cutter you can take a .059 deep pass.

We bought the screw fit head type and I was pleased with it.

[Murray Mold]

Iscar Feedmills work great. What you lose on d.o.c. you make up with feeds around 200ipm at .035 to .05 d.o.c. I cut H-13 mostly doing 3d surfacing and I use Iscar feedmills and Fraisa ONLY. When I came to MM&D we were making the same mold inserts and it was taking over 24 hours to cut one and I'm currently doing them in less than 7 hours.

I see you're in Alabama, my Fraisa rep might be in the same district. I will gladly give you his name if you want to look at some Fraisa tools.

www.fraisausa.com

[MotorCityMinion]

Cqualls, have you tried the Novex in D2, M2, A2? If so what results did you get with these?

 

Nobody here has asked what make of machine your running. Rigidity and HP are so important. We use Walters alot at work, Haas verticals, and I typically rough with a large radiused insert and have had good results.

[Colin Gilchrist]

Horsepower becomes less of a concern with high feed tools. The lower depth of cut tranlates into less torque/horsepower required...

 

Rigidity is very important though...

[High Sierra Plastics]

DOn't forget the only problem with indexable cutters is if one insert goes it really trashes the cutter and part. jm2c

 

Henri

[Goldorak]

you should not use extended flutes cutter less than 2.0 dia.

 

i will certainly use iscar's feed mill i always had good result with multimaster series they are very fast

 

[cqualls]

We used them a lot in P20 and H13 on a Haas machine when I was I PolyTech Molding. Same results in either material, 200 ipm at about 1400 rpm and .04 to .05 depth of cut. 1 1/4" diam. cutter taking a 1" step over. The inserts in these cutters hold up really well.

We didn't cut much A2, and don't believe we ever cut D2 or M2.

The only down side to the cutter is noise level. They are loud but I would presume that is the case with any of the new high feed mills.

I Would Check with the local rep when I bought these cutters they were gauranteed to do the job or they would give a full refund, even if I crashed the tools while testing them they would refund my money.