Limit of Cat 40 Tooling

[69owb]

Hi All,
Does any know the limit of where you start running in to problems with spindle bearings, pulling the tool out of the taper on a cat 40 machine.
Witch machines seam to be able to handle a bigger cut. Mori, Doosan, Haas with out spindle problems. I'm using a Iscar helitang 2" facemill with 5 inserts 0.900 woc, 0.400 doc, 24-32 ipm, 780 rpm on a 50 taper machine. Looking for future options if a 40 taper is capable of handling it on a daily beating.
Thanks

[trevj1]

You need the .4" DOC, or can you reprogram to run a lower DOC, Higher feed rate?

Most, if not all, of my 'max' cuts are worked out by pushing a little at a time, and seeing what the machine can do.

780 rpm? Why so slow? Stainless of the miserable variety?

You really need to be talking to a tooling supplier, as well as the machine sellers. Very likely, between the sources, someone can put you onto a far more productive solution.

Cheers
Trev

[69owb]

Well I have a total of 1.600" depth to rough out so I have the program loop 4 times, that and I like to use the hole cutting edge. I just updated to this cutter from a Kennametal Mill 1-18 and it works excellent. I was only getting 3 parts from one index of the inserts and usually the insert cracked across the screw now I can run about 13 parts before rotating the insert and also doubled the feed. I'm machining 4340 so I've been running 400 SFM, just looked in the Iscar book and they recommend 330-490 SFM for that material grade. I havn't looked in to the high feed mills yet to see if I can rough the part any faster by traveling faster, my current mill doesn't have the capability to machine at that speed. This process seams to work very well thats why I'm trying to find out if anybody else runs their 40 taper machines like this. Thanks

[dwolfhope]

What insert and grade are you using in the Mill1-18 cutter? How hard is your material?

[underthetire]

Spindle bearings are manufacture specific, so that depends on the builder. Most 40T have the same drawbar tension ~2200lbs. If will make more of a difference how rigid the machine is, tooling life will change depending on the quality of the machine construction. If your doing it day in and day out, and need as quick of roughing as you can get, and looking at new equipment, why not just step up to 50Taper and not have to worry about it?

[69owb]

The insert I think was the EP1808E or the EP1808S and the grade was KC725M. Material is 4340 normalized. (Underthetire) Really I’m trying to find out if a 40 taper could handle it without the additional cost of the 50 taper. The way it sounds from a few Machine dealers is to go the route of a high feed mill. Started running some numbers on some Iscar feed mills they claimed you can run them at 0.080 doc and 0.080 ipt load, a person can machine them faster that way but I would assume you would have to have a ridged machine with pretty good horsepower to run that? Won’t that still be hard on the spindle?

[dwolfhope]

The Kennametal high feed cutter we recommend stating at .040 DOC and .020 to .060 on the feed per tooth. The max DOC is .059. this should not be a problem for a 40 taper spindle. The feed rates can go up to .118 IPT for higher metal removal rates depending on set up and material condition.

[underthetire]

Maybe not on the bearings, but you will need to watch for fretting on the taper. That will tell you if the holder is moving around in the spindle.

[BobWarfield]

Calculator here says that's an 8HP cut you're making.

When you look at the range of spindle HP on CAT40 machines, you'd think that cut would not be a problem.

Try to pay attention to rolling the cutter into the cut if you want to take it even easier on the machine. Search for "Entering and Exiting a Cut" on this Cookbook article:

Machine Tools: Feeds and Speeds, Mill Cutters & Surface Finish

Cheers,

BW