Drilling cast with inclusions

[MDLang]

Over the last few months I've been hammering down the run time on a repeat job we get that is cast 4130.

Started at approx. 27 minutes and tomorrow I'll be trying, again, to make the final move into the 7.5 minute range. Each cycle produces a part finished both sides and ready for a second op on the 4th. I managed to take the second op run time from 16 minutes down to 7 but I'm still struggling to make my final move on the first op.

Feedmilling has produced the bulk of the gains. For the first op we face and pocket and drill with feedmills one side at a time on two pieces. this brings us down to 13 minutes Vs. the original 27 but so far I can't coax a reliable increase in my drilling time for 6 - 5/16 holes on each piece. If tomorrows attemp works I'll be at 7.5 minute but I expect failure.

Here's the problem. Inclusions will destroy all but HSS and Cobalt drills run at a stupidly slow speeds and the hole tolerance while not bad +.005 dictates a drill in fairly good shape at a fairly slow feed. I'm not drilling deep but the entries are problematic. On one set of holes we enter on a .125 radius and on another we enter through raised lettering on the casting. Self centering drills which typically handle higher feeds and with a coating higher speeds loose their flanks on the rad and the lettering and carbide blows up on the inclusions.

Tomorrow I will try a coated cobalt Nachi multi-facet style self centering drill so I can feed higher and run the higher speed but I will have to replace the center drill with an endmill to spot the hole locations. If this works yeha but I fear the inclusions are going to get me. Hss and the softer cobalt jobber drills will dull but the harder cobalt and carbide chip or explode.

Any suggestions for a 5/16 drill that will push through what I think are ferrosilicon inclusions, lettering and enter on a radius in customer supplied 4130 castings, at a minimum 110 SFPM and a .007 feed per rev. while not requiring a center drill and loving every minute of it. And if you have the solution have you patented it?

Mike

[ctate2000]

How deep?

[MDLang]

.9 to break through into a cavity on the deepest hole.

I've gone ahead and tried the Vega ESS Cobalt drills, no peck, 80 SFPM and a .006 feed, 60% feed on breakout.

6 minute time savings per cycle and I'm getting about 13 pieces per drill so, I'm going through the drills but at $48.00 CDN a drill I'm way ahead of where I was and I still have a drill I can send out for sharpening.

Mike

[ajl6549]

Have you tried solid carbide?

[HuFlungDung]

I'm old school I guess, I would not attempt to ever start a drill on any kind of inclined or rounded surface unless I either spot face a flat spot full diameter of the following drill, or less desirably, use a spot drill in a stubby collet to try to minimize drift of the starting hole.

[MDLang]

I've tried solid carbide but the inclusions are very hard and solid carbide chips badly or shatters if it hits one.

I should mention that I went ahead as in my origional post and am using a 5/16 endmill to spot the hole locations ahead of the drill.

Mike

[ajl6549]

There are some sub-micron grades of carbide with PVD coatings, on the market such as those made by Iscar,(see this site http://www.iscar.com then select e-catalog once there select "inch" so as not to view all metric tools) that are acctualy "tougher" (having higher transverse rupture strenth) than h.s.s., cobalt or powdered metal etc. we use them in some nasty forged and cast steels.

[tunitime]

Try Kennametal TF style drills. They are solid carbide with 3 flutes.