cutters for 1020 steel

[Saultspics]

Can someone give me some advise on what cutter to use on 1020 steel? We do 6061 aluminum most of the time so are cutter for steelare slim.

We are cutting hole in plates 2" to 3" OD + or -.001 x 1.5 to 2.75 deep all hole are thru. With a Haas vf6 10,000 rpm 30hp WITHOUT thru the spindle coolant.

 

I was thinking about drilling 1.5" or 1.75" then milling to size.

What type of drill what type of end mill?

 

Thanks

ssaults

[crazy^millman]

I would drill 1" to 1-1/4" with an inserted drill. I would then take an inserted cutter and run with it leaving .005 for bore then finish from there. SFM of about 950 to 1350 with .005 to .009 per tooth feed on the inserted tool. Make sure to keep chips flushed out might use an external air blast to clean them out of the hole or space the plate off the table on some 1-2-3 blocks to give the chips a place to go.

 

HTH

[G Caputo]

I personally having been using these . I'd try running about 1100 sfpm at .010" chip load per tooth with a .030" - .060" infeed. I'd get an appopriate cutter size that would allow you to helical interpolate the hole to say .005" - .010" per side, depending on what your machine can handle at those feedrates, and then go in and take 1 pass with a 1" carbide end mill to hit size. The chip must be going bye bye as millman stated or the tool is gonna have an explosive nature to it. jm2c.

[Saultspics]

Thanks! I will check in to those cutters.

 

How about drills can you drill 1-1/4 or 1-1/2 with a spade insert without step drilling?

 

Thanks!

ssaults

[Guest]

At our shop we use Kennametal DFX Drill body drills. Sorry, no link for this, but Catalog #3070, page H180. Basically you can buy any size of drill up to just above 2", with different shank diameters (which you need to buy a holder for).

 

Although Kennamental recomends thru coolant, I run a VF6 without thru coolant and the drills cut thru QT400 plate without a problem (that crap sucks to work with!). You just need to make sure you have a massive external flood. I actually tapped into the main coolant line and added a splitter and made 3 more coolant lines just for drilling (overkill? maybe, but at $300 + a drill, better safe then melt it into the workpiece).

 

These work good at around 1000 RPM and 3 - 10 IPM (Kennametal boasts up to 19IPM in steel, but I doubt it). And it's nice because they are indexable inserts. And you do not peck drill, although I have used G73 with a .01" retract with no problem.

 

Hope this helps

[Saultspics]

G Caputo

 

What insert are you using button,hi-feed or square for steel?

We are looking at a 1-1/4 cutter.

[G Caputo]

ssaualts,

For the application you are talking about, I'd use the button inserts. The high feed do not like cutting on there sides, but the button geometry it doesn't matter if you are facing or profiling. m2c.