inconel 625

[mig]

Hi ,

Current project from inconel 625 drive me crazy.

Spatially drilling holes (0.25 dia 1.5 deep and so ).

I looked thru the forum and still nothing works for me so far.

Carbide drills(garr) snaps, cobalt drills snapping too .

Surface speed 20 inch/min

Really don't know what to do .

Some people in forum saying that inconel it easy ,but i really stuck .

[Greg_J]

I was drilling Incoloy 925 100 sfpm @ .001 fpt with though coolant to keep the tip cool.

 

Maybe your drilling too slow?

[jeff]

Garr is ok for most mild steels, but they just can't compete with OSG,Titex, and Gurhing in the more harder/exotic materials.

[Guffie]

+1 to Titex...

[htm01]

did you heat treat first?

[chip]

Surface speed 20 inch/min

What numbers are you running? Spindle is? And what feed?

[mig]

For cobalt drill i trying :

s=250 f0.5 inch/min

[Guest CNC Apps Guy 1]

IIRC, the 925 has a higher nickel content. The hole is shrinking on the tool which is why they are breaking. I'd interpolate those with a stub LOC .1875 Varimill @ about 100-120 SFM and .0005 IPT feed.

[mig]

IIRC, the 925 has a higher nickel content. The hole is shrinking on the tool which is why they are breaking. I'd interpolate those with a stub LOC .1875 Varimill @ about 100-120 SFM and .0005 IPT feed.

 

agree i interpolate what possible to interpolate but 0.088 dia hole on 1.05 deep ......???

Also testing new line of Garr cutters for Inconel , works fine so far .

my biggest problem is deep holes .

[Guyinthedesert]

For cobalt drill i trying :

s=250 f0.5 inch/min

 

 

Feed sounds a little slow. Try .90/1.20 ipm. Are you pecking? If you are, don't.

[robk]

0.088 dia hole on 1.05 deep ......???

 

We have a job here that has been running for a couple of years now that requires (36x) Ø.065 (+/-.002) holes x 2.302 Deep" (.0058 True Position) in IN-100. We were not able to do it inhouse. We outsource the parts to a gun drilling outfit. The would not disclose the the tooling they use (I don't blame them).

 

That being said Mitsubishi has some off the shelf drills @ Ø.089 (Micro MZS Series) with coolant through capabilities. We use them on some pretty tough materials with good results.

The Ø.250x1.500 holes you mentioned in the original post do not sound like they should be much of a problem. We go smaller and deeper on regular basis in a bunch of different HRSA materials. For carbide I would use a Kennametal Y-Tech Series drill @ 66 SFM using .002 IPR. 1000 psi should be a must, but if you do not have the pressure you might have to give it a couple of pecks.

[mig]

IIRC, the 925 has a higher nickel content. The hole is shrinking on the tool which is why they are breaking. I'd interpolate those with a stub LOC .1875 Varimill @ about 100-120 SFM and .0005 IPT feed.

 

If hole is shrinking on the tool ,packing must be smallest possible ?

I did lots of materials in past,include Titanium ,but this one is drive me crazy .

[T_MALENA]

Have you tried OSG or Titex?! 1/4 dia drill #1 choice - Titex A3985 TFL drill 1400rpm .003ipr then A6485 TFT drill to depth same rpm & feed. #2 OSG list 5200 series is AlTin coated carb. @1400rpm .003ipr #3 OSG also list 1900 is powered metal TiCn also good 350rpm .003ipr. Only peck drill if you dont have enough coolant pressure to blow the chips out the hole. If pecking, a minimum of .07, youll create a somewhat hard surface if you baby the cut - then youll be drilling hardened Inconel! ALSO coolant condition is very important. When machining Inconel I charge it up! I run 12% sometimes higher. Chip removal is important.

 

HTH

[McLaren]

Don't c'drill the carbide drills, and if you are make sure the c'drill is 140º.