Drilling inconel sheet

[So not a Guru]

We have a couple of 0.063" thick inconel sheet jobs that we need to drill holes in. The hole sizes are 0.098" & 0.221" . Anyone have recommendations for drills?

[jslaero99]

I had good success with OSG Serie 1150, it's a HSS drill (so pretty cheap) and the tool life was very good. One thing to consider, our application was a blind hole.

                  Have a good day!

[So not a Guru]

23 minutes ago, jslaero99 said:

our application was a blind hole.

These are all thru holes. That's my concern, that the drills will chip when the break through the sheet.

[CEMENTHEAD]

IMHO I would ramp/circle mill the holes thru, much less pressure and waaay less of a burr. 

[Metallic]

ramp w/ helical solutions/harvey 6 or 7 flute endmills sounds like a good recipe.

[So not a Guru]

3 hours ago, Metallic said:

ramp w/ helical solutions/harvey 6 or 7 flute endmills sounds like a good recipe.

I'm not sure that's going to work on 0.098" & 0.221" holes.

[crazy^millman]

13 hours ago, So not a Guru said:

I'm not sure that's going to work on 0.098" & 0.221" holes.

Nope. Might drill 1/32 underside then plunge then with a close to size bull endmill to finish them. .095 with .02R and .218 with .03R and call it a day. 

https://www.harveytool.com/products/tool-details-51695-c3

https://www.harveytool.com/products/tool-details-863930-c3

[Metallic]

On 2/19/2021 at 5:46 PM, So not a Guru said:

I'm not sure that's going to work on 0.098" & 0.221" holes.

I guess im confused, Ron gave a link to a harvey EM that would do exactly what I said, helical mill. A 5/64 would give more clearance.

[So not a Guru]

Just now, Metallic said:

I guess im confused, Ron gave a link to a harvey EM that would do exactly what I said, helical mill.

Yes, after my post, he corrected me with those links.

To be fair though, they are 4 flute.

[huskermcdoogle]

Really it all depends on the workholding....  Most typical processes that will effectively cut inconel will do it if you can hold it properly for the op....  Using a drill will certainly be an issue given they are less than 1xd.  The .098" diameter hole might be ok to drill.  I suggest a Kennametal GOdrill for that, assuming it is well supported, such as on a sacrificial support plate.  Reduce feed to 40% of normal feed on exit to prevent blowing the corners off the drill.  The .221" hole, I think i'd go with a helical/circle milling solution.  Using the .098 to pre dill might help extend tool life of the end mill, but would possibly not be overall cost effective.  I think an 1/8" Endmill would be about perfect.  Preferably something with a 1/4" shank and stub length.  3 degree ramp angle, 65 sfm, .0002" chip load.  .005" finish pass on the wall.

[nickbe10]

If you have problems, Mikron Cross Pilots might do the trick.

170 degree point so good for sheet.

Not cheap but we normally get a couple of hundred holes drilling on a 30 degree slope in Inconel (not sheet).