Inconel 718 Machinability

[rdshear]

The most common material we machine here is 4140 Q&T.  I have a customer that wants us to quote on a shaft made from Inconel 718.  Can this be machined with normal carbide tooling and HS taps & Drills?  Just trying to figure a factor for machining this Vs what we are accustomed to.

[JParis]

Can this be machined with normal carbide tooling and HS taps & Drills? 

I found over the years that straight carbide worked best with 718 Inco...

HSS Drills & Taps....I wouldn't suggest it.  Carbide all the way

Understand, you will measure tool life in minutes

[rdshear]

Thank you, Looks like I'll be getting some tooling pricing.

[Thee Byte]

The most common material we machine here is 4140 Q&T.  I have a customer that wants us to quote on a shaft made from Inconel 718.  Can this be machined with normal carbide tooling and HS taps & Drills?  Just trying to figure a factor for machining this Vs what we are accustomed to.

Usually you can get material specific inserts that will perform better for inconel, I'm with JP I wouldn't try with the hss

[CNCAppsJames]

If you can machine it with ceramic tooling, DO IT! 

MRR is exponentially better. 

[gcode]

Thread milling is the only way to go in inconel

I did a job last year that had lots of threaded holes
I used MA Ford thru coolant 3X drills
The machine has 1000 psi thru coolant and Rego Fix PG25 tool holders were used.

I used https://carmexusa.com/default.aspx?page=item%20detail&itemcode=FMT10074F1616UNMT8 Carmex thread mill.

Note that is has 6 flutes and the OD is Ø.291 for a 3/8-16 thread
A nice tight machine and high pressure through coolant is mandatory

Feeds and speeds were 2153 RPM @ 1.5 ipm
cycle time per hole was under 30 secs and we got about 30 holes per tool.
These feeds and speeds are straight out of the Carmex thread milling wizards
and are on the conservative side.

Adding up the drill and thread mill, you are still looking at $10/hole in tooling costs.
but that is better than breaking taps in $20K parts.

I can't recall ever successfully tapping inconel.

[rdshear]

I've been a fan of carmex thread mills, I'll look into those.  Thank you all for your valuable information. 

[gcode]

Feeds and speeds were 2153 RPM @ 1.5 ipm

I should mention that the operator ruined the first thread mill on the first hole.
He ran it an 50% rpm and 25% feed rate crept up on it .001" at a time.

We bought 2 tools for the job.
I told him to load the 2nd tool, set CDC to 0, feeds and speeds at 100% and keep your paws off the dials.
The second tool ran the whole job.. and even salvaged the work hardened first hole which we saved for last.

[riverhunter]

plus 1 for Carmex.  Great thread mills and good online info.