So not a Guru

Inconel 625 & 718

Recommended Posts

Can anyone suggest good cutters for these? We are quoting several part numbers, they will be from billets, so we'll need good roughing cutters as well as some finishing bull mills of various corner radii.

Any tips on what works well as strategy is appreciated too. We've never cut any of this stuff & I've heard it can be difficult to master.

Share this post


Link to post
Share on other sites

High Feed  or 7 to 9 Solid Carbide cutters. I have seen some able to get up to 220 sfm and handle it for about 1 hour cut time.

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

My experience is with Incoloy 925 but I'm sure it similar enough.

I would use solid carbide endmills Incoloy likes sharp tools so if you have to use inserts get ones with positive geometry.

I've switched from indexable cutters to endmills and shaved hours and hours off of the parts we make.

When using indexable because your cutting so slow if your machine can handle it increase the depth of cut if possible.

Be prepared to use a lot of inserts.

 

For example:

Standard Z level roughing took 30 hours, same feature using Dynamic OptiRest took 7.5 hours. Huge difference. The endmill lasted the entire time never had to change it, in fact it's still in the machine. It was Kennametal Harvi 1 HPHV1000S4400 KCPM15.

I didn't even have the best coating for Incoloy on that endmill.

 

110SFPM at .005 fpt

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

If you've never cut it be careful with your quote, don't get caught with you pants down.  Its not difficult to cut once you learn what it likes, but tooling cost will be high and you're not gonna go super high feed.  I never cut it with anything more than 5 flutes, but I can see where more flutes would be very helpful, like Ron said.  This was about 6 years ago for me, but IIRC, we had great success with Kennametal Harvi tools on the mill, and for the roughing on the lathe we were using Walter inserts.  Things may have changed since then, but the ticket was low and slow.  I think we were running about 1800rpms on the mill.

First day on a new job boss calls a meeting and he says "we just got a large order for all inconnel…  I had never heard of the material...ooff!

 

 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites
1 minute ago, AMCNitro said:

If you've never cut it be careful with your quote, don't get caught with you pants down.  Its not difficult to cut once you learn what it likes, but tooling cost will be high and you're not gonna go super high feed.  I never cut it with anything more than 5 flutes, but I can see where more flutes would be very helpful, like Ron said.  This was about 6 years ago for me, but IIRC, we had great success with Kennametal Harvi tools got the mill, and for the roughing on the lathe we were using Walter inserts.  Things may have changed since then, but the ticket was low and slow.  I think we were running about 1800rpms on the mill.

First day on a new job boss calls a meeting and he says "we just got a large order for all inconnel…  I had never heard of the material...ooff!

I agree, I like to quote 8 to 9 times the cost of the part in 4140.

If parts made in 4140 run at 600 sfpm and Incoloy 100 sfpm so that's 6 times slower and then indexing time, operators are constantly changing inserts then there is "pucker factor". The cost of the part operators are measuring and remeasuring the part to make sure its right, it all adds up.

  • Like 3

Share this post


Link to post
Share on other sites
3 minutes ago, Greg_J said:

I agree, I like to quote 8 to 9 times the cost of the part in 4140.

If parts made in 4140 run at 600 sfpm and Incoloy 100 sfpm so that's 6 times slower and then indexing time, operators are constantly changing inserts then there is "pucker factor". The cost of the part operators are measuring and remeasuring the part to make sure its right, it all adds up.

Exactly the hidden cost of making parts most places never think about and then wonder why they can't make money doing it.

Share this post


Link to post
Share on other sites

It does not warp, due to the high nickel content. I've roughed large amounts from a billet/forging and it's very stable.

We turn many of the parts and we will finish with .500 wall thickness and there is no noticeable changes any thing thinner and I'm not too sure.

I plan to use ceramics on the next batch of parts that come through I hope to decrease the roughing cycles like we did on the mills using endmills.

  • Like 1

Share this post


Link to post
Share on other sites

IMCO has some 1/2" 7 flute cutters that run at 90sfm & .0084ipt at 2D adoc & .06D rdoc. Have any of you used this brand before?

Share this post


Link to post
Share on other sites
31 minutes ago, So not a Guru said:

IMCO has some 1/2" 7 flute cutters that run at 90sfm & .0084ipt at 2D adoc & .06D rdoc. Have any of you used this brand before?

Yes used that brand before and seems slow for their cutter. Might try 110 to 130 sfm and see what kind of tool life you get. Watch the ROC with a 7 flute more than 5% and you might have issues with building up the chips on the tools. 1000 psi with TSP is a night and day difference that just regular flood.

  • Like 1

Share this post


Link to post
Share on other sites

I've always been a fan of ceramics on the exotic nickel based alloys... Spendy, but worth every penny IMHO.

Share this post


Link to post
Share on other sites
2 minutes ago, cncappsjames said:

I've always been a fan of ceramics on the exotic nickel based alloys... Spendy, but worth every penny IMHO.

Ceramic endmills?

  • Like 1

Share this post


Link to post
Share on other sites
14 minutes ago, So not a Guru said:

Ceramic endmills?

Yep. Check out YouTube. Looks like they are on fire when you run them right. :rofl:

 

Cutting speeds of 350-1000m/min recommended. :D

  • Like 1

Share this post


Link to post
Share on other sites
7 minutes ago, cncappsjames said:

Yep. Check out YouTube. Looks like they are on fire when you run them right. :rofl:

That looks pretty awesome!

Share this post


Link to post
Share on other sites

Yon need a machine with the rpm, many of our mills only have 4k spindles but we have two new Mazak J400 that have 12k spindles so I would like to give it a try.

When it comes to turning it spins too fast to not use a tailstock, it would have to be application specific.

 

GreenLeaf seems to have impressive speeds and feeds in Incoloy.

Turning 600-700SFM / .008”-.010” IPR / .050” - .080” DOC - 7-8mins of tool life

Milling 2000SFM / .004” - .005” IPT / .050” - .080” IPT.

  • Like 1

Share this post


Link to post
Share on other sites
24 minutes ago, Greg_J said:

Yon need a machine with the rpm...

I forget that sometimes. :rofl: Our machines typically START at 12k. The majority of what I see is 15k and 20k spindles. 

Share this post


Link to post
Share on other sites
2 hours ago, So not a Guru said:
2 hours ago, cncappsjames said:

I've always been a fan of ceramics on the exotic nickel based alloys... Spendy, but worth every penny IMHO.

Ceramic endmills?

Yeah, looks pretty awesome..

This video walks through the do's and don't of programming with ceramic endmills/inserts

  • Like 2

Share this post


Link to post
Share on other sites
On 2/12/2021 at 9:54 AM, Greg_J said:

Standard Z level roughing took 30 hours, same feature using Dynamic OptiRest took 7.5 hours. Huge difference. The endmill lasted the entire time never had to change it, in fact it's still in the machine. It was Kennametal Harvi 1 HPHV1000S4400 KCPM15.

I didn't even have the best coating for Incoloy on that endmill.

 

110SFPM at .005 fpt

Was that with the square corner or bullnose?

Share this post


Link to post
Share on other sites
4 hours ago, donjbray56 said:

We have a new silicon nitride material, highest strength on the market.  Please contact me if you would like to explore a better cutting tool.

Don Bray

[email protected]

419-619-1872

Okay great shut up or put up. Show us some Endmills made of this material to cut 625 or 718 with some speed and feed recommendations. Then someone might call you until then I consider it just a sales pitch.

  • Like 2
  • Haha 2

Share this post


Link to post
Share on other sites
21 minutes ago, crazy^millman said:

Okay great shut up or put up. Show us some Endmills made of this material to cut 625 or 718 with some speed and feed recommendations. Then someone might call you until then I consider it just a sales pitch.

I was thinking that - I just didn't want to say it.  :lol: 

  • Haha 1

Share this post


Link to post
Share on other sites

Don't forget that if you are using Ceramic for Roughing, to leave at least 0.080 (2 mm) for Semi-Finishing and/or Finishing. This is to get underneath the Heat Affected Zone (HAZ) created by the roughing passes.

  • Like 1

Share this post


Link to post
Share on other sites

Ceramic for roughing and finishing, Greenleaf, seco, mitsubishi  comes to mind for tooling. Forget about coolant...not even a drop, lol

Count on spending 1-5 bucks per minute of cutting just for tooling, depending on what your part looks like....

Use tool life management on the machine....have several replacement sister tools on hand and such...FUN! ;)

 

Share this post


Link to post
Share on other sites

I have been trained to figure about 6-8 minutes planned tool life with inserted ceramic milling tools (round negative inserts) if you are running them at the optimum conditions.  Plan for using redundant spares if you need more than that and just divide up the time equally between them and change them every part.  Have spares ready outside the machine to swap it.  Roughing with ceramics is by far the fastest way to plow nickel based material off your part.  Through spindle air isn't a requirement, but is highly highly highly recommended.  It just helps to make sure the chips get away from the cutting zone and off of the workpiece.  

You will chip /  damage the paint in the enclosure, and any you won't be able to see through any plastic windows shortly after you start cutting. 

IT WILL BE LOUD, especially if you are getting the level of productivity what warrants the use of them.  But generally speaking ceramic inserts are on par or likely cheaper than the carbide inserts that might survive, but will smoke carbide on cost per cube removed, and time getting it done.  Let us not forget in a job shop environment where the next job is waiting, cash is king, and you need a balance of roughing cycle time / cost per cube removed, that you make sure to bias toward getting it roughed out as fast as possible while still falling within the tooling allowance quoted for the job or within the machine rate. 

If you are running negative rounds, and keep the depth of cut below a 45 degree engagement angle, in theory you should be able to get about 8 indexes per side.  But mind you they are typically infinitely indexable.  I use a marker to mark the insert where it was to help gage the amount of rotation.

For the solid ceramic end mills, I have never worked with them, but have spec'd them and the customer backed out because they didn't want to run their spindle full tilt for a few minutes of roughing, and we couldn't quite go fast enough for confidently applying 3/8 tool. 

I ended up using a Harvi III 6 flute (coated carbide) at about 175 base surface foot with an dynamic mill toolpath.  20% or 40% stepover I believe, don't be afraid to take some radial engagment, it will help with life, just try not to take more than 40%, back off on the width as the depth gets deeper.  If you go to fast, or have rigidity issues, it will just start peeling the edges off the endmill, gets knarly fast. A 25 sfm change can make a huge difference.   I didn't ramp but the final .025" for the entry for the pockets as I had a flat bottom drill to poke the start with.  I highly recommend drilling over ramping with carbide. 

Kennametal GOdrills work great in 718 and 625 Inconel. (any material actually) 85 sfm, feed with nickel based starting book values, through coolant for sure.   We were drilling 8mm holes 8xd deep with great success.  If drilling through, pay attention to the exits, you will want to slow the feed on exit by about 40%, not as important if you have through coolant, but is still a good idea to prevent chipping the drill corners, as you won't get far once you do.  When processing that part, I drilled then removed the material below the hole so as to not have to exit the material anywhere.  Customer couldn't believe the difference in tool life.  It was consistent for once!!!!

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us