Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

machining Inconel 600

Toby

By Toby,
in Industrial Forum

 Share

Recommended Posts

Toby Newbie

Toby

Posted
Posted

Does anyone have experiance machining Inconel 600. I have 1 part to make 1 and need to nail this one on the money. Some of the processes are drilling, rough/finish mill. Any speed, feed, pecks, depths of cut and recomended tooling would be greatly appreciated.

------------------

Toby Baughman

Programming Supervisor

Saint Gobain Semicon Group Inc.

Vs8.1.1 LvL3 Mill + solids

Link to comment
Share on other sites
mikee Newbie

mikee

Posted
Posted

Toby,

I ran inconel while working at Hughes. Its not real hard material but is tough and somewhat gummy. It is hard on tools. You will need finish tools for this material. Your roughing tools will wear out before the finish pass. Keep this in mind,you might need extra tools set up just in case.

As far as feeds and speeds, a good starting point is to run the same as 304 stainless.

For drilling, spot drill with dwell. About 2 sec. You will see the material push away from you tool. Use sharp drills. Colbolt or carbide. Small drills , .015 to .020 pecks.

Carbide end mills, coated if at all possible

6 flute for small stuff. (.125 or smaller). At least worked better for the small parts we did.

I used to take a final pass on the top of all surfaces, about .001 above. It gets rid of most of the burrs. (this would be the last tool you run ).

Last but not the least ask who you are running the job for if you can run coolant. This material needs it, but it can be a cleaning issue.

I would ask for a piece of extra material just to see how it works.

This should give you some starting points.

Good Luck

Mikee

Link to comment
Share on other sites
Guest CNC Apps Guy 1

Guest CNC Apps Guy 1

Posted
Posted

Also, if you're doing deep hole stuff with small diameters, you'll want coated and you'll want to grind the drill so that it it will open the hole up a bit because the inconel will collapse on the drill causing it to break down in the hole. Do this for approx. 5 diameters and deeper.

HSS tools will wear like you've never seen a tool wear! and should be avoided if at all possible. Robb Jack makes some coated End Mills that do very well all things considered. Like Mikee mentioned, it is not all that hard, it is just VERY, VERY, VERY tough.

Just my $.02

------------------

James M. wink.gif

Mastercam Enthusiast

[This message has been edited by James Meyette (edited 07-18-2001).]

Link to comment
Share on other sites
Guy Newbie

Guy

Posted
Posted

It's not that hard.

Pecking can go up to 0.200" depth (1/4 to 1/2 dia).For roughing I , if it's possible, use a insert cutter and for finishing I only have HSS and it make a nice job.

For HSS the SFM is about 35 to 45.(Drill and endmill)

Roughing with endmills: z-axis depth= about 0.150"

have a nice day

------------------

Guillaume Côté

Hexco inc, Montreal Canada

Stainless steel specialist

Link to comment
Share on other sites
awheeler Newbie

awheeler

Posted
Posted

I used to machine small round window mounts for soft x-rays and there was a part that needed a 1mm hole drilled thru it. The only way I could get through it was with HSS drill bits at about 600-800 rpm (lathe) and peck that were no more than .003-.004" deep at a time. I hated working with that stuff. For a hole that was about .1875" deep I would typically burn up 3-4 drills. I tried carbide but it couldnt take the shock and snapped. Nasty stuff.

Link to comment
Share on other sites
Michael Reynolds Newbie

Michael Reynolds

Posted
Posted

From my experience, if you're gonna use HSS, the sfm should be about 20, and you need to put the feed "right to it". Your cutter should have a pretty high shear angle, and you should flood the heck out of it, lest it work hardens, and your basically screwed.

I never had good luck cutting inconel with indexable tooling, either.

Hope that helps!

Mike R.

Link to comment
Share on other sites
toolmann Newbie

toolmann

Posted
Posted

POOR MIKE I AM AMAZED AT HOW MANY PEOPLE DO NOT KNOW HOW TO MACHINE THIS MATERIAL IT IS VERY SIMPLE, DO NOT HEAT UP THE MATERIAL WHEN CUTTING IT, IT WILL DESTROY YOUR TOOLS.

KEEP THE SFPM DOWN AS LOW AS POSSIBLE, AND USE LOTS OF COOLANT.

MACHINABILITY IS 15-30%, THAT IS NOT THAT BAD

KEEP SFPM DOWN TO 60-100 FOR CBD END MILLS.

ROUGH=60-65 SEMI=65-75 FINISH=75-100

FEED .001-.002 PER TOOTH. USE 50'-60' HELIX END MILLS IF YOU CAN THEY WORK GREAT. USE 1 END MILL FOR EACH PROCESS TO ROUGH, SEMI FINISH, & FINISH.

DRILLING USE 15-20 SFPM AND COBALT DRILL'S

FEED .002-IPR=1/8" DRILL .003-IPR=1/4 DRILL

YOU CAN USE CARBIDE BUT THEY DO BREAK DEPENDING ON THE APPLICATION, YOU NEED EXPERIENCE TO DO THIS, SO I DO NOT RECOMMEND

USING CARBIDE AT THIS TIME.

 

[This message has been edited by toolmann (edited 07-24-2001).]

Link to comment
Share on other sites
Toby Newbie

Toby

Posted
  • Author
Posted

Thanks for all the suggestions. I was able to get thru this part (15 tools) with no problems. There is a wide range of suggested speeds and feeds not only on this forum but in reputable reference books which adds to the confussion. I stuck with the hss drills 15-20 sfm /mill 16-35 / carb to 65 sfm and was successful.

Thanks again,

------------------

Toby Baughman

Programming Supervisor

Saint Gobain Semicon Group Inc.

Vs8.1.1 LvL3 Mill + solids

Link to comment
Share on other sites
  • 4 weeks later...
  • 14 years later...
nickelwiremesh Newbie

nickelwiremesh

Posted
Posted

The alloys which are nickel based and are good resistant of temperature and corrosion are considered to difficult when we are about to do machining of these. Still there are some conventional methods out there which can help you  machining your alloys at satisfactory rates.

 

Following are few key points which should be considered while machining inconel 600:-

 

1. Capacity - The most important factors on which the machining is dependent upon are speed, feed, depth of cut and tooling because these factors allow you to utilize machinery available for the job. Sturdy machinery is needed to to drill large holes and tapping .

 

2. Tooling - Alloys basic quality is being worked and because of this tooling needs to be changed  or resharpen on regular basis.

 

 

3. Lubrications / Coolants - Coolants and lubricants should be as you desire. Water miscible vegetable oil can help you obtain good results.

 

4. Drilling - Make sure to use the same speeds (SFM) while facing, turning and boring for specific alloy as you do while using insert drills in CNC machines.

 

 

Hope it helps.

 

-----------

Thanks,

James Root | Business Associate

I love to talk anything about inconel mesh

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...