Jump to content

Welcome to eMastercam.com
Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.
Login to Account Create an Account
Photo

A286 steel?

- - - - -

  • Please log in to reply
18 replies to this topic

#1
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
Has anyone ever machined A286?

#2
Jeremy Herron@DBS Solutions™

Jeremy Herron@DBS Solutions™

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 962 posts
  • Location:Greenville, SC
Tons. What you want to know?

#3
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
How machinable is it? What would be a good comparison?

#4
strabe

strabe

    Advanced Member

  • Members
  • PipPipPip
  • 768 posts
Cutting granite with a butter knife is comparable.

#5
strabe

strabe

    Advanced Member

  • Members
  • PipPipPip
  • 768 posts
Actually it's worse than 304 but better than Hastelloy.

#6
strabe

strabe

    Advanced Member

  • Members
  • PipPipPip
  • 768 posts
Machinability is 33% using 1212 as a base of 100%

#7
Jeremy Herron@DBS Solutions™

Jeremy Herron@DBS Solutions™

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 962 posts
  • Location:Greenville, SC
It is a superalloy with more iron than most. Here is a .pdf with material compostions.

Attached Files



#8
Jeremy Herron@DBS Solutions™

Jeremy Herron@DBS Solutions™

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 962 posts
  • Location:Greenville, SC
If you normally turn your your superalloys with ceramics, plan on using carbide on A286, milling you can rough with ceramics anf finish with carbide. 125-175 sfm as a staring point with carbide.

#9
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
Thanks for the info. Anything else to keep in mind for machining this stuff?

#10
Jeremy Herron@DBS Solutions™

Jeremy Herron@DBS Solutions™

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 962 posts
  • Location:Greenville, SC
Are you mill or turning?

#11
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
I haven't even seen the print yet the Salesman was just asking me if we could do it.

#12
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
I'm guessing it will be a milled part, most everything we do is horizontal work.

#13
Jeremy Herron@DBS Solutions™

Jeremy Herron@DBS Solutions™

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 962 posts
  • Location:Greenville, SC
It work hardens pretty easy. If you are familiar with milling superalloys with ceramics and you have alot of material to remove I have had some sucess with it. If not stay away from them because it a bit of a leap from the norm. If you run ceramics I suggest NTK and dry, otherwise I usually jack my coolant concentration up to 10-15% if I have a lot to run. Threadmill or rollform threads. Carbide drills if you can afford them. Variable helix variable pitch endmills for solid carbide. Stay away from square shoulder inserted cutters, button cutters are your friend here.

#14
Zoober

Zoober

    Anigilohi

  • Members
  • PipPipPip
  • 5,738 posts
  • Location:Valencia, Ca.
I've always treated it like inco 625. Thin walls will move (push) with moderate tool pressure.
I am dying to test some HSS paths on some high temp.
We are eating Ti up with them. And tool life in the hours.
Like Jeremy says, do not work harden it!

#15
Buddy J

Buddy J

    Member

  • Members
  • PipPip
  • 140 posts
  • Location:Baltimore, Md.
Nasty Nasty stuff!
Have a job with lots of small deep radiused slots. (.12W x .6L x .900 Deep on a 1.5 radius..Belive me, in this stuff, .900 is DEEP!) Lets just say I changed lots of tools.....some every part.
If Carbide isn't an option, Cobalt drills, depending on the brand and a lot of luck, hold up rather well.
About 40 SFM :o
I had to roll tap 0-80's in this stuff, after heat treat..Thank God for Molly-dee!
Good luck
You have my sympathy!

#16
andate caga

andate caga

    Member

  • Members
  • PipPip
  • 34 posts
  • Location:Seattle
Treat it like Inconel 625. I make lots of R&D parts out of this. It work hardens and grows back, moves all over the place. I would personally like to cut inco 625 over this. Every batch is different also. I do turn and mill work. Use of low stepover max depth of cut is the way to mill. Turning I use kc5510 grade from kennametal. Drilling I use Gurhing with firex coating 70sfpm.

This might sound conservative to some but my parts are six figures easy and we don't get a setup part.

I would never recommend HSS/cobalt unless your drilling a small a286 fastener out.

Dynamic high speed tool paths work really well with superalloys. Don't be afraid to use tool inspection points. I usually put a 30 min check when hogging.

#17
Storkman

Storkman

    Gigantic Member

  • Members
  • PipPipPip
  • 6,757 posts
  • Location:NY
It really depends on what heat treat condition it is. It can go from Granite to Kryptonite.

#18
JParis

JParis

    Advanced Member

  • Members
  • PipPipPip
  • 24,543 posts

It really depends on what heat treat condition it is. It can go from Granite to Kryptonite.


true dat!

#19
BenK

BenK

    Advanced Member

  • Members
  • PipPipPip
  • 1,486 posts
  • Location:Burnsville, MN
Thanks for the info. Sounds like this stuff will be a good challenge for me, I'm always up for something new.